The Onshape Standard Library

Modeling

geometry

This module makes all Onshape Standard Library features and functions available.

New Feature Studios begin with an import of this module,

import(path : "onshape/std/geometry.fs", version : "");

with current version inserted (e.g. 300.0). This gives that Feature Studio access to all functions, types, enums, and constants defined in the Onshape Standard Library.

common

This module makes most common Onshape Standard Library functions available. It can be imported in place of geometry.fs,

import(path : "onshape/std/common.fs", version : "");

into Feature Studios that do not require the full set of Onshape Standard Library features.

A Context is a builtin that stores modeling data, including bodies (solids, sheets, wires, and points), their constituent topological entities (faces, edges, and vertices), variables, feature error states, etc.

Every Onshape Part Studio uses a single Context. All features, operations, and evaluation functions require a context to operate on. Different contexts do not interact, but data may be transferred from one to another using opMergeContexts.

Each context keeps track of the version of the Onshape Standard Library at which it was created. While regenerating a feature that has been "held back" to an older version, the version reported by the context will be the older version, causing subfeatures and operations to emulate old behavior.

canBeContext (value) predicate

Typecheck for Context

isAtVersionOrLater (versionToCheck is FeatureScriptVersionNumber, versionToCompareAgainst is FeatureScriptVersionNumber) returns boolean

isAtInitialMixedModelingReleaseVersionOrLater (context is Context) returns boolean

Returns true if at or after mixed modeling release version.

Id type

An Id identifies a feature or operation in a context. Each feature, subfeature, and operation must have a unique id. Ids are used in queries, error reporting, and accessing data associated with features.

Ids are hierarchical. That is, each operation's id must have a parent id. The root id is constructed with newId() and subIds are added with the overloaded + operator.

EXAMPLE

id + "foo" represents an id named "foo" whose parent is id

EXAMPLE

id + "foo" + "bar" represents an id named "bar" whose parent equals id + "foo"

Internally, an Id is just an array whose elements are strings, representing the full path of the Id.

EXAMPLE

newId() + "foo" + "bar" is equivalent to ["foo", "bar"] as Id, though the expressions like the latter are not recommended in practice.

Within a feature, all operations' ids should be children of the feature's Id (which is always passed into the feature function as the variable id).

Subfeatures should use a similar pattern. For instance, in the snippet below, mySubfeature is a minimal example following good practices for breaking out a set of operations into a subroutine.

annotation { "Feature Type Name" : "My Feature" }
export const myFeature = defineFeature(function(context is Context, id is Id, definition is map)
    precondition {}
    {
        fCuboid(context, id + "startingCube", {
                "corner1" : vector(0, 0, 0) * inch,
                "corner2" : vector(1, 1, 1) * inch
        });
        mySubfeature(context, id + "subFeature", qCreatedBy(id + "startingCube", EntityType.EDGE));
        fCuboid(context, id + "endingCube", {
                "corner1" : vector(0, 0, 0) * inch,
                "corner2" : vector(-1, -1, -1) * inch
        });
    }, {});
function mySubfeature(context is Context, id is Id, entities is Query)
{
    opChamfer(context, id + "chamfer", {
            "entities" : entities,
            "chamferType" : ChamferType.EQUAL_OFFSETS,
            "width" : 0.1 * inch
    });
    opFillet(context, id + "fillet1", {
        "entities" : qCreatedBy(id + "chamfer", EntityType.EDGE),
        "radius" : 0.05 * inch
    });
}

The full id hierarchy must reflect creation history. That is, each Id (including parents) must refer to a contiguous region of operations on the context.

Thus, the following code will fail because id + "extrude" alone refers to two non-contiguous regions of history:

for (var i in [1, 2])
{
    opExtrude(context, id + "extrude" + i, {...}); // Fails on second iteration.
    opChamfer(context, id + "chamfer" + i, {...});
}

For the above code, a pattern like id + i + "extrude" or id + ("loop" ~ i) + "extrude" would work as expected, as would the unnested id + ("extrude" ~ i).

Only the following characters are allowed in a string that makes up an Id: a-z, A-Z, 0-9, _, +, -, /. An asterisk * is allowed at the beginning of the string to mark it an "unstable" component (see below).

canBeId (value) predicate

Typecheck for Id

newId () returns Id

Returns an empty id.

makeId (idComp is string) returns Id

Returns an id specified by the given string.

isTopLevelId (id is Id) predicate

True if the Id represents a top-level feature or default geometry (i.e. if the Id has length 1)

ANY_ID const

The string literal "*", which matches any id inside certain queries.

EXAMPLE

qCreatedBy(id + ANY_ID + "fillet")

unstableIdComponent (addend) returns string

Marks a given id component as "unstable" causing queries to treat it as a wildcard. This is useful for when the id component is not expected to be robust, such as an index into the results of an evaluated query.

setVariable (context is Context, name is string, value)

Attach a variable to the context, which can be retrieved by another feature defined later. If a variable of the same name already exists, this function will overwrite it.

EXAMPLE

setVariable(context, "foo", 1) attaches a variable named "foo", with value set to 1, on the context.

Parameter	Type	Additional Info
`value`		Can be any value, including an array or map with many elements.

setVariable (context is Context, name is string, value, description is string)

Attach a variable with a description to the context, which can be retrieved by another feature defined later. If a variable of the same name already exists, this function will overwrite it.

EXAMPLE

setVariable(context, "foo", 1, "the foo") attaches a variable named "foo", with value set to 1 and the description set to "the foo", on the context.

Parameter	Type	Additional Info
`value`		Can be any value, including an array or map with many elements.
`description`	`string`	A string describing the use or purpose of the variable.

getVariable (context is Context, name is string)

Retrieve a variable attached to the context by name. Throws an exception if variable by the given name is not found.

EXAMPLE

getVariable(context, "foo") returns the value assigned to a previously-set variable named "foo".

Variables on a context can also be accessed within a Part Studio using # syntax (e.g. #foo) inside any parameter which allows an expression.

getVariable (context is Context, name is string, defaultValue)

Retrieve a variable attached to the context by name. If variable by the given name is not found, returns defaultValue

EXAMPLE

getVariable(context, "foo", {}) returns the value assigned to a previously-set variable named "foo". If not found returns empty map.

libraryLanguageVersion ()

Returns the language version of the library. Note: this function calls @getLanguageVersion internally, but if you call @getLanguageVersion directly, you may get a different result. That is because @getLanguageVersion returns the language version of the module making the call (which, for a module in std will coincide with the version of std.)

geomOperations

Operations are the basic modeling primitives of FeatureScript. Operations can do extrusion, filleting, transforms, etc. An operation takes a context, an id, and a definition and modifies the context in accordance with the definition. The modifications can be referenced by the passed-in id. Operations return undefined but can fail by throwing an error or they can report warnings or infos. The status can be read with the getFeature... functions in error.fs.

When an operation parameter that requires one entity receives a query that resolves to multiple entities, it takes the first resolved entity.

The geomOperations.fs module contains wrappers around built-in Onshape operations and no actual logic.

opMoveCurveBoundary (context is Context, id is Id, definition is map)

Trims or extends a wire body to an entity or by a distance.

Parameter	Type	Additional Info
`definition`	`map`
`wires`	`Query`	The wire bodies to modify.
`moveBoundaryType`	`MoveCurveBoundaryType`	Optional Whether to trim or extend. Default is `TRIM`.
`trimTo`	`Query`	Required if `moveBoundaryType` is `TRIM`. Single entity to trim `wires` to.
`endCondition`	`CurveExtensionEndCondition`	Optional If `moveBoundaryType` is `EXTEND` defines whether to extend `wires` by a distance of to an entity. Default is `BLIND`.
`extensionDistance`	`ValueWithUnits`	Required if `endCondition` is `BLIND` Distance to extend `wires`.
`extendTo`	`Query`	Required if `endCondition` is `BLIND` Single entity to extend `wires` to.
`extensionShape`	`CurveExtensionShape`	Optional Specifies how to transition into the curve extensions. Default is `SOFT`.
`helpPoint`	`Query`	Required if `endCondition` is `BLIND` Specifies vertex used to choose a solution. If this is not provided, the closest vertex to the bounding entity will be used.
`flipHeuristics`	`boolean`	Optional If `true`, will trim or extend from the opposite end of `wires`. Default is `false`.

opBodyDraft (context is Context, id is Id, definition is map)

Apply draft to a part by adding material. The material is added between reference edges and a parting object. These reference edges can be supplied directly, or they can be inferred from face or part queries.

Parameter	Type	Additional Info
`definition`	`map`
`selectionType`	`BodyDraftSelectionType`	Optional Topology class for input. Default is `EDGES`
`topEdges`	`Query`	Required if `selectionType` is `EDGES` Edges to draft above parting entity.
`bottomEdges`	`Query`	Required if `selectionType` is `EDGES` and `bothSides` is `true` Edges to draft with `angleBelow`.
`faces`	`Query`	Required if `selectionType` is `FACES` Faces to draft. This will split the face with isoclines those for the draft. Additionally, any existing edges bounding `faces` will be used if they mark a transition from steep faces to non-steep faces for the given pull direction and draft angle.
`bodies`	`Query`	Required if `selectionType` is `PARTS` Parts to draft. This is equivalent to supplying all faces of the part in `faces`.
`excludeFaces`	`Query`	Optional Faces of `bodies` to exclude from drafting.
`angle`	`ValueWithUnits`	The draft angle above the parting object.
`bothSides`	`boolean`	Optional If `true`, draft on both sides of the parting object. Default is `false`.
`pullDirection`	`ValueWithUnits`	The pull direction.
`draftOnSelf`	`boolean`	Optional If true, then using the drafted part as the parting object. Default is `false`.
`partingObject`		Required if `draftOnSelf` is `false` A surface from surfaceGeometry.fs or a query to a face or sheet body.
`matchFacesAtParting`	`boolean`	Optional If true, then additional material will be added to make the top and bottom of the draft align. Default is `false`.
`matchFaceType`	`BodyDraftMatchFaceType`	Optional How to add material for `matchFacesAtParting` Default is `REFERENCE_EDGE`.
`cornerType`	`BodyDraftCornerType`	Optional The corner treatment to apply. Default is `EXTEND`.
`concaveRepair`	`BodyDraftConcaveRepairType`	Optional How to resolve intersecting draft faces. Default is `NONE`.
`concaveRepairRadius`	`ValueWithUnits`	Required if `concaveRepair` is `RADIUS` or `MIX`. The radius for intersection repair.
`keepMaterial`	`boolean`	Optional If true, an attempt will be made to keep the regions of the part protruding from the tapered faces. Default is false.
`showRefs`	`boolean`	Optional If true, then debug data will be generated to show the parting surface and draft edges.

opBoolean (context is Context, id is Id, definition is map)

Performs a boolean operation on multiple solid and surface bodies.

See also

processNewBodyIfNeeded for merging new solids.

joinSurfaceBodiesWithAutoMatching for merging new surfaces.

Parameter	Type	Additional Info
`definition`	`map`
`tools`	`Query`	The tool bodies.
`targets`	`Query`	Required if `OperationType` is `SUBTRACTION` or `SUBTRACT_COMPLEMENT`, or if `targetsAndToolsNeedGrouping` is true. The target bodies.
`operationType`	`BooleanOperationType`	The boolean operation to perform. EXAMPLE `BooleanOperationType.UNION` will merge any tool bodies that intersect or abut. All tool bodies have to be of the same type (solid or surface). When operating on surfaces, surfaces must have coincident or overlapping edges. When several bodies merge, the identity of the tool that appears earliest in the query is preserved (in particular, body color and body name are taken from it). EXAMPLE `BooleanOperationType.SUBTRACTION` will remove the union of all tools bodies from every target body. All tool bodies must be solid bodies. Target bodies could be either solids or surfaces. EXAMPLE `BooleanOperationType.INTERSECTION` will create the intersection of all tool bodies. All bodies must be solid bodies. EXAMPLE `BooleanOperationType.SUBTRACT_COMPLEMENT` will remove the complement of the union of all tool bodies from every target body. All tool bodies must be solid bodies. Target bodies could be either solids or surfaces.
`targetsAndToolsNeedGrouping`	`boolean`	Optional This option is for adjusting the behavior to be more suitable for doing the boolean as part of a body-creating feature (such as extrude). Default is `false`.
`keepTools`	`boolean`	Optional If true, the tools do not get consumed by the operation. Default is false.
`makeSolid`	`boolean`	Optional In case of surface union try to join surfaces into a solid. Default is false.

opBoundarySurface (context is Context, id is Id, definition is map)

Creates a boundary surface fitting two ordered sets of profiles.

Parameter	Type	Additional Info
`definition`	`map`
`uProfileSubqueries`	`array`	An ordered array of two or fewer queries for the profiles in the u direction. These can be edges or wire bodies. EXAMPLE `[ profileQuery1, profileQuery2 ]`
`vProfileSubqueries`	`array`	Optional An ordered array of two or fewer queries for the profiles in the v direction. These can be edges or wire bodies. EXAMPLE `[ profileQuery1, profileQuery2 ]`
`uDerivativeInfo`	`array`	Optional An array of maps that contain shape constraints at start and end profiles. Each map entry is required to have a profileIndex that refers to the affected profile. Optional fields include a vector to match surface tangent to, a magnitude, and booleans for matching tangents or curvature derived from faces adjacent to affected profile. EXAMPLE `[ { "profileIndex" : 0, "vector" : vector(1, 0, 0), "magnitude" : 2., "tangentToPlane" : true}, { "profileIndex" : 1, "adjacentFaces" : qFaces } ]` The first map would constrain the resulting boundary surface at the first u profile to be tangent to plane with normal vector(1,0,0) and magnitude 2. The second map constrains the boundary surface at the second u profile to match tangents of faces defined by the query qFaces.
`vDerivativeInfo`	`array`	Optional An array of maps analogous to uDerivativeInfo, but for v profiles.
`showIsocurves`	`boolean`	Optional Show graphical representation of a subset of isoparameteric curves on each face of the created boundary surface. Default `false`.
`curveCount`	`number`	Optional When `showIsocurves` is `true`, the number of curves to draw in each direction of each face's grid. Default `10`.

opCreateBSplineCurve (context is Context, id is Id, definition is map)

Generates a wire body given a BSplineCurve definition. The spline must have dimension of 3 and be G1-continuous.

Parameter	Type	Additional Info
`definition`	`map`
`bSplineCurve`	`BSplineCurve`	The definition of the spline.

opCreateBSplineSurface (context is Context, id is Id, definition is map)

Generates a sheet body given a BSplineSurface definition. The spline must have dimension of 3 and be G1-continuous.

Parameter	Type	Additional Info
`definition`	`map`
`bSplineSurface`	`BSplineSurface`	The definition of the spline surface.
`boundaryBSplineCurves`	`array`	Optional An array of `BSplineCurve`s defined in the parameter space of `bSplineSurface` to use as the boundary of the created sheet body. The boundary must form a single closed loop on the surface. The `dimension` of each curve must be `2`, as the boundaries are being defined in UV space of the created surface. If no boundary is supplied, the created sheet body will cover the full parameter range of `bSplineSurface`.
`makeSolid`	`boolean`	Optional When set to `true`, the operation will produce a solid instead of a sheet if the surface encloses a region. Default is `false`.

opCreateCompositePart (context is Context, id is Id, definition is map)

Create a composite part.

Parameter Type Additional Info

definition map

bodies

Query

Bodies from which to create the composite part. .

closed

boolean

Optional

A closed composite part consumes its constituent bodies, so that they are not available interactively for individual selection. Default is false.

opModifyCompositePart (context is Context, id is Id, definition is map)

Modifies a composite part.

Parameter	Type	Additional Info
`definition`	`map`
`composite`	`Query`	Existing composite part to modify.
`toAdd`	`Query`	Bodies to add to the composite part.
`toRemove`	`Query`	Bodies to remove from the composite part.

opChamfer (context is Context, id is Id, definition is map)

Adds a chamfer to given edges and faces.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	Edges and faces to chamfer.
`chamferType`	`ChamferType`	Determines where the new edges of the chamfer are positioned. EXAMPLE `ChamferType.EQUAL_OFFSETS` places both new edges `width` away from each original edge. EXAMPLE `ChamferType.TWO_OFFSETS` places edges `width1` and `width2` away. EXAMPLE `ChamferType.OFFSET_ANGLE` places one edge `width` away, and chamfers at an angle from that edge.
`width`	`ValueWithUnits`	Required if `chamferType` is `EQUAL_OFFSETS` or `OFFSET_ANGLE`. EXAMPLE `0.2 * inch`
`width1`	`ValueWithUnits`	Required if `chamferType` is `TWO_OFFSETS`.
`width2`	`ValueWithUnits`	Required if `chamferType` is `TWO_OFFSETS`.
`angle`	`ValueWithUnits`	Required if `chamferType` is `OFFSET_ANGLE`.
`oppositeDirection`	`boolean`	Required if `chamferType` is `OFFSET_ANGLE` or `TWO_OFFSETS`. `true` to reverse the two edges.
`tangentPropagation`	`boolean`	Optional `true` to propagate the chamfer along edges tangent to those passed in. Defaults to `false`.

CurveOnFaceDefinition type

Describes a set of isoparametric curves on a face.

Value	Type	Description
`CurveOnFaceDefinition`	`map`
`face`	`Query`	Face the curves are meant to lie on.
`creationType`	`FaceCurveCreationType`	Determines the type of curves. Currently supports isoparameter curves only in primary or secondary directions, either equally spaced or defined by a parameter array.
`names`	`array`	An array of distinct non-empty strings to identify the curves created.
`nCurves`	`number`	Required if `creationType` is `DIR1_AUTO_SPACED_ISO` or `DIR2_AUTO_SPACED_ISO` Number of curves.
`parameters`	`array`	Required if `creationType` is `DIR1_ISO` or `DIR2_ISO` Parameters to create curves at.

canBeCurveOnFaceDefinition (value) predicate

Typecheck for CurveOnFaceDefinition

curveOnFaceDefinition (face is Query, creationType is FaceCurveCreationType, names is array, nCurves is number) returns CurveOnFaceDefinition

Returns a new CurveOnFaceDefinition.

curveOnFaceDefinition (face is Query, creationType is FaceCurveCreationType, names is array, parameters is array) returns CurveOnFaceDefinition

opCreateCurvesOnFace (context is Context, id is Id, definition is map)

Generates isoparametric curves of faces. That is, for each specified surface parameter value, creates a new wire body following the curve which keeps the surface parameter at that constant value.

Parameter	Type	Additional Info
`definition`	`map`
`curveDefinition`	`array`	An array of `CurveOnFaceDefinition`s that describe group of curves per face.
`showCurves`	`boolean`	Optional Whether to display isoparameteric curves in color in the preview.
`useFaceParameter`	`boolean`	Optional For Onshape internal use.

opDeleteBodies (context is Context, id is Id, definition is map)

Deletes bodies from the context.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	Entities to delete. Passing in entities other than bodies deletes their owning bodies.

opDeleteFace (context is Context, id is Id, definition is map)

This is a direct editing operation that attempts to delete faces of a solid body and extend other faces to fill the hole.

Parameter	Type	Additional Info
`definition`	`map`
`deleteFaces`	`Query`	Faces to delete.
`includeFillet`	`boolean`	`true` to also delete fillets adjacent to the input faces.
`capVoid`	`boolean`	If `capVoid` is `true` and the deleted face cannot be filled by extending the surrounding faces, will attempt to replace the face with a planar face.
`leaveOpen`	`boolean`	Optional If `leaveOpen` is `true` the void from deleting faces is left open, potentially creating a surface out of a solid body. Default is `false`.

opDraft (context is Context, id is Id, definition is map)

Applies a given draft angle to faces.

Parameter	Type	Additional Info
`definition`	`map`
`draftType`	`DraftType`	Specifies a reference surface (e.g. a neutral plane) or reference entity draft. EXAMPLE `DraftType.REFERENCE_SURFACE` for a reference surface draft
`draftFaces`	`Query`	Required if `draftType` is `REFERENCE_SURFACE` The faces to draft for a `REFERENCE_SURFACE` draft.
`referenceSurface`		Required if `draftType` is `REFERENCE_SURFACE` A face or plane that defines the neutral surface for a `REFERENCE_SURFACE` draft. `draftFaces` will remain unchanged where they intersect `referenceSurface`. Can be either a `Query` or a `Plane`.
`referenceEntityDraftOptions`	`array`	Required if `draftType` is `REFERENCE_ENTITY` An array of maps of the form ("face", "references", "angle"). "face" should be a `Query` for exactly one face. "references" should be a `Query` for at least one edge attached to the face. The "face" will be drafted while the geometry of the "references" remains unchanged. "angle" is an optional `ValueWithUnits` parameter between -89.9 and 89.9 degrees which overrides the default `angle` parameter.
`pullVec`	`Vector`	The 3d direction relative to which the draft is applied. EXAMPLE `vector(0, 0, 1)` .
`angle`	`ValueWithUnits`	The draft angle, must be between 0 and 89.9 degrees. EXAMPLE `3 * degree`
`tangentPropagation`	`boolean`	Optional For a `REFERENCE_SURFACE` draft, `true` to propagate draft across tangent faces. Default is `false`.
`referenceEntityPropagation`	`boolean`	Optional For a `REFERENCE_ENTITY` draft, `true` to collect new reference entities and faces by pulling in edges connected to the specified reference edges. Connected edges on the same face or on tangent connected faces will be pulled in. Default is `false`.
`reFillet`	`boolean`	Optional `true` to attempt to defillet draft faces before the draft and reapply the fillets after. Default is `false`.

opExtractWires (context is Context, id is Id, definition is map)

Generates wire bodies from the supplied edges. If the edges are disjoint multiple wires will be returned. If the edges overlap or cross, or more than two meet at a point, the function will fail.

Parameter	Type	Additional Info
`definition`	`map`
`edges`	`Query`	The edges to be extracted.

opExtrude (context is Context, id is Id, definition is map)

Extrudes one or more edges or faces in a given direction with one or two end conditions. Faces get extruded into solid bodies and edges get extruded into sheet bodies.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	Edges and faces to extrude.
`direction`	`Vector`	The 3d direction in which to extrude. EXAMPLE `evOwnerSketchPlane(context, {"entity" : entities}).normal` to extrude perpendicular to the owner sketch EXAMPLE `evPlane(context, {"face" : entities}).normal` to extrude perpendicular to the first planar entity
`endBound`	`BoundingType`	The type of bound at the end of the extrusion. Cannot be `SYMMETRIC` or `UP_TO_VERTEX`. EXAMPLE `BoundingType.BLIND`
`endDepth`	`ValueWithUnits`	Required if `endBound` is `BLIND`. How far from the `entities` to extrude. EXAMPLE `1 * inch`
`endBoundEntity`	`Query`	Required if `endBound` is `UP_TO_SURFACE` or `UP_TO_BODY`. The face or body that provides the bound.
`endTranslationalOffset`	`ValueWithUnits`	Optional The translational offset between the extrude end cap and the end bound entity. The direction vector for this is the same as `direction`: negative values pull the end cap away from the bound entity when `endDepth` is positive. `endOffset` will only have an effect if `endBound` is `UP_TO_SURFACE`, `UP_TO_BODY`, or `UP_TO_NEXT`.
`startBound`	`BoundingType`	Optional The type of start bound. Default is for the extrude to start at `entities`. Cannot be `SYMMETRIC` or `UP_TO_VERTEX`.
`isStartBoundOpposite`		Required if is `UP_TO_SURFACE`, `UP_TO_BODY`, or `UP_TO_NEXT`. Whether the `startBound` extends in the opposite direction from the profile as the `endBound`. Defaults to `true` if not supplied.
`startDepth`	`ValueWithUnits`	Required if `startBound` is `BLIND`. How far from the `entities` to start the extrude. The direction vector for this is the negative of `direction`: positive values make the extrusion longer when `endDepth` is positive.
`startBoundEntity`	`Query`	Required if `startBound` is `UP_TO_SURFACE` or `UP_TO_BODY`. The face or body that provides the bound.
`startTranslationalOffset`	`ValueWithUnits`	Optional The translational offset between the extrude start cap and the start bound entity. The direction vector for this is the negative of `direction`: negative values pull the end cap away from the bound entity when `startDepth` is positive. `startOffset` will only have an effect if `startBound` is `UP_TO_SURFACE`, `UP_TO_BODY`, or `UP_TO_NEXT`.

opFaceBlend (context is Context, id is Id, definition is map)

Performs a face blend between two walls of faces.

Parameter	Type	Additional Info
`definition`	`map`
`side1`	`Query`	First set of faces, must belong to the same body.
`side2`	`Query`	Second set of faces, must belong to the same body.
`flipSide1Normal`	`boolean`	Wether to flip side 1's normal.
`flipSide2Normal`	`boolean`	Wether to flip side 2's normal.
`propagation`	`boolean`	Optional Whether to propagate the blend.
`propagationType`	`FaceBlendPropagation`	Optional How to propagate the blend. FaceBlendPropagation.TANGENT will propagate over tangent faces. FaceBlendPropagation.ADJACENT will propagate over all adjacent faces. FaceBlendPropagation.CUSTOM allows specification of a maximum angle between faces for propagation. Defaults is FaceBlendPropagation.TANGENT.
`propagationAngle`	`ValueWithUnits`	Optional Maximum angle between faces for propagation. Used if propagationType is FaceBlendPropagation.CUSTOM. Default is 0 * radian.
`crossSection`	`FaceBlendCrossSection`	The cross section type of the blend.
`spine`	`Query`	Required if `crossSection` is `DISC`. The spine of the blend. The blend's cross section will be orthogonal to the spine.
`blendControlType`	`BlendControlType`	Whether the blend is controled by a constant radius or a constant width.
`crossSectionShape`	`FaceBlendCrossSectionShape`	What shape the cross section of the blend will be.
`radius`	`ValueWithUnits`	Required if `blendControlType` is `RADIUS`. The radius of the cross section.
`width`	`ValueWithUnits`	Required if `blendControlType` is `WIDTH`. The width of the blend.
`asymmetric`	`boolean`	Optional Wether the radius or width is the same on each wall.
`secondRadius`	`ValueWithUnits`	Required if `blendControlType` is `RADIUS` and `asymmetric` is `true`. The radius of the cross section from side 2.
`widthRatio`	`number`	Required if `blendControlType` is `WIDTH` and `asymmetric` is `true`. How the blend will be divided between the walls. If widthRatio < 1, it will be wider towards side 1. If widthRatio > 1, it will be wider towards side 2.
`rho`	`number`	Required if `crossSectionShape` is `CONIC` Parameter of the conic cross section shape.
`magnitude`	`number`	Required if `crossSectionShape` is `CURVATURE` Parameter of the curvature cross section shape.
`tangentHoldLines`	`boolean`	Optional Whether to use the content of `tangentEdges` and `inverseTangentEdges`.
`tangentEdges`	`Query`	Optional Edges to use as tangent hold lines.
`inverseTangentEdges`	`Query`	Optional Edges to use as inverse tangent hold lines.
`conicHoldLines`	`boolean`	Optional Whether to use the content of `conicEdges` and `inverseConicEdges`.
`conicEdges`	`Query`	Optional Edges to use as conic hold lines.
`inverseConicEdges`	`Query`	Optional Edges to use as inverse conic hold lines.
`hasCliffEdges`	`boolean`	Optional Whether to use the content of `cliffEdges`.
`cliffEdges`	`Query`	Optional Edges to use as cliff edges.
`hasCaps`	`boolean`	Optional Whether to use the content of `caps`.
`caps`	`array`	Optional Entities and flip flags to use as caps. Each map should contain an `entity` Query element and a `flip` boolean element.
`hasLimits`	`boolean`	Optional Whether to use the content of `limitPlane1`, `limitPlane2`, `faceLimits` and `edgeLimit`.
`limitPlane1`	`Query`	Optional First plane to limit the blend.
`limitPlane1Flip`	`boolean`	Whether to flip the first plane normal. Defines which side of the plane the blend will be.
`limitPlane2`	`Query`	Optional Second plane to limit the blend.
`limitPlane2Flip`	`boolean`	Whether to flip the first plane normal. Defines which side of the plane the blend will be.
`faceLimits`	`Query`	Optional Faces to use as limits to the blend.
`edgeLimit`	`array`	Optional Edges and adjacent faces to use as limits. Each map should contain an `edge` Query element and an `edgeLimitSide` query element.
`hasHelpPoint`	`boolean`	Optional Whether to use the content of `helpPoint`.
`helpPoint`	`Query`	Optional Vertex or mate connector to use as help point. In case the blend parameters create several blends, only the blend closest to the help point will be kept.
`trim`	`FaceBlendTrimType`	Optional How to trim the blend.
`detach`	`boolean`	Optional Whether not to attach the blend(s) to the sides, creating new sheet bodies.
`showIsocurves`	`boolean`	Optional Show graphical representation of a subset of isoparameteric curves of the created surface. Default `false`.
`curveCount`	`number`	Optional When `showIsocurves` is `true`, the number of curves to draw in each direction of the grid. Default `10`.

opFillet (context is Context, id is Id, definition is map)

For edges, performs a fillet on the edge. For faces, performs a fillet on all edges adjacent to the face.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	Edges and faces to fillet.
`radius`	`ValueWithUnits`	The fillet radius. EXAMPLE `1 * inch`
`tangentPropagation`	`boolean`	Optional `true` to propagate the fillet along edges tangent to those passed in. Default is `false`.
`crossSection`	`FilletCrossSection`	Optional Fillet cross section. One of `CIRCULAR`, `CONIC`, `CURVATURE`. Default is `CIRCULAR`.
`rho`	`number`	Required if `crossSection` is `CONIC`. A number between 0 and 1, specifying the Rho value of a conic fillet EXAMPLE `0.01` creates a flat, nearly-chamfered shape. EXAMPLE `0.99` creates a pointed, nearly-unchanged shape.
`magnitude`	`number`	Required if `crossSection` is `CURVATURE`. A number between 0 and 1, specifying the magnitude of curvature match.
`partialFilletBounds`	`array`	Optional An array of maps representing the boundaries of a partial fillet. Each map should contain a `boundaryEdge` query, a `boundaryParameter` value, a `isFlipped` boolean EXAMPLE `[{ "boundaryEdge" : edgeQuery0, "boundaryParameter" : 0.3, "isFlipped" : false }, { "boundaryEdge" : edgeQuery1, "boundaryParameter" : 0.6, "isFlipped" : true }]`
`isVariable`	`boolean`	Optional Fillet controls can be varied at vertices via `vertexSettings`. Default is `false`.
`vertexSettings`	`array`	Optional An array of maps representing fillet settings at specified vertices. Each map should contain a `vertex` query, a `vertexRadius` value, a `variableMagnitude` if the `crossSection` is `FilletCrossSection.CURVATURE`, and a `variableRho` if the `crossSection` is `FilletCrossSection.CONIC`. EXAMPLE `[{ "vertex" : vertexQuery0, "vertexRadius" : 1 * inch, "variableRho" : 0.2 }, { "vertex" : vertexQuery1, "vertexRadius" : 2 * inch, "variableRho" : 0.8 }]`
`pointOnEdgeSettings`	`array`	Optional An array of maps representing fillet settings at specified points on edges. Each map should contain an `edge` query, an `edgeParameter` value, a `pointOnEdgeRadius` value, a `pointOnEdgeVariablMagnitude` if the `crossSection` is `FilletCrossSection.CURVATURE`, and a `pointOnEdgeVariableRho` if the `crossSection` is `FilletCrossSection.CONIC`. EXAMPLE `[{ "edge" : edgeQuery0, "edgeParameter" : 0.3, "pointOnEdgeRadius" : 1 * inch }, { "edge" : edgeQuery1, "edgeParameter" : 0.6, "pointOnEdgeRadius" : 2 * inch }]`
`smoothTransition`	`boolean`	Required if `isVariable` is `true` Whether to create a smoother transition between each vertex.
`allowEdgeOverflow`	`boolean`	Optional Allow `opFillet` to modify nearby edges to maintain the fillet profile. Default is `true`.
`keepEdges`	`Query`	Optional Edges you do not want `opFillet` to modify if `allowEdgeOverflow` is `true`.
`smoothCorners`	`boolean`	Optional Allow `opFillet` to smooth all suitable corners and prevent creation of sharp edges. Default is `false`.
`smoothCornerExceptions`	`Query`	Optional Vertices you do not want `opFillet` to smooth if `smoothCorners` is `true`.
`createDetachedSurface`	`boolean`	Optional Operation does not modify the body of the selected edges, but results in surface geometry of fillet. Default is `false`.

opFillSurface (context is Context, id is Id, definition is map)

Generates a surface body from supplied boundary and internal constraints. The boundaries are defined as edge queries for each continuity constraint. The internal constraints may be defined as a set of support vertices.

Parameter	Type	Additional Info
`definition`	`map`
`edgesG0`	`Query`	The edges with position constraints.
`edgesG1`	`Query`	The edges with tangency constraints.
`edgesG2`	`Query`	The edges with curvature constraints.
`guideVertices`	`Query`	The vertices the resulting surface is expected to interpolate.
`showIsocurves`	`boolean`	Optional Show graphical representation of a subset of isoparameteric curves of the created surface. Default `false`.
`curveCount`	`number`	Optional When `showIsocurves` is `true`, the number of curves to draw in each direction of the grid. Default `10`.

opFitSpline (context is Context, id is Id, definition is map)

Creates a 3D cubic spline curve through an array of 3D points.

Parameter	Type	Additional Info
`definition`	`map`
`points`	`array`	An array of `Vector`s with length units for the spline to interpolate. If the first point is the same as the last point, the spline is closed. EXAMPLE [ vector( 1, 1, 1) * inch, vector(-1, 1, -1) * inch, vector( 1, -1, -1) * inch, vector(-1, -1, 1) * inch, vector( 1, 1, 1) * inch ]
`parameters`	`array`	Optional An array of doubles, parameters corresponding to the points.
`startDerivative`	`Vector`	Optional A `Vector` with length units that specifies the derivative at the start of the resulting spline (according to the `arcLengthParameterization` set to `false`).
`endDerivative`	`Vector`	Optional A `Vector` with length units that specifies the derivative at the end of the resulting spline. Ignored if spline is closed.
`start2ndDerivative`	`Vector`	Optional A `Vector` with length units that specifies the second derivative at the start of the resulting spline. Ignored if spline is closed, or if `startDerivative` is not defined
`end2ndDerivative`	`Vector`	Optional A `Vector` with length units that specifies the second derivative at the end of the resulting spline. Ignored if spline is closed, or if `endDerivative` is not defined
`derivatives`	`map`	Optional A map of derivatives at non-end points. Entries should be `index : derivative`, where `index` is an integer between 1 and `size(points) - 2` and `derivative` is a `Vector` that specifies the derivative at `points[index]`.

opFlipOrientation (context is Context, id is Id, definition is map)

Reverses the orientation of sheet bodies.

Parameter	Type	Additional Info
`definition`	`map`
`bodies`	`Query`	Sheet bodies whose orientation should be flipped.

opFullRoundFillet (context is Context, id is Id, definition is map)

Creates a full round fillet, replacing the center face(s) with circular profile face(s) of varying radius, joining the selected side faces.

Parameter	Type	Additional Info
`definition`	`map`
`side1Face`	`Query`	A face on one side of the blend.
`side2Face`	`Query`	A face on another side of the blend.
`centerFaces`	`Query`	The face(s) to be replaced.
`tangentPropagation`	`boolean`	Optional `true` to propagate the fillet across side face tangencies. Default is `true`.

opHelix (context is Context, id is Id, definition is map)

Creates a helical and possibly spiral curve.

Parameter	Type	Additional Info
`definition`	`map`
`direction`	`Vector`	The direction of the helix axis. EXAMPLE `vector(0, 0, 1)`
`axisStart`	`Vector`	A point on the helix axis. EXAMPLE `vector(0, 0, 0) * inch`
`startPoint`	`Vector`	The start point of the infinite helix. Must be off the axis. This is the point at which the created curve would actually start if the first number of `interval` is 0. EXAMPLE `vector(1, 0, 0) * inch`
`interval`	`Vector`	An array of two numbers denoting the interval of the helix in terms of revolution counts. EXAMPLE `[0, 10]` will create a curve with 10 revolutions.
`clockwise`	`boolean`	EXAMPLE `true` if this is a clockwise helix when viewed along `direction`.
`helicalPitch`	`ValueWithUnits`	Distance along the axis between successive revolutions. EXAMPLE `0.1 * inch` will create a helix with 10 revolutions per inch. EXAMPLE `0 * inch` produces a planar Archimedean spiral.
`spiralPitch`	`ValueWithUnits`	Change in radius between successive revolutions. EXAMPLE `0 * inch` produces a helix that lies on a cylinder.

opHole (context is Context, id is Id, definition is map) returns array

Creates hole tools referencing a set of targets, optionally subtracting the tools from the targets. If some tools cannot be built, the operation will still succeed and indicate in its return value which holes failed to build. If no tools can be built, the operation will fail.

Parameter	Type	Additional Info
`definition`	`map`
`holeDefinition`	`HoleDefinition`	The definition of the shape of the desired holes. EXAMPLE `holeDefinition([holeProfile(HolePositionReference.AXIS_POINT, 0 * inch, 0.1 * inch), holeProfile(HolePositionReference.AXIS_POINT, 1 * inch, 0 * inch)])`
`axes`	`array`	An array of `Line`s each of whose `origin` represents the start position of a hole, and whose `direction` represents the drill direction of the hole. EXAMPLE `[line(vector(-1, -1, 0) * inch, vector(0, 0, -1)), line(vector(1, 1, 0) * inch, vector(0, 0, -1))]`
`identities`	`array`	Optional An array of queries, one per axis in `axes`, used to disambiguate each of the created holes. Each query should resolve to exactly one entity. Providing this information does not change the geometric outcome, but stabilizes references to the holes with respect to upstream changes to the model.
`targets`	`Query`	Required if `holeDefinition` contains any `profiles` that do not reference `HolePositionReference.AXIS_POINT`, or if `subtractFromTargets` is `true` A set of bodies to target. The shape of the produced holes is dependent on the shape of these targets (as specified in the supplied `HoleDefinition`), so the full set of targeted bodies should always be supplied, even if `subtractFromTargets` is `false`.
`subtractFromTargets`	`boolean`	Optional `true` if the hole geometry should be subtracted from the targets. `false` if the targets should not be modified, and the hole tools should be outputted as new solid bodies. Default is `true`. To subtract from a subset of targets, set this to `true` and supply a set of excluded targets as `targetsToExcludeFromSubtraction`. Removing the set of excluded targets from `targets` instead of using `targetsToExcludeFromSubtraction` is not the correct way to call this interface, and may result in the shape of the hole changing.
`targetsToExcludeFromSubtraction`	`Query`	Optional If supplied and `subtractFromTargets` is `true`, the given targets are excluded from the subtraction. Ignored if `subtractFromTargets` is `false`
`keepTools`	`boolean`	Optional If `subtractFromTargets` is `true`, controls whether the hole tools should be outputted as new solid bodies. Default is `false`. Ignored if `subtractFromTargets` is `false`; in that case hole tools are always outputted as new solid bodies.

Return type Description

Return type	Description
`array`	An array representing target intersection information for each hole. The array is aligned with the `axes` input. Each item in the array is a map containing a `boolean` field `success`, which indicates whether the tool was successfully built. If `success` is `true` the map will contain three additional entries: `targetToDepthExtremes`, `positionReferenceInfo` and `holeDepth`. The value of `targetToDepthExtremes` is a `map` mapping the `targets` that the given hole intersects to a map of intersection information for those targets. Only targets that are intersected by the hole will be present in the map. Each map key is a `Query` for one of the targets, and the corresponding value is itself a map of the form `{ "firstEntrance" : firstEntranceDistance, "fullEntrance" : fullEntranceDistance, "firstExit" : firstExitDistance, "fullExit" : fullExitDistance }` `firstEntranceDistance`, `fullEntranceDistance`, `firstExitDistance`, and `fullExitDistance` are `ValueWithUnits` representing distances, along the axis, from the origin point of the axis to various important markers on the infinite hole cylinder. `firstEntranceDistance` and `fullEntranceDistance` represent the range over which the infinite hole cylinder enters the part, with `firstEntranceDistance` representing where the infinite hole cylinder first enters the part, and `fullEntranceDistance` representing where the infinite hole cylinder fully enters the part. These values are distinct when the entrance face into the part is slanted (or otherwise irregular). `firstExitDistance` and `fullExitDistance` similarly represent the range over which the infinite hole cylinder exits the part. The value of `positionReferenceInfo` is a `map` whose keys are the `HolePositionReference`s found in the `holeDefinition` and whose value is a map of the form `{ "referenceRootStart" : referenceRootStartDistance, "referenceRootEnd" : referenceRootEndDistance, "target" : targetQuery }`. `referenceRootStartDistance` is a `ValueWithUnits` representing the distance, along the axis, from the origin point of the axis to the first coincidence between the infinite hole cylinder and the reference in question. `referenceRootEndDistance` is a similar measurement to the last coincidence between the infinite hole cylinder and the reference in question. For flat references, such as a `TARGET_START` referencing the top face of a cube, these two values will be the same. The values will differ for slanted (or otherwise irregular) references where the infinite hole cylinder interacts with the reference over a range, rather than at a single distance. `targetQuery` is a `Query` for the `target` that defines that position reference. `holeDepth` is a `ValueWithUnits` representing the distance, along the axis from the first entrance of the intersected targets to the termination entity. Used for references such as UP_TO_ENTITY and UP_TO_NEXT to get a calculated depth of a hole. EXAMPLE // For an opHole operation creating two holes, both going into two stacked // parts, the first of which being 1 inch thick with a slightly slanted top // and flat bottom and the second being 3 inches thick with a flat top and // bottom, and the holeDefinition referencing both TARGET_START and // LAST_TARGET_START the return value may look like: [ { // First hole (successful) "success" : true, "targetToDepthExtremes" : { (firstTargetQuery) : { "firstEntrance" : 0.1 * inch, "fullEntrance" : 0.3 * inch, "firstExit" : 1 * inch, "fullExit" : 1 * inch }, (secondTargetQuery) : { "firstEntrance" : 1 * inch, "fullEntrance" : 1 * inch, "firstExit" : 4 * inch, "fullExit" : 4 * inch } }, "positionReferenceInfo" : { HolePositionReference.TARGET_START : { "referenceRootStart" : 0.1 * inch, "referenceRootEnd" : 0.3 * inch, "target" : firstTargetQuery }, HolePositionReference.LAST_TARGET_START : { "referenceRootStart" : 1 * inch, "referenceRootEnd" : 1 * inch, "target" : secondTargetQuery }, } }, { // Second hole (successful) "success" : true, "targetToDepthExtremes" : { (firstTargetQuery) : { "firstEntrance" : 0.4 * inch, "fullEntrance" : 0.6 * inch, "firstExit" : 1 * inch, "fullExit" : 1 * inch }, (secondTargetQuery) : { "firstEntrance" : 1 * inch, "fullEntrance" : 1 * inch, "firstExit" : 4 * inch, "fullExit" : 4 * inch } }, "positionReferenceInfo" : { HolePositionReference.TARGET_START : { "referenceRootStart" : 0.4 * inch, "referenceRootEnd" : 0.6 * inch, "target" : firstTargetQuery }, HolePositionReference.LAST_TARGET_START : { "referenceRootStart" : 1 * inch, "referenceRootEnd" : 1 * inch, "target" : secondTargetQuery }, } }, { // Third hole (unsuccessful) "success" : false } ]

array

An array representing target intersection information for each hole. The array is aligned with the axes input. Each item in the array is a map containing a boolean field success, which indicates whether the tool was successfully built. If success is true the map will contain three additional entries: targetToDepthExtremes, positionReferenceInfo and holeDepth.

The value of targetToDepthExtremes is a map mapping the targets that the given hole intersects to a map of intersection information for those targets. Only targets that are intersected by the hole will be present in the map. Each map key is a Query for one of the targets, and the corresponding value is itself a map of the form { "firstEntrance" : firstEntranceDistance, "fullEntrance" : fullEntranceDistance, "firstExit" : firstExitDistance, "fullExit" : fullExitDistance }

firstEntranceDistance, fullEntranceDistance, firstExitDistance, and fullExitDistance are ValueWithUnits representing distances, along the axis, from the origin point of the axis to various important markers on the infinite hole cylinder. firstEntranceDistance and fullEntranceDistance represent the range over which the infinite hole cylinder enters the part, with firstEntranceDistance representing where the infinite hole cylinder first enters the part, and fullEntranceDistance representing where the infinite hole cylinder fully enters the part. These values are distinct when the entrance face into the part is slanted (or otherwise irregular). firstExitDistance and fullExitDistance similarly represent the range over which the infinite hole cylinder exits the part.

The value of positionReferenceInfo is a map whose keys are the HolePositionReferences found in the holeDefinition and whose value is a map of the form { "referenceRootStart" : referenceRootStartDistance, "referenceRootEnd" : referenceRootEndDistance, "target" : targetQuery }.

referenceRootStartDistance is a ValueWithUnits representing the distance, along the axis, from the origin point of the axis to the first coincidence between the infinite hole cylinder and the reference in question. referenceRootEndDistance is a similar measurement to the last coincidence between the infinite hole cylinder and the reference in question. For flat references, such as a TARGET_START referencing the top face of a cube, these two values will be the same. The values will differ for slanted (or otherwise irregular) references where the infinite hole cylinder interacts with the reference over a range, rather than at a single distance.

targetQuery is a Query for the target that defines that position reference.

holeDepth is a ValueWithUnits representing the distance, along the axis from the first entrance of the intersected targets to the termination entity. Used for references such as UP_TO_ENTITY and UP_TO_NEXT to get a calculated depth of a hole.

EXAMPLE

// For an opHole operation creating two holes, both going into two stacked
// parts, the first of which being 1 inch thick with a slightly slanted top
// and flat bottom and the second being 3 inches thick with a flat top and
// bottom, and the holeDefinition referencing both TARGET_START and
// LAST_TARGET_START the return value may look like:
[
    { // First hole (successful)
        "success" : true,
        "targetToDepthExtremes" : {
                    (firstTargetQuery)  : {
                            "firstEntrance" : 0.1 * inch,
                            "fullEntrance" : 0.3 * inch,
                            "firstExit" : 1 * inch,
                            "fullExit" : 1 * inch
                        },
                    (secondTargetQuery) : {
                            "firstEntrance" : 1 * inch,
                            "fullEntrance" : 1 * inch,
                            "firstExit" : 4 * inch,
                            "fullExit" : 4 * inch
                        }
                },
        "positionReferenceInfo" : {
                    HolePositionReference.TARGET_START : {
                            "referenceRootStart" : 0.1 * inch,
                            "referenceRootEnd" : 0.3 * inch,
                            "target" : firstTargetQuery
                        },
                    HolePositionReference.LAST_TARGET_START : {
                            "referenceRootStart" : 1 * inch,
                            "referenceRootEnd" : 1 * inch,
                            "target" : secondTargetQuery
                        },
                }
    },
    { // Second hole (successful)
        "success" : true,
        "targetToDepthExtremes" : {
                    (firstTargetQuery)  : {
                            "firstEntrance" : 0.4 * inch,
                            "fullEntrance" : 0.6 * inch,
                            "firstExit" : 1 * inch,
                            "fullExit" : 1 * inch
                        },
                    (secondTargetQuery) : {
                            "firstEntrance" : 1 * inch,
                            "fullEntrance" : 1 * inch,
                            "firstExit" : 4 * inch,
                            "fullExit" : 4 * inch
                        }
                },
        "positionReferenceInfo" : {
                    HolePositionReference.TARGET_START : {
                            "referenceRootStart" : 0.4 * inch,
                            "referenceRootEnd" : 0.6 * inch,
                            "target" : firstTargetQuery
                        },
                    HolePositionReference.LAST_TARGET_START : {
                            "referenceRootStart" : 1 * inch,
                            "referenceRootEnd" : 1 * inch,
                            "target" : secondTargetQuery
                        },
                }
    },
    { // Third hole (unsuccessful)
        "success" : false
    }
]

opImportForeign (context is Context, id is Id, definition is map)

Brings foreign geometry into the context. This function is used for importing uploaded parts.

Parameter	Type	Additional Info
`definition`	`map`
`blobData`	`CADImportData`	Reference to a blob element hosting uploaded CAD data.
`flatten`	`boolean`	Optional Whether to flatten assemblies; defaults to false.
`yAxisIsUp`	`boolean`	Optional If true, the y axis in the import maps to the z axis and z maps to -y. If false (default), the coordinates are unchanged.
`isModifiable`	`boolean`	Optional Whether the imported data is modifiable (default) or not.

opCreateIsocline (context is Context, id is Id, definition is map)

Creates wires corresponding to the given faces's isocline edges. Each isocline follows a path along a face with a constant angle in the (-90, 90) degree range (e.g., lines of latitude on a sphere). This angle is the face tangent plane's angle with respect to the direction with its sign determined by the dot product of direction and the face normal, and is analogous to the angle used in draft analysis. Depending on the face geometry, there may be zero, one, or multiple isoclines on each face.

Parameter	Type	Additional Info
`definition`	`map`
`faces`	`Query`	The faces on which to imprint isoclines.
`direction`	`Vector`	A reference direction.
`angle`	`ValueWithUnits`	The isocline angle with respect to the direction in the (-90, 90) degree range.

opLoft (context is Context, id is Id, definition is map)

Creates a surface or solid loft fitting an ordered set of profiles, optionally constrained by guide curves.

Parameter	Type	Additional Info
`definition`	`map`
`profileSubqueries`	`array`	An ordered array of queries for the profiles. For a solid loft, these must be sheet bodies, faces, or vertices. For a surface loft, these could be wire bodies, sheet bodies, faces, edges, or vertices. EXAMPLE `[ profileQuery1, profileQuery2 ]`
`guideSubqueries`	`array`	Optional An array of queries for guide curves. Each guide curve should intersect each profile once.
`connections`	`array`	Optional An array of maps to define multiple profile alignments. Each connection map should contain: (1) connectionEntities query describing an array of vertices or edges (one per profile), (2) connectionEdges an array of individual queries for edges in connectionEntities. The order of individual edge queries should be synchronized with connectionEdgeParameters. (3) connectionEdgeParameters array - an ordered and synchronized array of parameters on edges in connectionEdgeQueries EXAMPLE `[ {"connectionEntities" : qVertexAndEdge1, "connectionEdges" : [qEdge1], "connectionEdgeParameters" : [0.25]} {"connectionEntities" : qVertexAndEdge2, "connectionEdges" : [qEdge2], "connectionEdgeParameters" : [0.75]}]`
`connectionsArcLengthParameterization`	`boolean`	Optional Defaults to false for better performance. Controls interpretation of connectionEdgeParameters. If `evDistance`, `evEdgeTangentLine` etc. are called in conjunction with opLoft the same value should be passed as `arcLengthParameterization` there.
`makePeriodic`	`boolean`	Optional Defaults to false. A closed guide creates a periodic loft regardless of this option.
`bodyType`	`ToolBodyType`	Optional Specifies a `SOLID` or `SURFACE` loft. Default is `SOLID`.
`trimGuidesByProfiles`	`boolean`	Optional If false (default) use full length of guides. If true restrict resulting surface by the first and last profile. Meaningful only for non-periodic surface loft.
`trimProfiles`	`boolean`	Optional If false (default) use full length of profiles. If true restrict resulting surface by the first and last guide or connection. Meaningful only for surface loft with open profiles.
`derivativeInfo`	`array`	Optional An array of maps that contain shape constraints at start and end profiles. Each map entry is required to have a profileIndex that refers to the affected profile. Optional fields include a vector to match surface tangent to, a magnitude, and booleans for matching tangents or curvature derived from faces adjacent to affected profile. EXAMPLE `[ { "profileIndex" : 0, "vector" : vector(1, 0, 0), "magnitude" : 2., "tangentToPlane" : true}, { "profileIndex" : 1, "matchCurvature" : true, "adjacentFaces" : qFaces } ]` The first map would constrain the resulting loft at the start profile to be tangent to plane with normal vector(1,0,0) and magnitude 2. The second map constrains the loft at the end profile to match the curvature of faces defined by the query qFaces.
`showIsocurves`	`boolean`	Optional Show graphical representation of a subset of isoparameteric curves on each face of the created loft. Default `false`.
`curveCount`	`number`	Optional When `showIsocurves` is `true`, the number of curves to draw in each direction of each face's grid. Default `10`.
`loftTopology`	`LoftTopology`	Optional Specifies topology of lofted body. Default is `MINIMAL`.

opMateConnector (context is Context, id is Id, definition is map)

Creates a mate connector, which represents a coordinate system in the context. Currently it is a special type of point body.

Parameter	Type	Additional Info
`definition`	`map`
`coordSystem`	`CoordSystem`	The mate connector coordinate system.
`owner`	`Query`	The owner body of the mate connector: when the owner is brought into an assembly, owned mate connectors will be brought in and move rigidly with it. If the query resolves to multiple bodies, the first is taken as the owner.

opMergeContexts (context is Context, id is Id, definition is map) returns array

Bring all of the information from contextFrom into context. This is used, for example, for the Derived feature.

Parameter	Type	Additional Info
`context`	`Context`	The target context.
`definition`	`map`
`contextFrom`	`Context`	The source context. It is rendered unusable by this operation. EXAMPLE `MyPartStudio::build()`
`trackThroughMerge`	`array`	Optional Array of queries to map evaluation result in contextFrom to context post-merge

Return type	Description
`array`	Returns array of the same size as trackThroughMerge with evaluation results for each query(array of arrays of transient queries).

opModifyFillet (context is Context, id is Id, definition is map)

This is a direct editing operation that modifies or deletes fillets.

Parameter	Type	Additional Info
`definition`	`map`
`faces`	`Query`	The fillets to modify.
`modifyFilletType`	`ModifyFilletType`	Whether to change the fillet radii or remove them altogether.
`radius`	`ValueWithUnits`	Required if `modifyFilletType` is `CHANGE_RADIUS`. The new radius.
`reFillet`	`boolean`	Required if `modifyFilletType` is `CHANGE_RADIUS`. `true` to reapply adjacent fillets. Default is `false`.

opMoveFace (context is Context, id is Id, definition is map)

This is a direct editing operation that applies a transform to one or more faces.

Parameter	Type	Additional Info
`definition`	`map`
`moveFaces`	`Query`	The faces to transform.
`transform`	`Transform`	The transform to apply to the face. EXAMPLE `transform(vector(0, 0, 1) * inch)` will translate the face 1 inch along the world's z-axis.
`reFillet`	`boolean`	Optional `true` to attempt to defillet `moveFaces` prior to the move and reapply the fillet after. Default is `false`.
`mergeFaces`	`boolean`	Optional `true` to remove redundant edges from moveFaces. Default is `true`.

opOffsetFace (context is Context, id is Id, definition is map)

This is a direct editing operation that offsets one or more faces.

Parameter	Type	Additional Info
`definition`	`map`
`moveFaces`	`Query`	The faces to offset.
`offsetDistance`	`ValueWithUnits`	The positive or negative distance by which to offset. EXAMPLE `0.1 * inch` will offset the face 0.1 inches, normal to the face.
`reFillet`	`boolean`	Optional `true` to attempt to defillet `moveFaces` prior to the offset and reapply the fillet after. Default is `false`.
`mergeFaces`	`boolean`	Optional `true` to remove redundant edges from moveFaces. Default is `true`.

opPattern (context is Context, id is Id, definition is map)

Patterns input faces and/or bodies by applying transforms to them. The original faces and bodies are preserved.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	Bodies and faces to pattern.
`transforms`	`array`	An array of `Transform`s to apply to `entities`. The transforms do not have to be rigid.
`instanceNames`	`array`	An array of distinct non-empty strings the same size as `transforms` to identify the patterned entities. Similar to an `Id`, an instance names may consist only of letters, numbers, and any of `+`, `-`, `/`, `_`.
`copyPropertiesAndAttributes`	`boolean`	Optional If true (default), copies properties and attributes to patterned entities.

opPlane (context is Context, id is Id, definition is map)

Creates a construction plane.

Parameter	Type	Additional Info
`definition`	`map`
`plane`	`Plane`	The plane to create. EXAMPLE `plane(vector(0, 0, 6) * inch, vector(0, 0, 1))`
`width`	`ValueWithUnits`	Optional The side length of the construction plane, as it is initially displayed.
`height`	`ValueWithUnits`	Optional The side length of the construction plane, as it is initially displayed.
`defaultType`	`DefaultPlaneType`	Optional For Onshape internal use.

opPolyline (context is Context, id is Id, definition is map)

Creates a polyline passing through an array of 3D points.

Parameter Type Additional Info

definition map

points

array

An array of Vectors with length units corresponding the points of the polyline. If the firstpoint is the same as the last point, the polyline is closed.

EXAMPLE

[
    vector( 1,  1,  1) * inch,
    vector(-1,  1, -1) * inch,
    vector( 1, -1, -1) * inch,
    vector(-1, -1,  1) * inch,
    vector( 1,  1,  1) * inch
]

bendRadii

array

Optional

An array of ValueWithUnits, corresponding to the bend radii at each point. The value at index i corresponds to the bend at the point at index i + 1 in points. A value of 0 * meter means no bend at the corresponding point. Its size should be size(points) - 2 for an open polyline, size(points) - 1 for a closed one.

opDropCurve (context is Context, id is Id, definition is map)

Projects curves on a face.

Parameter	Type	Additional Info
`definition`	`map`
`tools`	`Query`	The edges to project.
`targets`	`Query`	The faces/bodies the edges are to be projected onto.
`projectionType`	`ProjectionType`	Projection method.
`direction`	`Vector`	Optional The direction in which to project the curve. Required if projectionType is ProjectionType.DIRECTION.

opIntersectFaces (context is Context, id is Id, definition is map)

Intersect two faces, creating curves appropriately.

Parameter	Type	Additional Info
`definition`	`map`
`tools`	`Query`	First array of faces to intersect.
`targets`	`Query`	Second array of faces to intersect.

opSphere (context is Context, id is Id, definition is map)

Creates a sphere.

Parameter Type Additional Info

definition map

radius

ValueWithUnits

The radius of the sphere.

EXAMPLE

1 * inch

center

Vector

The location of the center of the sphere.

EXAMPLE

vector(1, 1, 1) * inch

opSplineThroughEdges (context is Context, id is Id, definition is map)

Creates a 3D spline curve representing a sequence of edges. The edges must form a tangent-continuous chain.

Parameter	Type	Additional Info
`definition`	`map`
`edges`	`Query`	Edges to approximate.

opSplitEdges (context is Context, id is Id, definition is map)

Splits an array of edges with an entity or at specified parameters.

Parameter	Type	Additional Info
`definition`	`map`
`edges`	`Query`	Edges to split.
`parameters`	`array`	An array of array of parameters. Each edge gets split at the parameter values at the matching index in this array.
`splittingSurface`	`Query`	A sheet body, a construction plane or a face to cut with. Can be either a `Query` or a `Plane`. Either `splittingSurface` or `parameters` must be specified but not both.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter returned for edges measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-calculate parameterization. Default is `true`.

opPoint (context is Context, id is Id, definition is map)

Creates a construction point (a BodyType.POINT with one vertex).

Parameter Type Additional Info

definition map

point

Vector

The location of the point.

EXAMPLE

vector(0, 0, 1) * inch

origin

boolean

Optional

For Onshape internal use.

opReplaceFace (context is Context, id is Id, definition is map)

This is a direct editing operation that replaces the geometry one or more faces with that of another face, possibly with an offset.

Parameter	Type	Additional Info
`definition`	`map`
`replaceFaces`	`Query`	The faces whose geometry to replace.
`templateFace`	`Query`	The face whose geometry to use as the replacement.
`offset`	`ValueWithUnits`	Optional The positive or negative distance by which to offset the resulting face.
`oppositeSense`	`boolean`	Optional If true, flip the surface normal of the resulting face, which may be necessary to match the surface normals of surrounding faces. Default is `false`.

opRevolve (context is Context, id is Id, definition is map)

Revolves edges and faces about an axis to produce sheet and solid bodies. The edges and faces may abut, but not strictly intersect the axis.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	The edges and faces to revolve.
`axis`	`Line`	The axis around which to revolve. EXAMPLE `line(vector(0, 0, 0) * inch, vector(0, 0, 1))`
`angleForward`	`ValueWithUnits`	The angle where the revolve ends relative to `entities`. Normalized to the range \[0, 2 PI). EXAMPLE `30 * degree`
`angleBack`	`ValueWithUnits`	Optional The angle where the revolve starts relative to `entities`. Normalized to the range \[0, 2 PI). If `angleForward == angleBack`, the revolve is a full (360-degree) revolve. Defaults to `0`.

opRuledSurface (context is Context, id is Id, definition is map)

Creates a ruled surface along a set of paths. Direction of ruled surface is specified with either ruledDirection or angleFromFaces.

Parameter	Type	Additional Info
`definition`	`map`
`path`	`Query`	The edges that form the paths for the ruled surface.
`cornerType`	`RuledSurfaceCornerType`	Optional How corners in the ruled surface are handled. Default is `RuledSurfaceCornerType.SPUN`.
`useCubicInterpolation`	`boolean`	Optional Ruled surface will use a cubic interpolation if `true`. Otherwise, a linear interpolation will be used. Default is `true`.
`width`	`ValueWithUnits`	The width of the ruled surface.
`ruledSurfaceType`	`RuledSurfaceType`	Specifies how the ruled surface is constructed.
`ruledDirection`	`Vector`	Required if `ruledSurfaceType` is `ALIGNED_WITH_VECTOR` Ruled surface will be aligned with this vector.
`angle`	`ValueWithUnits`	The angle at which the ruled surface meets reference faces or `ruledDirection`. Default is `0`.
`referenceFaces`	`Query`	Required if `ruledSurfaceType` is `ANGLE_FROM_FACE` A set of faces from which to measure `angleFromFaces`.
`vertexOverrides`	`map`
`vertex`	`Query`	A vertex on the path where the override is applied.
`ruledDirection`	`Vector`	If specified, override will specify local direction of ruled surface along this vector.
`width`	`ValueWithUnits`	Required if `ruledDirection` != undefined or `angleFromFaces` != undefined Width of ruled surface at this override.
`angleFromFaces`	`ValueWithUnits`	If specified, override will specify direction as an angle to reference faces. This is only applicable if angleFromFaces is also specified at the top level.
`upToEntity`	`Query`	If specified, override will specify that ruled surface touches upToEntity at override.

opShell (context is Context, id is Id, definition is map)

Create a shell of a solid body with uniform thickness. The bodies that are passed in are hollowed, omitting the walls on the face entities passed in.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	The faces to shell and solid bodies to hollow.
`thickness`	`ValueWithUnits`	The distance by which to shell. Positive means shell outward, and negative means shell inward.

opSplitPart (context is Context, id is Id, definition is map)

Split solid, sheet, and wire bodies with the given sheet body.

Parameter	Type	Additional Info
`definition`	`map`
`targets`	`Query`	The solid, sheet, and wire bodies to split.
`tool`		A sheet body, a construction plane or a face to cut with. Can be either a `Query` or a `Plane`. If a planar face is passed in, the split will extend the plane infinitely unless `useTrimmed` is `true`.
`keepTools`	`boolean`	Optional If false, the tool is deleted. Default is `false`.
`keepType`	`SplitOperationKeepType`	Optional Controls which pieces to keep. Default is `KEEP_ALL`.
`useTrimmed`	`boolean`	Optional If true, the trimmed face boundaries are used as the tool, rather than the underlying surface. Default is `false`.

opSplitFace (context is Context, id is Id, definition is map)

Split faces with the given edges or faces.

Parameter	Type	Additional Info
`definition`	`map`
`faceTargets`	`Query`	The faces to split.
`edgeTools`	`Query`	Optional The edges to cut with.
`projectionType`	`ProjectionType`	Optional Edge projection method. Default is `ProjectionType.NORMAL_TO_TARGET`
`direction`	`Vector`	Required if `edgeTools` are present and `projectionType` is `ProjectionType.DIRECTION`. The projection direction.
`faceTools`	`Query`	Optional The faces to cut with.
`bodyTools`	`Query`	Optional The sheet or wire bodies to cut with.
`keepToolSurfaces`	`boolean`	Optional If `true`, the `bodyTools` do not get consumed by the operation. Default is `true`.
`planeTools`	`Query`	Optional These planar faces are treated as infinite, rather than bounded to the face extents.
`extendToCompletion`	`boolean`	Optional if `true`, imprinted edges are extended to complete split of faces. Default is `false`.
`mutualImprint`	`boolean`	Optional if `true` and only `bodyTools` are supplied target faces are used to split faces of `bodyTools`. Default is `false`.

SplitByIsoclineResult type

Map containing the results of splitting faces by their isoclines. Some faces may have been split, others may have been left intact.

Value	Type	Description
`SplitByIsoclineResult`	`map`
`steepFaces`	`array`	An array of steep faces.
`nonSteepFaces`	`array`	An array of non-steep faces.
`boundaryEdges`	`array`	An array of edges at the transition from non-steep faces to steep faces.

opSplitByIsocline (context is Context, id is Id, definition is map)

Split the given faces by isocline edges. Each isocline follows a path along a face with a constant angle in the (-90, 90) degree range (e.g., lines of latitude on a sphere). This angle is the face tangent plane's angle with respect to the direction with its sign determined by the dot product of direction and the face normal, and is analogous to the angle used in draft analysis. Depending on the face geometry, there may be zero, one, or multiple isoclines on each face. The isocline edges are created as new edges which split the provided faces. The resulting faces are either steep (i.e., the angle is less than the input angle) or non-steep. To instead leave the original faces intact, you can first extract the faces with opExtractSurface(), and create isoclines on the resulting surfaces. The isocline edges can be queried for with qCreatedBy. The split orientation is consistent such that the non-steep faces are always in "front" of the split, and can be reliably queried for with qSplitBy:

EXAMPLE

const isoclineEdges = qCreatedBy(id + "splitByIsocline1", EntityType.EDGE);
const steepFaces = qSplitBy(id + "splitByIsocline1", EntityType.FACE, true);
const nonSteepFaces = qSplitBy(id + "splitByIsocline1", EntityType.FACE, false);
Note that qSplitBy will return only those faces that were split, while the returned SplitByIsoclineResult will include the intact faces as well.

Parameter	Type	Additional Info
`definition`	`map`
`faces`	`Query`	The faces on which to imprint isoclines.
`direction`	`Vector`	A reference direction.
`angle`	`ValueWithUnits`	The isocline angle with respect to the direction in the (-90, 90) degree range.

SplitBySelfShadowResult type

Map containing the results of splitting bodies by their shadow curves. Some faces may have been split, others may have been left intact.

Value	Type	Description
`SplitBySelfShadowResult`	`map`
`visibleFaces`	`array`	An array of visible faces.
`invisibleFaces`	`array`	An array of invisible faces.

opSplitBySelfShadow (context is Context, id is Id, definition is map)

Splits the faces of the given bodies into visible and invisible regions with respect to the given viewDirection, creating shadow curves as necessary. A shadow curve represents the transition of one face from visible to invisible. Depending on the geometry, there may be zero, one, or more shadow curves per face. The shadow curve edges are created as new edges which split the faces of the provided bodies. Each of the resulting faces is wholly visible or wholly invisible. Edge-on faces are considered invisible. The shadow curve edges can be queried for with qCreatedBy. The split orientation is consistent such that the visible faces are always in "front" of the split, and can be reliably queried for with qSplitBy:

EXAMPLE

const shadowEdges = qCreatedBy(id + "splitBySelfShadow1", EntityType.EDGE);
const invisibleFaces = qSplitBy(id + "splitBySelfShadow1", EntityType.FACE, true);
const visibleFaces = qSplitBy(id + "splitBySelfShadow1", EntityType.FACE, false);
Note that qSplitBy will return only those faces that were split, while the returned SplitBySelfShadowResult will include the intact faces as well.

Parameter	Type	Additional Info
`definition`	`map`
`bodies`	`Query`	The bodies which cast shadows and on which to imprint shadow curves.
`viewDirection`	`Vector`	The viewing direction.

opSweep (context is Context, id is Id, definition is map)

Sweep the given edges and faces along a path resulting in solid and/or sheet bodies.

Parameter	Type	Additional Info
`definition`	`map`
`profiles`	`Query`	Edges and faces to sweep.
`path`	`Query`	Edges that comprise the path along which to sweep. The edges can be in any order but must form a connected path.
`keepProfileOrientation`	`boolean`	Optional If `true`, the profile maintains its original orientation as it is swept. If `false` (default), the profile rotates to remain normal to the path.
`lockFaces`	`Query`	Optional Keep profile aligned to the normals of these faces.
`lockDirection`	`Query`	Optional Keep profile perpendicular to this direction.
`profileControl`	`ProfileControlMode`	Optional Default is NONE EXAMPLE `ProfileControlMode.KEEP_ORIENTATION` the profile maintains its original orientation as it is swept. EXAMPLE `ProfileControlMode.LOCK_DIRECTION` the profile is perpendicular to given direction. EXAMPLE `ProfileControlMode.LOCK_FACES` the profile is aligned to the normals of given faces.

opThicken (context is Context, id is Id, definition is map)

Thicken sheet bodies and faces into solid bodies.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	The sheet bodies and faces to thicken.
`thickness1`	`ValueWithUnits`	The distance by which to thicken in the direction along the normal.
`thickness2`	`ValueWithUnits`	The distance by which to thicken in the opposite direction.
`keepTools`	`boolean`	Optional Default is `true`. If `false` the operation will attempt to delete the `entities`. The operation will not delete sheet bodies unless the sheet body or all faces of the sheet body are selected. The operation will not delete sketches or solid bodies.

opTransform (context is Context, id is Id, definition is map)

Applies a given transform to one or more bodies. To make transformed copies of bodies, use opPattern.

Parameter Type Additional Info

definition map

bodies

Query

The bodies to transform.

transform

Transform

The transform to apply.

EXAMPLE

transform(vector(0, 0, 1) * inch) will translate the body 1 inch along the world's z-axis.

EXAMPLE

rotationAround(myLine, 30 * degree) will rotate around a Line object.

EXAMPLE

scaleUniformly(factor) will scale uniformly about the origin.

EXAMPLE

scaleUniformly(factor, point) will scale uniformly about a given point.

EXAMPLE

toWorld(cSys) will (somewhat counterintuitively) perform a transform such that geometry on the world's origin and axes will move to the cSys origin and axes.

EXAMPLE

fromWorld(cSys) will (somewhat counterintuitively) perform a transform such that geometry on the cSys origin and axes will move to the world origin and axes.

EXAMPLE

transform2 * transform1 will perform transform1, followed by transform2.

opWrap (context is Context, id is Id, definition is map)

Wraps or unwraps faces from one surface onto another. The location and orientation of the wrapped faces on the destination surface are controlled by the anchorPoint and anchorDirection of the source and destination WrapSurfaces. The entities of the operation are not affected, the result of this operation is a new set of surface bodies or imprinted edges representing the wrapped or unwrapped faces. Faces that are topologically connected will remain topologically connected in the result body for WrapType.SIMPLE and WrapType.TRIM. This operation currently supports wrapping from a plane onto a cylinder, and unwrapping from a cylinder onto a plane.

(Formerly opRoll)

Parameter	Type	Additional Info
`definition`	`map`
`wrapType`	`WrapType`	The type of wrap to execute. EXAMPLE `WrapType.SIMPLE` wraps `entities` around the infinite definition of `destination`.
`entities`	`Query`	Faces to wrap from `source` to `destination`.
`source`	`WrapSurface`	The surface to wrap from. All `entities` must lie on this surface.
`destination`	`WrapSurface`	The surface to wrap onto. Must be defined using the `face` field for `WrapType.TRIM` or `WrapType.IMPRINT`.
`orientWithDestination`	`boolean`	Optional If true (default), the normals of the resulting surface will point in the same direction as the `destination`. If false, the normals of the resulting surface will point in the opposite direction. For the purpose of this parameter, the normals of a `WrapSurface` defined by an infinite `Cylinder` are always pointing outwards.

primitives

cube (context is Context, id is Id, definition is map)

Create a cube of a specified size, with one corner on the origin.

Parameter Type Additional Info

definition map

sideLength

ValueWithUnits

EXAMPLE

1 * inch

sphere (context is Context, id is Id, definition is map)

Feature creating a sphere. Internally, calls opSphere.

Parameter Type Additional Info

definition map

center

Query

A vertex query marking the sphere's center.

radius

ValueWithUnits

EXAMPLE

1 * inch

fCuboid (context is Context, id is Id, definition is map)

Create a simple rectangular prism between two specified corners.

Parameter Type Additional Info

definition map

corner1

Vector

EXAMPLE

vector(0, 0, 0) * inch

corner2

Vector

EXAMPLE

vector(1, 1, 1) * inch

fCylinder (context is Context, id is Id, definition is map)

Create a simple cylindrical solid between two points, with a specified radius.

Parameter	Type	Additional Info
`definition`	`map`
`topCenter`	`Vector`	A 3D length vector in world space. EXAMPLE `vector(0, 0, 0) * inch`
`bottomCenter`	`Vector`	A 3D length vector in world space. EXAMPLE `vector(1, 1, 1) * inch`
`radius`	`ValueWithUnits`	EXAMPLE `1 * inch`

fCone (context is Context, id is Id, definition is map)

Create a solid cone, possibly truncated.

Parameter	Type	Additional Info
`definition`	`map`
`topCenter`	`Vector`	EXAMPLE `vector(1, 1, 1) * inch`
`bottomCenter`	`Vector`	EXAMPLE `vector(0, 0, 0) * inch`
`topRadius`	`ValueWithUnits`	The radius at the top center. EXAMPLE `1 * inch`
`bottomRadius`	`ValueWithUnits`	The radius at the bottom center. EXAMPLE `0 * inch` produces a standard, non-truncated cone.

fEllipsoid (context is Context, id is Id, definition is map)

Create an ellipsoid (that is, a sphere scaled independently along the three major axes).

Parameter Type Additional Info

definition map

center

Vector

EXAMPLE

vector(0, 0, 0) * inch

radius

Vector

The three radii, as measured along the x, y, and z axes.

EXAMPLE

vector(0.5 * inch, 1 * inch, 2 * inch)

sketch

Functions used to create sketches, and add entities to sketches.

A sketch used in FeatureScript generally has the following form:

var sketch1 = newSketch(context, id + "sketch1", {
        "sketchPlane" : qCreatedBy(makeId("Top"), EntityType.FACE)
});
skRectangle(sketch1, "rectangle1", {
        "firstCorner" : vector(0, 0),
        "secondCorner" : vector(1, 1)
});
skSolve(sketch1);
extrude(context, id + "extrude1", {
        "entities" : qSketchRegion(id + "sketch1"),
        "endBound" : BoundingType.BLIND,
        "depth" : 0.5 * inch
});

A Sketch object should always be created first, with either newSketch or newSketchOnPlane.

Next, any number of sketch entities may be added to the sketch using the functions in this module. The inputs to sketch functions usually involve 2D Vectors, which are positions relative to the sketch plane's origin and x-axis. To create such a point based on a projected 3D point in world space, use worldToPlane(Plane, Vector).

When building sketches in FeatureScript, constraints may be added, but are almost always unnecessary, since you already have the ability to place the entities precisely where you intend them to be.

Finally, the sketch is solved and added to the context by calling skSolve. As a result of skSolve, all edges of the sketch will become WIRE bodies in the context. Any regions enclosed in the sketch will become SURFACE bodies in the context. Any vertices which are not edge endpoints (such as points created by skPoint or the center point of skCircle) will become POINT bodies in the context. These newly created bodies can be queried for and used in all subsequent operations and features.

Sketch type

A Sketch object represents a Onshape sketch, to which sketch entities can be added.

Sketches can be created by calls to newSketch or newSketchOnPlane.

canBeSketch (value) predicate

Typecheck for builtin Sketch

isIdForSketch (context is Context, id is Id)

Check whether an Id represents a Sketch operation.

newSketch (context is Context, id is Id, value is map) returns Sketch

Create a new sketch on an existing planar entity. The sketch coordinate system follows the canonical plane orientation and the sketch origin is the projection of the world origin onto the plane.

To make a sketch in the coordinate system of an arbitrary Plane, use newSketchOnPlane.

Parameter Type Additional Info

value map

sketchPlane

Query

A Query for a single, planar entity.

EXAMPLE

qCreatedBy(makeId("Top"), EntityType.FACE) to sketch on default "Top" plane.

disableImprinting

boolean

Optional

Prevents sketchPlane from imprinting on the sketch. Default is false.

newSketchOnPlane (context is Context, id is Id, value is map) returns Sketch

Create a new sketch on a custom plane, specified by a Plane object. The sketch coordinate system will match the coordinate system of the plane.

Parameter Type Additional Info

value map

sketchPlane

Plane

EXAMPLE

plane(vector(0, 0, 0) * inch, vector(0, 0, 1)) to sketch on the world XY plane.

skSolve (sketch is Sketch)

Solve any constraints in the sketch and add all sketch entities form the sketch to its context.

Even if there are no constraints, a sketch must be solved before its entities are created.

skPoint (sketch is Sketch, pointId is string, value is map) returns map

Add a point to a sketch.

Parameter Type Additional Info

value map

position

Vector

EXAMPLE

vector(0, 1) * inch

Return	Type	Description
	`map`
`pointId`

skLineSegment (sketch is Sketch, lineId is string, value is map) returns map

Add a line segment to a sketch.

Parameter	Type	Additional Info
`value`	`map`
`start`	`Vector`	EXAMPLE `vector(0, 0) * inch`
`end`	`Vector`	EXAMPLE `vector(1, 1) * inch`
`construction`	`boolean`	Optional `true` for a construction line

Return	Type	Description
	`map`
`startId`
`endId`

skText (sketch is Sketch, textId is string, value is map) returns map

Add a text rectangle to a sketch.

Parameter	Type	Additional Info
`value`	`map`
`text`	`string`	A string of text to write. May contain newlines (encoded as `\n`).
`fontName`	`string`	A font name, with extension ".ttf" or ".otf". To change font weight, replace "-Regular" with "-Bold", "-Italic", or "-BoldItalic". Must be one of the following fonts: EXAMPLE `"OpenSans-Regular.ttf"` Sans-serif font. Default if no match is found. EXAMPLE `"AllertaStencil-Regular.ttf"` Stencil font. No bold/italic options. EXAMPLE `"Arimo-Regular.ttf"` Sans-serif font. EXAMPLE `"DroidSansMono.ttf"` Monospaced sans-serif font. No bold/italic options. EXAMPLE `"NotoSans-Regular.ttf"` Sans-serif font. EXAMPLE `"NotoSansCJKjp-Regular.otf"` Japanese font. No italic options. EXAMPLE `"NotoSansCJKkr-Regular.otf"` Korean font. No italic options. EXAMPLE `"NotoSansCJKsc-Regular.otf"` Chinese (simplified) font. No italic options. EXAMPLE `"NotoSansCJKtc-Regular.otf"` Chinese (traditional) font. No italic options. EXAMPLE `"NotoSerif-Regular.ttf"` Serif font. EXAMPLE `"RobotoSlab-Regular.ttf"` Sans-serif font. No italic options. EXAMPLE `"Tinos-Regular.ttf"` Serif font. Metrically compatible with Times New Roman.
`construction`	`boolean`	Optional `true` for a construction line
`firstCorner`	`Vector`	Optional One corner of the rectangle into which the text will be placed. Text will start at the left of the rectangle and extend to the right, overflowing the right if necessary. The first line of text will fill the height of the rectangle, with subsequent lines below the rectangle (or above if mirrored vertically). EXAMPLE `vector(0, 0) * inch`
`secondCorner`	`Vector`	Optional The other corner of the rectangle into which the text will be placed. Text will start at the left of the rectangle and extend to the right, overflowing the right if necessary. The first line of text will fill the height of the rectangle, with subsequent lines below the rectangle (or above if mirrored vertically). EXAMPLE `vector(1, 1) * inch`
`mirrorHorizontal`	`boolean`	Optional `true` for flipping text horizontally
`mirrorVertical`	`boolean`	Optional `true` for flipping text vertically

Return	Type	Description
	`map`
`textId`

skImage (sketch is Sketch, imageId is string, value is map) returns map

Add an image rectangle and return ids of corner points.

To use an image uploaded in your document, import the image (possibly into a namespace).

Parameter	Type	Additional Info
`value`	`map`
`blobInfo`	`map`	EXAMPLE `BLOB_DATA` will use the image from an image file imported into this Feature Studio. EXAMPLE `MyImage::BLOB_DATA` will use an image imported into the namespace `MyImage` (e.g. using `MyImage::import(...)`)
`firstCorner`	`Vector`	One corner of the rectangle into which the image will be placed. EXAMPLE `vector(0, 0) * inch`
`secondCorner`	`Vector`	The other corner of the rectangle into which the image will be placed. EXAMPLE `vector(1, 1) * inch`

Return	Type	Description
	`map`
`imageId`

skCircle (sketch is Sketch, circleId is string, value is map) returns map

Add a circle to a sketch.

Parameter	Type	Additional Info
`value`	`map`
`center`	`Vector`	EXAMPLE `vector(0, 0) * inch`
`radius`	`ValueWithUnits`	EXAMPLE `1 * inch`
`construction`	`boolean`	Optional `true` for a construction line

Return	Type	Description
	`map`
`centerId`

skEllipse (sketch is Sketch, ellipseId is string, value is map) returns map

Add an ellipse to a sketch.

Parameter	Type	Additional Info
`value`	`map`
`center`	`Vector`	EXAMPLE `vector(0, 0) * inch`
`majorRadius`	`ValueWithUnits`	EXAMPLE `2 * inch`
`minorRadius`	`ValueWithUnits`	EXAMPLE `1 * inch`
`majorAxis`	`Vector`	Optional A unitless 2D direction, specifying the orientation of the major axis
`construction`	`boolean`	Optional `true` for a construction line

Return	Type	Description
	`map`
`centerId`

skArc (sketch is Sketch, arcId is string, value is map) returns map

Add an arc through three points to a sketch.

Parameter	Type	Additional Info
`value`	`map`
`start`	`Vector`	EXAMPLE `vector(1, 0) * inch`
`mid`	`Vector`	EXAMPLE `vector(0, 1) * inch`
`end`	`Vector`	EXAMPLE `vector(-1, 0) * inch`
`construction`	`boolean`	Optional `true` for a construction line

Return	Type	Description
	`map`
`startId`
`endId`

skEllipticalArc (sketch is Sketch, arcId is string, value is map) returns map

Add an elliptical arc to a sketch. The ellipse has a period of 1, a parameter of 0 at the major axis and 0.25 at the minor axis. The arc is drawn counterclockwise from the start point to the end point.

Parameter	Type	Additional Info
`value`	`map`
`center`	`Vector`	EXAMPLE `vector(0, 0) * inch`
`majorAxis`	`Vector`	The direction, in sketch coordinates, in which the major axis of the ellipse lies. EXAMPLE `normalize(vector(1, 1))`
`minorRadius`	`ValueWithUnits`	A non-negative value with length units. EXAMPLE `1 * inch`
`majorRadius`	`ValueWithUnits`	A non-negative value with length units. Does not need to be greater than the minor radius. EXAMPLE `2 * inch`
`startParameter`	`number`	The parameter of the start point. EXAMPLE `0`
`endParameter`	`number`	The parameter of the end point. EXAMPLE `0.25`
`construction`	`boolean`	Optional `true` for a construction line

Return	Type	Description
	`map`
`startId`
`endId`

skFitSpline (sketch is Sketch, splineId is string, value is map)

Create an interpolated spline through the given points.

Parameter	Type	Additional Info
`value`	`map`
`points`		An array of points. If the start and end points are the same, the spline is closed. EXAMPLE [ vector( 0, 0) * inch, vector( 0, -1) * inch, vector( 1, 1) * inch, vector(-1, 0) * inch, vector( 0, 0) * inch ]
`parameters`		Optional An array of doubles, parameters corresponding to the points.
`construction`	`boolean`	Optional `true` for a construction line
`startDerivative`	`Vector`	Optional A 2D `Vector` with length units that specifies the derivative at the start of the resulting spline. Ignored if spline is closed.
`endDerivative`	`Vector`	Optional A 2D `Vector` with length units that specifies the derivative at the end of the resulting spline. Ignored if spline is closed.

skBezier (sketch is Sketch, bezierId is string, value is map)

Create a Bezier curve from the given control points.

Parameter Type Additional Info

value map

points

An array of points.

EXAMPLE

[
       vector( 0, 0) * inch,
       vector( 0, 1) * inch,
       vector( 1, 1) * inch,
       vector( 1, 0) * inch
]

construction

boolean

Optional

true for a construction line

skRectangle (sketch is Sketch, rectangleId is string, value is map)

Add a rectangle (four line segments, properly constrained) to a sketch.

Parameter	Type	Additional Info
`value`	`map`
`firstCorner`	`Vector`	EXAMPLE `vector(0, 0) * inch`
`secondCorner`	`Vector`	EXAMPLE `vector(1, 1) * inch`
`construction`	`boolean`	Optional `true` for a construction line

skRegularPolygon (sketch is Sketch, polygonId is string, value is map)

Add a regular polygon to the sketch. Unconstrained.

Parameter	Type	Additional Info
`value`	`map`
`center`	`Vector`	EXAMPLE `vector(0, 0) * inch`
`firstVertex`	`Vector`	Distance to the center determines the radius. EXAMPLE `vector(0, 1) * inch`
`sides`	`number`	Number of polygon sides. Must be an integer 3 or greater.
`construction`	`boolean`	Optional `true` for a construction line

skPolyline (sketch is Sketch, polylineId is string, value is map)

Add a polyline (line segments, optionally with constrained endpoints) or a polygon to a sketch.

Parameter	Type	Additional Info
`value`	`map`
`points`	`array`	An array of points, each a `Vector` of two lengths. If first and last point are the same, the polyline is closed. EXAMPLE [ vector( 0, 0) * inch, vector( 0, -1) * inch, vector( 1, 1) * inch, vector(-1, 0) * inch, vector( 0, 0) * inch ]
`construction`	`boolean`	Optional `true` for a construction line. Default false.
`constrained`	`boolean`	Optional `true` if constraints should be created. Default false.

skConstraint (sketch is Sketch, constraintId is string, value is map)

Add a constraint.

Parameter	Type	Additional Info
`value`	`map`
`constraintType`	`ConstraintType`
`length`	`ValueWithUnits`	Optional For constraints that require a length. Must have length units.
`angle`	`ValueWithUnits`	Optional For constraints that require a angle. Must have angle units.

query

Functions for constructing queries. Features that take queries as inputs should re-export this module.

Queries are used to refer to topological entities (vertices, edges, faces, and bodies) that FeatureScript operation and evaluation functions work on. A query is a map that contains instructions for how to find entities. For example, a query for all edges in a context looks like qEverything(EntityType.EDGE). Many queries can take subqueries as arguments, allowing for more complex nested queries.

Queries in general do not contain a list of entities in any form. Rather, they contain criteria that specify a subset of the topological entities in a context. To get an array of the entities (if any) which match a query in a context, use evaluateQuery. There is no need to evaluate a query before passing it into a function, including any of the Standard Library's operation and evaluation functions.

There are two general types of queries: state-based and historical. State-based queries select entities based on the model state, e.g. "All edges adjacent to a cylindrical face which touches this point." Historical queries select entities based on the model history, e.g. "the edge that was generated by feature extrude_1_id from sketch vertex vertex_id from sketch sketch_id." State-based queries cannot refer to entities that have been deleted. Most automatically-generated queries are historical, while queries more commonly used in manually written code are state-based.

Query type

A Query identifies a specific subset of a context's entities (points, lines, planes, and bodies).

The fields on a Query map depend on its QueryType, and may include one or more subqueries.

Value	Type	Description
`Query`	`map`
`queryType`	`QueryType`
`entityType`	`EntityType`	Optional

canBeQuery (value) predicate

Typecheck for Query

BodyType enum

Specifies the topological type of a body.

All bodies have EntityType.BODY, but will generally own many entities of other EntityTypes.

For example, the result of an extrude with NewBodyOperationType.NEW is a body. This body will have BodyType.SOLID for a solid extrude, and BodyType.SHEET for a surface extrude. This extrude operation will create many geometric entities in the context (faces, edges, or vertices), which are owned by the body, and have the BodyType of their owning body.

See also

qBodyType

Value	Description
`SOLID`	A three-dimensional part (e.g. the result of a solid extrude)
`SHEET`	A two-dimensional sheet body (e.g. a sketch region, or the result of a surface extrude)
`WIRE`	A one-dimensional curve (e.g. a sketch line or curve, or the result of opHelix)
`POINT`	A zero-dimensional point (e.g. a sketch point, or the result of opPoint)
`MATE_CONNECTOR`	A part studio mate connector.
`COMPOSITE`	A composite part body, which can contain bodies of any other type

EntityType enum

Specifies the topological type of a given entity. Used in several queries as a filter, or on any query explicitly with qEntityFilter

Thus, one can obtain all the vertices in a part studio with qEverything(EntityType.VERTEX), and can obtain all the vertices attached to solid bodies with qBodyType(qEverything(EntityType.VERTEX), BodyType.SOLID)

A query for every part in a part studio is qBodyType(qEverything(EntityType.BODY), BodyType.SOLID)

Value	Description
`VERTEX`	A zero-dimensional point or vertex
`EDGE`	A one-dimensional line, curve, or edge
`FACE`	A two-dimensional surface, planar face, or non-planar face
`BODY`	A solid, surface, wire, or point body

AdjacencyType enum

Specifies the adjacency type of queried entities.

See also

qAdjacent

Value	Description
`VERTEX`	Entities share at least a vertex
`EDGE`	Entities share at least an edge

GeometryType enum

Specifies the geometric type of queried entities.

See also

qGeometry

Value	Description
`LINE`	A straight line or edge
`CIRCLE`	A circle of constant radius
`ARC`	A segment of a circle
`OTHER_CURVE`	Any one-dimensional entity which is not described above (e.g. splines, ellipses, etc.)
`PLANE`	A construction plane or planar face
`CYLINDER`	A surface which forms the side of a right circular cylinder
`CONE`	A surface which forms the side of a right circular cone
`SPHERE`	A surface which forms the boundary of a sphere
`TORUS`	A surface which forms the boundary of a torus
`REVOLVED`	A surface constructed by revolving a curve around an axis (unless it is simplified to one of the types above)
`EXTRUDED`	A surface constructed by extruding or sweeping a curve along a line (unless it is simplified to one of the types above)
`OTHER_SURFACE`	Any two-dimensional entity which is not described above (e.g. the side of an arbitrary loft)
`ALL_MESH`	A surface or a body that is fully mesh or an edge between two mesh surfaces.
`MIXED_MESH`	A body that contains both mesh and non-mesh surfaces or an edge between a mesh and a non-mesh surfaces.
`MESH`	A surface that is mesh, a body that contains mesh surfaces or an edge bordering a mesh surface.

CapType enum

Specifies which cap queried entities should belong to.

See also

qCapEntity

Value	Description
`START`	finds entities belonging to the start cap
`END`	finds entities belonging to the end cap
`EITHER`	finds entities belonging to either cap

ConstructionObject enum

Specifies whether the entity was created for construction (e.g. a construction line or construction plane).

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Edges to use", "Filter" : EntityType.EDGE && ConstructionObject.NO }
definition.edges is Query;

See also

qConstructionFilter

Value	Description
`YES`	Matches only entities which are created for construction
`NO`	Matches only entities which are not created for construction

SMFlatType enum

Specifies whether an entity appears in the sheet metal flat view, or the main view.

See also

qSheetMetalFlatFilter

Value	Description
`YES`	Matches entities which belong to a flattened sheet metal part.
`NO`	Matches entities which do not belong to a flattened sheet metal part.

AllowMeshGeometry enum

Specifies whether we allow meshes. Default is NO.

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Bodies", "Filter" : EntityType.BODY && AllowMeshGeometry.YES }
definition.body is Query;

Value	Description
`YES`	Allow meshes
`NO`	Disallow meshes

AllowFlattenedGeometry enum

Specifies whether we allow flat entities. Default is NO.

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Bodies", "Filter" : EntityType.BODY && AllowFlattenedGeometry.YES }
definition.body is Query;

Value	Description
`YES`	Allow flat entities
`NO`	Disallow flat entities

ActiveSheetMetal enum

Specifies whether the entities should belong to an active sheet metal model.

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Sheet metal bodies", "Filter" : EntityType.BODY && ActiveSheetMetal.YES }
definition.body is Query;

Value	Description
`YES`	matches only entities which belong to an active sheet metal model
`NO`	matches only entities which do not belong to an active sheet metal model

SheetMetalDefinitionEntityType enum

Specifies geometry corresponding to a certain type of topological entity in the sheet metal master body for active sheet metal models.

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Sheet metal definition edges", "Filter" : SheetMetalDefinitionEntityType.EDGE }
definition.entities is Query;

Value	Description
`VERTEX`	matches entities defined by a sheet metal master body vertex. This includes vertices, edges, and faces at the corners, bend ends, fillets, and chamfers of sheet metal models.
`EDGE`	matches entities defined by a sheet metal master body edge. This includes edges and faces along the sides of sheet metal walls.
`FACE`	matches entities defined by a sheet metal master body face. This includes faces of sheet metal walls.

ModifiableEntityOnly enum

Specifies whether we allow modifiable only entities. It is default to NO.

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Bodies", "Filter" : EntityType.BODY && ModifiableEntityOnly.YES }
definition.body is Query;

See also

qModifiableEntityFilter

Value	Description
`YES`	Only allow modifiable entities
`NO`	Allow both modifiable and unmodifiable entities

AllowEdgePoint enum

Specifies whether we allow edge points. Default is YES.

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Corners", "Filter" : EntityType.VERTEX && AllowEdgePoint.NO }
definition.body is Query;

Value	Description
`YES`	Allow edge points
`NO`	Disallow edge points

MeshGeometry enum

Specifies whether the entities are mesh geometries.

See also

qMeshGeometryFilter

Value	Description
`YES`	Matches only entities (edges, faces, and bodies) which are meshes
`NO`	Matches only entities (edges, faces, and bodies) which are not meshes

SketchObject enum

Specifies whether the entity is a part of a sketch.

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Sketch curves", "Filter" : EntityType.EDGE && SketchObject.YES }
definition.curves is Query;

See also

qSketchFilter

Value	Description
`YES`	Matches only entities which are part of a sketch
`NO`	Matches only entities which are not part of a sketch

QueryFilterCompound enum

A set of convenience filters, which are expanded during precondition processing. Can be used as a filter on query parameters, just like their corresponding expansions:

annotation { "Name" : "Axis", "Filter" : QueryFilterCompound.ALLOWS_AXIS }
definition.axis is Query;

Value	Description
`ALLOWS_AXIS`	Equivalent to `GeometryType.LINE \|\| GeometryType.CIRCLE \|\| GeometryType.ARC \|\| GeometryType.CYLINDER \|\| BodyType.MATE_CONNECTOR` and can be processed with `evAxis`
`ALLOWS_DIRECTION`	Equivalent to `GeometryType.LINE \|\| GeometryType.CIRCLE \|\| GeometryType.ARC \|\| GeometryType.CYLINDER \|\| GeometryType.PLANE` and can be processed with `extractDirection`
`ALLOWS_PLANE`	Equivalent to `GeometryType.PLANE \|\| BodyType.MATE_CONNECTOR` and can be processed with `evPlane`
`ALLOWS_VERTEX`	Equivalent to `EntityType.VERTEX \|\| BodyType.MATE_CONNECTOR` and can be processed with `evVertexPoint`

CompareType enum

Specifies a method of comparing two items.

See also

qFilletFaces

Value	Description
`EQUAL`
`LESS`
`LESS_EQUAL`
`GREATER`
`GREATER_EQUAL`

Consumed enum

Specifies whether to filter or allow bodies (and their vertices, edges, and faces) consumed by closed composite parts.

See also

qConsumed

Value	Description
`YES`	Matches only bodies that are consumed
`NO`	Matches only bodies that are not consumed

CompositePartType enum

Specifies whether to filter or allow closed or open composite parts.

See also

qCompositePartTypeFilter

Value	Description
`OPEN`	Matches only open composite parts
`CLOSED`	Matches only closed composite parts

InContextObject enum

Specifies whether an entity is from an assembly context.

Can be used in a filter on a query parameter to only allow certain selections:

annotation { "Name" : "Edges to use", "Filter" : EntityType.EDGE && InContextObject.NO }
definition.edges is Query;

Value	Description
`YES`	Matches only entities which are from an assembly context
`NO`	Matches only entities which are not from an assembly context

qNothing () returns Query

An empty query, which does not resolve to any entities.

qEverything (entityType is EntityType) returns Query

A query for all entities of a specified EntityType in the context.

See also

qAllModifiableSolidBodies

Parameter	Type	Additional Info
`entityType`	`EntityType`	Optional

qEverything () returns Query

A query for all entities in the context.

qAllNonMeshSolidBodies () returns Query

A query for all solid bodies that do not have mesh geometry.

qAllSolidBodies () returns Query

A query for all solid bodies.

qAllModifiableSolidBodiesNoMesh () returns Query

A query for all solid bodies that do not have mesh geometry or in context geometry, i.e. every non-mesh-containing part displayed in the Part Studio's "Parts" list.

See also

qAllModifiableSolidBodies

qAllModifiableSolidBodies () returns Query

A query for all modifiable solid bodies, including mesh-containing bodies.

See also

qAllModifiableSolidBodiesNoMesh

qNthElement (queryToFilter is Query, n is number) returns Query

A query for one entity in queryToFilter at a specified index. The order of entities resolved by a query is deterministic but arbitrary.

Parameter Type Additional Info

queryToFilter

Query

A query which resolves to at least n+1 entities

n

number

Zero-based index of entity in queryToFilter.

EXAMPLE

0 indicates the first entity

EXAMPLE

-1 indicates the last entity

qEntityFilter (queryToFilter is Query, entityType is EntityType) returns Query

A query for entities in a queryToFilter which match a given EntityType.

qHasAttribute (name is string) returns Query

Query for all entities marked with an attribute with name name

See also

setAttribute

qHasAttribute (queryToFilter is Query, name is string) returns Query

Query for all entities in queryToFilter marked with an attribute with name name

See also

setAttribute

qHasAttributeWithValue (name is string, value) returns Query

Query for all entities marked with an attribute with name name and value exactly equal to value

See also

setAttribute

qHasAttributeWithValue (queryToFilter is Query, name is string, value) returns Query

Query for all entities in queryToFilter marked with an attribute with name name and value exactly equal to value

See also

setAttribute

qHasAttributeWithValueMatching (name is string, attributePattern is map) returns Query

Query for all entities marked with an attribute with name name and a map value matching every key-value pair in the provided attributePattern map.

See also

setAttribute

Parameter Type Additional Info

attributePattern

map

EXAMPLE

{
    "key1" : valueToMatch,
}

qHasAttributeWithValueMatching (queryToFilter is Query, name is string, attributePattern is map) returns Query

Query for all entities in queryToFilter marked with an attribute with name name and a map value matching every key-value pair in the provided attributePattern map.

See also

setAttribute

Parameter Type Additional Info

attributePattern

map

EXAMPLE

{
    "key1" : valueToMatch,
}

qAttributeFilter (queryToFilter is Query, attributePattern) returns Query

Note: This query is used only for legacy unnamed attributes, which are still supported but no longer reccommended. See the Attributes module for details.

A query for entities in a queryToFilter which have been assigned a legacy unnamed attribute matching a given attributePattern.

Parameter Type Additional Info

attributePattern

Will only resolve to queries whose legacy unnamed attributes match the type (and possibly the values) of this pattern.

If attributePattern has a type tag, will only match attributes with that same type tag.

EXAMPLE

{} as MyCustomType will match all attributes with type tag MyCustomType

If the attribute has no type tag (i.e. it is a standard type like string or map), will match all attributes with that same standard type.

EXAMPLE

"asdf" will match all string attributes.

EXAMPLE

{} will match all map attributes.

If the attribute is a map, will only match maps which have identical values for every key-value pair in the pattern

EXAMPLE

{ "odd" : true } matches all unnamed map attributes that have a field "odd" whose value is true.

EXAMPLE

{ "odd" : true } as MyCustomType matches all unnamed map attributes with the that have a field "odd" whose value is true.

qAttributeQuery (attributePattern) returns Query

Note: This query is used only for legacy unnamed attributes, which are still supported but no longer reccommended. See the Attributes module for details.

A query for all entities which have been assigned a legacy unnamed attribute matching a given attributePattern. Equivalent to qAttributeFilter(qEverything(), attributePattern)

qCreatedBy (featureId is Id, entityType is EntityType) returns Query

A query for all the entities created by a feature or operation. The feature is given by its feature id, which was passed into the the operation function in order to create the feature.

An entity is "created by" an operation if the entity was added to the context as part of that operation. Entities modified, but not created, by an operation are not returned by this query.

If an entity is split (as in a split part operation), the resulting entities are "created by" both the original entity's creator and the split part operation.

If two entities are merged (as in a union of coincident faces), that entity is "created by" the creators of each merged entity, as well as the merging operation itself.

If a sketch's feature id is specified, returns a query for all sketch regions, points, and wire bodies created by the specified sketch.

Parameter Type Additional Info

featureId

Id

The Id of the specified feature.

EXAMPLE

id + "extrude1"

entityType

EntityType

Optional

qCreatedBy (featureId is Id) returns Query

qCreatedBy (features is FeatureList) returns Query

qCreatedBy (features is FeatureList, entityType is EntityType) returns Query

qCapEntity (featureId is Id, capType is CapType, entityType is EntityType) returns Query

A query for start/end cap vertex, edge, and face entities created by featureId. Cap entities are produced by extrude, revolve, sweep, loft and thicken features

Parameter	Type	Additional Info
`entityType`	`EntityType`	Optional

qCapEntity (featureId is Id, capType is CapType) returns Query

qNonCapEntity (featureId is Id, entityType is EntityType) returns Query

A query for vertex, edge, and face entities created by featureId that are not cap entities. Cap entities are produced by extrude, revolve, sweep, loft and thicken features

Parameter	Type	Additional Info
`entityType`	`EntityType`	Optional

qNonCapEntity (featureId is Id) returns Query

qOpHoleProfile (featureId is Id, filters is map) returns Query

A query for the profile edges or vertices created by an opHole operation.

Parameter	Type	Additional Info
`featureId`	`Id`	The `Id` of the specified operation. EXAMPLE `id + "hole1"`
`filters`	`map`
`name`	`string`	Optional Filter the query for profiles with a given name. See `name` field of `HoleProfile`.
`identity`	`Query`	Optional Filter the query for the hole associated with the given identity entity. See `identities` parameter of `opHole`.

qOpHoleProfile (featureId is Id) returns Query

qOpHoleFace (featureId is Id, filters is map) returns Query

A query for the hole faces created by an opHole operation.

Parameter	Type	Additional Info
`featureId`	`Id`	The `Id` of the specified operation. EXAMPLE `id + "hole1"`
`filters`	`map`
`name`	`string`	Optional Filter the query for faces with a given name. See `faceNames` field of `HoleDefinition`.
`identity`	`Query`	Optional Filter the query for the hole associated with the given identity entity. See `identities` parameter of `opHole`.

qOpHoleFace (featureId is Id) returns Query

qToleranceFilter (queryToFilter is Query) returns Query

qUnion (subqueries is array) returns Query

A query for entities which match any of a list of queries.

qUnion is guaranteed to preserve order. That is, entities which match queries earlier in the subqueries input list will also be listed earlier in the output of evaluateQuery.

qUnion (query1 is Query, query2 is Query) returns Query

qUnion (query1 is Query, query2 is Query, query3 is Query) returns Query

qUnion (query1 is Query, query2 is Query, query3 is Query, query4 is Query) returns Query

qIntersection (subqueries is array) returns Query

A query for entities which match all of a list of queries. qIntersection preserves the order of the first subquery.

qIntersection (query1 is Query, query2 is Query) returns Query

qSubtraction (query1 is Query, query2 is Query) returns Query

A query for entities which match query1, but do not match query2. qSubtraction preserves the order of query1.

qSymmetricDifference (query1 is Query, query2 is Query) returns Query

A query for entities which match either query1 or query2, but not both.

qOwnedByBody (body is Query, entityType is EntityType) returns Query

A query for all of the entities (faces, vertices, edges, and bodies) in a context which belong to a specified body or bodies.

Parameter	Type	Additional Info
`entityType`	`EntityType`	Optional

qOwnedByBody (body is Query) returns Query

qOwnedByBody (queryToFilter is Query, body is Query) returns Query

A query for all of the entities which match a queryToFilter, and belong to the specified body or bodies.

qOwnerBody (entities is Query) returns Query

A query for each body that any of the given entities belong to.

If a body is passed in, the result will include that body itself.

qContainedInCompositeParts (compositeParts is Query) returns Query

A query for each part contained in compositeParts.

qCompositePartsContaining (bodies is Query) returns Query

A query for each composite part containing bodies.

qCompositePartsContaining (bodies is Query, compositePartType is CompositePartType) returns Query

A query for each composite part of the given type containing bodies.

qFlattenedCompositeParts (entities is Query) returns Query

A query for non-composite entities in entities and constituents of composite parts in entities.

qConsumed (queryToFilter is Query, consumed is Consumed) returns Query

A query for all entities in queryToFilter which are consumed by any closed composite part, or all entities of queryToFilter which are not consumed by any closed composite part.

qCompositePartTypeFilter (queryToFilter is Query, compositePartType is CompositePartType) returns Query

A query for all bodies in queryToFilter which are either open or closed composite parts, depending on the second parameter.

qSourceMesh (selectedMeshVertices is Query, entityType is EntityType) returns Query

A query for each mesh element that any selectedMeshVertices belong to. selectedMeshVertices should be the point bodies created when a user selects a mesh vertex. Mesh vertices which have not been selected cannot be queried in FeatureScript

Parameter	Type	Additional Info
`selectedMeshVertices`	`Query`	One or more mesh vertices whose owning elements are queried.
`entityType`	`EntityType`	The type of resulting entities. Can be EntityType.BODY, EntityType.FACE or EntityType.EDGE.

qSourceMesh (selectedMeshVertices is Query) returns Query

Deprecated: Use qSourceMesh with EntityType.BODY

qAdjacent (seed is Query, adjacencyType is AdjacencyType, entityType is EntityType) returns Query

A query for entities that are adjacent to the given seed entities.

Parameter Type Additional Info

seed

Query

One or more entities whose adjacent neighbors are queried. The result does not include the original seed entities (unless they are adjacent to other seed entities)

adjacencyType

AdjacencyType

EXAMPLE

AdjacencyType.VERTEX will return entities that share at least a vertex with the seed entities.

EXAMPLE

AdjacencyType.EDGE will return entities that share at least an edge with the seed entities. For example, qAdjacent(whiteSquareOnChessBoard, AdjacencyType.EDGE) would return all four surrounding black squares, but not the four diagonal white squares.

entityType

EntityType

Optional

The type of resulting entities

qAdjacent (seed is Query, adjacencyType is AdjacencyType) returns Query

qVertexAdjacent (query is Query, entityType is EntityType) returns Query

Deprecated: Use qAdjacent with AdjacencyType.VERTEX

qEdgeAdjacent (query is Query, entityType is EntityType) returns Query

Deprecated: Use qAdjacent with AdjacencyType.EDGE

qEdgeTopologyFilter (queryToFilter is Query, edgeTopologyType is EdgeTopology) returns Query

A query for edges in a queryToFilter which match a given EdgeTopology.

qEdgeVertex (edgeQuery is Query, atStart is boolean)

A query for the start or end vertices of edges.

qGeometry (queryToFilter is Query, geometryType is GeometryType) returns Query

A query for all entities in queryToFilter with a specified GeometryType.

qBodyType (queryToFilter is Query, bodyType is BodyType) returns Query

A query for all entities in queryToFilter which are bodies of the a specified BodyType, or are owned by bodies with the specified BodyType

qBodyType (queryToFilter is Query, bodyTypes is array) returns Query

A query for all entities in queryToFilter with any of a list of BodyTypes.

Parameter	Type	Additional Info
`bodyTypes`	`array`	An array of `BodyType`s.

qConstructionFilter (queryToFilter is Query, constructionFilter is ConstructionObject) returns Query

A query for all construction entities or all non-construction entities in queryToFilter.

See also

ConstructionObject

qActiveSheetMetalFilter (queryToFilter is Query, activeSheetMetal is ActiveSheetMetal) returns Query

A query for all entities in queryToFilter belonging to an active sheet metal part.

See also

ActiveSheetMetal

qSheetMetalFlatFilter (queryToFilter is Query, filterFlat is SMFlatType) returns Query

A query for all entities in queryToFilter belonging to a flattened sheet metal part.

See also

SMFlatType

qSMFlatFilter (subquery is Query, filterFlat is SMFlatType) returns Query

Deprecated: Use qSheetMetalFlatFilter

qPartsAttachedTo (sheetMetalEntities is Query) returns Query

A query for parts to which sheetMetalEntities are attached (e.g. sheet metal bend line entities are attached to a flattened sheet metal part)

qCorrespondingInFlat (entitiesInFolded is Query) returns Query

A query for entities in sheet metal flattened body corresponding to any entitiesInFolded which are part of 3D sheet metal bodies

qMeshGeometryFilter (queryToFilter is Query, meshGeometryFilter is MeshGeometry) returns Query

A query for all mesh entities or all non-mesh entities in queryToFilter.

A body is considered a "mesh entity" if any of its faces or edges have mesh geometry.

See also

MeshGeometry

qModifiableEntityFilter (queryToFilter is Query) returns Query

A query for all modifiable entities in queryToFilter.

An entity is considered non-modifiable if it is an in-context entity.

See also

ModifiableEntityOnly

qAllModifiableSolidBodies

qSketchFilter (queryToFilter is Query, sketchObjectFilter is SketchObject) returns Query

A query for all sketch entities, or all non-sketch entities in queryToFilter.

qParallelPlanes (queryToFilter is Query, referencePlane is Plane, allowAntiparallel is boolean) returns Query

A query for all planar face entities that are parallel to the referencePlane.

Parameter	Type	Additional Info
`referencePlane`	`Plane`	The plane to reference when checking for parallelism.
`allowAntiparallel`	`boolean`	Whether to also return entities that are antiparallel.

qParallelPlanes (queryToFilter is Query, referencePlane is Plane) returns Query

A query for all planar face entities in queryToFilter that are parallel to the referencePlane.

Parameter	Type	Additional Info
`referencePlane`	`Plane`	The plane to reference when checking for parallelism.

qParallelPlanes (queryToFilter is Query, normal is Vector, allowAntiparallel is boolean) returns Query

A query for all planar face entities in queryToFilter that are parallel to a plane specified by the normal vector.

Parameter	Type	Additional Info
`normal`	`Vector`	The normal vector to reference when checking for parallelism.
`allowAntiparallel`	`boolean`	Whether to also return entities that are antiparallel.

qPlanesParallelToDirection (queryToFilter is Query, direction is Vector) returns Query

A query for all planar faces in queryToFilter that are parallel to the given direction vector (i.e., the plane normal is perpendicular to direction).

qFacesParallelToDirection (queryToFilter is Query, direction is Vector) returns Query

A query for all faces in queryToFilter that are parallel to the given direction vector e.g. if it is a planar face, the plane normal is perpendicular to direction if it is a cylindrical face, the axis is parallel to direction if it is an extruded face, the extrude direction is parallel to direction

qParallelPlanes (queryToFilter is Query, normal is Vector) returns Query

A query for all planar face entities in queryToFilter that are parallel to a plane specified by the normal vector.

Parameter	Type	Additional Info
`normal`	`Vector`	The normal vector to reference when checking for parallelism.

qConvexConnectedFaces (seed is Query) returns Query

A query for a set of faces connected to seed via convex edges, flood-filling across any number of convex edges.

A convex edge is an edge which forms a convex angle along the full length of the edge. A convex angle is strictly less than 180 degrees for flat faces, or faces with negative curvature. If one face has positive curvature, and the other has flat or positive curvature, a convex angle is less than or equal to 180 degrees. Thus, the two bounding edges of an exterior fillet are considered convex.

qConcaveConnectedFaces (seed is Query) returns Query

A query for a set of faces connected to seed via concave edges, flood-filling across any number of concave edges.

A concave edge is an edge which forms a concave angle along the full length of the edge. A concave angle is strictly greater than 180 degrees for flat faces, or faces with positive curvature. If one face has negative curvature, and the other has flat or negative curvature, a concave angle is less than or equal to 180 degrees. Thus, the two bounding edges of an interior fillet are considered concave.

qTangentConnectedFaces (seed is Query) returns Query

A query for a set of faces connected to seed via tangent edges, flood-filling across any number of tangent edges.

A tangent edge is an edge joining two faces such that the surface direction is continuous across the edge, at every point along the full length of the edge.

qTangentConnectedFaces (seed is Query, angleTolerance is ValueWithUnits) returns Query

A query for a set of faces connected to seed via tangent edges, flood-filling across any number of tangent edges.

A tangent edge is an edge joining two faces such that the surface direction is continuous across the edge, up to the given angleTolerance, at every point along the full length of the edge.

qTangentConnectedEdges (seed is Query) returns Query

A query for a chain of tangent edges connected to seed via tangent vertices, chaining across any number of tangent vertices.

qLoopEdges (seed is Query) returns Query

A query for a set of edges defining a loop. If the seed has laminar edges, this query will extend to include all laminar loops that contain any seed edges. If the seed has faces, the result will include the loops forming the outer boundary of the joined faces.

qParallelEdges (queryToFilter is Query, direction is Vector) returns Query

A query for all linear edges in queryToFilter which are parallel (or anti-parallel) to the given direction.

qParallelEdges (queryToFilter is Query, edges is Query) returns Query

A query to find all linear edges in queryToFilter which are parallel (or anti-parallel) to any linear edge in edges.

qLoopBoundedFaces (faceAndEdge is Query) returns Query

Given a face and an edge, query for all faces bounded by the given face, on the side of the given edge.

For example, to select an entire pocket, pass in the face which surrounds the pocket, and an edge of the face which touches that pocket.

Parameter	Type	Additional Info
`faceAndEdge`	`Query`	Should match a face and an edge. If multiple faces and edges match, used the first face and the first edge.

qFaceOrEdgeBoundedFaces (faceAndBoundingEntities is Query) returns Query

Given a seed face and bounding entities, matches all adjacent faces inside the bounding entities, expanding from the seed face.

Parameter	Type	Additional Info
`faceAndBoundingEntities`	`Query`	A Query for the seed face, followed by any boundary faces or edges. The seed face must be first, so a `qUnion` should be used to guarantee the order.

qHoleFaces (seed is Query) returns Query

Given a single face inside a hole or hole-like geometry, returns all faces of that hole.

Parameter	Type	Additional Info
`seed`	`Query`	A query for a single face inside the hole.

qSketchRegion (featureId is Id, filterInnerLoops is boolean) returns Query

A query for all fully enclosed, 2D regions created by a sketch.

Parameter Type Additional Info

featureId

Id

The feature id of the Sketch being queried.

filterInnerLoops

boolean

Optional

Specifies whether to exclude sketch regions fully contained in other sketch regions. A region whose border has a vertex or edge on the outside boundary is not considered "contained." Default is false.

qSketchRegion (featureId is Id) returns Query

qUniqueVertices (vertices is Query) returns Query

A query that filters out duplicate vertices. When duplicates are found, the vertex with the lowest deterministic ID is used.

qMateConnectorsOfParts (parts is Query) returns Query

A query for all mate connectors owned by parts.

qFilletFaces (facesToCompareTo is Query, compareType is CompareType) returns Query

A query for fillet faces of radius equal to, less than or equal to, or greater than or equal to the input faces. If facesToCompareTo does not match one or more fillet faces, the resulting query will not match any faces. Will find the fillet radius from each face and compare to find faces of all fillets on that body that satisfy the compareType.

If facesToCompareTo resolves to multiple fillet faces, all are matched independently. That is, qFilletFaces(qUnion([q1, q2], compareType)) returns the same thing as qUnion([qFilletFaces(q1, compareType), qFilletFaces(q2, compareType)]).

qMatching (referenceEntities is Query) returns Query

Matches any faces or edges within owner bodies of entities in referenceEntities which are geometrically identical (same size and shape) to the face or edge in referenceEntities.

If referenceEntities resolves to multiple entities, all are matched independently. That is, qMatching(qUnion([q1, q2])) returns the same thing as qUnion([qMatching(q1), qMatching(q2)]).

qPatternInstances (featureId is Id, instanceNames is array, entityType is EntityType) returns Query

A query for entities created by a specific instance or instances of an opPattern operation.

Parameter Type Additional Info

featureId

Id

The Id of the specified feature.

EXAMPLE

id + "pattern1"

instanceNames

array

The names of the instances to query for, a subset of the instanceNames passed into the opPattern operation.

qPatternInstances (featureId is Id, instanceName is string, entityType is EntityType) returns Query

qDependency (dependentEntities is Query) returns Query

A query for the true dependency of the given dependentEntities. For instance, the true dependency of the extruded body will be the face or sketch edges of the profile from which it is extruded.

qLaminarDependency (dependentEntities is Query) returns Query

A query for the true dependency of the given dependentEntities, specifically for use with wire edges that have been created from laminar edges. If the immediate dependency is not laminar then it will track back until it reaches a laminar dependency (if there is one).

qContainsPoint (queryToFilter is Query, point is Vector) returns Query

A query for all entities (bodies, faces, edges, or points) in queryToFilter containing a specified point.

Parameter	Type	Additional Info
`point`	`Vector`	A 3D point, in world space.

qIntersectsLine (queryToFilter is Query, line is Line) returns Query

A query for all entities (bodies, faces, edges, or points) in queryToFilter touching a specified infinite line.

qIntersectsPlane (queryToFilter is Query, plane is Plane) returns Query

A query for all entities (bodies, faces, edges, or points) in queryToFilter touching a specified infinite plane.

Parameter Type Additional Info

plane

Plane

EXAMPLE

plane(vector(0, 0, 0) * meter, vector(0, 0, 1))

qInFrontOfPlane (queryToFilter is Query, plane is Plane) returns Query

A query for all entities (bodies, faces, edges, or points) in queryToFilter in front of a specified infinite plane. Entities intersecting the plane will not be resolved. Only entities completely on one side or coincident with the plane will be selected. Use flip(plane) to query entities on the other side of the plane. For example, for the XY plane through the origin with the normal (0, 0, 1), qInFrontOfPlane will resolve the vertices (1, 1, 0) and (1, 1, 1) but not the vertex (1, 1, -1).

Parameter Type Additional Info

plane

Plane

EXAMPLE

plane(vector(0, 0, 0) * meter, vector(0, 0, 1))

qCoincidesWithPlane (queryToFilter is Query, plane is Plane) returns Query

A query for all entities (bodies, faces, edges, or points) in queryToFilter coinciding with a specified infinite plane.

Parameter Type Additional Info

plane

Plane

EXAMPLE

plane(vector(0, 0, 0) * meter, vector(0, 0, 1))

qWithinRadius (queryToFilter is Query, point is Vector, radius is ValueWithUnits) returns Query

A query for all entities (bodies, faces, edges or points) in queryToFilter that are within a specified radius from a point.

Parameter	Type	Additional Info
`point`	`Vector`	The point from which to check distance from.
`radius`	`ValueWithUnits`	The distance away from the point.

qClosestTo (queryToFilter is Query, point is Vector) returns Query

A query for the entity in queryToFilter closest to a point.

In the case of a tie, resolves to all entities within TOLERANCE.zeroLength of being the closest.

Parameter	Type	Additional Info
`point`	`Vector`	A position vector for the point to find entities closest to.

qFarthestAlong (queryToFilter is Query, direction is Vector) returns Query

A query for the entity in queryToFilter farthest along a direction in world space. In the case of a tie, resolves to all entities within TOLERANCE.zeroLength of being the farthest.

Parameter	Type	Additional Info
`direction`	`Vector`	A vector for the direction to find the entity farthest away.

qLargest (queryToFilter is Query) returns Query

A query to find the largest entity (by length, area, or volume) in queryToFilter.

If queryToFilter contains entities of different dimensionality (e.g. both solid bodies and faces), only entities of the highest dimension are considered. Entities are compared by length, area or volume. Multiple entities may be returned if they tie within tolerance.

qSmallest (queryToFilter is Query) returns Query

A query to find the smallest entity (by length, area, or volume) in queryToFilter.

If queryToFilter contains entities of different dimensionality (e.g. solid bodies and faces), only entities of the highest dimension are considered. Entities are compared by length, area or volume. Multiple entities may be returned if they tie within tolerance.

dummyQuery (operationId is Id, entityType is EntityType) returns Query

qSplitBy (featureId is Id, entityType, backBody is boolean) returns Query

Given the id of a split feature, get entities of a given EntityType on the front or the back side of the split. For a split by face or part, the front denotes the body in the direction of the split tool's surface normal, and the back denotes the body opposite the normal. For a split by isocline, the front denotes non-steep faces and edges, and the back denotes steep entities.

Parameter Type Additional Info

featureId

Id

EXAMPLE

id + "split1"

backBody

boolean

EXAMPLE

false indicates the entities in the front.

EXAMPLE

true indicates the entities in the back.

sketchEntityQuery (operationId is Id, entityType, sketchEntityId is string) returns Query

Gets the wire body entities created for a specific sketch entity. If the sketch id created multiple sketch entities, will return all the wire bodies.

Parameter Type Additional Info

operationId

Id

Id of the sketch feature.

entityType

EXAMPLE

EntityType.EDGE to match the edges on the wire bodies.

EXAMPLE

EntityType.BODY to match the bodies themselves.

EXAMPLE

undefined to match both.

sketchEntityId

string

Sketch id.

evaluateQuery (context is Context, query is Query) returns array

Returns an array of queries for the individual entities in a context which match a specified query. The returned array contains exactly one transient query for each matching entity at the time of the call. If the context is modified, the returned queries may become invalid and no longer match an entity.

It is usually not necessary to evaluate queries, since operation and evaluation functions can accept non-evaluated queries. Rather, the evaluated queries can be used to count the number of entities (if any) that match a query, or to iterate through the list to process entities individually.

The order of entities returned by this function is arbitrary (and generally not predictable) except in the case of a qUnion query. In that case, the entities matched by earlier queries in the argument to qUnion are returned first.

areQueriesEquivalent (context is Context, first is Query, second is Query) returns boolean

Returns true if the supplied queries evaluate to the same set of entities. This function is order-invariant, so if the two queries evaluate to the same entities, but in a different order, the function will still return true.

isQueryEmpty (context is Context, query is Query) returns boolean

Returns true if query evaluates to nothing. Equivalent to evaluateQuery(context, query) == [] or size(evaluateQuery(context, query)) == 0, but faster than either of those approaches if the query is not empty.

evaluate

Evaluation functions return information about the topological entities in the context, like bounding boxes, tangent planes, projections, and collisions. Evaluation functions take a context and a map that specifies the computation to be performed and return a ValueWithUnits, a FeatureScript geometry type (like Line or Plane), or a special type like DistanceResult. They may also throw errors if a query fails to evaluate or the input is otherwise invalid.

evApproximateCentroid (context is Context, arg is map) returns Vector

Find the centroid of an entity or group of entities. This is equivalent to the center of mass for a constant density object. Warning: This is an approximate value and it is not recommended to use this for modeling purposes that will be negatively affected in case the approximation changes. Consider using the center of a bounding box instead.

Parameter	Type	Additional Info
`arg`	`map`
`entities`	`Query`	The entities to take the center of mass of.

MassProperties type

The result of an evApproximateMassProperties call.

Value	Type	Description
`MassProperties`	`map`
`mass`	`ValueWithUnits`	The total mass.
`centroid`	`Vector`	The center of mass with respect to the given reference frame, or with respect to the origin if a reference frame is not specified.
`inertia`	`MatrixWithUnits`	The 3D inertia tensor, with units of mass * length ^ 2. Evaluated with respect to the reference frame, or with respect to the centroid if a reference frame is not specified.
`volume`	`ValueWithUnits`	Total volume. Only returned for solid bodies.
`area`	`ValueWithUnits`	Total area. Only returned for faces.
`length`	`ValueWithUnits`	Total length. Only returned for edges.
`count`	`number`	Total count. Only returned for vertices.

evApproximateMassProperties (context is Context, arg is map) returns MassProperties

Calculates approximate mass properties of an entity or group of entities. Returns mass, centroid, inertia tensor, and volume/area/length/count for bodies/faces/edges/vertices, respectively. Warning: These are approximate values and it is not recommended to use them for modeling purposes that will be negatively affected in case the approximation changes.

Parameter	Type	Additional Info
`arg`	`map`
`entities`	`Query`	The entities of which to compute mass properties. Only entities of the highest dimensionality will be considered.
`density`	`ValueWithUnits`	The density of the entities, with appropriate units. EXAMPLE `1 * kilogram / meter ^ 3` could be the density of 3D solid bodies EXAMPLE `1 * kilogram / meter ^ 2` could be the density of 2D faces or sheet bodies EXAMPLE `1 * kilogram / meter` could be the density of 1D edges or wire bodies EXAMPLE `1 * kilogram` could be the mass of each 0D vertex or point body
`referenceFrame`	`CoordSystem`	Optional Optional coordinate system. Defaults to the centroid with world axes for the inertia tensor, and world coordinates for the centroid.

evArea (context is Context, arg is map) returns ValueWithUnits

Return the total area of all the entities. If no matching 2D faces are found the total area will be zero.

Parameter	Type	Additional Info
`arg`	`map`
`entities`	`Query`

evAxis (context is Context, arg is map) returns Line

If the query finds one entity with an axis -- a line, circle, plane, cylinder, cone, sphere, torus, mate connector, or revolved surface -- return the axis. Otherwise throw an exception.

Parameter	Type	Additional Info
`arg`	`map`
`axis`	`Query`

evBox3d (context is Context, arg is map) returns Box3d

Find a bounding box around an entity, optionally with respect to a given coordinate system. There is also an option to use a faster but less accurate method.

Parameter	Type	Additional Info
`arg`	`map`
`topology`	`Query`	The entity to find the bounding box of.
`cSys`	`CoordSystem`	Optional The coordinate system to use (if not the standard coordinate system).
`tight`	`boolean`	Optional Get the tightest possible bounding box. Defaults to `true`. EXAMPLE `true` for a bounding box precisely at the extents of the given entities (and no bigger). EXAMPLE `false` for a bounding box at least as big as the given entities, using a faster algorithm.

evCollision (context is Context, arg is map) returns array

Find collisions between tools and targets. Each collision is a map with field type of type ClashType and fields target, targetBody, tool, and toolBody of type Query.

Parameter	Type	Additional Info
`arg`	`map`
`tools`	`Query`
`targets`	`Query`

evCornerType (context is Context, arg is map) returns map

Return the type of corner found at a vertex of a sheet metal model

Parameter	Type	Additional Info
`arg`	`map`
`vertex`	`Query`

Return	Type	Description
	`map`
`cornerType`	`SMCornerType`	the type of the corner
`primaryVertex`	`Query`	the vertex that defines the corner
`allVertices`	`array`	array of transient queries for all definition vertices associated with the corner

Throws	Additional info
`GBTErrorStringEnum.BAD_GEOMETRY`	The query does not evaluate to a single vertex

evCurveDefinition (context is Context, arg is map) returns map

Given a query for a curve, return a Circle, Ellipse, Line, or BSplineCurve value for the curve. If the curve is none of these types, return a map with unspecified contents.

Parameter Type Additional Info

arg map

edge

Query

The curve to evaluate.

returnBSplinesAsOther

boolean

Optional

If true, do not return B-spline curves (to avoid the associated time cost). Default is false.

Throws	Additional info
`GBTErrorStringEnum.INVALID_INPUT`	The first resolved entity was not an edge.
`GBTErrorStringEnum.CANNOT_RESOLVE_ENTITIES`	Input entities are invalid or there are no input entities.

evApproximateBSplineCurve (context is Context, arg is map) returns BSplineCurve

Given a query for a curve, return its approximation (or exact representation if possible) as a B-spline. The options forceCubic and forceNonRational may be used to restrict the type of spline that is returned, but even if these options are false, a cubic non-rational spline may be returned.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`	The curve to approximate.
`forceCubic`	`boolean`	Optional If true, a cubic spline will be returned. Defaults to false.
`forceNonRational`	`boolean`	Optional If true, a non-rational spline will be returned. Defaults to false.
`tolerance`	`number`	Optional Specifies the desired approximation tolerance: the maximum distance (in meters) between the original curve and the returned spline representation. Default is 1e-6, minimum is 1e-8, and maximum is 1e-2.

DistanceResult type

The result of an evDistance call -- information about the extremal distance and the attaining point / line / entity.

Value Type Description

DistanceResult map

distance

ValueWithUnits

The minimal or maximal distance.

sides

array

An array of 2 maps, containing information about where the extremum was found for each side. Each map has a:

point (Vector) : The position in world space that is closest or farthest to the other side. The distance field is measured between the two values of point.

index (integer) : the index into the line or point array or into the query results, if a query is passed in.

parameter (number or length or array of two numbers) : If the index refers to an edge, the parameter is a number between 0 and 1 (unless extend for that side was passed in). It is in the form that evEdgeTangentLine and evEdgeCurvature consume (with arcLengthParameterization set to the same value that was passed into evDistance).

If the index refers to a point, the parameter is 0.

If the index refers to a Line, the parameter is a length representing the distance along the direction.

If the index refers to a face, the parameter is a 2D Vector in the form that evFaceTangentPlane consumes. If this face is a mesh or a plane, the parameter is a 2D Vector of zeroes.

If the index refers to a Plane, the parameter is a 2D Vector representing the lengths along the plane's x and y axes.

evDistance (context is Context, arg is map) returns DistanceResult

Computes the minimum or maximum distance between geometry on side0 and geometry on side1. "Geometry" means entities, points, or lines. When the minimum or the maximum is not uniquely defined, ties will be broken arbitrarily.

EXAMPLE

evDistance(context, { "side0" : vector(1, 2, 3) * meter, "side1" : query }).distance returns the minimum distance from any entity returned by query to the point (1, 2, 3) meters.

EXAMPLE

result = evDistance(context, { "side0" : qEverything(EntityType.VERTEX), "side1" : qEverything(EntityType.VERTEX), "maximum" : true }) computes the pair of vertices farthest apart. qNthElement(qEverything(EntityType.VERTEX), result.sides[0].index) queries for one of these vertices.

See also

DistanceResult

Parameter	Type	Additional Info
`arg`	`map`
`side0`		One of the following: A query, or a point (3D Length Vector), or a `Line`, or a `Plane`, or an array of points, or an array of `Line`s, or an array of `Plane`s. EXAMPLE `qNthElement(qEverything(EntityType.FACE), 0)` or `vector(1, 2, 3) * meter` or `line(vector(1, 0, 1) * meter, vector(1, 1, 1)` or `plane(vector(1,1,1) * meter, vector(0,0,1), vector(1,0,0))`.
`extendSide0`	`boolean`	Optional If `true` and side0 is a query, bodies will be ignored and edges and faces extended to their possibly infinite underlying surfaces. Defaults to `false`.
`side1`		Like `side0`.
`extendSide1`	`boolean`	Optional Like `extendSide0`.
`maximum`	`boolean`	Optional If `true`, compute the maximum instead of the minimum. Defaults to `false`. Not allowed to be `true` if a line is passed in in either side or if either `extend` is true.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter returned for edges measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-calculate parameterization. This field only controls the parameter returned for edges. It does not control the parameter returned for points, `Line`s, faces, or `Plane`s.
`useFaceParameter`	`boolean`	Optional For Onshape internal use.

RaycastResult type

Map containing the results of one collision between a ray and an entity.

Value	Type	Description
`RaycastResult`	`map`
`entity`	`Query`	A query for the entity hit by the ray.
`entityType`	`EntityType`	The type of the entity.
`parameter`		Parameters for where the ray hit the entity. A unitless 2-vector for a face, a number for an edge, else undefined.
`intersection`	`Vector`	Intersection point.
`distance`	`ValueWithUnits`	Distance of the intersection point from the ray origin.

evRaycast (context is Context, arg is map) returns array

Detect intersections between a ray and the given entities.

Parameter	Type	Additional Info
`arg`	`map`
`entities`	`Query`	A query for target entities. If bodies are provided, the result will contain intersections for individual entities owned by the body.
`ray`	`Line`	The ray to intersect the entities. Because the passed-in `Line` is interpreted as a ray, by default, intersections with entities "behind" the ray origin are not detected. `includeIntersectionsBehind` can be set to `true` if those intersections are desired. EXAMPLE `line(vector(0, 0, 0) * inch, vector(1, 0, 0))` specifies the positive x-axis
`closest`	`boolean`	Optional Get only the closest intersection with any of the entities. Defaults to `true`.
`includeIntersectionsBehind`	`boolean`	Optional Return intersections that are behind the ray origin. Defaults to `false`. Cannot be set to `true` if `closest` is `true`.

Return type	Description
`array`	An array of `RaycastResult`s for each intersection in front of the ray, ordered from closest to farthest.

evEdgeConvexity (context is Context, arg is map) returns EdgeConvexityType

Return the convexity type of the given edge, CONVEX, CONCAVE, SMOOTH, or VARIABLE. If the edge is part of a body with inside and outside convex and concave have the obvious meanings.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`

Throws	Additional info
`GBTErrorStringEnum.TOO_MANY_ENTITIES_SELECTED`	The query evaluates to more than one entity
`GBTErrorStringEnum.BAD_GEOMETRY`	The query does not evaluate to a single edge.

EdgeCurvatureResult type

The result of an evEdgeCurvature call -- a coordinate system for the Frenet frame and the curvature defined at a point

Value	Type	Description
`EdgeCurvatureResult`	`map`
`frame`	`CoordSystem`	The frame. The Z vector is the tangent, the X vector is the normal and the Y vector is the binormal
`curvature`	`ValueWithUnits`	The curvature (inverse length units).

evEdgeCurvature (context is Context, arg is map) returns EdgeCurvatureResult

Return a Frenet frame along an edge, with curvature. If the curve has zero curvature at an evaluated point then the returned normal and binormal are arbitrary and only the tangent is significant.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`	The curve to use EXAMPLE `qNthElement(qEverything(EntityType.EDGE), 1)`
`parameter`	`number`	A number in the range 0..1 indicating the point along the curve to evaluate the frame at.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-evaluate parameterization. The parameterization is identical to that used by `evEdgeTangentLines`. Results obtained with arcLengthParameterization will have lower accuracy due to approximation.
`face`	`Query`	Optional If present, the edge orientation used is such that walking along the edge with "up" being the `face` normal will keep `face` to the left. Must be adjacent to `edge`.

Throws	Additional info
`GBTErrorStringEnum.NO_TANGENT_LINE`	A frame could not be calculated for the specified input.

evEdgeCurvatures (context is Context, arg is map) returns array

Return Frenet frames along an edge, with curvature. If the curve has zero curvature at an evaluated point then the returned normal and binormal are arbitrary and only the tangent is significant.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`	The curve to use EXAMPLE `qNthElement(qEverything(EntityType.EDGE), 1)`
`parameters`	`array`	An array of numbers in the range 0..1 indicating points along the curve to evaluate frames at.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-evaluate parameterization. The parameterization is identical to that used by `evEdgeTangentLines`. Results obtained with arcLengthParameterization will have lower accuracy due to approximation.
`face`	`Query`	Optional If present, the edge orientation used is such that walking along the edge with "up" being the `face` normal will keep `face` to the left. Must be adjacent to `edge`.

Return type	Description
`array`	An array of `EdgeCurvatureResult`s.

Throws	Additional info
`GBTErrorStringEnum.NO_TANGENT_LINE`	A frame could not be calculated for the specified input.

curvatureFrameTangent (curvatureResult is EdgeCurvatureResult) returns Vector

Returns the tangent vector of a curvature frame

Return type	Description
`Vector`	A unit 3D vector in world space.

curvatureFrameNormal (curvatureResult is EdgeCurvatureResult) returns Vector

Returns the normal vector of a curvature frame

Return type	Description
`Vector`	A unit 3D vector in world space.

curvatureFrameBinormal (curvatureResult is EdgeCurvatureResult) returns Vector

Returns the binormal vector of a curvature frame

Return type	Description
`Vector`	A unit 3D vector in world space.

evEdgeTangentLine (context is Context, arg is map) returns Line

Return one tangent Line to an edge.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`	The curve to use EXAMPLE `qNthElement(qEverything(EntityType.EDGE), 1)`
`parameter`	`number`	A number in the range 0..1 indicating a point along the curve to evaluate the tangent at.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-evaluate parameterization.
`face`	`Query`	Optional If present, the edge orientation used is such that walking along the edge with "up" being the `face` normal will keep `face` to the left. Must be adjacent to `edge`.

Throws	Additional info
`GBTErrorStringEnum.NO_TANGENT_LINE`	A tangent line could not be evaluated for the given query.

evEdgeTangentLines (context is Context, arg is map) returns array

Return tangent lines to a edge.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`	The curve to use EXAMPLE `qNthElement(qEverything(EntityType.EDGE), 1)`
`parameters`	`array`	An array of numbers in the range 0..1 indicating points along the curve to evaluate tangents at.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-evaluate parameterization.
`face`	`Query`	Optional If present, the edge orientation used is such that walking along the edge with "up" being the `face` normal will keep `face` to the left. Must be adjacent to `edge`.

Return type	Description
`array`	An array of `Line`s.

Throws	Additional info
`GBTErrorStringEnum.NO_TANGENT_LINE`	A tangent line could not be evaluated for the given query.

evEdgeCurvatureDerivative (context is Context, arg is map) returns Vector

Evaluate the derivative of the curvature vector with respect to arc length, that is, the third derivative of the curve with respect to arc length.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`	The curve to use EXAMPLE `qNthElement(qEverything(EntityType.EDGE), 1)`
`parameter`	`number`	A number in the range 0..1 indicating a point along the curve to evaluate the tangent at.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-evaluate parameterization.

Throws	Additional info
`GBTErrorStringEnum.NO_TANGENT_LINE`	The curvature derivative could not be evaluated for the given query.

evFacePeriodicity (context is Context, arg is map) returns array

Return the periodicity in primary and secondary direction of a face, returned in an array of booleans.

A particular direction is periodic when the face's underlying surface definition is wrapped along that direction. For instance, if primary direction is periodic, the parameters [0, v] and [1, v] will prepresent the same point for all valid v. If the secondary direction is periodic, the parameters [u, 0] and [u, 1] represent the same point for all valid u.

Parameter Type Additional Info

arg map

face

Query

The face on which to evaluate periodicity

trimmed

boolean

Optional

If true (default), return trimmed face periodicity instead of the underlying surface's.

FaceCurvatureResult type

The result of an evFaceCurvature call -- principal directions and curvatures at a point.

The curvature along a particular direction (in the tangent plane) is the inverse of the radius of curvature in that direction. This curvature is positive if the radius of curvature points away from the normal direction, negative if it points along the normal direction, or zero if there is no curvature in that direction. The principal curvatures at a point are the directions of minimal and maximal curvature along the surface at that point.

Value	Type	Description
`FaceCurvatureResult`	`map`
`minCurvature`	`ValueWithUnits`	The smaller of the two principal curvatures (inverse length units).
`maxCurvature`	`ValueWithUnits`	The larger of the two principal curvatures (inverse length units).
`minDirection`	`Vector`	A 3D unit vector corresponding to `minCurvature`.
`maxDirection`	`Vector`	A 3D unit vector corresponding to `maxCurvature`.

evFaceCurvature (context is Context, arg is map) returns FaceCurvatureResult

Given a face, calculate and return principal curvatures at a point on that face, specified by its parameter-space coordinates.

EXAMPLE

 // Ellipsoid measuring 10in x 4in x 6in
fEllipsoid(context, id + "ellipsoid", {
            "center" : vector(0, 0, 0) * inch,
            "radius" : vector(5 * inch, 2 * inch, 3 * inch)
        });
const ellipseFace = qCreatedBy(id + "ellipsoid", EntityType.FACE);
const topPoint = vector(0, 0, 3) * inch; // Point on top of ellipsoid
const distanceResult = evDistance(context, { // Closest position to topPoint on ellipseFace
            "side0" : ellipseFace,
            "side1" : topPoint
        });
var uvCoordinatesAtTopPoint = distanceResult.sides[0].parameter;
var curvatureResult = evFaceCurvature(context, {
        "face" : ellipseFace,
        "parameter" : uvCoordinatesAtTopPoint
    });
//  curvatureResult is {
//      minCurvature: 3 * inch / (5 * inch)^2,
//      maxCurvature: 3 * inch / (2 * inch)^2,
//      minDirection: vector(1, 0, 0),
//      maxDirection: vector(0, 1, 0)
//  }

Parameter Type Additional Info

arg map

face

Query

The face on which to evaluate the curvature. The face cannot be a mesh.

EXAMPLE

qNthElement(qEverything(EntityType.FACE), 1)

parameter

Vector

a 2d unitless parameter-space vector specifying the location on the face. The coordinates are relative to the parameter-space bounding box of the face.

EXAMPLE

vector(0.5, 0.5)

evFaceCurvatures (context is Context, arg is map) returns array

Given a face, calculate and return an array of principal curvatures at points on that face, specified by its parameter-space coordinates.

Parameter Type Additional Info

arg map

face

Query

A single face on which to evaluate the curvatures. The face cannot be a mesh.

EXAMPLE

qNthElement(qEverything(EntityType.FACE), 1)

parameters

array

an array of 2d unitless parameter-space vectors specifying locations on the face. The coordinates are relative to the parameter-space bounding box of the face.

EXAMPLE

[ vector(0.5, 0.5), vector(0, 1) ]

Return type	Description
`array`	An array of `FaceCurvatureResult`s.

evFaceCurvatureDerivative (context is Context, arg is map) returns MatrixWithUnits

Given a face, calculate and return the derivative of the second fundamental form of the face in a given direction.

The second fundamental form is a matrix that may be computed from the principal curvatures of a surface as

const curvature = evFaceCurvature(context, { ... });
const secondFF = - curvature.minCurvature * transpose(matrix([curvature.minDirection])) * matrix([curvature.minDirection])
                 - curvature.maxCurvature * transpose(matrix([curvature.maxDirection])) * matrix([curvature.maxDirection]);

Parameter	Type	Additional Info
`arg`	`map`
`face`	`Query`	The face on which to evaluate the curvature. The face cannot be a mesh. EXAMPLE `qNthElement(qEverything(EntityType.FACE), 1)`
`parameter`	`Vector`	a 2d unitless parameter-space vector specifying the location on the face. The coordinates are relative to the parameter-space bounding box of the face. EXAMPLE `vector(0.5, 0.5)`
`direction`	`Vector`	a 3d unitless vector specifying a direction in the tangent plane of the face. It should be a unit vector perpendicular to the face's normal at the given point.

Return type	Description
`MatrixWithUnits`	A 3x3 matrix with units of length ^ -2.

evFaceNormalAtEdge (context is Context, arg is map) returns Vector

Return the surface normal of a face at a position on one of its edges.

If the first result is not a face, throw an exception.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`
`face`	`Query`
`parameter`	`number`	A number in the range 0..1 indicating a point along the edge to evaluate the tangent at.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-evaluate parameterization.
`usingFaceOrientation`	`boolean`	Optional If true, the edge orientation used is such that walking along the edge with "up" being the `face` normal will keep `face` to the left. If false, use the default orientation of the edge, which is the same orientation used by `evEdgeTangentLine`. Default is `false`.

evFaceTangentPlaneAtEdge (context is Context, arg is map) returns Plane

Return a Plane tangent to face at a position on one of its edges.

If the first result is not a face, throw an exception.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`
`face`	`Query`
`parameter`	`number`	A number in the range 0..1 indicating a point along the edge to evaluate the tangent at.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-evaluate parameterization.
`usingFaceOrientation`	`boolean`	Optional If true, the edge orientation used is such that walking along the edge with "up" being the `face` normal will keep `face` to the left. If false, use the default orientation of the edge, which is the same orientation used by `evEdgeTangentLine`. Default is `false`.

evFaceTangentPlanesAtEdge (context is Context, arg is map)

Return an array of Planes tangent to a face at an array of parameters on one of its edges. The x-direction of the plane is oriented with the tangent of the edge with respect to usingFaceOrientation.

If the first result is not a face, throw an exception.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`
`face`	`Query`
`parameters`	`array`	An array of numbers in the range 0..1 indicating points along the edge to evaluate the tangent at.
`arcLengthParameterization`	`boolean`	Optional If true (default), the parameter measures distance along the edge, so `0.5` is the midpoint. If false, use an arbitrary but faster-to-evaluate parameterization.
`usingFaceOrientation`	`boolean`	Optional If true, the edge orientation used is such that walking along the edge with "up" being the `face` normal will keep `face` to the left. If false, use the default orientation of the edge, which is the same orientation used by `evEdgeTangentLine`. Default is `false`.

evFaceTangentPlane (context is Context, arg is map) returns Plane

Given a face, calculate and return a Plane tangent to that face, where the plane's origin is at the point specified by its parameter-space coordinates.

Parameter Type Additional Info

arg map

face

Query

The face to evaluate. The face cannot be a mesh.

EXAMPLE

qNthElement(qEverything(EntityType.FACE), 1)

parameter

Vector

2d unitless parameter-space vector specifying the location of tangency on the face. The coordinates are relative to the parameter-space bounding box of the face.

EXAMPLE

vector(0.5, 0.5) places the origin at the bounding box's center.

Throws	Additional info
`GBTErrorStringEnum.NO_TANGENT_PLANE`	Could not find a tangent plane or there was a problem with face parameterization.

evFaceTangentPlanes (context is Context, arg is map) returns array

Given a face, calculate and return an array of Planes tangent to that face, where each plane's origin is located at the point specified by its parameter-space coordinates.

Parameter	Type	Additional Info
`arg`	`map`
`face`	`Query`	The face to evaluate. The face cannot be a mesh. EXAMPLE `qNthElement(qEverything(EntityType.FACE), 1)`
`parameters`	`array`	an array of 2d unitless parameter-space vectors specifying locations of tangency on the face. The coordinates are relative to the parameter-space bounding box of the face. EXAMPLE `[ vector(0.5, 0.5), vector(0, 1) ]`
`returnUndefinedOutsideFace`	`boolean`	Optional If true, the function will only return a plane if vector is on the face, otherwise returns undefined. Default is false.

Throws	Additional info
`GBTErrorStringEnum.NO_TANGENT_PLANE`	Could not find a tangent plane or there was a problem with face parameterization.

evFilletRadius (context is Context, arg is map) returns ValueWithUnits

Given a face of a constant radius fillet, return the radius of fillet.

Parameter	Type	Additional Info
`arg`	`map`
`face`	`Query`

Throws	Additional info
`GBTErrorStringEnum.BAD_GEOMETRY`	The first resolved entity was not a filleted face.

evLength (context is Context, arg is map) returns ValueWithUnits

Return the total length of all the entities (if they are edges) and edges belonging to entities (if they are bodies). If no edges are found the total length will be zero.

Parameter	Type	Additional Info
`arg`	`map`
`entities`	`Query`

evLine (context is Context, arg is map) returns Line

If the edge is a line, return a Line value for the given edge.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`

Throws	Additional info
`GBTErrorStringEnum.INVALID_INPUT`	The first resolved entity was not a line.

evMateConnector (context is Context, arg is map) returns CoordSystem

Gets the coordinate system of the given mate connector

Parameter	Type	Additional Info
`arg`	`map`
`mateConnector`	`Query`	The mate connector to evaluate.

evOwnerSketchPlane (context is Context, arg is map) returns Plane

Return the plane of the sketch that created the given entity.

Parameter Type Additional Info

arg map

entity

Query

The sketch entity. May be a vertex, edge, face, or body.

checkAllEntities

boolean

Optional

If true, the function will only return a plane if all entities queried under 'entity' share coplanar sketch planes. Otherwise, the plane will only be evaluated for the first entity in the query. Default is false.

Throws	Additional info
`GBTErrorStringEnum.CANNOT_RESOLVE_PLANE`	Entities were not created by a sketch or do not share the same sketch plane.

evPlane (context is Context, arg is map) returns Plane

If the face is a planar face or a mate connector, return the Plane it represents.

Parameter	Type	Additional Info
`arg`	`map`
`face`	`Query`

Throws	Additional info
`GBTErrorStringEnum.CANNOT_RESOLVE_PLANE`	The first resolved entity was not a planar face or mate connector.

evPlanarEdge (context is Context, arg is map) returns Plane

If the edge lies in a plane, return a Plane it lies in.

Parameter	Type	Additional Info
`arg`	`map`
`edge`	`Query`

Throws	Additional info
`GBTErrorStringEnum.CANNOT_RESOLVE_PLANE`	The first resolved entity was not a planar edge.

evPlanarEdges (context is Context, arg is map) returns Plane

If all the edges in a query share the same plane, return a Plane they lie in.

Parameter	Type	Additional Info
`arg`	`map`
`edges`	`Query`

Throws	Additional info
`GBTErrorStringEnum.CANNOT_RESOLVE_PLANE`	Edges in the query were either not planar or do not share the same plane.

evSurfaceDefinition (context is Context, arg is map) returns map

Return a descriptive value for a face, or the first face if the query finds more than one. Return a Cone, Cylinder, Plane, Sphere, Torus, or BSplineSurface as appropriate for the face, or an unspecified map value if the face is none of these with surfaceType filled of type SurfaceType

Parameter Type Additional Info

arg map

face

Query

returnBSplinesAsOther

boolean

Optional

If true, do not return B-spline surfaces (to avoid the associated time cost). Default is false.

Throws	Additional info
`"GBTErrorStringEnum.CANNOT_RESOLVE_PLANE"`	The first result is not a face.

evApproximateBSplineSurface (context is Context, arg is map) returns map

Given a query for a face, return its approximation as a B-spline, including trim boundaries. The options forceCubic and forceNonRational may be used to restrict the type of spline that is returned for the surface, but even if these options are false, a cubic non-rational spline may be returned.

The returned representation includes a surface, the boundary loop as 2D splines in UV space, and any interior loops. The returned UV curves are typically degree 1 or 2 and non-rational. For periodic surfaces, outer and inner loops are not clearly defined and relying on them is not recommended.

Parameter	Type	Additional Info
`arg`	`map`
`face`	`Query`	The curve to approximate.
`forceCubic`	`boolean`	Optional If true, the returned surface will be a cubic spline. This does not affect the trim curves. Defaults to false.
`forceNonRational`	`boolean`	Optional If true, the returned surface will be non-rational. Defaults to false.
`tolerance`	`number`	Optional Specifies the desired approximation tolerance: the maximum distance (in meters) between the original face and the returned spline representation. Default is 1e-6, minimum is 1e-8, and maximum is 1e-4. The tolerance for trim curves is 10x the specified value.

Return	Type	Description
	`map`
`bSplineSurface`	`BSplineSurface`	the underlying 3D surface
`boundaryBSplineCurves`	`array`	array of 2D `BSplineCurve`s representing the trimming boundary of the face. May be empty if the face is the entirety of the surface.
`innerLoopBSplineCurves`	`array`	array of arrays of 2D `BSplineCurve`s representing the inner loops (if any) of the trimming boundary of the face.

evVertexPoint (context is Context, arg is map) returns Vector

Return the coordinates of a point, or the origin of a mate connector.

Parameter	Type	Additional Info
`arg`	`map`
`vertex`	`Query`

evVolume (context is Context, arg is map) returns ValueWithUnits

Return the total volume of all the entities. If no matching 3D bodies are found, the total volume will be zero.

Parameter	Type	Additional Info
`arg`	`map`
`entities`	`Query`
`accuracy`	`VolumeAccuracy`

evMaxPathDeviation (context is Context, arg is map) returns map

Returns the max deviation between two paths.

Parameter	Type	Additional Info
`arg`	`map`
`side1`	`Query`	Bodies and/or edges forming a single continuous path.
`side2`	`Query`	Bodies and/or edges forming a single continuous path.
`showDeviation`	`boolean`	Optional If true, will display a magenta comb for each deviation sample and a red line with a star for the maximum deviation. Default is `false`.

Return	Type	Description
	`map`
`deviation`	`ValueWithUnits`	value of the max deviation between `side1` and `side2`.
`side1Point`	`Vector`	position on `side1` where `side1` is `deviation` away from `side2`.
`side2Point`	`Vector`	position on `side2` where `side2` is `deviation` away from `side1`.

Math

approximationUtils

APPROXIMATION_SAMPLES const

Number of sample taken on the curve to perform the approximation.

MAX_CONTROL_POINTS const

Maximum number of control points to approximate the curve with.

MAX_DEGREE const

Maximum degree of the curve.

TOLERANCE_BOUND const

A LengthBoundSpec for approximation tolerance.

DEGREE_BOUND const

An IntegerBoundSpec for curve degree.

curveApproximationPredicate (definition is map) predicate

A predicate to add curve approximation parameters to a feature.

checkApproximationParameters (definition is map, path is Path)

Checks approximation options to see if the approximation would succeed and highlights the issue if not.

approximateResults (context is Context, id is Id, definition is map)

Approximates the curves created by the feature id. This meant to be used along with curveApproximationPredicate and it expects definition to have the parameters defined in the predicate.

box

This module refers to 3D bounding boxes, e.g. the result of a call to evBox3d.

This is not to be confused with the box standard type used for references.

Box3d type

A three-dimensional bounding box.

Value	Type	Description
`Box3d`	`map`
`minCorner`	`Vector`	A 3D position representing the corner with the smallest x, y, and z coordinates.
`maxCorner`	`Vector`	A 3D position representing the corner with the largest x, y, and z coordinates.

canBeBox3d (value) predicate

Typecheck for Box3d

box3d (minCorner is Vector, maxCorner is Vector) returns Box3d

Construct a bounding box from two opposite corners.

box3d (pointArray is array) returns Box3d

Construct a bounding box containing all points in pointArray

transformBox3d (boxIn is Box3d, transformation is Transform) returns Box3d

Return a box aligned with transformed coordinate system containing the input box

extendBox3d (bBox is Box3d, absoluteValue is ValueWithUnits, factor is number) returns Box3d

Return an enlarged bounding box. The box is scaled by 1 + factor around its midpoint, and then each face is moved outward by absoluteValue (inward if absoluteValue is negative).

Parameter	Type	Additional Info
`absoluteValue`	`ValueWithUnits`	The absolute distance to move each face of the box. The corners move `sqrt(3)` times as far.
`factor`	`number`	The relative amount to expand the box, with `0` leaving it unchanged.

box3dCenter (bBox is Box3d) returns Vector

Return the center of the bounding box.

box3dDiagonalLength (bBox is Box3d) returns ValueWithUnits

Return the length of the diagonal from the minCorner to the maxCorner of the bounding box.

insideBox3d (point is Vector, bBox is Box3d) predicate

Whether the specified point is within the bounding box.

coordSystem

WORLD_ORIGIN const

Position of the world origin, equivalent to vector(0, 0, 0) * meter

X_DIRECTION const

Direction parallel to the X axis, equivalent to vector(1, 0, 0)

Y_DIRECTION const

Direction parallel to the Y axis, equivalent to vector(0, 1, 0)

Z_DIRECTION const

Direction parallel to the Z axis, equivalent to vector(0, 0, 1)

WORLD_COORD_SYSTEM const

The world coordinate system, equivalent to coordSystem(vector(0, 0, 0) * meter, vector(1, 0, 0), vector(0, 0, 1))

CoordSystem type

A right-handed Cartesian coordinate system. Used for converting points and geometry between different reference frames, or for creating planes and mate connectors.

The y-axis of a coordinate system is not stored, but it can be obtained by calling the yAxis function, which simply performs a cross product.

See also

toWorld(CoordSystem)

fromWorld(CoordSystem)

coordSystem(Plane)

plane(CoordSystem)

opMateConnector

Value	Type	Description
`CoordSystem`	`map`
`origin`	`Vector`	A 3D point, in world space, representing the origin of the coordinate system.
`xAxis`	`Vector`	A 3D unit vector, in world space, representing the x-axis of the coordinate system.
`zAxis`	`Vector`	A 3D unit vector, in world space, representing the z-axis of the coordinate system. Must be perpendicular to the `xAxis`.

coordSystem (origin is Vector, xAxis is Vector, zAxis is Vector) returns CoordSystem

Creates a Cartesian coordinate system.

See also

CoordSystem

Parameter	Type	Additional Info
`origin`	`Vector`	A 3D point in world space.
`xAxis`	`Vector`	A 3D vector in world space. Need not be normalized.
`zAxis`	`Vector`	A 3D vector in world space. Need not be normalized but must be orthogonal to xAxis.

tolerantEquals (cSys1 is CoordSystem, cSys2 is CoordSystem) predicate

Check that two CoordSystems are the same up to tolerance.

toWorld (cSys is CoordSystem, pointInCSys is Vector) returns Vector

Convert a specified point from a specified coordinate system into world space.

EXAMPLE

toWorld(cSys, vector(0, 0, 0)) equals cSys.origin

Parameter	Type	Additional Info
`pointInCSys`	`Vector`	A 3D vector, measured with respect to the `cSys` provided.

Return type	Description
`Vector`	A 3D vector in world space.

toWorld (cSys is CoordSystem) returns Transform

Returns a Transform which will transform coordinates measured in cSys into world coordinates.

EXAMPLE

toWorld(cSys) * vector(0, 0, 0) equals cSys.origin

When used in operations which place or move parts (like opTransform, opPattern, or addInstance), this transform will (somewhat counterintuitively) move parts from the world origin and orientation to the cSys origin and orientation.

fromWorld (cSys is CoordSystem, worldPoint is Vector) returns Vector

Convert a specified point from world space into a specified coordinate system.

EXAMPLE

fromWorld(cSys, cSys.origin) equals vector(0, 0, 0)

Parameter	Type	Additional Info
`worldPoint`	`Vector`	A 3D vector, measured in world space.

Return type	Description
`Vector`	A 3D vector measured in `cSys`

fromWorld (cSys is CoordSystem) returns Transform

Returns a Transform which will transform coordinates measured in world space into cSys coordinates.

EXAMPLE

fromWorld(cSys) * cSys.origin equals vector(0, 0, 0)

When used in operations which place or move parts (like opTransform, opPattern, or addInstance), this transform will (somewhat counterintuitively) move parts from the cSys origin and orientation to the world origin and orientation.

scaleNonuniformly (xScale is number, yScale is number, zScale is number, cSys is CoordSystem) returns Transform

Returns a Transform that represents 3 independent scalings along the X, Y, and Z axes of a particular cSys, centered around cSys.origin.

yAxis (cSys is CoordSystem) returns Vector

Returns the y-axis of a coordinate system

Return type	Description
`Vector`	A 3D vector in world space.

toString (cSys is CoordSystem) returns string

Returns a representation of the coordinate system as a string.

curveGeometry

X_AXIS const

The global X axis, equivalent to line(vector(0, 0, 0) * meter, vector(1, 0, 0))

Y_AXIS const

The global Y axis, equivalent to line(vector(0, 0, 0) * meter, vector(0, 1, 0))

Z_AXIS const

The global Z axis, equivalent to line(vector(0, 0, 0) * meter, vector(0, 0, 1))

Line type

Represents a parameterized line in 3D space.

Value	Type	Description
`Line`	`map`
`origin`	`Vector`	A point on the line, as a 3D Vector with length units.
`direction`	`Vector`	A unitless normalized 3D Vector.

canBeLine (value) predicate

Typecheck for Line

line (origin is Vector, direction is Vector) returns Line

Creates a line from a point and a direction.

Parameter	Type	Additional Info
`direction`	`Vector`	The direction gets normalized by this function.

tolerantEquals (line1 is Line, line2 is Line) predicate

Check that two Lines are the same up to tolerance, including checking that they have the same origin.

To check if two Lines are equivalent (rather than equal), use collinearLines.

collinearLines (line1 is Line, line2 is Line) returns boolean

Returns true if the two lines are collinear.

transform (from is Line, to is Line) returns Transform

Returns the transformation that transforms the line from to the line to (including the origin) using the minimum rotation angle.

project (line is Line, point is Vector) returns Vector

Returns the projection of the point onto the line. See also other overloads of project.

rotationAround (line is Line, angle is ValueWithUnits) returns Transform

Returns a Transform that represents the rotation around the given line by the given angle. The rotation is counterclockwise looking against the line direction.

LineLineIntersection type

Represents an intersection between two lines. Depending on the lines, this intersection may be a point, a line, or nothing.

Value Type Description

LineLineIntersection map

dim

number

Integer representing the dimension of the intersection.

EXAMPLE

0 indicates that intersection is a 3D length Vector.

EXAMPLE

1 indicates that intersection is a Line. (i.e. the lines are collinear)

EXAMPLE

-1 indicates that the intersection does not exist.

intersection

undefined or Vector or Line (depending on dim) that represents the intersection.

canBeLineLineIntersection (value) predicate

Typecheck for LineLineIntersection

intersection (line1 is Line, line2 is Line) returns LineLineIntersection

Returns a LineLineIntersection representing the intersection between two lines. If the lines are collinear, line1 will be stored in the intersection field of that LineLineIntersection.

isPointOnLine (point is Vector, line is Line) returns boolean

Returns true if the point lies on the line.

toString (value is Line) returns string

Circle type

Represents a circle in 3D space.

Value	Type	Description
`Circle`	`map`
`coordSystem`	`CoordSystem`	The circle lies in the xy plane of this coordinate system and the origin of its parameterization is the x axis.
`radius`	`ValueWithUnits`	The radius of the circle.

canBeCircle (value) predicate

Typecheck for Circle

circle (cSys is CoordSystem, radius is ValueWithUnits) returns Circle

Returns a new Circle in the given coordinate system cSys.

circle (center is Vector, xDirection is Vector, normal is Vector, radius is ValueWithUnits) returns Circle

Returns a new Circle with the given parameters. xDirection and normal must be perpendicular.

tolerantEquals (circle1 is Circle, circle2 is Circle) predicate

Check that two Circles are the same up to tolerance, including the coordinate system.

toString (value is Circle) returns string

Ellipse type

Represents an ellipse in 3D space.

Value	Type	Description
`Ellipse`	`map`
`coordSystem`	`CoordSystem`	The ellipse lies in the xy plane of this coordinate system and the x axis corresponds to the major radius.
`majorRadius`	`ValueWithUnits`	The larger of the two radii.
`minorRadius`	`ValueWithUnits`	The smaller of the two radii.

canBeEllipse (value) predicate

Typecheck for Ellipse

ellipse (cSys is CoordSystem, majorRadius is ValueWithUnits, minorRadius is ValueWithUnits) returns Ellipse

Returns a new Ellipse with the given parameters.

ellipse (center is Vector, xDirection is Vector, normal is Vector, majorRadius is ValueWithUnits, minorRadius is ValueWithUnits) returns Ellipse

Returns a new Ellipse with the given parameters. xDirection and normal must be perpendicular.

tolerantEquals (ellipse1 is Ellipse, ellipse2 is Ellipse) predicate

Check that two Ellipses are the same up to tolerance, including the coordinate system.

toString (value is Ellipse) returns string

KnotArray type

An array of non-decreasing numbers representing the knots of a spline

canBeKnotArray (value) predicate

Typecheck for KnotArray

knotArray (value is array) returns KnotArray

Cast an array on non-decreasing numbers to a KnotArray

knotArrayIsCorrectSize (knots is KnotArray, degree is number, nControlPoints is number) predicate

Assure that size(knotArray) is 1 + degree + nControlPoints

BSplineCurve type

The definition of a spline in 3D or 2D world space, or unitless 2D parameter space.

See also

bSplineCurve(map)

Value	Type	Description
`BSplineCurve`	`map`
`degree`	`number`	The degree of the spline.
`dimension`	`number`	The dimension of the spline. Must be 2 or 3.
`isRational`	`boolean`	Whether the spline is rational.
`isPeriodic`	`boolean`	Whether the spline is periodic.
`controlPoints`	`array`	An array of control points of the required dimension. Size should be at least degree + 1. 2D spline control points can have world space units, or be unitless if they are intended to represent locations in parameter space (e.g. as a boundary input to `opCreateBSplineSurface`).
`weights`	`array`	Required if `isRational` is `true` An array of unitless values with the same size as the control points array.
`knots`	`KnotArray`	An array of non-decreasing knots of size equal to `1 + degree + size(controlPoints)`

canBeBSplineCurve (value) predicate

Typecheck for BSplineCurve

bSplineCurve (definition is map) returns BSplineCurve

Returns a new BSplineCurve, adding knot padding and control point overlap as necessary.

EXAMPLE

opCreateBSplineCurve(context, id + "bSplineCurve1", {
            "bSplineCurve" : bSplineCurve({
                        "degree" : 2,
                        "isPeriodic" : false,
                        "controlPoints" : [
                                vector(0, 0, 0) * inch,
                                vector(1, 0, 0) * inch,
                                vector(1, 1, 0) * inch,
                                vector(0, 1, 0) * inch],
                        "knots" : knotArray([0, .2, 1]) // Will be padded to [0, 0, 0, .2, 1, 1, 1]
                    })
        });

Creates a spline starting at the origin, moving first quickly along the x-axis (toward the second point), and finishing on the y-axis.

EXAMPLE

opCreateBSplineCurve(context, id + "bSplineCurve1", {
            "bSplineCurve" : bSplineCurve({
                        "degree" : 3,
                        "isPeriodic" : true,
                        "controlPoints" : [
                                vector(0, 0, 0) * inch,
                                vector(1, 0, 0) * inch,
                                vector(1, 1, 0) * inch,
                                vector(0, 1, 0) * inch], // Will be overlapped by repeating the first 3 points
                        "knots" : knotArray([0, .25, .5, .75, 1]) // Same as default when no knots provided. Will be padded to [-.75, -.5, -.25, 0, .25, .5, .75, 1, 1.25, 1.5, 1.75]
                    })
        });

Creates a closed, curvature-continuous, symmetric curve between the four given points.

Parameter	Type	Additional Info
`definition`	`map`
`degree`	`number`	The degree of the spline.
`isPeriodic`	`boolean`	Whether the spline is periodic.
`controlPoints`	`array`	An array of control points. See `BSplineCurve` for specific detail. For periodic splines, you may provide the necessary overlap, or provide control points without any overlap. If no overlap is provided, `degree` overlapping control points (corresponding to the first `degree` control points) will be added to the end of the control points list (unless you provide a set of knots that show no overlap is necessary). EXAMPLE `[vector(-1, 1, 0) * inch, vector(1, 1, 0) * inch, vector(1, -1, 0) * inch, vector(-1, -1, 0) * inch]`
`weights`	`array`	Optional An array of weights. See `BSplineCurve` for specific detail.
`knots`	`KnotArray`	Optional An array of knots. See `BSplineCurve` for specific detail. If knots are not provided a uniform parameterization wil be created such that the curve exists on the parameter range `[0, 1]`. For non-periodic curves with `n` control points, you may provide the full set of `n + degree + 1` knots, or you may provide `n - degree + 1` knots, and multiplicity will by padded onto the ends (which has the effect of clamping the spline to its two endpoints). For periodic curves with `n` unique control points (and optionally an additional `degree` overlapping control points), you may provide the full set of `n + 2 * degree + 1` knots, or you may provide `n + 1` knots, and the periodic knots will be padded onto the ends.

bSplineCurve (degree is number, isPeriodic is boolean, controlPoints is array, knots is KnotArray) returns BSplineCurve

Deprecated: Use bSplineCurve(map)

bSplineCurve (degree is number, isPeriodic is boolean, controlPoints is array, weights is array, knots is KnotArray) returns BSplineCurve

Deprecated: Use bSplineCurve(map)

math

A module containing many elementary math functions.

Some math functions (such as sin and cos) accept a ValueWithUnits, rather than a number, and are defined in the units module. There is no pow function: exponentiation is done using the ^ operator.

When writing a FeatureScript module which uses only basic math functionality, importing mathUtils (which imports this module along with matrix, transform, and vector) is recommended.

PI const

The mathematical constant pi, to floating-point precision.

EXAMPLE

myAngle = (PI / 4) * radian

In most cases, conversions using PI can be avoided if using ValueWithUnits appropriately. Thus, you should never find yourself writing a statement like sin(myAngle * PI / 180), since myAngle should already have correct units attached.

tolerantEquals (value1 is number, value2 is number) predicate

Returns true if numbers are equal up to a computational tolerance. The tolerance used is a specific number defined by TOLERANCE.computational (set to 1e-13) that is meant to adequately handle tolerances introduced by numerical operations. However, this tolerance may be too restrictive or generous for different situations, in which case tolerantEquals(number, number, number) should be used with the appropriate tolerance specified.

EXAMPLE

tolerantEquals(1, 1) returns true

EXAMPLE

tolerantEquals(1, 1 + 1e-14) returns true

EXAMPLE

tolerantEquals(1, 1 / 900 * 9e100 / 1e98) returns true

EXAMPLE

tolerantEquals(1, 1 / 9 / 9 / 9 / 9 * 9 * 9 * 9 * 9) returns true

tolerantEquals (value1 is number, value2 is number, tolerance is number) predicate

Returns true if numbers are equal up to a specified tolerance.

EXAMPLE

tolerantEquals(1, 1, 0) returns true

EXAMPLE

tolerantEquals(1, 1.01, 0.03) returns true

EXAMPLE

tolerantEquals(1, 0.99, 0.03) returns true

EXAMPLE

tolerantEquals(1, 1.01, 0.01) returns true

EXAMPLE

tolerantEquals(1, 1.03, 0.01) returns false

See also

tolerantEquals(number, number)

abs (value)

Absolute value.

EXAMPLE

abs(-1) returns 1

EXAMPLE

abs(-1.5 * inch) equals 1.5 * inch

sqrt (value is number)

Square root of a number.

EXAMPLE

sqrt(4) returns 2

EXAMPLE

sqrt(-4) throws an error

log (value is number)

Natural logarithm of a number.

EXAMPLE

log(exp(3)) returns 3

EXAMPLE

log(0) returns -inf

EXAMPLE

log(-1) throws an error

log10 (value is number)

Base 10 logarithm of a number.

EXAMPLE

log10(1000) returns 3

EXAMPLE

log10(0) returns -inf

EXAMPLE

log10(-1) throws an error

sinh (value is number)

Hyperbolic sine.

cosh (value is number)

Hyperbolic cosine.

tanh (value is number)

Hyperbolic tangent.

asinh (value is number)

Inverse hyperbolic sine.

acosh (value is number)

Inverse hyperbolic cosine.

atanh (value is number)

Inverse hyperbolic tangent.

exp (value is number)

e to the power of value.

EXAMPLE

exp(1) returns 2.71828...

EXAMPLE

exp(log(3)) returns 3

exp2 (value is number)

2 to the power of value.

EXAMPLE

exp2(10) returns 1024

hypot (a is number, b is number)

Hypotenuse function, as sqrt(a^2 + b^2), but without any surprising results due to finite numeric precision.

EXAMPLE

hypot(3, 4) returns 5

floor (value is number)

Round a number down to the nearest integer.

For values with units, first divide by a value with the same units.

EXAMPLE

floor(1.9) returns 1

EXAMPLE

floor(2.0) returns 2

EXAMPLE

floor(-3.3) returns -4

EXAMPLE

var numberOfBricks is number = floor(wallLength / brickLength);

ceil (value is number)

Round a number up to the nearest integer.

For values with units, first divide by a value with the same units.

EXAMPLE

ceil(1.1) returns 2

EXAMPLE

ceil(1.0) returns 1

EXAMPLE

ceil(-3.3) returns -3

EXAMPLE

var numberOfBricks is number = ceil(wallLength / brickLength)

round (value is number)

Round a number to the nearest integer.

EXAMPLE

round(1.4) returns 1

EXAMPLE

round(1.5) returns 2

EXAMPLE

round(-1.5) returns -1

roundToPrecision (value is number, precision is number)

Round a number to a given number of decimal places.

EXAMPLE

roundToPrecision(0.12345, 3) returns 0.123

EXAMPLE

roundToPrecision(9.9995, 3) returns 10

EXAMPLE

roundToPrecision(123.45, -1) returns 120

For positive values of precision, this method is more accurate than round(value, multiple). For instance, print(roundToPrecision(0.45682, 4)) prints 0.4568, but round(0.45682, 0.0001) prints 0.45680000000000004. This is because the floating point representation of 0.0001 is slightly imprecise, and that imprecision is compounded inside the call to round. The floating point value of 4, on the other hand, is precise, so the result of roundToPrecision will be the closest possible floating-point representation of 0.4568. Thus, print and other functions using string conversion (~) will not print extraneous digits.

min (value1, value2)

Return the lesser of two values, which must be comparable with <.

EXAMPLE

min(0, 1) returns 0

EXAMPLE

min(1 * meter, 1 * inch) equals 1 * inch

max (value1, value2)

Return the greater of two values, which must be comparable with <.

EXAMPLE

max(0, 1) returns 1

EXAMPLE

max(1 * meter, 1 * inch) equals 1 * meter

min (arr is array)

Return the least of an array of values, as determined by operator <, or undefined if the array is empty.

EXAMPLE

min([1, 2, 3]) returns 1

EXAMPLE

min([1 * inch, 2 * inch, 3 * inch]) equals 1 * inch

max (arr is array)

Return the greatest of an array of values, as determined by operator <, or undefined if the array is empty.

EXAMPLE

max([1, 2, 3]) returns 3

EXAMPLE

max([1 * inch, 2 * inch, 3 * inch]) equals 3 * inch

argMin (arr is array)

Return the index of the smallest element of an array, as determined by operator <, or undefined if the array is empty.

EXAMPLE

argMin([1 * inch, 2 * inch, 3 * inch]) returns 0

argMax (arr is array)

Return the index of the largest element of an array, as determined by the > operator, or undefined if the array is empty.

EXAMPLE

argMax([1 * inch, 2 * inch, 3 * inch]) returns 2

range (from is number, to is number)

Return an array of numbers in a range. Only integers are allowed.

EXAMPLE

range(0, 3) returns [0, 1, 2, 3]

range (from, to, count)

Return an array of numbers, (of type number or ValueWithUnits), in a range. Note: before FeatureScript 372 this function received as input the step size instead of the number of steps

EXAMPLE

range(0, 10, 6) returns [0, 2, 4, 6, 8, 10]

EXAMPLE

range(0, 4.5, 4) returns [0, 1.5, 3, 4.5]

EXAMPLE

range(1 * inch, 1.4 * inch, 3) returns [1 * inch, 1.2 * inch, 1.4 * inch]

clamp (value, lowerBound, higherBound)

Force a value into a range,

EXAMPLE

clamp(-1, 0, 20) returns 0,

EXAMPLE

clamp(10, 0, 20) returns 10

EXAMPLE

clamp(30, 0, 20) returns 20

EXAMPLE

clamp(30 * inch, 0 * inch, 20 * inch) equals 20 * inch

isInteger (value) predicate

True if value is a finite integer.

Note that all numbers in FeatureScript represented as floating point numbers, so an expression like isInteger(hugeInteger + 0.1) may still return true.

Used in feature preconditions to define an integer input.

isNonNegativeInteger (value) predicate

True if value is a finite integer greater than or equal to zero.

isPositiveInteger (value) predicate

True if value is a finite integer greater than zero.

mathUtils

This module imports the math, matrix, transform, and vector modules. It is designed to be imported instead of the geometry module in Feature Studios where only math (not higher-level modeling functionality) is needed.

matrix

Matrix type

A Matrix is an array of rows, all the same size, each of which is an array of numbers

canBeMatrix (val) predicate

Typecheck for Matrix

matrixSize (matrix is Matrix) returns array

Return a 2 element array containing the numbers of rows and columns of a matrix.

isSquare (matrix is Matrix) predicate

Check whether a matrix is square.

matrix (value is array) returns Matrix

Cast a two-dimensional array to a matrix.

identityMatrix (size is number) returns Matrix

Construct an identity matrix of a given dimension.

zeroMatrix (rows is number, cols is number) returns Matrix

Construct an all-zero matrix of a given dimension.

diagonalMatrix (diagonalValues is array) returns Matrix

Given an array of diagonalValues of size n, construct an nxn matrix which has those values along its main diagonal (starting in the top-left), and 0 everywhere else.

cwiseProduct (m1 is Matrix, m2 is Matrix) returns Matrix

Construct a matrix by multiplying corresponding elements of two matrices (which must be the same size).

transpose (m is Matrix) returns Matrix

Return the transpose of a matrix.

inverse (m is Matrix) returns Matrix

Compute the inverse of a matrix. Throws an exception if the matrix is not square. If the matrix is singular the resulting matrix will contain infinities.

squaredNorm (m is Matrix) returns number

Return the sum of the squares of matrix elements.

norm (m is Matrix) returns number

Return the square root of the sum of the squares of matrix elements.

svd (m is Matrix) returns map

Compute the singular value decomposition of a matrix, i.e. s, u, and v, where m == u * s * transpose(v) and s is a diagonal matrix of singular values.

Parameter	Type	Additional Info
`m`	`Matrix`	an n-by-p matrix.

Return	Type	Description
	`map`
`u`	`Matrix`	An n-by-n unitary matrix
`s`	`Matrix`	An n-by-p diagonal matrix
`v`	`Matrix`	A p-by-p unitary matrix

determinant (m is Matrix) returns number

Return the determinant of the matrix.

toString (value is Matrix) returns string

matrixWithUnits

MatrixWithUnits type

A MatrixWithUnits is analogous to ValueWithUnits, but wrapping a matrix.

canBeMatrixWithUnits (value) predicate

Typecheck for MatrixWithUnits

get (matrix is MatrixWithUnits, i is number, j is number) returns ValueWithUnits

Gets an element of a MatrixWithUnits, returning a ValueWithUnits.

matrixSize (matrix is MatrixWithUnits) returns array

Return a 2-element array containing the numbers of rows and columns of a matrix.

toString (value is MatrixWithUnits) returns string

nurbsUtils

removeKnots (points is array, knots is array, curveDegree is number) returns map

Remove as many knots as possible from a NURBS defined by points, knots and curveDegree.

separatePointsAndWeights (points is array) returns map

Separates a 4d array containing weighted points into a 3d unweighted points array and a 1d weights array.

combinePointsAndWeights (points is array, weights is array) returns array

Combines a 3d unweighted points array and a 1d weights array into a 4d weighted points array

persistentCoordSystem

PersistentCoordSystem type

A coordinate system that can persist as part of an attribute associated with an entity. This coordinate system will be transformed along with its parent entity as that entity undergoes transformations.

As with other attributes, the coordinate system will be propagated to copied entities, such as instances in a pattern. These copied persistent coordinate systems will take on the transforms of their new parents.

When getAttribute is used to retrieve a previously-set persistent coordinate system, the value of coordSystem will be in its transformed state for the current point in the feature execution. If a transform is applied such that the coordinate system is know longer right-handed, then the coordSystem value will be undefined. For instance, this would happen in the case of a mirrored coordinate system.

Value	Type	Description
`PersistentCoordSystem`	`map`
`coordSystem`	`CoordSystem`	The coordinate system to persist
`coordSystemId`	`string`	An id to associate with the coordinate system. This id must be unique within the context of the parent entity.

persistentCoordSystem (coordSystem is CoordSystem, coordSystemId is string) returns PersistentCoordSystem

Creates a persistent coordinate system.

See also

PersistentCoordSystem

Parameter	Type	Additional Info
`coordSystem`	`CoordSystem`	The coordinate system
`coordSystemId`	`string`	An id with which to associate the coordinate system. This id must be unique within the context of the parent entity that an becomes associated with this persistent coordinate system through `setAttribute`.

splineUtils

ApproximationTarget type

A set of points and optionally derivatives to approximate by a spline.

See also

approximateSpline(Context, map)

Value	Type	Description
`ApproximationTarget`	`map`
`positions`	`array`	An ordered array of points for the spline to pass closely to.
`startDerivative`	`Vector`	Required if `start2ndDerivative` is provided The desired start derivative of the spline.
`start2ndDerivative`	`Vector`	Optional The desired start second derivative of the spline.
`endDerivative`	`Vector`	Required if `end2ndDerivative` is provided The desired end derivative of the spline.
`end2ndDerivative`	`Vector`	Optional The desired end second derivative of the spline.

canBeApproximationTarget (value) predicate

Typecheck for ApproximationTarget

approximationTarget (value is map) returns ApproximationTarget

Construct an ApproximationTarget

approximateSpline (context is Context, definition is map) returns array

Compute a family of splines that approximates a family of ApproximationTargets to within a given tolerance. The resulting splines are consistently parameterized, so that, for example, lofting between them will match corresponding target positions. Note: If parameters are not specified, the magnitude of start and end derivatives in targets is ignored as well as the second component parallel with the first derivative.

Parameter	Type	Additional Info
`definition`	`map`
`degree`	`number`	The desired degree of the curve. The output may have a different degree, if for example there aren't enough points.
`tolerance`	`ValueWithUnits`	How far the output is allowed to deviate from the input. Must be at least 1e-8 meters.
`isPeriodic`	`boolean`	Whether the output spline is periodic.
`targets`	`array`	An array of `ApproximationTarget`s. All targets must have the same number of positions and specify corresponding derivative information.
`parameters`	`array`	Optional An array of numbers representing the parameters corresponding to the target points. Must be strictly increasing. If specified, the output spline at those parameters will match the target points. If specified, derivatives in approximation targets will not be rescaled.
`maxControlPoints`	`number`	Optional The maximum number of control points that will be returned by this function's output. Tolerance will not be satisfied if this limit is reached. Default is 10000.
`interpolateIndices`	`array`	Optional An array of indices into target positions that specifies which ones are to be interpolated exactly. This is currently supported only for non-periodic splines.
`suppressInterpolationNotice`	`boolean`	Optional Don't report an info if the result is fully interpolated. Default is false.

Return type	Description
`array`	An array of `BSplineCurve`s, one for each target.

evaluateSpline (definition is map) returns array

Evaluate a 3D spline at several parameters, possibly with derivatives.

Parameter	Type	Additional Info
`definition`	`map`
`spline`	`BSplineCurve`	The 3D spline to evaluate.
`parameters`	`array`	An array of numbers in the range of the spline's knot vector.
`nDerivatives`	`number`	Optional The number of derivatives to compute, in addition to the positions. Default is 0.

Return type	Description
`array`	An array of arrays of points. If `result` is returned, `result[i][j]` is the `i`th derivative at `j`th parameter.

elevateBezierDegree (pointsIn is array, newDegree is number) returns array

Elevate the degree of a bezier curve defined by an array of control points

Parameter	Type	Additional Info
`pointsIn`	`array`	The control points of the curve to be elevated. Must be non-empty.
`newDegree`	`number`	The desired degree. If it is less than the number of control points, the control points will be returned unchanged.

Return type	Description
`array`	The control points of the degree-elevated curve

surfaceGeometry

This module contains methods for creating and working with primitive surfaces: planes, cylinders, cones, spheres, and tori.

XY_PLANE const

The world XY plane, equivalent to plane(vector(0, 0, 0) * meter, vector(0, 0, 1), vector(1, 0, 0))

YZ_PLANE const

The world YZ plane, equivalent to plane(vector(0, 0, 0) * meter, vector(1, 0, 0), vector(0, 1, 0))

XZ_PLANE const

The world XZ plane, equivalent to plane(vector(0, 0, 0) * meter, vector(0, 1, 0), vector(0, 0, 1))

Plane type

A Plane is a data type representing an origin, a normal vector, and an X direction, perpendicular to the normal direction.

Value	Type	Description
`Plane`	`map`
`origin`	`Vector`	A 3D point, in world space.
`normal`	`Vector`	A 3D unit vector in world space.
`x`	`Vector`	A 3D unit vector in world space. Must be perpendicular to `normal`.

canBePlane (value) predicate

Typecheck for Plane

plane (cSys is CoordSystem) returns Plane

Create a Plane on the XY plane of a specified coordinate system.

plane (origin is Vector, normal is Vector, x is Vector) returns Plane

Create a Plane which fully specifies its orientation.

Parameter	Type	Additional Info
`origin`	`Vector`	A 3D point in world space.
`normal`	`Vector`	A 3D vector in world space. Need not be normalized.
`x`	`Vector`	A 3D vector in world space. Need not be normalized.

plane (origin is Vector, normal is Vector) returns Plane

Create a Plane from a point and a normal.

The x-axis of this Plane's coordinate system will be an arbitrary vector perpendicular to the normal.

Parameter	Type	Additional Info
`origin`	`Vector`	A 3D point in world space.
`normal`	`Vector`	A 3D vector in world space. Need not be normalized.

alignCanonically (context is Context, plane is Plane) returns Plane

Returns the plane that would represent the coordinate system of a face coplanar with the input plane. Used in plane transformation for computing sketch patterns.

yAxis (plane is Plane) returns Vector

Returns the y-axis of the specified plane as a 3D Vector in world space.

tolerantEquals (plane1 is Plane, plane2 is Plane) predicate

Check that two Planes are the same up to tolerance, including checking that they have the same the origin and local coordinate system.

To check if two Planes are equivalent (rather than equal), use coplanarPlanes.

coplanarPlanes (plane1 is Plane, plane2 is Plane) returns boolean

Returns true if the two planes are coplanar.

planeToCSys (plane is Plane) returns CoordSystem

Create a coordinate system whose XY-plane is a specified plane, with its origin at the plane's origin.

coordSystem (plane is Plane) returns CoordSystem

Create a coordinate system whose XY-plane is a specified plane, with its origin at the plane's origin.

Alias for planeToCSys.

toString (value is Plane) returns string

project (plane is Plane, point is Vector) returns Vector

Projects a 3D point onto a Plane, returning a 3D point on the plane.

project (plane is Plane, line is Line) returns Line

Projects a Line onto a Plane, returning a Line whose origin is on the Plane and whose direction is a normalized Vector on the Plane

Throws an error if the Line is in the same direction as the normal of the Plane

planeToWorld (plane is Plane, planePoint is Vector) returns Vector

Transforms a 2D point in a Plane's coordinates to its corresponding 3D point in world coordinates.

planeToWorld3D (plane is Plane) returns Transform

Returns a Transform which takes 3D points measured with respect to a Plane (such that points which lie on the plane will have a z-coordinate of approximately 0) and transforms them into world coordinates.

worldToPlane3D (plane is Plane, worldPoint is Vector) returns Vector

Transforms a 3D point in world coordinates into a 3D point measured in a Plane's coordinates. If the point lies on the Plane, the result will have a z-coordinate of approximately 0.

worldToPlane (plane is Plane, worldPoint is Vector) returns Vector

Transforms a 3D worldPoint in world coordinates into a 2D point measured in a Plane's (x,y) coordinates.

This is modified as of FeatureScript version 363.0. Older versions of FeatureScript use worldToPlane to return 3D vectors composed of the plane coordinate system baseis. This functionality is still available in the worldToPlane function above.

worldToPlane3D (plane is Plane) returns Transform

Returns a Transform which takes 3D points measured in world coordinates and transforms them into 3D points measured in plane coordinates (such that points which lie on the plane will have a z-coordinate of approximately 0).

transform (from is Plane, to is Plane) returns Transform

Returns a Transform which maps the plane from to the plane to.

mirrorAcross (plane is Plane) returns Transform

Returns a Transform which takes points on one side of a plane and transforms them to the other side. The resulting transform is non-rigid, and using this transform in an opTransform or similar operations will invert the transformed bodies.

intersection (plane1 is Plane, plane2 is Plane)

Returns a Line at the intersection between the two Planes. If the planes are parallel or coincident, returns undefined.

LinePlaneIntersection type

Represents an intersection between a line and a plane. Depending on the line and plane, this intersection may be a point, a line, or nothing.

Value Type Description

LinePlaneIntersection map

dim

number

Integer representing the dimension of the intersection.

EXAMPLE

0 indicates that intersection is a 3D length Vector.

EXAMPLE

1 indicates that intersection is a Line.

EXAMPLE

-1 indicates that the intersection does not exist (i.e. the line and the plane are parallel).

intersection

undefined or Vector or Line (depending on dim) that represents the intersection.

canBeLinePlaneIntersection (value) predicate

Typecheck for LinePlaneIntersection

intersection (plane is Plane, line is Line) returns LinePlaneIntersection

Returns a LinePlaneIntersection representing the intersection between line and plane.

isPointOnPlane (point is Vector, plane is Plane) returns boolean

Returns true if the point lies on the plane.

flip (plane is Plane) returns Plane

Returns a Plane with the reversed normal vector.

Cone type

Type representing a cone which extends infinitely down the positive z-axis of its coordSystem.

Value	Type	Description
`Cone`	`map`
`coordSystem`	`CoordSystem`	The position and orientation of the cone.
`halfAngle`	`ValueWithUnits`	The angle from z-axis of `coordSystem` to the surface of the cone.

canBeCone (value) predicate

Typecheck for Cone

cone (cSys is CoordSystem, halfAngle is ValueWithUnits) returns Cone

Constructs a Cone from a coordinate system and a half angle.

tolerantEquals (cone1 is Cone, cone2 is Cone) predicate

Check that two Cones are the same up to tolerance, including the local coordinate system.

toString (value is Cone) returns string

Cylinder type

Type representing a Cylinder which extends infinitely along the z-axis of its coordSystem.

Value	Type	Description
`Cylinder`	`map`
`coordSystem`	`CoordSystem`	The position and orientation of the cylinder.
`radius`	`ValueWithUnits`	The cylinder's radius.

canBeCylinder (value) predicate

Typecheck for Cylinder

cylinder (cSys is CoordSystem, radius is ValueWithUnits) returns Cylinder

Constructs a cylinder from a coordinate system and a radius.

tolerantEquals (cylinder1 is Cylinder, cylinder2 is Cylinder) predicate

Check that two Cylinders are the same up to tolerance, including the local coordinate system.

toString (value is Cylinder) returns string

Torus type

Type representing a torus, the shape of a circle revolved around a coplanar axis.

The torus represented is revolved about the z-axis of the coordSystem and centered in its xy-plane.

Value	Type	Description
`Torus`	`map`
`coordSystem`	`CoordSystem`	The position and orientation of the torus.
`radius`	`ValueWithUnits`	The major radius, i.e. the distance from the center of the torus to the center of the revolved circle.
`minorRadius`	`ValueWithUnits`	The minor radius, i.e. the radius of the revolved circle.

canBeTorus (value) predicate

Typecheck for Torus

torus (cSys is CoordSystem, minorRadius is ValueWithUnits, radius is ValueWithUnits) returns Torus

Constructs a torus from a coordinate system, the minor radius, and the major radius.

tolerantEquals (torus1 is Torus, torus2 is Torus) predicate

Check that two tori are the same up to tolerance, including the local coordinate system.

toString (value is Torus) returns string

Sphere type

Type representing a sphere of a given radius centered around a 3D point.

Value	Type	Description
`Sphere`	`map`
`coordSystem`	`CoordSystem`	The position and orientation of the sphere.
`radius`	`ValueWithUnits`	The sphere's radius.

canBeSphere (value) predicate

Typecheck for Sphere

sphere (cSys is CoordSystem, radius is ValueWithUnits) returns Sphere

tolerantEquals (sphere1 is Sphere, sphere2 is Sphere) predicate

Check that two Spheres are the same up to tolerance, including the local coordinate system.

toString (value is Sphere) returns string

ControlPointMatrix type

A two-dimensional array of 3D position vectors. Reading across a row represents a change in v, and reading down a column represents a change in u.

canBeControlPointMatrix (value) predicate

Typecheck for ControlPointMatrix

controlPointMatrix (value is array) returns ControlPointMatrix

Cast a two-dimensional array of 3D position vectors to a ControlPointMatrix.

BSplineSurface type

The definition of a spline in 3D space. For all matrices of the spline definition, reading across a row represents a change in v, and reading down a column represents a change in u.

See also

bSplineSurface

Value	Type	Description
`BSplineSurface`	`map`
`uDegree`	`number`	The degree of the spline in u.
`vDegree`	`number`	The degree of the spline in v.
`isRational`	`boolean`	Whether the spline is rational.
`isUPeriodic`	`boolean`	Whether the spline periodic in u.
`isVPeriodic`	`boolean`	Whether the spline periodic in v.
`controlPoints`	`ControlPointMatrix`	A grid of 3d control points. Must have at least `uDegree + 1` rows and `vDegree + 1` columns.
`weights`	`Matrix`	Required if `rational` is `true` A matrix of unitless values with the same shape as the control points grid.
`uKnots`	`KnotArray`	An array of non-decreasing knots of size equal to 1 + `uDegree` + number of rows in `controlPoints`
`vKnots`	`KnotArray`	An array of non-decreasing knots of size equal to 1 + `vDegree` + number of columns in `controlPoints`

canBeBSplineSurface (value) predicate

Typecheck for BSplineSurface

bSplineSurface (definition is map)

Returns a new BSplineSurface, adding knot padding and control point overlap as necessary.

EXAMPLE

opCreateBSplineSurface(context, id + "bSplineSurface1", {
            "bSplineSurface" : bSplineSurface({
                        "uDegree" : 2,
                        "vDegree" : 2,
                        "isUPeriodic" : false,
                        "isVPeriodic" : false,
                        "controlPoints" : controlPointMatrix([
                                    [vector(-2,  2, 0) * inch, vector(-1,  2, 0) * inch, vector(0,  2, 0) * inch, vector(1,  2, 0) * inch, vector(2,  2, 0) * inch],
                                    [vector(-2,  1, 0) * inch, vector(-1,  1, 0) * inch, vector(0,  1, 0) * inch, vector(1,  1, 0) * inch, vector(2,  1, 0) * inch],
                                    [vector(-2,  0, 0) * inch, vector(-1,  0, 0) * inch, vector(0,  0, 1) * inch, vector(1,  0, 0) * inch, vector(2,  0, 0) * inch],
                                    [vector(-2, -2, 0) * inch, vector(-1, -2, 0) * inch, vector(0, -2, 0) * inch, vector(1, -2, 0) * inch, vector(2, -2, 0) * inch]
                                ]),
                        "uKnots" : knotArray([0, .1, 1]), // Will be padded to [0, 0, 0, .1, 1, 1, 1]
                        "vKnots" : knotArray([0, 1/3, 2/3, 1]) // Same as default when no knots provided.  Will be padded to [0, 0, 0, 1/3, 2/3, 1, 1, 1]
                    })
        });

Creates a new spline surface on the XY plane with a protrusion at the origin, falling back to the XY plane more quickly in the +Y direction.

EXAMPLE

opCreateBSplineSurface(context, id + "bSplineSurface1", {
            "bSplineSurface" : bSplineSurface({
                        "uDegree" : 2,
                        "vDegree" : 1,
                        "isUPeriodic" : true,
                        "isVPeriodic" : false,
                        "controlPoints" : controlPointMatrix([
                                    [vector(0,  0, 1) * inch, vector(-1,  0, 0) * inch, vector(-2,  0, -1) * inch],
                                    [vector(1,  1, 1) * inch, vector( 0,  1, 0) * inch, vector(-1,  1, -1) * inch],
                                    [vector(2,  0, 1) * inch, vector( 1,  0, 0) * inch, vector( 0,  0, -1) * inch],
                                    [vector(1, -1, 1) * inch, vector( 0, -1, 0) * inch, vector(-1, -1, -1) * inch]
                                    // Will be overlapped by repeating the first two rows
                                ]),
                        "uKnots" : knotArray([0, .25, .5, .75, 1]), // Same as default when no knots provided. Will be padded to [-.5, -.25, 0, .25, .5, .75, 1, 1.25, 1.5]
                        "vKnots" : knotArray([0, .5, 1]) // Same as default when no knots provided.  Will be padded to [0, 0, .5, 1, 1]
                    })
        });

Creates a new spline surface which is a tube surrounding the origin, sheared in the X direction.

Parameter	Type	Additional Info
`definition`	`map`
`uDegree`	`number`	The degree of the spline in u.
`vDegree`	`number`	The degree of the spline in v.
`isUPeriodic`	`boolean`	Whether the spline periodic in u.
`isVPeriodic`	`boolean`	Whether the spline periodic in v.
`controlPoints`	`ControlPointMatrix`	A matrix of control points. See `BSplineSurface` for specific detail. If u or v is periodic, you may provide the necessary overlap, or provide control points without any overlap. If no overlap is provided, `degree` overlapping control point rows or columns (corresponding to the first `degree` control point rows or columns) will be added. (unless you provide a set of knots that show no overlap is necessary). EXAMPLE controlPointMatrix([ [vector(-1, -1, -1) * inch, vector(-1, 0, 0) * inch, vector(-1, -2, 1) * inch], [vector( 0, 1, -1) * inch, vector( 0, 2, 0) * inch, vector( 0, 0, 1) * inch], [vector( 1, -1, -1) * inch, vector( 1, 0, 0) * inch, vector( 1, -2, 1) * inch] ])
`weights`	`array`	Optional A matrix of weights. See `BSplineSurface` for specific detail.
`uKnots`	`KnotArray`	Optional An array of knots. See `BSplineSurface` for specific detail. If knots are not provided a uniform parameterization will be created such that the u parameterization exists on the range `[0, 1]`. For non-periodic u with `n` control point rows, you may provide the full set of `n + degree + 1` knots, or you may provide `n - degree + 1` knots, and multiplicity will by padded onto the ends (which has the effect of clamping the surface to the control points in the first and last rows). For periodic u with `n` unique control points (and optionally an additional `degree` overlapping control points), you may provide the full set of `n + 2 * degree + 1` knots, or you may provide `n + 1` knots, and the periodic knots will be padded onto the ends.
`vKnots`	`KnotArray`	Optional See `uKnots`.

MeshFaceParameter type

A MeshFaceParameter is a 2D array unitless array. It is functionnally indentical to a 2D vector but because there is no guarantee of continuity for mesh parameters, it does not make sense to expose vector math for it.

canBeMeshFaceParameter (value) predicate

Typecheck for MeshFaceParameter

meshFaceParameter (value is array) returns MeshFaceParameter

Make a MeshFaceParameter from an array.

transform

Transform type

A Transform typically represents a change of position and orientation in 3D space (other affine transformations, such as scaling and shearing, can also be represented).

rotationAround, scaleUniformly, transform(Vector), toWorld(CoordSystem) and fromWorld(CoordSystem) return useful transforms. Transforms are commonly used with opTransform, whose documentation has examples of calling these functions.

Transforms are also commonly used with their * operator overloads to easily work with geometry in multiple coordinate systems.

EXAMPLE

transform * (vector(1, 1, 1) * inch) yields a point which is the given point, transformed by the transform.

EXAMPLE

transform2 * transform1 yields a new transform which is equivalent to applying transform1 followed by transform2.

A Transform contains a linear portion (rotation, scaling, or shearing), which is applied first, and a translation vector, which is applied second. Generally, these individual fields on this type don't need to be directly used, and everything you need can be accomplished through the operator overloads above, or other functions in this module and the coordSystem module.

Value	Type	Description
`Transform`	`map`
`linear`	`Matrix`	A linear motion, which is generally a rotation, but can also be a scaling, inversion, or shearing.
`translation`	`Vector`	A 3D translation vector.

canBeTransform (value) predicate

Typecheck for Transform

transform (linear is Matrix, translation is Vector) returns Transform

Construct a Transform using the matrix argument for rotation and scaling and the vector argument for translation.

transform (translation is Vector) returns Transform

Construct a Transform that translates without rotation or scaling.

transform (value is map) returns Transform

identityTransform () returns Transform

Construct a transform that does nothing (no rotation, scaling, or translation).

tolerantEquals (transform1 is Transform, transform2 is Transform) predicate

Check that two Transforms are the same up to tolerance.

inverse (t is Transform) returns Transform

Compute the inverse of a Transform, such that inverse(t) * t == identityTransform().

scaleUniformly (scale is number) returns Transform

Returns a Transform that represents a uniform scaling around the origin.

scaleUniformly (scale is number, pointToScaleAbout is Vector) returns Transform

Returns a Transform that represents a uniform scaling around pointToScaleAbout.

scaleNonuniformly (xScale is number, yScale is number, zScale is number) returns Transform

Returns a Transform that represents 3 independent scalings along the X, Y, and Z axes, centered around the origin.

scaleNonuniformly (xScale is number, yScale is number, zScale is number, pointToScaleAbout is Vector) returns Transform

Returns a Transform that represents 3 independent scalings along the X, Y, and Z axes, centered around pointToScaleAbout.

transformUV

TransformUV type

A TransformUV represents a change of position and orientation in unitless 2D space.

A TransformUV contains a linear portion (rotation, scaling, or shearing), which is applied first, and a translation vector, which is applied second.

Value	Type	Description
`TransformUV`	`map`
`linear`	`Matrix`	A linear motion, which is generally a rotation, but can also be a scaling, inversion, or shearing.
`translation`	`Vector`	A 2D translation vector.

isUvVector (value) predicate

True for a single 2D unitless Vector

EXAMPLE

vector(0.5, 1)

canBeTransformUV (value) predicate

Typecheck for Transform

transformUV (linear is Matrix, translation is Vector) returns TransformUV

Construct a TransformUV using the matrix argument for rotation and scaling and the vector argument for translation.

transformUV (translation is Vector) returns TransformUV

Construct a TransformUV that translates without rotation or scaling.

transformUV (value is map) returns TransformUV

identityTransformUV () returns TransformUV

Construct a transform that does nothing (no rotation, scaling, or translation).

tolerantEquals (transform1 is TransformUV, transform2 is TransformUV) predicate

Check that two TransformUVs are the same up to tolerance.

inverse (t is TransformUV) returns TransformUV

Compute the inverse of a TransformUV, such that inverse(t) * t == identityTransform().

scaleUniformlyUV (scale is number) returns TransformUV

Returns a TransformUV that represents a uniform scaling around the origin.

scaleNonuniformly (xScale is number, yScale is number) returns TransformUV

Returns a TransformUV that represents two independent scalings along the X and Y axes, centered around the origin.

rotate (angle is ValueWithUnits) returns TransformUV

Returns a TransformUV that represents a rotation around the origin with the given angle.

units

ValueWithUnits type

A ValueWithUnits is a number with dimensions, such as 1.5 inches, 90 degrees, or 9.81 meters per second per second.

const width is ValueWithUnits = 1.5 * inch;
const angle is ValueWithUnits = 90 * degree;
const g     is ValueWithUnits = 9.81 * meter / second / second;

Values with the same dimensions can be added and subtracted, even if they were created in different unit systems.

const length       = 3 * meter + 1 * inch;
const longerLength = length + 0.01 * inch;
const nonsense     = 3 * meter + 3 * degree;     // Throws an error from dimension mismatch

Multiplication (*) will multiply both the values and the units. An expression where the units all cancel evaluates to plain number.

var doubleLength   = 2 * length;                 // ValueWithUnits with length units
var area           = (20 * foot) * (30 * foot);  // ValueWithUnits with area units
var numberOfBricks = (64 * foot) / (9 * inch);   // number with no units

Values with units can be raised to numerical powers with the ^ operator. Base units like inch or second can be exponentiated in the same way.

var squareArea   = (3 * meter)^2;
var g            = 9.81 * meter / second^2;

Functions in the standard library require a ValueWithUnits for arguments where units are needed. Thus, the depth in opExtrude requires a value with length units (rather than assuming meters). The argument of sin is a value with angle units (rather than assuming radians). The argument of sqrt can be any value whose units are even powers.

var ladderHeight   = ladderLength * sin(75 * degree); // Has length units
var pendulumPeriod = 2 * PI * sqrt(armLength / g);    // Has time units

Equality of ValueWithUnits considers the underlying value, so 25.4 * millimeter is equal to 1 * inch. However, PI * radian / 5 does not equal 36 * degree because of finite precision arithmetic. To check equality of ValueWithUnits, you should use tolerantEquals.

if (tolerantEquals(myLength, 0 * inch))
{
    ...

Keeping correct units on variables is always best practice, in order to benefit from easy unit conversions and runtime unit checks. However, when printing, you may wish to divide out the units in order to display a value in a different system of units.

const length = 42 * centimeter;
println(length);                                 // prints "0.42 meter"
println("length: " ~ toString(length));          // prints "length: 0.42 meter"
println(length / inch ~ " inches");              // prints "16.535433070866137 inches"
println(roundToPrecision(length / inch, 3) ~ " inches"); // prints "16.535 inches"

unitless const

The constant 1, with no units.

meter const

A constant equal to 1 meter.

centimeter const

A constant equal to 1 centimeter.

millimeter const

A constant equal to 1 millimeter.

inch const

A constant equal to 1 inch.

foot const

A constant equal to 1 foot.

yard const

A constant equal to 1 yard.

squareMeter const

A constant equal to one square meter.

squareCentimeter const

A constant equal to one square centimeter.

squareMillimeter const

A constant equal to one square millimeter.

squareInch const

A constant equal to one square inch.

squareFoot const

A constant equal to one square foot.

squareYard const

A constant equal to one square yard.

cubicMeter const

A constant equal to one cubic meter.

cubicCentimeter const

A constant equal to one cubic centimeter.

cubicMillimeter const

A constant equal to one cubic millimeter.

cubicInch const

A constant equal to one cubic inch.

cubicFoot const

A constant equal to one cubic foot.

cubicYard const

A constant equal to one cubic yard.

radian const

A constant equal to 1 radian.

Formally, radians are unitless, so in certain situations you may need to multiply or divide by radian

EXAMPLE

var myAngle = PI / 6 * radian

EXAMPLE

var arcLength = radius * arcAngle / radian

degree const

A constant equal to 1 degree.

kilogram const

A constant equal to 1 kilogram.

gram const

A constant equal to 1 gram.

ounce const

A constant equal to 1 ounce.

pound const

A constant equal to 1 pound.

second const

A constant equal to 1 second

newton const

A constant equal to 1 newton.

kilonewton const

A constant equal to 1 kilonewton.

poundForce const

A constant equal to 1 pound-force.

pascal const

A constant equal to 1 pascal.

kilopascal const

A constant equal to 1 kilopascal.

megapascal const

A constant equal to 1 megapascal.

gigapascal const

A constant equal to 1 gigapascal.

poundPerSquareInch const

A constant equal to 1 pound per square inch.

kilopoundPerSquareInch const

A constant equal to 1 ksi.

newtonMeter const

A constant equal to 1 newton-meter.

newtonMillimeter const

A constant equal to 1 newton-millimeter.

inchPound const

A constant equal to 1 inch-pound.

footPound const

A constant equal to 1 foot-pound.

meterPerSecondSquared const

A constant equal to 1 meter per second squared.

millimeterPerSecondSquared const

A constant equal to 1 millimeter per second squared.

inchPerSecondSquared const

A constant equal to 1 inch per second squared.

footPerSecondSquared const

A constant equal to 1 foot per second squared.

radianPerSecond const

A constant equal to 1 radian per second.

degreePerSecond const

A constant equal to 1 degree per second.

joule const

A constant equal to 1 Joule.

footPoundForce const

A constant equal to 1 foot-pound force.

isLength (val) predicate

True for any value with length units.

isArea (val) predicate

True for any value with area units.

isVolume (val) predicate

True for any value with volume units.

isAngle (val) predicate

True for any value with angle units.

isForce (val) predicate

True for any value with force units.

isPressure (val) predicate

True for any value with pressure units.

isMoment (val) predicate

True for any value with moment units.

isAcceleration (val) predicate

True for any value with acceleration units.

isAngularVelocity (val) predicate

True for any value with angular velocity units.

isEnergy (val) predicate

True for any value with energy units.

reciprocal (val is ValueWithUnits) returns ValueWithUnits

Inverts a value, including units.

tolerantEquals (value1 is ValueWithUnits, value2 is ValueWithUnits) predicate

Returns true if angles are equal up to zeroAngle or anything else is equal up to zeroLength

tolerantGreaterThan (greater, lesser) predicate

Returns true if greater is greater than and not tolerantly equal to lesser.

EXAMPLE

(1 * meter)->tolerantGreaterThan(0 * meter) returns true

EXAMPLE

1->tolerantGreaterThan(0) returns true

EXAMPLE

0->tolerantGreaterThan(-1e-14) returns false

EXAMPLE

0->tolerantGreaterThan(0) returns false

tolerantGreaterThanOrEqual (greater, lesser) predicate

Returns true if greater is greater than or tolerantly equal to lesser.

EXAMPLE

(1 * meter)->tolerantGreaterThanOrEqual(0 * meter) returns true

EXAMPLE

1->tolerantGreaterThanOrEqual(0) returns true

EXAMPLE

0->tolerantGreaterThanOrEqual(0) returns true

EXAMPLE

0->tolerantGreaterThanOrEqual(1e-14) returns true

tolerantLessThan (lesser, greater) predicate

Returns true if lesser is less than and not tolerantly equal to greater.

EXAMPLE

(0 * meter)->tolerantLessThan(1 * meter) returns true

EXAMPLE

0->tolerantLessThan(1) returns true

EXAMPLE

0->tolerantLessThan(1e-14) returns false

EXAMPLE

0->tolerantLessThan(0) returns false

tolerantLessThanOrEqual (lesser, greater) predicate

Returns true if lesser is less than or tolerantly equal to greater.

EXAMPLE

(0 * meter)->tolerantLessThanOrEqual(1 * meter) returns true

EXAMPLE

0->tolerantLessThanOrEqual(1) returns true

EXAMPLE

0->tolerantLessThanOrEqual(0) returns true

EXAMPLE

1e-14->tolerantLessThanOrEqual(0) returns true

tolerantWithinExclusive (value, lesser, greater) predicate

Returns true if value is tolerantly within the interval (lesser, greater).

EXAMPLE

(0.5 * meter)->tolerantWithinExclusive(0 * meter, 1 * meter) returns true

EXAMPLE

0.5->tolerantWithinExclusive(0, 1) returns true

EXAMPLE

1->tolerantWithinExclusive(0, 1) returns false

EXAMPLE

0->tolerantWithinExclusive(0, 1) returns false

EXAMPLE

0->tolerantWithinExclusive(1e-14, 1) returns false

tolerantWithinInclusive (value, lesser, greater) predicate

Returns true if value is tolerantly within the interval [lesser, greater].

EXAMPLE

(0.5 * meter)->tolerantWithinInclusive(0 * meter, 1 * meter) returns true

EXAMPLE

0.5->tolerantWithinInclusive(0, 1) returns true

EXAMPLE

1->tolerantWithinInclusive(0, 1) returns true

EXAMPLE

0->tolerantWithinInclusive(0, 1) returns true

EXAMPLE

0->tolerantWithinInclusive(1e-14, 1) returns true

tolerantEqualsZero (value) predicate

Returns true if value is tolerantly equal to the 0 value with the same units as value.

EXAMPLE

tolerantEqualsZero(0) returns true

EXAMPLE

tolerantEqualsZero(0 * meter) returns true

EXAMPLE

tolerantEqualsZero(1e-9 * meter) returns true

EXAMPLE

tolerantEqualsZero(1) returns false

EXAMPLE

tolerantEqualsZero(1 * meter) returns false

sqrt (value is ValueWithUnits) returns ValueWithUnits

Square root of a ValueWithUnits.

EXAMPLE

sqrt(4 * meter^2) equals 2 * meter.

EXAMPLE

2 * PI * sqrt(armLength / (9.8 * meter/second^2)) equals the period of a pendulum, in seconds.

EXAMPLE

sqrt(4 * meter) throws an error, since FeatureScript has no concept of the square root of a meter.

hypot (a is ValueWithUnits, b is ValueWithUnits)

Hypotenuse function, as sqrt(a^2 + b^2), but without any surprising results due to finite numeric precision.

EXAMPLE

hypot(3 * foot, 4 * foot) equals 5 * foot

sin (value is ValueWithUnits) returns number

Sine, the ratio of the opposite side over the hypotenuse in a right triangle of the specified angle.

EXAMPLE

sin(30 * degree) returns approximately 0.5

EXAMPLE

sin(PI * radian) returns approximately 0

cos (value is ValueWithUnits) returns number

Cosine, the ratio of the adjacent side over the hypotenuse in a right triangle of the specified angle.

EXAMPLE

cos(60 * degree) returns approximately 0.5

EXAMPLE

cos(PI * radian) returns approximately -1

tan (value is ValueWithUnits) returns number

Tangent, the ratio of the opposite side over the adjacent side in a right triangle of the specified angle.

EXAMPLE

tan(45 * degree) returns approximately 1

EXAMPLE

tan(PI * radian) returns approximately 0

asin (value is number) returns ValueWithUnits

Arcsine, i.e. inverse sine.

Returns a value between -90 * degree and 90 * degree.

EXAMPLE

asin(0.5) equals approximately 30 * degree

EXAMPLE

asin(1.5) throws an error, since there is no value where sin(value) is 1.5

acos (value is number) returns ValueWithUnits

Arccosine, i.e. inverse cosine.

Returns a value between 0 * degree and 180 * degree.

EXAMPLE

acos(0.5) equals approximately 60 * degree

EXAMPLE

acos(1.5) throws an error, since there is no value where cos(value) is 1.5

atan (value is number) returns ValueWithUnits

Arctangent, i.e. inverse tangent.

Returns a value between -90 * degree and 90 * degree.

EXAMPLE

atan(1) equals approximately 45 * degree

EXAMPLE

atan(inf) equals approximately 90 * degree

atan2 (y is number, x is number) returns ValueWithUnits

Returns the counterclockwise angle from the vector [0, 1] to the vector [x, y]. The angle is negative if y is negative. This is equivalent to atan(y/x) except the result respects the quadrant of the input and is well-behaved near x == 0.

EXAMPLE

atan2(0, 1) equals approximately 0 * degree

EXAMPLE

atan2(1, 0) equals approximately 90 * degree

EXAMPLE

atan2(0, -1) equals approximately 180 * degree

EXAMPLE

atan2(-1, 0) equals approximately -90 * degree

atan2 (y is ValueWithUnits, x is ValueWithUnits) returns ValueWithUnits

Returns the counterclockwise angle from the vector [0, 1] to the vector [x, y], assuming the units of y and x match.

See also

atan2(number, number)

isAngleBetween (queryAngle is ValueWithUnits, minAngle is ValueWithUnits, maxAngle is ValueWithUnits)

Returns true if the provided angle is within the given range (inclusive with tolerance), "winding" the query angle as necessary to put it within a positive full circle turn of the range. Ranges that encompass one or more full circles will return true regardless of the query angle.

Throws if range's maximum angle is less than the minimum angle.

EXAMPLE

isAngleBetween(0.5 * PI * radian, 0 * radian, PI * radian) returns true

EXAMPLE

isAngleBetween(0.5 * PI * radian, 2 * PI * radian, 3 * PI * radian) returns true

EXAMPLE

isAngleBetween(-1.5 * PI * radian, 0 * radian, PI * radian) returns true

floor (value, multiple)

Round a value down to nearest given multiple.

EXAMPLE

floor(125, 10) returns 120

EXAMPLE

floor(-15, 10) returns -20

EXAMPLE

floor(3.14 * inch, 0.1 * inch) equals 3.1 * inch

ceil (value, multiple)

Round a value up to nearest given multiple.

EXAMPLE

ceil(125, 10) returns 130

EXAMPLE

ceil(-15, 10) returns -10

EXAMPLE

ceil(3.14 * inch, 0.1 * inch) equals 3.2 * inch

round (value, multiple)

Round a value to nearest given multiple.

EXAMPLE

round(125, 10) returns 130

EXAMPLE

round(-15, 10) returns -10

EXAMPLE

round((10 / 3) * meter, centimeter) equals 3.33 * meter

EXAMPLE

round(1 * meter, .001 * inch) equals 39.37 * inch

For small values of multiple, roundToPrecision is preferred to reduce floating point errors.

toString (value is ValueWithUnits) returns string

General value to string conversion.

parseJsonWithUnits (s is string)

Parse a JSON string into either a map or array. Null values in the JSON are returned as undefined. Throws if the string is not well-formed JSON. Applicable strings are parsed into a ValueWithUnits. For instance, "3 inch" will map to a ValueWithUnits with length units that repreresents 3 inches.

Return type	Description
	A map or an array corresponding to the JSON value.

vector

Vector type

A Vector is a non-empty array. It should contain numbers or lengths.

Operators +, -, *, and / are overloaded for vectors, and other operations such as dot product are available. If a vector does not contain numbers or lengths, operations that assume number-like properties may fail.

canBeVector (value) predicate

Typecheck for Vector

vector (value is array) returns Vector

Make a Vector from an array.

vector (x, y) returns Vector

Construct a 2-dimensional vector.

vector (x, y, z) returns Vector

Construct a 3-dimensional vector.

isLengthVector (value) predicate

True for a Vector where all members are values with length units.

EXAMPLE

vector([1, 2, 3, 4, 5]) * inch

isUnitlessVector (value) predicate

True for a Vector where all members are simple numbers.

EXAMPLE

vector([1, 2, 3, 4, 5])

is2dPoint (value) predicate

True for a single 2D length Vector

EXAMPLE

vector(0.5, 1) * inch

is2dPointVector (value) predicate

True for an array where all members are 2D lengths.

EXAMPLE

[vector(0, 0) * inch, vector(0, 1) * inch, vector(1, 0) * inch]

is2dDirection (value) predicate

True for a unitless 2D Vector that is normalized (i.e. has length 1)

EXAMPLE

vector(0, 1)

is3dLengthVector (value) predicate

True for a 3D Vector where all members are values with length units.

EXAMPLE

vector(0, 1.5, 30) * inch

is3dDirection (value) predicate

True for a unitless 3D Vector that is normalized (i.e. has length 1)

EXAMPLE

vector(0, 0, 1)

zeroVector (size is number) returns Vector

Make an array filled with 0.

EXAMPLE

zeroVector(3) is equivalent to vector(0, 0, 0)

squaredNorm (vector is Vector)

Returns the squared length of a vector. This is slightly faster to calculate than the length.

norm (vector is Vector)

Returns the length (norm) of a vector.

dot (vector1 is Vector, vector2 is Vector)

Returns the dot product of two vectors.

cross (vector1 is Vector, vector2 is Vector) returns Vector

Returns the cross product of two 3-dimensional vectors.

angleBetween (vector1 is Vector, vector2 is Vector) returns ValueWithUnits

Returns the angle between two 3-dimensional vectors. Values are within the range [0, PI] * radian.

EXAMPLE

angleBetween(X_DIRECTION, Y_DIRECTION) equals PI/2 * radian

EXAMPLE

angleBetween(Y_DIRECTION, X_DIRECTION) equals PI/2 * radian

A plane is fitted to the two vectors and the shortest angle between them is measured on that plane.

angleBetween (vector1 is Vector, vector2 is Vector, ref is Vector) returns ValueWithUnits

Returns the counterclockwise angle between two 3-dimensional vectors as witnessed from the tip of a third 3-dimensional vector. Values are within the range (-PI, PI] * radian with negative values indicating clockwise angles.

EXAMPLE

angleBetween(X_DIRECTION, Y_DIRECTION, Z_DIRECTION) equals PI/2 * radian

EXAMPLE

angleBetween(Y_DIRECTION, X_DIRECTION, Z_DIRECTION) equals -PI/2 * radian

The first two vectors are projected onto a plane perpendicular to the reference vector and the angle is measured according to that projection.

normalize (vector is Vector) returns Vector

Returns the (unitless) result of normalizing vector. Throws if the input is zero-length.

Parameter	Type	Additional Info
`vector`	`Vector`	A Vector with any units.

project (target is Vector, source is Vector) returns Vector

Project the source vector onto the target vector. Equivalent to target * dot(source, target) / squaredNorm(target).

perpendicularVector (vec is Vector) returns Vector

Returns a vector perpendicular to the given vector. The choice of which perpendicular vector to return is arbitrary but consistent for the same input. The returned vector is unitless and of length 1.

rotationMatrix3d (from is Vector, to is Vector) returns Matrix

Construct a 3D rotation matrix that represents the minimum rotation that takes the normalized from vector to the normalized to vector. The inputs may have any units.

rotationMatrix3d (axis is Vector, angle is ValueWithUnits) returns Matrix

Construct a 3D matrix representing a counterclockwise (looking against the axis) rotation around the given axis by the given rotation angle.

scalarTripleProduct (vector1 is Vector, vector2 is Vector, vector3 is Vector)

Returns the scalar triple product, a dot (b cross c), of three 3-dimensional vectors.

toString (value is Vector) returns string

tolerantEquals (point1 is Vector, point2 is Vector) predicate

Returns true if two vectors designate the same point (within tolerance) or the same direction (within tolerance).

parallelVectors (vector1 is Vector, vector2 is Vector) returns boolean

Returns true if two vectors are parallel (within tolerance).

perpendicularVectors (vector1 is Vector, vector2 is Vector) returns boolean

Returns true if two vectors are perpendicular (within tolerance).

clusterPoints (points is array, tolerance is ValueWithUnits) returns array

Groups points into clusters. Two points farther than tolerance apart are guaranteed to be in separate clusters. A set of points all within tolerance of each other that has no other points within tolerance is guaranteed to be a single cluster.

Return type	Description
`array`	Array of arrays, where each array is a cluster of nearby points, represented as indices into points array.

Utilities

attributes

Attributes are data attached to individual entities, which can be set and retrieved by name in FeatureScript. The data can be of any type, and multiple attributes with different names can be associated with the same topological entity.

One common use case for attributes is to set attributes on an entity in one feature, and get them in another. For data not associated with entities, the same thing can be accomplished simply via setVariable and getVariable, but attributes allow that data to be set on specific bodies, faces, edges, or vertices.

setAttribute(context, {
   "entities" : somePart,
   "name" : "refPoint",
   "attribute" : vector(0, 0, 1) * inch
});
// Later, possibly in another feature:
const partRefPoint = getAttribute(context, {
   "entity" : somePart,
   "name" : "refPoint"
});
if (partRefPoint != undefined)
{
    // use partRefPoint...
}

Attributes are also a useful way to mark important groups of entities for other features or other deriving Part Studios. You can query for entities with a specific attribute, a specific attribute value, or a value matching a given pattern with the query functions qHasAttribute, qHasAttributeWithValue, or qHasAttributeWithValueMatching, respectively.

Attributes stay with the entity they are defined on, even as the Part Studio changes. An attribute on a face, edge, or body which is split in two will be set with the same name and value on both split pieces. An attribute on a patterned entity will be set on each patterned copy. If two or more entities are merged together (e.g. with a boolean union), then the attributes on both are kept on the result, though if they have attributes with the same name, the value of the primary entity (e.g. the first resolved body in the boolean tools) will be used.

Legacy unnamed attributes: A previous use of these attribute functions involved setting unnamed attributes by calling setAttribute without a "name". This workflow is still supported, but is no longer recommended. Legacy unnamed attributes can be identified and retrieved only by type, and two attributes of the same type are not allowed on the same entity. The behavior of these unnamed attributes, described in "Legacy unnamed attribute" notes like this one, can be safely ignored if all your attributes are set with a "name".

setAttribute (context is Context, definition is map)

Attach an attribute to one or several entities. Will overwrite any attribute previously set on the same entity with the same name.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	Entities to attach attribute to. Throws an error if the query resolves to nothing.
`name`	`string`	The name of the attribute
`attribute`		The data to set. Can be any type. If `undefined` is provided, any existing attribute will be unset (and this entity will no longer resolve in `qHasAttribute` and similar functions) Legacy unnamed attributes: If name is not provided, adds an unnamed attribute to the entities. If more than one unnamed attribute with the same type is set on any entity, throws an error.

getAttributes (context is Context, definition is map) returns array

Get attributes attached to entities.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	Entities to get attributes on. If query resolves to nothing, empty array is returned
`name`	`string`	The name of the attribute to get.
`attributePattern`		Optional Providing a map here will also filter out attributes which do not have entries precisely matching the keys and values of `attributePattern`, similar to `qHasAttributeWithValueMatching`. EXAMPLE `{ "odd" : true }` matches all attributes values are maps with a field `"odd"` whose value is `true`. Legacy unnamed attributes: If `attributePattern` is provided and `name` is not, getAttributes will only return unnamed attributes with the same type as `attributePattern`, using the same behavior documented in the legacy function `qAttributeFilter`.

Return type	Description
`array`	An array of all unique attributes on the given entities matching the pattern.

getAttribute (context is Context, definition is map)

Get the value of a single named attribute attached to a single entity, or undefined if no attribute of that name has been set.

EXAMPLE

setAttribute(context, { "entities" : someEntities, "name" : "importantData", "attribute" : 42});
for (const entity in evaluateQuery(entities)) {
    const value = getAttribute(context, {
        "entity" : entity,
        "name" : "importantData"
    });
    println(value); // prints 42
}

Parameter	Type	Additional Info
`definition`	`map`
`entity`	`Query`	Query resolving to a single entity to get the attribute from. If multiple entities are resolved, the first resolved entity is considered.
`name`	`string`	Name of the attribute

getAllAttributes (context is Context, definition is map) returns map

Get the named attributes attached to a single entity, or an empty map if the entity has no attributes.

Parameter	Type	Additional Info
`definition`	`map`
`entity`	`Query`	Query resolving to a single entity to get the attributes from.

Return type	Description
`map`	A map from attribute names to attribute values for all of the attributes on the given entity.

removeAttributes (context is Context, definition is map)

Has no effect on named attributes, instead use setAttribute with "attribute" : undefined.

Legacy unnamed attributes: Remove matching unnamed attributes attached to entities.

Parameter Type Additional Info

definition map

entities

Query

Optional

Entities to remove unnamed attributes from. Default is everything.

attributePattern

Optional

If provided, will only remove attributes with the same type, using the same behavior documented in the legacy function qAttributeFilter.

computedPartProperty

defineComputedPartProperty (propertyFunction is function) returns function

This function takes a computed part property function and wraps it to define a computed part property. It is analogous to defineFeature, except that it is used to define computed part properties. A typical usage is something like:

annotation { "Property Function Name" : "MyProperty" }  // annotation required for Onshape to recognize computed property function
export const myProperty = defineComputedPartProperty(function(context is Context, part is Query, definition is map)
    returns ValueWithUnits // may also return string or boolean or number
    // definition is an empty map and reserved for future use
    {
        ... // Compute and return the property value, using the context and the parameters
    });

For more information on writing computed part properties, see Computed part properties in the FeatureScript guide.

Parameter	Type	Additional Info
`propertyFunction`	`function`	A function that takes a `context`, a `part` Query that returns a single Part, and a `definition`, and that returns a value such as a number or a string or a ValueWithUnits.

containers

This module contains functions for working with FeatureScript arrays (e.g. [1, 2, 3]) and maps (e.g. { "x" : 1, "y" : true })

makeArray (size is number, fillValue) returns array

Create a new array with given size, filled with fillValue. Note: this is equivalent to assigning each individual array element to fillValue; boxes and builtins will not be deep-copied.

EXAMPLE

makeArray(3, 0) returns [0, 0, 0]

makeArray (size is number) returns array

Create a new array with given size, filled with undefined.

EXAMPLE

makeArray(3) returns [undefined, undefined, undefined]

size (container is array) returns number

Returns the size of an array. This counts only direct children; it does not recursively examine containers inside.

EXAMPLE

size([1, 2, 3]) returns 3

EXAMPLE

size([1, [2, 3]]) returns 2

size (container is map) returns number

Returns the size of an map. This counts only direct children; it does not recursively examine containers inside.

EXAMPLE

size({ "x" : 1, "y" : 2 }) returns 2

isIn (value, container is array) returns boolean

Returns true if value appears in an array, using == for comparison.

EXAMPLE

isIn(1 * inch, [0 * inch, 1 * inch, 2 * inch]) returns true

indexOf (container is array, value) returns number

Return the index of the value in container, or -1 if the value is not found.

indexOf (container is array, value, startIndex is number) returns number

Return the index of the value in container starting the search at a specified start index, or -1 if the value is not found.

isValueIn (value, container is map) returns boolean

Returns true if value appears as the value of a map entry, using == for comparison.

EXAMPLE

isValueIn(true, { "a" : true, "b" : 0 }) returns true

EXAMPLE

isValueIn("b", { "a" : true, "b" : 0 }) returns false

mapArray (arr is array, mapFunction is function) returns array

Returns a new array, with the same size as arr, created by mapping each element of arr through a mapFunction.

EXAMPLE

mapArray([0, 1], function(x) { return -x; }) returns [0, -1]

Parameter	Type	Additional Info
`mapFunction`	`function`	A function which takes in one argument (a member of the input array) and returns a value.

resize (arr is array, newSize is number, newValue) returns array

Returns a copy of an array with size changed to newSize. If the new size is larger than the original size, the extra values are set to newValue.

EXAMPLE

resize([1, 2, 3], 2, 0) returns [1, 2]

EXAMPLE

resize([1, 2, 3], 5, 0) returns [1, 2, 3, 0, 0]

resize (arr is array, newSize is number) returns array

Returns a copy of an array with size changed to newSize. If the new size is larger than the original size, the extra values are set to undefined.

append (arr is array, newValue) returns array

Returns a copy of an array with a single value added to the end.

EXAMPLE

append([1, 2], 3) returns [1, 2, 3]

concatenateArrays (arr is array) returns array

Given an array of arrays, concatenate the contents of the inner arrays.

EXAMPLE

concatenateArrays([[1, 2], [3, 4]]) returns [1, 2, 3, 4]

EXAMPLE

concatenateArrays([[1], [], [2, undefined], [[3]]]) returns [1, 2, undefined, [3]]

mergeMaps (defaults is map, m is map) returns map

Add each key-value pair in the second map to a copy of first and return the result. Since later-added entries take precedence, nothing from the second map will be lost.

In other words, any keys from defaults which are missing from m will be filled in with their values from defaults.

EXAMPLE

mergeMaps({a:0}, {a:1}) returns {a:1}

EXAMPLE

mergeMaps({a:0}, {b:1}) returns {a:0, b:1}

intersectMaps (maps is array) returns map

Compute the intersection of the keysets of the input maps. In other words, returns a map whose keys are present in all input maps and whose values are taken from the last map.

EXAMPLE

intersectMaps([{a:0}, {a:1}]) returns {a:1}

EXAMPLE

intersectMaps([{a:0}, {b:1}]) returns {}

EXAMPLE

intersectMaps([{a:0, b:1}, {a:0, b:2}]) returns {a:0, b:2}

reverse (arr is array) returns array

Return a copy of an array with elements in reverse order.

EXAMPLE

reverse([1, 2, 3]) returns [3, 2, 1]

sort (entities is array, compareFunction is function)

Return a sorted copy of an array. Current implementation uses merge sort.

EXAMPLE

sort([3, 1, 2], function(a, b) { return a - b; }) returns [1, 2, 3]

Parameter	Type	Additional Info
`compareFunction`	`function`	A function that takes two values, returns a negative value if the first is before the second, `0` if the two are equal, and positive value if the second is before the first.

tolerantSort (values is array, tolerance) returns array

Returns a sorted copy of values, where any sequence of values within tolerance of each other is sorted in the order of the original array.

This is useful when sorting by a geometric measurement (like length, area, or volume) because it makes it much less likely that a tiny change in that computed value will change the resulting sort order.

EXAMPLE

tolerantSort([5, 1.000001, 1, 8], 0.001) returns [1.000001, 1, 5, 8]

EXAMPLE

tolerantSort( [1 * inch, 1.00009 * inch, 0.99991 * inch], 0.0001 * inch) returns [1 * inch, 1.00009 * inch, 0.99991 * inch]. The order is entirely unchanged since two pairs of values are within the tolerance (even though the third pair isn't).

Parameter	Type	Additional Info
`values`	`array`	An array of `number` or `ValueWithUnits`.
`tolerance`		Tolerance for comparing elements of `values`.

tolerantSort (entities is array, tolerance, mapFunction) returns array

Performs a tolerantSort of entities, ordering by the value returned by mapFunction. Like tolerantSort, the original order will be preserved for values within tolerance for stability.

Parameter Type Additional Info

tolerance

EXAMPLE

1e-7 * meter

mapFunction

A function taking in a single entity and returning a sortable number or ValueWithUnits.

EXAMPLE

function(entity is Query) { return evLength(context, {"entities" : entity}); } to sort entities by increasing length.

filter (arr is array, filterFunction is function)

Return the members of an array matching a predicate function, preserving element order.

Throws exception if filterFunction throws, or if the filterFunction does not return boolean.

EXAMPLE

filter([1, 2, 3, 4, 5, 6], function(x) { return x % 2 == 0; }) returns [2, 4, 6]

Parameter	Type	Additional Info
`filterFunction`	`function`	A function which takes one argument (a member of the input array) and returns a `boolean`.

first (m is map)

Return the first item in a map

keys (container is map) returns array

Returns the keys in the supplied map in map iteration order.

EXAMPLE

keys({ "a" : 1, "c" : 2, "b" : 3 }) returns ["a", "b", "c"]

values (container is map) returns array

Returns the values in the supplied map ordered by the map iteration ordering of their associated keys.

EXAMPLE

values({ "a" : 1, "c" : 2, "b" : 3 }) returns [1, 3, 2]

subArray (input is array, startIndex is number) returns array

Returns the subarray beginning at startIndex

subArray (input is array, startIndex is number, endIndex is number) returns array

Returns the subarray [startIndex, endIndex)

insertIntoMapOfArrays (mapToInsertInto is map, key, value) returns map

Inserts value into the array keyed by key, returns the updated map

last (elements is array)

Returns last element of array.

rotateArray (elements is array, step is number) returns array

Returns a rotated array of the same elements. step less than zero moves elements towards the front. step greater than zero moves elements towards the back.

EXAMPLE

rotateArray([0, 1, 2], -1) returns [1, 2, 0]

insertElementAt (arr is array, index is number, value) returns array

Returns an array with value inserted at index.

removeElementAt (arr is array, index is number) returns array

Returns an array with the element at index removed.

all (arr is array, checkFunction is function) returns boolean

Returns true if and only if all elements of an array, when passed into the checkFunction, return true.

EXAMPLE

all([0, 2, 4], function(e){ return e % 2 == 0; }) returns true

EXAMPLE

all([], function(e){ return false; }) returns true

See also

all(array)

Parameter	Type	Additional Info
`arr`	`array`	An array of elements to be checked.
`checkFunction`	`function`	A unary function that returns a boolean.

Return type	Description
`boolean`	`true` if and only if all `checkFunction(element)` calls return `true`.

all (arr is array) returns boolean

Returns true if all elements in the passed array are true.

EXAMPLE

all([]) returns true

EXAMPLE

all([false, false, true]) returns false

EXAMPLE

all([true, true, true]) returns true

See also

all(array, function)

Parameter	Type	Additional Info
`arr`	`array`	An array of booleans.

Return type	Description
`boolean`	`true` if and only if all `element`s are `true`.

allCombinations (arr is array) returns array

Creates all possible combinations from arrays of values for each element.

EXAMPLE

allCombinations([[1,2], [3,4]]) returns [[1,3], [1,4], [2,3], [2,4]]

EXAMPLE

allCombinations([[0, 1, 2, 3]]) returns [[0], [1], [2], [3]]

EXAMPLE

allCombinations([[], [0, 1, 2]]) returns []

Parameter	Type	Additional Info
`arr`	`array`	An array of arrays, where each array represents all possible values for the given array's index in the returned arrays.

Return type	Description
`array`	An array of all possible combinations that have exactly one element from each of the input arrays.

any (arr is array, check is function) returns boolean

Returns true if any element of an array, when passed into the check function, returns true.

EXAMPLE

any([1, 3, 4], function(e){ return e % 2 == 0; }) returns true

EXAMPLE

any([], function(e){ return true; }) returns false

See also

any(array)

Parameter	Type	Additional Info
`arr`	`array`	An array of elements.

Return type	Description
`boolean`	`true` if and only if at least one `check(element)` call returns `true`.

any (arr is array) returns boolean

Returns true if any element in the passed array is true.

EXAMPLE

any([]) returns false

EXAMPLE

any([false, false, true]) returns true

See also

any(array, function)

Parameter	Type	Additional Info
`arr`	`array`	An array of booleans.

Return type	Description
`boolean`	`true` if and only if at least one `element` is `true`.

average (arr is array)

Returns the average of an array. All array elements must be mutually addable and divisible by a number.

EXAMPLE

average([1, 2, 3, 4]) returns 2.5

EXAMPLE

average([vector([1, 0, 0])*meter, vector([0, 0, 0])*meter, vector([0, 1, 0])*meter]) returns vector(1/3, 1/3, 0) * meter

Parameter	Type	Additional Info
`arr`	`array`	An array of mutually addable and divisible elements.

Return type	Description
	The average of values in the passed in array.

deduplicate (arr is array) returns array

Deduplicate an array. Maintains original array order, eliminating all but the first occurrence of a given duplicate.

EXAMPLE

deduplicate([1, 2, 1, 3, 2, 0, 0]) returns [1, 2, 3, 0]

EXAMPLE

deduplicate([]) returns []

Parameter	Type	Additional Info
`arr`	`array`	An array of values to be deduplicated.

Return type	Description
`array`	An array of deduplicated values.

foldArray (arr is array, seed, foldFunction is function)

Folds an array from left to right with a foldFunction.

EXAMPLE

foldArray([1, 2, 3], 0, function(accumulator, element) { return accumulator + element; }) returns 6

Parameter	Type	Additional Info
`arr`	`array`	An array to fold.
`seed`		The initial value of the accumulator to be passed into the `foldFunction`.
`foldFunction`	`function`	A binary function which takes in an accumulator (the seed for the first iteration, and the result of the previous call for subsequent iterations) and an element of the passed in array.

Return type	Description
	The accumulator after all elements of `arr` have been folded.

foldArray (arr is array, foldFunction is function)

Calls foldArray with the seed set to the first element of arr.

See also

foldArray

mapArrayIndices (arr is array, mapIndexFunction is function) returns array

Returns a new array, with the same size as arr, created by mapping each index of arr through a mapIndexFunction.

EXAMPLE

const myArray = [1, 3, 5]; mapArrayIndices(myArray, function(i) { return myArray[i] + myArray[ (i+1) % size(myArray)]; }) returns [4, 8, 6]

Parameter	Type	Additional Info
`mapIndexFunction`	`function`	A function which takes in one argument (an index of the input array) and returns a value.

Return type	Description
`array`	The results of calling `mapIndexFunction` on the indices of all elements in the passed in `arr`.

mapValue (value, mapFunction is function)

Map a value using a mapFunction and return the result. Particularly useful when using a lambda function inline to dynamically change some value.

EXAMPLE

mapValue(4, function(n){ return n+1; }) returns 5

EXAMPLE

couldBeUndefined->mapValue(function(v){ return v == undefined ? 'a great default' : v; })

Parameter	Type	Additional Info
`value`		Anything that the passed in mapFunction will accept as a parameter.
`mapFunction`	`function`	A function that will be called on the passed in `value`.

Return type	Description
	The result of calling `mapFunction` with `value`.

memoizeFunction (f is function) returns function

Memoize a unary (one-parameter) function. Once memoized, if the returned function is called with the same parameter twice, the second return value will be fetched from an internal cache. This can dramatically speed up calculations - particularly when f is called with the same parameter many times. The overhead of memoizing a function is negligible. Note that memoization will not properly work with functions that have side effects, such as modifying a box.

EXAMPLE

const square = memoizeFunction(function(n){ return n^2; });
println(square(5)); // calls f internally and prints 25
println(square(5)); // retrieves cached value of 25 and returns it

Parameter	Type	Additional Info
`f`	`function`	A unary function to be memoized.

Return type	Description
`function`	A memoized function that will return the same thing as f.

mergeMaps (defaults, keyList is array, newNode)

Merge maps at a particular location as specified by the keyList. If either the destination node specified by the keyList or the newNode is not a map, the newNode will replace the destination node.

EXAMPLE

mergeMaps({ a: [ { b: 2 } ] }, ['a', 0, 'b'], 4) returns { a : [ { b : 4 } ] }

EXAMPLE

mergeMaps(5, [], 4) returns 4

EXAMPLE

mergeMaps({ a : 5 }, ['a'], 4) returns {a: 4 }

See also

mergeMaps(map, map)

Parameter	Type	Additional Info
`defaults`		A container (array or map) that will be merged at the location specified by the `keyList`. If `defaults` is not an array or map and `keyList` is empty, the result is `newNode` since a merge isn't possible.
`keyList`	`array`	An array of map keys or array indices that collectively specify a location within `defaults` to perform the merge.
`newNode`		A value that will be merged into defaults at the location specified by `keyList`. If the `newNode` specified is a map and the node identified by `keyList` is a map, then this will perform a `mergeMaps` operation.

Return type	Description
	The merged or replaced value.

sum (arr is array)

Sum an array of elements that are all mutually addable. An empty array returns 0.

EXAMPLE

sum(range(0,5)) returns 15

EXAMPLE

sum([vector(1, 2, 3) * meter, vector(4, 5, 6) * meter]) returns vector(5, 7, 9) * meter

EXAMPLE

sum([]) returns 0

Parameter	Type	Additional Info
`arr`	`array`	An array of mutually addable elements to be summed.

Return type	Description
	The sum of values in the passed in array.

zip (arr is array) returns array

Makes an array that aggregates elements from each of the arrays. Returns an array of arrays, where the i-th array contains the i-th element from each of the argument arrays. The array stops when the shortest input array is exhausted. With a single array argument, it returns an array of single element arrays. With no arguments, it returns an empty array.

EXAMPLE

zip([range(0,3), range(10,13), range(20,26)]) returns [[0, 10, 20], [1, 11, 21], [2, 12, 22], [3, 13, 23]]

EXAMPLE

zip([]) returns []

EXAMPLE

zip([range(0, 3)]) returns [[0],[1],[2],[3]]

See also

zip(array, array)

Parameter	Type	Additional Info
`arr`	`array`	An array of arrays to aggregate.

Return type	Description
`array`	An array where the i'th element contains the i'th element from each of the passed in arrays.

zip (a is array, b is array) returns array

An alternative way to call zip(array) that facilitates chaining arguments.

EXAMPLE

zip(range(0,3), range(1, 4)) returns [[0, 1], [1, 2], [2, 3], [3, 4]]

EXAMPLE

zip(range(0,3), []) returns []

See also

zip(array)

Parameter	Type	Additional Info
`a`	`array`	The first array to zip.
`b`	`array`	The second array to zip.

Return type	Description
`array`	An array of length-2 arrays. For the i'th array, the first element is the i'th element of `a` and the second is the i'th element of `b`.

debug

debug (context is Context, value, color is DebugColor)

Print and, if applicable, display value in a Part Studio, highlighting or creating entities in a chosen color, red by default.

The displayed data will ONLY be visible when the feature calling the debug function is being edited. Entities displayed during debug are for display only, and will not appear in any queries.

Values which can be debugged are:

Query: Highlights entities matching the Query (bodies, faces, edges, and vertices) in red.

3D length Vector: Displays a single point in world space.

Unitless, normalized 3D Vector: Displays an arrow starting at the world origin, pointing in the given direction.

Line: Displays an arrow starting at the line's origin, pointing in the line's direction.

CoordSystem: Displays three perpendicular arrows from the coordinate system's origin, along its three axes. The arrowhead for the x-axis is largest, and the z-axis is smallest.

Plane: Displays a large square in the positive quadrant of the plane, along with three arrows along the plane's x-axis, y-axis, and normal.

Box3d: Displays the edges of the bounding box (in the given coordinate system, if provided)

The overloads in this module define these behaviors.

Parameter Type Additional Info

color

DebugColor

Optional

The color of the debug highlight

debug (context is Context, value)

debug (context is Context, value is ValueWithUnits, color is DebugColor)

debug (context is Context, value is Vector, color is DebugColor)

debug (context is Context, value is Query, color is DebugColor)

debug (context is Context, value is Line, color is DebugColor)

debug (context is Context, value is CoordSystem)

debug (context is Context, value is CoordSystem, color is DebugColor)

debug (context is Context, value is CoordSystem, xColor is DebugColor, yColor is DebugColor, zColor is DebugColor)

debug (context is Context, value is Plane, color is DebugColor)

debug (context is Context, point1 is Vector, point2 is Vector, color is DebugColor)

Draws a line between point1 and point2 and prints the points with the distance between them.

debug (context is Context, point1 is Vector, point2 is Vector)

debug (context is Context, boundingBox is Box3d, color is DebugColor)

Displays the edges of a Box3d in the world coordinate system with a chosen DebugColor.

debug (context is Context, boundingBox is Box3d, cSys, color is DebugColor)

Displays the edges of a Box3d in the given coordinate system with a chosen DebugColor.

EXAMPLE

const myBox = evBox3d(context, { "topology" : entities, "cSys" : myCSys });
debug(context, myBox, myCSys, DebugColor.RED);

debug (context is Context, boundingBox is Box3d, cSys)

addDebugEntities (context is Context, entities is Query, color is DebugColor)

Highlights entities in a given DebugColor, without printing anything.

As with debug, highlighted entities are only visible while the debugged feature's edit dialog is open.

addDebugEntities (context is Context, entities is Query)

addDebugPoint (context is Context, point is Vector, color is DebugColor)

Highlights a 3D point in a given DebugColor, without printing anything.

As with debug, highlighted entities are only visible while the debugged feature's edit dialog is open.

addDebugPoint (context is Context, point is Vector)

addDebugLine (context is Context, point1 is Vector, point2 is Vector, color is DebugColor)

Draws a line in 3D space from point1 to point2 with a chosen DebugColor.

As with debug, highlighted entities are only visible while the debugged feature's edit dialog is open.

Parameter	Type	Additional Info
`point1`	`Vector`	one endpoint of the line.
`point2`	`Vector`	the other endpoint of the line.

addDebugLine (context is Context, point1 is Vector, point2 is Vector)

addDebugArrow (context is Context, from is Vector, to is Vector, radius is ValueWithUnits, color is DebugColor)

Draws an arrow in 3D space from from to to with a chosen DebugColor.

As with debug, highlighted entities are only visible while the debugged feature's edit dialog is open.

Parameter Type Additional Info

radius

ValueWithUnits

Width of the four arrowhead lines

EXAMPLE

.25 * centimeter

addDebugArrow (context is Context, from is Vector, to is Vector, radius is ValueWithUnits)

startTimer (timer is string)

Starts the timer associated with the string timer or resets it. Use with printTimer(string).

startTimer ()

Starts the global timer associated with the empty string or resets it. Use with printTimer().

printTimer (timer is string)

Prints the elapsed milliseconds for the timer associated with the string timer. Use with startTimer(string).

Note that if the timer was set in a prior feature, the elapsed time may be very large because features can be regenerated at different times.

Throws an error if no such timer has been started.

printTimer ()

Prints the elapsed milliseconds for the global timer associated with the empty string. Use with startTimer().

Note that if the timer was set in a prior feature, the elapsed time may be very large because features can be regenerated at different times.

Throws an error if no such timer has been started.

decalUtils

DecalData type

Data representing a decal that is mapped onto a face.

Value	Type	Description
`DecalData`	`map`
`decalId`	`Id`	A unique id to represent the decal in the context of the face on which it is placed. The id should correspond to the id of the creating feature, or be a sub-id of the creating feature.
`imageMappingType`	`ImageMappingType`	The type of projection mapping to use for this decal
`image`	`ImageData`	The image that is being mapped.
`uvTransform`	`TransformUV`	A post-projection transformation that is applied in UV space. This can be used to further translate, rotate, and scale a projected image.
`planeSystem`	`PersistentCoordSystem`	Optional A coordinate system representing the plane for the ImageMappingType.PLANAR type. This field must be defined if the `imageMappingType` field is of type `ImageMappingType.PLANAR`. The center of the image will project to the plane's origin. The right edge of the image is along the positive X direction of the coordinate system. The top edge of the image is along the positive Y direction of the coordinate system. See `planeToCSys` for deriving a coordinate system from a `Plane` object.
`cylinder`	`Cylinder`	Optional The cylinder onto which the decal is mapped. This field must be defined if the `imageMappingType` field is of type `ImageMappingType.CYLINDRICAL`.
`cylinderSystem`	`PersistentCoordSystem`	Optional A coordinate system used in projecting the image onto the given cylinder. This field must be defined if the `imageMappingType` field is of type `ImageMappingType.CYLINDRICAL`. The coordinate system's origin must lie on the cylinder's axis with the system's Z axis aligned with the cylinder's own axis. The center of the horizontal extents of the image coincide with the intersection of the coordinate system's x axis and the cylinder. The center of the vertical extents of the image coincide with the projection of the coordinate system's origin on the cylinder. The top edge of the image is along the positive Z direction of the coordinate system projected on the cylinder.

createPlanarDecal (decalId is Id, image is ImageData, planeSystem is CoordSystem, uvTransform is TransformUV) returns DecalData

Creates data for a planar decal. This can be applied to a face using associateDecalAttribute.

See also

DecalData

Parameter	Type	Additional Info
`decalId`	`Id`	The id to for the decal
`image`	`ImageData`	The image to use for the data
`planeSystem`	`CoordSystem`	The coordinate system to use for the planar projection
`uvTransform`	`TransformUV`	A post-projection transform to apply to the decal

createCylindricalDecal (decalId is Id, image is ImageData, cylinder is Cylinder, uvTransform is TransformUV) returns DecalData

Creates data for a cylindrical decal. This can be applied to a face using associateDecalAttribute.

See also

DecalData

Parameter	Type	Additional Info
`decalId`	`Id`	The id to for the decal
`image`	`ImageData`	The image to use for the data
`cylinder`	`Cylinder`	The cylinder definition to use for projection
`uvTransform`	`TransformUV`	A post-projection transform to apply to the decal

associateDecalAttribute (context is Context, entities is Query, decalData is DecalData)

Associate the given decal data as an attribute on the entities provided. This will append the decal to any existing decals associated with the given entities.

Associating a decal in this way will cause the data to be transmitted to Onshape clients where they will be rendered.

createUvTransform (decalWidth is ValueWithUnits, mirrorHorizontal is boolean, decalHeight is ValueWithUnits, mirrorVertical is boolean, decalRotation is ValueWithUnits) returns TransformUV

Creates a UV transform suitable for scaling, mirroring, and rotating a decal after it's been projected.

Parameter	Type	Additional Info
`decalWidth`	`ValueWithUnits`	The width of the decal, post-transformation
`mirrorHorizontal`	`boolean`	If true, the image will be mirrored about its center horizontally
`decalHeight`	`ValueWithUnits`	The height of the decal, post-transformation
`mirrorVertical`	`boolean`	If true, the image will be mirrored about its center vertically
`decalRotation`	`ValueWithUnits`	An amount of rotation to apply to decal about the image center.

getWorldSpacePosition (decalData is DecalData, uv is Vector)

Unprojects the given point in UV space to its corresponding world position for the given decal data. The UV is equivalent to the texture coordinate for the UV that is ultimately used to render the decal.

See also

getDecalUvSpacePosition

getDecalUvSpacePosition (decalData is DecalData, worldPosition is Vector)

Projects the given world position into UV space for the given decal data. The UV computed is equivalent to the texture coordinate for the UV that is ultimately used to render the decal.

See also

getWorldSpacePosition

defaultFeatures

newContextWithDefaults () returns Context

Creates a Context with default planes and an origin.

qDefaultBodies () returns Query

A query for all default created bodies in a context, that is, the top, right, front planes and the origin point.

qFrontPlane (entityType is EntityType) returns Query

A query for the front plane.

Parameter	Type	Additional Info
`entityType`	`EntityType`	Specify type `FACE` or `BODY`.

qRightPlane (entityType is EntityType) returns Query

A query for the right plane.

Parameter	Type	Additional Info
`entityType`	`EntityType`	Specify type `FACE` or `BODY`.

qTopPlane (entityType is EntityType) returns Query

A query for the top plane.

Parameter	Type	Additional Info
`entityType`	`EntityType`	Specify type `FACE` or `BODY`.

qOrigin (entityType is EntityType) returns Query

A query for the origin point.

Parameter	Type	Additional Info
`entityType`	`EntityType`	Specify type `VERTEX` or `BODY`.

derive

derive (context is Context, id is Id, buildFunction is function, options is map) returns map

Merges context returned by buildFunction(options.configuration) into context.

Parameter	Type	Additional Info
`options`	`map`
`parts`	`Query`	Queries resolving to bodies in base context to be preserved.
`configuration`	`map`	The configuration of the part studio.
`clearSMDataFromAll`	`boolean`	Optional Default is `true`. If set to `false`, for every part in options.parts belonging to an active sheet metal model all 3d parts and flats of that sheet metal model survive and remain active.
`filterOutNonModifiable`	`boolean`	Optional Default is `true`.
`propagateMergeStatus`	`boolean`	Optional Default is `true`.
`noPartsError`	`ErrorStringEnum`	Optional Error to be reported if options.parts resolves to empty array. If field is not specified ErrorStringEnum.IMPORT_DERIVED_NO_PARTS is used.
`noPartsErrorParams`	`array`	Optional
`queriesToTrack`	`map`	Optional Map whose keys are `Query`s which resolve in the original derived context (that is, the context resulting from `buildFunction`). If set, the output field `trackingResults` will contain values which resolve to each query's equivalent entities in the current `context`.
`mateConnectors`	`array`	Optional Array of queries for mate connectors, to evaluate in the new context. If set, the output field `mateConnectors` will be a map from each query to its resulting transform.
`mateConnectorIds`	`array`	Optional Array of creating feature ids for mate connectors.
`mateConnectorFeatureIndices`	`array`	Optional Array of indices into mate connectors created by feature.
`loadedContext`	`Context`	Optional Preloaded context, if available, of the reference.

Return	Type	Description
	`map`
`mateConnectors`	`map`	Map from mate connector query to `Transform` to that mate connector
`trackingResults`	`map`	Map from `Query` keys of `queriesToTrack` to each query's value in the new context (given as an array of transient queries)

edgeBlendCommon

addFilletControlManipulator (context is Context, id is Id, definition is map, manipulatorEntity is Query)

Create a linear manipulator for radius or width parameter

onFilletControlManipulatorChange (context is Context, definition is map, newManipulators is map, manipulatorEntity is Query, widthFieldName is string) returns map

fillet manipulator change function

error

regenError (customMessage is string) returns map

regenError functions are used to construct maps for throwing to signal feature regeneration errors. Can either take a string for a custom message or an ErrorStringEnum for a built-in message. Custom messages are limited to ASCII characters. Messages longer than 200 characters will not be displayed fully.

EXAMPLE

throw regenError("Failed to attach widget: Boolean union failed")

EXAMPLE

throw regenError("Wall is too thin for this feature", ["wallWidth"]);

EXAMPLE

throw regenError(ErrorStringEnum.POINTS_COINCIDENT, ["points"]);

regenError (customMessage is string, faultyParameters is array) returns map

Parameter	Type	Additional Info
`faultyParameters`	`array`	An array of strings that correspond to keys in the feature definition map. Throwing a regenError with faultyParameters will highlight them in red inside the feature dialog.

regenError (customMessage is string, entities is Query) returns map

Parameter	Type	Additional Info
`entities`	`Query`	A query for entities to highlight in the Part Studio. Multiple queries can be combined and highlighted using the `qUnion` function. The entities are only highlighted when the feature dialog is open.

regenError (customMessage is string, faultyParameters is array, entities is Query) returns map

Parameter	Type	Additional Info
`faultyParameters`	`array`	An array of strings that correspond to keys in the feature definition map. Throwing a `regenError` with `faultyParameters` will highlight them in red inside the feature dialog.
`entities`	`Query`	A query for entities to highlight in the Part Studio. Multiple queries can be combined and highlighted using the `qUnion` function. The entities are only highlighted when the feature dialog is open.

regenError (message is ErrorStringEnum) returns map

The following overloads take an ErrorStringEnum rather than a custom message, and are using for all errors withing the Onshape Standard Library. The enum values correspond to messages which can be translated into multiple languages.

regenError (message is ErrorStringEnum, faultyParameters is array) returns map

Parameter	Type	Additional Info
`faultyParameters`	`array`	An array of strings that correspond to keys in the feature definition map. Throwing a `regenError` with `faultyParameters` will highlight them in red inside the feature dialog.

regenError (message is ErrorStringEnum, entities is Query) returns map

Parameter	Type	Additional Info
`entities`	`Query`	A query for entities to highlight in the Part Studio. Multiple queries can be combined and highlighted using the `qUnion` function. The entities are only highlighted when the feature dialog is open.

regenError (message is ErrorStringEnum, faultyParameters is array, entities is Query) returns map

Parameter	Type	Additional Info
`faultyParameters`	`array`	An array of strings that correspond to keys in the feature definition map. Throwing a `regenError` with `faultyParameters` will highlight them in red inside the feature dialog.
`entities`	`Query`	A query for entities to highlight in the Part Studio. Multiple queries can be combined and highlighted using the `qUnion` function. The entities are only highlighted when the feature dialog is open.

regenError (message is ErrorStringEnum, regenErrorOptions is map) returns map

Parameter	Type	Additional Info
`regenErrorOptions`	`map`
`faultyParameters`		An array of strings that correspond to keys in the feature definition map. Throwing a `regenError` with `faultyParameters` will highlight them in red inside the feature dialog.
`entities`		A query for entities to highlight in the Part Studio. Multiple queries can be combined and highlighted using the `qUnion` function. The entities are only highlighted when the feature dialog is open.

regenError (message is string, regenErrorOptions is map) returns map

Parameter	Type	Additional Info
`regenErrorOptions`	`map`
`faultyParameters`		An array of strings that correspond to keys in the feature definition map. Throwing a `regenError` with `faultyParameters` will highlight them in red inside the feature dialog.
`entities`		A query for entities to highlight in the Part Studio. Multiple queries can be combined and highlighted using the `qUnion` function. The entities are only highlighted when the feature dialog is open.

reportFeatureWarning (context is Context, id is Id, message is ErrorStringEnum) returns boolean

Attaches a warning-level status to the given feature id.

reportFeatureWarning (context is Context, id is Id, customMessage is string) returns boolean

Attaches a custom warning-level status to the given feature id. Will display a notification to the user containing the specified message.

reportFeatureWarning (context is Context, id is Id, message is ErrorStringEnum, associatedParameters is array) returns boolean

Attaches custom warning-level status to the given feature id. Will display a notification to the user containing the specified message.

reportFeatureInfo (context is Context, id is Id, message is ErrorStringEnum) returns boolean

Attaches an info-level status to the given feature id. Will display a notification to the user containing the specified message.

reportFeatureInfo (context is Context, id is Id, message is ErrorStringEnum, associatedParameters is array) returns boolean

Attaches an info-level status to the given feature id. Will display a notification to the user containing the specified message.

reportFeatureInfo (context is Context, id is Id, customMessage is string) returns boolean

Attaches a custom info-level status to the given feature id.

processSubfeatureStatus (context is Context, id is Id, options is map) returns boolean

Propagate the status of a subfeature to a feature.

Parameter	Type	Additional Info
`options`	`map`
`subfeatureId`	`Id`	The Id of the subfeature.
`overrideStatus`	`ErrorStringEnum`	Optional A status enum to use instead of the subfeature status enum if the subfeature has an info, warning, or error status.
`featureParameterMap`	`map`	Optional A mapping of the field names from subfeature to feature.
`featureParameterMappingFunction`	`function`	Optional A function to map field names from subfeature to feature.
`propagateErrorDisplay`	`boolean`	Optional Use subfeature error display when present. Default is false.
`additionalErrorEntities`	`Query`	Optional Additional error entities to display if the subfeature has an info, warning, or error status.

getFeatureStatus (context is Context, id is Id) returns FeatureStatus

Return the status of a feature as a FeatureStatus

reportFeatureStatus (context is Context, id is Id, status is FeatureStatus) returns boolean

Report the status of a feature

clearFeatureStatus (context is Context, id is Id, definition is map) returns boolean

Clear the status of a feature to StatusType.OK *

Parameter Type Additional Info

definition map

withDisplayData

boolean

Optional

Clear status display data attached to feature. Default true.

getFeatureError (context is Context, id is Id)

Returns the error (as a string or an ErrorStringEnum) associated with the given feature id or undefined if none.

getFeatureWarning (context is Context, id is Id)

Returns the warning (as a string or an ErrorStringEnum) associated with the given feature id or undefined if none.

getFeatureInfo (context is Context, id is Id)

Returns the info status (as a string or an ErrorStringEnum) associated with the given feature id or undefined if none.

setErrorEntities (context is Context, id is Id, definition is map)

Causes the given entities to be shown in red. This display is not rolled back even if the feature fails and the entities themselves are rolled back.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	The entities to display.

featureHasError (context is Context, id is Id) returns boolean

Return type	Description
`boolean`	`true` if the feature with the given id has an associated regeneration error.

featureHasNonTrivialStatus (context is Context, id is Id) returns boolean

Return type	Description
`boolean`	`true` if the feature with the given id has an associated status different from OK.

faultyArrayParameterId (arrayParameter is string, itemIndex is number, innerParameter is string) returns string

Return type	Description
`string`	A string identifier for marking an error on an array parameter when using the `faultyParameters` argument in any of the error reporting functions in `error.fs`.

FeatureStatus type

The status of a feature

Value	Type	Description
`FeatureStatus`	`map`
`statusType`	`StatusType`
`faultyParameters`	`array`
`statusEnum`	`ErrorStringEnum`
`statusMsg`	`string`

canBeFeatureStatus (value) predicate

The faultyParameters cannot exist when the statusType is StatusType.OK. The statusEnum must be ErrorStringEnum.CUSTOM_ERROR if the statusMsg exists.

verify (condition is boolean, error)

If the condition check fails, this function throws the error.

Parameter	Type	Additional Info
`condition`	`boolean`	The condition to test.
`error`		The error to throw if `condition` is `false`, where `error` is of type `ErrorStringEnum` or `string`.

verify (condition is boolean, error, regenErrorOptions is map)

If the condition check fails, this function throws the error.

Parameter	Type	Additional Info
`condition`	`boolean`	The condition to test.
`error`		The error to throw if `condition` is `false`, where `error` is of type `ErrorStringEnum` or `string`.
`regenErrorOptions`	`map`	The key-value pairs to pass to the thrown `regenError`, e.g. `entities` or `faultyParameters`.

extrudeCommon

SMExtrudeBoundingType enum

Bounding type used with SMProcessType.EXTRUDE

Value	Description
`BLIND`
`UP_TO_NEXT`
`UP_TO_SURFACE`
`UP_TO_BODY`
`UP_TO_VERTEX`

feature

defineFeature (feature is function, defaults is map) returns function

This function takes a regeneration function and wraps it to create a feature. It is exactly like the one-argument version of defineFeature but the additional argument enables setting default values for feature parameters when they are not passed in.

Parameter Type Additional Info

defaults

map

A map of default parameter values for when this feature is called in FeatureScript.

This does NOT control the user-visible default value when creating this feature. To change the user-visible default for booleans, enums, and strings, use the "Default" annotation. To change the user-visible default for a length, angle, or number, see the valueBounds module.

EXAMPLE

{} will not modify the definition.

EXAMPLE

{ "shouldFillet" : false } will set the parameter "shouldFillet" to false if the feature is called from FeatureScript without the "shouldFillet" parameter.

defineFeature (feature is function) returns function

This function takes a regeneration function and wraps it to create a feature. The wrapper handles certain argument recording for the UI and error handling. A typical usage is something like:

annotation { "Feature Type Name" : "Widget" } // This annotation is required for Onshape to recognize widget as a feature.
export const widget = defineFeature(function(context is Context, id is Id, definition is map)
    precondition
    {
        ... // Specify the parameters that this feature takes
    }
    {
        ... // Specify what the feature does when regenerating
    });

For more information on writing features, see Specifying feature UI in the language guide.

Parameter	Type	Additional Info
`feature`	`function`	A function that takes a `context`, an `id`, and a `definition` and regenerates the feature.

startFeature (context is Context, id is Id)

callSubfeatureAndProcessStatus (topLevelId is Id, fn is function, context is Context, subfeatureId is Id, definition is map)

This function can be used to call a subfeature or sub-operation (such as extrude or opExtrude, respectively). It will properly handle any statuses as if they came from the top level feature. That is, reported INFO will display as a blue message bubble, WARNING will turn the feature orange with a warning tooltip on hover, and ERROR will throw an error after status handling (aborting feature execution if it is not caught). Any error entities that the subfeature emits will also be displayed.

EXAMPLE

callSubfeatureAndProcessStatus(id, booleanBodies, context, id + "boolean", booleanDefinition); (where id is the top-level feature id passed into the feature) will call booleanBodies(context, id + "boolean", booleanDefinition), propagate its status onto the current feature, and show any error entities coming from the boolean.

Internally, calls the supplied function, and attaches any status it produces to the topLevelId using processSubfeatureStatus. If calling the function produces an error, the error is re-thrown. If the function produces a return value, that value is returned.

callSubfeatureAndProcessStatus (topLevelId is Id, fn is function, context is Context, subfeatureId is Id, definition is map, processSubfeatureStatusOptions is map)

See callSubfeatureAndProcessStatus.

Parameter	Type	Additional Info
`processSubfeatureStatusOptions`	`map`	Passed as the `definition` argument to `processSubfeatureStatus`. Setting `subfeatureId` in this map is not required, and will be ignored in favor of the `subfeatureId` passed into this function.

forEachEntity (context is Context, id is Id, query is Query, operationToPerform is function)

Iterate through all entities provided by a query, calling the provided function once for each geometric entity resolved by the provided query.

forEachEntity behaves much like the code:

const evaluated = evaluateQuery(context, query);
for (var i = 0; i < size(evaluated); i += 1)
{
    operationToPerform(id + i, evaluated[i]);
}

However, forEachEntity has one additional benefit: The entId this function provides to operationToPerform is tied to the entity itself, not its index i. This means that downstream features made in the Part Studio will hold up better across upstream changes.

For example, imagine the following scenario: A user inserts a custom feature which places a slot on every selected line. That feature calls forEachEntity(context, lineQuery ...). The user then makes a sketch downstream which uses geometry from e.g. the third slot. Finally, the user decides some slots are unnecessary and deletes some of the lines. Since the feature used forEachEntity, the user's downstream sketch will still reference the same slots. If the feature instead used the code above, the user's sketch would break or jump around, since a different slot would suddenly become "slot 3".

Aside from that difference, the two are interchangable.

Like any expression function, be warned that the provided operationToPerform can read but can NOT modify the values of variables outside the function. It can, however, modify values inside a box.

EXAMPLE

const allParts = qAllModifiableSolidBodies();
const threshold = 0.01 * inch^3;
var deletedSizes is box = new box([]); // box containing an empty array
forEachEntity(context, id + "deleteSmallParts", allParts, function(entity is Query, id is Id)
{
    const size = evVolume(context, {
            "entities" : entity
    });
    if (size < threshold)
    {
        opDeleteBodies(context, id + "deleteBodies1", {
                "entities" : entity
        });
        deletedSizes[] = append(deletedSizes[], size);
    }
});
println(deletedSizes[]);

Parameter Type Additional Info

operationToPerform

function

EXAMPLE

function(entity is Query, id is Id)
{
    // perform operations with the entity
}

The first argument to this function is a query resolving to one single entity of the input query.

The second argument to this function is a unique id tied to the entity. By default it is named "id", which will shadow (i.e. take precedence over) the outer variable named "id". If you need access to that outer id, simply rename this argument to e.g. innerId.

setFeatureComputedParameter (context is Context, id is Id, definition is map)

Associates a FeatureScript value with a given string. This value can then be referenced in a feature name using the string. The provided value can be used in a feature name by including e.g. "#myValue" in the Feature Name Template.

Parameter Type Additional Info

definition map

name

string

EXAMPLE

myValue

value

getFullPatternTransform (context is Context) returns Transform

When in feature pattern scope returns composition of all pattern transforms pushed by setFeaturePatternInstanceData returns identity transform when out of scope

getRemainderPatternTransform (context is Context, definition is map) returns Transform

Making a feature work correctly with feature patterns is usually done with two functions: this one and transformResultIfNecessary.

Feature patterns work by first computing a sequence of transforms, one for each instance. For each transform, the pattern pushes it onto the pattern stack (using setFeaturePatternInstanceData), executes the patterned features, and then pops the transform off the stack (using unsetFeaturePatternInstanceData) before pushing the next one. The stack depth corresponds to the level of nesting of feature patterns. Feature authors are responsible for reading the pattern stack and transforming themselves accordingly.

The basic principle is that inside one feature pattern (as opposed to nested feature patterns), if any entities that the feature references come from a feature that is also being patterned, then the feature ignores the pattern transform. Otherwise, the feature uses the pattern transform in a "natural" way, applying it to an input, the output, or somewhere in between.

For example, suppose the patterned feature creates a 3D line between two arbitrary vertices. If the first vertex is also patterned, but not the second, then the result should be a bunch of lines from different instances of the first vertex to the unpatterned second vertex (this is accomplished by not applying any transform to the line). If neither vertex is patterned, the line should be transformed by the pattern transform and the result will be as expected, as if a body pattern of these lines was performed. Other features may need to apply the transform differently: for example, a sweep can transform the result of opSweep prior to the boolean, but an extrude needs to transform the profile prior to opExtrude to accommodate up-to-next correctly.

The general case is more complicated because feature patterns may be nested, and this function is designed to handle them. This function takes references, a query for everything the feature geometrically depends on (typically a qUnion of the queries in the feature definition), and computes the portion of the pattern transform that is not applied to any of the references and hence should be applied to the feature. For example, if one of the references is patterned by the current feature pattern or if there is no feature pattern, it will return the identity transform. If references evaluates to nothing, it will return the current feature pattern transform.

More precisely: Among references find topology created by pattern instance deepest in the pattern transform stack. If the transformation on the stack for that instance is S and the full transformation is F, the remainder R is such that R * S = F

A simple feature may use this function and transformResultIfNecessary as follows:

... // Feature definition boilerplate and precondition
    { // Feature body
        // Call getRemainderPatternTransform before performing any operations
        var remainingTransform = getRemainderPatternTransform(context, { "references" : definition.vertexToBuildOn });
        ... // Create a cube using definition.vertexToBuildOn as the reference location
        // Inside a feature pattern, the following will transform the cube if definition.vertexToBuildOn is not getting patterned:
        transformResultIfNecessary(context, id, remainingTransform);
        ... // Perhaps boolean the results to something in the context
    });

Parameter	Type	Additional Info
`definition`	`map`
`references`	`Query`

transformResultIfNecessary (context is Context, id is Id, transform is Transform)

Applies transformation to bodies created by operation with id if transform argument is non-trivial

isAnything (value) predicate

A predicate which always returns true. Used to create a generic feature parameter that can be any featurescript expression.

Note that to change the user-visible default value, the "Default" annotation must be a string containing a valid parameter expression. For example, to make the default value the string "My string", pass in an escaped string: annotation{ "Default": "\"My string\"" }.

lastModifyingOperationId (context is Context, query is Query) returns Id

Returns id of operation that created or last modified the first entity to which query resolves.

Throws if query resolves to nothing.

startTracking (context is Context, arg is map) returns Query

Generates a tracking query, which will evaluate to entities derived from subquery in features between startTracking and when query is evaluated. If secondarySubquery is specified, the query would evaluate to entities derived from both objects. If trackPartialDependency is set to true, query would also include entities that are not exclusively derived from subquery1. Optional field lastOperationId can be used to specify the starting operation of tracking. Use example:

// "sketch1" constructs a polygon of "line0", "line1", etc.
var extrudedFromLine0 = startTracking(context, id + "sketch1", "line0");
extrudeOp(context, id + "extrude1", {"entities" : qSketchRegion(id + "sketch1",....});
var fromLine0 = evaluateQuery(context, extrudedFromLine0);
// fromLine0 contains a face and two edges (top and bottom) corresponding to line0 in the extrude.

startTracking (context is Context, subquery is Query) returns Query

startTracking (context is Context, sketchId is Id, sketchEntityId is string) returns Query

startTrackingIdentity (context is Context, subquery is Query) returns Query

Generates a tracking query, which will evaluate to the new entities inheriting the identity of subquery evaluation result.

makeRobustQuery (context is Context, subquery is Query) returns Query

Generates query robust to identity-preserving changes

makeRobustQueriesBatched (context is Context, subquery is Query) returns array

Generates array of robust queries for each entity of the subquery

setExternalDisambiguation (context is Context, id is Id, query is Query)

Used to set external disambiguation for operations with unstable component in id. The disambiguation will be applied to results of sub-operations which otherwise don't track dependency e.g. Sketch , opPlane, opPoint

Parameter	Type	Additional Info
`id`	`Id`	ends in unstable component

verifyNonemptyQuery (context is Context, definition is map, parameterName is string, errorToReport is string) returns array

Throws a regenError and marks the specified Query parameter as faulty if the specified Query parameter is not a Query which resolves to at least one entity. This happens when the user has not made any selection into the Query parameter, or when upstream geometry has changed such that the Querys of the Query parameter no longer resolve to anything. Should be used to check all non-optional Query parameters in a feature. By convention, errorToReport should take the form "Select parameter display name." For example, a parameter declared as follows:

annotation { "Name" : "Entities to use", "Filter" : EntityType.FACE }
definition.entitiesToUse is Query;

should verify that the input is nonempty in the following way:

EXAMPLE

verifyNonemptyQuery(context, definition, "entitiesToUse", "Select entities to use.")

Return type	Description
`array`	An array representing the result of evaluating the `Query` parameter with `evaluateQuery`

verifyNonemptyArray (context is Context, definition is map, parameterName is string, errorToReport is string)

Throws a regenError and marks the specified array parameter as faulty if the specified array parameter does not have any entries. A parameter declared as follows:

annotation { "Name" : "Array items", "Item name" : "Array item" }
definition.arrayItems is array;
for (var arrayItem in definition.arrayItems)
{
   ...
}

could verify that the input is nonempty in the following way:

EXAMPLE

verifyNonemptyArray(context, definition, "arrayItems", "Add an array item.")

verifyNoMesh (context is Context, definition is map, parameterName is string)

Verifies that the definition[parameterName] Query does not contain mesh or mixed entities. Throws a regenError if definition[parameterName] references mesh topologies.

verifyNoMeshInBody (context is Context, definition is map, parameterName is string)

Verifies no body containing the specified query contains any mesh.

Parameter	Type	Additional Info
`context`	`Context`	The application context.
`definition`	`map`	The feature definition.
`parameterName`	`string`	The key of `definition` that will be accessed to find the query.

adjustAngle (context is Context, angle is ValueWithUnits) returns ValueWithUnits

Adjust angle out of bounds angles to lie in [0 to 2pi] if the feature is new, do a range check otherwise.

isButton (value) predicate

True if the value is undefined and creates a button parameter.

featureList

Support functions for feature lists (as used for featurePattern)

FeatureList type

Parameter type for inputting a list of features, stored as a map from feature Id to feature function. For an example, see the circularPattern module.

canBeFeatureList (value) predicate

Typecheck for FeatureList

featureList (features is map) returns FeatureList

Takes a map from id to lambda to return it as type FeatureList

valuesSortedById (context is Context, idToValue is map) returns array

Takes a context and a map whose keys are subfeature ids from that context. Returns the values from that map sorted in the order that the subfeatures were started.

flatOperationType

FlatOperationType enum

Types of flat operations supported by SMFlatOp

Value	Description
`ADD`
`REMOVE`

formedUtils

setFormAttribute (context is Context, bodies is Query, attribute is string)

Attach the given FormAttribute to the bodies.

qBodiesWithFormAttribute (attribute is string)

Query for all bodies marked with a FormAttribute and value exactly equal to attribute

See also

setFormAttribute

qBodiesWithFormAttribute (queryToFilter is Query, attribute is string) returns Query

Query for all bodies in queryToFilter marked with a FormAttribute and value exactly equal to attribute

See also

setFormAttribute

qBodiesWithFormAttributes (queryToFilter is Query, attributes is array) returns Query

Query for all bodies in queryToFilter marked with a FormAttribute and value exactly equal to one of the attributes

See also

setFormAttribute

frameAttributes

FrameTopologyType enum

The possible types of a FrameTopologyAttribute.

Value	Description
`SWEPT_FACE`	The side faces of a frame, swept from the edges of the profile
`SWEPT_EDGE`	The side edges of a frame, swept from the vertices of the profile
`CAP_FACE`	The start and end cap faces of a frame

FrameProfileAttribute type

An attribute attached to the frame profile and the constructed frame body which defines the default cutlist associated with the frame.

frameProfileAttribute (value is map) returns FrameProfileAttribute

Construct a FrameProfileAttribute.

getFrameProfileAttributes (context is Context, frames is Query)

Get all FrameProfileAttributes attached to the frames.

getFrameProfileAttribute (context is Context, frame is Query)

Get the FrameProfileAttribute attached to the frame. Throw if a single attribute is not found.

setFrameProfileAttribute (context is Context, frame is Query, attribute is FrameProfileAttribute)

Attach the given FrameProfileAttribute to the frame.

FrameTopologyAttribute type

An attribute assigned to certain faces and edges of the frames to aid in tracking the frame as it changes over the series of frame-altering features.

frameTopologyAttributeForSwept (topologyType is FrameTopologyType) returns FrameTopologyAttribute

Construct a FrameTopologyAttribute for SWEPT_* types.

See also

frameTopologyAttributeForCapFace

frameTopologyAttributeForCapFace (isStartFace is boolean, isFrameTerminus is boolean, isCompositeTerminus is boolean) returns FrameTopologyAttribute

Construct a FrameTopologyAttribute for CAP_FACE.

See also

frameTopologyAttributeForSwept

getFrameTopologyAttributes (context is Context, faces is Query)

Get all FrameTopologyAttributes attached to the faces.

getFrameTopologyAttribute (context is Context, face is Query)

Get the FrameTopologyAttribute attached to the face. Throw if a single attribute is not found.

setFrameTopologyAttribute (context is Context, entities is Query, attribute is FrameTopologyAttribute)

Attach the given FrameTopologyAttribute to each of the entities.

CutlistAttribute type

An attribute attached to the composite created by the Cutlist feature which contains the cutlist table for that composite.

cutlistAttribute (featureId is Id, table is Table) returns CutlistAttribute

Construct a CutlistAttribute.

getCutlistAttributes (context is Context, composites is Query)

Get all CutlistAttributes attached to the composites.

getCutlistAttribute (context is Context, composite is Query)

Get the getCutlistAttribute attached to the composite. Throw if a single attribute is not found.

setCutlistAttribute (context is Context, composite is Query, attribute is CutlistAttribute)

Attach the given CutlistAttribute to the composite.

setCustomFrameAlignmentPointAttribute (context is Context, pointsQuery is Query)

Sets an attribute on the sketch entity point queries for later discovery and use during frame creation.

getCustomFrameAlignmentPoints (context is Context, profileId is Id) returns Query

Finds the sketch points in the profileId sketch with the custom alignment point attribute.

holeUtils

HoleStyle enum

Defines whether each hole should have a countersink, a counterbore, or neither.

Value	Description
`SIMPLE`
`C_BORE`
`C_SINK`

HoleProfile type

Describes a single profile for a HoleDefinition.

See also

holeProfile for standard circular profiles.

holeProfileBeforeReference for a circular profile meant to be used as the first profile of the hole.

matchedHoleProfile for a profile that geometrically matches the HolePositionReference.

Value	Type	Description
`HoleProfile`	`map`
`positionReference`	`HolePositionReference`	The reference along the hole axis to which this profile is relative.
`beforeReference`	`boolean`	Optional Whether the `position` of the profile should reference the start or end of the given `positionReference`. See `holeProfileBeforeReference` for more detail. Default is `false` if not provided. Only considered when `profileType` is `POSITIONED`, ignored otherwise.
`profileType`	`HoleProfileType`	How the profile should be constructed in relation to the given `positionReference`
`position`	`ValueWithUnits`	Required if `profileType` is `POSITIONED` The position of the profile along the hole axis, relative to the given `positionReference`.
`radius`	`ValueWithUnits`	The radius of the profile. Can be `0` to specify that the profile forms a point.
`targetMustDifferFromPrevious`	`boolean`	Optional If `true`, instructs `opHole` to skip the construction of any holes in which the target referenced by this profile's `positionReference` is not different than the target reference by the previous profile's `positionReference`. Cannot be set to `true` on the first profile or any profile that does not have a different `positionReference` than the previous profile. Default is `false`.
`notApplicableForFirstTarget`	`boolean`	Optional If `true`, instructs `opHole` to skip the profiles in which the target referenced by this profile's `positionReference` is not different than the target reference by the GBTHolePositionReference::TARGET_START. Cannot be set to `true` on the first profile Default is `false`.
`name`	`string`	Optional A name for to assign to the edge created by `opHole` which corresponds to this profile. Supplying a `name` allows for the querying of profile edges by name when using `qOpHoleProfile`.

canBeHoleProfile (value) predicate

Typecheck for HoleProfile

holeProfile (positionReference is HolePositionReference, position is ValueWithUnits, radius is ValueWithUnits, optionalParameters is map) returns HoleProfile

Returns a new circular HoleProfile at a given position in relation to the end of the range of the positionReference. See HolePositionReference for further detail about the range of the positionReference.

Parameter	Type	Additional Info
`optionalParameters`	`map`
`targetMustDifferFromPrevious`	`boolean`	Optional See `HoleProfile`.
`notApplicableForFirstTarget`	`boolean`	Optional See `HoleProfile`.
`name`	`string`	Optional See `HoleProfile`.

holeProfile (positionReference is HolePositionReference, position is ValueWithUnits, radius is ValueWithUnits) returns HoleProfile

holeProfileBeforeReference (positionReference is HolePositionReference, position is ValueWithUnits, radius is ValueWithUnits, optionalParameters is map) returns HoleProfile

Returns a new circular HoleProfile at a given position in relation to the beginning of the range of the positionReference. See HolePositionReference for further detail about the range of the positionReference. This type of profile is useful as the first profile of a hole, such that if the hole cylinder intersects the first target at a slanted or otherwise irregular face, the first profile is backed up enough such that when the hole tool is subtracted from the target, there is no undesirable overhang left behind.

Parameter	Type	Additional Info
`optionalParameters`	`map`
`targetMustDifferFromPrevious`	`boolean`	Optional See `HoleProfile`.
`notApplicableForFirstTarget`	`boolean`	Optional See `HoleProfile`.
`name`	`string`	Optional See `HoleProfile`.

holeProfileBeforeReference (positionReference is HolePositionReference, position is ValueWithUnits, radius is ValueWithUnits) returns HoleProfile

matchedHoleProfile (positionReference is HolePositionReference, radius is ValueWithUnits, optionalParameters is map) returns HoleProfile

Returns a new HoleProfile that is geometrically matched to the positionReference. This is useful for configurations like blind-in-last, where a transition from one radius to another must be made that matches the shape of the position reference, to avoid the hole tool intersecting incorrectly with the part(s) in question. To form a valid HoleDefinition, MATCHED profiles must come in pairs of different radii.

Parameter	Type	Additional Info
`optionalParameters`	`map`
`targetMustDifferFromPrevious`	`boolean`	Optional See `HoleProfile`.
`notApplicableForFirstTarget`	`boolean`	Optional See `HoleProfile`.
`name`	`string`	Optional See `HoleProfile`.

matchedHoleProfile (positionReference is HolePositionReference, radius is ValueWithUnits) returns HoleProfile

HoleDefinition type

Describes the shape of a hole using a series of HoleProfiles.

See also

opHole

Value Type Description

HoleDefinition map

profiles

array

An array of HoleProfiles which define the shape of the hole. The profiles are interpreted in order, from the top to the bottom of the hole. The final profile must have a radius of 0. Each profile must specify a unique name, or all of the profiles must leave their name field undefined. If two or more adjacent profiles in the list end up being identical (in the same position with the same radius) when their final placement is determined in opHole, the identical profiles will be collapsed into a single profile, which uses the name of the first of the identical profiles.

faceNames

array

Optional

A list of names to assign to the faces created by opHole. Should be the same length as the profiles array, where faceNames[i] is the name of the face created between profiles i - 1 and i, and faceNames[0] is the name of the top cap face (the face before profile 0). If any profiles are collapsed, the names of the faces between the collapsed profiles are skipped. Supplying faceNames allows for the querying of faces by name when using qOpHoleFace.

canBeHoleDefinition (value) predicate

Typecheck for HoleDefinition

holeDefinition (profiles is array, optionalParameters is map) returns HoleDefinition

Returns a new HoleDefinition.

Parameter Type Additional Info

optionalParameters map

faceNames

string

Optional

See HoleDefinition.

holeDefinition (profiles is array) returns HoleDefinition

instantiator

The instantiator makes it easy to efficiently bring in (possibly configured) bodies from other Part Studios and place them at specific positions and orientations. The usage pattern is generally as follows:

firstPartStudio::import(...);
secondPartStudio::import(...);
// later, in a feature
const instantiator = newInstantiator(id + "myId");
var firstQuery = addInstance(instantiator, firstPartStudio::build, {
                                 "configuration" : { "configurationInput" : configurationValue },
                                 "transform"     : transform(vector(1, 2, 3) * inch)
                             });
var secondQuery = addInstance(instantiator, secondPartStudio::build, {
                                  "configuration" : secondConfiguration,
                                  "transform"     : someOtherTransform,
                                  "mateConnector" : queryForMateConnectorInSecondPartStudio // Specifies the origin
                              });
// repeat the above as necessary
instantiate(context, instantiator); // This call actually brings in the bodies
// Now firstQuery and secondQuery will resolve to the instantiated geometry

Internally, the instantiator groups all added instances by Part Studio and configuration. The final call to instantiate() is optimized so that any duplicates of the same Part Studio and the same configuration are patterned instead of re-derived, resulting in better performance and scalability for features instantiating the same bodies multiple times.

Instantiator type

Stores the data associated with using instantiator functionality.

canBeInstantiator (value) predicate

Typecheck for Instantiator

newInstantiator (id is Id) returns Instantiator

Creates a new instantiator with the specified id and default options.

newInstantiator (id is Id, options is map) returns Instantiator

Creates a new instantiator.

Parameter	Type	Additional Info
`id`	`Id`	The root id for all instances that will be created by this instantiator. Multiple instantiators can be used simultaneously, as long as they have different ids.
`options`	`map`	Optional
`partQuery`	`Query`	Optional The query for all bodies to be brought in from the part studios. Default is all bodies except sketches.
`tolerances`	`map`	Optional The tolerances for variable configuration inputs. Default is 1e-8 meters for lengths, 1e-11 radians for angles, and 0 for numbers. The default tolerances for lengths, angles, and numbers can be specified using the `(LENGTH_UNITS)`, `(ANGLE_UNITS)`, and `(unitless)` keys, respectively. The tolerance for a specific configuration input can be specified using that input name as the key. EXAMPLE `{ (LENGTH_UNITS) : 1e-4 * meter, (unitless) : 1e-8, "count" : 0 }` causes length configuration variables that differ by less than 1e-4 meters to be considered identical, as well as numberical configuration variables that differ by less than 1e-8, except that configuration variables named "count" are compared exactly.

addInstance (instantiator is Instantiator, build is function, definition is map) returns Query

Adds an instance to the instantiator (does not actually create it in a context) with the given build function. The definition can specify the configuration, the transform, and how the result is identified.

Parameter	Type	Additional Info
`definition`	`map`
`configuration`	`map`	Optional The configuration of the part studio.
`partQuery`	`query`	Optional A query which evaluates to bodies in new context, to be instantiated for this instance. If absent `partQuery` of instantiator is used. When present, overrides `partQuery` of the instantiator.
`transform`	`Transform`	Optional The transform to be applied to the geometry.
`mateConnector`	`Query`	Optional A query for all mate connectors from the part studio being instantiated, specifying its coordinate system.
`mateConnectorId`	`Id`	Optional Creating feature Id of the mate connector used for transformation.
`mateConnectorIndex`	`number`	Optional Index into the creating feature of the mate connector used for transformation.
`name`	`string`	Optional The id component for this instance. Must be unique per instantiator. If it is not specified, one is automatically generated based on order. If it is specified, the query returned is `qCreatedBy(id + name, EntityType.BODY)`, where `id` is the id that was passed into `newInstantiator`
`identity`	`Query`	Optional If provided, specifies an entity whose identity controls the identity of the instance, so that queries for the instance can be robust. For example, if creating instances based on a layout sketch, one instance per line segment, the identity should be a query for the corresponding line segment.
`loadedContext`	`Context`	If a preloaded context is provided, use this context

Return type	Description
`Query`	a query that will resolve to the bodies instantiated once `instantiate` is run.

addInstance (instantiator is Instantiator, partStudio is PartStudioData, definition is map) returns Query

Add an instance with the buildFunction, partQuery, and configuration of a PartStudioData value.

Parameter	Type	Additional Info
`definition`	`map`
`transform`	`Transform`	Optional The transform to be applied to the geometry.
`mateConnector`	`Query`	Optional A query for a mate connector in the part studio being instantiated, specifying its coordinate system.
`mateConnectorId`	`Id`	Optional Creating feature Id of the mate connector used for transformation.
`mateConnectorIndex`	`number`	Optional Index into the creating feature of the mate connector used for transformation.
`configurationOverride`	`map`	Optional If set, the values will be merged with the configuration set in `partStudio`, overriding any configuration inputs with matching keys.
`name`	`string`	Optional The id component for this instance. Must be unique per instantiator. If it is not specified, one is automatically generated based on order. If it is specified, the query returned is `qCreatedBy(id + name, EntityType.BODY)`, where `id` is the id that was passed into `newInstantiator`
`identity`	`Query`	Optional If provided, specifies an entity whose identity controls the identity of the instance, so that queries for the instance can be robust. For example, if creating instances based on a layout sketch, one instance per line segment, the identity should be a query for the corresponding line segment.
`loadedContext`	`Context`	If a preloaded context is provided use this context

Return type	Description
`Query`	a query that will resolve to the bodies instantiated once `instantiate` is run.

addInstance (instantiator is Instantiator, partStudio is PartStudioData) returns Query

Add an instance with the buildFunction, partQuery, and configuration of a PartStudioData value.

Return type	Description
`Query`	a query that will resolve to the bodies instantiated once `instantiate` is run.

instantiate (context is Context, instantiator is Instantiator)

Create the instances (in the provided context) that were added to the instantiator

libraryValidation

LibraryValidationProblems type

A container for a list of distinct problems found when validating a part studio for use in a library

manipulator

A manipulator is an alternative, graphical UI for controlling a feature's definition. For example, in Onshape's extrude feature, the arrow which appears at the end of a blind extrusion is a manipulator controlling the depth parameter. A manipulator can be one of a few ManipulatorTypes, which are generally draggable arrows designed to control different degrees of freedom.

The manipulator is added inside the feature function, and will be rendered whenever that feature is being edited. Changes to a manipulator will be processed by a "Manipulator Change Function" associated with the feature.

A small example using a manipulator to control the depth and direction of an opExtrude is below:

annotation { "Feature Type Name" : "Fake extrude",
        "Manipulator Change Function" : "fakeExtrudeManipulatorChange" }
export const fakeExtrude = defineFeature(function(context is Context, id is Id, definition is map)
    precondition
    {
        annotation { "Name" : "Faces to extrude", "Filter" : EntityType.FACE }
        definition.faces is Query;
        annotation { "Name" : "My Length" }
        isLength(definition.depth, LENGTH_BOUNDS);
        annotation { "Name" : "Opposite direction", "UIHint" : UIHint.OPPOSITE_DIRECTION }
        definition.shouldFlip is boolean;
    }
    {
        var extrudePlane is Plane = evFaceTangentPlane(context, {
                "face" : definition.faces,
                "parameter" : vector(0.5, 0.5)
        });
        var extrudeManipulator is Manipulator = linearManipulator({
                "base" : extrudePlane.origin,
                "direction" : extrudePlane.normal,
                "offset" : definition.shouldFlip ? definition.depth : -definition.depth,
                "primaryParameterId" : "depth"
        });
        addManipulators(context, id, {
                "myManipulator" : extrudeManipulator
        });
        opExtrude(context, id + "extrude1", {
                "entities" : definition.faces,
                "direction" : definition.shouldFlip ? extrudePlane.normal : -extrudePlane.normal,
                "endBound" : BoundingType.BLIND,
                "endDepth" : definition.depth
        });
    }, {});
export function fakeExtrudeManipulatorChange(context is Context, definition is map, newManipulators is map) returns map
{
    var newDepth is ValueWithUnits = newManipulators["myManipulator"].offset;
    definition.depth = abs(newDepth);
    definition.shouldFlip = newDepth > 0;
    return definition;
}

The manipulator change function is responsible for changing the definition such that the feature will regenerate correctly. It may change the definition in any way, and need not be restricted to the pattern of one manipulator changing one parameter.

The feature function is only aware of the definition passed in; it makes no distinction about whether the definition was produced from a manipulator change, or by a change in the feature dialog, or by another custom feature.

Manipulator type

A Manipulator is a type which can be passed into addManipulators, containing the necessary information to position the manipulator in the context. Altered copies of these manipulators are passed into a manipulator change function as newManipulators.

Can be constructed with triadManipulator, linearManipulator, and other functions below.

canBeManipulator (value) predicate

Typecheck for Manipulator

triadManipulator (definition is map) returns Manipulator

Create a manipulator represented by a triad of perpendicular arrows, aligned with the world axes, which specify a 3D position. See transformCopy for an example.

Parameter	Type	Additional Info
`definition`	`map`
`base`		The position of the manipulator when the offset is `0`.
`offset`		The 3D position of the triad, relative to the `base`.
`sources`		Optional For Onshape internal use.

fullTriadManipulator (definition is map) returns Manipulator

Create a manipulator represented by a triad of perpendicular arrows, planes, angular position handles, which specify 3D transform.

Parameter	Type	Additional Info
`definition`	`map`
`base`		The coordinate system the manipulator is aligned with when `transform` is the identity transform. Default is WORLD_COORD_SYSTEM.
`transform`		The 3D transform of the triad, relative to the `base` coordinate system.

triadManipulator (base is Vector, offset is Vector, sources) returns Manipulator

Deprecated: Use triadManipulator(map)

linearManipulator (definition is map) returns Manipulator

Create a manipulator represented by a single arrow which can move along a single axis. See extrude for an example.

Parameter	Type	Additional Info
`definition`	`map`
`base`		The position of the manipulator when the offset is `0`.
`direction`		A 3D unit vector pointing on the axis on which the manipulator can be dragged.
`offset`		The positive or negative distance along `direction` from the base to the manipulator.
`sources`		Optional For Onshape internal use.
`minValue`	`ValueWithUnits`	Optional The minimum offset allowed.
`maxValue`	`ValueWithUnits`	Optional The maximum offset allowed.
`style`	`ManipulatorStyleEnum`	Optional
`primaryParameterId`	`string`	Optional The id of the `definition` field which is being manipulated. When set, the feature dialog focus will be shifted to the parameter in question when the manipulator is manipulated.

linearManipulator (base is Vector, direction is Vector, offset is ValueWithUnits, sources, style is ManipulatorStyleEnum) returns Manipulator

Deprecated: Use linearManipulator(map)

linearManipulator (base is Vector, direction is Vector, offset is ValueWithUnits, sources) returns Manipulator

Deprecated: Use linearManipulator(map)

linearManipulator (base is Vector, direction is Vector, offset is ValueWithUnits) returns Manipulator

Deprecated: Use linearManipulator(map)

angularManipulator (definition is map) returns Manipulator

Create a manipulator represented by a curved arrow which can move along a circumference to specify an angle, with the start and end of the rotation angle delimited by radial lines. See revolve for an example.

Parameter	Type	Additional Info
`definition`	`map`
`axisOrigin`	`Vector`	The origin of the axis to rotate around. EXAMPLE `project(axis, rotationOrigin)`
`axisDirection`	`Vector`	The direction of the axis to rotate around. EXAMPLE `axis.direction`
`rotationOrigin`	`Vector`	Point at the tip of the revolve manipulator.
`angle`	`ValueWithUnits`	Current angle value of the manipulator.
`sources`		Optional For Onshape internal use.
`minValue`	`ValueWithUnits`	Optional The minimum angle allowed.
`maxValue`	`ValueWithUnits`	Optional The maximum angle allowed.
`style`	`ManipulatorStyleEnum`	Optional
`primaryParameterId`	`string`	Optional The id of the `definition` field which is being manipulated. When set, the feature dialog focus will be shifted to the parameter in question when the manipulator is manipulated.
`disableMinimumOffset`	`boolean`	Optional Removes the minimum offset between the arrow and `axisOrigin`.

pointsManipulator (definition is map) returns Manipulator

A set of points which can be selected one at a time.

Parameter	Type	Additional Info
`definition`	`map`
`points`	`array`	Array of 3d locations for points
`index`	`number`	The index of the currently selected point

togglePointsManipulator (definition is map) returns Manipulator

A series of points which can each be selected individually.

Parameter	Type	Additional Info
`definition`	`map`
`points`	`array`	Array of 3d locations for points
`selectedIndices`	`array`	The indices of the currently selected points
`suppressedIndices`	`array`	The indices of any non-selectable points

flipManipulator (definition is map) returns Manipulator

Create a manipulator represented by a single arrow which flips direction when clicked.

Parameter	Type	Additional Info
`definition`	`map`
`base`	`Vector`	A 3d point at the manipulator's origin EXAMPLE `vector(0, 0, 0) * meter`
`direction`	`Vector`	A 3d vector pointing in the unflipped direction EXAMPLE `vector(0, 0, 1)` points manipulator along the z axis
`flipped`	`boolean`	EXAMPLE `false` points the manipulator along +direction EXAMPLE `true` points the manipulator along -direction, or otherDirection if defined
`sources`		Optional For Onshape internal use.
`style`	`ManipulatorStyleEnum`	Optional
`otherDirection`	`Vector`	Optional A 3d vector for the flipped direction

flipManipulator (base is Vector, direction is Vector, flipped is boolean, sources, style is ManipulatorStyleEnum) returns Manipulator

Deprecated: Use flipManipulator(map)

flipManipulator (base is Vector, direction is Vector, flipped is boolean, sources) returns Manipulator

Deprecated: Use flipManipulator(map)

flipManipulator (base is Vector, direction is Vector, flipped is boolean) returns Manipulator

Deprecated: Use flipManipulator(map)

addManipulators (context is Context, id is Id, manipulators is map)

Add a manipulator to this feature, which will be visible and interactable when a user edits the feature.

addManipulators should be called within the feature function, with the offset on the added manipulator set to match the state of the definition.

Parameter	Type	Additional Info
`manipulators`	`map`	A `map` whose keys will match the keys of `newManipulators` (passed into the Manipulator Change Function), and whose values are the `Manipulators` to be added.

path

Path type

Represents a series of connected edges which form a continuous path.

Value	Type	Description
`Path`	`map`
`edges`	`array`	The edges that form this Path, in the order of the Path.
`flipped`	`array`	An array of booleans corresponding to each edge in the path, set to `true` to traverse the edge backwards.
`closed`	`boolean`	Whether the Path is a closed path.
`adjacentFaces`	`Query`	Optional All adjacent faces on one side of the Path.

canBePath (value) predicate

Typecheck for Path

PathDistanceInformation type

Distance information returned by constructPath and evPathTangentLines when either function is provided with referenceGeometry

Value	Type	Description
`PathDistanceInformation`	`map`
`distance`	`ValueWithUnits`	The distance between the the start of the `Path` and the center of the bounding box of `referenceGeometry`, or infinity if `referenceGeometry` is empty
`withinBoundingBox`	`boolean`	Whether the start of the `Path` is within the bounding box of `referenceGeometry`, or `false` if `referenceGeometry` is empty

canBePathDistanceInformation (value) predicate

Typecheck for PathDistanceInformation

defaultPathDistanceInformation () returns PathDistanceInformation

Returns a PathDistanceInformation with distance set to infinity and withinBoundingBox set to false

reverse (path is Path) returns Path

Reverse the direction of a Path

Parameter	Type	Additional Info
`path`	`Path`	the `Path` to reverse.

constructPath (context is Context, edgesQuery is Query) returns Path

Construct a Path from a Query of edges, picking the starting point of the path based on query evaluation order for edgesQuery

Parameter	Type	Additional Info
`edgesQuery`	`Query`	A `Query` of edges to form into a `Path`. The edges are ordered with query evaluation order, so a `qUnion` should be used to ensure a stable ordering.

constructPath (context is Context, edgesQuery is Query, options is map) returns map

Construct a Path from a Query of edges, optionally picking the starting point as the closest viable starting point to the supplied referenceGeometry

Parameter	Type	Additional Info
`edgesQuery`	`Query`	A `Query` of edges to form into a `Path`.
`options`	`map`
`referenceGeometry`		Optional A geometry `Query` to determine the start of the `Path`. If unspecified, (or the query is empty) the starting point of the path will be based on query evaluation order for `edgesQuery`.
`tolerance`	`ValueWithUnits`	Optional Tolerance with length units indicating how close endpoints need to be to be considered part of the same path. Default is `1e-8 * meter` EXAMPLE `1e-5 * meter`

Return	Type	Description
	`map`
`path`	`Path`	The resulting constructed `Path`
`pathDistanceInformation`	`PathDistanceInformation`	A map containing the distance from the `Path` start point to the center of the bounding box of `referenceGeometry` and whether the `Path` start point falls inside that bounding box.

evPathLength (context is Context, path is Path) returns ValueWithUnits

Return type	Description
`ValueWithUnits`	The total length of the `Path`.

evPathTangentLines (context is Context, path is Path, parameters is array) returns map

Return tangent lines to a Path using arc length parameterization.

Parameter	Type	Additional Info
`path`	`Path`	The `Path` to use.
`parameters`	`array`	An array of numbers in the range 0..1 indicating where along the `Path` to evaluate tangents.

Return	Type	Description
	`map`
`tangentLines`	`array`	The tangent `Line`s corresponding to each parameter
`edgeIndices`	`array`	The indices of the edges in the `Path` corresponding to each parameter

evPathTangentLines (context is Context, path is Path, parameters is array, referenceGeometry) returns map

Return tangent lines to a Path using arc length parameterization. By default, the 0 parameter of the Path will be the start of the Path. If evaluating a closed path, providing reference geometry will alter the 0 parameter to be the closest point on the Path to the reference geometry. Providing reference geometry for a non-closed Path will not change the parameterization of the Path

Parameter	Type	Additional Info
`path`	`Path`	The `Path` to use.
`parameters`	`array`	An array of numbers in the range 0..1 indicating where along the `Path` to evaluate tangents.
`referenceGeometry`		A geometry `Query` to determine the 0 parameter of the `Path`, or `undefined`. If an empty `Query` or `undefined` is specified, the tangents will be evaluated starting at the beginning of the path.

Return	Type	Description
	`map`
`tangentLines`	`array`	The tangent `Line`s corresponding to each parameter
`edgeIndices`	`array`	The indices of the edges in the `Path` corresponding to each parameter
`pathDistanceInformation`	`PathDistanceInformation`	A map containing the distance from the remapped 0 parameter to the center of the bounding box of `referenceGeometry` and whether the remapped 0 parameter falls inside that bounding box. Only valid if the path is closed.

getPathEndVertices (context is Context, path is Path) returns Query

Return query to end vertices of path if open or qNothing if closed.

Parameter	Type	Additional Info
`path`	`Path`	The `Path` to use.

patternCommon

PatternType enum

The type of pattern.

Value	Description
`PART`	Creates copies of bodies.
`FEATURE`	Calls a feature function multiple times, first informing the `context` of the transform to be applied.
`FACE`	Creates copies of faces and attempts to merge them with existing bodies.

MirrorType enum

The type of mirror.

See also

PatternType

Value	Description
`PART`
`FEATURE`
`FACE`

patternUtils

applyPattern (context is Context, id is Id, definition is map, remainingTransform is Transform)

Applies the body, face, or feature pattern, given just transforms and instance names

Parameter	Type	Additional Info
`definition`	`map`
`patternType`	`PatternType`
`entities`	`Query`	Required if `patternType` is not `FEATURE` The faces or parts to pattern.
`instanceFunction`	`FeatureList`	Required if `patternType` is `FEATURE` The features to pattern.
`transforms`	`array`	An `array` of `Transform`s in which to place new instances.
`instanceNames`	`array`	An `array` of the same size as `transforms` with a `string` for each transform, used in later features to identify the entities created.

properties

Properties include name, appearance, material, and part number (see PropertyType). They can be set in FeatureScript, but not read.

setProperty (context is Context, definition is map)

Sets a property on a set of bodies and/or faces. The allowed properties are listed in PropertyType. Only APPEARANCE and NAME properties are supported for faces.

Note: Any properties set in this way will be overridden if they are set directly in the Part Studio (via "Rename", "Set appearance", or the properties dialog). In that case the property value provided in FeatureScript will become shadowed. For example, if a part number is set in a custom feature based on the configuration, manually editing the part number from the properties dialog will override the custom feature's part number for all configurations.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	The bodies and/or faces to apply the property to.
`propertyType`	`PropertyType`	The property to set. EXAMPLE `PropertyType.APPEARANCE` to change the part appearance.
`customPropertyId`	`string`	Required if `propertyType` is `CUSTOM` The id of the custom property. The property id is available from your company's custom properties page. Note that this call performs no checks as to whether the custom property value is valid, so invalid property values may be recorded.
`value`		A `Color` if the `propertyType` is `APPEARANCE`, a `Material` if it is `MATERIAL`, a boolean if it is `EXCLUDE_FROM_BOM`, a value with mass units if it is `MASS_OVERRIDE`, and a string otherwise. The value should be a string for a `CUSTOM` property even if the property is of a non-string type. EXAMPLE `color(1, 0, 0)` to make the part red.

getProperty (context is Context, definition is map)

NOTE: This function cannot be called inside custom features. It can only be called from table functions, editing logic, and manipulator change functions. Getting properties in custom features is not possible, since features are regenerated before any user-set properties are applied.

Returns the value of a property of a single body, which can be either an Onshape property (allowed properties listed on PropertyType) or a custom property defined in company settings.

The returned value's type will correspond to the property type: A Color if the propertyType is APPEARANCE, a Material if it is MATERIAL, a boolean if it is EXCLUDE_FROM_BOM, and a string otherwise. CUSTOM property's returned value will always be a string, even if the custom property is of a non-string type.

Parameter	Type	Additional Info
`definition`	`map`
`entity`	`Query`	A single body the property applies to.
`propertyType`	`PropertyType`	The property to get. EXAMPLE `PropertyType.NAME` to get the body's name
`customPropertyId`	`string`	Required if `propertyType` is `CUSTOM` The id of the custom property. The property id is available from your company's custom properties page.

Color type

Represents a color as red, green, blue, and alpha transparency components, each between 0 and 1 (inclusive).

canBeColor (value) predicate

Typecheck for Color

color (red is number, green is number, blue is number, alpha is number) returns Color

Create a Color from RGBA values, each between 0 and 1 (inclusive)

color (red is number, green is number, blue is number) returns Color

Create an opaque Color from RGB values, each between 0 and 1 (inclusive)

Material type

Represents a material.

canBeMaterial (value) predicate

Typecheck for Material

material (name is string, density is ValueWithUnits)

Constructs a material with a name and a density.

Parameter Type Additional Info

name

string

The displayed name of the material.

density

ValueWithUnits

EXAMPLE

19.3 * gram / centimeter ^ 3

string

Pretty printing and toString methods

toString (value) returns string

Return a string representation of any value.

Overloads of this method are found for many standard and custom types in this and other modules. When overloaded, the toString method will be called inside print and println, allowing users to change how custom types are printed.

toString (value is string) returns string

toString (value is array) returns string

toString (value is map) returns string

print (value)

Print a message to the FeatureScript notices pane.

This has no effect on model state or rendering.

println (value)

Print a message to the FeatureScript notices pane, followed by a newline.

This has no effect on model state or rendering.

println ()

Print a newline to the FeatureScript notices pane.

splitIntoCharacters (s is string) returns array

Split a string into an array of characters, each represented as a string.

parseJson (s is string)

Parse a JSON string into either a map or array. Null values in the JSON are returned as undefined. Throws if the string is not well-formed JSON.

Return type	Description
	A map or an array corresponding to the JSON value.

REGEX_NUMBER const

Matches a number in the string, with or without decimals or exponents.

REGEX_NUMBER_CAPTURE const

Matches a number in the string, with or without decimals or exponents and captures it.

addCustomNumberMatching (regExp is string) returns string

Extends regular expression syntax by adding \f to indicate a complete number

match (s is string, regExp is string) returns map

Test if s matches regExp in its entirety.

Return	Type	Description
	`map`
`hasMatch`	`boolean`	`true` if `regExp` matches `s`
`captures`	`array`	The first element is always the input string `s`. The following elements are a list of all captured groups.

replace (s is string, regExp is string, replacement is string) returns string

Returns a copy of s with every match of regExp replaced with the string replacement.

EXAMPLE

replace("a~~aa~a", "a.", "X") returns X~X~a

stringToNumber (s is string) returns number

Convert a number in string form, into a FS number. Note that this function will not accept trailing non numeric text, the entire string must be a single valid number.

EXAMPLE

stringToNumber("1") returns the number 1

EXAMPLE

stringToNumber("1.0") returns the number 1

EXAMPLE

stringToNumber("1e2") returns the number 100

length (s is string) returns number

Return the number of characters in a string.

substring (s is string, startIndex is number) returns string

Return a substring of a string starting at the specified start index.

EXAMPLE

substring("refactoring", 7) returns "ring"

substring (s is string, startIndex is number, endIndex is number) returns string

Return a substring of a string starting at the specified start index and ending at the specified end index.

EXAMPLE

substring("refactoring", 2, 6) returns "fact"

startsWith (s is string, prefix is string) returns boolean

Return whether a string starts with the specified prefix.

endsWith (s is string, suffix is string) returns boolean

Return whether a string ends with the specified suffix.

splitByRegexp (s is string, separatorRegexp is string) returns array

Split a string into parts based on a regular expression separator.

EXAMPLE

splitByRegexp("this, truly, is a test.", "[,. ]+") returns [ "this" , "truly" , "is" , "a" , "test" ]

EXAMPLE

splitByRegexp("fooooobazzoo", "oo") returns [ "f" , "" , "obazz" ]

EXAMPLE

splitByRegex("foo", "") returns [ "" , "" , "" , "" ]

indexOf (s is string, substr is string) returns number

Return the index of a substring in a string, or -1 if the substring is not found.

indexOf (s is string, substr is string, startIndex is number) returns number

Return the index of a substring in a string starting the search at a specified start index, or -1 if the substring is not found.

indexOfRegexp (s is string, regexp is string) returns number

Return the first index of a regular expression match in a string, or -1 if not found.

indexOfRegexp (s is string, regexp is string, startIndex is number) returns number

Return the first index of a regular expression match in a string starting at the specified start index, or -1 if not found.

repeatString (s is string, count is number) returns string

Return a string made by repeating the first argument a specified number of times. For example: repeatString("foo", 5) returns "foofoofoofoofoo".

isUndefinedOrEmptyString (val) predicate

Is undefined or empty string.

join (arr is array, separator is string) returns string

Concatenates all elements in an array into a string, delimited by a separator string.

join (arr is array) returns string

Concatenates all elements in an array into a string.

tabReferences

PartStudioData type

The value of a Part Studio reference parameter, specifying user-selected parts or other bodies from another Part Studio. The bodies can be added to the current context using an Instantiator.

Full documentation and examples uses can be found here.

Value	Type	Description
`PartStudioData`	`map`
`buildFunction`	`BuildFunction`	A function with one argument (a configuration map) which returns a new context containing all parts of the referenced Part Studio.
`configuration`	`map`	The user-input values for the configuration of the selected Part Studio. The keys of this map are the configuration inputs' FeatureScript ids, and the map can be passed (either as-is or modified) into the buildFunction above, or to `addInstance`.
`partQuery`	`Query`	A query for the user-selected parts in the other context.
`configurationData`	`map`	This maps configuration input FeatureScript ids to maps that have information about the configuration inputs. Each of these maps has a `defaultValue` field with the default value of the configuration input. Enum configuration inputs (configuration lists) also have an `options` field with the value of the Enum.

ImageData type

The value of an image reference parameter, which can be placed in a Part Studio using skImage. Outside of use with skImage, color data for individual pixels is not accessable from FeatureScript.

Full documentation and example uses can be found here.

Value	Type	Description
`ImageData`	`map`
`imageWidth`	`number`	Width of the image, in pixels
`imageHeight`	`number`	Height of the image, in pixels
`mediaType`	`string`	MIME type of the uploaded image

TableData type

The value of a CSV reference parameter, containing the file's tabular data as an array of arrays.

Full documentation and example uses can be found here.

Value	Type	Description
`TableData`	`map`
`csvData`	`array`	If the CSV contains a single rows, this value is a single array of strings or numbers. If the value contains multiple rows, this value is an array of arrays of strings or numbers. Individual cell values can be accessed by indexing into these arrays (`var row1column2 = definition.myTable.csvData[0][1]`), or by iterating through them (`for (var row in definition.myTable.csvData) { println(row); }`).

JSONData type

The value of a JSON reference parameter, containing the file's data.

Value	Type	Description
`JSONData`	`map`
`jsonData`		A value that represents the top-level entity of the imported JSON file: this is a map if the JSON entity is an object, an array if the JSON entity is an array, and likewise for the standard JSON types. Note that JSON `null` values are imported as `undefined`.

TextData type

The value of a Text reference parameter, containing the file's data.

Value	Type	Description
`TextData`	`map`
`textData`	`string`	A value that represents the top-level entity of the imported text file.

CADImportData type

The value of a CAD import reference parameter, which can be used by a Part Studio import feature. The data is not accessible outside of an import operation.

Full documentation and example can be found here.

table

defineTable (table is function) returns function

This function takes a table generation function and wraps it to define a table. It is analogous to defineFeature, except for tables. A typical usage is something like:

annotation { "Table Type Name" : "MyTable" } // This annotation is required for Onshape to recognize myTable as a table.
export const myTable = defineTable(function(context is Context, definition is map) returns Table
    precondition
    {
        ... // Specify the parameters that this table takes, if any
    }
    {
        ... // Compute and return the table, using the context and the parameters
    });

For more information on writing tables, see FeatureScript Tables (TODO) in the language guide.

Parameter	Type	Additional Info
`table`	`function`	A function that takes a `context` and a `definition` and returns a `Table` or a `TableArray`

Table type

A Table represents a read-only table, consisting of rows, columns, and associated entities. Custom tables return a Table or an array of Tables (tagged as a TableArray) as their output.

The user-visible strings in a table, like column headings and cell values can be specified as either a string, a number, a ValueWithUnits or a TemplateString. These are referred to as "table values" and checked by the isTableValue predicate.

Value	Type	Description
`Table`	`map`
`title`		A table value specifying the title of the table
`columnDefinitions`	`array`	An array of `TableColumnDefinition`s specifying the columns.
`rows`	`array`	An array of `TableRow`s specifying the data in the table.
`entities`	`Query`	Optional An optional `Query` specifying the entities associated with the entire table.

canBeTable (value) predicate

Typecheck for Table

table (title, columnDefinitions is array, rows is array) returns Table

Constructs a Table given a title, column definitions, and rows

TableColumnDefinition type

A TableColumnDefinition represents a column in a Table.

Value	Type	Description
`TableColumnDefinition`	`map`
`id`	`string`	The internal id of the column. Referenced in `TableRow`s to specify cell values.
`name`		A table value specifying the column name, which is displayed as the heading
`alignment`	`TableTextAlignment`	Optional How text is aligned in the column. Default is `LEFT`.
`entities`	`Query`	Optional An optional `Query` specifying the entities associated with the column.

canBeTableColumnDefinition (value) predicate

Typecheck for TableColumnDefinition

tableColumnDefinition (id is string, name) returns TableColumnDefinition

Constructs a TableColumnDefinition given an id and a name.

tableColumnDefinition (id is string, name, alignment is TableTextAlignment) returns TableColumnDefinition

Constructs a TableColumnDefinition given an id, a name, and a TableTextAlignment controlling how its cell content is aligned.

tableColumnDefinition (id is string, name, entities is Query) returns TableColumnDefinition

Constructs a TableColumnDefinition given an id, a name, and entities to cross-highlight when mousing over the column.

TableRow type

A TableRow represents a row in a table, including the cells in that row.

Value Type Description

TableRow map

columnIdToCell

map

The cell values. Keys are column ids, as specified in the table column definitions. Values are table values or TableCellErrors.

entities

Query

Optional

An optional Query specifying the entities associated with the row.

canBeTableRow (value) predicate

Typecheck for TableRow

tableRow (columnIdToCell is map) returns TableRow

Constructs a TableRow given the cell values.

tableRow (columnIdToCell is map, entities is Query) returns TableRow

Constructs a TableRow given the cell values and entities.

isTableValue (value) predicate

Returns true if the input is a table value, that is a string, a number, a ValueWithUnits or a TemplateString.

TableArray type

Represents an array of Tables. One possible output of a table function, the other being Table.

canBeTableArray (value) predicate

Typecheck for TableArray

tableArray (value is array) returns TableArray

Constructs a TableArray given an array.

TableCellError type

A TableCellError represents a table cell in an error state. Such a cell has a displayed value as well as an error message that appears as a tooltip over the cell.

Value	Type	Description
`TableCellError`	`map`
`value`		The displayed value, provided as a table value.
`error`		The error message, provided as a table value.

canBeTableCellError (value) predicate

Typecheck for TableCellError.

tableCellError (value, error) returns TableCellError

Constructs a TableCellError given a displayed value and an error message.

StringToleranceComponent type

Represents a component with an inline part followed by stacked upper and lower components.

Value	Type	Description
`StringToleranceComponent`	`map`
`value`		A value to be displayed as a regular row of text.
`upper`		The upper component of the tolerance.
`lower`		The lower component of the tolerance.

stringToleranceComponent (value is map) returns StringToleranceComponent

Constructor for StringToleranceComponent

StringWithTolerances type

Represents a compound string which may contain toleranced components.

Value	Type	Description
`StringWithTolerances`	`map`
`components`		An array of either strings, TemplateStrings, or StringToleranceComponents.

stringWithTolerances (value is map)

Constructor for StringWithTolerances

toString (value is StringToleranceComponent) returns string

toString (value is StringWithTolerances) returns string

concatenateStringsWithTolerances (a is StringWithTolerances, b is StringWithTolerances) returns StringWithTolerances

Concantenates two StringWithTolerances values together.

appendToleranceComponent (result is StringWithTolerances, component) returns StringWithTolerances

Appends either a string, a TemplateString, or a StringToleranceComponent to an existing StringWithTolerances.

createStringWithTolerances (component) returns StringWithTolerances

Creates a StringWithTolerances wrapping the specified component.

tolerancedValueToString (prefix is string, value is ValueWithUnits, tolerance) returns StringWithTolerances

Converts a ValueWithUnits and an associated ToleranceInfo into a StringWithTolerances.

allSolidsAndClosedComposites (context is Context) returns array

Returns an array of maps for all modifiable non-mesh solids and closed composites. Each map has a key part, which maps to a query for the solid or composite and bodies, which maps to either the solid or all constituent bodies. This is useful for iterating over what a user may consider to be "individual parts" in a context.

EXAMPLE

for (var partAndBodies in allSolidsAndClosedComposites(context))
{
    var name = getProperty(context, { "entity" : partAndBodies.part, "propertyType" : PropertyType.NAME } );
    var volume = evVolume(context, { "entities" : partAndBodies.bodies });
}

toString (table is Table) returns string

Tries to convert a table to string form. Because the actual table output depends on user-chosen units and precision, the result of this function may not match it.

toString (value is TemplateString) returns string

templatestring

ValueWithUnitsAndPrecision type

Represents a ValueWithUnits which, when put in a TemplateString will render with a specified precision override.

canBeValueWithUnitsAndPrecision (value) predicate

Typecheck for ValueWithUnitsAndPrecision

valueWithUnitsAndPrecision (value is ValueWithUnits, precision is number) returns ValueWithUnitsAndPrecision

Constructs a ValueWithUnitsAndPrecision given the value and precision.

TemplateString type

A TemplateString represents a value that will be formatted by template substitution. It is useful when, for instance, a table cell needs to display some text in combination with a length formatted in the document length units.

The TemplateString is a map with a string field template. Other fields represent parameters to substitute and may be strings, numbers or ValueWithUnits.

Formatting happens as follows: Text in template that does not contain the number sign # is unchanged. #identifier (where identifier is a valid FeatureScript identifier) causes a substitution with the result of looking up identifier in the map. ## is changed to #. # (The number sign followed by a space) is removed, which can be useful for separating a substitution from text.

EXAMPLE

{ 'template' : 'Length = #len', 'len' : foot } gets formatted as Length = 12 in if document units are inches.

EXAMPLE

{ 'template' : '###var# bar', 'var' : 'foo' } get formatted as #foobar.

canBeTemplateString (value) predicate

Typecheck for TemplateString.

templateString (value is map) returns TemplateString

Constructor for TemplateString.

Parameter Type Additional Info

value

map

A map with a "template" field and any number of other fields, which may be referenced in the template string as e.g. #myValue. Used in FeatureScript tables. See TemplateString docs for more info.

EXAMPLE

{ "template" : "Value of #myValue", "myValue" : 42 }

tolerance

ToleranceType enum

Defines the tolerance type of a hole feature's parameter.

Value	Description
`NONE`	Defines no tolerance.
`SYMMETRICAL`	Defines a tolerance type where the allowed tolerance is a symmetrical deviation.
`DEVIATION`	Defines a tolerance type where the allowed tolerance is an asymmetrical deviation.
`LIMITS`	Defines a tolerance type where the allowed tolerance has defined upper and lower limits.
`MIN`	Defines a tolerance type where the parameter's value is considered the minimum allowed value.
`MAX`	Defines a tolerance type where the parameter's value is considered the maximum allowed value.
`FIT`
`FIT_WITH_TOLERANCE`
`FIT_TOLERANCE_ONLY`

ToleranceTypeExtended enum

Defines the tolerance type of a hole feature's parameter.

Value	Description
`NONE`	Defines no tolerance.
`SYMMETRICAL`	Defines a tolerance type where the allowed tolerance is a symmetrical deviation.
`DEVIATION`	Defines a tolerance type where the allowed tolerance is an asymmetrical deviation.
`LIMITS`	Defines a tolerance type where the allowed tolerance has defined upper and lower limits.
`MIN`	Defines a tolerance type where the parameter's value is considered the minimum allowed value.
`MAX`	Defines a tolerance type where the parameter's value is considered the maximum allowed value.
`FIT`	Defines a tolerance type where the upper and lower limits are defined by the specified fit tolerance class.
`FIT_WITH_TOLERANCE`	Defines a tolerance type where the upper and lower limits are defined by the specified fit tolerance class.
`FIT_TOLERANCE_ONLY`	Defines a tolerance type where the upper and lower limits are defined by the specified fit tolerance class.

ToleranceInfo type

Stores tolerance-related info for a specific field in a feature. This info includes an optional precision override, a tolerance type, and, if applicable, an upper and lower bound associated with that tolerance type.

canBeToleranceInfo (val) predicate

Type checking predicate for the ToleranceInfo type.

toleranceInfo (info is map)

Constructor for the ToleranceInfo type.

ToleranceFitInfo type

Stores fit tolerance-related info for a specific field in a feature.

canBeToleranceFitInfo (val) predicate

Type checking predicate for the ToleranceFitInfo type.

toleranceFitInfo (info is map)

Constructor for the ToleranceFitInfo type.

PrecisionType enum

Defines the precision of a tolerant quantity.

Value	Description
`DEFAULT`
`ONES`	Display precision up to '1'.
`TENTHS`	Display precision up to '0.1'.
`HUNDREDTHS`	Display precision up to '0.01'.
`THOUSANDTHS`	Display precision up to '0.001'.
`TEN_THOUSANDTHS`	Display precision up to '0.0001'.
`HUNDRED_THOUSANDTHS`	Display precision up to '0.00001'.
`MILLIONTHS`	Display precision up to '0.000001'.

defineLengthTolerance (definition is map, field is string, parentParameterName is string) predicate

Creates a parameter group containing length tolerance controls for the specified field in the specified definition.

defineLengthToleranceExtended (definition is map, field is string, parentParameterName is string) predicate

Creates a parameter group containing length fit tolerance controls for the specified field in the specified definition.

defineAngleTolerance (definition is map, field is string, parentParameterName is string) predicate

Creates a parameter group containing angle tolerance controls for the specified field in the specified definition.

getToleranceInfo (definition is map, field is string) returns ToleranceInfo

Extracts the ToleranceInfo associated with a given field in the given feature definition. The ToleranceInfo is gathered from parameters which are created using either the defineLengthTolerance or defineAngleTolerance predicates.

updateFitToleranceFields (context is Context, id is Id, definition is map, field is string) returns map

Updates the fit tolerance field information associated with a specified field in the given feature definition. The tolerance information is extracted from parameters created using the defineLengthToleranceExtended predicates.

Parameter	Type	Additional Info
`context`	`Context`	The target context.
`id`	`Id`	Identifier of the feature.
`definition`	`map`	The feature definition from which to extract and update tolerance information.
`field`	`string`	The field name for which to update tolerance information.

Return type	Description
`map`	The updated feature definition with updated tolerance information.

isToleranceSet (tolerance is ToleranceInfo) returns boolean

Determines whether or not a tolerance is set in a given ToleranceInfo. A tolerance is considered to be "set" if either its tolerance type is set to a value other than NONE, or if it has a precision override value set.

isToleranceInfoOrUndefined (val) predicate

Determines if a given value is either a ToleranceInfo or undefined.

getToleranceBounds (nominal is ValueWithUnits, tolerance is ToleranceInfo, options is map) returns array

Produces an array containing the upper and lower bounds of a ValueWithUnits given a specified ToleranceInfo as well as a map of options.

Parameter	Type	Additional Info
`nominal`	`ValueWithUnits`	the nominal value
`tolerance`	`ToleranceInfo`	the tolerance info for the given value
`options`	`map`
`minimum`	`ValueWithUnits`	the upper bound if the tolerance type is maximum
`maximun`	`ValueWithUnits`	the lower bound if the tolerance type is minimum
`useDrawingLimitsFix`	`boolean`	if false, uses the old bounds calculation of \[lowerLim, upperLim\]

getToleranceBounds (nominal is ValueWithUnits, tolerance, minimum is ValueWithUnits, maximum is ValueWithUnits) returns array

Produces an array containing the upper and lower bounds of a ValueWithUnits given a specified ToleranceInfo.

topologyUtils

edgeIsTwoSided (context is Context, edge is Query) returns boolean

Returns true if edge has two adjacent faces, false if edge is a laminar or wire edge.

isClosed (context is Context, edge is Query) returns boolean

Returns true if edge is closed, false if edge is open

dissolveWires (edgesAndWires is Query) returns Query

Returns the union of any edges from the input query and all the edges of any body from the input query

followWireEdgesToLaminarSource (context is Context, query is Query) returns Query

If the query contains wire edges then this function will track the wire edges back through creation history to find laminar edges that the edge was copied from (or will return the original edge if none).

extractDirection (context is Context, entity is Query)

Extract a direction from an axis or a plane. Useful for processing query parameters with the QueryFilterCompound.ALLOWS_DIRECTION filter.

Return type	Description
	a 3D unit `Vector` if a direction can be extracted, otherwise `undefined`.

connectedComponents (context is Context, entities is Query, adjacencyType is AdjacencyType) returns array

Find connected components in the topological graph of provided entities. Each component is a group of topologically connected entities, and each component is disjoint with (does not connect topologically with) any other component. Connectivity is tested using qAdjacent with the specified adjacencyType.

Returns an array of components. Each component is an array of individual queries. The queries in any component will respect the query evaluation order of the supplied entities Query. The components themselves will also be ordered by query evaluation order, sorted by the first entity in each component.

Unlike constructPaths, this function operates on topological connections (underlying connections by a vertex or edge). Distinct bodies are not topologically connected, so even if two entities on distinct bodies are geometrically related by having a coincident vertex or edge, the entities connected to these coincident vertices or edges will fall into different components. Sketch edges are each represented as a distinct wire body, and are not topologically connected, so this method cannot be used for them.

groupEntitiesByBody (context is Context, entities is Query) returns map

Group entities by their owner body.

Return type	Description
`map`	a map from the transient query for an individual body to an array of transient queries for the individual entities which belong to that body.

sweptAlong (context is Context, face is Query, direction is Vector) returns boolean

Check whether a face is swept along a specified direction.

clusterBodies (context is Context, definition is map) returns array

Groups bodies into clusters of identical topology and identical geometry (up to a relative tolerance), allowing arbitrary 3D rotations (but not reflection).

Parameter Type Additional Info

definition map

bodies

Query

The bodies to cluster

relativeTolerance

number

A tolerance, expressed as a decimal value, to compare bodies with.

EXAMPLE

0.01 to cluster bodies that have a 1% similarity

valueBounds

Value bounds are used to define minimum, maximum, and default values for numbers and values with units. These bounds are in the feature dialog UI for parameters with the given bounds.

In standard usage, a parameter can be specified with e.g. angle bounds in a feature precondition as follows:

isAngle(definition.myAngle, ANGLE_360_BOUNDS);

To change the bounds and defaults on the above declaration, a user may replace ANGLE_360_BOUNDS with another AngleBoundSpec in this module, or define their own. For instance, the following code creates a parameter whose default value is 45 degrees (if the user's settings have degrees as the default) or 1 radian (if the user's settings have radians as the default).

const MY_BOUNDS =
{
    (degree) : [0, 45, 360],
    (radian) : 1
} as AngleBoundSpec;
...
    isAngle(definition.myAngle, MY_BOUNDS);
...

isLength (value, boundSpec is LengthBoundSpec) predicate

True for a value with length units which conforms to the given bounds.

Used in feature preconditions to specify a length parameter.

Parameter Type Additional Info

boundSpec

LengthBoundSpec

Specifies a min, a max, and a default value. These values are possibly different in different units for the sake of round numbers.

To specify a parameter with different default value or different limits, use a different or custom LengthBoundSpec.

isAngle (value, boundSpec is AngleBoundSpec) predicate

True for a value with angle units which conforms to the given bounds.

Used in feature preconditions to specify an angle parameter.

Parameter Type Additional Info

boundSpec

AngleBoundSpec

Specifies a min, a max, and a default value. These values are possibly different in different units for the sake of round numbers.

To specify a parameter with different default value or different limits, use a different or custom AngleBoundSpec.

isInteger (value, boundSpec is IntegerBoundSpec) predicate

True for a number that is an integer and conforms to the given bounds.

Used in feature preconditions to specify an integer or count parameter.

Parameter Type Additional Info

boundSpec

IntegerBoundSpec

Specifies a min, a max, and a default value. These values are possibly different in different units for the sake of round numbers.

To specify a parameter with different default value or different limits, use a different or custom IntegerBoundSpec.

isReal (value, boundSpec is RealBoundSpec) predicate

True for a real number which conforms to the given bounds.

Used in feature preconditions to specify a unitless numeric parameter.

Parameter Type Additional Info

boundSpec

RealBoundSpec

Specifies a min, a max, and a default value. These values are possibly different in different units for the sake of round numbers.

To specify a parameter with different default value or different limits, use a different or custom RealBoundSpec.

LENGTH_BOUNDS const

A LengthBoundSpec for a positive or negative length.

NONNEGATIVE_LENGTH_BOUNDS const

A LengthBoundSpec for a length strictly greater than 0.

NONNEGATIVE_ZERO_INCLUSIVE_LENGTH_BOUNDS const

A LengthBoundSpec for a length greater than or equal to 0.

NONNEGATIVE_ZERO_DEFAULT_LENGTH_BOUNDS const

A LengthBoundSpec for a length greater than or equal to 0, with UI defaults of 0.0 for all units.

NONPOSITIVE_ZERO_DEFAULT_LENGTH_BOUNDS const

A LengthBoundSpec for a length less than or equal to 0, with UI defaults of 0.0 for all units.

ZERO_DEFAULT_LENGTH_BOUNDS const

A LengthBoundSpec for a positive or negative length, with UI defaults of 0.0 for all units.

BLEND_BOUNDS const

A LengthBoundSpec for fillets and chamfers, with smaller defaults than NONNEGATIVE_LENGTH_BOUNDS (0.2 * inch, etc.).

SHELL_OFFSET_BOUNDS const

A LengthBoundSpec for a shell or offset thickness, with smaller defaults than NONNEGATIVE_LENGTH_BOUNDS. (0.1 * inch, etc.).

ZERO_INCLUSIVE_OFFSET_BOUNDS const

A LengthBoundSpec for an offset thickness, for a length greater than or equal to 0, with defaults greater than NONNEGATIVE_ZERO_INCLUSIVE_LENGTH_BOUNDS

ANGLE_360_BOUNDS const

An AngleBoundSpec for an angle between 0 and 360 degrees, defaulting to 30 degrees.

ANGLE_360_REVERSE_DEFAULT_BOUNDS const

An AngleBoundSpec for an angle between 0 and 360 degrees, defaulting to 330 degrees.

ANGLE_360_ZERO_DEFAULT_BOUNDS const

An AngleBoundSpec for an angle between 0 and 360 degrees, defaulting to 0 degrees.

ANGLE_360_FULL_DEFAULT_BOUNDS const

An AngleBoundSpec for an angle between 0 and 360 degrees, defaulting to 360 degrees.

ANGLE_360_90_DEFAULT_BOUNDS const

An AngleBoundSpec for an angle between 0 and 360 degrees, defaulting to 90 degrees.

ANGLE_STRICT_180_BOUNDS const

An AngleBoundSpec for an angle strictly less than 180 degrees.

ANGLE_STRICT_90_BOUNDS const

An AngleBoundSpec for an angle strictly less than 90 degrees.

ANGLE_180_MINUS_180_BOUNDS const

An AngleBoundSpec for an angle between -180 and 180 degrees, defaulting to 0 degrees.

NONPOSITIVE_ZERO_DEFAULT_ANGLE_BOUNDS const

AnAngleBoundSpec for an angle less than or equal to 0, with UI defaults of 0.0 for all units.

NONNEGATIVE_ZERO_DEFAULT_ANGLE_BOUNDS const

An AngleBoundSpec for an angle greater than or equal to 0, with UI defaults of 0.0 for all units.

POSITIVE_COUNT_BOUNDS const

An IntegerBoundSpec for an integer strictly greater than zero, defaulting to 2.

POSITIVE_REAL_BOUNDS const

A RealBoundSpec for a number greater than or equal to zero, defaulting to 1.

SCALE_BOUNDS const

A RealBoundSpec for the positive or negative scale factor on a transform, defaulting to 1.

LengthBoundSpec type

A spec to be used with the isLength predicate to define allowable lengths and customize UI behaviors for feature dialog parameters that take in a length.

A typical declaration looks like:

const MY_LENGTH_BOUNDS =
{
    (meter)      : [-500, 0.0025, 500],
    (centimeter) : .25,
    (millimeter) : 2.50,
    (inch)       : 0.1,
    (foot)       : 0.01,
    (yard)       : 0.0025
} as LengthBoundSpec;

The values for (meter), (inch), etc. define the bounds and default values for a feature parameter defined with MY_LENGTH_BOUNDS. The default values will be different for users who have set different default units.

Specifically, the first unit listed specified defines the minimum value, default value, and the maximum value (in terms of that unit) and the subsequent units define default values for those units, when a user with those default units first opens the dialog. The default value for a unit that is not listed is the default value of the first unit so { (inch) : [0, 1, 1e4] } as LengthBoundSpec will give a default of 2.54 cm in a Part Studio with centimeter units

canBeLengthBoundSpec (value) predicate

Typecheck for LengthBoundSpec

AngleBoundSpec type

A spec to be used with the isAngle predicate to define allowable angles and customize UI behaviors for feature dialog parameters that take in an angle.

A typical declaration looks like:

const ANGLE_360_BOUNDS =
{
    (degree) : [0, 30, 360],
    (radian) : 1
} as AngleBoundSpec;

For more information on what the various fields signify, see LengthBoundSpec.

canBeAngleBoundSpec (value) predicate

Typecheck for AngleBoundSpec

IntegerBoundSpec type

A spec to be used with the isInteger predicate to define allowable numbers and customize UI behaviors for feature dialog parameters that take in a number.

A typical declaration looks like:

const POSITIVE_COUNT_BOUNDS =
{
    (unitless) : [1, 2, 1e5]
} as IntegerBoundSpec;

For more information on what the various fields signify, see LengthBoundSpec.

canBeIntegerBoundSpec (value) predicate

Typecheck for IntegerBoundSpec

RealBoundSpec type

A spec to be used with the isReal predicate to define allowable real numbers and customize UI behaviors for feature dialog parameters that take in a real number.

A typical declaration looks like:

const POSITIVE_REAL_BOUNDS =
{
    (unitless) : [0, 1, 1e5]
} as RealBoundSpec;

For more information on what the various fields signify, see LengthBoundSpec.

canBeRealBoundSpec (value) predicate

Typecheck for RealBoundSpec

wrapSurface

WrapSurface type

Represents the source or destination surface for opWrap. Exactly one of face, plane, or cylinder must be defined.

(Formerly RollSurface)

Value	Type	Description
`WrapSurface`	`map`
`face`	`Query`	The face entity defining this `WrapSurface`.
`plane`	`Plane`	The plane geometry defining this `WrapSurface`.
`cylinder`	`Cylinder`	The cylinder geometry defining this `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`, used to align the `source` and `destination` `WrapSurface`s for `opWrap`. Must lie on the `WrapSurface`. If this condition is not met, `opWrap` will fail.
`anchorDirection`	`Vector`	The anchor direction of the `WrapSurface`, used to align the `source` and `destination` `WrapSurface`s for `opWrap`. Must lie on the tangent plane of the `WrapSurface` at the `anchorPoint`. If this condition is not met, `opWrap` will fail.

isWrapPlane (context is Context, val is WrapSurface) predicate

Returns whether the given WrapSurface is a plane.

Parameter	Type	Additional Info
`val`	`WrapSurface`	The `WrapSurface` to check.

isWrapCylinder (context is Context, val is WrapSurface) predicate

Returns whether the given WrapSurface is a cylinder.

Parameter	Type	Additional Info
`val`	`WrapSurface`	The `WrapSurface` to check.

makeWrapSurface (context is Context, face is Query) returns WrapSurface

Make a WrapSurface for opWrap defined by a planar or cylindrical face.

Parameter	Type	Additional Info
`face`	`Query`	A face to use as the definition face for the `WrapSurface`. For a planar face: The plane `origin` will be used as the `anchorPoint` and the plane `x` direction will be used as the `anchorDirection`. For a cylindrical face: The point at which the cylinder's `coordSystem`'s positive `xAxis` intersects the cylinder will be used as the `anchorPoint`. The cylinder's `yAxis` will be used as the `anchorDirection`. See `WrapSurface` documentation for descriptions of `anchorPoint` and `anchorDirection`.

makeWrapSurface (context is Context, face is Query, anchorPoint is Vector, spin is ValueWithUnits) returns WrapSurface

Make a WrapSurface for opWrap defined by a planar or cylindrical face.

Parameter	Type	Additional Info
`face`	`Query`	A face to use as the definition face for the `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`. See `WrapSurface` documentation.
`spin`	`ValueWithUnits`	For a planar face: Angle of a counter-clockwise spin to apply to the `plane`'s `x` axis about its positive `z` axis, which is then used as the `anchorDirection`. For a cylindrical face: Angle of a counter-clockwise spin to apply to the `cylinder`'s canonical `anchorDirection` at the given `anchorPoint` about the direction vector from the cylinder axis to the `anchorPoint`. The canonical `anchorDirection` at the given `anchorPoint` is defined as the "rightward" direction when looking at the cylinder in the direction from the `anchorPoint` to the cylinder axis with the cylinder's `zAxis` up. In other words: `cross(cylinder z axis, direction vector from cylinder axis to anchorPoint)`. This spun direction is then used as the `anchorDirection`. See `WrapSurface` documentation for a description of `anchorDirection`.

makeWrapSurface (context is Context, face is Query, anchorPoint is Vector, anchorDirection is Vector) returns WrapSurface

Make a WrapSurface for opWrap defined by a planar or cylindrical face.

Parameter	Type	Additional Info
`face`	`Query`	A face to use as the definition face for the `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`. See `WrapSurface` documentation.
`anchorDirection`	`Vector`	The anchor direction of the `WrapSurface`. See `WrapSurface` documentation.

makeWrapPlane (plane is Plane) returns WrapSurface

Make a WrapSurface for opWrap from a Plane.

Parameter	Type	Additional Info
`plane`	`Plane`	The definition plane for the `WrapSurface`. The plane `origin` will be used as the `anchorPoint` and the plane `x` direction will be used as the `anchorDirection`. See `WrapSurface` documentation for descriptions of `anchorPoint` and `anchorDirection`.

makeWrapPlane (plane is Plane, anchorPoint is Vector, spin is ValueWithUnits) returns WrapSurface

Make a WrapSurface for opWrap from a Plane.

Parameter	Type	Additional Info
`plane`	`Plane`	The definition plane for the `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`. See `WrapSurface` documentation.
`spin`	`ValueWithUnits`	Angle of a counter-clockwise spin to apply to the `plane`'s `x` axis about its positive `z` axis, which is then used as the `anchorDirection`. See `WrapSurface` documentation for a description of `anchorDirection`.

makeWrapPlane (plane is Plane, anchorPoint is Vector, anchorDirection is Vector) returns WrapSurface

Make a WrapSurface for opWrap from a Plane.

Parameter	Type	Additional Info
`plane`	`Plane`	The definition plane for the `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`. See `WrapSurface` documentation.
`anchorDirection`	`Vector`	The anchor direction of the `WrapSurface`. See `WrapSurface` documentation.

makeWrapPlane (context is Context, planarFace is Query, anchorPoint is Vector, anchorDirection is Vector) returns WrapSurface

Make a WrapSurface for opWrap from a planar face.

Parameter	Type	Additional Info
`planarFace`	`Query`	A planar face to use as the definition plane for the `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`. See `WrapSurface` documentation.
`anchorDirection`	`Vector`	The anchor direction of the `WrapSurface`. See `WrapSurface` documentation.

flipWrapPlane (wrapPlane is WrapSurface) returns WrapSurface

Flip the normal direction of the Plane described by this WrapSurface. Do not change the anchorPoint or anchorDirection.

makeWrapCylinder (cylinder is Cylinder) returns WrapSurface

Make a WrapSurface for opWrap from a Cylinder.

Parameter	Type	Additional Info
`cylinder`	`Cylinder`	The definition cylinder for the `WrapSurface`. The point at which the cylinder's `coordSystem`'s positive `xAxis` intersects the cylinder will be used as the `anchorPoint`. The cylinder's `yAxis` will be used as the `anchorDirection`. See `WrapSurface` documentation for descriptions of `anchorPoint` and `anchorDirection`.

makeWrapCylinder (cylinder is Cylinder, anchorPoint is Vector, spin is ValueWithUnits) returns WrapSurface

Make a WrapSurface for opWrap from a Cylinder.

Parameter	Type	Additional Info
`cylinder`	`Cylinder`	The definition cylinder for the `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`. See `WrapSurface` documentation.
`spin`	`ValueWithUnits`	Angle of a counter-clockwise spin to apply to the `cylinder`'s canonical `anchorDirection` at the given `anchorPoint` about the direction vector from the cylinder axis to the `anchorPoint`. The canonical `anchorDirection` at the given `anchorPoint` is defined as the "rightward" direction when looking at the cylinder in the direction from the `anchorPoint` to the cylinder axis with the cylinder's `zAxis` up. In other words: `cross(cylinder z axis, direction vector from cylinder axis to anchorPoint)`. This spun direction is then used as the `anchorDirection`. See `WrapSurface` documentation for a description of `anchorDirection`.

makeWrapCylinder (cylinder is Cylinder, anchorPoint is Vector, anchorDirection is Vector) returns WrapSurface

Make a WrapSurface for opWrap from a Cylinder.

Parameter	Type	Additional Info
`cylinder`	`Cylinder`	The definition cylinder for the `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`. See `WrapSurface` documentation.
`anchorDirection`	`Vector`	The anchor direction of the `WrapSurface`. See `WrapSurface` documentation.

makeWrapCylinder (context is Context, cylindricalFace is Query, anchorPoint is Vector, anchorDirection is Vector) returns WrapSurface

Make a WrapSurface for opWrap from a cylindrical face.

Parameter	Type	Additional Info
`cylindricalFace`	`Query`	A cylindrical face to use as the definition cylinder for the `WrapSurface`.
`anchorPoint`	`Vector`	The anchor point of the `WrapSurface`. See `WrapSurface` documentation.
`anchorDirection`	`Vector`	The anchor direction of the `WrapSurface`. See `WrapSurface` documentation.

Onshape features

bodyDraft

bodyDraft (context is Context, id is Id, definition is map)

An operation that performs an opBodyDraft.

bodyDraftEditLogic (context is Context, id is Id, oldDefinition is map, definition is map, isCreating is boolean, specifiedParameters is map) returns map

body draft editing logic

boolean

booleanBodies (context is Context, id is Id, definition is map)

The boolean feature. Performs an opBoolean after a possible opOffsetFace if the operation is subtraction.

convertNewBodyOpToBoolOp (operationType is NewBodyOperationType) returns BooleanOperationType

Maps a NewBodyOperationType (used in features like extrude) to its corresponding BooleanOperationType.

booleanStepTypePredicate (booleanDefinition is map) predicate

Predicate which specifies a field operationType of type NewBodyOperationType. Used by body-creating feature preconditions such as extrude, revolve, sweep or loft.

When used in a precondition, NewBodyOperationType creates UI like the extrude feature, with a horizontal list of the words "New", "Add", etc. When using this predicate in features, make sure to export an import of tool.fs so that NewBodyOperationType is visible to the Part Studios:

export import(path : "onshape/std/tool.fs", version : "");

booleanStepScopePredicate (booleanDefinition is map) predicate

Used by body-creating feature preconditions to allow post-creation booleans, specifying the merge scope (or "Merge with all") for that boolean.

Designed to be used together with booleanStepTypePredicate.

booleanPatternScopePredicate (booleanDefinition is map) predicate

Used by body-creating pattern feature preconditions to allow post-creation booleans with surfaces or solids, specifying the merge scope (or "Merge with all") for that boolean.

processNewBodyIfNeeded (context is Context, id is Id, definition is map, reconstructOp is function)

This function is designed to be used by body-creating features (like extrude) as a boolean post-processing step with options from booleanStepTypePredicate and booleanStepScopePredicate in the case where the preceding operations of the feature have created new solid or surface bodies. On top of the regular boolean operation, converts the operationType and creates error bodies on failure.

Parameter	Type	Additional Info
`id`	`Id`	identifier of the main feature
`definition`	`map`
`operationType`	`NewBodyOperationType`	EXAMPLE `NewBodyOperationType.ADD` performs a boolean union EXAMPLE `NewBodyOperationType.NEW` does nothing
`defaultScope`	`boolean`	Optional EXAMPLE `true` indicates merge scope of "everything else" (default) EXAMPLE `false` indicates merge scope is specified in `booleanScope`
`booleanScope`	`Query`	targets to use if `defaultScope` is false
`seed`	`Query`	Optional If set, will be included in the tools section of the boolean.
`mergeScopeExclusion`	`Query`	Optional If set, will be excluded from the targets section of the boolean.
`reconstructOp`	`function`	A function which takes in an Id, and reconstructs the input to show to the user as error geometry in case the input is problematic or the boolean itself fails. EXAMPLE `function() {}` . For a more elaborate example see the source code of revolve feature in the Standard Library.

surfaceOperationTypePredicate (surfaceDefinition is map) predicate

Predicate which specifies a field surfaceOperationType of type NewSurfaceOperationType. Used by surface-creating feature preconditions such as revolve, sweep or loft.

When used in a precondition, NewSurfaceOperationType creates UI like the sweep feature, with a horizontal list of the words "New" and "Add". When using this predicate in features, make sure to export an import of tool.fs so that NewSurfaceOperationType is visible to the Part Studios:

export import(path : "onshape/std/tool.fs", version : "");

surfaceJoinStepScopePredicate (definition is map) predicate

Used by surface-creating feature preconditions to allow post-creation booleans, specifying the merge scope (or "Merge with all") for that boolean.

Designed to be used together with surfaceOperationTypePredicate.

joinSurfaceBodiesWithAutoMatching (context is Context, id is Id, definition is map, makeSolid is boolean, reconstructOp is function)

This function is designed to be used by surface-body-creating features (like extrude) as a boolean post-processing step with options from surfaceOperationTypePredicate and surfaceJoinStepScopePredicate. It detects matching edges of adjacent bodies and joins surface bodies at these edges.

Parameter	Type	Additional Info
`id`	`Id`	identifier of the feature
`definition`	`map`
`defaultSurfaceScope`	`boolean`	Optional EXAMPLE `true` indicates merge scope of all the original and related surfaces used as input to create this surface (default) EXAMPLE `false` indicates merge scope is specified in `booleanSurfaceScope`
`booleanSurfaceScope`	`Query`	Optional targets to use if `defaultSurfaceScope` is false Default is `qNothing()`
`seed`	`Query`	Optional Default is `qNothing()` If set, will be included in the tools section of the boolean.
`makeSolid`	`boolean`	Tries to join the surfaces into a solid
`reconstructOp`	`function`	A function which takes in an Id, and reconstructs the input to show to the user as error geometry in case the input is problematic or the join itself fails. EXAMPLE `function() {}` . For a more elaborate example see the source code of revolve feature in the Standard Library.

bridgingCurve

BridgingCurveMatchType enum

Specifies how the bridging curve will match the vertex or edge at each side

Value	Description
`POSITION`	The bridging curve will end at the provided vertex. Direction of the curve is unspecified
`TANGENCY`	The bridging curve will end at the vertex and the curve will be tangent to the edge
`CURVATURE`	The bridging curve will end at the vertex and the curve will have same curvature as the edge at the vertex
`G3`

BIAS_BOUNDS const

A RealBoundSpec for bias of a tangency/tangency bridge, defaulting to 0.5.

bridgingCurve (context is Context, id is Id, definition is map)

Creates a curve between two points, optionally with matching of tangency or curvature to other curves at that point

SideQueries type

Data type for side queries

Value	Type	Description
`SideQueries`	`map`
`vertex`	`Query`	Optional The vertex element on a side query
`edge`	`Query`	Optional The edge element on a side query
`face`	`Query`	Optional The face element on a side query

SideData type

Data type for precomputed side data

Value Type Description

SideData map

point

Vector

The position

frame

EdgeCurvatureResult

Optional

The coordSystem and curvature at the given position

TwoSidesData type

Aggregation of both sides SideData

Value	Type	Description
`TwoSidesData`	`map`
`side1`	`SideData`	SideData map for start side
`side2`	`SideData`	SideData map for end side

BridgingSideData type

Data type for unified control points computation

Value	Type	Description
`BridgingSideData`	`map`
`degree`	`number`	0 for positional continuity (G0), 1 for tangent continuity (G1), 2 for curvature continuity (G2)
`position`	`Vector`	The position
`tangent`	`Vector`	Required if `degree` >= 1 The tangent direction vector
`speedScale`	`number`	Optional How much to scale the default speed
`curvatureDirection`	`Vector`	Required if `degree` == 2 The curvature direction vector
`curvature`	`ValueWithUnits`	Required if `degree` == 2 The curvature magnitude (inverse length units)
`curvatureOffsetScale`	`number`	Optional How much to scale the default third control point offset

computeBridgingControlPoints (context is Context, side1 is BridgingSideData, side2 is BridgingSideData) returns array

Returns an array of control points for a bridigng bezier curve given two side constraints

bsurf

BSurfEndDerivativeType enum

Specifies an end condition for one side of a boundary surface.

Value	Description
`DEFAULT`
`NORMAL_TO_PROFILE`
`TANGENT_TO_PROFILE`
`MATCH_TANGENT`
`MATCH_CURVATURE`
`NORMAL_DIRECTION`
`TANGENT_DIRECTION`

BSurfComputationType enum

How the boundary surface is computed

Value	Description
`COONS`
`MINIMIZATION`

boundarySurface (context is Context, id is Id, definition is map)

Feature for testing Boundary Surface strategies

chamfer

chamfer (context is Context, id is Id, definition is map)

The chamfer feature directly performs an opChamfer operation.

circularPattern

circularPattern (context is Context, id is Id, definition is map)

Performs a body, face, or feature circular pattern. Internally, performs an applyPattern, which in turn performs an opPattern or, for a feature pattern, calls the feature function.

Parameter	Type	Additional Info
`definition`	`map`
`patternType`	`PatternType`	Optional Specifies a `PART`, `FEATURE`, or `FACE` pattern. Default is `PART`.
`entities`	`Query`	Required if `patternType` is `PART` The parts to pattern. EXAMPLE `qCreatedBy(id + "extrude1", EntityType.BODY)`
`faces`	`Query`	Required if `patternType` is `FACE` The faces to pattern.
`instanceFunction`	`FeatureList`	Required if `patternType` is `FEATURE` The `FeatureList` of the features to pattern.
`axis`	`Query`	The axis of the pattern.
`angle`	`ValueWithUnits`	The angle between each pattern instance, or the total angle spanned by the pattern if `equalSpace` is `true`. EXAMPLE `360 * degree`
`instanceCount`	`number`	The resulting number of pattern entities, unless `isCentered` is `true`. EXAMPLE `4` to have 4 resulting pattern entities (including the seed).
`oppositeDirection`	`boolean`	Optional EXAMPLE `true` to switch the direction of the pattern around the axis.
`equalSpace`	`boolean`	Optional EXAMPLE `true` for the entire pattern to lie within `angle` EXAMPLE `false` for there to be `angle` between each pattern instance (default)
`isCentered`	`boolean`	Optional Whether to center the pattern on the seed. When set to `true`, `instanceCount - 1` pattern entities are created in each direction around the axis. Default is `false`.
`operationType`	`NewBodyOperationType`	Optional Specifies how the newly created body will be merged with existing bodies.
`defaultScope`	`boolean`	Optional EXAMPLE `true` to merge with all other bodies EXAMPLE `false` to merge with `booleanScope`
`booleanScope`	`Query`	Required if `defaultScope` is `false` The specified bodies to merge with.
`skipInstances`	`boolean`	Optional Whether to exclude certain instances of the pattern.
`skippedInstances`	`array`	Required if `skipInstances` is `true` Which instances of the pattern to skip. Each is denoted by a single index, which may be negative if `isCentered` is `true`. EXAMPLE `[{ index: -3 }, { index: 2 }, { index: 5 }]`

compositeCurve

compositeCurve (context is Context, id is Id, definition is map)

Creates one or more Curves that are a combination of edges from various sources, be they parts, surfaces, sketches or other Curves.

compositePart

compositePart (context is Context, id is Id, definition is map)

Feature that creates a composite part from provided bodies. Performs an opCreateCompositePart.

cplane

CPlaneType enum

The method of defining a construction plane.

Value	Description
`OFFSET`
`PLANE_POINT`
`LINE_ANGLE`
`LINE_POINT`
`THREE_POINT`
`MID_PLANE`
`CURVE_POINT`
`TANGENT_PLANE`

cPlane (context is Context, id is Id, definition is map)

Creates a construction plane feature by calling opPlane.

curvePattern

CurvePatternSpacingType enum

Specifies the type of spacing between pattern instances.

Value	Description
`EQUAL`	Equal-spaced instances along the length of curve
`DISTANCE`	Instances spaced by custom distance

curvePattern (context is Context, id is Id, definition is map)

Performs a body, face, or feature curve pattern. Internally, performs an applyPattern, which in turn performs an opPattern or, for a feature pattern, calls the feature function.

Parameter	Type	Additional Info
`definition`	`map`
`patternType`	`PatternType`	Optional Specifies a `PART`, `FEATURE`, or `FACE` pattern. Default is `PART`.
`entities`	`Query`	Required if `patternType` is `PART` The parts to pattern. EXAMPLE `qCreatedBy(id + "extrude1", EntityType.BODY)`
`faces`	`Query`	Required if `patternType` is `FACE` The faces to pattern.
`instanceFunction`	`FeatureList`	Required if `patternType` is `FEATURE` The `FeatureList` of the features to pattern.
`edges`	`Query`	A `Query` for a set of edges to pattern along. The edges must form a continuous path.
`spacingType`	`CurvePatternSpacingType`	Specifies the type of spacing between pattern entities. Default is `EQUAL`.
`distance`	`ValueWithUnits`	Required if `spacingType` is `DISTANCE` The distance between each pattern entity. EXAMPLE `1.0 * inch` to space the pattern entities 1 inch apart.
`instanceCount`	`number`	The resulting number of pattern entities. EXAMPLE `2` to have 2 resulting pattern entities (including the seed).
`keepOrientation`	`boolean`	Optional EXAMPLE `true` for the pattern entities to keep the orientation of the seed EXAMPLE `false` for the pattern entities to reorient along the path (default)
`operationType`	`NewBodyOperationType`	Optional Specifies how the newly created body will be merged with existing bodies.
`defaultScope`	`boolean`	Optional EXAMPLE `true` to merge with all other bodies EXAMPLE `false` to merge with `booleanScope`
`booleanScope`	`Query`	Required if `defaultScope` is `false` The specified bodies to merge with.
`skipInstances`	`boolean`	Optional Whether to exclude certain instances of the pattern.
`skippedInstances`	`array`	Required if `skipInstances` is `true` Which instances of the pattern to skip. Each is denoted by a single positive index. EXAMPLE `[{ index: 2 }, { index: 5 }]`

cutlist

cutlist (context is Context, id is Id, definition is map)

Create a cut list from a set of frame selections.

cutlistEditLogic (context is Context, id is Id, oldDefinition is map, definition is map, isCreating is boolean) returns map

internal

decal

decal (context is Context, id is Id, definition is map)

Feature to place and position decal attributes on a surface.

vectorInPlanePerpendicularToZ (planeNormal is Vector) returns Vector

For a plane, get the x direction that is perpendicular to the global Z axis

deleteBodies

CompositePartDeleteOptions enum

Options that determine how the Delete part feature handles composite parts

Value	Description
`DELETE`	Any selected composite parts are deleted along with their constituents
`DISSOLVE`	Constituents of composites are only deleted if explicitly selected
`IGNORE`	Disallow selection of composite parts

deleteBodies (context is Context, id is Id, definition is map)

Feature performing an opDeleteBodies.

deleteFace

DeleteFaceType enum

Specifies how the void resulting from delete face should be closed, if at all.

Value	Description
`HEAL`	Close void by shrinking or growing adjacent faces.
`CAP`	Close void by a simple surface passing through all edges.
`VOID`	Do not close the void. Creates surface out of solids.

deleteFace (context is Context, id is Id, definition is map)

Feature performing an opDeleteFace. Has options to heal the void created by removing the selected faces, or to leave it open.

draft

DraftFeatureType enum

Types of drafts available for the draft feature.

Value	Description
`NEUTRAL_PLANE`	Draft by holding the intersection between a set of faces and a neutral plane as a constant.
`PARTING_LINE`	Draft by holding a set of parting edges as a constant.

PartingLineSides enum

Specifies which faces to draft when drafting with DraftFeatureType.PARTING_LINE.

Value	Description
`ONE_SIDED`	Draft one of the faces attached to the parting line.
`SYMMETRIC`	Draft both of the faces attached to the parting line symmetrically.
`TWO_SIDED`	Draft both of the faces attached to the parting line with separate draft angles.

draft (context is Context, id is Id, definition is map)

Feature performing an opDraft.

Parameter	Type	Additional Info
`definition`	`map`
`draftFeatureType`	`DraftFeatureType`	Optional Specifies a `NEUTRAL_PLANE` or `PARTING_LINE` draft. Default is `NEUTRAL_PLANE`.
`neutralPlane`	`Query`	Required if `draftFeatureType` is `NEUTRAL_PLANE` A planar face or mate connector defining both the neutral plane and pull direction of the the draft. The intersection of the drafted faces and the neutral plane remains unchanged. The pull direction of the draft will be the face normal or mate connector z-axis.
`draftFaces`	`Query`	Required if `draftFeatureType` is `NEUTRAL_PLANE` The faces to draft for a `NEUTRAL_PLANE` draft.
`pullDirectionEntity`	`Query`	Required if `draftFeatureType` is `PARTING_LINE` An entity defining the pull direction of the draft. This entity should conform to the `ALLOWS_DIRECTION` specification in `QueryFilterCompound`.
`partingEdges`	`Query`	Required if `draftFeatureType` is `PARTING_LINE` Edges defining the parting line of the draft. These edges will remain unchanged as some adjacent faces, as defined by `partingLineSides`, are drafted.
`hintFaces`	`Query`	Optional For Onshape internal use. For `PARTING_LINE` draft, specifies in advance which adjacent faces of `partingEdges` should be treated as more along the pull direction. When unspecified, the feature will use a geometric calculation to determine this distinction.
`partingLineSides`	`PartingLineSides`	Required if `draftFeatureType` is `PARTING_LINE` Specifies whether to draft one or both faces adjacent to the parting edges, and whether the draft should be symmetrical if drafting both faces. See `PartingLineSides`.
`alongPull`	`boolean`	Required if `PartingLineSides` is `ONE_SIDED` Specifies which face will be drafted in a `ONE_SIDED` `PARTING_LINE` draft. If `true`, the face which is more along the pull direction from the perspective of the parting edge is drafted. If `false`, the face which is more away from the pull direction from the perspective of the parting edge is drafted.
`angle`	`ValueWithUnits`	The draft angle, must be between 0 and 89.9 degrees. EXAMPLE `3 * degree`
`pullDirection`	`boolean`	Optional Whether the pull direction of the draft should be reversed. In equivalent terms, whether the draft should use `-angle` as the draft angle (`true`), or `angle` as the draft angle (`false`). Default is `false`.
`secondAngle`	`ValueWithUnits`	Required if `PartingLineSides` is `TWO_SIDED` The second draft angle for a `TWO_SIDED` `PARTING_LINE` draft. Must be between 0 and 89.9 degrees. Note that when using `TWO_SIDED`, `angle` will be applied to faces that are away from the pull direction, from the perspective of the edge. `secondAngle` will be applied to faces that are along the pull direction, from the perspective of the edge. EXAMPLE `3 * degree`
`secondPullDirection`	`boolean`	Optional Whether the pull direction of the draft should be reversed for the second angle of a `TWO_SIDED` draft. In equivalent terms, whether the draft should use `-secondAngle` as the second draft angle (`true`), or `secondAngle` as the second draft angle (`false`). Default is `false`.
`tangentPropagation`	`boolean`	Optional For a `NEUTRAL_PLANE` draft, `true` to propagate draft across tangent faces. Default is `false`.
`referenceEdgePropagation`	`boolean`	Optional For a `PARTING_LINE` draft, `true` to extend the parting line across connected edges of already included faces and tangent faces. Default is `false`.
`reFillet`	`boolean`	Optional `true` to attempt to defillet draft faces before the draft and reapply the fillets after. Default is `false`.

editCurve

CONTROL_POINT_INDEX_BOUND const

An IntegerBoundSpec for control point indices.

PlaneReference enum

Reference plane enum for planarization

Value	Description
`BEST`
`YZPLANE`
`XZPLANE`
`XYPLANE`
`CUSTOM`

editCurve (context is Context, id is Id, definition is map)

A curve editing feature.

onEditCurveManipulatorChange (context is Context, definition is map, newManipulators is map) returns map

Manipulator change handling for curve editing

editCurveEditLogic (context is Context, id is Id, oldDefinition is map, definition is map, isCreating is boolean) returns map

Edit logic function for curve editing

enclose

enclose (context is Context, id is Id, definition is map)

Feature performing an opEnclose.

endcap

endcap (context is Context, id is Id, definition is map)

Construct a endcap.

extend

ExtendBoundingType enum

Bounding type used with extend.

Value	Description
`BLIND`
`UP_TO_FACE`
`UP_TO_BODY`
`UP_TO_VERTEX`

extendSurface (context is Context, id is Id, definition is map)

Extends a surface body by calling opExtendSheetBody.

externalThread

externalThread (context is Context, id is Id, definition is map)

Given a list of edge or selections and an optional offset, find the cylindrical faces corresponding to them split the face at the offset, and add external thread size data.

getSplitData (context is Context, topLevelId is Id, endEdge is Query, minorDiameter is ValueWithUnits) returns map

From a starting edge selection, get data about a valid cylindrical face to annotation and/or cut and data about the direction to cut.

extrude

extrude (context is Context, id is Id, definition is map)

Create an extrude, as used in Onshape's extrude feature.

Internally, performs an opExtrude, followed by an opBoolean, possibly followed by a opDraft, possibly in two directions. If creating a simple extrusion, prefer using opExtrude alone.

Parameter	Type	Additional Info
`definition`	`map`
`bodyType`	`ExtendedToolBodyType`	Optional Specifies a `SOLID` or `SURFACE` or `THIN` extrude. Default is `SOLID`.
`entities`	`Query`	Required if `bodyType` is `SOLID` The planar faces and/or sketch regions to extrude. EXAMPLE `qSketchRegion(id + "sketch1")` specifies all sketch regions of a given sketch.
`surfaceEntities`	`Query`	Required if `bodyType` is `SURFACE` The sketch curves to extrude. EXAMPLE `qCreatedBy(id + "sketch1", EntityType.EDGE)`
`endBound`	`BoundingType`	Optional The end bounding condition for the extrude. Default is `BLIND`.
`oppositeDirection`	`boolean`	Optional EXAMPLE `true` to flip the direction of the extrude to point opposite the face/sketch normal.
`depth`	`ValueWithUnits`	Required if `endBound` is `BLIND` A length specifying the extrude depth. For a blind extrude, specifies the depth of the first extrude direction. For a symmetric extrude, specifies the full extrude depth. EXAMPLE `0.5 * inch`
`endBoundEntityFace`	`Query`	Required if `endBound` is `UP_TO_SURFACE` Specifies the face or surface to bound the extrude.
`endBoundEntityBody`	`Query`	Required if `endBound` is `UP_TO_BODY` Specifies the surface or solid body to bound the extrude.
`endBoundEntityVertex`	`Query`	Required if `endBound` is `UP_TO_VERTEX` Specifies the vertex to bound the extrude.
`hasOffset`	`boolean`	Optional EXAMPLE `true` to add a translational offset from the selected face, surface, solid body or vertex.
`offsetDistance`	`ValueWithUnits`	Required if `offset` is `true` The translational distance between the selected face, surface, solid body or vertex and the cap of the extrude. EXAMPLE `0.5 * inch`
`offsetOppositeDirection`	`boolean`	Optional EXAMPLE `false` to offset away from the selected end bound (default) EXAMPLE `true` to offset into the selected end bound
`hasDraft`	`boolean`	Optional EXAMPLE `true` to add a draft to the extrude.
`draftAngle`	`ValueWithUnits`	Required if `hasDraft` is `true` The angle, as measured from the extrude direction, at which to draft. EXAMPLE `10 * degree`
`draftPullDirection`	`boolean`	Optional EXAMPLE `false` to draft outwards (default) EXAMPLE `true` to draft inwards
`hasSecondDirection`	`boolean`	Optional EXAMPLE `true` to specify a second direction.
`secondDirectionBound`	`BoundingType`	Optional The bounding type of the second direction. Can be different from the bounding type of the first direction.
`secondDirectionOppositeDirection`	`boolean`	Optional EXAMPLE `true` will flip the second end direction to align opposite the plane/face's normal.
`secondDirectionDepth`	`ValueWithUnits`	Required if `secondDirectionBound` is `BLIND` A length specifying the second direction's extrude depth.
`secondDirectionBoundEntityFace`	`Query`	Required if `secondDirectionBound` is `UP_TO_SURFACE` specifies the face or surface to bound the extrude.
`secondDirectionBoundEntityBody`	`Query`	Required if `secondDirectionBound` is `UP_TO_BODY` specifies the surface or solid body to bound the extrude.
`secondDirectionBoundEntityVertex`	`Query`	Required if `secondDirectionBound` is `UP_TO_VERTEX` specifies the vertex to bound the extrude.
`hasSecondDirectionOffset`	`boolean`	Optional EXAMPLE `true` to add a translational offset from the selected face, surface, solid body or vertex.
`secondDirectionOffsetDistance`	`ValueWithUnits`	Required if `offset` is `true` The translational distance between the selected face, surface, solid body or vertex and the cap of the extrude. EXAMPLE `0.5 * inch`
`secondDirectionOffsetOppositeDirection`	`boolean`	Optional EXAMPLE `false` to offset away from the selected second direction end bound (default) EXAMPLE `true` to offset into the selected second direction end bound
`hasSecondDirectionDraft`	`boolean`	Optional EXAMPLE `true` to add a draft to the second direction extrude.
`secondDirectionDraftPullDirection`	`boolean`	Optional EXAMPLE `false` to draft the second direction outwards (default) EXAMPLE `true` to draft the second direction inwards
`operationType`	`NewBodyOperationType`	Optional Specifies how the newly created body will be merged with existing bodies.
`defaultScope`	`boolean`	Optional EXAMPLE `true` to merge with all other bodies EXAMPLE `false` to merge with `booleanScope`
`booleanScope`	`Query`	Required if `defaultScope` is `false` The specified bodies to merge with.
`wallShape`	`Query`	Required if `bodyType` is `THIN` The specified planar face or sketch edges defining the thin wall shape.
`thickness1`	`ValueWithUnits`	Required if `bodyType` is `THIN` The outwards thickness of the thin wall.
`thickness2`	`ValueWithUnits`	Required if `bodyType` is `THIN` The inwards thickness of the thin wall.
`flipWall`	`boolean`	Optional EXAMPLE `true` to apply the first offset value instead of the second and vice versa

faceBlend

faceBlend (context is Context, id is Id, definition is map)

Feature performing a face blend.

faceIntersection

intersectionCurve (context is Context, id is Id, definition is map)

Creates curves where two faces intersect.

fillSurface

fill (context is Context, id is Id, definition is map)

Creates a surface bounded by input edges with prescribed continuity conditions, using opFillSurface.

fillet

fillet (context is Context, id is Id, definition is map)

Feature performing an opFillet or opFullRoundFillet.

fitSpline

FitSplineType enum

The type of fit spline.

Value	Description
`VERTICES`	Creates spline through selected vertices.
`EDGES`	Approximates a set of edges by a single spline.

fitSpline (context is Context, id is Id, definition is map)

Feature performing either opFitSpline or opSplineThroughEdges depending on selection

frame

frame (context is Context, id is Id, definition is map)

Create frames from a profile and set of path selections.

frameTrim

frameTrim (context is Context, id is Id, definition is map)

Trim frames against faces, or perform an ordered trim of frame groups.

gusset

GussetStyleType enum

Defines the shape of the gusset.

Value	Description
`TRIANGLE`
`RECTANGLE`

GussetPosition enum

Defines the alignment of the gusset.

Value	Description
`CENTERED`
`ALIGNED`

gusset (context is Context, id is Id, definition is map)

Create gussets based on the selected edges.

helix

AxisType enum

Describes the type of body on which to create a helix.

Value	Description
`SURFACE`	Impose a helix onto a cylinder or cone.
`AXIS`	Revolve a helix around an axial edge or mate connector.
`CIRCLE`	Revolve a helix along a circular path.

PathType enum

Describes the parameter(s) to vary when computing the path of a helix.

Value	Description
`TURNS`	Allow only the number of turns (revolutions) to be varied.
`PITCH`	Allow only the space between each turn (helical pitch) to be varied.
`TURNS_PITCH`	Allow both turns and pitch to be varied. Always results in a cylindrical helix.

StartType enum

Describes the starting condition of a helix.

Value	Description
`START_ANGLE`	Start the helix at an angle around the origin of the base.
`START_POINT`	Start the helix at a point of choice along the plane of the base.

EndType enum

Describes the ending condition of a helix.

Value	Description
`HEIGHT`	End the helix at a specified height.
`END_POINT`	End the helix at a specified point along a perpendicular plane to the base.

Direction enum

Describes the direction a helix turns while traveling along its axis.

Value	Description
`CW`	Clockwise.
`CCW`	Counterclockwise.

helix (context is Context, id is Id, definition is map)

Feature performing an opHelix.

hole

HoleEndStyle enum

Defines the end bound for the hole cut.

Value	Description
`BLIND`	Cut holes to a specific depth.
`BLIND_IN_LAST`	Cut holes through all parts but the last, then cut to a specific depth in the last part.
`UP_TO_NEXT`
`UP_TO_ENTITY`
`THROUGH`	Cut holes with a through-all extrude.

HoleEndStyleV2 enum

Defines the end bound for the hole cut.

Value	Description
`BLIND`	Cut holes to a specific depth.
`UP_TO_NEXT`
`UP_TO_ENTITY`
`THROUGH`	Cut holes with a through-all extrude.

TipAngleStyle enum

Defines the tip angle style for the hole tip

Value	Description
`DEGREE118`	Tip angle is set at 118 degrees
`DEGREE135`	Tip angle is set at 135 degrees
`FLAT`	Tip angle is flat or 180 degrees
`CUSTOM`	User inputs specific angle value

HoleStartStyle enum

Defines the options to adjust hole position.

Value	Description
`PART`	Cut holes starting from the hole location.
`SKETCH`	Cut holes starting from the first full entrance.
`PLANE`	Cut holes starting at the selected input.

parsePitch (context is Context, pitch is string)

Parse and split the numerical and unit portion of a pitch string, e.g. "20 tpi"

buildPitchAnnotation (context is Context, pitch is string)

Parse a pitch string, e.g. "20 tpi" or "1.5 mm, and return its annotation suffix in imperial or metric format, e.g. -20 or x1.5

hole (context is Context, id is Id, definition is map)

Creates holes of specific dimensions and style, based either on standard hole size, or by user-defined values. Each hole's position and orientation are specified using sketch points.

CSINK_ANGLE_BOUNDS const

Angle bounds for a hole countersink.

computePitchValue (context is Context, pitch is string)

Extract value from pitch string

holeTable

holeTable const

Computes one hole table for each part

importDerived

DerivedPlacementType enum

Enum controlling the placement of derived entities in the target part studio.

Value	Description
`AT_ORIGIN`
`AT_MATE_CONNECTOR`

BuildFunction type

A special type for functions defined as the build function for a Part Studio, which return a context containing parts.

canBeBuildFunction (value) predicate

Typecheck for BuildFunction

importDerived (context is Context, id is Id, definition is map)

Feature using PartStudioData for including parts in one Part Studio that were designed in another.

Location query determines where in the current Part Studio the selections will be located. Bringing in multiple instances using multiple location queries is allowed but not recommended.

One can use the origin or a mate connector from the base Part Studio for placement in the current Part Studio.

importForeign

ForeignId type

A string representing a foreign element, such as the dataId from an imported tab.

canBeForeignId (value) predicate

Typecheck for ForeignId

importForeign (context is Context, id is Id, definition is map)

Feature performing an opImportForeign, transforming the result if necessary.

isocline

isocline (context is Context, id is Id, definition is map)

Creates curves or split faces in a given direction at a given degree.

isoparametricCurve

isoparametricCurve (context is Context, id is Id, definition is map)

Creates isoparametric curves on faces by using opCreateCurvesOnFace

linearPattern

linearPattern (context is Context, id is Id, definition is map)

Performs a body, face, or feature linear pattern. Internally, performs an applyPattern, which in turn performs an opPattern or, for a feature pattern, calls the feature function.

Parameter	Type	Additional Info
`definition`	`map`
`patternType`	`PatternType`	Optional Specifies a `PART`, `FEATURE`, or `FACE` pattern. Default is `PART`.
`entities`	`Query`	Required if `patternType` is `PART` The parts to pattern. EXAMPLE `qCreatedBy(id + "extrude1", EntityType.BODY)`
`faces`	`Query`	Required if `patternType` is `FACE` The faces to pattern.
`instanceFunction`	`FeatureList`	Required if `patternType` is `FEATURE` The `FeatureList` of the features to pattern.
`directionOne`	`Query`	The direction of the pattern. EXAMPLE `qCreatedBy(newId() + "Right", EntityType.FACE)`
`distance`	`ValueWithUnits`	The distance between each pattern entity. EXAMPLE `1.0 * inch` to space the pattern entities 1 inch apart.
`instanceCount`	`number`	The resulting number of pattern entities, unless `isCentered` is `true`. EXAMPLE `2` to have 2 resulting pattern entities (including the seed).
`oppositeDirection`	`boolean`	Optional EXAMPLE `true` to switch the direction of the pattern along `directionOne`.
`isCentered`	`boolean`	Optional Whether to center the pattern on the seed. When set to `true`, `instanceCount - 1` pattern entities are created along each direction of `directionOne`. Default is `false`.
`hasSecondDir`	`boolean`	Optional EXAMPLE `true` if the pattern should extend in two directions rather than one, creating a grid of pattern entities.
`directionTwo`	`Query`	Required if `hasSecondDir` is `true` The second direction of the pattern.
`distanceTwo`	`ValueWithUnits`	Required if `hasSecondDir` is `true` The distance between each pattern entity in the second direction.
`instanceCountTwo`	`number`	Required if `hasSecondDir` is `true` The resulting number of pattern entities in the second direction, unless `isCentered` is `true`.
`oppositeDirectionTwo`	`boolean`	Optional EXAMPLE `true` to switch the direction of the pattern along `directionTwo`.
`isCenteredTwo`	`boolean`	Optional Whether to center the second direction of the pattern on the seed. When set to `true`, `instanceCount - 1` pattern entities are created along each direction of `directionTwo`. Default is `false`.
`operationType`	`NewBodyOperationType`	Optional Specifies how the newly created body will be merged with existing bodies.
`defaultScope`	`boolean`	Optional EXAMPLE `true` to merge with all other bodies EXAMPLE `false` to merge with `booleanScope`
`booleanScope`	`Query`	Required if `defaultScope` is `false` The specified bodies to merge with.
`skipInstances`	`boolean`	Optional Whether to exclude certain instances of the pattern.
`skippedInstances`	`array`	Required if `skipInstances` is `true` Which instances of the pattern to skip. Each is denoted by one index for each direction, either of which may be negative if `isCentered` or `isCenteredTwo` respectively is `true`. EXAMPLE `[{ index1: -3, index2: 1 }, { index1: 0, index2: -2 }, { index1: 5, index2: 0 }]`

loft

LoftEndDerivativeType enum

Specifies an end condition for one side of a loft.

Value	Description
`DEFAULT`
`NORMAL_TO_PROFILE`
`TANGENT_TO_PROFILE`
`MATCH_TANGENT`
`MATCH_CURVATURE`
`NORMAL_DIRECTION`
`TANGENT_DIRECTION`

LoftGuideDerivativeType enum

Specifies derivative condition for a guide

Value	Description
`DEFAULT`
`NORMAL_TO_GUIDE`
`TANGENT_TO_GUIDE`
`MATCH_TANGENT`
`MATCH_CURVATURE`

loft (context is Context, id is Id, definition is map)

Feature performing an opLoft.

mateConnector

mateConnector (context is Context, id is Id, definition is map)

Feature performing an opMateConnector.

The parameters below are designed for interactive use in the feature dialog. In FeatureScript, it is preferred to calculate the resulting coordinate system directly, and pass this coordinate system to opMateConnector.

Parameter	Type	Additional Info
`definition`	`map`
`originQuery`	`Query`	The entity on which to place the mate connector EXAMPLE `qFarthestAlong(qCreatedBy(id + "extrude1", EntityType.VERTEX), vector(1, 1, 1))`
`entityInferenceType`	`EntityInferenceType`	A method of producing the coordinate system EXAMPLE `EntityInferenceType.POINT` to place on a vertex, with the world coordinate system EXAMPLE `EntityInferenceType.MID_POINT` to place at the midpoint of an edge, with the Z axis along the edge
`secondaryOriginQuery`	`query`	Optional Additional entity to inference with, used in some inference types.
`originType`	`OriginCreationType`	Optional EXAMPLE `OriginCreationType.BETWEEN_ENTITIES` to place mate connector origin on the midpoint between the speicified origin and the location of `originAdditionalQuery`. Default is `OriginCreationType.ON_ENTITY`.
`originAdditionalQuery`	`Query`	Required if `originType` is `OriginCreationType.BETWEEN_ENTITIES`
`flipPrimary`	`boolean`	Optional EXAMPLE `true` to flip the resulting Z axis
`secondaryAxisType`	`MateConnectorAxisType`	Optional Changes which axis (perpendicular to Z) will point along the secondary direction. Default is `MateConnectorAxisType.PLUS_X`
`realign`	`boolean`	Optional `true` to change direction of axes
`primaryAxisQuery`	`Query`	Required if `realign` is `true` Entity with axis to define the resulting Z direction
`secondaryAxisQuery`	`Query`	Required if `realign` is `true` Entity with axis to define the secondary axis (set by `secondaryAxisType`)
`transform`	`boolean`	Optional Whether to change the origin position with `translationX`, `translationY`, and `translationZ`. The X/Y/Z directions of this translation are affected by `primaryAxisQuery` and `secondaryAxisQuery` and `secondaryAxisType`, but not by `rotationType` and `rotation`
`translationX`	`ValueWithUnits`	Required if `transform` is `true` Distance to move the resulting origin along resulting X direction.
`translationY`	`ValueWithUnits`	Required if `transform` is `true` Distance to move the resulting origin along resulting Y direction
`translationZ`	`ValueWithUnits`	Required if `transform` is `true` Distance to move the resulting origin along resulting Z direction
`rotationType`	`RotationType`	Optional Axis to rotate around (does not change origin position)
`rotation`	`ValueWithUnits`	Optional Angle to rotate
`requireOwnerPart`	`boolean`	Optional Whether to error if owner part is not provided. Default is `true`. If `false`, the mate connector may be an independent body with no owner part.
`ownerPart`	`Query`	Required if `requireOwnerPart` is not `false` Part on which to attach the resulting mate connector
`specifyNormal`	`boolean`	Optional EXAMPLE `true` override the Z direction with the known vector `(definition.nx, definition.ny, definition.nz)`. Used internally when the mate connector is placed on a mesh.
`nx`	`number`	Required if `specifyNormal` is `true`
`ny`	`number`	Required if `specifyNormal` is `true`
`nz`	`number`	Required if `specifyNormal` is `true`

mirror

mirror (context is Context, id is Id, definition is map)

Feature creating a single copy of some features, bodies, or faces, mirrored about a given entity. Internally, performs an applyPattern, which in turn performs an opPattern or, for a feature mirror, calls the feature function.

modifyFillet

ModifyFilletType enum

Defines the action of a modifyFillet feature.

Value	Description
`CHANGE_RADIUS`
`REMOVE_FILLET`

modifyFillet (context is Context, id is Id, definition is map)

Feature performing an opModifyFillet.

moveCurveBoundary

trimCurve (context is Context, id is Id, definition is map)

Extend or trim a curve. This is a thin wrapper around opMoveCurveBoundary.

moveFace

moveFace (context is Context, id is Id, definition is map)

Feature performing an opMoveFace.

deripEdges (context is Context, id is Id, edges is Query) returns boolean

Splits input sheet metal edges and adjusts them to lie on corresponding sheet metal part faces.

mutualTrim

mutualTrim (context is Context, id is Id, definition is map)

Trim two adjacent surfaces by extending intersections to complete the trim.

offsetCurveOnFace

OffsetCurveScope enum

Drives the extend and imprint booleans in opOffsetCurveOnFace.

Value	Description
`OFFSET`
`OFFSET_AND_EXTEND`
`OFFSET_EXTEND_AND_SPLIT`

GapFill enum

Whether to use linear or rounded extensions to connect discontinuities within offset wires.

Value	Description
`LINEAR`
`ROUND`

offsetCurveOnFace (context is Context, id is Id, definition is map)

Feature performing an offset curve.

offsetSurface

offsetSurface (context is Context, id is Id, definition is map)

Feature performing an opExtractSurface. Allows creation of an offset surface from faces, surfaces, or sketch regions. Offset may be zero. Offset direction may be flipped using the oppositeDirection flag.

projectCurves

CurveProjectionType enum

Specifies the method used for generating intersection curves.

Value	Description
`TWO_SKETCHES`	Performs `opExtrude` to convert sketches into surface, then uses `opBoolean` to intersect those surfaces.
`CURVE_TO_FACE`	Performs `opDropCurve` to project curves onto faces.

projectCurves (context is Context, id is Id, definition is map)

Feature creating projected curves.

Parameter	Type	Additional Info
`definition`	`map`
`curveProjectionType`	`CurveProjectionType`	Optional The method used for generating intersection curves. Default is `TWO_SKETCHES`.
`sketchEdges1`	`Query`	Required if `curveProjectionType` is `TWO_SKETCHES` Edges from a single sketch that will be extruded to perform an intersection.
`sketchEdges2`	`Query`	Required if `curveProjectionType` is `TWO_SKETCHES` Edges from a single sketch that will be extruded to perform an intersection.
`dropTools`	`Query`	Required if `curveProjectionType` is `CURVE_TO_FACE` Edges that will be projected onto `targets`.
`projectionType`	`ProjectionType`	Required if `curveProjectionType` is `CURVE_TO_FACE` Specifies whether to project along a direction or the face normal of `targets`.
`directionQuery`	`Query`	Required if `projectionType` is `DIRECTION` Specifies the direction of projection.
`oppositeDirection`	`boolean`	Required if `projectionType` is `DIRECTION` If true, negates the direction supplied by `directionQuery`.
`targets`	`Query`	Required if `curveProjectionType` is `CURVE_TO_FACE` Faces, sheet bodies, or solid bodies to project onto.

replaceFace

replaceFace (context is Context, id is Id, definition is map)

Feature performing an opReplaceFace.

revolve

RevolveType enum

Specifies how a revolve's end condition should be defined.

Value	Description
`FULL`
`ONE_DIRECTION`
`SYMMETRIC`
`TWO_DIRECTIONS`

revolve (context is Context, id is Id, definition is map)

Feature performing an opRevolve, followed by an opBoolean. For simple revolves, prefer using opRevolve directly.

rib

RibExtrusionDirection enum

Specifies the direction of the rib extrusion starting from the profile going up to the part.

Value	Description
`PARALLEL_TO_SKETCH_PLANE`	The direction of the rib extrusion goes parallel to the profile sketch plane.
`NORMAL_TO_SKETCH_PLANE`	The direction of the rib extrusion goes normal to the profile sketch plane.

rib (context is Context, id is Id, definition is map)

Creates ribs from selected profiles. The ribs can be either free standing or merged with their mating part. Profiles must be non-construction sketch edges.

Parameter	Type	Additional Info
`definition`	`map`
`profiles`	`Query`	Edges which form the center lines of the ribs.
`parts`	`Query`	Parts which form the boundary of the ribs.
`thickness`	`ValueWithUnits`	Thickness of the ribs.
`ribExtrusionDirection`	`RibExtrusionDirection`	Whether the rib is extruded perpendicular or parallel to the plane.
`oppositeDirection`	`boolean`	Whether the ribs are extruded in the positive or negative direction.
`hasDraft`	`boolean`	Optional EXAMPLE `true` to add a draft to the rib.
`draftAngle`	`ValueWithUnits`	Required if `hasDraft` is `true` The angle of the draft with respect to the extruded direction of the rib. EXAMPLE `10 * degree`
`draftPullDirection`	`boolean`	Optional EXAMPLE `false` to draft outwards (default) EXAMPLE `true` to draft inwards
`extendProfilesUpToPart`	`boolean`	Whether the ribs are extruded up to a boundary part.
`mergeRibs`	`boolean`	Whether the ribs are merged with the mating part.

ruledSurface

VertexOverrideType enum

The type of ruled surface to apply at a specific vertex.

Value	Description
`NORMAL`
`TANGENT`
`ALIGNED_WITH_VECTOR`
`UP_TO_VERTEX`

RuledSurfaceInterfaceType enum

The type of ruled surface to apply for the overall operation.

Value	Description
`NORMAL`
`TANGENT`
`ALIGNED_WITH_VECTOR`
`ANGLE_FROM_VECTOR`

ruledSurface (context is Context, id is Id, definition is map)

Feature creating a ruled surface.

sheetMetalAttribute

Modules prefixed with "sheetMetal" here and below control functionality related to working with sheet metal models in Onshape.

Sheet metal models are created with the sheetMetalStart feature. The geometry of these models is not modifiable with ordinary geometry operations, and an operation which attempts to modify a sheet metal model will always throw the error ErrorStringEnum.SHEET_METAL_PARTS_PROHIBITED

Onshape's sheet metal operations are instead encapsulated in features defined with defineSheetMetalFeature. These features directly modify the underlying sheet metal master body, a hidden surface body not accessible from other features. The master body (along with SMAttributes set on its entities) provides the information necessary for updateSheetMetalGeometry to build both sheet metal bodies: the 3D folded body and the flat pattern. The result is simultaneous sheet metal editing, where geometry and errors are always available to the end user on both the folded and the flat sheet metal models.

Most custom features will function only on bodies which are not active sheet metal, because the feature's effects are not readily translatable from the folded model back to the flattened master model. A custom feature's user will typically discover this when an operation within the custom feature throws a SHEET_METAL_PARTS_PROHIBITED error, giving the user-facing message "Active sheet metal models are not allowed."

Additionally, a custom feature's query parameter can disallow selection of entities from sheet metal bodies using the ActiveSheetMetal.NO filter. Any other query can be filtered for non-sheet-metal geometry using separateSheetMetalQueries.

SMAttribute type

Sheet metal object definition attribute type.

canBeSMAttribute (value) predicate

parameters in SMAttribute (e.g. radius in BEND, angle in JOINT, thickness in MODEL) are specified as maps

EXAMPLE

{
 value : {ValueWithUnits},
 canBeEdited : {boolean},
 controllingFeatureId : {string}, : feature to be edited when editing this parameter
 parameterIdInFeature : {string}
 }

smAttributeDefault const

Empty map as SMAttribute convenient for attribute lookup

asSMAttribute (value is map) returns SMAttribute

Attach SMAttribute type to a map. convenient for attribute lookup and queries.

makeSMJointAttribute (attributeId is string) returns SMAttribute

Start SMAttribute for joint.

makeSMWallAttribute (attributeId is string) returns SMAttribute

Start SMAttribute for wall.

makeSMCornerAttribute (attributeId is string) returns SMAttribute

Start SMAttribute for corner.

getSmObjectTypeAttributes (context is Context, topology is Query, objectType is SMObjectType) returns array

Get attributes with matching objectType.

clearSmAttributes (context is Context, entities is Query)

Clear SM attributes from entities.

hasSheetMetalAttribute (context is Context, entities is Query, objectType is SMObjectType) returns boolean

Check for presence of SMAttribute types.

replaceSMAttribute (context is Context, existingAttribute is SMAttribute, newAttribute is SMAttribute) returns Query

For all entities annotated with attribute matching existingAttribute pattern, replace it with newAttribute. Return query for entities whose attributes have been modified.

getSMDefinitionEntities (context is Context, selection is Query) returns array

Find sheet metal master body entities corresponding to feature input.

getSMDefinitionEntities (context is Context, selection is Query, entityType is EntityType) returns array

isSheetMetalModelActive (context is Context, sheetMetalModel is Query) returns boolean

Check if sheet metal model is active.

areEntitiesFromSingleSheetMetalModel (context is Context, entities is Query) returns map

Check if all entities belong to the same sheet metal model

areEntitiesFromSingleActiveSheetMetalModel (context is Context, entities is Query) returns boolean

Check if all entities belong to the same active sheet metal model

getWallAttribute (context is Context, wallFace is Query)

Get wall attribute on a single entity

getJointAttribute (context is Context, jointEdge is Query)

Get joint attribute on a single entity

getCornerAttribute (context is Context, cornerVertex is Query)

Get corner attribute on a single entity

SMAssociationAttribute type

Used by sheet metal features to maintain correspondence between master sheet body entities and folded and flat solid body entities.

canBeSMAssociationAttribute (value) predicate

Association attribute stores attributeId. The association is established by assigning the same attribute to associated entities. Every entity in sheet metal master sheet body has a distinct association attribute.

makeSMAssociationAttribute (attributeId is string) returns SMAssociationAttribute

Create an association attribute with the given attributeId.

assignSMAssociationAttributes (context is Context, entities is Query)

Assign new association attributes to entities using their transient queries to generate attribute ids.

smAssociationAttributePattern const

An attribute pattern for finding attributes which are SMAssociationAttributes.

getSMAssociationAttributes (context is Context, entities is Query)

Get all of the association attributes for a given set of entities.

SMCornerBreak type

Information corresponding to a single sheet metal corner break (fillet or chamfer)

canBeSMCornerBreak (value) predicate

Corner break must hold the break style, the range (radius and distance of fillet and chamfer respectively), and the wallId of the wall that owns the corner.

makeSMCornerBreak (cornerBreakStyle is SMCornerBreakStyle, range is ValueWithUnits, wallId is string) returns SMCornerBreak

Create a corner break

addCornerBreakToSMAttribute (attribute is SMAttribute, cornerBreakMap is map) returns SMAttribute

Adds an SMCornerBreak and any additional information to an SMAttribute, initializing the cornerBreaks array if necessary.

findCornerBreak (attribute is SMAttribute, wallId is string)

Finds an SMCornerBreak in attribute corresponding to wallId, returns undefined if nothing found

updateCornerAttribute (context is Context, vertex is Query, attribute is SMAttribute)

Clears existing SMAttribute, sets new one only if non-trivial

sanitizeControllingInformation (context is Context, attribute is SMAttribute, replaceExisting is boolean) returns SMAttribute

Removes all controllingFeatureId and parameterIdInFeature information from an SMAttribute. Replaces the provided attribute with sanitized attribute if replaceExisting is true. Return the sanitized attribute

Fail if the attribute is a model attribute as a safety precaution, as removing the controllingFeatureId information from a model attribute would invalidate it from being the same model attribute as it was before

sheetMetalBend

BendAlignment enum

Values specifying the alignment of sheet metal after it is bent, relative to the line

Value	Description
`BEND_LINE`
`HELD_EDGE`
`BENT_EDGE`
`BENT_INSIDE`
`BENT_OUTSIDE`
`BENT_MIDPLANE`

BendAngleControlType enum

Angle types for the bend

Value	Description
`BEND_ANGLE`
`ALIGN_GEOMETRY`
`ANGLE_FROM_DIRECTION`

sheetMetalBend (context is Context, id is Id, definition is map)

Bend a sheet metal model along a reference line, with additional bend control options.

sheetMetalBendRelief

sheetMetalBendRelief (context is Context, id is Id, definition is map)

Bend relief feature is used to override default bend relief of sheet metal model at individual bend end.

sheetMetalCorner

sheetMetalCorner (context is Context, id is Id, definition is map)

Corner feature is used to override default sheet metal model corner relief style or dimensions for an individual corner

sheetMetalCornerBreak

EdgeBlendType enum

Specifies type of edge blend

Value	Description
`FILLET`
`CHAMFER`

sheetMetalCornerBreak (context is Context, id is Id, definition is map)

Sheet metal specific feature combining functionality of edge fillet and chamfer. It calls SMEdgeBlendImpl to apply fillets or chamfers in flat and then change the definition surface accordingly As a result of this change rips corner/bend reliefs are also "baked" into the definition surface and flexibility of sheet metal model is lost. For this reason we recommend that this feature is used after sheet metal flanges, joints and reliefs are finalized.

sheetMetalEnd

sheetMetalEnd (context is Context, id is Id, definition is map)

Deactivate the sheet metal model of selected parts. Continued modeling on deactivated sheet metal parts will not be represented in the flat pattern or the table.

sheetMetalFlange

SMFlangeAlignment enum

Describes the position of a virtual sharp with respect to "flange face", defined as the face that corresponds to the edge selected for flange in the underlying sheet.

For Middle alignment, the virtual sharp at the intersection of the existing sheet and the sheet that corresponds to the flange wall, lies in the middle of the flange face.

For Inner alignment, the virtual sharp at the intersection of the planes defined by the faces of the solid to the interior of the bend, lies coincident with the edge of the flange face closest to the bend.

For Outer alignment, the virtual sharp at the intersection of the planes defined by the faces of the solid to the exterior of the bend, lies coincident with the edge of the flange face farthest from the bend.

Value	Description
`INNER`
`OUTER`
`MIDDLE`
`BEND`

SMPartialFlangeChainType enum

Sets the handling for chains of edges while creating a partial flange.

Value	Description
`PER_EDGE`	The partial flange conditions will be applied to the ends of each individual edge.
`PER_CHAIN`	The partial flange conditions will be applied to the ends of each chain of selected edges.

sheetMetalFlange (context is Context, id is Id, definition is map)

Create sheet metal flanges on selected edges of sheet metal parts. Length of flange may be defined by distance (as measured from the virtual sharp along outer edge of wall) or limiting entity. Bend angle may be flipped using the oppositeDirection flag. When auto-miter is not selected, flange sides are rotated by miter angle.

sheetMetalInFlat

SMFlatOp (context is Context, id is Id, definition is map)

Adds or removes material of sheet metal part as specified by faces attached to its its flat pattern Is the implementation of sheet metal extrude in flat.

Parameter	Type	Additional Info
`definition`	`map`
`faces`	`Query`	Faces associated with sheet metal flat, typically sketch faces or region of sketch in flat
`flatOperationType`	`FlatOperationType`

SMEdgeBlendImpl (context is Context, id is Id, definition is map)

Applies a requested feature in sheet metal flat, changes definition surfaces to reflect this and updates sheet metal geometry Used by fillet and chamfer

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	Sheet metal edges or vertices (flat selections are allowed) associated with vertices in definition
`crossSection`	`FilletCrossSection`
`chamferType`	`ChamferType`	Required if `crossSection` is `CHAMFER`
`width`	`ValueWithUnits`	Required if `chamferType` is `EQUAL_OFFSETS` or `OFFSET_ANGLE`.
`width1`	`ValueWithUnits`	Required if `chamferType` is `TWO_OFFSETS`.
`width2`	`ValueWithUnits`	Required if `chamferType` is `TWO_OFFSETS`.
`angle`	`ValueWithUnits`	Required if `chamferType` is `OFFSET_ANGLE`.
`oppositeDirection`	`boolean`	Optional
`radius`	`ValueWithUnits`	Required if `crossSection` is `CIRCULAR` or `CONIC` or `CURVATURE`.
`isAsymmetric`	`boolean`	Optional
`flipAsymmetric`	`boolean`	Optional
`otherRadius`	`ValueWithUnits`	Required if `isAsymmetric` is true.
`rho`	`number`	Required if `crossSection` is `CONIC`.
`magnitude`	`number`	Required if `crossSection` is `CURVATURE`.

sheetMetalJoint

sheetMetalJoint (context is Context, id is Id, definition is map)

sheetMetalJoint feature modifies sheet metal joint by changing its attribute.

sheetMetalMakeJoint

MakeJointType enum

MakeJointType is a subset of SMJointType to restrict options visible in sheetMetalMakeJoint

Value	Description
`BEND`
`RIP`

sheetMetalMakeJoint (context is Context, id is Id, definition is map)

Produces a sheet metal joint of type RIP or BEND by extending or trimming walls of selected edges. Rip is created as an edge joint by default.

sheetMetalStart

SMProcessType enum

Method of initializing sheet metal model

Value	Description
`CONVERT`
`EXTRUDE`
`THICKEN`

SMCornerStrategyType enum

Default corner relief style setting

Value	Description
`SIZED_RECTANGLE`
`RECTANGLE`
`SIZED_ROUND`
`ROUND`
`CLOSED`
`SIMPLE`

SMBendStrategyType enum

Default bend relief style setting

Value	Description
`RECTANGLE`
`OBROUND`
`TEAR`

SMBendCalculationType enum

Bend calculation setting

Value	Description
`K_FACTOR`
`BEND_ALLOWANCE`
`BEND_DEDUCTION`

CORNER_RELIEF_SCALE_BOUNDS const

Corner relief scale bounds

BEND_RELIEF_DEPTH_SCALE_BOUNDS const

Bend relief depth scale bounds

BEND_RELIEF_WIDTH_SCALE_BOUNDS const

Bend relief width scale bounds

FLIP_DIRECTION_UP_MANIPULATOR_NAME const

Manipulator name for the "flip direction up" manipulator

sheetMetalStart (context is Context, id is Id, definition is map)

Create and activate a sheet metal model by converting existing parts, extruding sketch curves or thickening. All operations on an active sheet metal model will automatically be represented in the flat pattern and the table. Sheet metal models may consist of multiple parts. Multiple sheet metal models can be active.

sheetMetalTab

sheetMetalTab (context is Context, id is Id, definition is map)

Feature adding tabs to parallel sheet metal faces.

sheetMetalUtils

defineSheetMetalFeature (feature is function, defaults is map) returns function

Exposes sheet metal definition sheet body to the queries within feature.

updateSheetMetalGeometry (context is Context, id is Id, args is map)

Based on current state of sheet metal definition sheet body update solid bodies

Parameter	Type	Additional Info
`args`	`map`
`entities`	`Query`	sheet metal definition entities changed (or attributes changed) in this feature
`deletedAttributes`	`array`	associated attributes of deleted sheet metal definition entities
`associatedChanges`	`Query`	sheet metal definition entities representing the change of this feature

SMThicknessDirection enum

Direction of material from definition body. For old models (before V629_SM_MODEL_FRONT_N_BACK) It is BOTH, for new models FRONT/BACK depends on oppositeDirection in sheetMetalStart

Value	Description
`BOTH`
`FRONT`
`BACK`

setCylindricalBendAttribute (context is Context, face is Query, frontThickness is ValueWithUnits, backThickness is ValueWithUnits, attributeId is string)

Set a bend attribute on a cylindrical face

Parameter	Type	Additional Info
`face`	`Query`	face to set bend attribute on
`attributeId`	`string`	id of new bend attribute

annotateSmSurfaceBodies (context is Context, id is Id, args is map, objectCount is number) returns number

Assign SMAttributes to topology of sheet metal definition sheet body

Parameter	Type	Additional Info
`args`	`map`
`surfaceBodies`	`Query`
`bendEdgesAndFaces`	`Query`
`specialRadiiBends`	`array`	array of pairs "(edge, bendRadius)"
`defaultRadius`	`ValueWithUnits`	bend radius to be applied to edges in bendEdgesAndFaces
`controlsThickness`	`boolean`
`thickness`	`ValueWithUnits`
`defaultCornerReliefScale`	`number`
`defaultRoundReliefDiameter`	`ValueWithUnits`
`defaultSquareReliefWidth`	`ValueWithUnits`
`defaultBendReliefScale`	`number`

K_FACTOR_BOUNDS const

A RealBoundSpec for sheet metal K-factor between 0. and 1., defaulting to .45.

ROLLED_K_FACTOR_BOUNDS const

A RealBoundSpec for rolled sheet metal K-factor between 0. and 1., defaulting to .5.

SM_MINIMAL_CLEARANCE_BOUNDS const

A LengthBoundSpec for minimal clearance of sheet metal rips

SM_BEND_RADIUS_BOUNDS const

A LengthBoundSpec for bend radius in sheet metal features

SM_THICKNESS_BOUNDS const

A LengthBoundSpec for thickness in sheet metal features. default to (1/16)" (i.e. steel)

SM_RELIEF_SIZE_BOUNDS const

A LengthBoundSpec for relief size, corners or bend relief, in sheet metal features.

partitionSheetMetalParts (context is Context, allParts is Query)

Partitions allParts into non-sheet metal parts and sheet metal parts. To preserve existing behavior of code the returned non-sm query is exactly the same as what is passed in for non-sm cases and a query is returned for them. The sheet metal results will usually be iterated through and so are returned as a map with the keys being the sheet metal ID and the values being the parts associated with that model.

See also

separateSheetMetalQueries

getActiveSheetMetalId (context is Context, query is Query)

Get the first id of active sheet metal model the entities of query belong to.

getModelParameters (context is Context, model is Query) returns map

Extract sheet metal model parameters in a convenient form

separateSheetMetalQueries (context is Context, targets is Query) returns map

Separates queries which are part of an active sheet metal model (either in the folded model or the flat pattern).

See also

partitionSheetMetalParts

Return	Type	Description
	`map`
`sheetMetalQueries`	`Query`	`targets` which are part of an active sheet metal model
`nonSheetMetalQueries`	`Query`	`targets` which are not part of an active sheet metal model

sheetMetalExtendSheetBodyCall (context is Context, id is Id, definition is map)

Wrapper around opExtendSheetBody used in sheet metal operations to handle remapping of cornerBreak data

sheetMetalEdgeChangeCall (context is Context, id is Id, edges is Query, definition is map)

Wrapper around opEdgeChange used in sheet metal operations to handle remapping of cornerBreak data

getOwnerSMModel (context is Context, selection is Query) returns array

Returns an array of sm models associated with selection in a way that works outside of sheet metal features.

getSMCorrespondingInPart (context is Context, selection is Query, entityType is EntityType) returns Query

Returns a query for all sheet metal part entities of entityType related to the input sheet metal model entities.

collectCornerBreakTracking (context is Context, bodies is Query) returns map

Collect information before adding material which may merge sheet metal walls. The map returned by this function should be passed directly into remapCornerBreaks after making the desired geometry changes.

Only walls which have broken corners are tracked.

Return	Type	Description
	`map`
`wallIdToPersistentWall`	`map`	a map from wall id to a tracked query for the wall
`wallIdToVerticesWithBreaks`	`array`	a map from wall id to an array of tracked vertices which break the wall

remapCornerBreaks (context is Context, cornerBreakTracking is map)

Remap corner breaks on walls whose wall id has changed. Takes the output of collectCornerBreakTracking as cornerBreakTracking.

getSelectionsForSMDefinitionEntities (context is Context, definitionEntities is Query, originalSelections is Query)

Map a group of sheet metal definition entities back to the original entities selected by the user.

separateByModelVersion (context is Context, targets is Query, version is FeatureScriptVersionNumber) returns map

Separates queries which are part of an active sheet metal model (either in the folded model or the flat pattern) with additional separation of active sheet metal queries based on feature script version of the coresponding sheet metal model.

See also

separateSheetMetalQueries

Return	Type	Description
	`map`
`sheetMetalQueries`	`Query`	`targets` which are part of an active sheet metal model
`nonSheetMetalQueries`	`Query`	`targets` which are not part of an active sheet metal model
`legacyModelQueries`	`Query`	`targets` which are part of an active sheet metal model with fsVersion earlier than `version`
`newModelQueries`	`Query`	`targets` which are part of an active sheet metal model with fsVersion equal or later than `version`

shell

shell (context is Context, id is Id, definition is map)

Feature performing an opShell.

splitpart

SplitType enum

Defines whether a split should split whole parts, or just faces.

Value	Description
`PART`
`FACE`

splitPart (context is Context, id is Id, definition is map)

Feature performing an opSplitPart.

sweep

sweep (context is Context, id is Id, definition is map)

Feature performing an opSweep, followed by an opBoolean. For simple sweeps, prefer using opSweep directly.

tagProfile

tagProfile (context is Context, id is Id, definition is map)

Tag a frame profile with metadata. The metadata will be displayed in the cut list for frames derived from the tagged profile.

thicken

thicken (context is Context, id is Id, definition is map)

Feature performing an opThicken, followed by an opBoolean. For simple thickens, prefer using opThicken directly.

transformCopy

TransformType enum

Defines how a the transform for a transform feature should be specified. SCALE_UNIFORMLY actually also supports non-uniform scaling.

Value	Description
`TRANSLATION_ENTITY`
`TRANSLATION_DISTANCE`
`TRANSLATION_3D`
`TRANSFORM_MATE_CONNECTORS`
`ROTATION`
`COPY`
`SCALE_UNIFORMLY`

transform (context is Context, id is Id, definition is map)

Move and/or rotate bodies or mate connectors with a single Transform, constructed with input according to the selected TransformType.

Internally, performs an opTransform when not copying, and an opPattern when copying. For simple transforms, prefer calling opTransform or opPattern directly.

Parameter	Type	Additional Info
`definition`	`map`
`entities`	`Query`	The bodies or mate connectors to transform. An error is thrown if anything else is included. EXAMPLE `qCreatedBy(id + "extrude1", EntityType.BODY)`
`transformType`	`TransformType`	Defines how the transform type should be specified. EXAMPLE `TransformType.TRANSLATION_3D`
`dx`	`ValueWithUnits`	Required if `transformType` is `TransformType.TRANSLATION_3D` A value with length units specifying the distance to move in the world `x` direction. EXAMPLE `1 * inch`
`dy`	`ValueWithUnits`	Required if `transformType` is `TransformType.TRANSLATION_3D` A value with length units specifying the distance to move in the world `y` direction. EXAMPLE `1 * inch`
`dz`	`ValueWithUnits`	Required if `transformType` is `TransformType.TRANSLATION_3D` A value with length units specifying the distance to move in the world `z` direction. EXAMPLE `1 * inch`
`transformLine`	`Query`	Required if `transformType` is `TransformType.TRANSLATION_ENTITY` A `Query` for either a single line or a pair of points, specifying the direction and distance to transform.
`oppositeDirectionEntity`	`boolean`	Required if `transformType` is `TransformType.TRANSLATION_ENTITY` EXAMPLE `true` to flip the transform direction.
`transformAxis`	`Query`	Required if `transformType` is `TransformType.ROTATION` A `Query` for a line, cylinder, etc. to specify the transform direction.
`angle`	`ValueWithUnits`	Required if `transformType` is `TransformType.ROTATION` A value with angle units specifying the angle to rotate.
`transformDirection`	`Query`	Required if `transformType` is `TransformType.TRANSLATION_DISTANCE` A `Query` for either a single line or a pair of points, specifying the direction to transform.
`distance`	`ValueWithUnits`	Required if `transformType` is `TransformType.TRANSLATION_DISTANCE` A value with length units specifying the distance to move.
`oppositeDirection`	`boolean`	Required if `transformType` is `TransformType.TRANSLATION_DISTANCE` or `TransformType.ROTATION` EXAMPLE `true` to transform in the opposite direction.
`uniform`	`boolean`	Optional True if the scale is uniform in all directions (default)
`scale`	`number`	Required if `transformType` is `TransformType.SCALE_UNIFORMLY` and `uniform` is true A positive real number specifying the scale factor.
`scalePoint`	`Query`	Required if `transformType` is `TransformType.SCALE_UNIFORMLY` A point specifying the center of the scale or a mate connector specifying the coordinate system for a non-uniform scale.
`scaleX`	`number`	Required if `transformType` is `TransformType.SCALE_UNIFORMLY` and `uniform` is false
`scaleY`	`number`	Required if `transformType` is `TransformType.SCALE_UNIFORMLY` and `uniform` is false
`scaleZ`	`number`	Required if `transformType` is `TransformType.SCALE_UNIFORMLY` and `uniform` is false
`baseConnector`	`Query`	Required if `transformType` is `TransformType.TRANSFORM_MATE_CONNECTORS` The mate connector to transform from.
`destinationConnector`	`Query`	Required if `transformType` is `TransformType.TRANSFORM_MATE_CONNECTORS` The mate connector to transform to.
`oppositeDirectionMateAxis`	`boolean`	Required if `transformType` is `TransformType.TRANSFORM_MATE_CONNECTORS`
`secondaryAxisType`	`MateConnectorAxisType`	Required if `transformType` is `TransformType.TRANSFORM_MATE_CONNECTORS`
`makeCopy`	`boolean`	Required if `transformType` is not `TransformType.COPY` EXAMPLE `true` to keep the original bodies.

copyPart (context is Context, id is Id, definition is map)

Deprecated: Use opPattern, or the transform feature instead.

variable

VariableMode enum

Whether the variable is measured or assigned.

Value	Description
`ASSIGNED`
`MEASURED`

VariableMeasurementMode enum

Whether to measure distance or length.

Value	Description
`DISTANCE`
`LENGTH`
`DIAMETER`

AxisWithCustom enum

Axis selection

Value	Description
`DISTANCE`
`X`
`Y`
`Z`
`CUSTOM`

VariableMinMaxSelection enum

Min or max selection

Value	Description
`MINIMUM`
`MAXIMUM`

assignVariable (context is Context, id is Id, definition is map)

Feature performing a setVariable allowing a user to assign a FeatureScript value to a context variable. This variable may be retrieved within a feature by calling getVariable, or in a Part Studio using # syntax (e.g. #foo) inside any parameter which allows an expression (including the value parameter of another variable!)

Parameter	Type	Additional Info
`definition`	`map`
`mode`	`VariableMode`	Whether the variable is measured or assigned.
`name`	`string`	Must be an identifier.
`description`	`string`	Description of the variable. Maximum length of 256 characters.
`variableType`	`VariableType`	The type of variable. If it is not ANY, the value is restricted to be a length, angle, or number and is passed through the `lengthValue`, `angleValue`, or `numberValue` field, respectively.
`lengthValue`	`ValueWithUnits`	Used if `variableType` is `LENGTH`.
`angleValue`	`ValueWithUnits`	Used if `variableType` is `ANGLE`.
`numberValue`	`number`	Used if `variableType` is `NUMBER`.
`anyValue`		Used if `variableType` is `ANY`. Can be any immutable FeatureScript value, including a length, an array, or a function.
`measurementMode`	`VariableMeasurementMode`	Whether to measure distance, length, or diameter.
`entityCouple`	`Query`	Query for distance mode, containing two entities to measure the distance between.
`minmax`	`VariableMinMaxSelection`	Whether to measure the minimum or maximum distance.
`axis`	`AxisWithCustom`	Axis to measure distance along.
`extendEntities`	`boolean`	Extend selected planes and lines out to infinity. Incompatible with maximum.
`measureFromAxis`	`boolean`	Measure from the axis of geometry with an axis, rather than from the edge. Incompatible with maximum.
`componentSelector`	`AxisWithCustom`	Select an axis to measure along.
`customDirection`	`Query`	If componentSelector is CUSTOM, a query containing geometry with a directon to measure along.
`lengthEntities`	`Query`	Query for length mode, containing entities to measure the length of.
`radius`	`boolean`	Whether to measure the radius rather than the diameter.
`diameterEntity`	`Query`	Query for diameter mode, containing an entity to measure the diameter of.

verifyVariableName (name is string, faultyParameter is string)

Throws an error if name is not a valid identifier.

makeLookupFunction (context is Context, id is Id) returns function

Make a function to look up variables from the given context. Used in generated part studio code.

measureDistance (context is Context, arg is map) returns map

Measure the distance between two entities.

Parameter	Type	Additional Info
`arg`	`map`
`entities`	`Query`	a query containing two entities to measure the distance between.
`measureFromAxis`	`boolean`	Optional measure from the axis of the selected geometry, if an axis is available. Incompatible with the `maximum` option. Defaults to `false`.
`customDirection`	`Query`	Optional measure the distance between two entities along a direction selected by this query.
`extendEntities`	`boolean`	Optional extend the entities out to infinity. Incompatible with the `maximum` option. Defaults to `false`.
`maximum`	`boolean`	Optional measure the maximum distance between the selected entities, instead of the minimum by default. Defaults to `false`.

selectDistanceComponent (distanceMap is map, componentSelector is AxisWithCustom)

Returns appropriate entry in distanceMap returned from measureDistance given the selected AxisWithCustom.

measureDiameter (context is Context, arg is map)

Measure the diameter (or radius) of the selected entity.

Parameter Type Additional Info

arg map

entity

Query

a query containing an entity of GeometryType.CIRCLE, GeometryType.ARC, GeometryType.CYLINDER, or GeometryType.SPHERE.

radius

boolean

Optional

measure the radius instead of the diameter. Defaults to false.

wrap

WrapResultType enum

Defines what type of output the Wrap feature should produce.

Value	Description
`SOLID`	The wrap operation will produce thickened solid bodies.
`SURFACE`	The wrap operation will produce surface bodies.
`IMPRINT`	The wrap operation will imprint edges onto the destination face.

wrap (context is Context, id is Id, definition is map)

Feature performing an opWrap.

enums

blendcontroltype

BlendControlType enum

Specifies the controlled quantitiy for fillet operation.

Value	Description
`RADIUS`
`WIDTH`

bodydraftconcaverepairtype

BodyDraftConcaveRepairType enum

Specifies how to repair miter at concave corners.

Value	Description
`NONE`
`RADIUS`
`MIX`

bodydraftcornertype

BodyDraftCornerType enum

Specifies how to fill the gap between adjacent tapered faces.

Value	Description
`EXTEND`
`PLANE`

bodydraftmatchfacetype

BodyDraftMatchFaceType enum

Specifies how to match drafted faces.

Value	Description
`TANGENT_TO_FACE`
`REFERENCE_EDGE`

bodydraftselectiontype

BodyDraftSelectionType enum

Specifies the topology type for body draft.

Value	Description
`PARTS`
`FACES`
`EDGES`

booleanoperationtype

BooleanOperationType enum

See opBoolean.

Value	Description
`UNION`
`SUBTRACTION`
`INTERSECTION`
`SUBTRACT_COMPLEMENT`

boundingtype

BoundingType enum

Specifies how an extrude should terminate.

Value	Description
`BLIND`	Extrude a specific distance.
`UP_TO_NEXT`	Extrude up to the next solid body or surface body in the context.
`UP_TO_SURFACE`	Extrude up to the specified face, construction plane, or surface body.
`UP_TO_BODY`	Extrude up to the specified solid body.
`UP_TO_VERTEX`	Extrude up to the specified vertex.
`THROUGH_ALL`	Extrude an unspecified distance, guaranteed to be further in the extrude direction than any other solid or surface in the context.
`UP_TO_FACE`

chamfermethod

ChamferMethod enum

See opChamfer.

Value	Description
`FACE_OFFSET`
`APEX_RANGE`

chamfertype

ChamferType enum

See opChamfer.

Value	Description
`EQUAL_OFFSETS`
`TWO_OFFSETS`
`OFFSET_ANGLE`
`RAW_OFFSET`

clashtype

ClashType enum

Specifies the class of intersection between two bodies. *

See also

evCollision

Value	Description
`NONE`	No intersection.
`INTERFERE`	Bounding topologies interfere.
`EXISTS`	Vertex or edge intersection.
`ABUT_NO_CLASS`	Bounding topologies abut.
`ABUT_TOOL_IN_TARGET`	Bounding tool abuts bounding target on inside.
`ABUT_TOOL_OUT_TARGET`	Bounding tool abuts bounding target on outside.
`TARGET_IN_TOOL`	Target completely inside tool.
`TOOL_IN_TARGET`	Tool completely inside target.

constrainttype

ConstraintType enum

Specifies a type of sketch constraint.

See also

skConstraint

Value	Description
`NONE`
`COINCIDENT`
`PARALLEL`
`VERTICAL`
`HORIZONTAL`
`PERPENDICULAR`
`CONCENTRIC`
`MIRROR`
`MIDPOINT`
`TANGENT`
`EQUAL`
`LENGTH`
`DISTANCE`
`ANGLE`
`RADIUS`
`NORMAL`
`FIX`
`PROJECTED`
`OFFSET`
`CIRCULAR_PATTERN`
`PIERCE`
`LINEAR_PATTERN`
`MAJOR_DIAMETER`
`MINOR_DIAMETER`
`QUADRANT`
`DIAMETER`
`SILHOUETTED`
`CENTERLINE_DIMENSION`
`INTERSECTED`
`RHO`
`EQUAL_CURVATURE`
`BEZIER_DEGREE`
`FREEZE`

coordinatesysteminferenceselectionfilter

CoordinateSystemInferenceSelectionFilter enum

Specifies the filter type when requesting inference mate connectors.

Value	Description
`NONE`
`HOLE_GEOMETRY`

curveextensionendcondition

CurveExtensionEndCondition enum

Specifies the end condition for curve extension.

Value	Description
`BLIND`
`UP_TO_ENTITY`

curveextensionshape

CurveExtensionShape enum

Specifies the shape of curve extension.

Value	Description
`CURVATURE`
`TANGENT`

curvepatternorientationtype

CurvePatternOrientationType enum

Specifies the orientation type of patterned entities in curve pattern.

Value	Description
`DEFAULT`	Patterned entities will be reoriented tangent to curve (default orientation).
`LOCK_FACES`	Lock the orientation of patterned entities normal to a set of faces.
`KEEP_ORIENTATION`	Match the orientation of patterned entities with the seed entity orientation.

curvetype

CurveType enum

The subset of GeometryType which applies to 1-dimensional entities.

Value	Description
`CIRCLE`
`LINE`
`OTHER`
`ELLIPSE`
`SPLINE`

debugcolor

DebugColor enum

Color choices for the debug function

Value	Description
`RED`
`GREEN`
`BLUE`
`CYAN`
`MAGENTA`
`YELLOW`
`BLACK`
`ORANGE`

dimensionalignment

DimensionAlignment enum

Specifies how a constraint between lines or axes (such as parallel or coincident) should align the two constrained axes.

Value	Description
`UNSPECIFIED`
`ALIGNED`
`ANTI_ALIGNED`

drafttype

DraftType enum

Specifies the type of draft to execute.

Value	Description
`REFERENCE_ENTITY`	Draft faces holding a specific reference entity constant for each face.
`REFERENCE_SURFACE`	Draft faces relative to a single neutral surface.

edgeconvexitytype

EdgeConvexityType enum

Specifies how two faces join at a given edge. This is a function of the interior angle between the adjoining surfaces, measured inside the owner body.

Value	Description
`CONVEX`	The interior angle is less than 180 degrees along the whole edge.
`CONCAVE`	The interior angle is greater than 180 degrees along the whole edge.
`SMOOTH`	The interior angle is equal to 180 degrees along the whole edge.
`VARIABLE`	None of the above, i.e. the edge convexity varies along the edge.

edgetopology

EdgeTopology enum

Specifies the topology of an edge entity.

Can be used in a filter on a query parameter to only allow certain selections:

 annotation { "Name" : "Surface edges", "Filter" : EntityType.EDGE && EdgeTopology.ONE_SIDED } definition.edges is Query;

See also

qEdgeTopologyFilter

Value	Description
`WIRE`	edge without adjacent faces, belonging to a wire body.
`ONE_SIDED`	An edge adjacent to one face (e.g. the edge of a surface extrude).
`TWO_SIDED`	An edge which joins two faces (e.g. the edge of a cube).

entityinferencetype

EntityInferenceType enum

Specifies how a mate connector's coordinate system is defined with respect to an entity.

See also

mateConnector

Value	Description
`POINT`	Place a mate connector at a vertex with the world coordinate system, or at the tip of a conical face with its Z-axis along the cone axis.
`CENTROID`	Place a mate connector at the centroid of a face, with its Z-axis along the face normal at that point.
`CENTER`	Place a mate connector at the center of a circular or elliptical edge with its Z-axis along the normal of the plane which the edge lies on, or at the center of a sphere with the world coordinate system.
`MID_POINT`	Place a mate connector at the midpoint of an edge, with its Z-axis along the edge.
`TOP_AXIS_POINT`	Place a mate connector at the projection of the top extreme of a cylindrical or other revolved face onto the central axis of that face, with its Z-axis along the central axis.
`MID_AXIS_POINT`	Place a mate connector at the projection of the point midway betwen the top and bottom extremes of a cylindrical or other revolved face onto the central axis of that face, with its Z-axis along the central axis.
`BOTTOM_AXIS_POINT`	Place a mate connector at the projection of the bottom extreme of a cylindrical or other revolved face onto the central axis of that face, with
`LOOP_CENTER`	Place a mate connector at the center of a loop of planar edges, with its Z-axis along the normal of the plane. Only one edge of the loop needs to be selected for this inference.
`VIRTUAL_SHARP`	Place a mate connector at locations along a loop of planar edges where a single nonlinear edge sits between two nonparallel lines and is tangent to both. The mate origin will be the projected intersection of the two lines, with its Z-axis along the normal of the plane.

extendendtype

ExtendEndType enum

See opExtendSheetBody.

Value	Description
`EXTEND_BLIND`
`EXTEND_TO_TARGET`

extendsheetshapetype

ExtendSheetShapeType enum

See opExtendSheetBody.

Value	Description
`LINEAR`
`SOFT`

faceblendcrosssection

FaceBlendCrossSection enum

Specifies the type of cross section of the blend.

Value	Description
`ROLLING_BALL`
`SWEPT_PROFILE`

faceblendcrosssectionshape

FaceBlendCrossSectionShape enum

Specifies the cross sectional control for a fillet operation.

Value	Description
`CIRCULAR`
`CONIC`
`CURVATURE`
`CHAMFER`

faceblendpropagation

FaceBlendPropagation enum

Specifies the propagation type of the blend.

Value	Description
`TANGENT`
`ADJACENT`
`CUSTOM`

faceblendtrimtype

FaceBlendTrimType enum

Specifies how to trim the created blend.

Value	Description
`WALLS`
`SHORT`
`LONG`
`NO_TRIM`

facecurvecreationtype

FaceCurveCreationType enum

Specifies type of curve on face.

See also

opCreateCurvesOnFace

Value	Description
`DIR1_ISO`	Iso-parameter curves in primary direction
`DIR2_ISO`	Iso-parameter curves in secondary direction.
`DIR1_AUTO_SPACED_ISO`	Equally spaced iso-parameter curves in primary direction.
`DIR2_AUTO_SPACED_ISO`	Equally spaced iso-parameter curves in secondary direction.

faulttype

FaultType enum

Description of possible faults.

Value	Description
`NO_FAULT`
`CORRUPT_ENTITY`
`BODY_INVALID_IDENTIFIERS`
`BODY_INSIDE_OUT`
`EDGE_OPEN`
`EDGE_BAD_VERTEX`
`EDGE_REVERSED`
`VERTICES_TOUCH`
`WIRE_INTERSECT`
`ENTITY_INVALID`
`FACE_BAD_VERTEX`
`FACE_BAD_EDGE`
`FACE_INTERSECTS_EDGE`
`CHECKING_FAILED`
`FACE_FACE_INTERSECTION`
`SELF_INTERSECTION`
`ENTITY_NOT_G1`
`BOUNDING_BOX_VIOLATION`
`NO_GEOMETRY`
`UNDEFINED_FACE_SENSE`
`TOLERANCE_TOO_SMALL`
`EDGES_TOUCH`
`DEGENERATE_GEOMETRY`
`GENERAL_FAULT`

featuredimensiontype

FeatureDimensionType enum

Used to specify the type of a feature dimension, as in setDimensionedEntities.

Value	Description
`DISTANCE`
`ANGLE`
`RADIUS`
`DIAMETER`

filletcrosssection

FilletCrossSection enum

Specifies the cross sectional control for a fillet operation.

Value	Description
`CIRCULAR`
`CONIC`
`CURVATURE`
`CHAMFER`

fittolerancetables

getFitToleranceLimits (nominalSize is ValueWithUnits, standard is string, toleranceClass is string, isHoleBasis is boolean) returns map

Retrieves fit tolerance limits for a given nominal size, tolerance class, and basis.

Parameter	Type	Additional Info
`nominalSize`	`ValueWithUnits`	The nominal size with units for which the fit tolerance limits are required.
`standard`	`string`	The standard of the fit tolerance table ("ANSI" or "ISO").
`toleranceClass`	`string`	The tolerance class as a string.
`isHoleBasis`	`boolean`	Indicates whether the basis of the tolerance class is hole or shaft.

Return type	Description
`map`	A map containing the fit tolerance limits. Returns an empty map if no suitable tolerance limits are found.

fixedparameterposition

FixedParameterPosition enum

Specifies where a constraint should be resolved FIXED_AT_START or FIXED_AT_END will fix the constraint to coincide with the start or end of parametric curves. FIXED_ON_CURVE will fix the help point.

Value	Description
`FIXED_AT_START`
`FIXED_AT_END`
`FIXED_ON_CURVE`
`FREE`

geometriccontinuity

GeometricContinuity enum

Specifies the level of geometric continuity.

Value	Description
`G0`
`G1`
`G2`

holepositionreference

HolePositionReference enum

For a HoleProfile, a reference point along the hole axis to which the position of the profile is relative. To calculate these references, the cylinder of the hole is intersected with the targets of the hole. If the hole cylinder encounters a slanted or otherwise irregular face at the intersection with the target, the reference may by a range rather than a single point. Users may specify that they want the end of this range by using a holeProfile, or the beginning of this range by using a holeProfileBeforeReference; or they may control this behavior directly by setting the beforeReference flag of the HoleProfile.

Typically, the beginning of the reference range should be used for the first profile of the hole, and the end of the reference range should be used for the rest of the profiles of the hole. Using the beginning of the reference range for the first profile ensures that when the hole tool is cut from a target with a slanted or otherwise irregular entrance face, the first profile is far back enough to ensure that no undesirable overhang is left behind on the target, preventing the fastener from entering the hole. Using the end of the reference range for the rest of the profiles ensures that any nominal distances are measured from where the hole cylinder fully enters the part. As an example of both of these concepts, set the first two profiles of a HoleDefinition as a holeProfileBeforeReference referencing TARGET_START with a position of 0 inches, and a holeProfile referencing TARGET_START with a position of 2 inches, respectively. If this layout of profiles is used against a target that has a slanted entrance face, the first profile will be placed right where the cylinder first intersects the part, ensuring that there is no overhang when the hole tool is subtracted from the target. The second profile will be placed 2 inches from where the hole cylinder fully enters the target, such that the request for the hole to be 2 inches deep is understood as the hole having a full two inches of depth in the target, exluding the area where the hole is only partially cut into the target. Notably, to accomplish this the first and second profiles are placed more than two inches apart.

When calculating references, any intersection which is fully behind the origin of the axis Line (i.e. the axis point) is always ignored. Range intersections where the end of the range is ahead of the axis point but the start of the range is behind the axis point are not ignored.

Value	Description
`AXIS_POINT`	When calling `opHole`, the user will supply one or more `axes` defining where the holes are to be placed. When using this reference, the `position` of the profile will be in reference to the `origin` of the axis `Line` of the hole.
`TARGET_START`	When using this reference, the `position` of the profile will be in reference to the closest intersection of the hole cylinder with any target.
`LAST_TARGET_START`	For each target, find the first intersection of the hole cylinder into the target. When using this reference, the `position` of the profile will be in reference to the furthest of those intersections. Notably, this means that if certain targets are geometrically constructed such that the hole cylinder enters and exits the target multiple times, only the first of the entrances into the target is considered.
`LAST_TARGET_END`	When using this reference, the `position` of the profile will be in reference to the furthest exit of the hole cylinder from any target.
`UP_TO_ENTITY`
`UP_TO_NEXT`
`LAST_TARGET_START_IN_DEPTH`	For each target, find the first intersection of the hole cylinder into the target. When using this reference, the `position` of the profile will be in reference to the furthest of those intersections within the hole depth.

holeprofiletype

HoleProfileType enum

Describes how a HoleProfile is constructed in relation to its HolePositionReference.

Value	Description
`POSITIONED`	See `holeProfile`.
`MATCHED`	See `matchedHoleProfile`.

icon

Icon enum

Specifies an icon resource available in Onshape.

Value	Description
`X_LINEAR_LIMIT_MIN`	Minimum X linear limit.
`X_LINEAR_LIMIT_MAX`	Maximum X linear limit.
`Y_LINEAR_LIMIT_MIN`	Minimum Y linear limit.
`Y_LINEAR_LIMIT_MAX`	Maximum Y linear limit.
`Z_LINEAR_LIMIT_MIN`	Minimum Z linear limit.
`Z_LINEAR_LIMIT_MAX`	Maximum Z linear limit.
`X_ROTATION_LIMIT_MIN`	Minimum X rotation limit.
`X_ROTATION_LIMIT_MAX`	Maximum X rotation limit.
`Y_ROTATION_LIMIT_MIN`	Minimum Y rotation limit.
`Y_ROTATION_LIMIT_MAX`	Maximum Y rotation limit.
`Z_ROTATION_LIMIT_MIN`	Minimum Z rotation limit.
`Z_ROTATION_LIMIT_MAX`	Maximum Z rotation limit.
`CONE_ANGLE_LIMIT`	Cone angle limit.
`HOLE_DIAMETER`	Hole diameter.
`HOLE_DEPTH`	Hole depth.
`HOLE_DRILL_ANGLE`	Hole drill angle.
`HOLE_COUNTERBORE_DIAMETER`	Hole counterbore diameter.
`HOLE_COUNTERBORE_DEPTH`	Hole counterbore depth.
`HOLE_COUNTERSINK_DIAMETER`	Hole countersink diameter.
`HOLE_TAP_DIAMETER`	Hole tap diameter.
`HOLE_COUNTERSINK_ANGLE`	Hole countersink angle.
`HOLE_TAPPED_DEPTH`	Hole tapped depth.
`HOLE_TAP_CLEARANCE`	Hole tap clearance.
`ALONG_X`	Along the X-axis.
`ALONG_Y`	Along the Y-axis.
`ALONG_Z`	Along the Z-axis.
`DOF_TRANSLATION`	Degrees of freedom translation.
`DOF_ROTATION`	Degrees of freedom rotation.
`DIHEDRAL_LOW`	Dihedral low.
`DIHEDRAL_HIGH`	Dihedral high.

lofttopology

LoftTopology enum

Specifies topology option for opLoft.

Value	Description
`MINIMAL`	Minimal number of faces created.
`COLUMNS`	One face is created for each matching set of profile segments.
`GRID`	Faces created for COLUMNS option are split at each profile.

lookupTablePath

LookupTablePath type

A LookupTablePath identifies a map of keys into a multi-level table.

The fields on a LookupTablePath depend on its related LookupTable.

Value	Type	Description
`LookupTablePath`	`map`
`entityType`	`EntityType`	Optional

canBeLookupTablePath (value) predicate

Typecheck for LookupTablePath

lookupTablePath (source is map) returns LookupTablePath

Creates a lookupTablePath.

lookupTableEvaluate (expression is string) returns ValueWithUnits

Convert a table expression in string form into a ValueWithUnits.

Parameter Type Additional Info

expression

string

Currently the following forms are supported:

EXAMPLE

{number} <*> {units}

EXAMPLE

{number}/{number} <*> {units}

EXAMPLE

{number} <+> {number}/{number} <*> {units} Where {number} is <-><.>nnn> or <->inf

EXAMPLE

{} indicate an entity, <> indicate the contents are optional spaces between entities are optional unless they are required to separate entities.

lookupTableFixExpression (expression is string) returns string

insert plus sign and parenthesis as needed to make a valid expression

getLookupTable (table is map, path is LookupTablePath)

Find a terminal/content table from a path and convert into expression/value form

lookupTableGetValue (value) returns ValueWithUnits

Extract the value portion of expression/value maps or evaluate expressions. value maybe an expression or a value with units

isLookupTableViolated (definition is map, table is map) returns boolean

Test if the current definition violates the table.

manipulatorstyleenum

ManipulatorStyleEnum enum

Specifies the style of a manipulator intended to look unique.

See also

addManipulators

Value	Description
`DEFAULT`	the standard display of the manipulator. *
`SECONDARY`	the angular or linear manipulator has two arrow heads. *
`SIMPLE`	the display of the angular or linear manipulator is simpler. *
`TANGENTIAL`	the linear manipulator has two smaller arrows around a circular base.

manipulatortype

ManipulatorType enum

Specifies a specific type of interactive manipulator.

Value	Description
`LINEAR_1D`	A single arrow which can move along a single axis. See `extrude` for an example.
`LINEAR_3D`	A triad of perpendicular arrows which specify a 3D position. See `transformCopy` for an example.
`ANGULAR`	A curved arrow, with two radii, which can move along a circumference to specify an angle. See `revolve` for an example.
`FLIP`	A static arrow which can be clicked to toggle a flip direction. See `extrude` (with BoundingType.THROUGH_ALL) for an example.
`POINTS`	A series of points which can be selected one at a time.
`TOGGLE_POINTS`	A series of points which can each be selected individually.
`TRIAD_FULL`	A triad of perpendicular arrows, planar and angular manipulators.

mateconnectoraxistype

MateConnectorAxisType enum

Defines what direction the X-axis of a mate connector should face, relative to the reference defined. Thus, a mate connector defined with PLUS_Y will differ from the selected coordinate system by a 90-degree rotation about that coordinate system's Z-axis.

Value	Description
`PLUS_X`
`PLUS_Y`
`MINUS_X`
`MINUS_Y`

matedoftype

MateDOFType enum

Specifies a single degree of freedom of a mate.

Value	Description
`Tx`	Translation along the X axis.
`Ty`	Translation along the Y axis.
`Tz`	Translation along the Z axis.
`Rz`	Rotation around the Z axis.
`Ryp`	Rotation around the transformed Y axis from previous transform sequence.
`Rzp`	Rotation around the transformed z axis from previous transform sequence .

movecurveboundarytype

MoveCurveBoundaryType enum

Specifies whether to trim or extend the curve.

Value	Description
`TRIM`
`EXTEND`

offsetcurvetype

OffsetCurveType enum

Defines what kind of offset distance is used in offset curve on face.

Value	Description
`GEODESIC`	The distance is calculated along the faces of the body in which the selected edges lie in.
`EUCLIDEAN`	The distance is the distance in world coordinates.

origincreationtype

OriginCreationType enum

Specifies how a mate connector origin is defined, and how many entities define it.

Value	Description
`ON_ENTITY`
`BETWEEN_ENTITIES`

partstudioitemtype

PartStudioItemType enum

Enumeration of the types of items that can be selected inside a Part Studio reference parameter. By default this parameter allows selecting all of the item types below. It can be filtered by specifying a union of any number of PartStudioItemTypes (e.g. "Filter" : PartStudioItemType.SOLID || PartStudioItemType.ENTIRE_PART_STUDIO) in the parameter's annotation.

Value	Description
`SOLID`	A body with `BodyType.SOLID` (i.e. a part in the parts list)
`SURFACE`	A non-sketch body with `BodyType.SURFACE` (i.e. a surface in the parts list)
`WIRE`	A non-sketch body with `BodyType.WIRE` (i.e. a curve in the parts list)
`MESH`	An imported mesh (i.e. a mesh in the parts list)
`SKETCH`	An entire sketch feature (i.e. all `POINT`, `WIRE`, and `SURFACE` bodies created by the sketch)
`FLATTENED_SHEET_METAL`	A flattened sheet metal part (available from any Part Studio with sheet metal features)
`ENTIRE_PART_STUDIO`	The entire Part Studio. Setting this option allows clicking the top item (with the full Part Studio's tumbnail and name), which sets the `partQuery` to `qEverything(EntityType.BODY)`.
`CONSTRUCTION_PLANE`	A plane created with Plane feature or with `opPlane`
`COMPOSITE_PART`

profilecontrolmode

ProfileControlMode enum

Specifies how a profile should be controlled while sweeping.

Value	Description
`NONE`	No additional profile control.
`KEEP_ORIENTATION`	Keep the orientation constant.
`LOCK_FACES`	Lock the sweep operation to a set of faces.
`LOCK_DIRECTION`	Lock the sweep operation to a direction.:

projectiontype

ProjectionType enum

See opDropCurve.

Value	Description
`DIRECTION`
`NORMAL_TO_TARGET`

propertytype

PropertyType enum

Defines the type of property that is being applied to a part.

Value	Description
`NAME`
`MATERIAL`
`APPEARANCE`
`DESCRIPTION`
`PART_NUMBER`
`VENDOR`
`PROJECT`
`PRODUCT_LINE`
`TITLE_1`
`TITLE_2`
`TITLE_3`
`EXCLUDE_FROM_BOM`
`CUSTOM`	Requires a custom property id to specify fully.
`MASS_OVERRIDE`
`REVISION`

recordpatterntype

RecordPatternType enum

Allows differentiation of patterns in computed data

Value	Description
`NONE`
`LINEAR`
`CIRCULAR`
`CURVE`
`TRANSFORM`
`MIRROR`
`INSTANTIATED`

rotationtype

RotationType enum

Specifies an axis for rotation.

Value	Description
`ABOUT_X`
`ABOUT_Y`
`ABOUT_Z`

ruledsurfacecornertype

RuledSurfaceCornerType enum

Describes how a Ruled Surface creates corners.

Value	Description
`SPUN`	Conical corners are created by spinning an edge.
`EXTENDED`	Ruled surfaces are altered so that they meet at corners.
`LOFTED`	Curvature continuous lofts are created patching corners.
`NO_CORNER`	Leave corners open.

ruledsurfacetype

RuledSurfaceType enum

Describes how a Ruled Surface is defined.

Value	Description
`ANGLE_FROM_FACE`	Ruled surface is perpendicular to reference faces.
`ALIGNED_WITH_VECTOR`	Ruled surface is in direction of reference direction.
`ANGLE_FROM_VECTOR`	Ruled surface will meet a reference direction at an angle when viewed from the path tangent direction.

sectionpart

sectionPart (context is Context, id is Id, definition is map)

Feature creating a section of a part behind a plane. Internally, performs an opSplitPart followed by an opDeleteBodies.

Not exposed in the Part Studio UI.

planeSectionPart (context is Context, id is Id, definition is map)

Split a set of parts with a plane and delete all bodies in front of the face. Unlike sectionPart, bodies which are entirely behind the split plane are retained. Any bodies not included in the target query are deleted.

Parameter	Type	Additional Info
`definition`	`map`
`target`	`Query`	Bodies to be split.
`plane`	`Plane`	Plane that splits the bodies. Everything on the positive z side of the plane will be removed.

jogSectionPart (context is Context, id is Id, definition is map)

Split a part down a jogged section line and delete all back bodies. Used by drawings. Needs to be a feature so that drawings created by queries can resolve. Any bodies not included in the target query are deleted.

Parameter	Type	Additional Info
`definition`	`map`
`target`	`Query`	Bodies to be split.
`sketchPlane`	`Plane`	Plane that the jog line will be drawn in and extruded normal to. Everything on the positive x side of the jog line will be removed.
`jogPoints`	`array`	Points that the cutting line goes through in world coordinates.
`isPartialSection`	`boolean`	Whether or not it is a partial section cut.
`keepSketches`	`boolean`	Whether or not sketches will be kept in the section cut results.
`isBrokenOut`	`boolean`	Whether or not it is a broken-out section cut.
`isCropView`	`boolean`	Whether or not it is a crop section cut.
`brokenOutPointNumbers`	`array`	Array of the number of spline points of each broken-out section cut.
`brokenOutEndConditions`	`array`	Array of end conditions of each broken-out section cut.
`offsetPoints`	`array`	Array of points for offsetting the section lines.
`isAlignedSection`	`boolean`	Whether or not it is an aligned section cut.

sidegeometryrule

SideGeometryRule enum

See opThicken.

Value	Description
`REVOLVED`
`SUPPLIED`

smcornertype

SMCornerType enum

Specifies the type of corner at a vertex of a sheet metal model.

Value	Description
`OPEN_CORNER`	The corner has more than two bends or, when folded the edges of the metal do not meet.
`CLOSED_CORNER`	The corner has two bends and when folded the edge of the metal meet.
`BEND_END`	The 'corner' is the end of a bend and there may be bend relief.
`NOT_A_CORNER`	The vertex is not associated with a corner

splitoperationkeeptype

SplitOperationKeepType enum

See opSplitPart.

Value	Description
`KEEP_ALL`
`KEEP_FRONT`
`KEEP_BACK`

surfacetype

SurfaceType enum

The subset of GeometryType which applies to 2-dimensional entities

Value	Description
`PLANE`
`CYLINDER`
`CONE`
`SPHERE`
`TORUS`
`OTHER`
`REVOLVED`
`EXTRUDED`
`MESH`
`SPLINE`

tabletextalignment

TableTextAlignment enum

How text in a table column should be aligned

Value	Description
`LEFT`
`CENTER`
`RIGHT`

tessellatedloftreturnstatus

TessellatedLoftReturnStatus enum

Enumerates failure modes for tessellated loft.

Value	Description
`OK`	No error.
`CRISS_CROSSED_MATCHES`	At least two matches cross each other.
`UNDERNOURISHED_MATCHES`	At least one match consists of fewer than 2 match points.
`NON_CONSECUTIVE_MATCHES`	A match jumps across a profile without specifying a match point.
`MATCHING_CYLINDER_CREATION_FAILED`	Most likely due to two profiles touching.
`NON_CURVE_INPUT`	Only curves are allowed within profiles.
`UNIDENTIFIED`	Some unknown error occurred.
`INVALID_MATCH_POINT_INDEX`	At least one of the match indices points to a non-existent match point.
`INVALID_MATCH_POINT`	At least one match point is specified on non-profile topology.

tool

The tool.fs module contains enum types shared by multiple features.

MoveFaceType enum

Defines how face should be transformed in a moveFace feature.

Also used by boolean.

Value	Description
`OFFSET`
`TRANSLATE`
`ROTATE`

ToolBodyType enum

Defines what type of body a body-creating feature (extrude, revolve, etc.) should create.

Value	Description
`SOLID`
`SURFACE`

ExtendedToolBodyType enum

Defines what type of body a body-creating feature (extrude, revolve, etc.) should create.

Value	Description
`SOLID`
`SURFACE`
`THIN`

NewBodyOperationType enum

Defines how a new body from a body-creating feature (extrude, revolve, etc.) should be merged with other bodies in the context.

To include this enum with the same styling as the extrude dialog (and others), use booleanStepTypePredicate(definition).

Value	Description
`NEW`	Creates a new body in the context with the geometry resulting from the operation.
`ADD`	Performs a boolean union between the new body and all bodies in the merge scope.
`REMOVE`	Performs a boolean subtraction of the new body from all bodies in the merge scope.
`INTERSECT`	Performs a boolean intersection between each new body and each body in the merge scope.

NewSurfaceOperationType enum

Defines how a new surface from a surface-creating feature (sweep, loft, revolve, etc.) should be merged with other surfaces in the context.

To include this enum with the same styling as the extrude dialog (and others), use booleanStepTypePredicate(definition).

Value	Description
`NEW`	Creates a new surface in the context with the geometry resulting from the operation.
`ADD`	Performs a surface union between the new surface and all surfaces used as input.

uihint

UIHint enum

List of available UI Hints, which control how a parameter input is displayed in the feature dialog.

EXAMPLE

annotation { "Name" : "Flip", "UIHint" : UIHint.OPPOSITE_DIRECTION }
definition.isFlipped is boolean;

Multiple UIHints can be specified in an array (e.g. [ UIHint.OPPOSITE_DIRECTION, UIHint.REMEMBER_PREVIOUS_VALUE ]).

Raw strings (e.g. "OPPOSITE_DIRECTION") may be used in place of the enum access (e.g. UIHint.OPPOSITE_DIRECTION) for the same result.

OPPOSITE_DIRECTION and ALWAYS_HIDDEN behaviors are considered stable. Other UIHints can be used, but their behaviors may change in future versions of Onshape.

Value	Description
`OPPOSITE_DIRECTION`	For a boolean parameter, display as a toggle button with arrow next to the previous parameter.
`ALWAYS_HIDDEN`	Do not display this parameter or allow a user to edit it (useful for parameters changed only in editing logic or manipulator change functions).
`SHOW_CREATE_SELECTION`	For a query parameter, include a button to open the "Create selection" dialog.
`CONTROL_VISIBILITY`	For Onshape internal use.
`NO_PREVIEW_PROVIDED`	For a feature, hide the preview slider which controls before/after transparency, and only show the final version.
`REMEMBER_PREVIOUS_VALUE`	When a user makes a new instance of this feature, set this parameter's default value to the value they set the last time they used this feature.
`DISPLAY_SHORT`	Two consecutive boolean or quantity parameters marked as DISPLAY_SHORT may be placed on the same line.
`ALLOW_FEATURE_SELECTION`	For Onshape internal use.
`MATE_CONNECTOR_AXIS_TYPE`	For Onshape internal use.
`PRIMARY_AXIS`	For Onshape internal use.
`SHOW_EXPRESSION`	If an expression (like #foo or 1/4 in) is entered, always show the expression, and never the resulting value.
`OPPOSITE_DIRECTION_CIRCULAR`	Like `OPPOSITE_DIRECTION`, but with circular arrows.
`SHOW_LABEL`	Show a label above an enum parameter.
`HORIZONTAL_ENUM`	Display an enum as a horizontal list of clickable text, rather than the default select control
`UNCONFIGURABLE`	For Onshape internal use.
`MATCH_LAST_ARRAY_ITEM`	Inside an array parameter, set the default value on a new item to match what is set on the last item.
`COLLAPSE_ARRAY_ITEMS`	For an array parameter, create new items (and items in a newly opened dialog) as collapsed by default.
`INITIAL_FOCUS_ON_EDIT`	When an existing feature is edited, the first visible parameter with this UI hint will get focus.
`INITIAL_FOCUS`	When creating or editing, the first visible parameter with this UI hint will get focus (but when editing, a parameter with INITIAL_FOCUS_ON_EDIT takes precedence).
`DISPLAY_CURRENT_VALUE_ONLY`	For Onshape internal use.
`READ_ONLY`	Prevent changes to the parameter from the feature dialog. A read-only parameter can be modified by the editing logic function.
`PREVENT_CREATING_NEW_MATE_CONNECTORS`	For a query parameter allowing BodyType.MATE_CONNECTOR, only allow preexisting mate connectors, and don't provide a button to allow creating new mate connectors specificaly for this parameter.
`FIRST_IN_ROW`	Guarantee that, regardless of other layout requirements, this parameter will always be the first parameter in its displayed row.
`ALLOW_QUERY_ORDER`	Enable reordering of queries in a query parameter.
`PREVENT_ARRAY_REORDER`	Disable reordering of items in an array parameter.
`FOCUS_INNER_QUERY`	When adding a new item to an array parameter, focus the driving inner QLV if the parameter is selection-driven, and focus the first inner QLV otherwise.
`SHOW_TOLERANCE`	For a boolean parameter, display as a toggle button with tolerance icon next to the previous parameter.
`ALLOW_ARRAY_FOCUS`	Allow focusing an array parameter with no driving or inner QLV, as if it were selection-driven.
`SHOW_INLINE_CONFIG_INPUTS`	Inline the configuration parameters in the configure dialog for the feature.
`FOCUS_ON_VISIBLE`	For a query parameter, selects it when it becomes visible during editing.
`CAN_BE_TOLERANT`	Used with length or angle parameters to indicate that they can be tolerant quantities.

variabletype

VariableType enum

See assignVariable.

Value	Description
`LENGTH`
`ANGLE`
`NUMBER`
`ANY`

volumeaccuracy

VolumeAccuracy enum

Level of accuracy to use for computing the volume of a solid body. The values are:

LOW: fastest, least accurate, good for approximations
MEDIUM: moderately fast, moderately accurate
HIGH: slowest, most accurate, required for regeneration

Value	Description
`LOW`
`MEDIUM`
`HIGH`

wraptype

WrapType enum

Specifies the type of wrap to execute.

Value	Description
`SIMPLE`	Wrap around the infinite definition of the destination surface.
`TRIM`	Wrap around a defined destination face, and trim anything that falls off of it.
`IMPRINT`	Imprint edges onto a defined destination face.