Surface Modeling

Curve and surface continuity is a measure of the smoothness of the between 2 curves or 2 surfaces where they connect. As curves and surfaces are built up to create geometric models, continuity becomes important in order to create the most fluid or continuous organic shape.

The G (or Geometry) designation is used to determine curve/surface continuity (G0 to G3). In Onshape, these designations correlate to the "Match" options in many curve and surface features (for example, Bridging curves, Fillet, Face blend, and others). These continuity classifications are outlined below, along with their definitions:

• G0 (Match position) - The position is matched between the 2 curves/surfaces. Both curves/surfaces share a common position at the joint.

• G1 (Match tangent) - Tangency is matched between the 2 curves/surfaces. Both curves/surfaces touch and share a common angle that is equal at both ends. A fillet is a good example of this type of continuity match.

• G2 (Match curvature) - Curvature (radius) is matched between the 2 curves/surfaces. Both curves/surfaces touch, are tangent, and have the same curvature at the point where they touch (they both have identical radii).

• G3 (Match flow) - Flow is matched between the 2 curves/surfaces. Both curves/surfaces touch, are tangent, have similar curvature, and show the amount of change in the curvature over the curvature's length (flow).

Using the Bridging curve feature, you can create a bridging curve (shown below in orange) between two curves and match its start and end position, tangency, curvature, and flow (or some combination between the two; for instance, Match position at the start and Match curvature at the end):

From left to right: G0 (Match position), G1 (Match tangent), G2 (Match curvature), G3 (Match flow)

Extending this beyond curves, you can create a surface between 2 surfaces, and match its start and end continuity in the same way:

From left to right: G0 (Match position), G1 (Match tangent), G2 (Match curvature), G3 (Match flow)

When analyzing curve or surface continuity using the Curve/surface analysis tool, you can see that with each progressive continuity match, the connections between the curves/surfaces becomes smoother and show smoother curvature combs. G0 (Match position) cannot be analyzed using the Curve/surface analysis because a straight line has no curvature.

From left to right: G1 (Match tangent), G2 (Match curvature), G3 (Match flow)

From left to right: G1 (Match tangent), G2 (Match curvature), G3 (Match flow)

When analyzing curve or surface continuity using the Zebra stripes tool, with each progressive continuity match, the connection between the curves/surfaces becomes smoother. Zebra stripes at the surface edges become increasingly smooth as you go up from G0 (Match position) to G2 (Match continuity):

From left to right: G0 (No continuity), G1 (Match tangent), and G2 (Match curvature)

The following examples illustrate the continuities on a bridging curve between two other non-linear curves. The bridging curve is colored magenta. The first column shows the Bridging curve dialog and continuity selection with the result (and Edit control points enabled), the middle column shows the bridging curve with Edit control points disabled, and the final column shows the Curve/surface analysis for all curves:

The continuity selected for the curve and surface connections in your model depends entirely on the level of continuity required at each junction/edge. There is no right or wrong surface continuity.

Additionally, higher orders of continuity require more control points to enforce. G0 needs only one control point (the endpoint), G1 needs two, G2 needs three, and G3 needs four. A Bezier curve that is G3 constrained at both ends requires at least eight control points, four for each end.

Modeling with surfaces requires additional steps to create high quality surfaces, These steps increase performance, avoid imperfections, and streamline complex surface creation.

This lists the collection of surface feature tools. This is not an exhaustive list. Additional Feature tools may be used when modeling surfaces. See Surfacing for additional information.

• Thicken - Add depth to a surface. Create a new part or modify an existing one by giving thickness to a surface and converting it to a solid, adding or removing material from an existing part or surface, or intersecting parts in its path.
• Enclose - Create a part by selecting all boundaries surrounding an empty space to form a solid. Use any set of surfaces and solids (including planes and faces) that intersect each other or connect at a boundary to create a volume. Create a new part or modify an existing one by adding, removing, or intersecting parts.
• Fillet - Round sharp interior and exterior edges and define as a standard constant radius, more stylized conic, or variable by selecting Edge fillet. Optionally apply a Full round fillet to create a seamless blend of one or more faces between two opposing sides.
• Face blend - Round sharp connected or disconnected interior and exterior faces to create a seamless blend between the faces or detach the blend to create new faces, defining a radius or constant width. Further define the blend cross section (rolling ball or swept profile), symmetry, control, trim, constraints, and limits.
• Delete face - Remove geometry from a part. Select whether to heal the surrounding faces (by extending until they intersect), cap the void, or leave the void open. This Direct Editing tool is especially convenient if you don't have the parametric history of the part, as is often the case with an imported part.
• Move face - Translate, rotate, or offset one or more selected faces. This Direct Editing tool is especially convenient if you don't have the parametric history of the part, as is often the case with an imported part.
• Replace face - Trim a face or extend a face to a new surface. This Direct Editing tool is especially convenient if you don't have the parametric history of the part, as is often the case with an imported part.
• Offset surface - Create a new surface by offsetting an existing face, surface, or sketch region. Set offset distance to 0 to create a copy in place.
• Boundary surface - Create or add a surface specified by its boundary profiles.
• Fill - Create a surface (or a part from surfaces) by defining boundaries and refine the surface with boundary conditions (instead of requiring the use of reference surfaces).
• Move boundary - Move boundary edges of a surface in order to extend or trim it.
• Ruled surface - Create a new or additional ruled surface from an existing edge or multiple edges of a sketch region.
• Mutual trim - Trim two adjacent surfaces by extending intersections to complete the trim.

In addition to the surfacing tools, curves are used to create the basic building blocks of surfaces.

This lists the collection of curve feature tools. This is not an exhaustive list. Additional Feature tools may be used when manipulating curves.

• Sketch tools - Tools in the Sketch toolbar such as Line, Corner rectangle, Center point rectangle, Center point circle, 3 point circle, Tangent arc, 3 point arc, Spline, Point, and Construction used to create a sketch in a Part Studio.
• Helix - Create a helix using a conical or cylindrical face, single axis or z-axis of a mate connector, or circular edge.
• 3D fit spline - Create a 3D fit spline through a series of vertices. Creates a curve which is listed in the Parts list under Curves.
• Projected curve - Create a curve from the projection of two sketches (Two sketches option) or from the projection of a curve on a face (Curve to face option).
• Bridging curve - Create a Curve connecting any two points, vertices, or Mate connectors. The resulting Curve is listed in the Feature list and the Parts list.
• Composite curve - Represent multiple edges as one Curve. Select multiple adjacent edges, sketch entities, and other curves. Selecting non-contiguous edges may result in multiple Curves created. Selections for each Curve must meet at their vertices. (Curves are listed in the Parts > Curves list.)
• Intersection curve - Create a curve at the intersection of two or more surfaces or faces. The selections must intersect.
• Trim curve - Trim or extend a curve by a distance or to a bounding entity.
• Isocline - Create an isocline on a sloped face. An isocline runs on a face at positions where the face has a certain slope compared to its reference definition. The resulting isocline is listed in the Feature list and Parts list.
• Offset curve - Create and extend and/or split a new curve by offsetting edges on surrounding faces.
• Isoparametric curve - Create smooth curves that run along a face or surface in the U or V direction.
• Edit curve - Edit an existing curve by selecting sketch entities or curves to apply a simplified approximation, elevate the degree, reposition control curve vertices and/or planarize into any 2D plane.