Fill
This functionality is available on Onshape's browser, iOS, and Android platforms.
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).
In the Feature toolbar:
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).
The Fill feature allows you to 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). Click the Fill feature tool on the toolbar. Select the edges to act as the boundaries of the fill. Optionally, define the continuity of the Fill. Select Zebra stripes from the View tools. Position is the default, which makes edges meet with no tangent or curvature relationship to each other. Select Tangency to create an implicit tangency, or Curvature to Match the curve of the adjacent surface. Click the green checkmark to accept the new fill.
Here is another example of a sketch on the Front plane and a single vertex on an offset plane. Select Fill. Then select the edges of Sketch 1. Click the Guides checkbox. Then select the vertex in Sketch 2, which is used to influence the shape. The resulting surface intersects the vertex in the interior of the boundary. Check Show isocurves to evaluate how the underlying surface is defined. Adjusting the count up or down increases or decreases the number of curves displayed. Click the green checkmark to accept the new fill.
- Click .
- Select the Edges, which act as the boundaries of the fill.
- Optionally, define Continuity for each selected edge or curve (you can select Zebra stripes from the small View cube menu to see the effects):
- Position
- Make edges meet with no tangent or curvature relationship to each other
- Tangency
- Create an implicit tangency (normal to the plane of the selected surface) between the boundaries and the new surface (as if you had a reference surface). This works for sketch selections only, not for other planar curves. Optionally, when selected, the Adjacent faces field is enabled. Pick any face in which underlying geometry is coincident with at least one profile part's curve (the face and edge do not need to intersect or be part of the same part).
- Curvature
- Match the actual curve of the adjacent surface. Optionally, when selected, the Adjacent face field is enabled. Pick any face in which underlying geometry is coincident with at least one profile part's curve (the face and edge do not need to intersect or be part of the same part).
For example, for the left most selected edge, below, each of the Continuity options were selected. Note the differences in the visualization stripes:
Position:
Tangency:
Curvature:
- Select
Guides
(points, vertices, points on a sketch, or curves) with which to influence the shape. The resulting surface intersects these points which will lie in the interior of the boundary. When curves are selected, the surface pushes through the curves and you can select from two types of calculations:
- Sampled
- Uses the Sample Size to determine the number of vertices along the curves are used to calculate the surface. A long Sample size may result in the surface following the entire curve:
Sample size of 3:
Sample size of 10:
Depending on the Sample size, some rippling of the surface may occur.
- Sampled
- Uses the Sample Size to determine the number of vertices along the curves are used to calculate the surface. A long Sample size may result in the surface following the entire curve:
- Precise - Uses the exact curve to form the surface. Note that this option requires very carefully designed and selected curves. See the examples below for more information.
- Check
Show isocurves
to evaluate how the underlying surface is defined.
The untrimmed underlying surface is shown as a mesh to display the iso parametric curves, enabling you to evaluate the quality of the underlying surface.
- Click .
The edges of the surfaces and the two bridging curves are selected as boundaries. A new surface is created:
Guide vertices
The Guide vertices are selected to further define the shape of the surface:
Guides with Precise option
When using the Precise option with guide curves especially, if the curves meet each other, the intersection must be at a point such that the curve and the point are tangent to each other. Also, when using the Precise option, the curves must touch the boundary but not cross the boundary.
Guides that do not intersect
Guides that meet tangentially
Guide that touches one boundary
Guide that does not touch a boundary
This scenario can work when Sampled is selected:
But will not succeed when Precise is selected.
Guides that intersect at tangent plane
Failure due to lack of tangency
Guides that meet tangent criteria
Show isocurves
Show isocurves is selected to display the iso parametric curves, enabling you to evaluate the quality of the underlying surface:
- When selecting edges, you might see red dots; these indicate missing or open curves in the boundary.
- If the operation results in a closed surface (creating a volume), Onshape automatically creates a solid part (if Add is selected). If the creation of a part is an undesired result, use New to keep all surfaces and not create a part.
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).
- Tap Fill tool.
- Select the Edges, which are boundaries of the fill.
Optionally, define Continuity for each selected edge or curve:
- Tangent
- Create an implicit tangency (normal to the plane of the surface) between the boundaries and the new surface (as if you had a reference surface). Optionally, when selected, the Adjacent faces field is enabled. Pick any face in which underlying geometry is coincident with at least one profile part's curve (the face and edge do not need to intersect or be part of the same part).
- Curvature
- Match the actual curve of the other surface. Optionally, when selected, the Adjacent faces field is enabled. Pick any face in which underlying geometry is coincident with at least one profile part's curve (the face and edge do not need to intersect or be part of the same part).
- Position
- Make edges meet with no tangent or curvature relationship to each other
- Tangent
- Create an implicit tangency (normal to the plane of the surface) between the boundaries and the new surface (as if you had a reference surface). Optionally, when selected, the Adjacent faces field is enabled. Pick any face in which underlying geometry is coincident with at least one profile part's curve (the face and edge do not need to intersect or be part of the same part).
- Select Guide (points, vertices, points on a sketch, or curves) with which to influence the shape. The resulting surface intersects these points. When curves are selected, the surface pushes through the curves and you can select from two types of calculations:
- Sampled - Uses the Sample size to determine the number of vertices along the curves used to calculate the surface. A large sample size may result in the surface following the entire curve. A smaller Sample size may result in some rippling of the surface.
- Precise - uses the exact curve to form the surface. Note that this option requires very carefuflly designed and selected curves.
- Check Show isocurves to evaluate how the underlying surface is defined.
The untrimmed underlying surface is shown as a mesh to display the iso parametric curves, enabling you to evaluate the quality of the underlying surface.
- Tap the checkmark.
The edges of the surfaces and the two bridging curves are selected as boundaries. A new surface is created.
The Guide vertices are selected to further define the shape of the surface.
Show isocurves is selected to display the iso parametric curves, enabling you to evaluate the quality of the underlying surface
When selecting edges, you might see red dots; these indicate missing or open curves.
If the operation results in a closed surface (creating a volume), Onshape automatically creates a solid part (if Add is selected). If the creation of a part is an undesired result, use New to keep all surfaces and not create a part.