# 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).

This functionality is available on Onshape's browser and iOS platforms only.

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).

- Click .
- Select the Edges, which act as the boundaries of the fill.
- Optionally, define
**Continuity**for each selected edge or curve (you can select Curvature visualization 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. **Curvature**- Match the actual curve of the adjacent surfaceFor 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.

**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 iso curves**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 iso curves

Show iso curves 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)**Curvature**- Match the actual curve of the other surface**Position**- Make edges meet with no tangent or curvature relationship to each other

- 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 iso curves 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.

**Guide vertices**

The Guide vertices are selected to further define the shape of the surface.

**Show iso curves**

Show iso curves 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.