Sweep
Define a shape using a selected region, curves, or planar face moving along a path (either solid or surface). Create a new part or modify an existing one by adding or removing material, or intersecting parts in its path.
In the Feature toolbar:
Define a shape using a selected region, curves, or planar face moving along a path (either solid or surface). Create a new part or modify an existing one by adding or removing material, or intersecting parts in its path.
The Sweep feature allows you to define a shape using a selected region, curves, or planar face moving along a path (either solid or surface). Create a new part or modify an existing one by adding or removing material, or intersecting parts in its path.
Click the Sweep feature on the feature toolbar. Select Solid to create a part. Select the Faces and sketch regions to sweep. Here, the circle on Plane 1 is selected. Click the Sweep path field in the dialog, and select the path for the sweep in the graphics area, in this case the spline on the Front plane.
By default, the New type is selected, which creates a new part. Select Add to add the swept part to the existing part. If multiple parts exist, the Merge scope field in the dialog has focus. Select a part in the graphics area to use as a merge scope, or check Merge with all to merge with all parts intersecting the sweep path. Select Remove to remove the sweep from the existing parts in the merge scope, or Intersect to keep only the intersection of the sweep and the parts in the merge scope.
Select Keep profile orientation to maintain the profile relationship along the sweep path. Leave it unchecked to maintain the profile relationship with the global plane.
Click the checkmark to accept the Sweep feature.
- Click .
- Select Solid Creation type.
- Select a Result operation type:
- New - Create a new solid
- Add - Add to an existing solid
- Remove - Subtract from an existing solid
- Intersect - Keep the intersection of two (or more) solids
- Select the faces and/or sketch regions to sweep.
- Click to make the Sweep path field active. Select a line segment or curve on the sketch or an edge on the part.
- Select a Profile control type:
Onshape remembers the selection (Solid, Surface, or Thin) and opens the dialog with the last selected option in subsequent operations.
- None - No profile control (maintain the profile relationship with the global plane).
- Keep profile orientation - Maintain the profile relationship along the sweep path.
-
Lock profile faces - Lock the selected profile face or faces of the sweep into place.
-
Lock profile direction - Lock the profile direction of the sweep into place. (Select the direction to lock.)
- If necessary, select a Merge scope (or Merge with all) to select parts with which to merge the new (additional) part.
- Click .
If the sweep feature references a face or sketch region that is along the sweep path (not at an end) the path is broken where the profile plane touches it and the sweep is created in both directions, for the length of the sweep path.
For best results, the profile and the path should touch.
- Click .
- Select Surface creation type.
- Select a Result operation type:
- New - Create a new surface
- Add - Add to an existing surface
- Select the edges and sketch curves to sweep.
- Click to make the Sweep path field active. Select a line segment or curve on the sketch or an edge.
- Select a Profile control type:
Onshape remembers the selection (Solid, Surface, or Thin) and opens the dialog with the last selected option in subsequent operations.
- None - No profile control (maintain the profile relationship with the global plane).
- Keep profile orientation - Maintain the profile relationship along the sweep path.
-
Lock profile faces - Lock the selected profile face or faces of the sweep into place.
-
Lock profile direction - Lock the profile direction of the sweep into place. (Select the direction to lock.)
- If necessary, select a Merge scope (or Merge with all) to select parts with which to merge the new (additional) part.
- Click .
If the sweep feature references a face or sketch region that is along the sweep path (not at an end) the path is broken where the profile plane touches it and the sweep is created in both directions, for the length of the sweep path.
For best results, the profile and the path should touch.
- Click .
- Select Thin creation type.
- Select a Result operation type:
- New - Create a new thin sweep
- Add- Add to an existing solid
- Remove- Subtract from an existing solid
- Intersect- Keep the intersection of two (or more) solids
- Select the face, single line, sketch region, and/or sketch profile to sweep.
- Do one of the following:
- To create a sweep with a symmetric thickness, check the Mid plane option and then enter the Thickness value.
- To specify individual wall thicknesses, uncheck the Mid plane option. Then, enter the Thickness 1 wall value and Thickness 2 wall value. Click the Flip wall arrow to flip Thickness 1 with Thickness 2.
- Click to make the Sweep path field active. Select a line segment or curve on the sketch or an edge on the part.
- Select a Profile control type:
- None - No profile control (maintain the profile relationship with the global plane).
- Keep profile orientation - Maintain the profile relationship along the sweep path.
Lock profile faces - Lock the selected profile face or faces of the sweep into place.
Lock profile direction - Lock the profile direction of the sweep into place. (Select the direction to lock.)
- Check the Trim ends option to start and terminate the sweep at the endpoint of the sweep path. Uncheck it to create end faces tangent to the sweep path.
- If necessary, select a Merge scope (or Merge with all) to select parts with which to merge the new (additional) part.
- Click .
Onshape remembers the selection (Solid, Surface, or Thin) and opens the dialog with the last selected option in subsequent operations.
If the sweep feature references a face or sketch region that is along the sweep path (not at an end), the path is broken where the profile plane touches it, and the sweep is created in both directions, for the length of the sweep path.
For best results, the profile and the path should touch.
New - Create new material that results in a new part:
Add - Add material to the existing material:
When adding material, you have the option to merge that material with other parts that touch or intersect its geometry:
- If the geometry touches or intersects with only one part then that part is automatically added to the merge scope.
- If multiple parts touch or intersect the geometry, then there is ambiguity and you must select which parts to merge with (the merge scope).
- A shortcut to selecting multiple touching or intersecting parts, you can check Merge with all to add all touching or intersecting parts to the merge scope.
If the Boolean is set to Add, Remove, or Intersect and nothing is set in the merge scope, the feature will result in an error. For New, no merge scope is available since New does not boolean the result.
Remove material from existing material; not available for surfaces.
Leave material only where geometry intersects; not available for surfaces.
Merge scope is available with parts and surfaces and allows you to select the specific part or surface with which to merge the newly created part or surface. By default, Merge all is selected. You are able to uncheck that box to access the Merge scope field, then select the part or surface with which to merge. Surfaces must be merged with surfaces and parts with parts.
Merge scope: with all
Merge with all parts the new part intersects:
Merge scope: particular part
Select a specific part with which to merge:
- Tap Sweep tool.
- Select Creation type:
- Solid - Create parts or modify existing parts by sweeping a sketch region along a path.
- Surface - Create a surface by sweeping a sketch curve along a path.
- Thin - Create or modify thin parts by sweeping a sketch along a path
- If you select to create a solid, also select a result body operation type:
- New - Create a new solid.
- Add - Add to an existing solid.
- Remove - Subtract from an existing solid.
- Intersect - Keep the intersection of two (or more) solids.
- Select the faces and sketch regions to sweep.
- Specify the sweep path (select a line segment or curve on the sketch or an edge on the part).
- Select a Profile control type:
- None - No profile control (maintain the profile relationship with the global plane).
- Keep profile orientation - Maintain the profile relationship along the sweep path.
-
Lock profile faces - Lock the selected profile face or faces of the sweep into place.
-
Lock profile direction - Lock the profile direction of the sweep into place. (Select the direction to lock.)
- If necessary, select a Merge scope (or Merge with all) to select parts with which to merge the new (additional) part.
- Tap the checkmark.
New - Create new material that results in a new part
Add - Create material and add to the existing material
When adding material, you have the option to merge that material with other parts that touch or intersect its geometry:
- If the geometry touches or intersects with only one part then that part is automatically added to the merge scope.
- If multiple parts touch or intersect the geometry, then there is ambiguity and you must select which parts to merge with (the merge scope).
-
A shortcut to selecting multiple touching or intersecting parts, check Merge with all to add all touching or intersecting parts to the merge scope.
If the Boolean is set to Add, Remove, or Intersect and nothing is set in the merge scope, the feature will result in an error. For New, no merge scope is available since New does not boolean the result.
Remove - Take material away
Intersect - Leave material only where intersections exist
Create a surface by sweeping a sketch curve along a path.
- Tap Sweep tool.
- Select Creation type:
- Solid - Create parts or modify existing parts by sweeping a sketch region along a path.
- Surface - Create a surface by sweeping a sketch curve along a path.
- Thin - Create or modify thin parts by sweeping a sketch along a path
- If you select to create a solid, also select a result body operation type:
- New - Create a new solid.
- Add - Add to an existing solid.
- Remove - Subtract from an existing solid.
- Intersect - Keep the intersection of two (or more) solids.
- Select the face or edge to sweep.
- Specify the sweep path (select a line segment or curve on the sketch or an edge on the part).
- Select a Profile control type:
- None - No profile control (maintain the profile relationship with the global plane).
- Keep profile orientation - Maintain the profile relationship along the sweep path.
-
Lock profile faces - Lock the selected profile face or faces of the sweep into place.
-
Lock profile direction - Lock the profile direction of the sweep into place. (Select the direction to lock.)
- If necessary, select a Merge scope (or Merge with all) to select parts with which to merge the new (additional) part.
- Tap the checkmark.
New - Create new material that results in a new part
Add - Create material and add to the existing material
When adding material, you have the option to merge that material with other parts that touch or intersect its geometry:
- If the geometry touches or intersects with only one part then that part is automatically added to the merge scope.
- If multiple parts touch or intersect the geometry, then there is ambiguity and you must select which parts to merge with (the merge scope).
-
A shortcut to selecting multiple touching or intersecting parts, you can check Merge with all to add all touching or intersecting parts to the merge scope.
If the Boolean is set to Add, Remove, or Intersect and nothing is set in the merge scope, the feature will result in an error. For New, no merge scope is available since New does not boolean the result.
Remove - take material away
Intersect - Leave material only where intersections exist
Create a surface by sweeping a sketch curve along a path.