Tools menu: Sweep tool

What is the Sweep tool?

You can use the Sweep tool to create a 3D body by extending a sketch profile or face along a path. Sweep is useful for:

• Creating pipes and tubes – Build parts that follow curved or angled routes.
• Modeling wires and cables – Follow a defined path with a consistent cross-section.
• Creating handles and rails – Extend a profile along straight or curved edges.

How to use the Sweep tool

Before you start

Prepare a sketch profile or face and a connected path for it to follow. Positioning the profile near the start of the path can make the result easier to control. For supported geometry and setup guidance, refer to Sweep profiles and paths.

Using the Sweep tool

1. Go to Tools > Sweep. For other ways to open the tool, visit Accessing tools.
2. Select a sketch profile or face under Profile.
3. Under Path, select the connected sketch curves or edges that the profile should follow.
4. If necessary, adjust Profile Position and Orientation to control how the profile is placed and aligned along the path.
5. If necessary, adjust Twist, Scale, and Corner Type to refine the shape.
6. If necessary, choose a different Result to create a new body or apply a Boolean operation to an existing body.
7. To finish, select Done.

Sweep profiles and paths

A sweep requires a profile to define its cross-section and a path to define where that cross-section travels.

Profiles

• Closed sketch profiles – Use a closed sketch region to define the shape of the resulting solid.
• Faces – Use a suitable existing face as the cross-section.
• Profile placement – Position the profile near the path's starting point when possible. You can refine its placement using Profile Position.

Paths

• Sketch curves – Use connected sketch lines or curves to define the route.
• Body edges – Use connected edges of existing geometry as the path.
• Sharp corners – Tight turns may cause the swept body to overlap itself. You can adjust Corner Type or smooth the path to improve the result.

Parameter Card and History Settings

Shapr3D records the tools you use as steps in History, allowing you to revisit and modify them later. Each History step stores its parameters, which you can access through the parameter card. You can adjust these parameters while using the tool or reopen the parameter card from History after completing the step.

Adjust Sweep parameters

The Sweep parameter card includes:

• Profile – Select the sketch profiles or faces to sweep.
• Path – Select the connected edges or curves that define the route of the sweep.
• Profile Position – Choose how the profile is positioned relative to the path:
  • Auto – Let the tool determine the placement from the selected geometry.
  • Path Intersection – Position the profile where it intersects the path.
  • Closest Point – Use the point on the path closest to the profile.
  • Closest Endpoint – Use the nearest endpoint of the path.
• Orientation – Choose how the profile is aligned as it follows the path:
  • Normal to Path – Keep the profile perpendicular to the path's direction.
  • Parallel to Profile – Maintain the profile's original orientation.
• Twist – Set how much the profile rotates along the path. The default is 0°.
• Scale – Adjust the profile's size along the sweep. A value of 1 preserves its original scale.
• Corner Type – Choose how sharp turns in the path are handled:
  • Mitre – Join the swept sections at a sharp corner.
  • Round – Create a rounded transition at corners.
• Result – Choose New Body to create a separate body, Union to combine with an existing body, Subtract to remove material, or Intersect to keep overlapping volume. The tool can select a result automatically based on the geometry.

Edit Sweep in History

To modify a completed sweep, find its step in History and review the available settings:

• Profile – Change the sketch profile or face used for the sweep.
• Path – Change the selected path.
• Profile Position – Change where the profile is placed relative to the path.
• Orientation – Change how the profile aligns as it travels along the path.
• Twist – Change the amount of rotation along the path.
• Scale – Change the profile's scale along the path.
• Corner Type – Change how the sweep handles corners.

Automatic Boolean actions

When creating geometry, Shapr3D automatically selects a result based on how the new geometry interacts with existing bodies. You can change the result manually using the Boolean badge or the Result parameter.

Result	What it does	When it's selected automatically
New Body	Creates a separate solid body.	When the new geometry does not touch or overlap an existing body.
Union	Combines the new geometry with an existing body.	When geometry is created from an existing body or extended outward from a connected sketch profile.
Subtract	Removes overlapping material from an existing body.	When a sketch profile or face is pushed into an existing solid body.
Intersect	Keeps only the overlapping volume shared by the new geometry and an existing body.	Not selected automatically. Choose Intersect manually from the Boolean badge or Result parameter.

When to use the Sweep tool

Use Sweep when a shape needs to follow a defined path. Common situations include:

• Routing tubes and cables – Create solids that follow bends and turns.
• Building rails and handles – Extend a profile along an existing edge or sketch path.
• Controlling the cross-section – Adjust orientation, twist, or scale as the profile travels.
• Choosing between Sweep and Loft – Sweep moves a profile along a path, while Loft creates a transition between two or more profiles.

Best practices and troubleshooting

• Use a connected path so the profile can follow the intended route.
• Position the profile near the start of the path, or adjust Profile Position when its placement is unexpected.
• Use Corner Type to control how sharp changes in direction are handled.