Extrude

You can use the Extrude tool to create 3D geometry by pushing or pulling a face or closed sketch in a linear direction. If necessary, you can specify a draft angle, which adds a taper to the side faces of the geometry.

The type of extrude created is automated based on geometric conditions but can be modified if necessary. Using the Extrude tool can result in geometry that is:

• A new body.
• Added to an existing body.
• Removed from an existing body, creating a hole or void.
• The intersection of the revolved profile with an existing body.

How to use the Extrude tool

To use the Extrude tool:

1. Go to Tools > Extrude.
   For other methods of accessing this tool Accessing tools.
2. Select the face(s) or sketch profile(s) you want to extrude.
3. Use the gizmo to extrude the selected items to your desired distance.
4. Optional: Use the Boolean badge to manually select a boolean action.
5. Optional: Use the gizmo to define a draft angle.
6. Select Done.
   Note: When using Extrude from the adaptive menu, select an empty area of the grid to complete the tool.

History settings

To manage history settings for the Extrude action, find the step for your specific extrusion and then view or modify the following:

• Profile – Click/tap Edit… or Select… to choose a different sketch profile for the Extrude action. 
• Sides – Select the dropdown to choose between One-Sided and Symmetric for your extrude extension.
• Extent – Select the dropdown to choose between Distance, To Object, and Through All as the extent type for the extrusion.
  • Distance – Enter your preferred distance.
  • To Object –  Click/tap Select… beside To Object to select the object where you want to extend the extrusion.
  • Through All – Choose whether to turn on or turn off Flip Direction.
• Draft Angle – Enter your preferred draft angle for the extrusion.
• Start – To choose from where you want to start your extrusion, select the dropdown to choose between From Profile, Offset, and From Plane.
  • From Profile – Starts your extrusion from the selected profile.
  • Offset – Enter values for the Start Offset and End Offset fields.
  • From Plane – Select Edit… beside Start Plane to choose from which plane you want the extrusion to start.
    
    

Automatic Boolean actions

The type of Boolean operation created is automated based on geometric conditions. Here is a summary of the automatic Boolean actions and when they are triggered:

Boolean type	Result	Automatic trigger
New Body	Creates a new, stand-alone solid body.	Automatically triggers when new geometry does not intersect or make contact with any existing body.
Union	Executes a Union boolean operation, adding the new geometry directly to an existing body and sharing intersecting edges.	Triggers with any of the following conditions: • A face on an existing body is selected to generate the geometry path. • A sketch profile connected to an existing body is pulled or extended away from it.
Subtract	Executes a Subtract boolean operation, removing the new geometry from an existing body to produce a cut, hole, or void.	Triggers when a sketch profile or face is selected and pushed or extended directly into an existing solid body.
Intersect	Restricts the output to an Intersect boolean type, retaining only the shared volume where the new geometry overlaps an existing body.	An intersection is not applied automatically and must be selected manually from the Boolean badge menu.

Extrude vs Offset Face

While the tools look similar, Offset Face cannot be used to create a body from a closed sketch, while Extrude created a 3D body from a 2D sketch by linearly extending a face on a body.

• Offset Face: Adjacent faces are extended or trimmed.
• Extrude: Creates a new prismatic shape from a face, while offset modifies a body.

Additionally, you can only Extrude planar faces, but this is not a limitation of the Offset Face tool.

Offset Face	Extrude

Video walkthrough