Tools menu: Extrude tool

What is the Extrude tool?

You can use the Extrude tool to create 3D geometry by extending a closed sketch profile or planar face in a linear direction. You can also specify a draft angle to taper the side faces of the extrusion.

Extrude automatically suggests a result based on the selected geometry, but you can change the result as needed. An extrusion can:

• Create a new body.
• Add material to an existing body with Union.
• Remove material from an existing body with Subtract, such as when creating a hole or cutout.
• Keep only the overlapping volume with an existing body using Intersect.

How to use the Extrude tool

Using the Extrude tool

To create an extrusion:

1. Go to Tools > Extrude. 
   For other ways to access the tool, visit Accessing tools.
2. Select the sketch profiles or planar faces you want to extrude.
3. Drag the arrow to set the extrusion distance, or enter a value in the dimension field. You can use the gizmo to adjust the extrusion.
4. Optional: Adjust the draft angle to taper the side faces.
5. Optional: Select the Boolean badge to change the result, or select Extrude again while the tool is active to open the parameter card and adjust the available settings.
6. To finish and exit the tool, click anywhere in an empty area of the modeling space.

Extrusion direction and extent

You can control how far the extrusion extends and whether it grows in one direction or symmetrically around its starting position.

• One-Sided: Extends the extrusion in one direction from its starting position.
• Symmetric: Extends the extrusion equally in opposite directions.

Under Extent, choose how the extrusion ends:

• Distance: Extends the profile by a specified distance.
• To Object: Extends the profile until it reaches a selected object.
• Through All: Extends through the relevant geometry. Where available, use Flip Direction to reverse the direction.

Extrusion start options

The Start setting controls where the extrusion begins:

• From Profile: Starts at the selected sketch profile or face.
• Offset: Uses offset values to define the extrusion's starting and ending positions.
• From Plane: Starts the extrusion from a selected plane.

Automatic Boolean actions

Extrude automatically suggests a Boolean result based on how the extrusion relates to existing bodies. You can override this result using the Boolean badge or the Result setting in the parameter card.

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.

Choose New Body to create separate geometry, Union to add material, Intersect to keep overlapping geometry, or Subtract to remove material. For Union, Intersect, and Subtract, you can review or edit the bodies involved in the operation.

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 Extrude parameters

While Extrude is active, select Extrude again from the menu to open its parameter card. The available parameters include:

• Profile: Review or change the selected sketch profiles or faces.
• Sides: Choose One-Sided or Symmetric to control the extrusion direction.
• Extent: Choose Distance, To Object, or Through All to control where the extrusion ends.
• Distance: Set the extrusion length when using the Distance extent.
• Draft Angle: Set the taper angle of the extrusion's side faces.
• Start: Choose From Profile, Offset, or From Plane to control where the extrusion begins. Additional offset or plane selection fields appear as applicable.
• Result: Choose New Body, Union, Intersect, or Subtract. The initial result may be selected automatically based on the geometry.
• Union With / Intersect With / Subtract From: Review or edit the bodies involved in the selected Boolean operation. The field name depends on the chosen result.

To learn more about parameter cards, visit Parameter Cards.

Edit Extrude in History

To modify a completed extrusion:

1. Open the History sidebar.
2. Select the Extrude step to reopen its parameter card.
3. Modify the profile, distance, extent, draft angle, start position, or Boolean result as needed.
4. To finish editing, click anywhere in the modeling space.

To learn more about editing modeling steps, visit History.

When to use the Extrude tool

Common Extrude use cases

• Create solid geometry: Turn a closed sketch profile into a three-dimensional body.
• Add features: Extend a sketch profile or planar face to add material to an existing body.
• Create holes and cutouts: Extrude a profile through a body with a Subtract result.
• Design tapered features: Apply a draft angle to create sloped side faces.
• Control precise endpoints: Use To Object or Through All to define the extent relative to other geometry.

Extrude vs. Offset Face

Extrude creates or modifies geometry by extending a closed sketch profile or planar face in a linear direction. Offset Face modifies existing geometry by moving selected faces inward or outward, including non-planar faces.

• Extrude: Use it to create a body from a closed sketch profile, add material, or remove material through an extrusion.
• Offset Face: Use it to adjust existing faces while extending or trimming adjacent geometry.

To learn more, visit Tools menu: Offset Face tool.

Offset Face	Extrude

Best practices and troubleshooting

Best practices

• Confirm the selected profile: Review the selected sketch profiles or planar faces before setting the extrusion distance.
• Choose the appropriate extent: Use Distance for a fixed value, To Object for a geometric endpoint, or Through All when the extrusion should pass through the relevant geometry.
• Review the Boolean result: Check whether the extrusion creates a new body, adds material, removes material, or keeps overlapping geometry.
• Use History for adjustments: Edit the existing Extrude step to refine its dimensions or settings later.

Troubleshooting common issues