solvecraft/docs/book/command-guides/solid.extrude.md

Turn a flat sketch region into a solid, or add or remove material from an existing body. For example, a rectangle extruded 20 mm becomes a rectangular block.

Before you start

• For a solid extrusion, finish a sketch with at least one closed region. Select the region you want, rather than an individual edge or point.
• You can also select a planar face of an existing body instead of a sketch.
• To add or remove material, an existing body must meet the extrusion. Choose New Body when you want an independent piece.
• Thin Extrude uses sketch curves instead of filled regions; open chains are allowed. This is useful for a wall or a ring.

Options

Choice	What it does	When to use it
Profiles	Chooses the filled sketch regions to extrude. A loop inside another loop makes a hole.	Select just the regions you need when a sketch contains several.
Distance	Sets how far the shape extends. Values can include units, such as 20 mm, or a named design parameter.	Make a part to a known size.
Reverse Direction	Sends the extrusion to the other side of the sketch.	The preview points away from the intended body.
Symmetric	Splits the entered total distance equally across the sketch plane. 10 mm extends 5 mm on each side.	Keep the sketch at the middle of a part.
Two Sides	Sets a separate distance on each side.	The sketch is between two unequal extensions.
Through All	Reaches through the target body.	Cut a hole that must stay open when the body becomes thicker.
To Object	Stops at a selected target face, vertex or point. An offset can stop before or beyond that target.	Let the end follow another part of the design.
Start	Starts at the sketch, at an offset from it, or from a selected object.	Leave a gap before the extrusion begins.
Taper Angle	Slopes the side walls.	Make drafted sides; reduce the angle if the profile's narrow details cannot support it.
Operation	New Body makes a separate piece; Join adds material; Cut removes it; Intersect keeps only the overlap.	Choose the intended result explicitly when the automatic preview is not what you want.
Target bodies	Chooses which existing bodies take part in a join, cut or intersection.	Several bodies lie in the extrusion's path.
Thin Extrude	Builds walls along curves; thickness and side control where the material lies. Two-sided walls can have different thicknesses.	Make ribs, walls or rings without drawing both wall boundaries.

Try it: a 20 mm block

1. Create a sketch on the XY plane and draw a closed rectangle.
2. Finish the sketch and choose Extrude.
3. Select the rectangular region, set Distance to 20 mm, and choose New Body.
4. Check the preview's direction and confirm. You should have one solid block.
5. Edit the extrusion in the timeline to change its distance later.

Tips and common mistakes

• Do check the operation before confirming. Automatic operation can join an addition or cut into an existing body; it is not a promise of a separate part.
• Do use Through All for a cut that should follow later thickness changes.
• Don't expect an open outline to make a filled solid. Close it, or choose Thin Extrude for a wall.
• Don't assume a symmetric distance is the distance on each side. New symmetric extrusions use the total distance; older saved designs can retain their earlier convention.
• Taper with a two-sided or symmetric extent is not supported. A very steep taper can also be refused rather than creating an invalid result.

Examples and community resources

The bracket starts with a closed L-shaped profile; another extrusion removes the two holes. Its dimensions are controlled by design parameters.

Resource	What to explore	Author and licence
Editable bracket recipe	A complete SolidCraft example using an extrusion, a fillet and a cut.	SolidCraft contributors; MIT OR Apache-2.0.

Contribute a tip, demo, model or screenshot to add a reviewed resource beside this explanation.

See also

{{#command solid.revolve}} turns a profile around an axis. {{#command solid.sweep}} carries a profile along a path. {{#command sheet.flange}} creates sheet metal with a thickness rule.