Victor Santos Oliveira
91638cb1f3
* claim: #5237 command-level guide follow-up * docs: add practical command guides and resource contributions (#5237) * docs: index practical guides and reject incomplete command links
72 lines
4.5 KiB
Markdown
72 lines
4.5 KiB
Markdown
Turn a flat sketch region into a solid, or add or remove material from an existing
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body. For example, a rectangle extruded 20 mm becomes a rectangular block.
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#### Before you start
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- For a solid extrusion, finish a sketch with at least one closed region. Select
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the region you want, rather than an individual edge or point.
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- You can also select a planar face of an existing body instead of a sketch.
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- To add or remove material, an existing body must meet the extrusion. Choose
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**New Body** when you want an independent piece.
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- **Thin Extrude** uses sketch curves instead of filled regions; open chains are
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allowed. This is useful for a wall or a ring.
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#### Options
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| Choice | What it does | When to use it |
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| --- | --- | --- |
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| 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. |
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| 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. |
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| Reverse Direction | Sends the extrusion to the other side of the sketch. | The preview points away from the intended body. |
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| 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. |
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| Two Sides | Sets a separate distance on each side. | The sketch is between two unequal extensions. |
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| Through All | Reaches through the target body. | Cut a hole that must stay open when the body becomes thicker. |
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| 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. |
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| Start | Starts at the sketch, at an offset from it, or from a selected object. | Leave a gap before the extrusion begins. |
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| Taper Angle | Slopes the side walls. | Make drafted sides; reduce the angle if the profile's narrow details cannot support it. |
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| 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. |
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| Target bodies | Chooses which existing bodies take part in a join, cut or intersection. | Several bodies lie in the extrusion's path. |
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| 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. |
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#### Try it: a 20 mm block
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1. Create a sketch on the XY plane and draw a closed rectangle.
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2. Finish the sketch and choose **Extrude**.
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3. Select the rectangular region, set **Distance** to **20 mm**, and choose
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**New Body**.
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4. Check the preview's direction and confirm. You should have one solid block.
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5. Edit the extrusion in the timeline to change its distance later.
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#### Tips and common mistakes
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- **Do** check the operation before confirming. Automatic operation can join an
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addition or cut into an existing body; it is not a promise of a separate part.
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- **Do** use Through All for a cut that should follow later thickness changes.
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- **Don't** expect an open outline to make a filled solid. Close it, or choose
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Thin Extrude for a wall.
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- **Don't** assume a symmetric distance is the distance on each side. New
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symmetric extrusions use the total distance; older saved designs can retain
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their earlier convention.
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- Taper with a two-sided or symmetric extent is not supported. A very steep
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taper can also be refused rather than creating an invalid result.
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#### Examples and community resources
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The bracket starts with a closed L-shaped profile; another extrusion removes
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the two holes. Its dimensions are controlled by design parameters.
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| Resource | What to explore | Author and licence |
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| --- | --- | --- |
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| [Editable bracket recipe](https://github.com/tangency-labs/solidcraft/blob/main/examples/bracket.json) | A complete SolidCraft example using an extrusion, a fillet and a cut. | SolidCraft contributors; MIT OR Apache-2.0. |
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[Contribute a tip, demo, model or screenshot](../dev/command-guides.md) to add a
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reviewed resource beside this explanation.
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#### See also
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{{#command solid.revolve}} turns a profile around an axis.
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{{#command solid.sweep}} carries a profile along a path.
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{{#command sheet.flange}} creates sheet metal with a thickness rule.
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