Sketches and Extrusion

Sketches keep editable planar geometry that you can use to create an extruded shape.

Create a sketch

1. Open the outliner's Sketches tab.
2. Right-click a standard plane and choose its New Sketch on ... action.
3. For a custom construction plane, use New Sketch on Plane on that plane.
4. To reopen an existing sketch, use its Edit Sketch context action.

Use Back To Plane to return the camera to the sketch plane after orbiting.

Draw geometry

Construction Line creates reference geometry. Construction geometry helps define a sketch but does not become the boundary of an extruded region.

With Rectangle active, open Quick Ops (Q) and choose Corner or Center. Center mode previews the full width and height symmetrically around the first point. The rectangle includes a construction diagonal whose midpoint is its center. Snapping that first point to the origin with Auto Constraints enabled keeps the center at the origin when you change the side dimensions. A freely placed center is still movable. The diagonal does not split the extruded region.

Finish or cancel an open drawing gesture before extruding. If an unfinished draft prevents the action, follow the viewport message.

Edit points and curves

Expand a sketch in the outliner's Sketches tab to see its individual elements. Click a name to select an element; Ctrl adds or removes elements and Shift selects a range. The selection is shared with the sketch viewport.

Use the Visible checkbox to show or hide an element. Clicking a selected row's checkbox applies the same visibility to all selected rows, without changing the selection or active element. Clicking an unselected row's checkbox changes only that row. Hiding a whole sketch preserves each element's individual visibility. Visibility supports Undo/Redo and is saved with the project; hidden elements remain editable geometry but are excluded from viewport picking and snapping.

Choose Edit under Modify, or press M. Hover over an endpoint, corner, or circle/arc center to highlight that point; hover over a curve to highlight the complete line, circle, or arc. Click to select the highlighted item. The move gizmo appears immediately at the selection.

Drag a selected item to move it freely, or drag a gizmo axis to constrain movement. Hold Ctrl while clicking to add or remove items. Points and complete curves can be selected and moved together. Ctrl+Drag adds enclosed curves and individual points from partially enclosed curves. Dragging an empty area starts a new selection rectangle.

Connected endpoints remain connected, and existing constraints remain active. Esc cancels a drag; otherwise it clears the editing selection. Undo and Redo restore geometry changes. Escape from a drawing tool returns to Edit after cancelling any unfinished draft.

The toolbar highlights one active tool across all categories. Quick Ops (Q) shows only options for that tool: Edit and drawing tools offer Grid Snap, and Rectangle also offers Corner / Center. Tools without their own options, such as Trim and Fillet, hide the panel. Dimension and constraint visibility remains in the sketch settings.

Add dimensions and constraints

Select geometry to edit its properties. Double-click a displayed dimension to edit it. Length and radius values act as persistent driving dimensions.

A line with a driving length dimension shows that value once; the extra selection length label is omitted. Tab opens the existing length dimension for editing. An undimensioned line keeps its editable selection label. Horizontal or vertical dimensions replace the length label only for lines aligned with that axis; a diagonal line's total length remains a separate value.

Auto Constraints is enabled by default for new geometry. Hold Alt while drawing to suppress it for the gesture. A geometric snap can create a persistent endpoint connection when auto constraints are enabled; existing unconnected endpoints are not retroactively joined.

Use the selection context menu for available constraints. Conflicting edits are rejected without replacing the existing sketch. Undo and Redo apply to sketch edits.

The sketch settings offer three Constraints display modes:

• On Selection (default): show geometric relationships for the selected point or curve.
• All: show all geometric relationships for inspection.
• Off: hide the symbols while keeping the relationships active and accessible in Properties.

Normal symbols use a neutral color. Nearby symbols form a badge with a count; click it to choose an individual relationship from a readable list. Hovering a relationship highlights its participating geometry. The constraint list in Properties also supports hover and selection, and its selection follows the viewport. Select a relationship and press Delete, or use its delete button in Properties. Undo restores it. Changing display mode does not modify the sketch; dimension visibility has its own setting.

Trim or round a corner

Trim removes the clicked segment of a line, arc, or circle between intersections or endpoints. Hover to see the entire segment highlighted in red, with markers at its boundaries, then click anywhere on that segment to remove it. The cursor selects the segment; it does not define a new cut point. An isolated line or circle is removed completely. Undo restores the edit.

Fillet rounds a connected corner. The original virtual corner can remain represented by construction geometry, allowing its original dimensions to keep controlling the sketch.

Click each remaining sharp corner to round it. Center-rectangle diagonals and construction references from earlier fillets do not block corner selection, including when reference geometry is selected. The radius must fit the remaining straight segments.

To change an existing fillet, switch to Edit (M) and select its arc in the viewport or under the sketch in the Outliner. Change Radius in Properties → Item, or double-click its radius dimension in the viewport. You can adjust it repeatedly; the adjoining lines follow the new tangent points while the original dimensions remain in control. Undo and Redo restore the radius and connected geometry together.

Offset curves

Choose Offset under Modify. Existing curve selections are carried into the tool, or click curves directly in the view to select them. By default, each click selects or deselects only that element. Construction lines are ignored both in the selection and when picking overlapping curves.

Enable Select chain in QuickOps to select the whole connected contour with one click on a side or fillet. Enabling it also completes an existing partial selection. Clicking a selected chain deselects that chain; Clear resets the selection. Turn Select chain off to pick individual curves again. The option follows shared endpoints without changing or merging geometry; separate contours and branching selections still require a more specific selection.

Set Distance / side in QuickOps in the project units. Closed contours offset outward by default; Flip direction offsets inward. Open chains offset to one side, with Flip changing the side. Both directions generates both sides at once: a distance of 5 mm produces a 10 mm wide band between them.

The orange curves are the selected originals and the blue curves show the proposed offsets. Apply in QuickOps (or Enter) adds editable lines, arcs and circles while keeping the originals. Cancel or Esc discards the preview and returns to Edit; one Undo removes the entire offset operation. Offsets are independent copies, so later changes to the original do not automatically update them.

For a closed contour, when an inward offset exceeds the radius of a convex fillet between two tangent straight sides, that rounded corner becomes a sharp corner. Larger fillets remain rounded. Collapsed circles, other unsupported arc collapses, vanishing contours and self-intersections are rejected; reduce the distance or choose a simpler chain. Use Extrude to select the resulting center or bands. For a band across both sides of the original, select both adjacent bands together.

Extrude a region

1. Create a closed region, optionally with inner contours.
2. Click Extrude.
3. Click the desired areas directly in the view, then Apply in QuickOps or press Enter. Orange areas are selected; clicking again deselects them. A single area is preselected. Cancel or Esc returns to Edit.
4. The shape starts flat at Depth 0, with a visible depth handle beside the Move gizmo. Drag the handle or set Depth in Properties to extrude. A negative depth reverses direction; setting it back to 0 returns to the flat profile.
5. Choose Add in the shape's Actions Panel to create a new object, or choose the intended boolean operation, then apply the shape.

A single region can be used directly. With nested contours, both the center and the surrounding bands are selectable. Select adjacent areas together to combine them into one extrusion; their shared boundaries disappear. Disconnected areas require separate extrusions. Unselected enclosed areas remain holes.

Switching to Objects also starts a newly selected profile flat. New profiles start at zero regardless of the depth used for a previous extrusion.

The shape's pivot is the center of its bounding box in the sketch plane, including for profiles with holes. Changing extrusion depth keeps that pivot in place, and the created object inherits it.

Return to the source sketch

Use Edit Source Sketch from the extrusion properties to reopen the sketch. Already created bodies remain independent objects; later sketch edits do not automatically rebuild them.

See Shapes and Placement for the shape confirmation workflow.