Modeling features¶

Features are the operations in a part's history, grouped here by what they take as input. Every one is reachable from the F1 command palette, and most show a live semi-transparent preview before you apply them.

Sketch-based features¶

These consume one or more closed sketch profiles.

• Extrude a profile into a solid: symmetric or one-directional, bidirectional, with a boolean mode (add, cut, intersect). An extrude inside an existing body becomes a pocket automatically, and a cut uses the entered distance as depth with the inward direction inferred. Through all drops that depth and clears the whole body, for the first direction only, so a second direction still stops at its own distance.
• Revolve a profile around an axis (origin axis, selected edge or datum axis), with an angle and boolean mode.
• Loft between multiple profiles. The panel shows each profile's regions so you pick one per profile.
• Sweep a profile along a path, both from sketches.
• Rib thickens a sketch profile into a thin support wall and unions it with the part. Draw an open chain (offset to a wall of the chosen thickness) or pick a closed region; the wall grows along the sketch normal, one side, the other or symmetric, and is auto-sized and clipped so it never pokes through the far face. Needs an existing solid to stiffen.

Face and edge modifications¶

These act on existing solid geometry and are topologically anchored, so they re-resolve on rebuild.

While a tool picks a face (thread, hole, shell, draft), only faces are selectable, so clicking just inside a hole selects the wall or bottom face instead of snapping to the rim. Edge tools (fillet, chamfer) are the reverse. This also makes edges easier to hit on dense parts, since the pick lands on the edge under the cursor rather than the nearest one in 3D.

• Fillet (edge): constant or variable radius, multi-edge.
• Chamfer (edge): distance, distance-and-angle or edge-length.
• Shell (face): hollow a solid to a wall thickness, optionally removing selected faces.
• Draft (face): a draft angle about a neutral plane.
• Thread (cylindrical faces): a real helical thread, internal or external, with ISO metric / UNC / UNF presets or a custom pitch. Select several faces to thread them all with the same pitch and handedness in one feature; a face already selected when you open the tool is carried in. Set a start and/or end depth to thread only part way down a hole, measured from a planar reference face you pick or from the open end. The smooth section above an internal thread's start is widened to the thread diameter so a bolt can pass through and reach it.
• Hole (planar face): click to place, in simple / counterbore / countersink modes, blind or through-all, with ISO clearance or tap-drill sizing. When editing, drag the on-face X/Y arrows to reposition it or type the coordinates. By default it drills along the face normal; set a Direction (a planar face for its normal, or a datum axis, origin axis or edge) to drill along something else, for example a hole placed on a wedge's slanted face but drilled perpendicular to the base. With a direction set the hole is auto-extended opposite the drill so uphill material does not cap the opening; Back clearance overrides that reach (blank = auto, 0 = off) while depth still governs how far it drills inward.
• Surface pattern (face): displace a face with a math function, smooth (fitted B-spline) or faceted.
• Text emboss (face): raise or engrave text with bundled fonts, alignment, rotation and a mirror toggle. Curved faces wrap conformally, with a toast warning that the preview may be slow.

Patterns and decomposition¶

• Linear pattern: array along a direction with count and spacing.
• Circular pattern: array around an axis with count and total angle.
• Mirror: mirror the body about a plane. The operation picker decides what happens where the copy meets the original: a new body (default), add, cut or intersect.
• Split: divide a solid into separate bodies by a plane, choosing which pieces to keep.

Mirror, split and datum planes define their plane the same way and show it in the viewport while you set it up, with a drag handle for the offset.

Datums¶

Datum planes and axes are reference features that sketches, patterns, mirrors, splits and mates can use.

• Datum plane: offset from a plane, midplane between two parallel planes, through 3 points, at an angle to a plane about an axis, or perpendicular to an axis or edge. Flip reverses the normal, and the offset and angle accept expressions.
• Datum axis: two-point, from a cylindrical or conical face, plane intersection, or a reference line.

Repairing failed references¶

Face and edge features (fillet, chamfer, shell, draft, thread, surface pattern) store anchors, geometric signatures of what they act on, and re-resolve them on every rebuild. Sometimes that fails: the upstream geometry was deleted or reshaped so the edge no longer exists, or several candidates are too close to tell apart. The feature then enters an unresolved reference state and everything downstream is held stale.

Its edit panel then shows a Repair button, opening a list of each unresolved anchor with its candidates, scored and highlighted in the viewport (the best match pre-selected and shown brightest). Pick the right one for each anchor and press Repair; they are applied one at a time, rebuilding between each.

Tick fix similar elsewhere first to also correct the same broken reference on other features. The count is reported once the repair completes.

If the model is rebuilt elsewhere while the panel is open, the candidate list refreshes, so you never repair against a stale state.

Re-applying a warned feature¶

Extrude, revolve, rib, sweep and loft remember which areas of a sketch they were built from. Edit that sketch enough and the remembered area can no longer be identified with certainty: the feature still builds, against the closest match the rebuild could find, and is flagged with a warning saying so.

Open the feature and the viewport shows which areas it is using now. If those are right, the panel's primary button reads Re-apply and is enabled even though you changed nothing; pressing it commits the areas as shown, re-anchors them and clears the warning for good. If they are wrong, re-pick the areas and the button goes back to Apply.

Re-apply is offered only where it helps. A fillet that failed to build, an imported body with open edges or a sketch with dangling curves keeps Apply disabled, because committing again would produce the same result. Those warnings mean fix the geometry, or use Repair / Use best guess for a lost reference.

Simplified display pin¶

Threads, embossed text, surface patterns and small fillets or chamfers count as detail and are hidden when simplified display is on. Open one of those features to override that with Simplified display:

• Auto: follow the rule (the default).
• Hide: always drop this feature in simplified display, whatever its size.
• Keep: always draw it, for example a functional 1 mm fillet.

The pin only affects display. The feature stays in the model and in every export, measurement and simulation either way.

Deleting features and sketches¶

Deleting is best-effort. Removing a feature takes out only that feature; removing a sketch also takes out the features built directly on it, since an extrude or revolve cannot exist without its profile. Anything downstream that can no longer compute is flagged in the tree rather than deleted for you, so you decide whether to repair or remove it. Deletes are undoable.