Solid features

For prerequisites, a readable options table and a first example, open the practical Extrude guide.

Features live on the timeline and rebuild incrementally from the first one that changed. Each one can be edited (double-click), suppressed, renamed, reordered (if nothing it depends on moves after it), rolled back to, and deleted. Deleting asks first when other features depend on it.

Step by step

The sketch from Sketching step by step becomes an open box: extruded, hollowed, its rim rounded, holes added round the tube, then made taller from the timeline. In each dialog, Enter is the same as OK.

1. Extrude. Click Extrude, then the sketch’s profile: a preview appears with an arrow. Drag the arrow, or type the distance (12) and press Enter.

2. Shell. Click Shell, then the face to leave open (the top). Keep the 2 mm wall and press Enter.

3. Fillet. Click Fillet, then the four outer top edges, type the radius (1.5) and press Enter. Rounding after the shell keeps it simple: Shell doesn’t have to follow the rounds.

4. Hole. Click Hole, then the box’s floor beside the tube: the hole goes where you click. Set Diameter to 4 and click OK. Its distance from two edges can be set too (below).

5. Pattern. Open the Arrange panel and choose Circular Pattern. Set Object Type to Features and click Hole1 on the timeline; for Axis, click the tube’s rim. Type 4 for the quantity and press Enter: four holes, evenly round the tube.

6. Change it. Double-click Extrude1 on the timeline: the model rolls back to it and its dialog opens. Type 20 and press Enter. Everything after it (shell, fillet, hole and pattern) rebuilds on the taller block.

The features

Quick measurement (off by default; turn it on under Preferences › Interface): with edges, faces, sketch curves or points selected, the view’s bottom right corner, above History, shows what they measure: an edge’s length (Ø and R for a round one), a face’s area and perimeter, a point’s position, two items’ distance and angle, several edges’ or faces’ total. A click copies it. The Measure tool (I) does more.

Extrude, Revolve, Sweep, Loft, Coil and the Box, Cylinder, Sphere and Torus choose their operation from what their material does, until you pick one: Join when it makes one body with a body it touches (a block against a wall, a ring round a hole, a boss meeting only part of a face), New Body when it would be a separate piece, and Cut when it goes into a body (Extrude) or lies inside one (Revolve and the Box, Cylinder, Sphere and Torus). The window finds out by running the Join on a copy of the design in the background, so its choice is what OK makes; it changes only when that check is in, and OK waits for it. An operation you pick stays, and a feature you edit keeps its own. Pipe, Thicken and Boundary Fill start as a New Body. Only shown bodies take part: with some bodies hidden, the feature names the shown ones as its targets, so a hidden body is never joined or cut, and showing it again later changes nothing. Choose the operation automatically (Preferences › Design, on by default) turns this choice off: each window then keeps the operation it opens with, Extrude its own Join or Cut, as before.

A Join you pick whose material touches none of its target bodies still joins it, to the first one as a separate piece, and the feature’s warning says so: “Body1 is now in 2 separate pieces”. Combine joins the bodies it is given without that warning. Changing the default does not alter operations already saved in a design.

Extrude to a picked target (Preferences › Tools, on by default) lets a pick choose the extent. With it on and a profile selected in the solid Extrude dialog, picking a face away from its plane, a curved face, an off-plane vertex or a parallel plane automatically switches Distance to To Object. Coplanar faces still join the profile selection; non-parallel planes are not targets. Clicking into the Profiles box first makes the next picks profiles again, even off the plane. The extent can still be chosen manually. For a new extrusion without start or end offsets or a From Object input, the target also sets the stored distance and one-sided direction, so returning to Distance keeps that reach. Thin Extrude keeps its existing picks. With the setting off, picks only add profiles.

Dragging Extrude’s distance arrow stops at flat faces parallel to the profile that lie over it, such as the far side of the block a cut goes into: once the arrow’s tip comes within a few screen points of such a face, the distance becomes exactly that face’s and the face is outlined. Elsewhere the distance moves in round steps. Hold Alt or Ctrl for a free drag, which stops at neither. Extrude arrow stops at faces (Preferences › Tools, on by default) turns the face stops off; the arrow then moves in round steps only, as before. The distance stays a number; to follow the face when the model changes, use To Object or Through All.

A positive extrude taper slopes the side walls outward, so the profile grows along the extrusion direction and the far end is larger; a negative taper slopes them inward, making the far end smaller. For example, a 10 × 10 mm square extruded 10 mm with taper: "5 deg" has an approximately 11.75 × 11.75 mm far face; with taper: "-5 deg", it is approximately 8.25 × 8.25 mm.

A taper slopes the sides of any profile, sketch text included: lines, arcs and spline or conic curves move in or out together, and a flat tip shorter than the taper closes to a point. On spline and conic sides the slope is approximate: the moved outline is a curve of the same kind within 2 % of the taper’s offset (or 10 µm) of the true one, a curve that turns too much for that being cut into pieces first; where a curve bends tighter than the offset, the offset folds and is smoothed over. A taper steeper than the profile’s details (a stroke, a curve or a gap narrower than it) is refused with that reason; a smaller taper or distance builds. A taper composes with a start offset (a drafted pocket that starts part way up a part): the offset moves the profile along the normal and the sides are drafted from there, so the profile is the section at the start whatever the offset. A taper with a two-sided or symmetric extent is not built yet and says so.

Thin Extrude (thin: true on solid.extrude, the Thin Extrude box in its dialog) builds a wall of constant thickness along sketch curves instead of filling profiles: open chains (a single wall) and closed loops (a ring), lines, arcs, circles, ellipses and splines. In the dialog, a picked profile stands for the curves around it (its outline and its holes). The wall lies on the curves’ centre, inside, outside, or on both sides with two thicknesses (side: center, inside, outside, two_sides with thickness2). A closed loop’s inside is the area it encloses; an open chain’s is the side it bends toward (the inside of a U), and a straight line’s is the left of its first curve as drawn. Curves that meet end to end are one chain whose corners are mitred; walls that cross or meet (a ring and a cross, a honeycomb) become one piece. Every extent, operation and target of an extrude applies, and a taper for walls of straight lines or of whole circles. A wall thicker than the radius of a curve it follows on the inside is refused. Spline walls follow the exact offset within 0.0001 mm.

Editing an extrusion retains its signed distances, From/To Object inputs, taper expressions and explicit body targets. Revolve edits retain world, sketch, explicit-line and model-edge or face axes, both angle expressions and To Object targets. An unchanged All profiles selection continues to include profiles added later. Cancel restores the complete timeline; a successful edit is one undo step, including downstream parameter changes. Editing a placed component previews the edited feature before its downstream history. Cylindrical Emboss profile guides follow the sketch’s chosen occurrence frame.

Newly selected adaptive profiles store complete outer and hole source identities when the entire boundary can be qualified. Changing an ellipse or periodic offset after extrusion can then change its spline span count while keeping the same selected material region. A partial, intersected or ambiguous boundary cannot satisfy that whole-source reference; changing the hole identities also makes it lost. Older curve-span selections retain their exact stored multisets. If an older feature has already lost its profile after subdivision changed, edit the feature and reselect the intended current region to capture the new identity.

New symmetric solid extrusions treat the entered distance as the total thickness and split it evenly around the start plane: 10 mm spans -5 to +5 mm on an XY sketch. Switching from One Side to Symmetric keeps the entered total thickness. Through All still reaches targets in both directions, and Two Sides retains its independent distances. Symmetric extrusions saved before this change keep their original per-side distances when reopened or edited. Selecting another direction in the feature editor uses the current total-distance convention.

New symmetric revolves split the entered angle evenly around the sketch profile, regardless of which way the selected axis points. Two Sides measures the second angle backward and the first angle forward along the sketch-normal sweep direction. Profiles on opposite sides of an axis each use their own sweep direction. Designs saved before format 11 keep their original angular placement when opened, edited or copied; creating another revolve uses the new behavior. To Object follows that same direction for each selected profile, including curved target faces. Pick a target away from the axis so its angular position is defined.

For cylindrical Emboss, select a supported exterior cylinder face and a tangent sketch profile. Deboss cuts radially into the wall. Orthogonal line profiles, including holes and concave outlines, wrap with exact radial walls; the profile must stay clear of seams and ends. Complete cylinders and coaxial sleeves are supported. Capture pending component positions before applying. The feature stores the selected target and author occurrence paths, so edits and reopening retain the chosen instances. Other curved surfaces and free-form profiles remain unsupported. A new Emboss without an explicit face infers a unique eligible supported cylinder; select the face when the target is ambiguous. Older saved features without a face retain their planar placement.

A Hole with Single placement can also sit at distances from up to two straight edges of its face. After picking the face, click Reference 1 and pick an edge, then pick a second one into Reference 2. Each edge gets a Distance row, measured from where you picked; the canvas shows each one as a dimension from the edge to the hole’s centre, with a box beside it. Type a distance in either place and the hole moves so its centre is that far from the edge, measured in the face’s plane. Moving the hole measures the distances again. The hole keeps its distances when the part changes: it follows its edges, and the distances are parameters like its diameter.

A Cylinder placed on a planar face takes reference edges the same way. Select the face, then start Cylinder: it stands where you clicked, and the window has Reference 1 and Reference 2. Pick one or two straight edges of that face; each gets a Distance, measured from where you clicked, which you can also type in the window or in its box on the canvas. The cylinder’s base centre then follows the edges when the part changes, and the distances are parameters like its radius. Edit Feature picks the edges again.

A Hole with Single placement drills where you pick a planar face. A pick on or near a point of a shown sketch that lies on that face, such as a circle’s centre, places the hole exactly at that point, as Multiple placement picks it; Select Other (press and hold) also offers the face where you clicked. The corners of text outlines don’t count, nor do projected points while the sketch hides projected geometry. The hole keeps that place on the face; to have holes follow later edits of the sketch, place them with Multiple.

Two settings under Create Hole in Preferences › Design, both off by default, change how a Single hole is placed:

• Snap to face and edge centres: the face itself offers snap points too: its middle, and the centre of each round edge on it (a boss standing on it, a rounded corner, a hole already in it). While the cursor is over the face they show as small marks; a pick near one, or on or beside one of those round edges, places the hole at that centre, and the mark it takes is named. Hold Alt or Ctrl to place the hole exactly where you click.
• Move holes by clicking or dragging: each placed hole has a handle at its centre. Drag it to move the hole (it snaps when snapping is on), or click it to take the hole out. A pick elsewhere on a face that already has a hole moves the hole there instead of taking it out. Edit Feature shows the handle as well, so a hole can be moved later.

The Hole dialog draws a section through the hole as its options make it (type, extents, drill point, tapped) and puts each size in a field beside the dimension it sets; hovering a field, or typing in it, lights its dimension.

Hole Tap Type is Simple (type the diameter), Clearance (a hole a bolt passes through) or Tapped (a thread). With Clearance, pick the bolt Size (M1.6 to M64) and the Fit (Close, Normal or Loose): the hole takes the ISO 273 clearance diameter, shown in Clearance diameter as a default you can change, the way Tap drill diameter works for a tapped hole; the section shows the bolt’s shank through the hole. Scripts use clearance: "M4" with fit: "normal" on solid.hole. The hole stores its diameter, not the bolt: Edit Feature opens it as a Simple hole of that diameter.

With Hole Type Counterbore and Clearance, Screw head sizes the counterbore for a cap screw: a socket head (ISO 4762) or a button head (ISO 7380-1) of the bolt’s size. It fills Counterbore Ø and Counterbore depth with the head’s diameter and height plus 0.5 mm each side and below; change either to use your own. Scripts use head: "ISO 4762" with clearance on solid.hole.

The Thread feature’s Hand is Right (the default), Left, or Both (a right- and a left-handed groove crossing, as on a reversing screw). Scripts use hand: "left" (or "right", "both") on solid.thread; omitted, a thread is right-handed. Tapped holes are right-handed.

Fillets and chamfers handle straight edges between planar faces, whole smooth loops, runs of neighbouring edges with mitred or spherical corners, and closed chains of curved edges (a rolling ball). See the roadmap’s known limitations for the rest.

Curvature continuous (G2) in the Fillet dialog’s Type blends straight edges between two planar faces with an exact quintic section. The tangent plane and curvature match each side face: curvature goes to zero at both contact rails, unlike a circular G1 fillet. Each end must meet one planar face; perpendicular and sloped planar ends are supported. Curved edges/faces, multi-face ends, and intersecting corner blends are not supported; they return an error, not a G1 fallback. Equivalent Radius sets the same contact setback as a circular fillet (for a right angle, setback equals the entered value); it is not a constant curvature radius. Reduce/Taper to Fit are unavailable for this type.

Scripts and MCP use the same command, for example on a 20 mm box:

{"command": "solid.fillet", "params": {"edges": [[20, 0, 10]], "radius": 2, "type": "curvature"}}

type: "g2" is an alias. Existing fillets still default to circular, constant-radius G1 blends.

Where three or more rounded edges meet at a corner, the Fillet dialog shows Corners: Ball (the default, a piece of the rolling ball’s sphere, tangent (G1) to each round) or Smooth patch (corner: "g2": the corner is set back along each edge and filled with a curvature-continuous (G2) patch, so reflections run through it without a kink). A smooth patch takes Constant radius and Exact fit. Its Setback is how far along each edge from the corner the patch starts, one distance for every corner (setbacks); left empty, it is 1.5 × the radius.

Feature references to faces and edges are stored by name, so an upstream edit that moves geometry keeps them on the right face (see Persistent naming). When a reference can’t be found, the feature warns instead of silently picking another face.

Plane Along Path accepts one sketch curve (including a drawn 3D wire) or model edge. Pick the path in the viewport and enter Position (0 to 1): 0 starts the path, 1 ends it, and 0.5 places the plane halfway along its length. The plane is perpendicular to the path’s local segment. Preview does not change the design; OK creates one editable timeline feature. The plane follows later path edits. Curved paths use their sampled polyline; absolute distance, reference-object placement and multi-curve chains are not yet available in this dialog.

Comparing two bodies

Compare Bodies (inspect.compare) lays two versions of one part over each other, such as a part and the same part exported by another program, and finds the places where only one of them has material. It works from the two surfaces, not from a boolean of the bodies, so it also compares bodies that share almost every face, the case a boolean (Combine, Interference) handles worst.

{"command": "inspect.compare", "params": {"a": "Bracket", "b": "Bracket (2)", "tolerance": 0.01, "color": true}}

Without a and b it compares the two selected bodies, or the design’s only two. Both bodies are measured (volume, area, centre of mass and box, and difference: b − a of each). Each surface is sampled at the corners of its triangles and at points at most spacing (0.5 mm) apart on larger faces, and every sample measures its distance to the other surface: deviation gives the largest and the mean distance each way. Samples further than tolerance (0.01 mm) form the regions: only_in_a where a has material and b has none, only_in_b the other way round. Each region gives its volume, the deviating surface area, the largest deviation and where it is, its centre and box, and the faces of each body it lies on (faces_a, faces_b, numbered as model.faces lists them), largest volume first. The volume, centre and box are exact (measured_by: "boolean"): the pieces of the cut a − b (or b − a) that lie in the region, measured as inspect.measure measures a body. When the cut cannot be made, the region’s volume and centre are not measured (measured_by: "not measured", null values, not_measured gives the cut’s error), and never estimated; its deviation, area, faces and box are still given, and the side’s total is null. identical is true when no region is found, and verdict says it in one line. warnings lists what makes the result less certain: a body whose surface does not enclose the volume it measures (open, or with faces that failed to import), and a cut that could not be made. With color, the faces that hold a region turn red where only a has material and green where only b has, on both bodies: the faces mostly beyond the tolerance (a small change on a large face leaves the face alone), or, for a region with none, the face with the largest share. That is one undo step; without color the command changes nothing.

The bodies are meshed within a quarter of the tolerance. The kernel meshes no finer than a millionth of a body’s size, so keep the tolerance at least twice that (0.02 mm for a part 10 m across). Large bodies are sampled more coarsely, at about max_points (eight million) points each; sampling.spacing_mm says what was used, and a larger max_points (up to 50 million) samples them finer, at the cost of time.

When editing an Extrude in the UI, the Browser’s bodies, sketches, construction objects and feature rows follow the history marker before that feature. Later objects return when editing ends. Rolling back manually keeps feature rows listed, so they remain available to edit. A hidden body supplying the profile’s face is shown temporarily during the edit, including when a folder or component hides it. OK, Cancel and Escape end that display override; the body’s saved visibility and unrelated visibility changes are preserved.

Editing a feature from a script

For solid.pattern.circular, axis accepts X, Y, Z, {origin, dir}, or an edge or round face of the model, {edge: [x, y, z]} or {face: [x, y, z]} (a point on it). An explicit origin must contain three finite numeric coordinates in millimetres ([x, y, z] or {x, y, z}); omitting it uses the world origin. Expressions and construction-axis references are not supported. Invalid origins are rejected rather than silently replaced with zero.

Axes and points on round edges and faces

Wherever a 3D command takes an axis (Revolve, Surface Revolve, Circular Pattern, Plane at Angle, and Move’s Rotate) you can pick a circular edge, which gives the axis through its centre along its normal, or a cylinder, cone or torus face, which gives that surface’s axis. Hovering one in an axis input draws the axis as a dashed construction line, and the line stays drawn once the axis is picked. Flat faces and edges that are neither straight nor circular can’t be picked there.

Revolve, Surface Revolve, Circular Pattern and Plane at Angle keep the picked edge or face as a reference ({edge: [x, y, z]} or {face: [x, y, z]} from a script), found again by its persistent name every time the design is evaluated. If a parameter moves the cylinder, the feature turns about it where it is now. The axis always points the same way, with its largest component positive, so a rebuild that reverses the edge doesn’t flip the turn. Straight edges picked as axes keep working as before, as a fixed line.

Where a 3D command takes a point (the construction points, axes and planes built from points, Revolve and Extrude’s To Object, a surface patch’s pass-through points, and Move’s pivot and points), a circular edge stands for its centre. A hovered circle shows a small star at its centre. A construction point keeps the edge, so it follows the circle’s centre as the model changes.

timeline.inspect {feature} returns a feature’s definition: the fields timeline.edit changes, with their current values. timeline.edit {feature, set} merges set into that definition (objects are merged field by field, anything else replaces the value), rebuilds the feature and reports recomputed and restored. The feature’s type cannot change, and sketch geometry is edited with the sketch commands. Expressions are text ("30", "30 mm", "width / 2", "45 deg"); a bare number is a length in the design’s units, or degrees for an angle.

{"command": "timeline.inspect", "params": {"feature": "Slab"}}
→ {"type": "extrude", "type_name": "ExtrudeFeature",
   "definition": {"sketch": 1, "profiles": {"type": "all"}, "operation": "new_body",
                  "extent": {"distance": "10", "direction": "positive"}},
   "inputs": [{"label": "Distance", "param": "d1", "expression": "10", "unit": "mm"}], …}
{"command": "timeline.edit", "params": {"feature": "Slab", "set": {"extent": {"distance": "12"}}}}

inputs lists the feature’s named inputs. parameters.change {name: "d1", expression} sets one of those directly. Optional fields that are not set do not appear in the definition; they can still be added through set. The fields of the common features:

For any other feature, timeline.inspect shows the fields.

Where a command takes a face as a point (face.delete, solid.shell, solid.draft, solid.offset_face, solid.split_face, the faces of solid.replace_face, and the face of sheet.convert), a script can give the face’s name instead, as model.faces lists it: {"command": "face.delete", "params": {"faces": ["F2:side#1", "F2:side#2"], "body": "Plate"}}. model.faces also lists a point on each face that picks it (the centroid of a face with a hole in it is in the hole, that of a half cylinder inside the cylinder) and, for a cylindrical face, its cylinder: origin and axis of its axis, and radius. A name that is more than one face (the pieces of a split face, or one face of several bodies) is refused; body says which body to look on.

Press Delete on anything selected (bodies, faces, sketches, features, planes, components, canvases). It runs as one undoable step and lists the features that would go with it or fail.

Face Extrude, face Revolve, and Press Pull retain linked generated profiles. When a modified planar face has no construction certificate, these internal profiles use the legacy named-face attachment and projection behavior so upstream edits still update the plane and outline. This compatibility path is private to those modeling tools: newly attached user sketches require a certified face or an explicitly fixed plane. Legacy internal attachments can follow the nearest matching face after topology changes; inspect their result after major upstream edits. Activate the intended occurrence before generating a face profile from a repeated component; capture a separately moved source position before creating a legacy profile across components.

Negative Press Pull across supported aligned prismatic faces retains round through-holes, including after a joined extrusion and in a rotated component occurrence. The cut partitions the current material into axial sections, preserving the hole through undo, redo, and reopen. Walls that cannot be qualified as a parallel extrusion still use the general Boolean path and may report an unsupported coincident-surface operation atomically.