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© Dystr, Inc. · RunMat v0.7.1, Nov 17, 2026

RunMat® is a registered trademark of Dystr, Inc. MATLAB® is a registered trademark of The MathWorks, Inc. RunMat is not affiliated with, endorsed by, or sponsored by The MathWorks, Inc.

/
    • The design language
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    • Agent tools and the command line
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    • Design commands
Docs>CAD

Design commands

design_propose_edit runs one of these commands: give its id as command and its fields as values, one per field id. A pick field takes the item's reference text or Outline id as its value, for example {"command": "part.sketch", "values": {"plane": "origin.xy"}}. A command that runs on existing items also takes them in selection (feature:boss, component:R1). Numbers are in the unit shown. A field marked when applies only while another field has that value.

Plane picks take an origin plane (origin.xy, origin.yz, origin.zx), a datum plane (plane.<name>) or a planar face (feature.body.face.end). Writing the file's text with replace or text works for any change; see design/mcad/part/features.md and design/ecad/circuit for the syntax.

This file is generated from the command catalog.

assembly. commands (.assembly)

  • assembly.bom: Show the bill of materials: top level, indented or parts only.
    • Required: type (one of top, indented, parts, default top)
  • assembly.clearance: Find components closer than a clearance.
    • Required: minimum (number in mm, default 2)
    • Optional: components (picks: component)
  • assembly.component-configuration: Use another configuration of the component's file.
    • Required: configuration (text)
    • Runs on the selection: occurrence
  • assembly.delete: Delete components or mates.
    • Runs on the selection: occurrence, mate
  • assembly.edit-mate: Change the mate's type, distance, angle, limits or alignment.
    • Required: type (one of fasten, revolute, slider, cylindrical, planar, ball, parallel, distance, angle, tangent, pin_slot, gear, rack_pinion, screw, cam, width, symmetric, path, linear_coupler, hinge, universal_joint, default fasten); offset (number in mm, default 0) when type is distance; angle (number in deg, default 0) when type is angle; min (number in deg, default -30) when angle_limits is true; max (number in deg, default 45) when angle_limits is true; near (number in mm, default 0) when distance_limits is true; far (number in mm, default 10) when distance_limits is true; ratio (number, default 1) when type is gear or linear_coupler; pitch (number in mm, default 1) when type is screw or rack_pinion; radius (number in mm, default 5) when type is tangent; profile (text) when type is cam
    • Optional: angle_limits (true or false, default false) when type is revolute or cylindrical or hinge; distance_limits (true or false, default false) when type is slider or cylindrical; flip (true or false, default false); first2 (pick: mate connector or face or edge or vertex or plane or axis or point or component) when type is width; second2 (pick: mate connector or face or edge or vertex or plane or axis or point or component) when type is width; plane (pick: mate connector or face or edge or vertex or plane or axis or point or component) when type is symmetric; path (picks: edge) when type is path; joint_point (true or false, default true) when type is universal_joint
    • Runs on the selection: mate
  • assembly.export: Export as a STEP assembly, glTF or USD.
    • Required: format (one of step, gltf, usd, default step)
    • Optional: hidden (true or false, default false)
  • assembly.fix: Fix a component in place, or let mates move it.
    • Required: components (picks: component); state (one of fixed, float, default fixed)
    • Runs on the selection: occurrence
  • assembly.flip-mate: Flip the mate's alignment.
    • Runs on the selection: mate
  • assembly.insert: Insert a part, assembly or circuit board from the project.
    • Required: source (one of part, assembly, circuit, default part); file (text); quantity (whole number, default 1); x (number in mm, default 0); y (number in mm, default 0); z (number in mm, default 0)
    • Optional: configuration (text); fix (true or false, default false)
  • assembly.interference: Find components that overlap.
    • Optional: components (picks: component); fasteners (true or false, default false)
  • assembly.mass-properties: Mass, center of mass and inertia of the assembly.
    • Optional: components (picks: component)
  • assembly.mate: Constrain two components: standard, advanced and mechanical mates, with limits.
    • Required: type (one of coincident, concentric, distance, angle, parallel, perpendicular, tangent, fasten, revolute, slider, cylindrical, planar, ball, pin_slot, gear, rack_pinion, screw, cam, width, symmetric, path, linear_coupler, hinge, universal_joint, default coincident); first (pick: mate connector or face or edge or vertex or plane or axis or point or component); second (pick: mate connector or face or edge or vertex or plane or axis or point or component); offset (number in mm, default 0) when type is distance; angle (number in deg, default 0) when type is angle; min (number in deg, default -30) when angle_limits is true; max (number in deg, default 45) when angle_limits is true; near (number in mm, default 0) when distance_limits is true; far (number in mm, default 10) when distance_limits is true; ratio (number, default 1) when type is gear or linear_coupler; pitch (number in mm, default 1) when type is screw or rack_pinion; first2 (pick: mate connector or face or edge or vertex or plane or axis or point or component) when type is width; second2 (pick: mate connector or face or edge or vertex or plane or axis or point or component) when type is width; plane (pick: mate connector or face or edge or vertex or plane or axis or point or component) when type is symmetric; profile (text) when type is cam; path (picks: edge) when type is path
    • Optional: flip (true or false, default false); angle_limits (true or false, default false) when type is revolute or cylindrical or hinge; distance_limits (true or false, default false) when type is slider or cylindrical; joint_point (true or false, default true) when type is universal_joint
    • Runs on the selection: occurrence
  • assembly.mirror: Mirror components about a plane, as copies or as an opposite-hand part.
    • Required: plane (pick: plane or face); components (picks: component); result (one of copy, opposite, default copy); opposite (text) when result is opposite
  • assembly.move: Move components by dragging, with a triad or by aligning.
    • Required: mode (one of drag, triad, align, default drag); components (picks: component); dx (number in mm, default 0) when mode is triad; dy (number in mm, default 0) when mode is triad; dz (number in mm, default 0) when mode is triad; rx (number in deg, default 0) when mode is triad; ry (number in deg, default 0) when mode is triad; rz (number in deg, default 0) when mode is triad; along (pick: edge or axis or face) when mode is align
    • Optional: collisions (true or false, default false)
  • assembly.new-part: Create a part inside the assembly, referencing its neighbors.
    • Required: name (text)
    • Optional: plane (pick: plane or face)
  • assembly.pack-and-share: Collect the assembly and every file it references.
    • Required: folder (text)
  • assembly.pattern: Repeat components in a line, a circle, or by a part's feature pattern.
    • Required: layout (one of linear, circular, feature, default linear); components (picks: component); direction (pick: edge or axis or face) when layout is linear or circular; spacing (number in mm, default 20) when layout is linear; angle (number in deg, default 360) when layout is circular; instances (whole number, default 3) when layout is linear or circular; feature (pick: feature) when layout is feature
    • Runs on the selection: occurrence
  • assembly.replace: Replace components with another file; mates follow where they can.
    • Required: components (picks: component); with (text)
    • Optional: remate (true or false, default true)
    • Runs on the selection: occurrence
  • assembly.smart-mate: Drag a component onto another and accept the suggested mate.
    • Required: component (pick: component); target (pick: mate connector or face or edge or vertex or plane or axis or point or component)
  • assembly.subassembly: Form a subassembly from components, dissolve one, or make it flexible or rigid.
    • Required: action (one of form, dissolve, flexible, rigid, default form); components (picks: component); name (text) when action is form
    • Runs on the selection: occurrence
  • assembly.suppress: Leave components out of this configuration.
    • Runs on the selection: occurrence, mate
  • assembly.where-used: List where a component's file is used.
    • Runs on the selection: occurrence

board. commands (.circuit, .circuit.layout)

  • board.autoroute: Route the unrouted connections of the picked nets, or of every net not on a plane.
    • Required: width (number in mm, default 0.2); via (text)
    • Optional: nets (picks: net); layers (text)
  • board.capability: Load a board-house capability set: the fabrication limits every design rule falls back to.
    • Required: capability (one of standard, advanced, hdi, default standard)
  • board.copy-room-formats: Copy one channel room's placement and routing into the other channels' rooms.
    • Required: source (pick: room)
    • Optional: targets (picks: room); placement (true or false, default true); routing (true or false, default true); pours (true or false, default true); room_shape (true or false, default true); rotate (true or false, default false)
    • Runs on the selection: room
  • board.diff-pair: Route a differential pair together, at its gap from pad to pad.
    • Required: pair (pick: net)
    • Optional: width (number in mm); gap (number in mm); layer (text)
  • board.dimension: Add a board dimension annotation.
    • Required: layer (text)
    • Optional: points (picks: point); items (picks: pad or track or via or component)
  • board.export: Export the board and its components as a STEP model for mechanical design.
    • Optional: copper (true or false, default false); mask (true or false, default true)
  • board.fab-outputs: Make the fabrication and assembly files for the board.
    • Required: preset (one of fab_house, assembly, full, custom, default fab_house)
  • board.fanout: Fan out a component's pads to vias: BGA balls to the diagonals, other pads past their outer end.
    • Required: component (picks: component); via (text)
    • Optional: nets (picks: net); signals (true or false, default false)
  • board.fill: Draw a solid copper fill.
    • Required: points (picks: point); layer (text)
    • Optional: net (pick: net)
  • board.flip: Move components to the other side of the board, mirrored where they stand.
    • Required: components (picks: component)
  • board.keepout: Draw an area where copper, vias or components may not go.
    • Required: points (picks: point); applies (one of all, copper, tracks, vias, components, default all); layer (text)
  • board.layer-stack: Edit the stackup, with the impedance calculator and thermal properties.
    • Required: layers (whole number, default 4); material (text); thickness (number in mm, default 1.6)
    • Optional: target_z (number in ohm, default 50)
  • board.lock: Lock components or copper so they don't move.
    • Runs on the selection: component, track, via, zone
  • board.move: Move components or copper; tracks follow where they can.
    • Required: items (picks: component or track or via or pour); dx (number in mm, default 0); dy (number in mm, default 0); rotation (number in deg, default 0)
  • board.outline: Draw the board outline, or take it from an enclosure part.
    • Required: source (one of draw, enclosure, default draw); points (picks: point) when source is draw; part (text) when source is enclosure; face (pick: face) when source is enclosure
  • board.place-via: Place a via.
    • Required: points (picks: point); size (text); span (one of through, blind, buried, micro, default through)
    • Optional: net (pick: net)
  • board.pour: Draw a copper pour, repour, shelve or split a plane.
    • Required: action (one of draw, repour, shelve, split_plane, default draw); net (pick: net) when action is draw or split_plane; points (picks: point) when action is draw; layer (text) when action is draw or split_plane; clearance (number in mm, default 0.25) when action is draw; connect (one of relief, relief-tht, solid, none, default relief) when action is draw; priority (whole number, default 0) when action is draw
  • board.room: Define a room that keeps a group of components together.
    • Required: name (text); components (picks: component)
    • Optional: points (picks: point); keep_inside (true or false, default true)
  • board.route: Route a track interactively; walkaround now, push and shove later behind the same button.
    • Required: net (pick: net or pad or track or via); points (picks: point); width (number in mm, default 0.15); via (text); layer (text); mode (one of walkaround, ignore, stop, default walkaround); corner (one of 45, 90, arc45, any, default 45)
  • board.route-net: Route the net's open connections with the interactive router.
    • Runs on the selection: net
  • board.stitch: Stitch a pour with vias, or shield a net with a row of them.
    • Required: mode (one of stitch, shield, default stitch); target (pick: pour or net); shield_net (text) when mode is shield; pitch (number in mm, default 1.5); via (text)
  • board.teardrops: Add or remove teardrops at pads and vias.
    • Required: action (one of add, remove, default add)
    • Optional: all (true or false, default true)
  • board.test-points: Add test points on nets.
    • Required: nets (picks: net); side (one of bottom, top, default bottom); diameter (number in mm, default 1)
  • board.tune-group: Tune every short member of a matched-length group to the group's target length or delay.
    • Required: group (text); pattern (one of trombone, accordion, sawtooth, default trombone)
  • board.tune-length: Add meanders to a net's longest straight track until it meets its target length or delay.
    • Required: net (pick: net or track); basis (one of length, delay, default length); target (number in mm, default 50) when basis is length; tolerance (number in mm, default 0.1) when basis is length; target_delay (number in s) when basis is delay; pattern (one of trombone, accordion, sawtooth, default trombone)
    • Optional: tolerance_delay (number in s) when basis is delay
  • board.update-schematic: Send board changes (renumbering, pin and gate swaps, footprints) back to the schematic; review each line.
    • Required: changes (picks: change)
    • Runs on the selection: eco_back_change

direct. commands (.part)

  • direct.delete-face: Delete faces and heal the gap from the neighbors.
    • Required: faces (picks: face); heal (one of heal, patch, leave, default heal)
  • direct.move-body: Move or rotate bodies directly.
    • Required: bodies (picks: body); dx (number in mm, default 0); dy (number in mm, default 0); dz (number in mm, default 0); angle (number in deg, default 0)
    • Optional: axis (pick: axis or edge)
  • direct.move-face: Move or rotate faces; neighboring faces follow. Recorded as a feature.
    • Required: faces (picks: face); motion (one of translate, rotate, normal, default translate); distance (number in mm, default 1); direction (pick: edge or axis or plane) when motion is translate; axis (pick: axis or edge) when motion is rotate; angle (number in deg, default 0) when motion is rotate
  • direct.offset-face: Offset faces along their normals.
    • Required: faces (picks: face); distance (number in mm, default 1)
  • direct.pull: Push or pull faces; adds or removes material.
    • Required: faces (picks: face); distance (number in mm, default 1)
  • direct.replace-face: Replace faces with another face or surface.
    • Required: faces (picks: face); with (pick: face)

drawing. commands (.drawing)

  • drawing.align: Line items up on the first one selected.
    • Required: align (one of horizontal, vertical, default horizontal)
    • Runs on the selection: view, annotation
  • drawing.auto: Lay out views, dimensions and tables for a model; fasteners are skipped.
    • Required: model (text); sheet (one of a3, a2, a4, b, d, default a3)
    • Optional: dimensions (true or false, default true); tables (true or false, default true)
  • drawing.auxiliary: Project a view normal to an edge.
    • Required: parent (pick: view); edge (pick: edge); label (text)
    • Optional: at (pick: point)
  • drawing.balloon: Label a component with its BOM item number.
    • Required: attach (pick: edge)
    • Optional: at (pick: point)
  • drawing.baseline: Dimension features from one baseline.
    • Required: base (pick: edge); items (picks: edge)
    • Optional: at (pick: point)
  • drawing.broken-out: Cut away part of a view to show the inside.
    • Required: parent (pick: view); boundary (picks: point); depth (number in mm, default 10)
    • Optional: at (pick: point)
  • drawing.center-mark: Mark the center of circles and arcs.
    • Required: edges (picks: edge)
    • Optional: auto (true or false, default false)
  • drawing.centerline: Draw a centerline between edges or on a cylinder.
    • Required: edges (picks: edge)
  • drawing.chain: Dimension features end to end.
    • Required: items (picks: edge)
    • Optional: at (pick: point)
  • drawing.datum: Add a datum feature symbol.
    • Required: label (text); attach (pick: edge or annotation)
    • Optional: at (pick: point)
  • drawing.datum-target: Add a datum target point, line or area.
    • Required: label (text); shape (one of point, line, circle, rectangle, default point); attach (pick: edge)
    • Optional: size (number in mm, default 5); at (pick: point)
  • drawing.delete: Delete views, annotations or tables.
    • Runs on the selection: view, annotation, table, drawing_dimension, sheet
  • drawing.detail: Enlarge a circled area of a view.
    • Required: parent (pick: view); center (pick: edge); radius (number in mm, default 5); label (text); scale (text)
    • Optional: at (pick: point)
    • Runs on the selection: view
  • drawing.export: Export as PDF, DXF, DWG or SVG.
    • Required: format (one of pdf, dxf, dwg, svg, default pdf); sheets (one of all, current, default all)
  • drawing.gdt: Add a feature control frame.
    • Required: frame (text); attach (pick: edge or annotation)
    • Optional: at (pick: point)
  • drawing.hole-callout: Label a hole with its size, depth and thread from the model.
    • Required: hole (pick: edge)
    • Optional: at (pick: point)
  • drawing.isometric: Place an isometric view.
    • Required: model (text); scale (text); display (one of hidden_removed, shaded, default hidden_removed)
    • Optional: at (pick: point)
  • drawing.model-view: Place one view of a model in any orientation.
    • Required: model (text); orientation (one of front, back, top, bottom, left, right, isometric, default front); scale (text); display (one of hidden_visible, hidden_removed, shaded, default hidden_visible)
    • Optional: at (pick: point)
  • drawing.move: Move views, annotations or tables to a picked point, or by a distance.
    • Optional: to (pick: point); dx (number in mm, default 0); dy (number in mm, default 0)
    • Runs on the selection: view, annotation
  • drawing.note: Add a note, with an optional leader.
    • Required: text (text)
    • Optional: attach (pick: edge or view); at (pick: point)
  • drawing.ordinate: Dimension features from a zero line.
    • Required: origin (pick: edge); items (picks: edge)
    • Optional: at (pick: point)
  • drawing.projected: Project a view from an existing one.
    • Required: parent (pick: view); direction (one of up, down, left, right, default up)
    • Optional: at (pick: point)
    • Runs on the selection: view
  • drawing.section: Cut a section through a view, along a cutting line through a picked edge or hole.
    • Required: parent (pick: view); through (pick: edge); label (text)
    • Optional: aligned (true or false, default false); at (pick: point)
    • Runs on the selection: view
  • drawing.smart-dimension: Dimension edges, points or circles.
    • Required: items (picks: edge); measure (one of auto, linear, angular, radius, diameter, default auto); tolerance (one of none, symmetric, bilateral, fit, default none)
    • Optional: plus (number in mm, default 0.1); minus (number in mm, default 0.1); fit (text); at (pick: point)
  • drawing.standard: Choose the drafting standard.
    • Required: standard (one of iso, asme, default iso)
  • drawing.standard-3: Place front, top and right views of a model.
    • Required: model (text); scale (text); projection (one of third, first, default third)
    • Optional: configuration (text); at (pick: point)
  • drawing.surface-finish: Add a surface finish symbol.
    • Required: ra (text); attach (pick: edge)
    • Optional: at (pick: point)
  • drawing.view-display: Draw the view with hidden lines removed or visible, or shaded.
    • Required: style (one of hidden_removed, hidden_visible, shaded, default hidden_removed)
    • Runs on the selection: view
  • drawing.view-label: Relabel a section, detail or auxiliary view.
    • Required: label (text)
    • Runs on the selection: view
  • drawing.view-scale: Use the sheet scale or a custom scale for the view.
    • Required: scale (one of sheet, 1:1, 1:2, 1:5, 1:10, 2:1, default sheet)
    • Runs on the selection: view
  • drawing.weld-symbol: Add a weld symbol.
    • Required: type (one of fillet, groove, plug, spot, default fillet); size (number in mm, default 4); attach (pick: edge)
    • Optional: all_around (true or false, default false); field (true or false, default false); at (pick: point)

evaluate. commands (.part)

  • evaluate.clearance: Find places closer than a clearance.
    • Required: items (picks: body or face); minimum (number in mm, default 1)
  • evaluate.draft: Color faces by draft angle.
    • Required: direction (pick: plane or face or axis); angle (number in deg, default 1)
  • evaluate.interference: Find bodies that overlap.
    • Optional: bodies (picks: body)
  • evaluate.mass-properties: Mass, volume, area, center of mass and inertia.
    • Required: mass (number in kg, default 1) when override_mass is true
    • Optional: bodies (picks: body or part); about (pick: coordinate system); override_mass (true or false, default false)
    • Runs on the selection: body
  • evaluate.undercut: Find undercut faces for a pull direction.
    • Required: direction (pick: plane or face or axis)

explode. commands (.assembly)

  • explode.lines: Draw lines showing how components move.
    • Optional: steps (picks: explode step)
  • explode.new: Create an exploded view.
    • Required: name (text)
  • explode.radial: Spread components out radially about an axis.
    • Required: components (picks: component); axis (pick: axis or edge); distance (number in mm, default 50)
  • explode.step: Move components along a direction in one step.
    • Required: components (picks: component); direction (pick: edge or axis or face); distance (number in mm, default 50)

library. commands (.circuit, .circuit.layout)

  • library.place: Search the library and manufacturer parts, and place one on the sheet.
    • Required: query (text)
    • Optional: in_stock (true or false, default true); designator (text)

manage. commands (.part)

  • manage.appearance: Set the display color of the part or a body.
    • Required: color (text)
    • Optional: targets (picks: part or body)
    • Runs on the selection: body, part
  • manage.configurations: Add configurations and edit the design table.
    • Required: name (text)
    • Optional: based_on (text)
  • manage.equations: Set an input's value, or add or change a named value or equation.
    • Required: name (text); value (text)
  • manage.export: Export the part as STEP AP242, IGES, STL, 3MF, glTF or a face as DXF.
    • Required: format (one of step_ap242, iges, stl, 3mf, gltf, dxf_face, default step_ap242); face (pick: face) when format is dxf_face; resolution (one of fine, standard, coarse, default fine) when format is stl or 3mf or gltf
    • Optional: pmi (true or false, default true) when format is step_ap242
  • manage.material: Assign a material to the part or a body.
    • Required: material (one of material.aluminum_6061_t6, material.aluminum_7075_t6, material.aluminum_2024_t3, material.steel_1018, material.steel_4140, material.stainless_304, material.stainless_316, material.titanium_ti_6al_4v, material.copper_c110, material.brass_c360, material.abs, material.nylon_pa12, material.glass_filled_nylon, material.pom_acetal, material.peek, material.polycarbonate, material.acrylic, material.carbon_fiber, material.fr4, material.silicone_rubber, material.oak, material.concrete, material.douglas_fir_lumber, material.osb, material.gypsum_board, material.xps_foam, default material.aluminum_6061_t6)
    • Optional: bodies (picks: body or part)
    • Runs on the selection: body, part
  • manage.split-to-files: Save bodies as separate parts and an assembly.
    • Optional: bodies (picks: body); assembly (true or false, default true)

mold. commands (.part)

  • mold.core-cavity: Split a mold block round the part into core and cavity.
    • Required: part (pick: body or face); parting (pick: plane or face); margin (number in mm, default 10)
  • mold.draft-analysis: Color faces by draft angle for a pull direction.
    • Required: direction (pick: plane or face or axis); angle (number in deg, default 1)
  • mold.parting-line: Find the parting line for a pull direction.
    • Required: direction (pick: plane or face or axis or edge); draft (number in deg, default 1)
  • mold.scale: Scale the part for the material's shrinkage.
    • Required: factor (number, default 1.005); fx (number, default 1.005) when uniform is false; fy (number, default 1.005) when uniform is false; fz (number, default 1.005) when uniform is false
    • Optional: uniform (true or false, default true)
  • mold.undercut: Find faces that can't release in the pull direction.
    • Required: direction (pick: plane or face or axis)

part. commands (.part)

  • part.axis: Add a reference axis.
    • Required: type (one of edge, two_planes, two_points, cylinder, point_face, default edge); references (picks: edge or plane or face or vertex or point)
  • part.body-combine: Merge touching bodies into one.
    • Required: bodies (picks: body)
  • part.body-delete: Delete bodies, or keep only the chosen ones.
    • Required: bodies (picks: body); keep (one of delete, keep, default delete)
    • Runs on the selection: body
  • part.body-indent: Press one body into another, leaving a clearance.
    • Required: target (pick: body); tool (pick: body); clearance (number in mm, default 0.5)
  • part.body-move: Move, rotate or copy bodies.
    • Required: bodies (picks: body); dx (number in mm, default 0); dy (number in mm, default 0); dz (number in mm, default 0); angle (number in deg, default 0); copies (whole number, default 1) when copy is true
    • Optional: axis (pick: axis or edge); copy (true or false, default false)
    • Runs on the selection: body
  • part.body-promote: Make a body its own part in this file, with its own number and material.
    • Required: body (pick: body); name (text)
    • Runs on the selection: body
  • part.body-scale: Scale bodies about the origin by one factor.
    • Required: bodies (picks: body); factor (number, default 1)
  • part.boolean: Combine bodies by union, subtract or intersect.
    • Required: kind (one of union, subtract, intersect, default union); target (pick: body); tools (picks: body)
    • Optional: keep_tools (true or false, default false)
  • part.boundary: Make a solid from curves in two directions.
    • Required: direction1 (picks: sketch or curve or edge); op (one of add, remove, intersect, new, default add)
    • Optional: direction2 (picks: sketch or curve or edge); merge (pick: body) when op is add or remove or intersect
  • part.chamfer: Bevel edges, faces, a feature's edges or vertices by distance and angle or two distances.
    • Required: type (one of distance_angle, distance_distance, equal, vertex, default distance_angle); edges (picks: edge or face or feature or vertex); distance (number in mm, default 1); distance2 (number in mm, default 1) when type is distance_distance or vertex; angle (number in deg, default 45) when type is distance_angle
    • Optional: flip (true or false, default false)
  • part.coordinate-system: Add a coordinate system from an origin and axes, or on a planar face.
    • Required: type (one of axes, face, default axes); origin (pick: vertex or point) when type is axes; z (pick: edge or axis) when type is axes; face (pick: face) when type is face
    • Optional: x (pick: edge or axis) when type is axes
  • part.curve-composite: Join edges end to end into one curve.
    • Required: curves (picks: edge)
  • part.curve-equation: Draw a curve from x(t), y(t), z(t).
    • Required: x (text); y (text); z (text); t0 (number, default 0); t1 (number, default 6.283185307179586)
  • part.curve-helix: Add a helix or spiral by pitch, turns and height.
    • Required: type (one of helix, spiral, default helix); axis (pick: axis or edge) when type is helix; start (pick: vertex or point or sketch point) when type is helix; plane (pick: plane or face) when type is spiral; start_radius (number in mm, default 5) when type is spiral; pitch (number in mm, default 2); revolutions (whole number, default 5); taper_step (number in mm, default 0.5) when taper is true
    • Optional: clockwise (true or false, default false) when type is helix; taper (true or false, default false) when type is helix
  • part.curve-intersection: Make the curve where a planar face meets a plane.
    • Required: face (pick: face); plane (pick: plane or face)
  • part.curve-through-points: Fit a curve through points.
    • Required: points (picks: vertex or point or sketch point)
    • Optional: closed (true or false, default false)
  • part.delete: Delete the item, after showing what depends on it.
    • Runs on the selection: feature, sketch, region, input, plane, mate_connector, annotation
  • part.draft: Taper faces for molding by neutral plane, parting line or step.
    • Required: type (one of neutral_plane, parting_line, step, default neutral_plane); faces (picks: face); neutral (pick: plane or face) when type is neutral_plane; parting (picks: edge or curve) when type is parting_line or step; angle (number in deg, default 1)
    • Optional: flip (true or false, default false)
  • part.emboss: Raise or engrave a sketch or text on a face.
    • Required: profile (pick: sketch); face (pick: face); depth (number in mm, default 0.5); mode (one of emboss, deboss, default emboss)
  • part.export-body: Write the selected bodies to a STEP or STL file.
    • Required: format (one of step, stl, default step)
    • Runs on the selection: body
  • part.extrude: Extend a profile along a direction to add, cut or intersect material.
    • Required: profile (picks: sketch region or sketch or face); op (one of add, remove, intersect, new, default add); from (one of sketch_plane, surface, vertex, offset, default sketch_plane); from_face (pick: face) when from is surface; from_vertex (pick: vertex or point) when from is vertex; from_offset (number in mm, default 5) when from is offset; end (one of blind, through_all, up_to_next, up_to_vertex, up_to_face, up_to_plane, offset_from_face, up_to_body, mid_plane, default blind); distance (number in mm, default 10) when end is blind or mid_plane or offset_from_face; up_to (pick: face or vertex or body or plane) when end is up_to_vertex or up_to_face or up_to_plane or offset_from_face or up_to_body; second_end (one of blind, through_all, up_to_next, up_to_vertex, up_to_face, up_to_plane, offset_from_face, up_to_body, mid_plane, default blind) when second_direction is true; second_distance (number in mm, default 10) when second_direction is true; second_up_to (pick: face or vertex or body or plane) when second_direction is true; draft_angle (number in deg, default 0) when draft is true; thin_thickness (number in mm, default 1) when thin is true; thin_side (one of one, mid, two, default one) when thin is true
    • Optional: flip (true or false, default false); second_direction (true or false, default false); draft (true or false, default false); draft_outward (true or false, default false) when draft is true; thin (true or false, default false); merge (pick: body) when op is add or remove or intersect
  • part.fillet: Round edges, faces or a feature's edges, or blend faces: constant, variable, face or full round.
    • Required: type (one of constant, variable, face, full_round, default constant); edges (picks: edge or face or feature); radius (number in mm, default 2) when type is constant or face; radii (list of number in mm, default 2) when type is variable; profile (one of circular, conic, curvature, default circular)
    • Optional: tangent_propagation (true or false, default true)
  • part.hole: Add standard holes: simple, counterbore, countersink, tapped, pipe tap or slot.
    • Required: type (one of simple, counterbore, countersink, tapped, pipe_tap, slot, default simple); standard (one of iso, ansi_metric, ansi_inch, default iso); size (text); fit (one of normal, close, loose, default normal) when type is simple or counterbore or countersink or slot; diameter (number in mm, default 6) when type is simple; cbore_diameter (number in mm, default 11) when type is counterbore; cbore_depth (number in mm, default 6) when type is counterbore; csink_diameter (number in mm, default 12) when type is countersink; csink_angle (number in deg, default 90) when type is countersink; slot_length (number in mm, default 10) when type is slot; end (one of blind, through_all, up_to_next, up_to_face, default blind); depth (number in mm, default 12) when end is blind; thread_depth (number in mm, default 10) when type is tapped or pipe_tap; face (pick: face); positions (list of pick: sketch point or vertex or point)
    • Optional: cosmetic_thread (true or false, default true); series (true or false, default false)
  • part.loft: Blend between two or more profiles, with guides and end tangency.
    • Required: profiles (picks: sketch or sketch region or face or point); op (one of add, remove, intersect, new, default add); start_tangency (one of none, normal, direction, faces, default none); end_tangency (one of none, normal, direction, faces, default none); thin_thickness (number in mm, default 1) when thin is true
    • Optional: guides (picks: sketch or curve or edge); centerline (pick: sketch or curve or edge); closed (true or false, default false); thin (true or false, default false); merge (pick: body) when op is add or remove or intersect
  • part.mate-connector: Add a named frame other files mate to.
    • Required: name (text); on (pick: face or edge or vertex); origin (one of centroid, center, default centroid); offset_x (number in mm, default 0); offset_y (number in mm, default 0); offset_z (number in mm, default 0); rotate (number in deg, default 0)
    • Optional: flip (true or false, default false)
  • part.mirror: Mirror features, faces or bodies about a plane.
    • Required: plane (pick: plane or face); seeds (picks: feature or face or body)
  • part.move-down: Move the feature one place later in the tree.
    • Runs on the selection: feature
  • part.move-up: Move the feature one place earlier in the tree.
    • Runs on the selection: feature
  • part.pattern: Repeat features, faces or bodies: linear, circular, curve, sketch, table, fill or variable.
    • Required: layout (one of linear, circular, curve, sketch, table, fill, variable, default linear); seeds (picks: feature or face or body); direction (pick: edge or axis or plane or face) when layout is linear or fill; spacing (number in mm, default 10) when layout is linear or fill; instances (whole number, default 3) when layout is linear or circular or curve; direction2 (pick: edge or axis or plane) when second_direction is true; spacing2 (number in mm, default 10) when second_direction is true; instances2 (whole number, default 2) when second_direction is true; axis (pick: axis or edge or face) when layout is circular; angle (number in deg, default 360) when layout is circular; curve (pick: curve or edge or sketch) when layout is curve; sketch (pick: sketch) when layout is sketch; table (text) when layout is table or variable; boundary (pick: face or sketch) when layout is fill
    • Optional: second_direction (true or false, default false) when layout is linear; equal_spacing (true or false, default true) when layout is circular; skip (list of whole number, default 1)
  • part.plane: Add a reference plane: offset, angle, 3-point, mid, normal to curve or tangent to surface.
    • Required: type (one of offset, angle, three_point, mid, normal_to_curve, tangent_to_face, default offset); base (pick: plane or face) when type is offset or angle or mid; distance (number in mm, default 10) when type is offset; count (whole number, default 1) when type is offset; axis (pick: axis or edge) when type is angle; angle (number in deg, default 45) when type is angle; points (picks: vertex or point or sketch point) when type is three_point; other (pick: plane or face) when type is mid; curve (pick: curve or edge) when type is normal_to_curve; at (pick: vertex or point) when type is normal_to_curve; face (pick: face) when type is tangent_to_face
    • Optional: flip (true or false, default false)
  • part.point: Add a reference point.
    • Required: type (one of coordinates, center, face_center, intersection, along_curve, default coordinates); references (picks: edge or face or vertex or curve) when type is center or face_center or intersection or along_curve; x (number in mm, default 0) when type is coordinates; y (number in mm, default 0) when type is coordinates; z (number in mm, default 0) when type is coordinates; parameter (number, default 0.5) when type is along_curve
  • part.reorder: Move the feature before or after another one.
    • Required: position (one of before, after, default before); anchor (pick: feature or sketch)
    • Runs on the selection: feature, sketch
  • part.revolve: Turn a profile around an axis.
    • Required: profile (picks: sketch region or sketch or face); axis (pick: axis or edge or sketch entity); op (one of add, remove, intersect, new, default add); type (one of one, mid, two, default one); angle (number in deg, default 360); angle2 (number in deg, default 0) when type is two; thin_thickness (number in mm, default 1) when thin is true
    • Optional: thin (true or false, default false); merge (pick: body) when op is add or remove or intersect
  • part.rib: Add a thin wall from an open sketch.
    • Required: profile (pick: sketch); thickness (number in mm, default 2); depth (number in mm, default 10)
    • Optional: reverse (true or false, default false)
  • part.shell: Hollow a body, with different thicknesses on chosen faces.
    • Required: body (pick: body); thickness (number in mm, default 2); face_thickness (number in mm, default 3) when thick_faces is set
    • Optional: open_faces (picks: face); outward (true or false, default false); thick_faces (picks: face)
  • part.sketch: Start a sketch on a plane or planar face.
    • Required: plane (pick: plane or face)
  • part.split: Split a body with a plane, face or surface.
    • Required: body (pick: body); tool (pick: plane or face or body)
  • part.suppress: Turn the feature off without deleting it.
    • Runs on the selection: feature, sketch
  • part.sweep: Move a profile along a path, with guide curves, twist and tangency.
    • Required: profile (picks: sketch region or sketch or face); path (pick: sketch or curve or edge); op (one of add, remove, intersect, new, default add); orientation (one of follow_path, keep_normal, follow_path_first_guide, default follow_path); twist (one of none, turns, angle, default none); twist_angle (number in deg, default 0) when twist is turns or angle; start_tangency (one of none, normal, default none); end_tangency (one of none, normal, default none); thin_thickness (number in mm, default 1) when thin is true
    • Optional: guides (picks: sketch or curve or edge); thin (true or false, default false); merge (pick: body) when op is add or remove or intersect
  • part.thread: Add a cosmetic thread on a cylindrical face, for drawings and inspection.
    • Required: face (pick: face); standard (one of iso, unified, default iso); designation (text)
    • Optional: length (number in mm, default 10); left_hand (true or false, default false)
  • part.unsuppress: Turn a suppressed feature back on.
    • Runs on the selection: feature, sketch

schematic. commands (.circuit, .circuit.layout)

  • schematic.annotate: Assign designators to parts that have none.
    • Required: order (one of across, down, default across)
    • Optional: reset (true or false, default false)
  • schematic.directive: Attach a directive: differential pair, net class, parameter set or blanket.
    • Required: type (one of diff_pair, net_class, parameters, blanket, default diff_pair); nets (picks: net or wire)
    • Optional: value (text)
  • schematic.disconnect: Take a pin off its net: its wire to the rest of the net goes.
    • Required: pin (pick: pin)
    • Runs on the selection: pin
  • schematic.export-pdf: Export every schematic page, each with its title block, as one PDF.
  • schematic.move: Move selected items; wires stay connected.
    • Required: items (picks: component or wire or port or sheet symbol); dx (number in mm, default 0); dy (number in mm, default 0); rotation (number in deg, default 0)
    • Optional: mirror (true or false, default false); drag_wires (true or false, default true)
  • schematic.net-label: Name a net with a label.
    • Required: name (text); on (pick: wire or net or pin)
    • Runs on the selection: pin
  • schematic.no-erc: Mark a pin so ERC doesn't report it.
    • Required: pin (pick: pin)
    • Runs on the selection: pin
  • schematic.paste: Paste copies of the copied parts under the next free designators.
    • Required: dx (number in mm, default 5.08); dy (number in mm, default -5.08)
    • Optional: items (picks: component)
  • schematic.place-bus: Draw a bus carrying a range of signals.
    • Required: name (text)
    • Optional: from (pick: pin or wire or net or port); to (pick: pin or wire or net or port)
  • schematic.place-harness: Draw a harness that carries an interface (USB, SPI).
    • Required: name (text); interface (text); from (pick: pin or wire or net or port); to (pick: pin or wire or net or port)
  • schematic.place-part: Place a part from the pool.
    • Required: part (text); designator (text); rotation (number in deg, default 0)
    • Optional: value (text); at (pick: point); mirror (true or false, default false)
  • schematic.place-wire: Draw a wire between pins.
    • Required: from (pick: pin or wire or net or port); to (pick: pin or wire or net or port); mode (one of ortho, diagonal, any, default ortho)
    • Optional: path (picks: point); net (text)
    • Runs on the selection: pin
  • schematic.port: Place a port that connects this sheet to its parent.
    • Required: name (text); direction (one of input, output, bidirectional, power, passive, default input)
    • Optional: on (pick: pin or wire or net)
  • schematic.power-port: Place a power or ground symbol.
    • Required: net (text); on (pick: pin or wire or net)
    • Optional: power_flag (true or false, default false)
    • Runs on the selection: pin
  • schematic.repeat-channel: Repeat a sheet as channels with their own designators.
    • Required: symbol (pick: sheet symbol); channels (whole number, default 4)
    • Optional: designators (text)
  • schematic.sheet-entry: Add an entry to a sheet symbol for a port of its sheet.
    • Required: symbol (pick: sheet symbol); port (text)
    • Optional: to (pick: pin or wire or net); bus (text); offset (whole number, default 0) when bus is set
  • schematic.sheet-symbol: Place a child sheet in the hierarchy.
    • Required: name (text); sheet (text); channels (whole number, default 1)
  • schematic.text: Place a note on the sheet.
    • Required: text (text)
    • Optional: at (pick: point)
  • schematic.update-board: Send schematic changes to the board; review each line.
    • Required: changes (picks: change)
    • Optional: ignore_parameters (true or false, default false); ignore_values (true or false, default false); ignore_footprints (true or false, default false); ignore_fitting (true or false, default false); ignore_net_classes (true or false, default false); ignore_rules (true or false, default false); ignore_diff_pairs (true or false, default false); ignore_component_classes (true or false, default false); ignore_rooms (true or false, default false); ignored_parameters (list of text); remove_orphaned_copper (true or false, default false)
    • Runs on the selection: eco_change

sheet. commands (.drawing)

  • sheet.add: Add a sheet.
    • Required: name (text); size (one of a3, a4, a2, a1, a0, a, b, c, d, default a3)

sheet-metal. commands (.part)

  • sheet-metal.base-flange: Start a sheet metal part from a sketch.
    • Required: profile (pick: sketch); thickness (number in mm, default 1.5); radius (number in mm, default 1); depth (number in mm, default 20); bend_rule (one of k_factor, table, allowance, deduction, default k_factor); k (number, default 0.44) when bend_rule is k_factor
    • Optional: gauge (text)
  • sheet-metal.break-corner: Chamfer or round a flat corner.
    • Required: edges (picks: edge); break (one of chamfer, fillet, default chamfer); distance (number in mm, default 2)
  • sheet-metal.closed-corner: Close the gap between flanges at a corner.
    • Required: faces (picks: face); type (one of butt, overlap, underlap, default butt); gap (number in mm, default 0.1)
  • sheet-metal.convert: Turn a thin solid into sheet metal: the walls on the fixed face's edges become bends.
    • Required: fixed (pick: face); thickness (number in mm, default 1.5); radius (number in mm, default 1)
    • Optional: bends (picks: edge)
  • sheet-metal.edge-flange: Add a flange along edges.
    • Required: edges (picks: edge); length (number in mm, default 10); angle (number in deg, default 90); position (one of inside, outside, bend_outside, default inside); radius (number in mm, default 1); relief (one of rectangular, obround, tear, default rectangular)
  • sheet-metal.flat-pattern: Show the flat pattern with bend lines, for drawings and DXF.
  • sheet-metal.fold: Fold unfolded bends back.
    • Optional: bends (picks: face)
  • sheet-metal.form-tool: Stamp a form (louver, dimple, bead) into a face.
    • Required: tool (one of louver, dimple, bead, default louver); face (pick: face); position (pick: sketch point or point or vertex); rotation (number in deg, default 0)
  • sheet-metal.hem: Fold an edge back on itself.
    • Required: edges (picks: edge); hem (one of closed, open, teardrop, rolled, default closed); length (number in mm, default 5); gap (number in mm, default 0.5) when hem is open
  • sheet-metal.jog: Add two bends that offset a flat.
    • Required: line (pick: sketch entity or sketch); offset (number in mm, default 5); angle (number in deg, default 90)
  • sheet-metal.lofted-bend: Bend between two open profiles (transitions, hoppers).
    • Required: profile1 (pick: sketch); profile2 (pick: sketch); thickness (number in mm, default 1.5); bends (whole number, default 8)
  • sheet-metal.miter-flange: Add flanges along a chain of edges with mitered corners.
    • Required: profile (pick: sketch); edges (picks: edge); gap (number in mm, default 0.25)
  • sheet-metal.relief: Cut relief at bend corners.
    • Required: corners (picks: vertex or edge); relief (one of rectangular, round, tear, default rectangular); size (number in mm, default 1.5)
  • sheet-metal.sketched-bend: Bend along a sketched line.
    • Required: line (pick: sketch entity or sketch); angle (number in deg, default 90); radius (number in mm, default 1); fixed (pick: face)
  • sheet-metal.tab-and-slot: Add interlocking tabs and slots between flanges.
    • Required: edge (pick: edge); face (pick: face); length (number in mm, default 10); count (whole number, default 2); clearance (number in mm, default 0.1)
  • sheet-metal.unfold: Unfold chosen bends to work on the flat.
    • Required: fixed (pick: face)
    • Optional: bends (picks: face)

simulate. commands (.circuit, .circuit.layout, .part, .assembly)

  • simulate.ac: Add an AC sweep (gain and phase over frequency) to the simulation section.
    • Required: start (number in Hz, default 10); stop (number in Hz, default 1000000); points (whole number, default 20)
    • Optional: name (text)
  • simulate.check: Check fit and mass before a study meshes the design: overlapping parts, open contacts and parts without a material.
    • Required: gap (number in mm, default 0.1)
  • simulate.dc-sweep: Add a DC sweep of a source to the simulation section.
    • Required: source (text); start (number in V, default 0); stop (number in V, default 5); step (number in V, default 0.1)
    • Optional: name (text)
  • simulate.monte-carlo: Add a Monte Carlo over the section's tolerances that reruns another analysis of the section.
    • Required: kind (one of monte_carlo, default monte_carlo); of (text); runs (whole number, default 1000); seed (whole number, default 1)
    • Optional: name (text)
  • simulate.noise: Add a noise sweep: the output noise density at a net and the noise referred to an input source.
    • Required: output (text); input (text); start (number in Hz, default 10); stop (number in Hz, default 1000000); points (whole number, default 20)
    • Optional: name (text)
  • simulate.op-point: Add a DC operating point to the simulation section.
    • Optional: name (text)
  • simulate.probe: Probe a net's voltage or the current into a pin: click it on the schematic, or pick it.
    • Required: at (pick: net or pin)
  • simulate.probe-net: Plot the net's voltage when the simulation section runs.
    • Runs on the selection: net
  • simulate.probe-pin: Plot the current into the pin when the simulation section runs.
    • Runs on the selection: pin
  • simulate.publish: Publish a region, frame, value or path for assemblies and studies to use.
    • Required: name (text); target (one of region, frame, value, path, default region); item (pick: region or mate connector or input) when target is region or frame or value; edges (picks: edge) when target is path
  • simulate.set-tolerance: Set the tolerance a Monte Carlo varies parts by (it replaces the parts' own bands).
    • Required: match (text); percent (number, default 1)
    • Optional: name (text)
  • simulate.temperature: Add a temperature sweep that reruns another analysis of the section at each temperature.
    • Required: of (text); values (text)
    • Optional: name (text)
  • simulate.transient: Add a transient (over time) to the simulation section.
    • Required: stop (number in s, default 0.001); step (number in s, default 0.000001)
    • Optional: name (text)

sketch. commands (.part)

  • sketch.arc: Draw an arc by center, tangent to an end or through three points.
    • Required: type (one of center, tangent, three_point, default center); start (pick: sketch point or vertex or point); end (pick: sketch point or vertex or point); center (pick: sketch point or vertex or point) when type is center
    • Optional: radius (number in mm, default 10)
  • sketch.auto-constrain: Suggest relations and dimensions; accept them one at a time.
    • Required: tolerance (number in mm, default 0.01)
    • Optional: entities (picks: sketch entity)
  • sketch.chamfer: Bevel sketch corners.
    • Required: corners (picks: sketch point or sketch entity); distance (number in mm, default 1); angle (number in deg, default 45)
  • sketch.circle: Draw a circle by center or through three points.
    • Required: type (one of center, three_point, default center); center (pick: sketch point or vertex or point) when type is center; radius (number in mm, default 10) when type is center; points (picks: sketch point or vertex) when type is three_point
  • sketch.constraint: Add a geometric relation between sketch entities.
    • Required: relation (one of coincident, horizontal, vertical, parallel, perpendicular, tangent, equal, concentric, midpoint, symmetric, collinear, coradial, fix, default coincident); entities (picks: sketch entity or sketch point or edge)
    • Runs on the selection: sketch_entity, sketch_point
  • sketch.construction: Draw new entities as construction geometry, or toggle selected ones.
    • Runs on the selection: sketch_entity
  • sketch.dimension: Add a driving or driven dimension.
    • Required: type (one of smart, horizontal, vertical, ordinate, path_length, default smart); entities (picks: sketch entity or sketch point)
    • Optional: value (number in mm); driven (true or false, default false)
  • sketch.extend: Extend an entity to the next one it meets.
    • Required: entities (picks: sketch entity)
  • sketch.fillet: Round sketch corners.
    • Required: corners (picks: sketch point or sketch entity); radius (number in mm, default 2)
    • Optional: keep_corner (true or false, default true)
  • sketch.line: Draw lines, centerlines or a line from its midpoint.
    • Required: type (one of line, centerline, midpoint, default line); start (pick: sketch point or vertex or point); end (pick: sketch point or vertex or point)
    • Optional: length (number in mm, default 0); angle (number in deg, default 0); chain (true or false, default true)
  • sketch.mirror: Mirror entities about a line, with an optional live mirror.
    • Required: entities (picks: sketch entity); about (pick: sketch entity)
    • Optional: copy (true or false, default true); dynamic (true or false, default false)
  • sketch.offset: Offset entities by a distance.
    • Required: entities (picks: sketch entity or edge); distance (number in mm, default 2)
    • Optional: both (true or false, default false); cap (true or false, default false); chain (true or false, default true)
  • sketch.pattern: Repeat entities in a line or a circle.
    • Required: layout (one of linear, circular, default linear); entities (picks: sketch entity); spacing (number in mm, default 10) when layout is linear; direction (number in deg, default 0) when layout is linear; center (pick: sketch point or vertex or point) when layout is circular; angle (number in deg, default 360) when layout is circular; instances (whole number, default 4)
  • sketch.point: Place a sketch point.
    • Required: at (pick: sketch point or vertex or point)
  • sketch.rectangle: Draw a rectangle by corners, center, three points or as a parallelogram.
    • Required: type (one of corner, center, three_point, parallelogram, default corner); first (pick: sketch point or vertex or point); second (pick: sketch point or vertex or point); third (pick: sketch point or vertex or point) when type is three_point or parallelogram
    • Optional: construction_diagonals (true or false, default false)
  • sketch.slot: Draw a straight, center-point or arc slot.
    • Required: type (one of straight, center, arc, default straight); start (pick: sketch point or vertex or point); end (pick: sketch point or vertex or point); width (number in mm, default 6)
    • Optional: dimension (true or false, default true)
  • sketch.split: Split an entity at a point.
    • Required: entity (pick: sketch entity); at (pick: sketch point or vertex or point)
  • sketch.transform: Move, copy, rotate or scale entities.
    • Required: type (one of move, copy, rotate, scale, default move); entities (picks: sketch entity or sketch point); base (pick: sketch point or vertex or point); dx (number in mm, default 0) when type is move or copy; dy (number in mm, default 0) when type is move or copy; angle (number in deg, default 0) when type is rotate; factor (number, default 1) when type is scale
  • sketch.trim: Trim entities by power trim, to a corner, inside or outside.
    • Required: type (one of power, corner, inside, outside, default power); entities (picks: sketch entity); boundaries (picks: sketch entity) when type is inside or outside

study. commands (.circuit, .circuit.layout)

  • study.new: Create a .fea study from this design.
    • Required: physics (one of structural, modal, thermal, ir_drop, warpage, thermal_structural, default structural); name (text)

surface. commands (.part)

  • surface.boundary: Make a surface from curves in two directions.
    • Required: direction1 (picks: edge); continuity (one of g0, g1, g2, default g0)
    • Optional: direction2 (picks: edge)
  • surface.cut: Cut a solid with a surface, keeping one side.
    • Required: surface (pick: face or body); body (pick: body or face); keep (one of positive, negative, default positive)
  • surface.delete-hole: Remove a hole's boundary from a surface.
    • Required: edges (picks: edge)
  • surface.extend: Extend a surface past its edges.
    • Required: edges (picks: edge); distance (number in mm, default 5)
  • surface.extrude: Extrude a sketch's curves, open or closed, into a surface.
    • Required: profile (pick: sketch); depth (number in mm, default 10)
    • Optional: symmetric (true or false, default false)
  • surface.fill: Patch a closed boundary with G0, G1 or G2 continuity.
    • Required: boundary (picks: edge); continuity (one of g0, g1, g2, default g0)
  • surface.knit: Knit surfaces together, and make a solid when they close.
    • Required: bodies (picks: face or body)
    • Optional: solid (true or false, default true)
  • surface.loft: Loft a surface through curves.
    • Required: profiles (picks: sketch or curve or edge)
    • Optional: guides (picks: curve or edge)
  • surface.mid-surface: Make mid-surfaces between pairs of opposite faces for shell studies.
    • Required: pairs (picks: face)
  • surface.offset: Offset faces into a new surface.
    • Required: faces (picks: face); distance (number in mm, default 1)
  • surface.planar: Fill a closed sketch with a flat surface.
    • Required: profile (pick: sketch)
  • surface.revolve: Revolve a sketch's curves into a surface.
    • Required: profile (pick: sketch); axis (pick: axis or edge); angle (number in deg, default 360)
  • surface.ruled: Grow strips from edges along their faces' normal, tilted outward by an angle.
    • Required: edges (picks: edge); distance (number in mm, default 10); angle (number in deg, default 0)
  • surface.sweep: Sweep a sketch's curves along another sketch's path.
    • Required: profile (pick: sketch); path (pick: sketch)
  • surface.thicken: Give a surface thickness to make a solid.
    • Required: surface (pick: face or body); thickness (number in mm, default 1); side (one of one, both, other, default one)
  • surface.trim: Trim surfaces with a plane, keeping one side.
    • Required: bodies (picks: face or body); tool (pick: plane or face); keep (one of positive, negative, default positive)

table. commands (.drawing)

  • table.bend: List bends of a flat pattern.
    • Required: view (pick: view)
  • table.bom: Add a bill of materials table.
    • Required: view (pick: view); type (one of top, parts, indented, default top)
    • Optional: fasteners (true or false, default true); at (pick: point)
  • table.cut-list: List weldment members by profile and length.
    • Required: view (pick: view)
    • Optional: at (pick: point)
  • table.hole: List holes with positions from an origin.
    • Required: origin (pick: edge)
    • Optional: faces (picks: edge); combine (true or false, default true); at (pick: point)
  • table.revision: Add the revision table, or a revision to it.
    • Required: rev (text); description (text)
    • Optional: date (text); by (text); at (pick: point)

view. commands (.part, .assembly)

  • view.measure: Measure distance, angle, radius or path length; results stay pinned in the view.
    • Required: mode (one of distance, angle, radius, path, default distance); items (picks: face or edge or vertex or body or component or pad or track or via)
    • Optional: pin (true or false, default true)
    • Runs on the selection: face, edge, vertex, sketch_entity, sketch_point, plane, feature, sketch, body, occurrence, mate

weldment. commands (.part)

  • weldment.cut-list: Show the cut list: members grouped by profile and length.
  • weldment.end-cap: Close a member's open end with a plate.
    • Required: face (pick: face); thickness (number in mm, default 3); inset (number in mm, default 0)
  • weldment.gusset: Add a triangular plate between two members' faces at a corner.
    • Required: faces (picks: face); leg (number in mm, default 50); thickness (number in mm, default 5)
  • weldment.structural-member: Place profiles along sketch segments.
    • Required: standard (one of iso, ansi, company, default iso); profile (one of rect_tube, square_tube, pipe, angle, channel, i_beam, flat_bar, default rect_tube); size (text, default 40x40x3); material (one of s235, al_6061, stainless_304, default s235); segments (picks: sketch entity or sketch); corner (one of miter, butt1, butt2, none, default miter); rotation (number in deg, default 0)
    • Optional: mirror_profile (true or false, default false)
  • weldment.trim-extend: Trim or extend a member to a flat face of another body.
    • Required: member (pick: body or face); to (pick: face)
  • weldment.weld-bead: Add a fillet weld along the edges between members.
    • Required: edges (picks: edge); leg (number in mm, default 4)
On this page
  • assembly. commands (.assembly)
  • board. commands (.circuit, .circuit.layout)
  • direct. commands (.part)
  • drawing. commands (.drawing)
  • evaluate. commands (.part)
  • explode. commands (.assembly)
  • library. commands (.circuit, .circuit.layout)
  • manage. commands (.part)
  • mold. commands (.part)
  • part. commands (.part)
  • schematic. commands (.circuit, .circuit.layout)
  • sheet. commands (.drawing)
  • sheet-metal. commands (.part)
  • simulate. commands (.circuit, .circuit.layout, .part, .assembly)
  • sketch. commands (.part)
  • study. commands (.circuit, .circuit.layout)
  • surface. commands (.part)
  • table. commands (.drawing)
  • view. commands (.part, .assembly)
  • weldment. commands (.part)