Create, edit, verify and export parametric FreeCAD models (STEP, STL, 3MF) and DXF drawings from JSON; STL import; mass and stress checks; parts from GitHub.
FreeCAD skill
Build parametric CAD models with FreeCAD by sending a JSON request to one command. Every operation creates a
native FreeCAD feature (Part::Box, Part::Cut, Part::Fillet, ...), so the model stays editable: change a
dimension later and everything downstream updates. After every step the response reports volumes and bounding
boxes, and failures name the step, the cause and a fix.
{baseDir} below means the directory that contains this SKILL.md.
Run
Write the request to a file and run:
python3 {baseDir}/scripts/fcskill.py run request.json
On Windows, use python instead of python3. The launcher needs Python 3.12 or newer; if it reports
PYTHON_VERSION, run it with a newer interpreter (e.g. python3.12).
The request can also be inline JSON or come from stdin (run -). Use a file for anything non-trivial, because
it avoids shell-quoting problems. The working directory is the workspace. Documents and exports are relative
to it and cannot leave it.
Other commands:
python3 {baseDir}/scripts/fcskill.py library <keywords>: search ready-made parts (see below).python3 {baseDir}/scripts/fcskill.py describe: list every op with its parameters (*= required).python3 {baseDir}/scripts/fcskill.py describe fillet shell: full parameter details for those ops.python3 {baseDir}/scripts/fcskill.py doctor: check the FreeCAD installation.
If doctor says FreeCAD is missing, ask the user to install FreeCAD 1.1+ or to set FCSKILL_FREECAD to its
freecadcmd executable. Do not try to model without it.
Request
{
"doc": "bracket.FCStd",
"steps": [
{"op": "box", "name": "Plate", "length": 80, "width": 50, "height": 6},
{"op": "cylinder", "name": "Hole", "radius": 3.25, "height": 8, "position": [10, 10, -1]},
{"op": "cut", "name": "Drilled", "base": "Plate", "tool": "Hole"},
{"op": "fillet", "name": "Bracket", "target": "Drilled", "radius": 5, "edges": "|Z and %LINE",
"expect": {"bbox_size": [80, 50, 6], "solids": 1}},
{"op": "export", "filename": "bracket.step"}
]
}
doc: the.FCStdfile (defaultmodel.FCStd). It is created if missing and re-opened on later requests.new: true: start from an empty document, replacing the file's content.dry_run: true: run and report without saving or exporting.brief: true: leave volume and bounding box out of the per-step entries. Use it for long requests;results,warningsand errors are reported as usual.- All or nothing: if any step fails, nothing is saved or exported and the file on disk is unchanged. Fix the reported step and resend the whole request.
- Before anything runs, the whole request is validated. Unknown ops or parameters, typos and missing values are all reported at once.
Response
Actual output for the request above (abridged):
{"status": "success", "doc": "bracket.FCStd", "saved": true,
"steps": [{"index": 0, "op": "box", "object": "Plate", "volume": 24000.0,
"bbox": {"min": [0,0,0], "max": [80,50,6], "size": [80,50,6]}, "solids": 1},
{"index": 2, "op": "cut", "object": "Drilled", "volume": 23800.902, "...": "..."},
{"index": 3, "op": "fillet", "object": "Bracket", "volume": 23672.14, "...": "..."},
{"index": 4, "op": "export", "data": {"file": "bracket.step"}}],
"results": [{"name": "Bracket", "type": "Part::Fillet", "role": "result", "inputs": ["Drilled"],
"volume": 23672.14, "bbox": {"min": [0,0,0], "max": [80,50,6], "size": [80,50,6]}, "solids": 1, "valid": true}],
"intermediates": ["Plate", "Hole", "Drilled"],
"exports": [{"file": "bracket.step", "format": "step", "objects": ["Bracket"], "bytes": 13775,
"verified": {"faces": 11, "bbox_size": [80,50,6], "solids": 1, "volume": 23672.14}}],
"files_written": ["bracket.FCStd", "bracket.step"]}
When something is wrong, warnings appears, e.g.
{"step": 2, "code": "NO_EFFECT", "message": "cut removed no material from 'Plate'; ['Hole'] do not overlap it. ..."}.
resultsare the finished parts: objects that no other feature consumes. Exports default to these.- Read
warnings. For example,NO_EFFECTmeans a cut missed the part, andDISJOINTmeans a fusion produced separate pieces. These are geometry mistakes even though the status is success. OVERLAPPING_RESULTSmeans two finished parts occupy the same space. Usually one is a leftover helper (a cutter you never used, which then hides the part in renders), or two parts that should touch are sized wrong. Every result is rendered and exported, so delete leftovers before trusting a render.SELF_INTERSECTIONmeans a result passes through itself (e.g. a spring whose wire is thicker than its pitch). Its volume and mass are wrong and other CAD systems may reject it: fix it, don't deliver it.SELF_INTERSECTION_UNCHECKEDmeans that check could not give an answer for a result (the message says why: too many faces, invalid geometry, or the checker failed). The result is then unconfirmed, not clean: tell the user, or simplify or repair the part and run again.DEEP_CHAINmeans many booleans are stacked one on another, which gets slow. See Workflow, step 3.- On failure,
errorhascode,message,hint,step,opand oftendetails(available names, measured values). Exit code is 0 on success, 1 when the request failed, 2 when FreeCAD is missing or crashed.
Conventions
- Units are mm and degrees, and the axes are right-handed X/Y/Z with +Z up.
box:positionis the minimum corner; the box extends along +X/+Y/+Z. To centre a 40×20 box on (0, 0), useposition: [-20, -10, z].cylinder,cone,prism:positionis the centre of the bottom face; the axis is +Z unless you givedirection(e.g.[1, 0, 0]).sphere,torus:positionis the centre.extrude,revolve: the profile lies inplane(XYdefault,XZ,YZ), with 2D coordinates. Extrusion goes along the plane normal: XY→+Z, XZ→+Y, YZ→+X. See Profiles.- Names are identifiers (
Base_plate, notbase plate) and must be unique. Name every object you will refer to later. - Make cutting tools pass through the faces they cut: a hole in a 6 mm plate should run from z = -1 to z = 7. Exactly coincident faces make booleans fail or leave skins.
Operations
| Op | Purpose | Key parameters (* required) |
|---|---|---|
box | Box | length* width* height* position rotation |
cylinder | Cylinder | radius* height* position direction |
sphere | Sphere | radius* position |
cone | Cone / frustum | radius1* (bottom) radius2* (top) height* position direction |
torus | Torus | radius1* (ring) radius2* (tube) position direction |
prism | Regular polygon prism | sides* circumradius* height* position direction |
extrude | Profile → solid (pad/pocket in a body) | shapes or points, height or direction, plane offset symmetric; in a body: body mode through_all reversed |
revolve | Profile → solid of revolution (revolution/groove in a body) | shapes or points, plane axis center angle; in a body: body mode |
loft | Smooth solid through cross-sections (organic shells, bottles, square-to-round) | sections* ruled closed; in a body: body mode |
sweep | Profile along a path or helix (tubes, handles, springs, threads) | shapes*, path (+smooth, corner_radius) or helix, up; in a body: body mode |
text | Lettering as a solid, to engrave (cut) or emboss (fuse) | text* size* height* position plane align angle reversed font |
body | PartDesign body: one solid built feature by feature | name position rotation |
assembly | Assembly of parts (links to solids/bodies); first part grounded; returns a bill of materials (bom) | parts* (object, name, position, ground) |
joint | Connect two assembly parts and solve: fixed, revolute, cylindrical, slider, ball, parallel, perpendicular | assembly* type* a* b* ({"part", "face"/"edge"}) offset |
hole | Drilled holes in a body: simple, counterbore, countersink, threaded | body* at* offset size (M2…M20) or diameter, fit threaded type depth |
cut | Subtract | base* tool or tools |
fuse | Union | objects* (≥2) |
common | Intersection | objects* (≥2) |
fillet | Round edges | target* radius* edges (selector, default all) |
chamfer | Bevel edges | target* size* edges |
shell | Hollow out, open faces | target* thickness* open_faces* (selector) outward |
linear_array | Repeat along a vector | target* count* step* (offset between copies) |
grid_array | Repeat on a grid | target* count_x* count_y* step_x* step_y* |
polar_array | Repeat around an axis | target* count* angle axis center |
move | Translate | target* offset* |
rotate | Rotate about an axis through a point | target* angle* axis center |
place | Absolute position/rotation | target* position rotation |
mirror | Mirrored copy (of a solid, or of a feature inside its body) | target* plane (XY/XZ/YZ) or normal, point |
copy | Linked copy that follows the original | target* offset |
scale | Scaled version (about origin) | target* factor* (number or [sx, sy, sz]) |
set | Change properties, recompute downstream | target* properties* |
set_params | Named parameters (Params spreadsheet) | values* |
delete | Delete objects | targets or all, with_dependents |
rename | Change label | target* label* |
inspect | Document tree, or one object in detail | target topology |
check | Assert geometry | target* expect* |
measure | Clearance, interference, closest points; mass, centre of mass, inertia | objects require (min_clearance, no_interference) material density |
import | Solid from a STEP/IGES/BREP/FCStd file or a closed STL/OBJ/3MF mesh, or a ready-made part from the FreeCAD library | library or file, anchor position rotation refine name |
material | Material and/or colour of finished parts (FreeCAD material, GUI colour, renders, masses) | targets* material color transparency |
fem_static | Stress analysis: displacement, von Mises stress, safety factor | target* fixed* loads* material require report mesh_size |
export | STEP/IGES/BREP/STL/OBJ/3MF, or a flat DXF/SVG outline (laser/CNC), verified | filename* targets tolerance view |
drawing | Technical drawing (DXF): views, verified dimensions, hole table, title | filename* sheet projection scale dimensions title author preview |
render | Shaded PNG views for a visual check | filename* views (default iso, front, top, right) size |
rotation is {"axis": [x, y, z], "angle": deg}. Full details are in describe <op> or
docs/OPERATIONS.md. Complete, tested requests to start from are in {baseDir}/examples/:
pd_bracket.json (PartDesign body, counterbored holes, fillet), mounting_plate.json, gasket.json (sketch
profile with holes), enclosure.json, flanged_bushing.json, l_bracket.json, wheel.json and table.json.
Profiles
shapes builds a real, editable FreeCAD sketch from closed shapes. Shapes inside another shape become holes:
{"op": "extrude", "name": "Gasket", "height": 2, "shapes": [
{"rect": [0, 0, 90, 60], "corner_radius": 8},
{"slot": [[30, 30], [60, 30]], "radius": 9},
{"circle": [10, 10], "radius": 3.5},
{"polygon": [[40, 5], [50, 5], [45, 12]], "corner_radius": 1},
{"path": [[70, 40], [80, 40], {"arc_to": [80, 50], "center": [80, 45]}, [70, 50]]}
]}
rect:[x_min, y_min, x_max, y_max], optionalcorner_radius.circle: centre plusradius.slot: the centres of its two rounded ends plusradius.polygon: corners plus optionalcorner_radius, orradiiwith one radius per corner.spline: a smooth closed curve through 3 or more points, e.g.{"spline": [[58, 0], [40, 22], [0, 30], [-45, 24], [-58, 0], [-45, -24], [0, -30], [40, -22]]}.path: a start point, then[x, y](a line to that point),{"arc_to": [x, y], "center": [cx, cy], "clockwise": false}, or{"spline_to": [x, y], "through": [[x, y], ...], "start_tangent": [dx, dy], "end_tangent": [dx, dy]}(a smooth curve; tangents are optional). The path closes back to its start automatically.
Splines pass exactly through their points but can bulge between them. Use more points where the curve must be
controlled, and a path with straight segments for flat sides, e.g. a flat-bottomed dome:
{"path": [[-30, 0], [30, 0], {"spline_to": [-30, 0], "through": [[20, 25], [0, 32], [-20, 25]], "start_tangent": [0, 1], "end_tangent": [0, -1]}]}.
Shapes must be separate or fully nested; partial overlaps are rejected. offset moves the profile plane
along its normal. To change the outline later, use set with {"shapes": [...]}. points is a shortcut for
a plain polygon.
Parametric profiles. The numbers of rect, circle and slot (coordinates, radius,
corner_radius) can be expressions, so the outline follows the parameters:
{"op": "set_params", "values": {"width": 90, "depth": 50, "bore": 12}},
{"op": "extrude", "name": "Plate", "height": 6, "shapes": [
{"rect": [0, 0, "=Params.width", "=Params.depth"], "corner_radius": 5},
{"circle": ["=Params.width / 2", "=Params.depth / 2"], "radius": "=Params.bore / 2"}]}
Changing width with set_params then resizes the plate and keeps the bore centred. These three shapes
are stored as fully dimensioned sketches (one named dimension per number), so they also stay put when a
person opens the sketch in FreeCAD. polygon, spline and path take numbers only; so do sweep profiles
and loft sections.
More operations (read the guide first)
These need more than the table above. Read the guide before the first use in a session:
loft,sweep(springs, tubes, threads) andtext(engraving, embossing): docs/SHAPES.md.importof STEP/IGES/BREP/FCStd files and closed meshes, and ready-made parts from the FreeCAD library (librarycommand): docs/PARTS.md. The library is the skill's only network use: anonymous downloads from github.com/FreeCAD/FreeCAD-library, off withFCSKILL_OFFLINE=1. Library parts are CC-BY 3.0: pass the reportedattributionon to the user.assemblyandjoint: docs/ASSEMBLIES.md.fem_static(stress analysis): docs/ANALYSIS.md.
PartDesign bodies
A body is one solid built feature by feature: the way FreeCAD users model mechanical parts, and the most editable kind of model. Prefer a body for a single part, and stand-alone solids plus booleans for quick shapes or multi-part layouts.
{"op": "body", "name": "Bracket"},
{"op": "extrude", "body": "Bracket", "name": "Base", "height": 8, "shapes": [{"rect": [0, 0, 90, 50], "corner_radius": 6}]},
{"op": "extrude", "body": "Bracket", "name": "Boss", "height": 12, "offset": "=Base.Length", "shapes": [{"circle": [45, 25], "radius": 12}]},
{"op": "extrude", "body": "Bracket", "mode": "remove", "through_all": true, "offset": "=Base.Length + Boss.Length", "shapes": [{"circle": [45, 25], "radius": 6}]},
{"op": "hole", "body": "Bracket", "at": [[10, 10], [80, 10]], "offset": "=Base.Length", "size": "M5", "type": "counterbore"},
{"op": "fillet", "target": "Bracket", "radius": 2, "edges": "%CIRCLE and r=12 and not >Z"}
- Placing features:
- Profiles always use body coordinates.
offsetplaces the profile plane, e.g. on top ofBase. - Use an expression (
"=Base.Length") so the feature follows when dimensions change.
- Profiles always use body coordinates.
- Directions:
mode: "add"(pad) goes along the plane normal: XY→+Z, XZ→+Y, YZ→+X.mode: "remove"(pocket) andholego against it, so they cut down into a part from a profile on its top face.- For the bottom, back or left faces, use
reversed: true. - A feature that misses the part gets a
NO_EFFECTwarning, and a hole that starts in air getsHOLE_OUTSIDE.
- The first feature must add material. A body stays one solid, so added material must touch the existing part.
- Dress-ups and patterns:
fillet,chamferandshelltake the body astargetand are added at the end of its feature tree.linear_array,grid_array,polar_arrayandmirrortake a feature of the body (e.g. a pocket, hole or pad) astargetand repeat it inside the body. A pattern or mirror can't be repeated again: name the original feature (onegrid_arraygives a grid).
- Holes:
sizeuses ISO tables:fit: "clearance"(default) for a screw to pass,"tap"for a tap drill.threaded: true(withsize, typesimple) models a real ISO metric thread over the hole depth. Givedepthfor a blind hole. Prefer a plain hole for small printed threads (below about M5).- Counterbores fit ISO 4762 socket heads; countersinks fit ISO 10642 (90°).
- Editing:
- Use
seton a feature for native properties (Length,Diameter, ...), or forshapes,offsetandat(holes). - Fillet and chamfer selectors are re-evaluated after every edit.
- Move the whole part by moving the body; features have no placement of their own.
- Use
- Combining with other solids: a body can be used like any solid in
cut,fuse,mirror,copyandexport.
Edge and face selectors
edges (fillet/chamfer) and open_faces (shell) accept "all", 1-based indices [1, 3], or an expression:
| Selector | Meaning |
|---|---|
>Z / <Z | elements whose centre is highest / lowest in Z (same for X, Y) |
|Z | straight edges parallel to Z; planar faces whose normal is parallel to Z |
#Z | straight edges / face normals perpendicular to Z |
+Z / -Z | planar faces facing +Z / -Z |
%LINE %CIRCLE %PLANE %CYLINDER | geometry type |
r<5 r=3 r>2 | radius of circular edges / cylindrical faces |
face(>Z) | edges bounding the selected faces (e.g. all top edges) |
and or not ( ) | combine |
Examples: vertical corners of a plate "|Z and %LINE", top outline "face(>Z)", hole edges "%CIRCLE and r<4",
open top of a box ">Z". Prefer selectors to indices. They are re-evaluated when upstream dimensions change,
while indices can point at different edges after an edit. Use inspect with "topology": true to see faces and
edges with their type, centre, normal, direction and radius.
Workflow
- Plan the part as solids, profiles, booleans, then features: fillets and chamfers last, after the cuts they should round.
- Parametrise dimensions the user may change:
{"op": "set_params", "values": {"wall": 2}}, then use"height": "=Params.wall * 3". Expressions can also reference other objects:"=Plate.Length - 10". Parameter names must not be unit symbols or constants:h,l,t,s,g,e,W,H,mm,in,degand similar are rejected (Lhappens to be allowed). Use descriptive names such asheight,length,thicknessorwall; the error suggests one. - Send one request per coherent change, with
expecton the steps that matter (volume,bbox_size,bbox_min,bbox_max,solids,self_intersecting). An expectation that doesn't hold is an error, so mistakes never slip through as a success.- Batch repeated features. Don't cut 30 holes with 30
cutsteps: each boolean stacked on the last is slower than the one before (50 chained cuts take about 20 s, the same holes in one step about 1 s). Use oneholewith all centres inat(in a body), several circles in one profile, onecutwith all thetools, or an array of the tool.
- Batch repeated features. Don't cut 30 holes with 30
- Read the response: per-step
bbox/volume,results,warnings. - Modify existing models in place rather than rebuilding them:
{"doc": "bracket.FCStd", "steps": [{"op": "set_params", "values": {"wall": 3}}]}or{"op": "set", "target": "Plate", "properties": {"Length": 120}}. For an unfamiliar document, start with{"doc": "x.FCStd", "op": "inspect"}, theninspectthe objects you need. Theirpropertiesare exactly whatsetaccepts. - Check fits between parts with
measure, e.g.{"op": "measure", "objects": ["Lid", "Box"], "require": {"min_clearance": 0.3}}. It fails if any gap is smaller, andclosestgives the points where the gap is smallest. Each pair is reported asclear,touchingorinterfering(with the overlap volume).- Mass properties:
{"op": "measure", "objects": ["Bracket"]}gives volume, area, centre of mass and the inertia tensor (about the centre of mass, global axes) inproperties; with a material assigned (ormaterial/densitygiven) also the mass, and for several parts thetotalmass and centre of mass.
- Mass properties:
- Check strength with
fem_staticwhen the user cares whether a part will hold. Read docs/ANALYSIS.md first: loads need units, and every result comes with checks (equilibrium,convergence) that you must report to the user when they did not pass. - Look at it. Numbers can't show a hole on the wrong face. Add
{"op": "render", "filename": "preview.png"}and view the PNG if you can read images.- It shows a 2×2 grid: iso, front (looking along +Y), top (looking down), right (looking along -X).
- Each view has an axis triad: X red, Y green, Z blue.
mm_per_pixelin the result lets you estimate sizes.
- Drawings and cutting files:
- For laser, waterjet or CNC cutting, use
{"op": "export", "filename": "plate.dxf"}: a 1:1 outline in mm, viewed fromtopby default. - For a dimensioned workshop drawing, use
{"op": "drawing", "filename": "part.dxf", "title": "...", "preview": "part.png"}. It places front, plan and side views (ISO first angle by default) at a standard scale. Its overall and hole dimensions are checked against the model, and thedimensionslist in the result gives their values. Equal holes get one diameter with a count (4x ⌀5.5), and a hole table on the sheet (alsoholesin the result) gives each vertical hole's X/Y from the lower-left corner of the plan view. - Re-run
drawingafter editing the model; it regenerates the page. - PDF and SVG pages need the FreeCAD GUI: the page is kept in the
.FCStd.
- For laser, waterjet or CNC cutting, use
- Give finished parts a material so they look right when opened in FreeCAD and in renders, and so
measurereports masses:{"op": "material", "targets": ["Rim"], "material": "aluminium"},{"op": "material", "targets": ["Tire"], "material": "rubber"}, or a colour for prints:{"op": "material", "targets": ["Case"], "material": "pla", "color": "#E03020"}. Presets: steel (+ _s235, _s355), stainless_steel, stainless_304, cast_iron, aluminium (+ _6061, _7075, _5754), titanium, copper, brass, bronze, gold, silver, chrome, pla, abs, petg, nylon, nylon_pa12, pom, polypropylene, polycarbonate, acrylic, ptfe, pvc, rubber, glass, wood, concrete; or any FreeCAD library material name. Materials of assembly parts go to their source objects.fem_staticuses the assigned material when it is a specific grade (e.g.steel_s235,aluminium_6061). - Export at the end. Each export is read back and verified. STEP files carry each part's name, and an
assembly as a product structure (
verified.part_names). Mesh exports reportclosed,non_manifoldandself_intersections. The extension sets the format.
Fixing errors
error.code | What to do |
|---|---|
INVALID_REQUEST | Fix every item in details.problems (each names its step and param) and resend. |
OBJECT_NOT_FOUND | Use a name from details.available. Names are case-sensitive. |
NAME_CONFLICT | Choose a new name, or edit the existing object with set. |
RECOMPUTE_FAILED / GEOMETRY_INVALID | Read hint and details.freecad_message. Typical causes: fillet radius too large (hint gives the shortest edge), coincident boolean faces, self-intersecting profile. |
EMPTY_RESULT | The cut removed everything, or the objects of a common don't overlap. Check positions. |
EXPECTATION_FAILED | Compare details.failures (expected vs actual) to find the wrong dimension or position. |
INVALID_SELECTOR | The selector matched nothing. inspect the base with topology: true. |
DEPENDENCY | Delete the dependents first, or pass with_dependents: true. |
PATH_NOT_ALLOWED | Use a path inside the workspace. |
FREECAD_NOT_FOUND / FREECAD_VERSION / FREECAD_CRASHED / TIMEOUT | Environment problem (FreeCAD missing, older than 1.1, or crashed): run doctor and tell the user. |
DOCUMENT_BUSY | Another request is editing the same document. Wait for it, then retry. |
Don't resend an unchanged request after an error. Change what the error points at.
Limits
- Only
rect,circleandslotprofiles are dimensioned and can take expressions;polygon,splineandpathprofiles are fixed outlines, edited by resendingshapes. Profiles lie in the XY, XZ or YZ plane (with anoffset), not on inclined planes. - Assemblies: no nested assemblies, no motion (gear, belt, screw) joints, and no limits. FEM is linear static only (no contact, buckling, thermal or modal analysis). Drawings are DXF only (PDF/SVG from the GUI); automatic dimensions are the overall sizes and hole diameters, with hole positions in a table rather than as dimension lines, and there are no section views or tolerances: tell the user when a drawing needs them. PartDesign supports pad, pocket, revolution, groove, hole, fillet, chamfer, shell, loft, sweep, mirror and linear/grid/polar patterns. No surface modelling (free-form patches, blends between arbitrary faces). Imported meshes stay faceted.
- If a request needs something these operations can't do, tell the user it isn't supported. Don't work around the skill with your own FreeCAD scripts: they skip validation and checks.
- Placement (
position) values are literal numbers; expressions apply to dimensions. - The self-intersection check is skipped on results with more than 3000 faces, and cannot run on invalid
geometry. A result it did not clear is never reported as clean: it carries
self_intersection_check: "not checked (reason)", the response has aSELF_INTERSECTION_UNCHECKEDwarning, and a STEP/BREP export lists it underverified.self_intersection_unchecked. When a part must be confirmed free of self-intersection, put"expect": {"self_intersecting": false}on its step: the request then fails unless the check ran and passed. Shapes are checked when a request makes or changes them: a request that only reads (inspect,measure,export,render) reportsresultswithoutvalid, andinspectof a whole document lists objects without it.inspectone object forvalidandself_intersecting. - A STEP import becomes one fixed solid (or compound): part names, colours and assembly structure of the file are not kept.
Scope
What the skill does on the machine, and nothing else:
- Commands: it is used through one command,
python3 {baseDir}/scripts/fcskill.py. The launcher starts FreeCAD's command-line program (found automatically, or the one named byFCSKILL_FREECAD) with the environment it was started in;fem_staticmakes FreeCAD run its bundled Gmsh and CalculiX. No shell, no other program, and requests cannot carry code. - Files: it reads and writes inside the workspace only (documents, exports, renders, and the parts cache
.fcskill/library), plus temporary files it removes afterwards (in the system temporary folder, or in~/snap/freecad/common/fcskillwhen FreeCAD is a snap). Paths that leave the workspace are refused, and the parts cache is never used through links. - Network: only the optional parts library, as anonymous downloads of fixed GitHub URLs
(
api.github.comandraw.githubusercontent.com, repository FreeCAD/FreeCAD-library), each checked against the library's index. Nothing is uploaded.FCSKILL_OFFLINE=1turns it off. - Environment variables: it reads the four
FCSKILL_*settings (FreeCAD command, workspace, local library clone, offline switch); on Windows it also reads the standard program-folder variables to find FreeCAD. It uses no credentials and stores none.
Compatibility
Version 3 changes from version 2:
exporthas noformatparameter any more: the file extension sets the format.fem_static:materialis optional (default: the part's assigned material) and must be a specific grade;aluminium_6061_t6andtitanium_gr5are still accepted as names foraluminium_6061andtitanium.- A part added to an
assemblywithoutpositionstays where it was modelled (it used to move to the origin). inspectwithout a target no longer reportsvalidper object, nor do theresultsof a request that changes nothing.
v1 requests ({"operation": ..., "parameters": ...}) and scripts/cad_engine.py are not supported, and there
is no python op: requests use only the operations above. Use only the format described here.
Related skills
- Downloads
- 2.2kAll time
- Security audit
- Pass
- Last updated
- 1w ago
- Current version
- v3.0.1
- License
- MIT-0
