Part Modeling

Everything CoPilot can build in a part — sketches, solid and surface features, patterns, sheet metal, materials, measurement and export — with prompts you can type as-is. All values are millimetres and degrees unless you say otherwise.

Start here: a worked bracket

If you read nothing else, read this. It is the shape of a session that goes well: one feature at a time, each one checked before the next.

Create a new part, then a 120 x 80 x 15 mm plate — sketch on the XY plane and extrude 15 mm in +Z

Expected volume 144,000 mm³.
What is the volume and bounding box?

Confirm 144,000 mm³ and 120 × 80 × 15 before continuing.
Add four Ø9 mm through holes on the top face, 15 mm in from each corner

Four holes through 15 mm of plate remove about 3,817 mm³.
How many holes are in the tree, and what is the volume now?
Add 5 mm fillets to the four vertical corner edges
Assign 6061-T6 aluminium and tell me the mass

Sketching

Choosing the sketch plane — the single most important thing on this page

A sketch can go on a standard plane (XY, XZ, YZ), on an existing face, or on any plane in space defined by a point and a normal direction. For anything that is not on a standard plane through the origin, use the third form and say both parts out loud:

Create a sketch on a plane through the world point (0, 0, 11) with normal (0, 0, 1)

Create a sketch on a plane through (-115, 0, 0) with normal (1, 0, 0), for a cut on the left face

Do not say “sketch on the XY plane at Z = 11”. An offset without a direction is ambiguous, and the failure it produces is the nastiest kind: the sketch lands on the base plane at Z = 0, every subsequent operation reports success, and the volume can come out exactly right while the feature sits 11 mm from where you wanted it. Give the point and the normal, every time.

To sketch on a face, get the face from a query first rather than guessing at a name:

List the faces of this body with their normals and areas, then sketch on the one whose normal is +Z at the top

Sketch entities

Lines, circles, arcs, rectangles, regular polygons, points, ellipses and splines are all available, plus arbitrary closed polygons given as a list of vertices.

Draw a 60 x 40 mm rectangle centred on the sketch origin

Draw a circle of radius 12 at (25, 0)

Draw a closed polygon through (0,0), (60,0), (60,25), (30,45) and (0,25)

Draw a hexagon of across-flats 24 mm centred at the origin

Draw a spline through (0,0), (20,15), (45,18) and (70,0)

Arcs: give the exact angles if you have them

An arc is defined by centre, radius, start angle and end angle. If you know the exact angles, paste them — rounding a computed angle by half a degree can leave a profile open by a fraction of a millimetre, and an open profile will not extrude.

Draw an arc centred at (0,0), radius 32, from 231.375° to 488.625° counter-clockwise

Constraints and dimensions

Coincident, concentric, parallel, perpendicular, horizontal, vertical, tangent, equal and fix constraints can all be added, along with linear, radial, diameter and angular sketch dimensions.

Make the two vertical lines equal and add a 40 mm dimension between them

Make the arc tangent to the top line and fix the bottom-left corner

List the constraints and dimensions in the active sketch

Editing sketches

List the sketches in this part

Open Sketch2 for editing and move the circle to (30, 0)

Offset the outer profile 3 mm inwards

Trim the line where it crosses the circle

Delete Sketch4

One extrusion per sketch. The first extrude consumes the sketch. If an extrude goes the wrong way and you want to retry, ask for the profile to be redrawn in a fresh sketch — otherwise the retry finds no profile to work with.

Solid features

Extrude and cut

Give the direction as a world vector rather than “positive” or “negative”. Positive means different things on different planes and in different CAD systems; +Z does not.

Extrude the sketch 40 mm in the +Z direction

Cut 10 mm into the body in the -X direction

Extrude the sketch 30 mm symmetric about the sketch plane with a 3 degree draft

If a cut reports success but the volume did not change, the direction was wrong. Say so and ask for the flip:

The volume did not change — flip the cut direction and try again

Revolve

An axis named simply “X” passes through the world origin. For an axis anywhere else, give a point on the axis and its direction — this is the most common cause of a revolve that produces a giant ring instead of a shaft.

Revolve the profile 360° about an axis through (0, 0, 25) in the X direction

Revolve-cut the groove profile 360° about the Z axis

Sweep and loft

Sweep the 8 mm circle profile along the path sketch

Create a helical sweep: 6 mm profile, 30 mm diameter, 5 mm pitch, 8 turns

Loft between Sketch1, Sketch2 and Sketch3, normal to the profile at both ends

Lofts accept guide curves, tangency conditions at each end (none, normal to profile, tangent to face, or a direction), and a closed-loop option.

Fillets — identify edges by world point

This is the technique that makes fillets reliable. Give one world-coordinate point near the midpoint of each edge you want blended, in millimetres. Each point selects exactly the nearest body edge; nothing else is filleted.

Add an R8 fillet to the four cut-end edges. Use these world midpoints in mm: [[-90,-13.3,20.2],[-90,13.1,44.1],[-90,-13.3,44.1],[-90,13.1,20.2]]. Report the per-edge evidence and the volume change.

Where do you get the points? Ask for them:

List the edges of this body with their type, length and midpoint coordinates

Descriptive selection also works for the easy cases — and is fine when the geometry is unambiguous:

Add a 3 mm fillet to all the edges of the top face

Add a 2 mm fillet with tangent propagation along the rib

Reading a fillet result

Per-edge evidence — each edge's type, midpoint, length, and the distance from the point you gave. A distance of 0.00 mm means a dead-on pick.
Measured volume change. A fillet on a convex edge removes material; on a concave edge it adds. Zero change means nothing happened.
Refusals name the real geometry. If your point is more than about 3 mm from any edge, or two edges are within half a millimetre of being equally close, the operation stops and tells you the candidates and their actual coordinates — which is exactly what you need to correct the request.

If a fillet fails on what looks like a single edge, the run has probably been split into several segments. Ask for one fillet with a point on every segment of the chain; tangent propagation will not bridge a non-tangent junction.

Chamfers

Add a 2 x 45° chamfer to the four vertical corner edges

Add a 1.5 mm chamfer to all edges of the bore

Holes and threads

Hole types: simple, counterbore, countersink and tapped. A tapped hole creates a genuinely threaded hole. Target a face either by asking for the face from a query, or by naming its outward normal as a world axis — x, -x, y, -y, z, -z.

Add a Ø12 mm through hole at (30, 20) on the face whose outward normal is +Z

Add an M8 tapped hole 20 mm deep at the centre of the top face

Add a Ø10 counterbore, 16 mm counterbore diameter, 6 mm deep, at (25, 25)

If the face you asked for cannot be resolved, the operation fails rather than drilling some other face and reporting success. Read the error and name the face differently — usually by getting it from a face query first.

Threads can also be added to an existing hole or shaft. Leave the diameter out and the thread is derived from the hole's actual measured geometry, which is more reliable than typing a size that may not match:

Add an ISO internal thread to the Ø8.5 hole — derive the size from the hole itself

Add an M20 x 2.5 external thread 30 mm long to the shaft end

Shell, draft, boolean, split

Shell the body to 2.5 mm wall thickness, removing the top face

Add 3° draft to the four side faces, using the bottom face as the neutral plane

Subtract the tool body from the main body

Split the body with the XY plane and keep both halves

Face-level edits

Offset the top face 4 mm outwards

Move the boss face 10 mm in +X

Reference geometry

Create a datum plane 25 mm above the top face

Create a datum axis through the centre of the bore

Create a coordinate system at (50, 0, 15) aligned with the world axes

Editing existing features

You never have to delete and rebuild to change a value. Refer to the feature by name and say what should change.

Change the extrusion depth to 25 mm

Change the fillet radius on Fillet2 from 5 to 8 mm

List every feature in the tree with its parameters

What are the dimensions of the feature called "Cut-Extrude1"?

Patterns and mirrors

Create a linear pattern of the hole: 4 instances, 20 mm apart in X

Create a rectangular pattern of the hole: 3 in X at 25 mm and 2 in Y at 40 mm

Create a circular pattern of the slot: 6 instances over 360° about the Z axis

Mirror the boss across the YZ plane

Mirror the whole body across a plane through (0,0,0) with normal (0,1,0)

Parameters and equations

Named parameters and driving equations can be listed, read, created, changed and exchanged as JSON — in all four 3D CAD systems, using each one's own mechanism.

List all parameters and equations in this part with their values and units

Create a parameter "Thickness" set to 15 mm and drive the extrusion depth from it

Set Thickness to 20 and rebuild

Export all equations to C:\parts\bracket_equations.json

Materials, appearance and properties

Assign 6061-T6 aluminium to this part and report the mass

What material libraries are available, and which steels do they contain?

Find materials with a density between 2600 and 2800 kg/m³

Colour the whole part light grey, and make the two bosses red

Make the housing 40% transparent

Set the Description property to "Clamp bracket" and Part Number to BR-2041

Show me all custom properties on this document

Measuring and querying

Measurement is how you check everything else on this page, so it is worth knowing what is available.

What is the volume, surface area, mass and centre of gravity?

Give me the exact bounding box — min and max corners and the size in X, Y and Z

List the faces with their type, area, centre and normal

List the edges with their type, length and midpoint

Which faces are adjacent to the top face?

What is the face opposite the mounting face, and what edges do they share?

What is the minimum distance between the two bosses?

Which face is at the point (30, 20, 15)?

How many solid bodies are in this part?

Verification prompts

Verify the volume is 144,000 mm³ within 0.5%

Verify there is exactly one shell feature and two fillet features in the tree

Verify the overall height is 15 mm

And the probe technique, for when volume alone cannot tell you where something is:

Cut a 1 mm test slab from Z=45 to Z=55 across the whole part, tell me the volume removed, then undo it

The volume removed tells you how much material genuinely exists in that height band — which a total volume never can. See Verifying results.

Checkpoints

Take a checkpoint called "before the shell"

Revert to the "before the shell" checkpoint

Sheet metal

Sheet metal is supported in all four 3D CAD systems (not AutoCAD). The first feature of a sheet metal part must be a base flange — not an extrusion — because that is what establishes the thickness, bend radius and the sheet body that everything else depends on.

Create a new sheet metal part, then a base flange from a 200 x 120 mm rectangle, 2 mm thick with a 2 mm bend radius

Add a 40 mm edge flange bent 90° down along the long front edge

Add a contour flange along the right edge from the profile sketch

Add a 6 mm open hem to the top edge

Add a 15 mm jog 60 mm from the left edge

Break the two front corners with a 3 mm radius

Create the flat pattern and tell me the flat size

Export the flat pattern to C:\cut\panel.dxf for the laser

In Solid Edge the part must be created as a sheet metal part before tabs and flanges will work — say “create a new sheet metal part” rather than creating a normal part and hoping.

Nesting for cutting

Nest the flat patterns of every part in C:\panels onto 2500 x 1250 mm sheets and export the layouts to C:\cut

How this runs depends on your CAD system:

CAD system	Nesting
Autodesk Inventor	Uses Inventor's own Nesting Utility — requires Inventor Professional with the Nesting Utility add-in installed.
Solid Edge	Uses Solid Edge's built-in Nest utility, which requires a Premium licence; otherwise falls back to the built-in engine.
SOLIDWORKS	No native nesting API — CoPilot's own nesting engine does the layout from exported flat-pattern DXFs.
Siemens NX	No native nesting API — same built-in engine as SOLIDWORKS.

Surfaces

Surface modelling is more unevenly supported than solid modelling, so check this table before planning a workflow around it.

Operation	SOLIDWORKS	Inventor	NX	Solid Edge
Offset surface	Yes	Yes	Yes	Yes
Extend surface	Yes	Yes	Yes	Yes
Trim surface	Yes	Yes	Yes	Yes
Thicken surface into a solid	Yes	Yes	Yes	Yes
Planar surface from boundary curves	Yes	Yes	Yes	No
Project curve onto a surface	No	No	No	No

Offset the top face 5 mm to a new surface, then thicken it 2 mm into a solid

Trim the surface with the boundary sketch and extend the remaining edge 10 mm

Design for manufacture

CoPilot can score a part against manufacturing rules and write the result up as a Word document, with screenshots.

Run a DFM analysis on this part for machining and tell me what fails

Run a full sheet-metal DFM report with screenshots and save it to C:\reports\panel_dfm.docx

Domains: machining, sheet metal, injection moulding, casting, 3D printing and welding, or let CoPilot infer the domain from the part.

Mould tooling

Draft analysis, parting lines, parting and shutoff surfaces, core/cavity split, mould bases, runners and cooling channels are available — but with real differences between CAD systems.

Operation	SOLIDWORKS	Inventor	NX	Solid Edge
Draft angle analysis	Yes	Yes	Yes	Yes
Parting line	Yes	Yes	Yes	Yes
Parting surface	Yes	Yes	Yes	Guidance only — creates a reference plane, not a surface
Shutoff surface	Yes	Manual only — you must name the opening faces	Yes	Guidance only
Core / cavity split	Yes	Yes	Yes	Yes
Mould base, runners, cooling channels	Yes	Yes (built from plate geometry)	Yes (built from generic modelling)	Guidance only

Analyse this part for draft with a 1.5° minimum and a Z pull direction, and list the faces that fail

Create the parting line and split the core and cavity along Z

“Guidance only” means CoPilot replies with what to do and why, but creates no geometry. Read the reply — it says so.

Import and export

Export this part to STEP at C:\transfer\bracket.step

Export to STL for printing

Open C:\transfer\housing.step

STEP, IGES, STL, Parasolid, SAT and JT are available for solids; PDF, DXF and DWG for drawings. To move a part with its feature history instead of as a dumb solid, see Feature Tree Translation.

Known gaps worth knowing about

Not currently available in any CAD system: projecting a curve onto a surface, and CAM setup / toolpath generation. Requests in these areas will not produce geometry — on some CAD systems the reply may nevertheless read as though something was done, which is exactly why the measurement habits on this page matter.

Face divide, face delete and face replace are similarly unreliable outside SOLIDWORKS. If you use them, verify with a face count and a volume before building on the result.