Exercise 1. Four holes in a plate — your first model in 5 minutes

Input files	Time	What you end up with	What you learn
none	5 min	plate.FCStd — one Body (Pad + Pocket), 5 parameters	Building by talking, checking, changing dimensions, saving

Original and finished

There is no original file. You build it from dimensions alone.

Finished One Body — Pad + Pocket, two sketches at DoF 0, volume 29,316 mm³

	File	Description	Size
Finished	01-plate-done.FCStd	FreeCAD file	15 KB
Finished	01-plate-done.step	STEP	13 KB
Finished	01-plate-done.stl	STL	52 KB

The finished files are real

They were produced by running this page’s steps on FreeCAD 1.1.3, and the image is an actual screen capture of that file opened in the FreeCAD 1.1.3 GUI (isometric, white background). Download it and you can look at the tree, the sketches and the Params directly.

Setup

1. Launch FreeCAD 1.1.3. Check the Report view for [CAD X-ray] 서버 시작 http://127.0.0.1:9877 (툴 36개).
2. File → New. Keep exactly one document open.
3. In a terminal, go to your working folder and open your AI tool (claude, codex, gemini).

Steps

1. Check the connection

Say this

Check the FreeCAD connection and tell me the open document.

What the AI does — reads the FreeCAD version and the open document.

What the AI says back

Connected to FreeCAD 1.1.3. Open document: Unnamed (0 objects).

2. Make the plate

Say this

A 100×60×5 plate, origin at its bottom-left corner. Put the dimensions in a Params spreadsheet as width, height, thickness. Iso screenshot when done.

What the AI does — creates a Body, draws a rectangle sketch on XY with every constraint applied (DoF 0), and pads it 5 mm. The three dimensions go into the Params spreadsheet as aliases, and the sketch and the Pad reference those cells. It recomputes, confirms there are no errors, and shows you a screenshot.

How to check — the tree gains Params and Body › Sketch, Pad (the spreadsheet sits outside the Body). Double-click the sketch and the status bar at the bottom says “fully constrained”. Close to leave.

If no screenshot appears

Codex and Gemini may summarise images as text. Look at the FreeCAD window directly with View → Standard views → Axonometric (key 0).

3. Drill the holes

Say this

Four Ø6.6 through holes, 10 in from each corner. Diameter Params.hole_d, corner distance Params.margin.

What the AI does — creates a sketch with four circles at the top face height (centres at (10,10), (90,10), (10,50), (90,50)), sets the diameter constraint to the expression Params.hole_d, and cuts them through with a Pocket. It recomputes and confirms again.

How to check — the tree gains Sketch001, Pocket. Double-click Params and you see five rows (width 100, height 60, thickness 5, hole_d 6.6, margin 10).

4. Confirm with numbers

Say this

Volume, sketch DOF, hole count and whether they go through.

What the AI says back

Volume 29,316 mm³ (plate 30,000 − 684 for four holes). Both sketches at DoF 0. Four Ø6.6 holes, all through, rectangular pattern 80×40.

Subtract the hole volume (π × 3.3² × 5 × 4 ≈ 684) from 30,000 and you get the right number.

5. Change a dimension — what parametric means

Do this one yourself, without the AI. Double-click Params in the tree, change thickness from 5 to 8, and recompute (F5, or Edit → Refresh). The plate gets thicker and the holes still go through. Put it back to 5.

You can have the AI do it too.

Say this

Set margin to 12 in Params, recompute, and check nothing broke.

6. Save

Say this

Save it to D:\cad-work\plate.FCStd.

How to check — the window title changes to plate and the file appears at that path. The AI does not save before you say this.

Checking your result

Item	Criterion
Tree	Params, Body › Sketch, Pad, Sketch001, Pocket
Sketch DoF	both 0
Volume	about 29,316 mm³ (at thickness 5, margin 10)
Params	width, height, thickness, hole_d, margin
Recompute	0 objects in error

When it doesn’t work

• “Cannot connect” — FreeCAD is closed or the server did not start. See Troubleshooting.
• The AI asks which document — close the others or give it the name.
• The holes ended up outside the plate — you did not state the origin, so the plate got centred on the origin. Add “the bottom-left corner of the plate is the origin” and ask again.
• The sketch is not “fully constrained” — say “the Sketch still has degrees of freedom. Find what’s missing and show me candidates.” Same flow as Exercise 6.
• The plate went downward — say “reverse the Pad direction”.

Going further

1. Add R5 fillets on the four vertical edges and C0.5 chamfers at the hole mouths.
2. Instead of Ø6.6, just say “clearance holes for M6 bolts” and see what diameter the AI picks.
3. Take this plate through Exercise 7 and produce a three-view drawing.

What runs behind the scenes

Step	Tools
Connect	ping, list_documents
Plate and holes	build_features (pad, pocket, params)
Check	tracked_recompute, get_screenshot, analyze_shape, find_holes, get_sketch_diagnostics
Save	save_document