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FreeCAD document setup

Summary

Before modelling any part, a correctly configured FreeCAD document must exist with the Variables spreadsheet populated and the global preferences set. This is done once per build. Skipping or rushing this step creates hard-to-debug problems later — missing aliases cause sketch dimensions to fail silently, and wrong units or navigation settings cost hours of confusion. The entire setup takes under ten minutes using the FCMacro.

Concept

Why setup before modelling

FreeCAD preferences (navigation style, units, decimal places) affect how the model behaves during editing. Wrong settings do not break the model but they make it significantly harder to use — CAD navigation feels wrong, dimensions show in incorrect units, and the sketcher solver gives misleading messages.

The Variables spreadsheet must exist before any sketch references a variable. A sketch that references =Variables.ArmWidth on a document that has no Variables spreadsheet generates a broken reference that is annoying to fix retroactively. Create the spreadsheet first, model second.

Reference

Required FreeCAD version

FreeCAD 1.1 stable — download from https://www.freecad.org/downloads.php

FreeCAD 1.0 is also compatible but 1.1 has improved topological naming resistance. Do not use nightly/development builds — they may introduce instability mid-build.

Preference settings — set once after install

Preference location Setting Value
Edit → Preferences → Display → Navigation Navigation style CAD
Edit → Preferences → Display → Navigation Zoom at cursor Checked
Edit → Preferences → General → Units Unit system Standard (mm/kg/s)
Edit → Preferences → General → Units Number of decimals 3

Document structure

One .FCStd file contains the entire drone model:

Variables ← Spreadsheet (create first) Body: Arm Body: Arm Tab Body: Arm Cover Active Body: Arm Cover Passive Body: X Body PCCF Base Body: X Body PETG Bottom Body: X Body PETG Top Body: Platform Body: Backplane Body: GPS Camera Bracket Body: Camera Tilt Plate Body: ASA Bumper Assembly

Macro locations by OS

OS Macro folder
macOS ~/Library/Preferences/FreeCAD/Macro/
Linux Flatpak Confirm via Tools → Macros → read path shown in dialog
Linux native ~/.FreeCAD/Macro/
Windows %APPDATA%\FreeCAD\Macro\

⚠ FreeCAD 1.1 Flatpak may use a versioned subfolder: ~/.var/app/org.freecad.FreeCAD/data/FreeCAD/1.1/Macro/ Always confirm the actual path via the dialog before copying macros.

Procedure

First-time FreeCAD setup

  1. Download and install FreeCAD 1.1 from https://www.freecad.org/downloads.php
  2. Launch FreeCAD.
  3. Linux Flatpak only: run once in terminal: flatpak override org.freecad.FreeCAD --filesystem=home
  4. Set navigation style: Edit → Preferences → Display → Navigation → Navigation style: CAD → Zoom at cursor: checked → OK.
  5. Set units: Edit → Preferences → General → Units → Unit system: Standard (mm/kg/s) → Decimals: 3 → OK.
  6. Close and reopen FreeCAD to confirm preferences applied.

Creating the document

  1. File → New (Ctrl+N).
  2. File → Save As → navigate to your libdrone project folder.
  3. Name: LD_V34.FCStd (or your preferred version identifier).
  4. Click Save.
  5. Ctrl+S immediately — FreeCAD does not autosave.

Installing and running the Variables macro

  1. Locate your FreeCAD Macro folder (see table above).
  2. Copy LD_V343_Variables.FCMacro into that folder.
  3. In FreeCAD: Tools → Macros.
  4. Select LD_V343_Variables from the list.
  5. Click Execute.
  6. The Variables spreadsheet appears in the Model Tree.
  7. Double-click Variables to open it — verify rows and aliases are present.
  8. Spot-check: click cell B1 → Properties → confirm Alias shows Wheelbase.
  9. Ctrl+S to save.

Verifying the spreadsheet

The spreadsheet should contain: - Column A: variable names (human-readable labels) - Column B: values (with aliases set — shown in Properties panel) - No empty alias cells in column B

If any alias is missing: right-click the cell → Properties → Alias → type the variable name exactly → OK. Variable names are case-sensitive.

Save discipline

FreeCAD has no autosave. Establish this habit immediately: - Ctrl+S every 10–15 minutes during active modelling - File → Save a Copy before any major edit session Name the copy with a version suffix: LD_V34_pre-xbody.FCStd - This is your restore point if topology breaks

Rationale

Why CAD navigation style specifically

FreeCAD supports multiple navigation styles (Blender, Inventor, OpenCascade, CAD). The CAD style matches the mouse button conventions used in most professional CAD software and in the FreeCAD Cookbook instructions. Using a different style means every pan/zoom/rotate instruction in the Cookbook maps to different mouse buttons, creating friction during the build.

Why 3 decimal places

libdrone dimensions range from 2.1 mm (rod channel interference fit) to 333 mm (rod length). Three decimal places gives 0.001 mm resolution — more than sufficient for 3D printing, which has a practical resolution of ~0.05 mm. Two decimal places is adequate but can cause rounding artefacts when variables are used in chains of calculations. Four decimal places adds no practical precision and clutters the dimension display.

Connections

requires: - parametric-modelling-philosophy related: - variable-table-structure - freecad-workbenches - topological-naming-problem leads_to: - variable-table-structure - freecad-workbenches