FreeCAD 1.1.x UI click map

Summary¶

This article is a version-locked UI click map for FreeCAD 1.1.x. It documents exact menu paths, dialog names, toolbar locations, and keyboard shortcuts for every operation used in libdrone modelling. When FreeCAD changes its UI in a future release, only this article needs updating — all geometry articles and the FreeCAD skeleton document remain valid because they reference operations by name, not by click path.

Use this article alongside the FreeCAD skeleton document. The skeleton tells you what to do. This article tells you exactly where to click to do it.

Verified against: FreeCAD 1.1 stable (all platforms). macOS primary.

Concept¶

Reference¶

Screen layout — FreeCAD 1.1¶

┌─────────────────────────────────────────────────────────┐
│  Menu bar: File  Edit  View  Tools  [Workbench menus]   │
│  Toolbar row 1: [Workbench dropdown] [tool icons]       │
├──────────────┬──────────────────────────────────────────┤
│              │                                          │
│  Model Tree  │           3D Viewport                    │
│  (left panel)│           (centre)                       │
│              │                                          │
│  Tasks panel │                                          │
│  (appears    │                                          │
│  below tree  │                                          │
│  during ops) │                                          │
├──────────────┴──────────────────────────────────────────┤
│  Status bar: coordinates / solver state / snap info     │
└─────────────────────────────────────────────────────────┘

The Workbench dropdown is in the top toolbar, left side. In FreeCAD 1.1 it may show as a text label or an icon depending on your toolbar configuration. If you cannot find it: View → Toolbars → Workbench → enable.

A — First-time preferences¶

Set navigation style¶

Edit → Preferences → Display → Navigation (tab)
  Navigation style: CAD
  Orbit style: Rounded Arcball (default in 1.1 — leave as is, or change to Trackball)
  ☑ Zoom at cursor
Click OK

⚠ FreeCAD 1.1 introduced Rounded Arcball as the default orbit style. If you opened Preferences and see Rounded Arcball already selected — this is correct for 1.1. The Cookbook was written against an earlier default. CAD navigation style still applies; only the orbit sub-style changed.

Set units¶

Edit → Preferences → General → Units (tab)
  Unit system: Standard (mm/kg/s)
  Number of decimals: 3
Click OK

B — Macros¶

Find macro folder (do this first — path varies by OS and install method)¶

Tools → Macros
  Read the "Macro path:" shown at the top of the dialog
  This is where to copy .FCMacro files
Close

Run a macro¶

Tools → Macros
  Select macro name from list
Click Execute

First-time Flatpak filesystem access (Linux only — run once in terminal)¶

bash
flatpak override org.freecad.FreeCAD --filesystem=home

C — Documents¶

New document¶

File → New    (Ctrl+N)

Save / Save As¶

File → Save           Ctrl+S
File → Save As        Ctrl+Shift+S
File → Save a Copy    (use before major edits — creates a restore point)

⚠ FreeCAD has no autosave. Ctrl+S regularly. Save a Copy before any session where you will make significant structural changes to the model.

D — Workbench switching¶

Workbench dropdown (top toolbar) → select workbench name

Switching workbench does not close or lose current work.

E — Spreadsheet workbench¶

Create a spreadsheet¶

Workbench → Spreadsheet
Spreadsheet menu → Create Spreadsheet
Model Tree: right-click "Spreadsheet" → Rename → type: Variables → Enter
Double-click Variables to open the grid

Set an alias on a cell¶

Right-click the cell (column B) → Properties
  Alias field: type the variable name exactly (case-sensitive)
Click OK

Reference a variable in a sketch dimension¶

Type exactly: =Variables.VariableName Example: =Variables.ArmWidth

The prefix Variables. is always required. No # prefix (that was the Variables file notation — FreeCAD uses the spreadsheet name as prefix).

F — Part Design workbench — bodies¶

Create a new Body¶

Workbench → Part Design
Part Design menu → Body → Create Body
  (alternative: Model menu → Body → Create Body)
Model Tree: right-click the new Body → Rename → type name → Enter

The active Body is shown in bold in the Model Tree. All features you create next belong to this Body.

Activate a different Body (if you have multiple)¶

Model Tree: double-click the Body to activate it

G — Part Design workbench — datum planes¶

Create a datum plane¶

Part Design menu → Datum → Create a Datum Plane
  (alternative: Part Design toolbar → datum plane icon)

In the Attachment dialog: Select a reference (base plane, face, or another datum plane) Attachment mode: choose mode (Flat Face, XY/XZ/YZ Plane, etc.) Offset: type value in Z field to move the plane outward Click OK

After creating: rename immediately in the Model Tree.

Model Tree: right-click datum plane → Rename → type descriptive name → Enter
Example: DatumPlane_MotorHead, DatumPlane_RodTop

H — Sketcher — creating sketches¶

Create a sketch on a base plane¶

Model Tree: click the plane to select it (XY_Plane, XZ_Plane, or YZ_Plane)
Sketch menu → New Sketch
  (alternative: Part Design toolbar → New Sketch icon)

Sketcher opens. Grid and axes appear in viewport.

Create a sketch on a datum plane¶

Model Tree: click the datum plane to select it Sketch menu → New Sketch FreeCAD offers to use the selected plane → click OK

Create a sketch on a face (use sparingly — topological naming risk)¶

Viewport: click the face to select it
Sketch menu → New Sketch
  FreeCAD offers to use the selected face → click OK

Prefer datum planes over face references wherever possible.

Close a sketch¶

Sketcher Tasks panel (left): click Close button
  (alternative: press Escape)
  (alternative: Sketch menu → Close Sketch)

I — Sketcher — geometry tools¶

Rectangle (centred)¶

Sketcher menu → Sketcher Geometries → Create Rectangle
  In the dropdown next to the tool: select Centered Rectangle
Click once at origin (0,0) → move mouse → click to set approximate size

Circle¶

Sketcher menu → Sketcher Geometries → Create Circle
Click centre point → move mouse → click to set approximate radius

Sketch fillet (rounds 2D corners)¶

Sketcher menu → Sketcher Geometries → Create Fillet
Click a corner point (where two lines meet)
Type radius value in the Tasks panel → Enter
Repeat for each corner

This is a 2D sketch fillet — different from Part Design 3D Fillet.

Line¶

Sketcher menu → Sketcher Geometries → Create Line
Click start point → click end point → right-click to stop

J — Sketcher — constraints¶

Dimension (generic — applies horizontal, vertical, or angular automatically)¶

Sketcher menu → Sketcher Constraints → Constrain internal angle
  (or press D in Sketcher for dimension shortcut)
Click the element to constrain
Type value or formula in dialog → OK

Horizontal distance (X distance between two points)¶

Sketcher menu → Sketcher Constraints → Constrain Horizontal Distance
Click element or two points
Type value or =Variables.Name → OK

Vertical distance (Y distance between two points)¶

Sketcher menu → Sketcher Constraints → Constrain Vertical Distance
Click element or two points
Type value or =Variables.Name → OK

Coincident (two points or a point and origin share position)¶

Select two points (Ctrl+click both)
Sketcher menu → Sketcher Constraints → Constrain Coincident
  (alternative: press C)

Fully constrained check¶

A fully constrained sketch shows all elements green. Status bar at bottom shows: Fully constrained

White or yellow elements are under-constrained — add more dimensions or constraints until all turn green before closing the sketch.

K — Part Design — features¶

Pad (push sketch into 3D)¶

Model Tree: click the sketch to select it
Part Design menu → Additive → Pad
  (alternative: Part Design toolbar → Pad icon)

In Pad dialog:
  Type: Dimension
  Length: type value or =Variables.Name
  Symmetric: leave unchecked (pad in one direction only)
  Reversed: check if solid appears on wrong side
Click OK

Pocket (remove material)¶

Model Tree: click the sketch to select it Part Design menu → Subtractive → Pocket

In Pocket dialog: Type: Through All (for channels and holes that go full depth) — or — Type: Dimension → type depth value Reversed: check if cutting in wrong direction Click OK

Additive Loft (blend between two profiles)¶

Part Design menu → Additive → Additive Loft

In Loft dialog:
  Profile section → Add Section → click first sketch
  Add Section again → click second sketch
  Closed: unchecked
  Ruled: unchecked (smooth blend)
Click OK

The two sketches must be on parallel planes at different positions.

Part Design Fillet (rounds 3D edges)¶

Select edge(s) in viewport (Ctrl+click for multiple edges)
Part Design menu → Fillet
  Size: type radius value
Click OK

This is the 3D edge fillet — different from Sketcher 2D fillet.

Part Design Chamfer¶

Select edge(s) in viewport
Part Design menu → Chamfer
  Size: type chamfer size
Click OK

L — Fixing broken features¶

Yellow warning triangle in Model Tree¶

Model Tree: click the warned feature
Tasks panel: read what reference was lost
Re-select the lost reference (face, edge, datum plane) in the viewport
Click OK

This is the topological naming problem. It is normal. It is always fixable. Do not delete and recreate — re-select the reference.

Sketch solver messages¶

While in Sketcher:
Sketch menu → Sketcher Preferences → General
  Solver messages: set to Full / Verbose

M — Assembly workbench¶

Create an assembly¶

Workbench → Assembly
Assembly menu → Create Assembly
  (alternative: Assembly toolbar → Create Assembly icon)
Model Tree: rename the assembly container

Insert a component (Body) into the assembly¶

Assembly menu → Insert Component
  Navigate to the Body → select → Insert
  (alternative: drag a Body from the Model Tree into the Assembly container)

Create a fixed joint (anchors first part to world origin)¶

Assembly menu → New Joint → Fixed Joint
Select the Body to fix
Click OK

Create a coincident joint (face-to-face flush)¶

Assembly menu → New Joint → Coincident
Select first face → select second face
Click OK

Solve assembly (applies all joints)¶

Assembly menu → Solve Assembly

Interference check¶

Tools menu → Part → Check Geometry → Check for Intersections

Section cut view¶

View menu → Standard Views → Section Cut
Select plane: XY / XZ / YZ
Adjust Z offset slider to desired height

N — STL export¶

Export a single Body as STL¶

Model Tree: right-click the Body → Export Mesh
  (alternative: select Body → File → Export)

In export dialog:
  Format: STL Mesh
  Units: mm  ← verify — not inches
  Deviation: 0.01 mm

Click Save

O — Viewport navigation (CAD style)¶

P — Essential keyboard shortcuts¶

Q — Common mistakes and fixes¶

Procedure¶

Rationale¶

Why a separate UI article rather than UI steps in each geometry article¶

FreeCAD changes its menu structure, dialog names, and toolbar layouts between releases. If UI clicks are embedded in geometry articles, every FreeCAD update requires hunting through all affected articles to find and correct the stale paths — typically while mid-build and under time pressure.

Isolating UI paths here means a FreeCAD release that moves a menu item requires updating one article. All geometry articles and the skeleton document remain unchanged. The versioning (freecad-ui-110, freecad-ui-120) makes it clear which UI map applies and when a new one is needed.

Why this is version-locked to 1.1.x¶

FreeCAD 1.0 shipped the Assembly workbench built-in. FreeCAD 1.1 changed the default orbit style to Rounded Arcball and refined the Assembly joint workflow. Future versions may move menus further. Each major UI change that affects libdrone modelling steps warrants a new article. Minor patch releases within 1.1.x are covered here unless they introduce breaking UI changes.

Connections¶

requires: [] related: - freecad-document-setup - freecad-workbenches - parametric-modelling-philosophy leads_to: - freecad-document-setup - variable-table-structure