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