Skip to content

CAM Workbench

In one sentence: The CAM workbench generates CNC toolpaths from a 3-D model — you set up a Job, add machining operations (profile, pocket, drilling, engraving), apply dress-ups (tabs, lead-ins, dogbone corners), simulate the result, and post-process to G-code for your machine.

What is the CAM workbench for?

CAM (Computer-Aided Manufacturing, formerly called Path) produces machine-readable G-code from FreeCAD geometry. It supports:

  • 2.5D milling — profiling, pocketing, face milling, slot milling, adaptive clearing, helix drilling.
  • 3D machining — 3-D pocket, surface machining, and waterline passes (the last two require the optional OpenCamLib library).
  • Drilling — drilling, boring, and (experimental) tapping cycles.
  • Engraving and V-carving — following edges, text, or artwork at varying depths.
  • Dress-ups — post-processing modifiers applied on top of operations: holding tabs, lead-in/out arcs, dogbone corner compensation, ramping entry.

The output is machine-neutral — a post-processor script converts the internal path representation to the G-code dialect of a specific controller (Grbl, LinuxCNC, Mach3, Fanuc, etc.).

The Job — the central document object

Everything in the CAM workbench lives inside a Job object (Path::Job / CAM_Job). The Job holds:

  • A reference to the model (the Part Design body or solid to be machined).
  • Stock — the raw material block (auto-sized bounding box or custom).
  • Tool Controller list — which tool bits are used, with feed/speed.
  • Setup Sheet — default feeds, speeds, and depths for the job.
  • Operations — the list of machining operations, in execution order.

The Job is created first; all operations are added to it. G-code is produced by running Post Process (CAM_Post) which calls the selected post-processor script.

Concepts

Coordinate system

CAM uses the same coordinate system as the FreeCAD model. The origin is typically at the bottom-left-front corner of the stock, or at the top-centre of the stock (depending on the post-processor configuration). Always check your machine's work coordinate system (WCS) matches.

Tool Controllers

A Tool Controller (CAM_ToolController) connects a tool bit to a set of parameters:

Parameter Description
Tool Reference to a tool bit definition
Feed rate (horizontal) XY cutting feed in mm/min
Feed rate (vertical) Z plunge feed in mm/min
Spindle speed RPM
Spindle direction CW / CCW

Each operation can be assigned a specific Tool Controller from the job's list.

Stock

The Stock defines the workpiece material envelope. It can be: - Box stock — auto-computed bounding box of the model + an offset. - Cylinder stock — circular bar stock. - Extended box — manual dimensions. - From existing solid — use an existing FreeCAD shape.

Depths and heights

Each operation has depth parameters:

Parameter Meaning
Start Depth Z level where the tool first engages
Final Depth Z level at the bottom of the cut
Step Down Maximum depth of cut per pass
Clearance Height Z level for rapid moves between cuts
Safe Height Z level for rapid moves over stock

Workflow overview

Create Part Design solid
        │
        ▼
CAM → New Job (select solid, configure stock)
        │
        ▼
Add Tool Controllers (select tool bits, set feeds/speeds)
        │
        ▼
Add Operations (Profile, Pocket, Drilling, …)
  for each operation:
    ├── Select geometry (faces, edges, holes)
    ├── Set depths (Start Depth, Final Depth, Step Down)
    └── Configure operation-specific parameters
        │
        ▼
Apply Dress-ups (Tabs, LeadInOut, Dogbone, RampEntry, …)
        │
        ▼
Simulate (GL Simulator or legacy Simulator)
        │
        ▼
Post Process → G-code file

Post-processors

FreeCAD ships with post-processors for common controllers:

  • grbl — for Grbl-based routers and laser cutters
  • linuxcnc — LinuxCNC / EMC2
  • mach3_milling, mach4_milling — Mach3/Mach4
  • centroid — Centroid CNC controllers
  • fanuc — Fanuc-compatible controllers
  • smoothie — Smoothieware
  • Many others in Path/Post/scripts/

Post-processors are Python scripts in Mod/CAM/Path/Post/scripts/. Custom post-processors can be added to the user's macro directory.

See also