Skip to content

Tool Controller

In one sentence: A bridge between a tool bit definition and a Job operation — stores the feed rates, spindle speed, and tool number for a specific tool in a specific job.

Overview

Workbench: CAM
Command: CAM_ToolController

A Tool Controller (CAM::ToolController) connects a tool bit from the library to a Job. While the tool bit file stores the tool's geometry, the Tool Controller stores the cutting parameters for that tool in the context of the current job: feed rates, spindle speed, and tool number.

Intuition

The same end mill may be run at different speeds and feeds depending on the material. The tool bit file is the geometry (diameter, flute count); the Tool Controller is the recipe (RPM, feed rate) for a particular job. Multiple Tool Controllers in the same job can reference the same tool bit with different speeds and feeds.

Tool Controller properties

Property Description
Tool Reference to the tool bit (.fctb file)
HorizFeed Horizontal cutting feed rate (mm/min)
VertFeed Vertical (plunge) feed rate (mm/min)
SpindleSpeed Spindle speed (RPM)
SpindleDir Clockwise (CW) or counter-clockwise (CCW)

Adding a Tool Controller

  1. Open the Tool Bit Library or Tool Bit Dock.
  2. Select a tool from the library.
  3. Click Add to Job or drag the tool onto the Job.
  4. A new Tool Controller appears in the Job's tool controller list.
  5. Set the HorizFeed, VertFeed, SpindleSpeed, and SpindleDir properties.

Assigning a Tool Controller to an operation

Each operation has a Tool Controller property. Click the dropdown in the operation's properties and select from the job's tool controller list.

Calculating feeds and speeds

FreeCAD does not auto-calculate feeds and speeds — you must set them manually or use a separate speeds-and-feeds calculator.

A rough starting guide:

RPM from surface speed:
  RPM = (surface_speed_m_min × 318.3) / diameter_mm

Feed rate:
  feed_mm_min = RPM × chip_load_mm × number_of_flutes
Material End mill surface speed (m/min)
Aluminium 200–500
Mild steel 30–60
Hardwood 100–200
MDF / Plywood 100–300
HDPE / Acrylic 150–400

Always verify feeds/speeds against your tool manufacturer's data

The values above are starting approximations. Tool geometry, coolant, machine rigidity, and material grade all affect safe cutting parameters.

Common mistakes and pitfalls

All operations use the same tool

Each operation's Tool Controller property defaults to the first tool controller when the operation is created. Explicitly set the Tool Controller for every operation.

Spindle speed is zero in the G-code

The Tool Controller's SpindleSpeed defaults to 0. Always set a non-zero RPM value before running the post-processor.

See also