CAM Probe

CAM Probe CAM Probe

Menu location

CAM  Supplemental Commands  Probe

Workbenches

CAM

Default shortcut

None

Introduced in version

-

See also

Z Depth Correction

Description

The CAM Probe CAM Probe command creates a Probe operation. The operation generates a rectangular grid of straight-probe moves (G38.2) over the Job Stock and records the probed Z values in a file. The resulting file can be used by the Z Depth Correction dressup to adapt a toolpath to a surface that is not parallel to the machine bed (for example PCB auto-levelling). The operation requires a Tool Controller whose Tool Bit uses the probe Tool Shape.

Usage

  1. Select CAM  Supplemental Commands  Probe (a Job must exist; the command is not on a toolbar).

  2. In the task panel set the number of grid points, the probe offsets and the output file name.

  3. On the Tool Controller tab select a Tool Controller with a probe Tool Bit; otherwise the error "This operation requires a tool controller with a probe tool" is shown.

  4. Set Final Depth (the lowest Z the probe may travel to) and Safe Height (the Z from which each probe move starts) on the Depths and Heights tabs.

  5. Press OK.

Options

The task panel provides:

  • Probe grid points X/Y: number of probe points along X and Y (3 to 1000). Points are spread evenly between the minimum and maximum of the Stock (or Base Shape) bounding box.

  • X offset / Y offset: offset between the probe tip and the tool position, added to every probe point.

  • File name: output file the controller should write the probe results to (default ProbePoints.txt), with a … save-file button.

  • Depths: Final depth is the probe target Z.

  • Heights: Safe height is the start Z of each probe move, Clearance height is used for the first rapid.

  • Tool Controller: must reference a Tool Bit with the probe shape.

Generated G-code

The operation emits a comment (Begin Probing <file name>), a rapid to Clearance Height, then for every grid point: G0 X Y Z<SafeHeight>, G38.2 Z<FinalDepth> F<vertical feed of the Tool Controller>, G0 Z<SafeHeight>, and finally the comment (PROBECLOSE). introduced in 26.3: the opening and closing comments carry the annotations probe_open (with the file name) and probe_close so that Post-Processors can open and close the probe log file; currently only the OpenSBP Post-Processor implements this.

Properties

Probe

  • Xoffset (Length): X offset between tool and probe.

  • Yoffset (Length): Y offset between tool and probe.

  • PointCountX (Integer): Number of points to probe in X-direction.

  • PointCountY (Integer): Number of points to probe in Y-direction.

  • BaseShape (Link): Limit probe area by shape; the grid is built on the shape’s bounding box and points outside the shape at final depth are skipped. Not exposed in the task panel. introduced in 26.3

Path

  • OutputFileName (File): The output location for the probe data to be written.

  • ToolController (Link), CoolantMode, Active, Comment, UserLabel, CycleTime: standard Operation properties.

  • The Operation works in the Work Plane that the Operation links to; an Operation with no link works in the XY of the Job.

Depth

  • StartDepth, FinalDepth, StepDown, FinishDepth, ClearanceHeight, SafeHeight: standard depth and height properties; only FinalDepth, SafeHeight and ClearanceHeight affect the probe moves.

Notes

  • FreeCAD ships a probe Tool Shape and a probe Tool Bit in the default library; the operation checks the Tool Bit’s shape name and refuses other tools.

  • The Z Depth Correction dressup reads a probe log in the LinuxCNC G38 format (one line per point with 9 coordinates XYZABCUVW); the file produced by your controller must follow that format.

Scripting

See also: FreeCAD Scripting Basics.

Example:

import Path.Op.Probe

obj = Path.Op.Probe.Create("Probe", parentJob=job)
obj.PointCountX = 5
obj.PointCountY = 5
obj.OutputFileName = "/tmp/ProbePoints.txt"
FreeCAD.ActiveDocument.recompute()