Tomas Mudrunka edited this page Aug 29, 2018 · 17 revisions

The WCS tab provides:

  • Work Coordinate Systems and TLO (Tool Length Offset)
  • An easy way to use the probe function of Grbl
  • Z mapping of a desired area for possible deformation in the z, and to compensate during the milling process, very useful for PCB milling when errors of a few microns can destroy the board

WCS (Work Coordinate System)

  • G54 to G59 buttons switch between different coordinate system
  • set button force coordinate for non null values of X,Y and Z input box
  • Zero button force all coordinate to zero
  • X=0, Y=0 and Z=0 force specific axis reference to zero
  • TLO set button save Tool Offset as specify into input box
  • G28, G30 and G92 send their relative commands to grbl


Just enter the 3 coordinates of the probe direction and click Probe. Once the probe hits or the path is ended the probed coordinate (Machine coordinate) will be displayed


  1. Be sure the machine has been homed.

  2. Enter the values of the working area you wish to probe on X/Y min and maximum coordinates.
    Alternatively, you can click on the button Margins which will get the margins of the loaded g-code file

  3. Set the number of steps in X and Y you wish to scan.

  4. Enter the Zmin for probing and Zmax (equivalent to Zsafe) and the desired feed rate for probing. Too high feed rates might results in inaccurate probing. Too slow will take quite some time. Height of probe tip must be less than Zmax above the work surface.

  5. When everything is ready and the probe tool is connected click on Scan. bCNC will run a probing cycle testing every individual point and its z coordinate will be displayed on the canvas. (If you have the Menu->View->Probe selected)

  6. Once the probe cycle is finished move the gantry to any location you wish to set the z coordinate as known/set and click the Zero (on the autoLevel screen). This action will make the z-height map relative to this X/Y location. Then set z-axis to zero.

  • Failure to click Zero under Probe -> Autolevel will prompt you with a dialog box. This is a safety feature to prevent machine crashes when loading a probe file.

    • Dialog box of Error
  • An easy way is to move to any desired location X/Y inside probed area

  • Use the Probe command on the Probe Group Box to probe only in negative Z direction

  • When the tool touches the surface click on the Set Zero

  • Set the Z coordinate as zero using the Z=0 button

  1. Now if you run a g-code with the probe information loaded the g-code will be altered during run-time to take care of the z-deformation.


  1. G1 commands will be split in multiple segments if needed.
  2. G2/G3 commands will be converted to multi-line segments (unfortunately). The precision of the conversion is controlled in the Configuration with the variable accuracy.
  3. Probing information can be saved/recall from a file. Menu->File->probe.
  4. The probe information file must be given a .probe extension.
    WARNING If a file exists with the same filename as the g-code and with an extension .probe it will automatically be loaded. This can be dangerous if it is done by mistake!

External Reference

  • A good post on PCB-Milling experience using bCNC as autoleveler (courtesy of Frank Piesik)
You can’t perform that action at this time.
You signed in with another tab or window. Reload to refresh your session. You signed out in another tab or window. Reload to refresh your session.
Press h to open a hovercard with more details.