Using Z Probe With LinuxCNC

Z axis probing is a nice addition to a CNC allowing for accurate locating of the top surface of a workpiece. I made a touchplate from a 5mm disc of aluminium, a crocodile clip, and a length of 2 pin cable. 

The operating principle is simple:

• Move the CNC spindle in the XY plane and position over the workpiece. Lower the Z axis so the bit is approximately 10mm above the workpiece.
• Place the probe plate on the work piece surface under the bit. This forms one contact of a switch.
• Attach the second wire to the spindle bit using the crocodile clip. This forms the second contact of the switch.
• G-code G38.2 probe command is issued to lower the bit until it touches the probe plate and completes the circuit. The Z axis zero is calculated as the contact position minus the thickness of the probe plate. 

To configure LinuxCNC for Z probing there are a number of elements to configure. First is the physical wiring of the probe. My CNC uses a Mesa 7i96 controller which has 11 opto-isolated inputs. The probe is set up as a sourcing input on the Mesa card with the input common pin connected to +5V. The connection to the spindle bit is connected to ground as the spindle chassis is typically grounded.

LinuxCNC Z Probe Wiring
Mesa Input Common (COM+)	+5V
Spindle bit	GND
Probe plate	Mesa Input 6

LinuxCNC HAL uses pin motion.probe−input during probing. G-code G38.n probe commands uses the value on this HAL pin to determine when the probe has made contact with the touch plate. Edit the io.hal file and add a net to connect Mesa card input 6 to the HAL motion.probe-input pin.

  net probe-input motion.probe-input <= hm2_7i96.0.gpio.006.in

The PyVCP (Python Virtual Control Panel) allows the LinuxCNC AXIS interface to be customised. In the LinuxCNC config folder create a file called ztouch.xml and add the following definition for a 'Touch Off Z' button. 

  <?xml version='1.0' encoding='UTF-8'?>

  <pyvcp>

    <button>

      <relief>RAISED</relief>

      <bd>3</bd>

      <halpin>"ztouch"</halpin>

      <text>"Touch Off Z"</text>

      <font>("Helvetica",16)</font>

    </button>

  </pyvcp>

In the postgui.hal file add a net connecting the newly created button (pyvcp.ztouch) to a MDI command (halui.mdi-command-00). This command will later be used to call the G-code probe subroutine file.

  net ztouch halui.mdi-command-00 <= pyvcp.ztouch


I place my subroutines in a subfolder of my LinuxCNC config folder, linuxcnc/configs/subroutines/. In this folder create a file called z_touch.ngc and add the following G-code subroutine to perform Z axis probing.

  O <z_touch> sub

  G10 L20 P0 Z0 (set current Z = 0)

  G91 (switch to relative coordinates)

  G38.2 Z-10 F25 (probe down using a fast feedrate)

  G92 Z5.0 (set Z = plate thickness)

  G0 Z.1 F10 (move up by 0.1mm)

  G38.2 Z-1 F1 (2nd pass: probe down using a slow feedrate to get better accuracy)

  G92 Z5.0 (set Z = plate thickness)

  G90 (switch to absolute coordinates)

  G0 Z10 F25 (move to 10mm above work piece)

  O <z_touch> endsub

Now to link all these parts together in the config ini file by adding a DISPLAY reference to the new button definition XML file, set SUBROUTINE_PATH to the location of the G-code subroutine file, define the POSTGUI_HALFILE to load once the LinuxCNC AXIS GUI has started, and finally the definition for the MDI_COMMAND which is used to call the probing subroutine.

  [DISPLAY]

  PYVCP = ztouch.xml

  [RS274NGC]

  SUBROUTINE_PATH = /home/seand/linuxcnc/configs/subroutines/

  [HAL]

  HALFILE = io.hal

  POSTGUI_HALFILE = postgui.hal

  HALUI = halui

  [HALUI]

  # Z axis touch plate subroutine

  MDI_COMMAND = O <z_touch> CALL