My CNC Workflow / Wasteboard Surface Patch

Macro 1: Move tool head to probe location in G53 Machine or Absolute Coordinates.

G53 G0 X-26.1 Y-5.3 Z-30.0;

G53 sets the following commands in the G53 machine or absolute coordinates. G0 is a rapid move – set by the maximum move speed in your firmware. My location for probing is X-26.1 Y-5.3 Z-30.0 but yours may differ. To find it put a tool into the spindle and after homing jog the machine to that location and take note of the G53 machine coordinates.

Macro 2: Two stage probe location.

G38.4 F500 Z-150;
G91 G1 F200 Z10;
G10 P1 L20 Z0;
G38.4 F50 Z-10;

G38.4 is the type of probe cycle using a normally closed signal, where the probe cycle will stop when the signal opens or is broken. F500 is the speed of the probing movement. Z-150 is the coordinate to move too in the G90 absolute movement type. In retrospect I could have written this differently, starting in G91 incremental or relative movement type, but as I knew the distance of my Z axis I kept it on G90. Upon contact of the probe, I change over to the G91 movement, and perform a G1 move to raise the tool head up 10mm at F200 speed. Returning to G90 and preform, setting the current Z location in the (P1) G54 WCS to zero, and performing another probe cycle at a slower rate.

What I’ve since change probing cycle too:

G38.4 F500 Z-150;
G1 F200 Z10;
G38.4 F50 Z-15;

Macro 3: Set G54 Work Coordinate System…

…so the tip of the current tool is on the surface of the wasteboard.

G10 P1 L20 X-24.6 Y33.7 Z-12.7;

To find this location, once probed I moved the tool to the location I wanted and updated the G10 Set workplace coordinate offset / tool offset command. P1 refers to the WCS which is G54, and L20 is a type of adjustment – so that the current tool head position has the specified coordinates.

Macro 4: Move to X Y Datum position

G53G0Z-1; G90; G0Z30; G0X0Y0;

Move to location 30mm above the Z0 axis.

Leave a Reply