[sanddrag]

Help me figure this out. My post processor is set to add a G28 Z0 near the end of the program to take the spindle up and out of the way. When the tool offset matches the tool number, this works as intended. However, when I use a different offset and tool number (setting 15 is set to allow this), the G28 Z0 command rapid plunges the tool down into the part. What do I need to do differently? Thanks.

[CThomas715]

Try adding a G91 on the same line as the G28. Just be sure to add a G90 before your next move after your tool change.

[ROBBY 68]

That is correct, And movement is because it references Z0 (work offset) prior going Z home.
Adding G91 you command incremental move.
Robby

[Matt@RFR]

G53 FTW!

[haastec]

G53 FTW!

+1

[dougtyler]

I changed my post to replace the G28 code with G53

Not sure why most posts use the G28

[angelw]

I changed my post to replace the G28 code with G53

Not sure why most posts use the G28

The main reason why G28 is used mostly, is if there is a value registered in the G53 Z offset registry, to globally set the coordinate system for all Work Shift offsets, then executing G53 Z0 will not result in the Z slide ending up at the Z Reference Return position; G91 G28 Z0 will, irrespective of what might be set in G53.

As your stated use of G28 is related to the Z axis only, there is no great advantage in using G53 over G28 to return the slide to the Z Machine Zero. G53 is more useful when the slides have to be moved to a specific X Y position, for a tool change for example.

G28 is a two shot code, returning to the specified axes Reference Return point via an intermediate point. In single block, the cycle start button has to be pressed twice to complete the execution of G28. Because of the return through an intermediate point, its important, as CThomas715 states in his Post, that G91 is specified if Z0 is the intermediate point specified in the G28 block. In G90 Mode, and G28 Z0 specified, the Z slide will return to the Z Reference Return via the Z absolute zero. Depending on how you arrange the tool length offsets, ie, if the tool length offset is a plus value, this could result in the tool hitting the workpiece, as the tool length offset is cancelled when G28 is executed.

Did you try CThomas715 suggestion and program G91 with G28? Is so what was the result? What should have happened if testing G91 G28 Z0 in Single Block Mode, is:
1. On the first press of the cycle start button to execute the G28 block, there should have been no movement of the Z slide and the Feed Hold indicator illuminated.
2. On the second press of the cycle start button, the Z slide should have move straight to the Z Reference Return point.

Regards,

Bill

[Matt@RFR]

There is no G53 line in the Haas offset page. There's a G52, but that has nothing to do with any of this.

I personally like G53 because it's simple, and I like knowing that I am NEVER in G91, ever. It's also nice that sending the Z home and parking the table at the end of the program uses the same code.

[dougtyler]

The main reason I changed to the G53 is because on the MiniMill, with the umbrella tool changer, Z0 is not the highest point on the Z axis. It's Z+4.
Also, I wanted to position the X and Y axis to the middle of the door, to make loading and unloading the vise more accessible. Not much room in the MiniMill.

[MetalZilla]

I use this bit of code for the retract:
G91 G28 Z0

and this line of code to lower the tool:
G43 H01 Z1.0