[Paul_S]

If your control supports G54 thru G59 fixture offsets use them instead of G92.

If you have the local fixture offset feature G52, that will allow you move your coordinate system and back.

G92 defines where you are at in you coordinate system. And unless you are back to the same machine postion at the end of your program from when you started. Your coordinate system will drift.

G54 sets your program coordinate system relative to the machine zero.

The machine being one shot G53 command.

Now G52 is a local coordinate system shift. Which is canceled by a G52 X0 Y0 or Z0

G52 is very useful for a program pattern written in absolute mode verses having to use G91 mode.

I stopped using G92 when I started using G54 thru G59 fixture offsets.

When writing manual code, I sometimes use G52 to shift the coordinate system so I can use numbers right off the drawing. Especially for hole patterns from another hole from a datum. To make the program more readable. (If it doesn't make the code more understandable don't bother.)


One thing to remember the local offset G52 is universal in effect. Whether it is used before fixture offset call or after. The G52 local offset shifts relative to all coordinate systems. So don't forget to cancel with the G52 X0 Y0 Z0, between calls.

And depending on the control G52 Z0 before tool changes. And any fixture offset during tool change Z value may need to be zero too. (On a Mark Century 1050 control once dropped 6" radius cutter because the Z value fixture offset I was using had a non-zero Z value. {suprise suprise} From that point on I used fixture offset pairs. One for machining and the second for tool change. Only the X and Y values would be the same.)