[inflateable]

I need to do some patterned stuff, and I've forgotten how a g52 works.

Well, not forgotten how it works, but how it behaves.

If I'm at machine coords X0Y0Z0 and I then run the line
G52 X10, Y10, Z10 to shift the coord system - does the tool move to the new zero position on reading the G52 line?

[magneto259]

Yes from my understanding it should. I just went though this with using G57.

[Geof]

...If I'm at machine coords X0Y0Z0 and I then run the line
G52 X10, Y10, Z10 to shift the coord system - does the tool move to the new zero position on reading the G52 line?

No. Well I will qualify that, on a Haas running in Fanuc mode the answer is no and I think G52 is a no motion command.

G52 simply puts the X, Y, Z coordinates in a G52 register. These coordinates are always added into the controller calculations for any active Work Coordinate system.

For example if your G54 has coordinates X-10. Y-10. Z0. and you have the command G52 X5. Y5. Z0. any motion command after the G52 uses the combination to figure out where to go to. G00 X0. Y0. will move to a location that is X5. from X-10. and Y5. from Y-10. that is the current G52 work zero.

To go back to just using the G54 location you use G52 X0. Y0.

EDIT: I checked and in the Haas manual it say "G52 is a non-modal, no motion code" but whether this is just Haas or whether this is the standard for G52 I do not know.

[Al_The_Man]

I don't program on a regular basis, but I seem to remember from my Fanuc course days, that G52 is termed a Local or Child Coordinate system within a work coordinate system, and as geof said the G52 basically shifts the existing work coordinate e.g. G54, by the amount in the G52 command.
Any subsequent move are from this new local system.
Al.

[inflateable]

Nice, thanks chaps.

[joecnc1234]

For yasnac g52 resets to machine coordinate system, I don't know if your'e talking about g92 or some fucntion I've never used before, and I've programmed and ran haas machines for quite a few years. I just don't ever remember using g52. for g92 you shift with g91 and set g92 x0 y0 and move in g90. Just a thought and my confusion.
Joe

I believe if you added a value with G52 it would probably work for a work shift. I have never tried it, sounds interesting though.

[inflateable]

G52 can used in a similar way to G92, but it's MUCH easier to use - you can use it regardless of the current position of the tool -it's like a temporary work offset, valid only for the program you're running.

Personally I think G92 commands are obsolete (and dangerous) and use work offsets G54-g59 and tool length offsets instead.

[joecnc1234]

Thanks inflateable like I said I've never used g52 except to reset to machine zero I will try it today and see what happens. I personally don't like g92 also it creates to much confusion so I'm looking forward to trying G52. Again thanks. Thats why I like this forum I learn every time on on it.
Joe

[gar]

070503-0626 EST USA

inflateable:

On a HAAS machine in HAAS mode the G52 values remain unchanged unless you change them. This includes program start and machine power down and up. But on the HAAS lathe there is no HAAS mode. The HAAS mode is extremely useful and we always operate in this mode. However, there are many people that are afraid of using this mode.

I do not use G92, but on a HAAS machine I believe G92 is almost identical to G52 HAAS mode. There may be fewer ways to set it, and its content is displayed in a less obvious location. This needs further study.

On HAAS in Fanuc mode there are many conditions that reset G52 to 0.

.

[omarelec77]

Can anybody familiar with Fanuc controls explain something to me? When I command say G52 x10, how the position display update? For example if absolute position displays x= 50 before the command, what will be shown after?

[metalmayhem]

if g54x0 is 50" from absolute zero position (home) then g52 x10 followed by g0 x0 should show 60 on the display after the x10 move