what is the G52 function

[glovebox20]

Hello.

I'm retivaly new to the HAAS controls (VF-2) and was wondering what the G52 offset is used for. Is it another work offset or is it a shift offset like a Fanuc (work offset #00). I just like the Fanuc controls (OM,16M) how they have the shift offset and would like to know if HAAS has something like this.

thanks

glovebox20

[orizaba]

G 52 resets the the part zero, I think. If wrong somebody let me know.

[orizaba]

I found this, hope it helps
http://www.mmsonline.com/articles/0100cnc.html

[gar]

080422-1442 EST USA

glovebox20:

In HAAS or Fanuc mode this is a very useful function.

There are memory registers for each axis for G52, G54 .....

The contents of G52 are added to the current active G5x to define the work zero coordinates. In HAAS mode the contents of G52 remain unchanged until explicitly changed, even thru power down and up. There are a number of conditions in Fanuc mode where automatic reset of G52 occurs.

.

[Andre' B]

I know it as the local work offset and use it to temporarily reset the work zero.
Very useful when used in subs as it can almost completely eliminate the need for incremental programming.

Edit: Add example sub.

O1004(EM-DO-STUFF-PROGRAM )
#1=#5001(SAVE X POSITION)
#2=#5002(SAVE Y POSITION)
#3=#5003(SAVE Z POSITION)
G52X#1Y#2(SET LOCAL COORDINATE)

(DO STUFF)

G0X0.000Y0.000
G52X0Y0
M99

[orizaba]

Is there a "conversational" equivlent. I would like to find a way to put a second vice on the the mill. I'm using Bobcad V22

[Geof]

Originally Posted by orizaba G 52 resets the the part zero, I think. If wrong somebody let me know.

It does not reset it but adds to it.

For example you could have the G54 work zero set at X-8. Y-6. Z0.

Program:

G54 G00 X0. Y0. Z0.

And the machine moves to -8. on the X axis, -6. on the Y axis and stays at Z zero.

Now program:

G54 G52 X2. Y4. Z-8.
G00 X0. Y0. Z0.

And the machine will move to -6. on X, -2. on Y and -8. on Z.

As GAR says the machine adds the G52 values to any other work coordinate values.

You use G52 X0. Y0. Z0. to set the G52 values back to zero.

Very usefule for subroutines and fixtures holding multiple parts. A reference point on the fixture is located at G54 and all the parts have G52 coordinates calibrated from there.

Not really needed if all you have is two vises; just make one vise G54 and the other vise G55.

[gar]

080423-1014 EST USA

When I use the term G52 is added to G5x it does not mean that G5x is modified.

What it means is that internally there is some set of computer registers that represent where the current tool position is supposed to be and there are various components that are added into these registers to define that location. These components always include G52 and the current G5x as well as other components.

So even if you never put a non-zero value in G52 the content of G52 is combined with G5x.

.

[glovebox20]

Thanks for the help guys. That clears thing up for me.

glovebox20

[orizaba]

Originally Posted by Geof It does not reset it but adds to it. For example you could have the G54 work zero set at X-8. Y-6. Z0. Program: G54 G00 X0. Y0. Z0. And the machine moves to -8. on the X axis, -6. on the Y axis and stays at Z zero. Now program: G54 G52 X2. Y4. Z-8. G00 X0. Y0. Z0. And the machine will move to -6. on X, -2. on Y and -8. on Z. As GAR says the machine adds the G52 values to any other work coordinate values. You use G52 X0. Y0. Z0. to set the G52 values back to zero. Very usefule for subroutines and fixtures holding multiple parts. A reference point on the fixture is located at G54 and all the parts have G52 coordinates calibrated from there. Not really needed if all you have is two vises; just make one vise G54 and the other vise G55.

Does conversational code have this ability?

[pdoherty]

Andre' B wrote:

"I know it as the local work offset and use it to temporarily reset the work zero."

Nice! Thanks for sharing this. Very powerful.

[CNCRim]

Originally Posted by orizaba Does conversational code have this ability?

From what I know "no". It need all the infomation then spit out the long XY coord.....