Hass VF-1 work coordinate problems

[gar]

051028-1244 EST USA

Hu:

The G52 contents are stored at the previously said #5201 ... locations. These can be loaded via #5201 = something, or G52 something, or on the OFFSET page by entering something. The values on the OFFSET page are derived from said #5201 ... locations. When you write a value into G52 on the offset page it is entered into #520x, and then displayed on the OFFSET page, or at least the equivalent of this. All of this you can experimentally determine.

Machine position excluding cutter comp is determined from #5201 + #5221 + #2001 + #2201 + X command, #5202 + #5222 + #2002 + #2202 + Y command, #5203 + #5223 + #2003 + #2203 + Z command, etc. These generate the desired absolute machine position. You can also check the values at #5201 .... via the following technique:
#101 = #5201
#102 = #5202
#103 = #5203
then go view #101 ....

If I do G52 X2.0 Y1.3 Z-2.7 in a program in HAAS mode, single step thru this instruction, then switch to the OFFSETS page I will see these programmed values at G52. If I follow this with G52 X0 Y0 Z0, and after executing this instruction and I check G52 OFFSETS, then G52 XYZ will all be zero.

I did not test this at this point in time, but I have previously done the equivalent.

.

[HuFlungDung]

Oh, ok, I think I get it now
I was thinking that I would have to enter values directly into the offset page at G52, but of course, that would not be handy in real life, and I suppose it is actually impossible to enter any values into G52 "manually". Now I get it!!

[Geof]

Hu:

I just checked and it is possible to enter values into the G52 page and because the Haas mode does not zero them at RESET or M30 they stay there. This could prove interesting if you did something like this accidentally.

[gar]

051028-1351 EST USA

Hu:

You can enter values manually into G52 in the OFFSET page. But here is how it gets confusing.

If you are in HAAS mode the values you enter manually thru the OFFSET page, or thru the other means will stick. This is because G52 in HAAS mode is not cleared on RESET or other ways to get to your program.

However, in Fanuc mode G52 is cleared as specified in the HAAS manual under G52 Fanuc. Also cleared in going from the OFFSET page to the program via PROGRAMS, MEMORY.

.

[HuFlungDung]

And 1Stroke has been switching controller emulations all over the place trying to solve his problem. What might that do to any existing variables and offsets?

So back to Haas mode, if you can enter values in the G52 offsets by hand, then command additional G52 via the main program, do they add up? Do they cancel out completely with a single G52 X0Y0Z0? I don't want to screw up my machine to find out

[Geof]

Do they cancel out completely with a single G52 X0Y0Z0? I don't want to screw up my machine to find out

That, among other reasons, is why I bought a Simulator.

They cancel completely with G52X0Y0Z0; although the way it works I think it is more correct to say they are overwritten by what is in the G52 command.

[gar]

051028-1436 EST USA

Hu:

Geof is correct.

The G52 memory locations are simply locations where values can be placed.

The instruction
G52 Xa Yb Zc
moves the "X value a" to memory location #5201, b to #5202, and c to #5203.

If you do
#5201 = a
#5202 = b
#5203 = c
in your program you get exactly the same result, just harder to write and not as clear.

If you do
#5201 = #5201 + a --- you will get the X component of G52 increased by the value of a.

If you do
G52 Xa Yb
you will change the X and Y components but leave the Z component unchanged. What this is useful for is controlling your XY position independent of changes to Z which you might do manually. For example the height of your stock might vary and you want to be able to adjust for this.

.

[Geof]

Two comments:

1), I think it is really good how some of these threads turn into quite a serious learning experience; with apologies to 2strokes for the partial hijack.

2), Hu, GAR; do you guys ever do any work or are you sitting in front of your computer all day responding to CNCzone stuff.

[HuFlungDung]

Geof,
I've been online quite a bit lately (sort of between jobs at the moment), so the answer is yes I do work, but no, not for the last few days I am quoting a few jobs though, and turning a few of my old Bobcad drawings into nice solid models in OneCNCXR2. I'm having quite a hoot at it

I'm keen to learn whatever I can about Haas maintenance and problems, though, since I'm my own serviceman

[Geof]

I'm keen to learn whatever I can about Haas maintenance and problems, though, since I'm my own serviceman

I would guess it costs a few pennies to bring in a tech from Skinners who would be your Haas service provider I assume. I have it a bit lucky, they are about 2-1/2 minutes drive from me.

[choquer]

This may not be your problem but I thought it might be helpful anyways.

I would first recommend that you make sure you have the most current software available because I found out as a new owner of a TM1 that I needed the latest version of software to run the metric version on the machine. It got to the point where I was thinking I was an idiot only to finally call Haas and they explained they were having problems with the Metric sytem on the machine. I switched over to Imperial and voila the machine worked like it was supposed to. Since then my dealer upgraded the software and it seems like everything works fine now.

My point is that it could be a bug in their software.

Good Luck

[1strokedrs]

choquer,
I am starting to think my problem is in the software also,because no matter if the positioning is right or wrong the machine will repeat.If you call up a G54 X0.0 Y0.0 Z0.0 it does fine but if you call up G55-G59 X0.0 Y0.0 Z0.0 it will go to G55 X0.0 Y0.0 but it moves in Z to the Z0.0 G54 position.I do not think it is just a factory flaw though. The machine has been operating for years with no problems like this until recently.