MPmaster bug (Fanuc AICC)

[Cannon]

I made the changes that Matt Berube posted earlier, works perfect now

[Guest CNC Apps Guy 1]

Of course it shsould be brought to their atttention. I'm just saying that when people wine about a free post, that's not cool IMHO.

[Guest CNC Apps Guy 1]

quote:

---

...but if there is code in the post that does not work on "ANY" machine without causing an issue...

---

FYI!!!

 

Did some Testing today on a Matsuura MAM72-63V and G49 DID NOT crash the machine when I commanded it while a height offset and Work Offset were active.

[Cannon]

quote:

---

FYI!!!

 

Did some Testing today on a Matsuura MAM72-63V and G49 DID NOT crash the machine when I commanded it while a height offset and Work Offset were active.

---

That would depend how the tools are set. if you have a reference tool that is much shorter than the tool you are cutting and you have a line G49, the tool would go down the height difference of those two tools and possibly crash.

[Guest CNC Apps Guy 1]

Tools are set THE BEST WAY; Gage Length.

 

My main point was that Z Axis DID NOT move when G49 was commanded thus no crash.

[neurosis]

quote:

---

Did some Testing today on a Matsuura MAM72-63V and G49 DID NOT crash the machine when I commanded it while a height offset and Work Offset were active.

---

I guess that my concern is only when dealing with the multiple depth contour.

 

I noticed this but as I am not 100% clear of the rules, I shouldnt even be asking until I am clear.

 

But have you posted out this scenario and looked at the code?

 

I havent tried to run this in a machine so this may just be a learning experience for me.

 

 

code:

---

 N170 G49

N180 G94

N190 G05.1 Q1

N200 G43 H1 Z3.

N210 Z.1

N220 G01 Z-.25 F6.42

N230 G41 D1 Y3.0323

N240 G03 X-.0048 Y2.9823 R.05

N250 G01 X1.0183

N260 G02 X1.2683 Y2.7323 R.25

N270 G01 Y.9699

N280 G02 X1.0183 Y.7199 R.25

N290 G01 X-1.0279

N300 G02 X-1.2779 Y.9699 R.25

N310 G01 Y2.7323

N320 G02 X-1.0279 Y2.9823 R.25

N330 G01 X-.0048

N340 G03 X.0452 Y3.0323 R.05

N350 G01 G40 Y3.0823

N360 Z-.15

N370 G00 Z3.

N380 X-.0548

N390 Z-.15

N400 G49

N410 G05.1 Q1

N420 G01 Z-.5

N430 G41 D1 Y3.0323

N440 G03 X-.0048 Y2.9823 R.05

N450 G01 X1.0183

N460 G02 X1.2683 Y2.7323 R.25

N470 G01 Y.9699

N480 G02 X1.0183 Y.7199 R.25

N490 G01 X-1.0279

N500 G02 X-1.2779 Y.9699 R.25

N510 G01 Y2.7323

N520 G02 X-1.0279 Y2.9823 R.25

N530 G01 X-.0048

N540 G03 X.0452 Y3.0323 R.05

N550 G01 G40 Y3.0823

N560 Z-.4

N570 G00 Z3.

N580 X-.0548

N590 Z-.4

N600 G49

N610 G05.1 Q1

---

This is how the code comes out of that post. The G49 is issued canceling the height offset. It never picks a height offset back up. That is possible?

[cnc22]

Look at my post on 5-15-2009 above. If you change parameter 5006.6 to 0 this sets tool length compensation to happen on the next axis movement. Prior to changing this parameter as soon as it read G49 it wanted to move Z by the tool length. I do not know if this works on all fanuc controls but my post is set that when it cancels the height offset as in the code above, it calls the H offset right after canceling or changing the G5.1 settings. By doing this there is no axis movement and no crash. Prior to changing parameter 5006.6 we crashed our share of toolholders/parts. Hope this helps

[Greg Williams]

quote:

---

Of course it should be brought to their atttention. I'm just saying that when people wine about a free post, that's not cool IMHO.

---

Yeah I have to agree.

[Guest CNC Apps Guy 1]

quote:

---

...But have you posted out this scenario and looked at the code?

---

When In-House issues a new MPMaster, I always do a few things to it and changing how High Speed Code is output is one of them. I have a bunch of cut and past post blocks, variables, and logic that I add so I guess I take the statement

quote:

---

...Posts are generic and are intended for modification to the machine tool requirements, operator preference, and established internal standards...

---

VERY seriously and act accordingly.

 

JM2C

[SledGeek]

You have to have this at the beginning of every toolpath AFAIK. You can't just turn it on at the beginning of the program and off at the end. G8 P1 will allow that but it not as powerful nor as fast on the processing as G5.1Q1.

 

 

I turn mine on at the beginning of multiple toolpath/toolchange programs and turn it off at the end. It goes on after M03 and before G43 and turns off at the end or before drill/tap cycles before G91G28 Z0. Not on and off for every toolpath within the program. I don't use G49 because the next tool callout cancels the previous offset.No G49, no reason to turn back on. Make sense ? Just my thinking, mebbe it's wrong ?? I'm not a post or fanuc expert on this so i don't 100% know the rules either.

Is there a difference between how the AICC and AIAPC need to be posted ? I'm AIAPC.

 

I'm curious because what i'm hearing hear, and what's actually happening on our equipment sounds like opposing scenarios. What else (besides machine parameters) can affect this, specifically? I've done alot of reading on this and it seems the common denom is a parameter , or choices by programmers on what they r comfy with.

[Guest CNC Apps Guy 1]

Is there a difference between how the AICC and AIAPC need to be posted ?

From the machines I've run, no.