MPmaster bug (Fanuc AICC)

[Cannon]

There is something wrong in the high speed machining part of the post. One of our machine has the Fanuc AICC (G05.1) option so I turned it on From the machine definition. Now if I machine a 2d- contour and use cut depths and check the keep tool down between cuts, the posted nc- program shows that after every depth of cut, when it is time to move to the next depth, the post turns off height compensation (G49) and after that turns the AICC back on (G05.1 Q1). I know that if I change the post to use use the other Fanuc high speed option, HPCC (G05 P10000), the code post right without the Height compensation cancelled.

[J Coulston]

Just bumped a holder, scrapped a part and collet because of this in a re-machine operation.

 

if mr1$ = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1

[

#pbld, n$, *sg49, e$ <------ commented out this line #Must be in G49 and remain before G43

if ipr_type > 1, ipr_type = 0 #Must be in G94

pbld, n$, sgfeed, e$

pbld, n$, "G05.1", "Q1", [if mr2$, "R", no_spc$, *mr2$], e$ #Mr2 gives accel/decel value/coefficient, usually R or P

 

 

Seems ok whit the G49 commented out so far but only ran a few programs thru it.

[Guest SAIPEM]

Fanuc AICC and AIAPC both REQUIRE that this mode be set and canceled individually for each tool.

 

You MUST cancel an active height offset with G49 BEFORE activating AICC or AIAPC.

 

You must also activate it BEFORE calling a tool height offset with G43.

 

If it is canceled mid-program, before the end tool's work is done,

you'll need to cancel an active height offset and reactivate AICC or AIAPC.

Once it's canceled, you need to follow the rules to restart it.

[Cannon]

Okay thanks. I dont have much post editing experience so I didnt want to start mess with it myself. I got away without any crash, just the machine alarming in G05.1 Q1 line.

[Guest CNC Apps Guy 1]

If it alarms it means it was not canceled properly.

 

G5.1Q0

G49

 

MUST be executed BEFORE you can call it again.

[robh]

James, Can it be in the first line of the next tool and get the same result? ie.G17G0G80G40G90G49

or should it be immediatly after G5.1Q0? TAI

[Guest CNC Apps Guy 1]

I don't believe it matters so long as it(G49) is executed before the next HPCC/AI-NANO call just because it's not big deal to have an extra G49 hanging around. I really don't look too closely to code unless I'm doing post work anymore. My posts are pretty dialed. I usually have some technically redundant stuff in there

 

code:

---

.

.

.

G0Z7.1682M9

G5P0(HPCC OFF)

G91G28Z0.

G4X3.

/G65P9863Z5.(TL. BRK. DET.)

G0G91G28Z0.M5

G49

G90

M1

 

N49(PARTS 4, 5, AND 6 ROUGH THE BACK SIDE - TOP)

G91G0G28Z0.

G17G80G49

G90

T96(1/2 FLAT HSM-L ENDMILL)

M6

M8

.

.

.

---

[robh]

quote:

---

Fanuc AICC and AIAPC both REQUIRE that this mode be set and canceled individually for each tool.

 

You MUST cancel an active height offset with G49 BEFORE activating AICC or AIAPC.

 

You must also activate it BEFORE calling a tool height offset with G43.

 

If it is canceled mid-program, before the end tool's work is done,

you'll need to cancel an active height offset and reactivate AICC or AIAPC.

Once it's canceled, you need to follow the rules to restart it.

---

I think G48 is the cancel command for G49, G49 is required to activate AICC etc. Might be wrong on that.

[Guest CNC Apps Guy 1]

G49 is "Tool Length Compensation Cancel".

 

FYI

G48 is "Tool Offset Double Decrease" according to the FANUC manuals I have access to. (0/15/16/18/21/30/31/32)

[Guest SAIPEM]

quote:

---

I think G48 is the cancel command for G49, G49 is required to activate AICC etc. Might be wrong on that.

---

You are.

 

G49 is required as it cancels tool length compensation.

 

AICC and AI APC can NOT be activated while a tool length offset is active.

[Cannon]

quote:

---

AICC and AI APC can NOT be activated while a tool length offset is active.

---

In HPCC, This is controlled by parameter. HPCC can be put on before or after the tool length activation depending how the parameter is set.

[Guest CNC Apps Guy 1]

There's like 10 parameters that handle how HPCC functions when certain codes are executed.

 

#5000.0 - Handling Cutter Comp C

#5003.3 & #5003.4 - Handling Cutter Comp C INterference Checks

 

#7054.0 - HOw commands not usable in HPCC mode are handled

 

#8403.1 - Handling rapids or aux. functions while in HPCC mode.

#8403.2 - Handling stroke check

#8403.3 - Handling Stroke Check

#8403.7 - Hnadling Rapids in HPCC mode

 

#8481 - Rapid Feedrate in HPCC mode

 

#8485.0 to #8485.5 - modes allowed while in HPCC Mode.

 

HTH

[robh]

Thanks for the heads up. I'd always heard the same about AICC needed G49 prior to G5.1Q1 but nothing about canceling it(G5.1Q0) with the same command. I also found reference in the Machinist Handbook about G48 cancelling G49. Fanuc trumps that outdated version it seems.

[Guest SAIPEM]

You don not need to use G49 when you cancel Fanuc AI.

 

You need to cancel any active tool length offset before you activate AI.

 

You can cancel AI at any time with G5.1 Q0

 

G48 is not a cancel for G49.

 

G49 is tool length offset cancel.

[cnc22]

Hi,

This is my first post so bear with me.I just went through this with my Fanuc 21i. If you change parameter 5006.6 to 0 this sets tool length compensation to happen on the next axis movment. By changing this parameter you can change the precision of your high speed look ahead using the same tool for chamfering holes (drill cycle) then edges with a chamfering tool (contour)(Ex. Q2 to Q5) (my machine uses G5.1 Q1 to turn on and G5.1 Q0 to turn off look ahead with M300 Q1 thru Q5 to set precision) . Or when you may want to rough & finish surfaces with the same ball mill. This way when you cancel tool length compensation G49 then change the M300Q1 thru M300Q5 value of G5.1 (or turn it on as with the chamfer tool) before the next move call up G43 again (none of these are axis moves). Hope this helps. If it does not make sense maybe one of the post or control gurus can chime in.

[Newbeeee™]

If it helps, here's our code for a fanuc oi:-

 

N0101T1M6

M1

{ 40MM DIA CUTWELL FACEMILL }

 

G05.1Q1<<<<<<<<<<<<<<<<<<< Activates lookahead

G54G0G40G80G90X-75.Y97.S9000M3

T2

G43Z100.H1

Z25.

Z11.65F5000.

CODE

CODE

Z-5.

M98P2932

G0Z25.M9

G28Z100.M19

G05.1Q0<<<<<<<<<<<<<<< Cancels lookahead

G49<<<<<<<<<<<<<<<<<<< Cancels tool length offset

 

 

You MUST have a G49 after the cancel {GO5.1Q0}.

You could put the G05.1Q0 followed by the G49 into your toolchange macro, so it cancels automatically everytime.

Don't run it for drill or tap cycles.

We run our machines in G05.1 all of the time with no detriment at all {+ faster cycle times}.

However, we did have to tune the parameters 1st.

 

Cheers

[Guest CNC Apps Guy 1]

The heart of it is this;

 

quote:

---

You don not need to use G49 when you cancel Fanuc AI.

 

You need to cancel any active tool length offset before you activate AI.

---

But just for the sake of ease, I ALWAYS issue a G49 after I turn off AI-NANO/HPCC, etc... That way there are no issues when I wish to turn it on again.

 

 

JMHO

[Cannon]

I see the same bug is still on the X4 version of mpmaster post. I tryed to fix it how J Coulston 1 adviced

quote:

---

Just bumped a holder, scrapped a part and collet because of this in a re-machine operation.

 

if mr1$ = 2, #AI-NANO 2, AI(nano)CC output (Artificial Intelligence Contour Control) - G05.1 Q1

[

#pbld, n$, *sg49, e$ <------ commented out this line #Must be in G49 and remain before G43

if ipr_type > 1, ipr_type = 0 #Must be in G94

pbld, n$, sgfeed, e$

pbld, n$, "G05.1", "Q1", [if mr2$, "R", no_spc$, *mr2$], e$ #Mr2 gives accel/decel value/coefficient, usually R or P

 

 

Seems ok whit the G49 commented out so far but only ran a few programs thru it.

---

After this fix I dont have the G49 posted before every depth of cut but I still have G05.1 Q1 line. I havent tried if it works in a machine but would like the G05.1 Q1 line to only post in the program beginning. How could I fix this myself?

[Guest CNC Apps Guy 1]

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.

[Matt Berube at Ferron Mold]

I changed from this

 

 

code:

---

   if mr1$ = 2, 

---

to this

 

 

code:

---

   if mr1$ = 2 & mr1_flg <> 2, 

---

In the phsm1_on section.

 

I have a hard time understanding posts but I had the same trouble with MPMaster and this fix works wonderfully.

 

My MP Master has been running G05.1 without any errors for a long time. Let me know if you need to see any more of the post. I am 99%sure I didn't comment out any lines in the post as was discussed further up in this thread.

 

Hope this helps !

 

P.S. You can not turn this on only at the beginning of the program because the AICC can't be active during toolchange.

[Cannon]

quote:

---

P.S. You can not turn this on only at the beginning of the program because the AICC can't be active during toolchange.

---

Yes I knew this, I meant to say once in operation because what the mpmaster does is post G05.1 Q1 line after EVERY depth of cut, at least in a 2d-profile toolpath that I tried it. Im going to try what Matt Berube suggested and see if it solves this. Thanks!

[neurosis]

So with the G49 being posted on each Z depth of a multi depth 2D contour, does "any" machine handle this without a crash? Does InHouse know that this is an issue?

[Guest CNC Apps Guy 1]

From the Post Download Page... emphasis mine.

 

quote:

---

Master In-House Solutions Posts

Generic master posts based on CNC control model. Download the self-extracting executable and install to your Posts directory.

 

Posts are provided 'as is' with no warranties, either expressed or implied

, that code generated through use of the posts is safe or suitable for your machine tool. Please employ your own established code verification procedures prior to running code on your machine tool. Posts are generic and are intended for modification to the machine tool requirements, operator preference, and established internal standards. In short,

use at your own risk

.

---

[Matt Berube at Ferron Mold]

@CNC Apps Guy >

 

@ anybody else, send them a message about it. I don't believe I ever mentioned it to In-House.

[neurosis]

CNC Apps Guy,

 

I understand that, but if there is code in the post that does not work on "ANY" machine without causing an issue, you would think that it would be worth looking in to or at least bringing to their attention.

 

Yes? No?