Mori G05.1 post help

[Rstewart]

Hey guys, need a little help if possible.

 

Using X5 and Mpmaster post:

 

I'm getting tired if going through and modifing the code for the AICC to work without alarming on our Mori Dura with the Mapps IV controller. I've looked through the .pst file and kind-of see what needs to happen, but I'm gonna need sum help.

 

When it posts the G49-> G05.1 Q0 then a rapid Z move the control alarms Over travel or something. There is No need for the G49 on my control when using G05.1 at the end. The mapps cutting mode selection is G332 R1. - R4. Rough to finish.

 

A piece of example code I need would be

 

T1

M06

G00 G17 G90 G54 X0. Y0. M3 S10000

G49

G332 R2.

G05.1 Q1

G43 H01 Z1.

G01 Z0. F50.

Bla

Bla

Bla

G05.1 Q0

G00 Z1.

M05

M09

G91 G28 Z0.

G28 Y0.

M30

[fillingdave]

Just comment out the line that is generating the g49 and that should do it. g49 is a tool height offset cancel. your tool change macro should have the g49 in it. g5.1 q1 is needed before the g43 but cannot be deactivated midprogram with out using a g49 and then using a g43 again to set height. be careful not to turn aicc on and off mid program.(on is more of the issue (g5.1q1). you can turn off anytime (g5.1q0))

[Rstewart]

Funny thing is that I Can turn off G05.1 Q1 and then back On WithOut using tool length offset cancel or G43 and everything works great. I just manually have been turning it on right before cutting at the Z depth and Off just before any Z Rapid.

 

Also, any tips on how to change the cutting mode secection in the post? It's G332 R1. - R4.

 

I emailed my reseller for a copy of the post editing ref guide like two months ago with NO Luck...

 

Thanks in advance for any help.

[fillingdave]

its not very hard to edit posts. always save a copy in a safe place, make change, save, check posted code is what you want, and repeat. just start the debug mode and step through your code that way. pick a small program to begin with. (a single line with contour) you can assign the special gcode "g332 whatever r value" in with the aicc(g5.1 q1) and everything will post when you turn that button on or not if off. post edit ref guide is installed with mastercam. do a search for "post" its a pdf of debug guide that should point you in right direction. also be careful activating and deactivating g5.1q1 mid program thats what our tech support says and fanuc says, fyi its not recommended could mess things up ie.. rotations, pallet moves, work shifts, etc...

[Jasond0530]

As dave said, comment out the G49!

 

i have this in my post which is activated by the misc inters and seems to work well for my Mori NH5000.

 

if mi8$ = 1, "G332 R1.(SPEED PRIORITY)", e$

if mi8$ = 2, "G332 R2.(INTERMEDIATE MODE)", e$

if mi8$ = 3, "G332 R3.(ACCURACY-DEFAULT)", e$

if mi8$ = 4, "G332 R4.(ACCURACY TOP PRIORITY)", e$

 

if (mi6$ = 1),

[

pbld, n$, "G8 P1", e$

hssw = 1

]

if (mi6$ = 2),

[

pbld, n$, "G5.1 Q1", e$

hssw = 2

]

 

bla

bla

bla

bla

 

if (hssw = 1),

[

pbld, n$, "G8 P0 ", scoolant, e$

hssw = 0

]

if (hssw = 2),

[

pbld, n$, "G5.1 Q0 ", scoolant, e$

hssw = 0

]

hope this helps!

 

Jason.

[Rstewart]

Haven't looked at this thread in a bit, But Thanks a lot Jason!!!!

 

I will dig through the post to try and figure where to place those comments. Not really the best at these things, and if anyone would like to chime in and help it Would be Greatly Appreciated.

 

Again, Thanks!!

[Jasond0530]

Ok what you need to do is add this to end of general output settings;

 

hssw : 0

hsse : 0

 

and after the G43 line add these(I had to enter twice in my post)

 

 

if mi8$ = 1, "G332 R1.(SPEED PRIORITY)", e$

if mi8$ = 2, "G332 R2.(INTERMEDIATE MODE)", e$

if mi8$ = 3, "G332 R3.(ACCURACY-DEFAULT)", e$

if mi8$ = 4, "G332 R4.(ACCURACY TOP PRIORITY)", e$

 

if (mi6$ = 1),

[

pbld, n$, "G8 P1", e$

hssw = 1

]

if (mi6$ = 2),

[

pbld, n$, "G5.1 Q1", e$

hssw = 2

]

 

and the remainder i added at the end of the toolchange part before the M30.

also to change the info in the misc inters page you change either the misc inter strings in post

or goto your md/cd to change them.

if not message me and i will try my best to help!

 

HTH

 

Jason.

[SledGeek]

I dug this up because I seem to have a similar issue. But only with contour paths ! When I turn G5.1 Q1 on in Misc. Values by setting Real to 2.0 it posts out the G49 and G5.1 Q1 just before feeding to every z depth.....

 

When I hand edit, I simply put it in before G43 and at end of program the G5.1 Q0 with a G49 (which I assume i have to do because my toolchange macro doesn't have a G49 in it ?) if i don't, it alarms out when running the next program....

 

Is this just an error or a setting I am ignorant about ? Why does it post out with all those extra lines that causes the Z retract and error......haven't seen it anywhere but the contour ops.

 

Simple engraving prgrm.....

 

T8 M06 (3MM BALL)

(MAX - Z2.11)

(MIN - Z1.997)

G00 G17 G90 G54 X2.2946 Y-.859 S5000 M03

G49

G94

G05.1 Q1 R3

G43 H8 Z2.11

G01 Z1.997 F5.

X2.2147 F10.

G49

G05.1 Q1 R3

X2.1348

G00 Z2.097

Z2.11

X2.0848

G49

G05.1 Q1 R3

G01 Z1.997 F5.

Y-.609 F10.

X2.0151

G03 X1.94 Y-.6626 R.0919

Y-.8054 R.2227

X2.0151 Y-.859 R.0919

G01 X2.0848

G00 Z2.097

Z2.11

X2.2147

G49

G05.1 Q1 R3

G01 Z1.997 F5.

Y-.609 F10.

G00 Z2.097

Z2.11

X1.8689 Y-.6654

G49

G05.1 Q1 R3

G01 Z1.997 F5.

G02 X1.8639 Y-.8082 R.2227 F10.

X1.7284 Y-.8218 R.0743

G00 Z2.097

Z2.11

X1.6055 Y-.7429

G49

G05.1 Q1 R3

G01 Z1.997 F5.

X1.5894 F10.

G49

G05.1 Q1 R3

G03 Y-.859 R.058

X1.6323 Y-.8524 R.0813

X1.6055 Y-.7429 R.0581

G49

G05.1 Q1 R3

[Guest CNC Apps Guy 1]

Funny thing is that I Can turn off G05.1 Q1 and then back On WithOut using tool length offset cancel or G43 and everything works great.

That's because you don't have a FANUC control.

[Guest SAMCRO]

FANUC AI High-Speed Modes - Simplified

 

http://www.mtbtech.net/blog/2012/11/09/FANUC-AI-High-Speed-Modes-Simplified.aspx

[wfarrington]

Bump...I am having the same issue as sled geek. When I use misc integers to turn on G8 P1 it posts it out at every pass..

 

My post code...

#region Null tool change
ptlchg0$         #Call from NCI null tool change (tool number repeats)                       
      pcuttype
      toolchng0 = one
      pcom_moveb
      pcheckaxis
      c_mmlt$ #Multiple tool subprogram call
      if mi1$ > one & workofs$ <> prv_workofs$,
        [
         pbld, "G91 G28 Z0.", e$
         pbld, " ", e$
        ]
     
      comment$
      if mi4$ = 1, "G8P1", e$
      pcan
      result = newfs(15, feed)  #Reset the output format for 'feed'
      pbld, n$, sgplane, e$     
      pspindchng
      pbld, n$, pscool, e$
      if use_rot_lock & (cuttype <> zero | (index = zero & prv_cabs <> fmtrnd(cabs))), prot_unlock
      if mi1$ > one & workofs$ <> prv_workofs$,

 

Gives me this...

G0 Z2.
G8P1
X7.2428 Y1.3609
Z.1
G1 Z-.2 F200.
X7.1928 Y1.2743 F250.
G3 X7.2294 Y1.1377 I.0866 J-.05
G1 X8.1526 Y.6047
G3 X7.9977 Y1.6932 I-8.1526 J-.6047
X7.8792 Y1.7703 I-.0978 J-.0207
G1 X7.7814 Y1.7496
G8P1
X7.2428 Y1.3609
Z-.4 F200.
X7.1928 Y1.2743 F250.
G3 X7.2294 Y1.1377 I.0866 J-.05
G1 X8.1526 Y.6047
G3 X7.9977 Y1.6932 I-8.1526 J-.6047
X7.8792 Y1.7703 I-.0978 J-.0207
G1 X7.7814 Y1.7496
G8P1
X7.2428 Y1.3609
Z-.6 F200.
X7.1928 Y1.2743 F250.
G3 X7.2294 Y1.1377 I.0866 J-.05
G1 X8.1526 Y.6047
G3 X7.9977 Y1.6932 I-8.1526 J-.6047
X7.8792 Y1.7703 I-.0978 J-.0207
G1 X7.7814 Y1.7496
G8P1
X7.2428 Y1.3609
Z-.8 F200.
X7.1928 Y1.2743 F250.
G3 X7.2294 Y1.1377 I.0866 J-.05
G1 X8.1526 Y.6047
G3 X7.9977 Y1.6932 I-8.1526 J-.6047
X7.8792 Y1.7703 I-.0978 J-.0207
G1 X7.7814 Y1.7496

 

Thanks,

 

Joey