MPMASTER to output hpcc code

[Cannon]

I just downloaded MPMASTER post and have been trying to get it output the Fanuc hpcc code G05 P10000 in the program. I have tried many things but I can only get it to output the end string p05 Q1 but not the one that turns it on. So could some one explain where I need to make the changes to get this work. Thanks.

[Guest]

 

By placing a 3 in the MR1 box, as shown above

 

code:

---

N180 G00 G17 G90 G54 X1.1569 Y1.25 S1069 M03

N190 G43 H239 Z.25

N200 G94

N210 G05 P10000

N220 Z.1

N230 G01 Z0. F15.

N240 Y.75 F25.

N250 G03 X1.6569 Y.25 I.5 J0.

N260 G01 X3.3139

N270 G02 X3.5639 Y0. I0. J-.25

N280 G01 Y-3.4902

N290 G02 X3.3139 Y-3.7402 I-.25 J0.

N300 G01 X0.

N310 G02 X-.25 Y-3.4902 I0. J.25

N320 G01 Y0.

N330 G02 X0. Y.25 I.25 J0.

N340 G01 X1.6569

N350 G03 X2.1569 Y.75 I0. J.5

N360 G01 Y1.25

N370 Z.1

N380 G00 Z.25

N390 G05 P0

N400 M05

N410 G91 G28 Z0.

N420 G28 X0. Y0.

N430 G90

N440 M30

---

[Cannon]

Thanks! Easier than I thought. I went straight to edit the post file and obviosly messed something up. haha

[kkominiarek]

JP, i would like to turn on G5 P10000 also. My MV page doesn't look anything like yours????

 

I'm using a surface finish contour toolpath.

 

What MV page should I BE LOOKING AT?

[Guest CNC Apps Guy 1]

I set my post up to automatically output it EXCEPT when opcode=3 (Drilling type cycles) and this is how I did it;

 

code:

---

phsm1_on         #High speed functions before G43 

# if opcode$ = 3 | opcode$ = 16, #ORIGINAL

# [ #ORIGINAL

# mr1$ = 0 #ORIGINAL

# mr2$ = 0 #ORIGINAL

# ] #ORIGINAL

if opcode$ <> 3,

[

mr1$ = 3 #FORCING HPCC MODE

mr2$ = 0

]

---

HTH

[Guest]

Ken are running the latest version of the MPMaster?

 

If it is an older version it may not be built in.

 

also if you renamed the post and machine and control defs, you may have to make sure your machine def is referencing the correct control def or your listing may not be correct.

[Tony35]

cnc apps guy

can i ask why you run HPCC on all the time i was thinking about doing this too. pros/cons of doing it

[Guest CNC Apps Guy 1]

No cons, only Pros.

 

The machine processes data faster with it on. Even if I don't "need" it I still run it regardlelss if I'm running at 200 IPM or 1900 IPM.

 

JM2C

[Tony35]

thanks cnc apps guy

[spade117]

I was playing around with this today.

 

Everything straight from the latest mpmaster versions...for some reason, it is posting the code ahead of the G43 line...what do I need to change to get it to post in the correct place?

[Guest CNC Apps Guy 1]

AI-NANO goes ahead, HPCC goes after.

[spade117]

What about G8?

[Guest CNC Apps Guy 1]

I don't believe G8 matters.

[spade117]

Ok, I guess I can test it at a machine. I always thought it had to be after the G43 line.

 

Thx.