sub routines

[CAM]

get right to it

i have a plate,want to profile 28 parts out of this in depth cuts.toolpath's/next menu/transform etc..it is posting sub's but the prog. is a guzillion lines long.i can edit the program and get it to be 100 lines or less.but there has to be a way mastercam/post will do this work for me.any suggestions?

fanuc controller

sub box checked

using latest mpfan post

thanks

[robk]

Can you use extended work offsets?

[J. Rod Rood Warmoth Guitar]

It is better to use the Fanuc Macro B language to array your part rather than have a guzillion lines of part code that you get with the transform function. Just post the single part out and then use a main program to call out the part for different G52 XY coordinates. Using the macro language, you can increment G52 in a while loop, and very easily have maintainable and understandable code.

[Hardmill]

quote:

---

i can edit the program and get it to be 100 lines or less

---

What are you editing out of the prog??

 

 

PEACE

[robk]

+1 Hardmill...

Going from guzillion to under 100 is pretty drastic.

 

 

You could also write just 1 program. Run it as a sub for the program I have in the example. Example below if for a horizontal machine with 2 four sided tombstones. Same idea though.

 

quote:

---

%

O1000(MAIN-PROG.SUB.100 )

G0G17G40G80G90

G0G91G28Z0.

G0G91G28X0.Y0.

G90G53X0.Y0.Z0.

B0.

G91G30Z0.

G30X0.Y0.

M1

N1G0G90G54

B0.

M98P100

M1

N2G0G90G55

B0.

M98P100

M1

N3G0G90G56

B0.

M98P100

M1

N4G0G90G57

B0.

M98P100

M1

G0G90G53B0.

G0G91G30XYZ0.

M0

M60

N5G0G90G58

B0.

M98P100

M1

N6G0G90G59

B0.

M98P100

M1

N7G0G90G54.1P1

B0.

M98P100

M1

N8G0G90G54.1P2

B0.

M98P100

M1

G0G90G53B0.

G0G91G30XYZ0.

M60

M30

%

---

[Guest]

Make sure that when you pick the sub box you also pick incremental for the subs.

[CAM]

yes, i can use extended work ofsetts(28 parts?)and what i am edeting out is all the subs.each part is identical,but it post's out a sub for each individual part 27 subs.and i am going .250 total z depth on each part with depth cuts of.03 each cut on profile,so in the main prog. it has all of the z depths then calls sub thats about 233 z depths just in the main program!i guess i will create some kind of macro for this.any more suggestions is welcome,and thanks for your input

[Mike Whitten CAD/CAM Contractors]

Try the mpmaster mpsubrep post

 

Mike

[robk]

quote:

---

yes, i can use extended work ofsetts(28 parts?)

---

Sure, standard option for a fanuc 16i is 48 sets and optional is 400. If you have them, why not use them? Also using mpmaster .pst here.

[Mike Whitten CAD/CAM Contractors]

Here is a link

 

http://www.emastercam.com/posts/mpsubrep/mpsubrep.html

 

I changed mine so that it just calls the subs with work offset like this:

 

/G55M98P101

/G56M98P102

ETC.

 

also make sure the subs have a G90 position in front of them

 

Mike

[Mike Whitten CAD/CAM Contractors]

Oops

actually like this:

 

/G55M98P101

/G56M98P101

ETC.

[CAM]

down loading a couple of things you mentioned did it thanks every one been a big help