Mulitple parts

[CNCMike]

I am trying to run two parts at a time and would like to know the best way of doing this. I need to keep the program as short as possible due to controller capacity. I would also like to run all ops with the first tool then all ops with the second tool.....

 

I did a search and came up with some info on Toolpaths/Transform toolpaths which I have been playing with, but it seems to double the program length (stores moves as subprograms and calls them later). Is there a way to use G54 and G55?

 

Thanks for the help,Mike

[Flycut]

This post did it for me.

[Randy Morton @ Clem Industrial]

Mike,

 

What I would be thinking here would be to set a WCS for each part, and toolpath each part the same (u likely could use transform for this). If you are running on limited memory space in the machine, you could do these up in Subprogams for each tool.

 

Dunno if this is what you are looking for, but have a look at the code below and see if this suits your needs;

 

Basically what it is, is 2 identical parts, one at G54, one at G55. I toolpathed the first box, told it to use DOC -> Subprogram and made the depth of cut to be more then I was going. Thus only outputting 1 sub run. Then I did the same for the second part, thus creating a base program, a WCS change in the base, and a sub callout for each.

 

This kinda what you are looking for?

 

 

code:

---

N120 M06 ( 1-3/16 FLAT ENDMILL)

(DAEWOO ACE-H80 - H47)

(T-1)

N130 G00 G54 G90 X-3.9688 Y-1.1875 S1286 M03

N140 G43 H313 Z2.

Z.1

N150 G01 Z-.25 F20.59

N160 M98 P0001 ( SUB FOR T )

N170 G90 Z-.15

G00 Z2.

N180 G90 G55 X-3.9688 Y-1.1875

N190 Z2.

Z.1

N200 G01 Z-.25

N210 M98 P0001 ( SUB FOR T )

N220 G90 Z-.15

G00 Z2.

N230 G91 G28 X0. Y0. Z0. M05

N240 G90

N250 M60

N260 M30

 

O0001 ( SUB FOR T )

N100 X-2.7813

N110 G03 X-1.5938 Y0. R1.1875

N120 G01 Y1.

N130 G02 X-1. Y1.5938 R.5938

N140 G01 X1.

N150 G02 X1.5938 Y1. R.5938

N160 G01 Y-1.

N170 G02 X1. Y-1.5938 R.5938

N180 G01 X-1.

N190 G02 X-1.5938 Y-1. R.5938

N200 G01 Y0.

N210 G03 X-2.7813 Y1.1875 R1.1875

N220 G01 X-3.9688

N230 M99

---

[CNCMike]

Thank you both for the suggestions. That is what I am looking for. I found I can do this by using Transform toolpaths, but it always does the first part as a whole then the second part as a whole. Any way to do all ops in order?

 

Thanks, Mike

[john316]

.

 

When you do your transform/toolpath check the "subprogram" box. There are several different settings you can experiment with to get the results you want.

 

.

[CNCMike]

I think I have what I am looking for. I had to check the "copy source ops" box and then check the "disable posting in selected source ops" box. This gives me two offsets with the subprograms listed at the bottom.

 

When I didn't check the "diasable posting in selected source ops" box I got the original program, the new offsets, then the subprograms which doubles the program size.

 

This looks to be the smallest file size possible. Now to load it in the control and see if it works.

 

Thanks, Mike

[JDowe]

In the group NCI Output box

Check "operation type"

[john316]

.

 

They usually work good right out of the box. I would save any programs in the control and clear the program memory so that when your done you can save all programs in memory to ensure that you save the subs without getting a lot of extra programs.

 

.

[CNCMike]

Hi Guys,

I loaded the main program along with the subs, but the main program does not perform the sub ops. After the first sub program call it over travels in the Z-Axis.

 

To load the subs I had to post each op seperatly then send to the controller. Is there a different way of doing this? Or a correct way? The program names are 0001, 0002 .... just like in the main program.

 

I did notice there was no "L" designation to call how many times the sub program should be performed. Is this normal or a post issue?

 

Mike

[john316]

.

 

I suppose we should have asked you what machine control you're using and what post processor. It'll help to determine how to set-up the subs.

 

.

[CNCMike]

Fanuc OMC controller, MILL 3-AXIS VMC.MMD post.

 

Here is a sample of the code output. I cut the third sub program short to save space.

 

N1 G20

N2 G0 G17 G40 G49 G80 G90

( SPOT DRILL. )

N3 T1 M6

N4 G0 G90 G54.1 P50 X4.0625 Y-.9375 S2500 M3

N5 G43 H1 Z1.

N6 M98 P0001

( SPOT DRILL. )

N7 G90 G54.1 P51 X21.0625 Y-.9375 Z1.

N8 M98 P0001

N9 M5

N10 G91 G28 Z0.

N11 M01

( DRILL THRU HOLES. )

N12 T2 M6

N13 G0 G90 G54.1 P50 X4.0625 Y-.9375 S1500 M3

N14 G43 H2 Z1.

N15 M98 P0002

( DRILL THRU HOLES. )

N16 G90 G54.1 P51 X21.0625 Y-.9375 Z1.

N17 M98 P0002

N18 M5

N19 G91 G28 Z0.

N20 M01

( C'BORE. )

N21 T3 M6

N22 G0 G90 G54.1 P50 X4.0479 Y-.9341 S1000 M3

N23 G43 H3 Z1.

N24 M98 P0003

( C'BORE. )

N25 G90 G54.1 P51 X21.0479 Y-.9341 Z1.

N26 M98 P0003

N27 M5

N28 G91 G28 Z0.

N29 G28 X0. Y0.

N30 M30

 

O0001

N7 G91

N8 G98 G81 Z-1.2 R-.9 F5.

N9 X3.875

N10 G80

N11 M99

 

O0002

N16 G91

N17 G98 G83 Z-3.0596 R-.9 Q.75 F5.

N18 X3.875

N19 G80

N20 M99

 

O0003

N25 G91

N26 Z-.9

N27 G1 Z-.4832 F5.

N28 G3 X.0292 Y-.0068 R.015 F4.

N29 X.0004 Y.0034 R.015

N30 X-.0296 Y.0034 R.015

N31 G1 Z.0999 F5.

N32 G0 Z.5333

[?Mark]

Mike, if the file is not large send it my way (not zipped) and I'll adjust the settings for you.

Mark

[HEED]

you can always copy the operations then re label them g54 and g55 then change the work offset to 1 on g55 side. It looks like your using a controller that supports g54.1 and it will depend on your post to oputput g54.1 rather than g55...there are also TONS of ways to sub program this thing out, it all just depends on how you want to do it I would stay away from transform I personally dont like the way that it works when you post it, i.e. does the whole first part like you mentioned it.

[CNCMike]

Mark,

How can I go about getting you the file? Thanks for the offer.

 

Mike

[?Mark]

Your above sample looks good, except change subprogram to absolute instead of incremental.

hth

If you still have problems send it to me at:

jmqminc at aol dot com

 

Mark

[?Mark]

Back at you.

Let me know how it worked out for you.

[Tim Simmermon]

Flycut,

 

That post you linked to is exactly what I needed for a new machine we got in. I like to run my suprograms internally within the main program (M97 Call w/ N numbers). This post uses M98 and gives the subprogram a program number (O....). Could someone pint me in the right direction on how to post out internally.

 

Thanks!