Translating drilled hole 3 times posting a sub routine for each hole

[DC CNC]

I'm translating a simple drilled hole 3 times. I want the main program to call location and 1 subroutine to drill the hole. When I post it I get the main with 3 subroutine P1 thru P3 and the subs O1 thru O3 . I just need it to post one sub for all 3. Is this something in the post or the machine/control def?

[CEMENTHEAD]

check the Incremental button.

 
( 1/8 DRILL )
(TOOL NO. 1)
(TOOL DIA. .125)
(LEN. OFFSET 1)
(DIA. OFFSET 41)
 
 
N1G17G98G40G49G80G90
N2G0X0.Y7.
N3T1M6
N4S2139M3
N5G0G90G54X0.Y0.B0.
N6G43H1Z4.
N7M08
N8M98P0001
N13G90X1.
N14M98P0001
N19G90X2.
N20M98P0001
N25G90X3.
N26M98P0001
N31G90X4.
N32M98P0001
N37M09
N38G0G28G53G49Z0.M19
N39G90X0.Y7.
N40M30
 
O0001
N9G91
N10G83Z-4.R-3.9Q.06F4.11
N11G80
N12M99
%
 

[DC CNC]

We've decided to use multiple work offsets but would like to only post one subroutine for each operation. There are several profile ops besides the drilling. Can this be done in absolute?

[crazy^millman]

58 minutes ago, DC CNC said:

We've decided to use multiple work offsets but would like to only post one subroutine for each operation. There are several profile ops besides the drilling. Can this be done in absolute?

Will need to get a hold of your dealer since you are going off in Custom Posting land. They way the logic is written and how it also work with Mp.dll just not sure there is an easy method to handle it with absolute. Maybe Colin or someone else will come along and teach us there is a simple method, but I am not knowledgeable enough to make such a claim there is.

[cruzila]

Using work offsets uses absolute based on the position of the work offset as a new datum location. I don't get what you are trying to accomplish

[DC CNC]

We want to post multiple work offsets with one subroutine program for each op

[crazy^millman]

15 minutes ago, DC CNC said:

We want to post multiple work offsets with one subroutine program for each op

Using absolute for the control and not incremental.

[Tim Johnson]

On 5/4/2022 at 9:49 AM, DC CNC said:

We've decided to use multiple work offsets but would like to only post one subroutine for each operation. There are several profile ops besides the drilling. Can this be done in absolute?

I do that every day but that is a lot of post work. The trick is to use routers for each type of process.

[Tim Johnson]

This is our routers list for our Kurt clustertowers running up to eight parts in each pallet. The probing has to have different subprograms because you can't rotate the probing toolpaths but it's one toolpath sub for each of the other different paths and the router will do the work offsets, rotations and check if the next particular fixture is turned on. If the fixture turned off the router will check the next one in line.

1. CLUSTER VISES 8 PARTS

 11. CLUSTER VISES 8 PARTS (5001~5007)

 12. CLUSTER VISES 8 PARTS WITH PART INVERT MACRO (5001~5007)

 13. CLUSTER VISES 8 PARTS WITH PARTS SAME POSITION TWO DIFFERENT JAWS WITH TWO  PART OPERATION (5001~5007)

 14. CLUSTER VISES 8 PARTS RUNNING FOUR PARTS AT 0 AND 180 DEGREE (5001~5007)

 15. CLUSTER VISES SYSTEM 11 PALLET A (5001~5007), SYSTEM 34 PALLET B (5301~5307)

 16. CLUSTER VISES 8 PARTS RUNNING FOUR PARTS AT 0 AND 180 DEGREE WITH PART INVERT MACRO (5001~5007)

 17.CLUSTER VISES 8 PARTS WITH RUNNING FOUR PARTS AT 0 AND 180 DEGREE TWO DIFFERENT JAWS WITH TWO PART OPERATION (5001~5007)

 

 

[DC CNC]

So if I understand this correctly the post must be modified to do this. I'm not clear on the "router" and how that works.

[Tim Johnson]

7 minutes ago, DC CNC said:

So if I understand this correctly the post must be modified to do this. I'm not clear on the "router" and how that works.

 

Heavy modification. Our post has 10,542 lines without including the XML crap (19,445 lines with it) but we have five machines and 39 routing systems. All five machines use the same routers. But once the work is done the programming time is significantly reduced.

 

[crazy^millman]

35 minutes ago, DC CNC said:

So if I understand this correctly the post must be modified to do this. I'm not clear on the "router" and how that works.

On 5/4/2022 at 7:49 AM, crazy^millman said:

Will need to get a hold of your dealer since you are going off in Custom Posting land. They way the logic is written and how it also work with Mp.dll just not sure there is an easy method to handle it with absolute. Maybe Colin or someone else will come along and teach us there is a simple method, but I am not knowledgeable enough to make such a claim there is.

Not to repeat myself, but yes the post must be modified and you should get a hold of your dealer. Tim is an experience Post person and has helped me with different issues over the last 18+ years on the forum. I imagine it took well over 40-60 hours of work to dial this in with his years of experience. You are more than welcome to download the MP documentation and learn. I am never trying to stop someone from learning, but if my back is against the wall and I can get help I have learned that is faster and cheaper in the long run.

[Tim Johnson]

Sorry, I missed the router part.

The router is basically a roadmap for the machine to follow the variable codes that states what the operator wants it to do.

[DC CNC]

Thanks for the replies. Looks like we have our work cut out for us.

[crazy^millman]

45 minutes ago, DC CNC said:

Thanks for the replies. Looks like we have our work cut out for us.

As you try things and get stuck post them up with a sample file in the Post section of the forum and plenty of people will be glad to help. Make a sample file and share your work and when people see your trying they willing to help those helping themselves.

[Tim Johnson]

DC, Check your messages

[metalmansteve]

Maybe I'm misunderstanding the question but this is how I use transform using multiple work offsets with the operations as subroutines on a VMC.

[crazy^millman]

17 hours ago, metalmansteve said:

Maybe I'm misunderstanding the question but this is how I use transform using multiple work offsets with the operations as subroutines on a VMC.

Click the absolute Sub Program and try that again.