Different CNC programs from one Mcam file

[Joels]

Hello,

Say i am going to machine a block to clean up the sides on a 3 axis fadal. I would like to make 3 separate tool motions, one for each side and have mcam output prog 1000, 2000 and 3000. in a single file. is this possible?

[Colin Gilchrist]

Yes, very easy to do.

 

To make it easy, create 3 toolpath groups in your operations manager. Now create a set of toolpaths for each side you want to cut. Use a WCS for each side, and set the origin for each WCS like you will on the actual machine.

 

Select each group of toolpaths, right click, edit selected operations, change NC filename. The select each group again, right click, edit selected operations, change program number.

[Joels]

Colin, Thank you for your help. that is almost what i want but i would like all 3 programs to come out in one file. I could cut and paste the separate files but i would like them to come out in one file. is that posiible? kind of like a subprogram does.

[Joels]

Kind of like this,

 

o1000

 

m30

 

o2000

 

m30

 

o3000

 

m30

 

all in one file.

[Stan_z]

not gonna happen unless you do some manual entry operations etc. which I have done and it outputs OK. I have asked my reseller about this type of programming and he said it cant be done...So if anyone has some ideas it would help me to

[K2csq7]

????

Why do you want multiple programs in one file

????

 

I don't know how it could be done...

 

if "end of toolpath group"

pbld, "M30"

 

if start of toolpath group

psof

 

Just thinking out loud...

[Santa Fe]

I don't see why you want:

o1000

m30

o2000

m30

o3000

m30

all in one file.

 

Would it be the same if:

You put it all in one toolpath group except make sure your toolpaths will have a specific WCS (you will have to create two new WCS). The places where you need to stop the machine to flip the stock do a toolpath manual entry and send the y-axis to home and insert an M00.

 

Make sure all the toolpaths will share the same NC file name.

[Stan_z]

HERES HOW I DO IT. Its alot of manual entry but it works and I still have to do minimal editing to make it perfect. I deleted code in the middle just so you can see what I did.

 

 

%

O0001( T.TXT )

( DATE - 09-23-10 )

( TIME - 9:22 AM )

N10 M98 P9998

O0001

M98 M9998

(ROUGH 1420 LONG V-RAIL)

M00 (ROUGH LONG V-RAIL MILLING ONLY)

(CLAMP ON THE 2" STOCK)

(PROGRAM WILL LEAVE .050 PER SIDE)

( RGH TOP )

N12 T1 M6 ( 1/2 CARB LONG EM 1.5" FLUTE )

N14 G20

N16 G0 G17 G40 G49 G80 G90

N18 M8

N20 G0 G90 G55 X3.849 Y-2.49 S6000 M3

N

N250 G1 Z-.235

N252 Y0.

N254 G0 Z.5

N256 M98 P9998

N258 M01

M00 (DONE ROUGHING LONG V-RAIL)

M30

O0002

M98 M9998

(ROUGH 1455 SHORT V-RAIL)

M00 (ROUGH SHORT V-RAIL MILLING ONLY)

(CLAMP ON THE 2" STOCK)

(PROGRAM WILL LEAVE .050 PER SIDE)

( RGH TOP )

N260 T1 M6 ( 1/2 CARB LONG EM 1.5" FLUTE )

N262 G20

N264 G17 G40 G49 G80

N266 M8

N268 G0 G90 G55 X3.849 Y-2.49 S6000 M3

N270 G43 H1 Z.5

N272 Z.05

 

N484 X1.409 Y0.

N486 Z.05

N488 G1 Z-.235

N490 Y-1.97

N492 G0 Z.5

N494 X4.059

N496 Z.05

N498 G1 Z-.235

N500 Y0.

N502 G0 Z.5

M00 (DONE ROUGHING SHORT V-RAIL)

M30

O0003

M98 M9998

(FINISH 1455 LONG V-RAIL)

M00 (FINISH LONG V-RAIL MILLING AND DRILLING)

(CLAMP ON THE 1.97 STOCK)

( MILL UNIFORCE RIB )

N504 X2.734 Y-2.27

N506 Z.05

N508 G1 Z-.275

N510 Y.3

N512 G0 Z.5

N514 Y-2.27

N516 Z.05

N518 G1 Z-.285

N520 Y.3

N522 G0 Z.5

N524 M98 P9998

N526 M01

M00 (DONE WITH LONG V-RAIL)

M30

O0004

M98 M9998

(FINISH 1455 SHORT V-RAIL)

M00 (FINISH SHORT V-RAIL MILLING AND DRILLING)

(CLAMP ON THE 1.97 STOCK)

( MILL UNIFORCE RIB )

N528 T1 M6 ( 1/2 CARB LONG EM 1.5" FLUTE )

N530 G20

N532 G17 G40 G49 G80

N534 M8

N536 G0 G90 G55 X2.734 Y-2.27 S6000 M3

N538 G43 H1 Z.5

N540 Z.05

N542 G1 Z-.275 F60.

N544 Y.3

N546 G0 Z.5

N548 Y-2.27

N550 Z.05

N552 G1 Z-.285

N554 Y.3

N556 G0 Z.5

N558 M98 P9998

M00 (DONE WITH SHORT V-RAIL)

M30

N560 M30

%

[Craig-B]

This is the post way.

Note: Save a copy of your post.

Try adding the following to your post in the (ptlchg) section after (sm01)

 

if mi9$=one,

[

n$, "M30", e$

n$, " ", e$

*progno$, " (", sprogname$,sextnc$, ")", e$

pbld, n$, *sgcode, *sgplane, *smetric, "G40", "G49", "G80", *sgabsinc, e$

]

Then just right click each operation set program number., Then open each operation click tool and check the force tool change, open and misc values and set mi9 to 1 on each operation and post.

[mkd]

i would do what Colin said except assign the same NC file name to all operations.

i assume the only reason you would want to do this is to have multiple operations (multi-vises) setup on the machine using a single program. if so you would also want to setup different work offsets in the "planes" window; E1, E2, E3 etc

[Joels]

Yes it is for one program to download and machine different operations. We put it together manually now, i was wondering if it was possible to met mastercam to do it a simple way. i guess the easy way would be have the sater and end of programs and manually past them to the program that was output. Thank you all for your replies.

[mkd]

manually pasting together is not the easy way.

let mastercam do the work.

[Tim Johnson]

Craig (FNMI) just showed you how to edit your post and what process changes to make to accomplish what you want. Give it a shot.

 

I also find it hard to believe that a reseller or their tech guy would say such an easy task can't be done.

[Guest SAIPEM]

I just uploaded a small utility I wrote to merge files.

 

NCFileMerge.zip is on the FTP site in the ..Text_&_post_files_&_misc folder

 

Extract the NCFileMerge.exe file to your Desktop.

 

From Windows Explorer, Select the NC Files you wish to merge into one single NC file.

 

Drag your multiple file selections from Windows Explorer and Drop them on the NCFileMerge.exe .

 

The program will prompt you for a File Name to Save the Merged File as.