Programming multiple parts using G54, G55 etc.

[Murray Mold]

Hello all,

I have some square cores that we do several times a year and I am gearing up for "lights out" machining and want to do 2 of them at one time. The cycle time on 1 part is 5.5 hours and we usually make 12 or 18 at a time.

These are h/t H-13 48-50 Rc.

My question is, can I do this and post it right out of MCX3 or am I gonna have to manually edit and paste code to get it to work correctly? (I've done multi parts before by copy & paste but I would like to learn how to do this in MC of possible)

 

You can see where the origin is on part #1 and it needs to be the origin on part #2 as well so can you use(and post from) multiple wcs in 1 program?

I can not get my "Print Screen" button to show just one screen so sorry about the big pic.

The left side is the correct one

 

[Simtech]

Have you tried a Transform Translate toolpath using the Tool Plane Method?

[YoDoug®]

If the parts a identical you could program 1 part and use a transform rotate assinging a new work coordinate to get you G54, G55, etc.

 

If the parts are not identical you can create multiple WCS to get G54, G55, etc.

 

Can you share the file or put it on the ftp, or I could share a sample file of either if you would like.

[Murray Mold]

I would put it on the ftp, but when I rotated the part I forgot to select "Copy" instead of "Move" and now I have 108 dirty ops!!! &%*#$@

Stupid me was in a hurry. One of these days I'll learn to "Walk" down the hill and get em all instead of "Run" down and get one of em.

 

Doug,

If you would put a sample on thr ftp I would appreciate it

[Tim Johnson]

There are several ways to run multiple parts. If your only going to run two at a time the transform operations may be the easiest way to go. The process is not hard to figure out. If you're going to run more than two parts at a time then you'll probably want to variable offsets and run all your parts on one toolpath (per tool).

[YoDoug®]

I put a file on the ftp that has a contour operation rotated 4 times. If you post it, it uses G54-58 for the five total contours.

 

File is a zip-2-go = PAC-142-01A-OP30M-TOOLPATH.Z2G

 

location on ftp = MCX2_Files

[?Mark]

Murray Mold & Die , I sent you a sample part with multiple transform ops. that should be self explanatory...

check your mail.

hth

[Murray Mold]

Thanks guys

[Murray Mold]

Thanks for the samples and the info. It's posting out code that will work except there are no G54, G55. It's also posting 2 files and there is no text in my .nc file but it creates a .ext file with the same name as the .nc file and all the code is in the .ext file???? Crazy....anyone ever had this happen?

[Brad St.]

Murray, the ideas above are all good ones I'd like to offer another if it fits your use. I've tweeked my post to drop the WCS output (ex no G54. . .) and wrote a main program call on the mill to call the WCS I want the program to run on. Thus you can call the same program to multiple locations add in rotations if you wish.

 

Here's and example of my main call doing this:

O1001

G90 G54

M198 P0001

G90 G55

M198 P0001

G90 G56

M198 P0001

M30

 

You can go on and on this way but your more or less simply running subs. Oh, make sure in the program posted you change the end M30 to a M99 =).

 

The ideas above will get you going now but if you have a habit of doing this more often than not if you make this change you will step into a whole nother world of freedom for the operators and setup guys. Picture if you have a setup you don't wish to take out and want to run on another coordinate system, simply change the main program call. NO file editing necessary at the control or by a programmer. If your into a lot of one ups it's the cats meow for me.

[Murray Mold]

BRADST,

I cant even get it to post 2 parts correctly, I know I cant get it to post 17 operations into subprograms....lol

I copied & pasted just to get chips flying but I'm gonna work on this until I get it right.

 

Thanks

[Brad St.]

Well don't let it fool ya buddy, with what I suggested the files would be your programs posted as normal. Your post would then send out the correct file and you would simply have your setup people place the correct WCS for the operations to be run on in the control. Or you could write the main quickly to go with the programs. With the lights out it can be very helpfull especially if like i mentioned above you are doing 1-ups and want to run different parts at different WCS's. It doesn't have to be the same program.

[Tony35]

murray

are you setting the work offsets in the planes tab?

do you have the work offsets set in the wcs?

check misc interger #9 lock on first wcs?

work offset numbers

-1 G54 default, 0=G54 1=G55 2=G56 etc.

check to see if you have them setup right

HTH

[Murray Mold]

Here's what I have

 

 

 

[Tony35]

in your translate tab how do you have it setup?

between views?

did you try a new wcs for part#2?

if you can zip2go it to me and i will take a quick look at it for ya

[Murray Mold]

The z2g file is 22mb and I cant email over 10mb and I cant upload to ftp. It keeps asking for username and password

[Tony35]

username= mastercam

pass= swiss

[Murray Mold]

It has 23 minutes to go

square core_current.ztg

Thanks

 

edit: ops 61 thru 77 are the ones I'm trying to transform

 

[ 10-28-2008, 11:37 AM: Message edited by: Murray Mold & Die ]

[Tony35]

tick tock tick tock

[Murray Mold]

It's done uploading

It's in x3 files folder

[Tony35]

ding

[htm01]

if the parts are the same just copy the toolpath group and then edit the copy,right click,edit selected operations,and renumber work offsets

[Jack Neelands™]

Turn your copy source operations off and your sub programs off and see what you get first....make sure you are only highlighting the translate operation when you post or you will get the first set posted twice....you can ghost the original so that they do not post out when you click on the whole machine def.

 

Hope that Helps

[Murray Mold]

When I turn "Copy source Ops" off, I get nothing...it will not regen and toolpath has 0.0k

 

The way I have it, it posts (almost) correctly except no G54, G55 and the file is an .ext instead of .nc

 

I'm going to lunch now thanks to everybody for help and I will return @ 12:30 CST

[Jack Neelands™]

N100 O0000 ( 5373 )

N110 ( CREATED ON 10-28-08 AT 12:46 PM )

N120 ( MCX FILE - C:DOCUMENTS AND SETTINGSJOHNNDESKTOPCLEANUP5373.MCX )

N130 ( NC FILE - C:MCAMX3MILLNC5373.NC )

N140 ( MATERIAL - ALUMINUM INCH - 2024 )

N150 G20

N160 G0 G17 G40 G49 G80 G90 H0 E0 Z0

N170 ( 2.0 UDRILL TOOL - 1 DIA. OFF. - 0 LEN. - 0 DIA - 2.0 )

N180 T1 M6

N190 A-0.

N200 G0 G90 S250 M3 G54 X0. Y6.13 FIRST LOC

N210 H0 Z16.

N220 G81 G98 X0. Y6.13 Z-5.5 R0.1 F2.5

N230 X-43.113

N240 X-46.113

N250 G80

N260 G55 X0. Y6.13 Z16.--------SECOND LOC

N270 G81 G98 X0. Y6.13 Z-5.5 R0.1 F2.5

N280 X-43.113

N290 X-46.113

N300 G80

N310 M5

N320 G90 H0 Z0.

N330 M1

N340 ( 3.00 SUMOTOMO FACE MILL TOOL - 2 DIA. OFF. - 0 LEN. - 0 DIA - 3.0 )

N350 T2 M6

N360 G0 G90 S1800 M3 G54 X1. Y12.125

N370 H0 Z16.

 

 

This is what I am getting with the MP master poster ....but the G54 is coming up as an "E" of course...I have not edited the post yet.