Same Part Multiple fixtures?

[pp-TG]

Hi All,

Just wondering if it is possible to cam 1 part and have mastercam v9.1 post it for mutiple fixtures using different WC.(ex. 1 part- 3 seperate vises G54,G55,G56) Currently 1 cam the one part and cut and past the program for different wcs and it is time consumming.

Any help would be very helpfull..

Thanks, Travis

Similar Threads:

• Need Help!- MasterCam X Multiple Fixtures
• multiple part profiles
• Multiple part offest on M2 control
• SAME part 2 fixtures ..VMC with no 4th Axis
• Machining Multiple of the same part

[Tim Bailey]

If block labeling and repeat block cycles are available on your control, then just call up the work offset (G54 ect) and repeat the blocks of the program, then call G55 and do the same. Another method is to label the program as a subroutine then position to G54 then call the subroutine , then G55, ECT

[Geof]

Do it the way Tim recommends; locate all your G5n's then turn your Mastercam output into a subroutine and call it using each G5n. This way if for some reason you have to change the post you only have to change one copy; less chance of errors this way.

[pp-TG]

Thanks, Geof and Tim I will give it a try and see how that works. By the way welcome Tim.....

Travis,

[mark c]

Try this link:
http://www.emastercam.com/posts/mpsubrep/mpsubrep.html

It is a post where you program a part then tell it how many locations you want to run it. I used it for years
HTH

[rickyt]

if you use the mpsubrep.pst choose your post first, then in your first toolpath open misc values and then put in the number of parts on one of the lines. I can't remember which one but it should say.

[mark c]

I should have remembered to mention that; I modified mine so that it would ask for a number upon posting cuz I always forgot to input the misc variable

[pp-TG]

Thanks, rickyt and marc

I will give that a try. Sounds like what I am looking for....

Also Geof & Tim you both said to use sub's not sure if i am missing something but some operations do not give you the sub option(ex. Face Milling) do you guys just turn that into a sub manually?

What I am trying to do is call up a tool and use it on all WCS and then call up the next tool and use it on all WCS and so on....

Thanks allot for the Help guys.

[Geof]

....Also Geof & Tim you both said to use sub's not sure if i am missing something but some operations do not give you the sub option(ex. Face Milling) do you guys just turn that into a sub manually?....

I can't help with "how to do" only suggest what to do. In my opinion you want the program information in only one location; a subroutine which you access from each location. If you cannot get out what you need you may need to do some manual editing.

[cadcam]

if you post your file or email it to me I will use the WCS and transform for the rest and send it back with some info.

[Tim Bailey]

I am not sure but it sounds to me like your confusing a subroutine with canned cycles. An entire program with multiple tools can be labeled as a subroutine. Normally a little manual editing is necessary to achieve the proper configuration. Imagination is the key!!!

[mark c]

If you use that post and have it dialed in, then there will be no hand editing involved. It does everything for you. I HATE hand editing; I find that this is where I will make mistakes rather than the CAM side of things
HTH

[Mountainwildman]

In the tool parameters page click the "T/C Plane" button then check the box in the bottom left corner that says "work offset" 0=G54 1=G55 2=G56 3=G57 and so forth. If your post supports the WCS it will work. All you have to do to make it go to each fixture before changing tools is copy the operation after and change your work offsets.

[Mountainwildman]

In the "Tool Parameters" page (the one you enter your feeds and speeds in) click the "T/C Plane" button, then in the bottom left corner check the box that says "Work Offset" change the -1 to 0 for G54, 1 for G55, 2 for G56, and so forth. Then to machine on each offset before changing tools just copy that operation after itself and change the work offset. Its also a good idea to turn on your clearance plane when doing this in case of different Z heights.

[cadcam]

Wow this hole posting is a simple "Tool Path Transform" and it will even give to you as subs and diffrent offsets. All from programming one part.

[pp-TG]

Wow this hole posting is a simple "Tool Path Transform" and it will even give to you as subs and diffrent offsets. All from programming one part.
.


Can you give me an example of this?

do you do the whole part programming then do a tool path transform?

Thanks,

[pp-TG]

Thanks CadCam you are right that transform does work great! The only part i have yet to figure out is how to get it to call up the different work offsets
G55,G56..... it only has the first g54 the transform does not call up a work offset is it possible or do you just have to manually put it in?

Thanks again for your help.

[cadcam]

Review picture sir.

[pp-TG]

Thanks for all your help CadCam. But i am still having trouble i can get it to sort of work if i use a different post then i normally do but the first work offset called up is allways the bigger number and the second is always the
G54 any way to change that so the G54 is the first and so on? Also is there something i can change in my normal post to get this to work with it....? I have most of it set up the way i like.

Thanks again for your help...

[cadcam]

Can you send me your file and post so I may review?