584,808 active members*
5,062 visitors online*
Register for free
Login
IndustryArena Forum > CAM Software > Mastercam > Same Part Multiple fixtures?
Page 1 of 3 123
Results 1 to 20 of 58
  1. #1
    Join Date
    Sep 2006
    Posts
    179

    Same Part Multiple fixtures?

    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

  2. #2
    Join Date
    Nov 2006
    Posts
    3
    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

  3. #3
    Join Date
    Jul 2005
    Posts
    12177
    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.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  4. #4
    Join Date
    Sep 2006
    Posts
    179
    Thanks, Geof and Tim I will give it a try and see how that works. By the way welcome Tim.....:cheers:

    Travis,

  5. #5
    Join Date
    Sep 2004
    Posts
    145
    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
    Insanity "doing the same thing and expecting a different result"
    Mark

    www.mcoates.com

  6. #6
    Join Date
    Nov 2005
    Posts
    174
    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.

  7. #7
    Join Date
    Sep 2004
    Posts
    145
    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
    Insanity "doing the same thing and expecting a different result"
    Mark

    www.mcoates.com

  8. #8
    Join Date
    Sep 2006
    Posts
    179
    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.

  9. #9
    Join Date
    Jul 2005
    Posts
    12177
    Quote Originally Posted by pp-TG View Post
    ....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.
    An open mind is a virtue...so long as all the common sense has not leaked out.

  10. #10
    Join Date
    Apr 2003
    Posts
    3578
    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.
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

  11. #11
    Join Date
    Nov 2006
    Posts
    3
    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!!!

  12. #12
    Join Date
    Sep 2004
    Posts
    145
    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
    Insanity "doing the same thing and expecting a different result"
    Mark

    www.mcoates.com

  13. #13
    Join Date
    Apr 2005
    Posts
    9
    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.
    ,Buster

  14. #14
    Join Date
    Apr 2005
    Posts
    9
    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.
    ,Buster

  15. #15
    Join Date
    Apr 2003
    Posts
    3578
    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.
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

  16. #16
    Join Date
    Sep 2006
    Posts
    179
    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,

  17. #17
    Join Date
    Sep 2006
    Posts
    179
    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.

  18. #18
    Join Date
    Apr 2003
    Posts
    3578
    Review picture sir.
    Attached Thumbnails Attached Thumbnails transoffsets.jpg  
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

  19. #19
    Join Date
    Sep 2006
    Posts
    179
    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...

  20. #20
    Join Date
    Apr 2003
    Posts
    3578
    Can you send me your file and post so I may review?
    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
    Cadcam
    Software and hardware sales, contract Programming and Consultant , Cad-Cam Instructor .

Page 1 of 3 123

Similar Threads

  1. Deluxe Stand and Tormack 1100 and interference with holding fixtures
    By ddixon in forum Tormach Personal CNC Mill
    Replies: 3
    Last Post: 05-26-2007, 03:15 PM
  2. Lifting fixtures on and off the machine.
    By Smackre in forum Uncategorised MetalWorking Machines
    Replies: 5
    Last Post: 04-02-2007, 06:18 PM
  3. WorkHolding Fixtures
    By hstanki in forum News Announcements
    Replies: 0
    Last Post: 03-22-2006, 08:36 PM
  4. Workholding Fixtures
    By hstanki in forum Employment Opportunity
    Replies: 0
    Last Post: 03-06-2006, 07:35 PM
  5. eroding Wire EDM fixtures
    By Rivet head in forum Waterjet General Topics
    Replies: 4
    Last Post: 09-30-2005, 01:15 PM

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •