Programming multiple parts per fixture
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 38
  1. #1
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,300
    Post Thanks / Like
    Likes (Given)
    746
    Likes (Received)
    1792

    Default Programming multiple parts per fixture

    Hello,
    I suspect this comes down to a mixture of personal preference and resource limitations but I wanted to ask anyway.

    If you're milling multiple identical pieces per fixture, do you program each piece as a new fixture offset or set the fixture as one offset and have multiple entities in the model? It seems like the biggest decision is whether you want to make individual tweaks in the control or in the model, but maybe I'm missing something.

    Are there distinct advantages to either method and which do you prefer?

  2. #2
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,725
    Post Thanks / Like
    Likes (Given)
    1537
    Likes (Received)
    1763

    Default

    Quote Originally Posted by Cole2534 View Post
    Hello,
    I suspect this comes down to a mixture of personal preference and resource limitations but I wanted to ask anyway.

    If you're milling multiple identical pieces per fixture, do you program each piece as a new fixture offset or set the fixture as one offset and have multiple entities in the model? It seems like the biggest decision is whether you want to make individual tweaks in the control or in the model, but maybe I'm missing something.

    Are there distinct advantages to either method and which do you prefer?
    I use a combination of both. For example, might lay out multiple pieces for a sanity check, then program one face pass (for example) setting stock up for G54 only. Then I might transform the spot/hole drilling ops. Depends entirely on part and features IMO.

  3. #3
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,300
    Post Thanks / Like
    Likes (Given)
    746
    Likes (Received)
    1792

    Default

    Reason for my Q was that I need to drill/tap Al bars in the vise, no critical features or dims. In the manual mill I'd line them up, locate one hole, and then offset by the spacing. In the CNC, the vise is already a fixture so just model up however many pieces fit in the vise, or do them individually.

    I think it depends on how picky the parts are, I'd rather make individual tweaks for location in the control rather than the model.

  4. Likes cmainman liked this post
  5. #4
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    10,099
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2622

    Default

    advantage with a different work offset for each part is when each part is probed and different work offset used for each part. the probing can get exact location on specific features like a bore or specific surfaces
    ....often parts spaced the spacing is not exact and can vary .001 to .010" if edge locators are not exact in position or torque used not exactly the same or even uneven temperature control, probing will give a more exact current position of specific features

  6. #5
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,660
    Post Thanks / Like
    Likes (Given)
    4269
    Likes (Received)
    2825

    Default

    It depends really.
    Are these 1st op parts where you're qualifying the outside to make sure the holes will be in location?
    Or are they 2nd op parts where a finished edge is up against a stop?
    If you're locating a finished edge up against a stop I would go with separate work offsets.
    If it's raw stock, just 1 offset will suffice.

    I do both, sometimes in the situation above, or how I'm feeling that day.

  7. Likes AARONT, wheelieking71 liked this post
  8. #6
    Join Date
    Jul 2012
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    2,855
    Post Thanks / Like
    Likes (Given)
    1104
    Likes (Received)
    1141

    Default

    As long as the quantities support it I always program 1 or 4 parts then shift the coordinate system to make more, usually with fixture offsets. Of course, the best answer to your question is "it depends". For lower quantites I just make one part at a time since I make them on a fast drill/tap mill, another important detail to how to program is what are you programming for.

  9. #7
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    992
    Post Thanks / Like
    Likes (Given)
    1127
    Likes (Received)
    648

    Default

    Personally I like to use a separate work offset for each part. Just because I like to have the most control over my parts. But as stated above if it's the first op it's usually not an issue to just pattern out the toolpaths on the CAM side.

  10. Likes Rstewart liked this post
  11. #8
    Join Date
    Sep 2017
    Country
    UNITED STATES
    State/Province
    Wisconsin
    Posts
    622
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    301

    Default

    If I am cutting fixtures (or soft jaws) and putting the parts in them, then I'll use pattern outputs from CAM and a single WCS zero since the machine will repeat. If it is something like vise work I use multiple WCS. If I have probing this also changes things since I will generally probe certain types of features on a machine that won't be slowed down much by it (Speedio, Robodrill, etc.) for vise work.

  12. #9
    Join Date
    Sep 2010
    Location
    Oklahoma City, OK
    Posts
    4,300
    Post Thanks / Like
    Likes (Given)
    746
    Likes (Received)
    1792

    Default

    Quote Originally Posted by DavidScott View Post
    As long as the quantities support it I always program 1 or 4 parts then shift the coordinate system to make more, usually with fixture offsets. Of course, the best answer to your question is "it depends". For lower quantites I just make one part at a time since I make them on a fast drill/tap mill, another important detail to how to program is what are you programming for.
    I usually do that, but I'm trying to train myself to step back from the machine so I can multitask.

  13. #10
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    361
    Post Thanks / Like
    Likes (Given)
    30
    Likes (Received)
    94

    Default

    You also could try G52 local coordinate system with each shift calling a subprogram for each machining operation. Only have to set one work offset that way, and spacing can be easily altered by the value on the G52 line.

  14. #11
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    South Carolina
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    0

    Default

    Generally speaking, I use a different coordinate system for each loose piece of material. If I am making 2pcs. from one block then they will be modeled and programmed together in one system.

    Sent from my SM-J737V using Tapatalk

  15. #12
    Join Date
    Sep 2013
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    292
    Post Thanks / Like
    Likes (Given)
    90
    Likes (Received)
    64

    Default

    When I program multiple parts I like to use a MCS for each part unless multiples are being milled from one block, as cmainman mentioned. It is desirable to use multiple MCS if you are nesting parts with multiple orientations and non-nominal spacing. In those cases it's nice to have your cam system use one program and apply to to all MCS's regardless of how and where the part are situated and still be able to do full tool path checking and simulation. The icing on the cake is the ability to deviate from instanced tool paths and tweak individual parts if needed but still have full associativity and be able to revert back to the instanced paths if needed. I love that feature of NX. On a tangent, another cool feature which comes in handy is the ability to use an IPW (stock model for the MC guys) on various parts with MCS's all over the place. Again with full associativity, gouge checking and simulation.

  16. #13
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,081
    Post Thanks / Like
    Likes (Given)
    225
    Likes (Received)
    2096

    Default

    I vote for compact code, one program called multiple times with datum shifts or offsets or whatever. It ensures that the same code is run on each part.

  17. Likes cmainman, TeachMePlease, Rstewart liked this post
  18. #14
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    270
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    Quote Originally Posted by gustafson View Post
    I vote for compact code, one program called multiple times with datum shifts or offsets or whatever. It ensures that the same code is run on each part.
    I concur. Also safer. One local drawing. One local program. Once proofed you can dance it around the stock and/or machine any way you want using on the fly G10 offset changes or simple work coordinate changes or both. I'll create programs that have all the additional part program calls block skipped out. Button in... one part. Button out... many parts.

    Dave

  19. Likes cmainman, gmoushon liked this post
  20. #15
    Join Date
    May 2018
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    50
    Post Thanks / Like
    Likes (Given)
    45
    Likes (Received)
    38

    Default

    Keep in mind the amount of tool changes with some of these suggestions.

  21. Likes wheelieking71 liked this post
  22. #16
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    708
    Post Thanks / Like
    Likes (Given)
    104
    Likes (Received)
    365

    Default

    Quote Originally Posted by Rick Finsta View Post
    If I am cutting fixtures (or soft jaws) and putting the parts in them, then I'll use pattern outputs from CAM and a single WCS zero since the machine will repeat. If it is something like vise work I use multiple WCS. If I have probing this also changes things since I will generally probe certain types of features on a machine that won't be slowed down much by it (Speedio, Robodrill, etc.) for vise work.
    I do the same. Both ways depending on the setup or qty. Multiple or perhaps different vises I program one part and the post spits out sub calls and separate WCS for each.

    Dedicated fixture? Array or pattern in CAM and make it one big program. One offset per group of parts.

    Quote Originally Posted by Jmaks View Post
    Keep in mind the amount of tool changes with some of these suggestions.
    Either way you can still minimize toolchanges. In both methods each tool is run through the whole lot, before changing to next tool.

  23. #17
    Join Date
    Jun 2015
    Country
    UNITED STATES
    State/Province
    Minnesota
    Posts
    270
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    86

    Default

    Quote Originally Posted by Jmaks View Post
    Keep in mind the amount of tool changes with some of these suggestions.
    The program style I speak of has the exact same amount of tool changes regardless of how many parts. The block skipped blocks that call for additional offsets or parts to be made are included in each tools' programming.

    Dave

  24. Likes Jmaks liked this post
  25. #18
    Join Date
    Sep 2002
    Location
    People's Republic
    Posts
    3,081
    Post Thanks / Like
    Likes (Given)
    225
    Likes (Received)
    2096

    Default

    Quote Originally Posted by Jmaks View Post
    Keep in mind the amount of tool changes with some of these suggestions.
    absolutely

    It does depend on machine tool change time, but most of my programs consist of a series of subprograms then datums shifts and label calls[heidenhain speak]

    I tend to write them as a single position then label them after so the program rarely begins at block 1, just a note at the beginning saying 'starts ad block 456'

    keeps it so I can run one part if need be.

  26. #19
    Join Date
    Apr 2013
    Location
    South Australia
    Posts
    431
    Post Thanks / Like
    Likes (Given)
    112
    Likes (Received)
    145

    Default

    Depends on the machine as well. In Mazatrol you can set up multiple pieces at the start of the program Then prioritize the tools to save on tool changes. Works great for me

  27. #20
    Join Date
    Feb 2012
    Location
    California
    Posts
    1,373
    Post Thanks / Like
    Likes (Given)
    883
    Likes (Received)
    1470

    Default

    Pros:
    - Fewer tool changes
    - Potentially less air cutting from fewer lead-ins/outs
    - Easier to re-run finishing ops for high accuracy features
    - Higher density fixtures are possible

    Cons:
    - Tweaking programs in CAM may require reselecting a lot of geometry
    - Programs can be much longer, a problem if your machines are memory-limited
    - Proving out programs can be tiresome (babysitting a much longer cycle)

    So we split the difference.

    On a 4-sided tombstone in an HMC, running identical parts on all faces and multiple parts per face, we machine all identical parts on one face simultaneously. Then index 90, run again, rinse and repeat.


Tags for this Thread

Bookmarks

Posting Permissions

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