Mill Part Setups (SolidWorks/MasterCam)
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 22
  1. #1
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Mill Part Setups (SolidWorks/MasterCam)

    I'm trying to figure out how to separate my different mill part setups in SolidWorks Cam so my machine will automatically stop between each operation.

    For example, I've got a three operation part right now with three different mill part setups- one for each operation. However, when I generate the code, it runs the whole program through without any stops in the program. Which means I have to physically stop the machine and restart it manually instead of it finishing an op and holding waiting for a restart after I flip the part.

    I know there's got to be a way to enable some sort of stop between mill part setups. I just can't seem to find anything on the web or the search on here.

    Any help is great appreciated.

  2. #2
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Arkansas
    Posts
    40
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    19

    Default

    Just add an M00 (flip and or rotate part); where you want it to stop.

  3. Likes Winterfalke, KFALCON954 liked this post
  4. #3
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,992
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2591

    Default

    Quote Originally Posted by quickid71 View Post
    I'm trying to figure out how to separate my different mill part setups in SolidWorks Cam so my machine will automatically stop between each operation.

    For example, I've got a three operation part right now with three different mill part setups- one for each operation. However, when I generate the code, it runs the whole program through without any stops in the program. Which means I have to physically stop the machine and restart it manually instead of it finishing an op and holding waiting for a restart after I flip the part.

    I know there's got to be a way to enable some sort of stop between mill part setups. I just can't seem to find anything on the web or the search on here.

    Any help is great appreciated.
    .
    you maybe talking adding manual op in mastercam and you can manually type in gcode like a M0 to stop. you can often add a (COMMENT) too if needed. its there in mastercam adding a manual op, not the easiest to find if never done before but its there
    .
    make sure there is code after to turn spindle and coolant back on after the M0. tapping dont work too well if tap not turning when going down into hole. usually M0 stops spindle and coolant on majority of machines

  5. #4
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,161
    Post Thanks / Like
    Likes (Given)
    1420
    Likes (Received)
    1487

    Default

    Quote Originally Posted by quickid71 View Post
    I'm trying to figure out how to separate my different mill part setups in SolidWorks Cam so my machine will automatically stop between each operation.

    For example, I've got a three operation part right now with three different mill part setups- one for each operation. However, when I generate the code, it runs the whole program through without any stops in the program. Which means I have to physically stop the machine and restart it manually instead of it finishing an op and holding waiting for a restart after I flip the part.

    I know there's got to be a way to enable some sort of stop between mill part setups. I just can't seem to find anything on the web or the search on here.

    Any help is great appreciated.

    Not sure about Mastercam for Solidworks, but in older versions of MCX you can use a "manual entry"toolpath. Check the box at the bottom that says "output - as code" and in the text box type in M00 between your parts/setups. Depending on machine, you may need to do something like

    G91G28Z0.
    G91G28Y0.
    M05
    M09

    etc, depending on machine make and what you want it to do/where to go while you are flipping parts.

  6. #5
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,992
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2591

    Default

    adding manual op is also common to move table off to the side out of the way so long tool during tool change dont hit anything. its not always in tool change macro to move in X and Y all the way over to make room for long length tool change
    .
    you can type in gcode as needed, usually you need to test it to make sure working as expected
    .
    i have also used to turn spindle backwards with coolant to try to get chips to unwind off a drill or mill, sometimes works like 95% of the time, can add M0 to confirm chips off and or manually pull chips off a tool. not exactly something thats programmed in mastercam, that is you use or add a manual op in mastercam to manually type in gcode

  7. #6
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Thanks for the suggestions, guys. I can add an M00, add code to move the spindle/table out of the way then the code to bring everything back and restart. I just figured that the software would already have all of that so I didn't have to manually enter that info in code.

    Where it really sucks is if I'm making changes to a part and have to keep posting it. Every time I post, I have to hunt for the places I need stops and put all that info back in.

    I honestly feel like there should be a little box to check that automatically puts stops in the code between mill part setups. What's the purpose of having "mill part setups" if they don't actually act as different mill part setups?

  8. #7
    Join Date
    Jan 2014
    Location
    Temecula, Ca
    Posts
    2,646
    Post Thanks / Like
    Likes (Given)
    1210
    Likes (Received)
    3462

    Default

    Try checking the "Force Toolchange" button on the toolpath. If I'm understanding your question right, this will do what you want.

  9. Likes Mike1974 liked this post
  10. #8
    Join Date
    Nov 2014
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    3,161
    Post Thanks / Like
    Likes (Given)
    1420
    Likes (Received)
    1487

    Default

    Quote Originally Posted by quickid71 View Post
    Thanks for the suggestions, guys. I can add an M00, add code to move the spindle/table out of the way then the code to bring everything back and restart. I just figured that the software would already have all of that so I didn't have to manually enter that info in code.

    Where it really sucks is if I'm making changes to a part and have to keep posting it. Every time I post, I have to hunt for the places I need stops and put all that info back in.

    I honestly feel like there should be a little box to check that automatically puts stops in the code between mill part setups. What's the purpose of having "mill part setups" if they don't actually act as different mill part setups?
    If you use the manual entry toolpath (if available in your version) it will post it into the code. You just put the manual toolpath where you want it. No need to edit the nc code.

  11. #9
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    293
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    178

    Default

    Right click under the last step you want to insert an M0, you should see an option that says post operations, insert the program stop.
    Attached Thumbnails Attached Thumbnails m0.jpg  

  12. Likes AARONT liked this post
  13. #10
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by Shawnrs View Post
    Right click under the last step you want to insert an M0, you should see an option that says post operations, insert the program stop.
    Shawn,

    It looks like you're on the right track. Unfortunately, it doesn't look like SolidWorks Cam has that option like CamWorks does.
    Attached Thumbnails Attached Thumbnails capture4.jpg  

  14. #11
    Join Date
    Feb 2013
    Location
    Madison, WI
    Posts
    927
    Post Thanks / Like
    Likes (Given)
    1063
    Likes (Received)
    596

    Default

    Quote Originally Posted by Shawnrs View Post
    Right click under the last step you want to insert an M0, you should see an option that says post operations, insert the program stop.
    Nevermind. Just validated SolidCam doesn't have that option

  15. #12
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Missouri
    Posts
    900
    Post Thanks / Like
    Likes (Given)
    208
    Likes (Received)
    570

    Default

    Turn on the option stop on the control if it has it the machine will stop at the next tool change and wait for a green button push


    Sent from my iPhone using Tapatalk Pro

  16. #13
    Join Date
    May 2007
    Location
    Australia Qld
    Posts
    55
    Post Thanks / Like
    Likes (Given)
    5
    Likes (Received)
    29

    Default

    [QUOTE=quickid71;3366937]
    Where it really sucks is if I'm making changes to a part and have to keep posting it. Every time I post, I have to hunt for the places I need stops and put all that info back in.

    Make each setup a separate program that can be run as a sub program once the individual programs are sorted, the main program runs sub 1, then M01, runs sub 2 then M01 and so on.

  17. Likes mhajicek liked this post
  18. #14
    Join Date
    Nov 2006
    Location
    Jupiter, Florida
    Posts
    248
    Post Thanks / Like
    Likes (Given)
    147
    Likes (Received)
    11

    Default

    Our post processor has the option in the "Posting" tab of the tool operation to change the stop choice from M01 to M00. It's been a few years so I'm unsure if we requested that our if it's standard. Worth a look.
    Just change it on the last tool before you need the stop.

  19. #15
    Join Date
    Dec 2008
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    9,992
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    2591

    Default

    CAM program doesnt know what you want and you need to tell it. that includes M0 stops and even picking tooling. CAM software needs to know your preferences.
    .
    for example even if you tell it you got a 6" facemill if it sets up a cut requiring 50hp and or you cant hold the part and it goes flying out of vise / fixture and or do a lot of damage its almost always requires some decisions to be made. or part vibrates too much with 6" facemill and it works better if you use a 4" facemill. CAM aint going to know part fixture vibration limits
    .
    same if you need a 4" dia hole if CAM picks a 4" drill and it tries to drill it in one go requiring over 30 hp on a 10hp machine that can be a problem
    .
    same as adding a M0 to rechuck part at lighter pressure before finish cuts so it doesnt warp so much when released from vise fixture. CAM not going to make those types of decisions for you usually

  20. #16
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by DMF_TomB View Post
    CAM program doesnt know what you want and you need to tell it. that includes M0 stops and even picking tooling. CAM software needs to know your preferences.
    .
    for example even if you tell it you got a 6" facemill if it sets up a cut requiring 50hp and or you cant hold the part and it goes flying out of vise / fixture and or do a lot of damage its almost always requires some decisions to be made. or part vibrates too much with 6" facemill and it works better if you use a 4" facemill. CAM aint going to know part fixture vibration limits
    .
    same if you need a 4" dia hole if CAM picks a 4" drill and it tries to drill it in one go requiring over 30 hp on a 10hp machine that can be a problem
    .
    same as adding a M0 to rechuck part at lighter pressure before finish cuts so it doesnt warp so much when released from vise fixture. CAM not going to make those types of decisions for you usually
    Tom,

    What you're describing is way beyond what I'm asking for. What I'm requesting is very simple and has nothing to do with the physical abilities of the machine guessing our intentions.

    The operation tree (see attached picture) in SolidWorks is made up of one or more "mill part setups." Unless I'm an idiot, I use each mill part setup as a different side of a part or any time I need to adjust or move a part in the machine- a different "mill part setup."

    That being said, the ability to simply have the post processor put an M0 after each "mill part setup" would be extremely nice. This could easily be done with the click of a button rather than having to manually go in and modify the code manually.

    It appears that there are some of you that are following what I'm asking for and have experience using this function on certain software. Maybe I need to update to something more than the SolidWorks cam software.
    Attached Thumbnails Attached Thumbnails capture6.jpg  

  21. #17
    Join Date
    Nov 2006
    Location
    Jupiter, Florida
    Posts
    248
    Post Thanks / Like
    Likes (Given)
    147
    Likes (Received)
    11

    Default

    Have you looked at the Operation tree/Edit definition/Posting tab? Do you have that option or not? We use CAMWorks here so I'm assuming it's the same.
    If you don't have it, you can get it with a new post.

  22. #18
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by Chris59 View Post
    Have you looked at the Operation tree/Edit definition/Posting tab? Do you have that option or not? We use CAMWorks here so I'm assuming it's the same.
    If you don't have it, you can get it with a new post.
    Chris,

    Here's what I have available. Let me know if you need to see anything else.

    Also, if you're using SolidWorks with the CamWorks add-on, you should be able to go to the SolidWorks Cam tab and see everything that I'm seeing. (Assuming you've got the SolidWorks Cam add-on enabled)
    Attached Thumbnails Attached Thumbnails capture7.jpg  

  23. #19
    Join Date
    Nov 2006
    Location
    Jupiter, Florida
    Posts
    248
    Post Thanks / Like
    Likes (Given)
    147
    Likes (Received)
    11

    Default

    I'm using SolidWorks with CAMWorks 2012 Pretty old but it should be similar.
    OK, edit your last tool before the next op. There should be a "Posting" tab between the "Advanced" tab and the "Optimize" tab. Do you have that? I'm beginning to think you don't and my advice is no good.

  24. #20
    Join Date
    Mar 2016
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    293
    Post Thanks / Like
    Likes (Given)
    70
    Likes (Received)
    178

    Default

    Quote Originally Posted by quickid71 View Post
    Shawn,

    It looks like you're on the right track. Unfortunately, it doesn't look like SolidWorks Cam has that option like CamWorks does.
    I can see your image that well but it look like you are under the feature tree tab instead of the operations tree tab. Go to the operations tree and right click on the last before inserting the M0.

  25. Likes Chris59 liked this post

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
  •