Two fold post, Wasino LJ63M m12 ?? and hex milling on it.
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default Two fold post, Wasino LJ63M m12 ?? and hex milling on it.

    Going through old programs that were in the control trying to learn it's milling and I see an M12 right after the start.
    N2(3/4 END MILL T0202)
    G0M41G99G97G80G40
    M12
    M4S2000T0202
    G0M8X0Z.1F300.
    The manual for this live tooling lathe doesn't list M12, just M10/11(chuck clamping) and next in line is M19. Anyone familiar with that M12 critter?

    Also, can anyone supply a small sample of a milling program for a hex or square on the end of a shaft using an old live tooling lathe like this. Once I get my head wrapped around how cutting from a square or hex point and somehow making code go closer to X0 and back out to the next point while the C axis is rotating I can start understanding the rest. Just cutting that simple feature has me stumped.

  2. #2
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    308
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    92

    Default

    We have some newer live tool Wasinos, but none of them have any description in the book for M12. Is that sample code you posted for using the live tooling? If so, it may be a C-axis engage or spindle clamp or live tooling engage code. Have you tried that code in MDI? What does the M41 in the 2nd line do?

    What control is on the machine? Are you sure that it has full C-axis? I think this is a pretty old machine and am a little doubtful that it has full C-axis capabilities- in which case, you couldn't do any cutting with the C-axis turning.

  3. #3
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    Quote Originally Posted by wmpy View Post
    We have some newer live tool Wasinos, but none of them have any description in the book for M12. Is that sample code you posted for using the live tooling? If so, it may be a C-axis engage or spindle clamp or live tooling engage code. Have you tried that code in MDI? What does the M41 in the 2nd line do?

    What control is on the machine? Are you sure that it has full C-axis? I think this is a pretty old machine and am a little doubtful that it has full C-axis capabilities- in which case, you couldn't do any cutting with the C-axis turning.
    That is the code from the control I assume there were running. All those you mentioned (C axis, spindle locking, C axis gear on) are all accounted for in the manual. I haven't tried it in mdi yet, need to do that. M41 is high gear main spindle. This is a Fanuc 10T control. Whether it's full C or not is part of what I'm trying to figure out.

  4. #4
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    This is part of another program with M54(C axis gear on) and M12.1(idk what that is as it's not listed either).
    N3(3/4 END MILL T0909)
    G0G40G80G97G98G18M41
    M54
    G28H-30.
    G50C0.
    T0909
    M4S400
    G1X1.0Z.5F300.
    M8
    G12.1
    G1G98G41X1.5708F30.
    G1Z-.365F10.
    X.7854C-.6802F2.0
    X-.7854
    X-1.5708C0
    X-.7854C.6802
    X.7854
    X1.5708C0

  5. #5
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    308
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    92

    Default

    It looks like your machine does indeed have a full C-axis. That code you just posted is to mill a hex on the end of a part. G12.1 is polar interpolation. Do a search on that to learn more.

    I don't know what M12 is. It could be something like parts counter. Maybe?

  6. #6
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    Ran across a video showing C milling 12.1, the poster mentioned swapping whatever Y value you would have for a feature for a comparable C value. Drawing it on CAD it looks to work.

  7. #7
    Join Date
    Feb 2014
    Location
    FL
    Posts
    4,013
    Post Thanks / Like
    Likes (Given)
    13030
    Likes (Received)
    4787

    Default

    Quote Originally Posted by DMSentra View Post
    Ran across a video showing C milling 12.1, the poster mentioned swapping whatever Y value you would have for a feature for a comparable C value. Drawing it on CAD it looks to work.
    That is exactly how polar works.

    On some controls, you actually program with an X and Y coordinate even. This is polar interpolation. You turn it on, program in X/Y (or X/C) for the feature you want, and the control does the math to make C and X work to create a Y axis.

  8. #8
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    So far it runs the sample program without issue, but I think tool touchoff for the endmill may be wrong. I'm setting that the same I do a turning tool but it's nowhere close to the dimensions programmed. I've got job coming that I need this hex to work to get the job. I'll try to post my program tonight if someone doesn't post a clue to my failure by then.

    G1Z-.2F5.
    X.463C.801
    X-.463C.801
    X-.925C0
    X-.463C-.801
    X.463C.801
    X.925C0
    X.463C.801
    G0Z.5

    Seems simple enough but cuts a slim diamond instead of a hex.
    Last edited by DMSentra; 12-08-2020 at 12:29 AM.

  9. #9
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    Quote Originally Posted by TeachMePlease View Post
    That is exactly how polar works

    On some controls, you actually program with an X and Y coordinate even. This is polar interpolation. You turn it on, program in X/Y (or X/C) for the feature you want, and the control does the math to make C and X work to create a Y axis.
    You have any idea why I'm getting a diamond shape instead of a hex? I've tried with and without re-stating the C values with no C movement. I've read yesterday I may need to double the C values and of course that only changed that movement. 3/4" end mill with spindle centerline set for it's offset value. The diamond is roughly 1" long and .2" wide. Tried G42 also.

  10. #10
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    308
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    92

    Default

    What size hex are you trying to make? The X and C values in the code you posted don't look right.

  11. #11
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    308
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    92

    Default

    OK, I just did some math, and you need to double your X numbers. Even with polar interpolation, you still need to program the X as if you're giving diameters. So, when the X point is 0.925" away from center, you need to tell it X1.85 .

  12. Likes TeachMePlease liked this post
  13. #12
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    The point values of the hex are X.925Y (C)0, X.463Y(C).801, and continued around using the appropriate + and - where needed.

  14. #13
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    I started with these values and doubled the C values per some posts when the originals wouldn't work. The weird thing is the diamond shape it cuts instead of a hex.

  15. #14
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    Ohhhh, so my modified C are right now but going radius values for X are not. I'll try that next then. Gracias.

  16. Likes wmpy liked this post
  17. #15
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    I have it cutting a hex finally. And the distance across the flats is correct. But, the flats are slightly convex, enough to make the distance across the points 1.797 instead of the correct 1.85. Seen this issue before?
    X1.85,C0/ X.926,C.801/ X-.926C.801/ X-1.85C0/ X-.926,C-.801/ X.926,C-.801/ X1.85,C0.

  18. #16
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    308
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    92

    Default

    Maybe you're feeding too fast? Try slowing the feed down and see if you get the same results.

    Are you using G41/G42 cutter compensation? If so, what value do you have for R on the offset page?

  19. #17
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    Quote Originally Posted by wmpy View Post
    Maybe you're feeding too fast? Try slowing the feed down and see if you get the same results.

    Are you using G41/G42 cutter compensation? If so, what value do you have for R on the offset page?
    Feed is slow enough it's hard to believe that's a problem. G41, and I forgot to even look at the R so that's next after the dinner break. Thanks.

  20. #18
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    All comp and T and R values were 0 so I tried several different things, only change was adding diameter to the part when changing the X comp.

  21. #19
    Join Date
    Dec 2011
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    308
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    92

    Default

    Some of the things you posted aren't quite adding up to me... You said, "3/4" end mill with spindle centerline set for it's offset value". That's good. The end mill should have an offset value in X such that when the center of the end mill is in line with the center of the spindle, it should be at zero.

    You said that the R value is at 0. Great. That's what I do. I only use it for compensation once the tool wears.

    But then, you said that you're expecting to measure the points at 1.85" as programmed. Here's where you're losing me. Since your R value is 0 in the offset, you need to compensate for the radius of the end mill in the program. I thought you were trying to make a 0.852" hex. That would be (0.801-0.375)*2. The 0.801 is the C position from the program. The 0.375 is the radius of the end mill. What size hex are you trying to make? If you're trying to make a 1.602" hex, then you need to re-figure your hex points as if it were a (1.602 + 0.750) hex.

    My guess is that you're looking for a 1.602" hex, didn't compensate for the end mill in the program, and got the machine to kind of cut to size by moving the X offset up so that the center of the tool is no longer zeroed at the center of the spindle. That would give some funky geometry like you're getting.

    I hope this helps. I suppose I could be way off base. If I am, and your program is good, then I would start looking for mechanical issues with the machine like loose belts on the spindle.

  22. #20
    Join Date
    Sep 2008
    Location
    Eugene Oregon
    Posts
    219
    Post Thanks / Like
    Likes (Given)
    3
    Likes (Received)
    11

    Default

    Let me say now this is my first go with C axis and so far it's a totally foreign critter. So I'm starting from scratch on this and what I'm doing may make little sense as I'm trying whatever might seem to be a solution.
    The size of the hex I'm working for is 1.85 ptp, 1.62 flat to flat. 2 points are on C0(Y0) for hex orientation, which is also something I may be doing wrong as I am starting from a program left in the control when I purchased the machine. No idea if the C orientation is right to cut the widest points on the X plane or I need to change that in the program too.
    I've since found out the X1.85 is not right, and am now on to X.926(2x the X vector of .463 to that point. I'm now at X.926C.801 for the point at 60deg, and cutting points to the left as I go. I just this second realized it's cutting CW with my programming going CCW around the hex.
    I am using g41 But no idea if the system is picking it up yet.
    Does that clear some of my mud?


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
  •