Rigid tapping help


Page 1 of 3 123 LastLast
Results 1 to 20 of 41

Thread: Rigid tapping help

  1. #1
    Registered Genguy's Avatar
    Join Date
    Nov 2005
    Location
    Canada
    Posts
    83
    Downloads
    0
    Uploads
    0

    Default Rigid tapping help

    I can't get rigid tapping to work properly on an Oi mate-c.
    The problem is that after the tapping is complete, the machine hangs/stops and won't process any more blocks of code.
    It will complete all 4 of the hole locations perfectly then just hangs up.
    When it does this, I can hear the spindle motor making a slightly different sound than usual. I assume this is because of the M29.
    It's like it won't cancel the M29.
    I modified the code output by gibbs to get rigid tapping working in the first place.
    I need to get a working sample so we can get our post processor file modified.

    Any idea what I did wrong?

    G54
    S458M3
    G90G0X28.575Y15.875
    G43Z25.H9
    M8
    Z5.
    G94
    M29S458
    G84G99X28.575Y15.875Z-30.R5.F727.08
    Y-15.875
    X-28.575
    Y15.875
    G80G95
    G0Z5.
    M9
    G91G28Z0.
    M5
    M30
    %


    Similar Threads:


  2. #2
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Do you need the M3 and M5? Most machines start, stop, reverse and stop the spindle within the G84 logic.

    I'm not sure about the G94 and G95 either. If needed, you might try putting the G95 on a line by itself after the G80. I've never used those codes except on a lathe for changing from synchronous feed to asynchronous.

    Is M29 for gear shift override?

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  3. #3
    Registered cnc-king's Avatar
    Join Date
    Jul 2003
    Location
    united states
    Posts
    263
    Downloads
    0
    Uploads
    0

    Default

    M29 orients the spindle, are you sure you don't need a M80 instead of a M29
    you are not unlocking the spindle afterwards, i know the older fanucs require a M80 to initiate rigid tapping, I will post a tapping cycle from the older machines when i go to work in the am

    If you can ENVISION it I can make it


  4. #4
    Registered Genguy's Avatar
    Join Date
    Nov 2005
    Location
    Canada
    Posts
    83
    Downloads
    0
    Uploads
    0

    Default

    Thanks for the replies, I really appreciate your help.

    Quote Originally Posted by HuFlungDung View Post
    Do you need the M3 and M5? Most machines start, stop, reverse and stop the spindle within the G84 logic.
    Possibly not, I have not tried it without.
    Is M29 for gear shift override?
    The manual says M29 syncronizes the feed with the spindle rotation.
    I guess I should have mentioned it's on a 3 axis vertical mill.

    Quote Originally Posted by cnc-king View Post
    M29 orients the spindle, are you sure you don't need a M80 instead of a M29
    you are not unlocking the spindle afterwards, i know the older fanucs require a M80 to initiate rigid tapping, I will post a tapping cycle from the older machines when i go to work in the am
    The Fanuc manual also says the M29 is cancelled by any feed command such as G01 G00.

    Tommorow I'll try to move the codes around and also try an M80 instead of M29 like you guys have suggested.

    I'll scan that page of the manual and post it up as well. I have probably overlooked something.



  5. #5
    Member
    Join Date
    Mar 2006
    Location
    Australia
    Posts
    167
    Downloads
    0
    Uploads
    0

    Default

    Put in a speed/direction after the G80 line. Eg. S500 M3

    The manual should tell you this. BTW, M29 is correct for rigid tapping. If you use G84 without commanding M29 first, you need to use a floating tap holder, as the spindle and feed are not synchronised.

    regards, Oz



  6. #6
    Registered
    Join Date
    Mar 2005
    Location
    Silicon Valley, CA
    Posts
    988
    Downloads
    0
    Uploads
    0

    Default

    I'd like to know what you're cutting at a feed of F727.08 @ 458rpm??

    It's just a part..... cutter still goes round and round....


  7. #7
    Registered Genguy's Avatar
    Join Date
    Nov 2005
    Location
    Canada
    Posts
    83
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by psychomill
    I'd like to know what you're cutting at a feed of F727.08 @ 458rpm??
    That is what Gibbs came up with based on the thread pitch and rpm I entered. I let Gibbs recalculate the feed and rpm.The threads turned out fine, so I didn't mess with the settings. It was a 3/8" tap in 6061.

    Quote Originally Posted by Ozemale6t9
    If you use G84 without commanding M29 first, you need to use a floating tap holder
    Gibbs does exactly that (with the post I am using). Rigid shredding was the result.

    I'm going to try all of the suggestions tonight.

    Last edited by Genguy; 12-18-2006 at 08:47 PM.


  8. #8
    Member
    Join Date
    Mar 2006
    Location
    Australia
    Posts
    167
    Downloads
    0
    Uploads
    0

    Default

    Must have overlooked the feedrate...usually rigid tapping is programmed as thread lead(pitch).

    regards, Oz



  9. #9
    Registered
    Join Date
    Mar 2005
    Location
    Silicon Valley, CA
    Posts
    988
    Downloads
    0
    Uploads
    0

    Default

    You need to fix a few settings with your Gibbs. If you're tapping in G95 (IPR), then for a 3/8 tap (assuming its say a 3/8-16), your feed should only be F.0625 . Even as a programmed feed in IPM, at 458 rpm, your feed would still only be F28.625 .

    Something else I see is you're calling G95 at the end of the tap cycle with G80. You should get rid of the G95. Machine might be hanging up because you're placing it into IPR mode....

    Just a thought...

    It's just a part..... cutter still goes round and round....


  10. #10
    Member
    Join Date
    Mar 2006
    Location
    Australia
    Posts
    167
    Downloads
    0
    Uploads
    0

    Default

    Quote Originally Posted by psychomill View Post
    You need to fix a few settings with your Gibbs. If you're tapping in G95 (IPR), then for a 3/8 tap (assuming its say a 3/8-16), your feed should only be F.0625 . Even as a programmed feed in IPM, at 458 rpm, your feed would still only be F28.625 .

    Something else I see is you're calling G95 at the end of the tap cycle with G80. You should get rid of the G95. Machine might be hanging up because you're placing it into IPR mode....

    Just a thought...

    Feed per minute rate is spot on if the program is metric, which I assume it is because the tap would be going 55 inches if it is imperial (big machine). All the fanucs I deal with rigid tap in feed/rev mode, but the machine puts itself in that mode and goes back to feed/min mode upon G80.

    regards, Oz



  11. #11
    Registered
    Join Date
    Mar 2005
    Location
    Silicon Valley, CA
    Posts
    988
    Downloads
    0
    Uploads
    0

    Default

    I thought of metric after my post and saw that he's in Canada....

    but the machine puts itself in that mode and goes back to feed/min mode upon G80.
    I've never come across a FANUC parameter that controls that. Do you know? and for what version? I've seen FANUC based machines with a machine builder add-on on top of it that had parameters for it, just never on a FANUC stand-alone....

    It's just a part..... cutter still goes round and round....


  12. #12
    Registered Genguy's Avatar
    Join Date
    Nov 2005
    Location
    Canada
    Posts
    83
    Downloads
    0
    Uploads
    0

    Default

    I finally got a chance to play with this again today.
    I re-read the rigid tapping page in the programming manual and at the very bottom it says "Specify G84 for rigid tapping (parameter G84 No. 5200 #0 set to 1)".
    Since I have never messed with the parameters on this machine before I took a look at the parameter manual. The explanation for that bit is opposite of what the operators manual says.
    So I figured I would try that first and set bit 0 of parameter 5200 to 1 and give it another try.

    %
    ( OUTPUT IN ABSOLUTE MILLIMETERS )
    ( PARTS PROGRAMMED: 1 )
    ( FIRST TOOL NOT IN SPINDLE )
    N5G17G40G80
    N10T2
    N15M6
    ( OPERATION 2: HOLES )
    ( WORKGROUP )
    ( TOOL 2: 6. RIGID TAP )
    N20G54
    N25S1200M3
    N30G90G0X12.7Y0.
    N35G43Z25.H2
    N40M8
    N45Z5.
    N50G84G99X12.7Y0.Z-15.R5.F1200.
    N55X-12.7
    N60G80G0Z5.
    N65M9
    N70G91G28Z0.
    N75M5
    N80M30
    %
    That was an M6x1 in a fir 2x4, or maybe hemlock, not sure.

    Low and behold G84 works fine now without the M29. Woo Hoo progress!
    It still stalls at the R position after the last hole though.
    So next I tried moving the G28 up.
    N60G80G28G91X0Y0Z0
    This was shown as an example in the manual under canned cycle cancel.
    No change, same stall.

    This time I left the program running in auto and tried some diagnostics.
    On the screen that shows the active G&M codes the only one I noticed that changes when I reset the program is G26. The manual says G26 is "Spindle speed fluctuation detection on".
    That is as far as I got for today.



  13. #13
    Registered
    Join Date
    Mar 2005
    Location
    Silicon Valley, CA
    Posts
    988
    Downloads
    0
    Uploads
    0

    Default

    And you get no alarm messages when it "stalls"?? Have you tried running it in single block to see exactly which line it stalls on? The control lookahead may be hanging up on something else....

    It's just a part..... cutter still goes round and round....


  14. #14
    Member HuFlungDung's Avatar
    Join Date
    Mar 2003
    Location
    Canada
    Posts
    4826
    Downloads
    0
    Uploads
    0

    Default

    Try removing the M3.
    Since the G84 itself should issue an M3 and and M4 for every hole, I wonder if there is some kind of spindle rotation status check built into the ladder logic which might not accommodate the non-rotation condition of the spindle when the G84 completes, since M3 was the commanded status before the cycle was called. I dunno.

    First you get good, then you get fast. Then grouchiness sets in.

    (Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)


  15. #15
    Registered Genguy's Avatar
    Join Date
    Nov 2005
    Location
    Canada
    Posts
    83
    Downloads
    0
    Uploads
    0

    Default

    No error. It stalls on the line with the G80 in it.
    It seems to be processing it because I tried adding in a G25 on that line and it complains with an error.

    I tried removing the M03 line and it gives the error "illegal s command".

    It seems like it's dwelling but there is no dwell command.



  16. #16
    Registered
    Join Date
    Nov 2005
    Location
    Australia
    Posts
    70
    Downloads
    0
    Uploads
    0

    Default

    Hi
    We had troubles with rigid tapping also on our lathe, manual said use M12 to engage. After looking at the parameters and speaking to fanuc rep we need to use M112. I think the parameter number is around 6700, but once again it is on my lathe, could perhaps something similar be happening as mine do dwelled but was before the cycle as my m-code was incorrect.

    Cheers



  17. #17
    Registered
    Join Date
    Mar 2005
    Location
    Silicon Valley, CA
    Posts
    988
    Downloads
    0
    Uploads
    0

    Default

    No error. It stalls on the line with the G80 in it.
    It seems to be processing it because I tried adding in a G25 on that line and it complains with an error.
    You can't put the G25 on the same line as a G80. Try putting it in before you tap. Make sure its on a line (might even need to be by itself) before the G84 line and before the M29.....

    It's just a part..... cutter still goes round and round....


  18. #18
    Registered
    Join Date
    Jan 2005
    Location
    Finland
    Posts
    2
    Downloads
    0
    Uploads
    0

    Default

    Hi
    Don’t let M29 away, it synchronises spindle to the axis.
    Without M29 it is ordinary G84 block.
    I am pretty sure the problem is G95 with G80

    Try to edit your original program something like this

    G54
    G90G0X28.575Y15.875
    G43Z25.H9
    M8
    G94
    M29S458
    G84G99Z-30.R5.F727.08
    Y-15.875
    X-28.575
    G98Y15.875
    G80M9
    G91G28Z0.
    M5
    M30

    Jukka



  19. #19
    Member
    Join Date
    Dec 2006
    Location
    USA
    Posts
    51
    Downloads
    0
    Uploads
    0

    Default

    I haven't noticed it mentioned so I'll add it here.
    On some Fanucs, then M29 is used for Rigid Tap, and it is Canceled by using the M28.

    Since you changed the Parameter 5200 this may no longer be required.

    Try Changnig 5200 back.

    Use the M29 as before

    After the last Hole

    use

    G80M28



  20. #20
    Registered
    Join Date
    Dec 2006
    Location
    Indiana
    Posts
    84
    Downloads
    0
    Uploads
    0

    Default

    With parameter 5200 set to 1 it tells the machine not to use an M code to go into rigid tapping mode. 0 will have it use an M code. If your machine programming manual says M29 activates rigid tap, check parameter 5210 and verify that the value is 0. 5210 is rigid tapping specification M code. A setting of 0 defaults to 29. Verify that parameter 5212 is set to 29. 5212 is the M code that specifies a rigid tapping mode.

    If you have 5200 set to 0 so that an M code is used, 5210 set to 0, and for some reason 5212 is another value it will confuse the machine when it tries to initialize and cancel.

    As far as using an M code to cancel M29 I've never heard of that. G80 should cancel it as the M29 becomes part of the G84 cycle. I guess it is possible the builder could have put something goofy like that in the ladder, and your M29 is staying latched up.

    Go into the logic, select search, type in M29 and press the WSRCH softkey.
    Once you find the write coil, go back to the mdi screen and type m29, and go back to the ladder and press cycle start. The write coil should latch up.
    Jump back to mdi, and type g80, back to the logic, cycle start. The coil should drop out. If it doesn't they've got something else in their keeping it latched. If that's the case, search for an M29 write coil again and look for a reset coil. (R) You'll have to use whatever they are using to reset it to cancel rigid tap.

    What is parameter 5200 bit 2 set as?



Page 1 of 3 123 LastLast

Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

Rigid tapping help

Rigid tapping help