Trouble rigid tapping with FANUC 21-TB 2-axis lathe
Close
Login to Your Account
Likes Likes:  0
Results 1 to 10 of 10
  1. #1
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    55
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    8

    Default Trouble rigid tapping with FANUC 21-TB 2-axis lathe

    I am trying to use rigid tapping on my EMCO Turn 325. It has a FANUC 21-TB control.

    The manual for the machine says it does have rigid tapping (G84) and I can either set up parameter 5200, "bit 0" as a "0" and use a M29Sxxxx command prior to the G84 command or set "bit 0" to "1", do not use a M29, and have G84 as a default rigid tapping cycle.

    When I try either, I get the same result; the spindle turns at the commanded tapping speed, then attempts to stop at position, but slowly rotates back and forth for a few seconds and the control throws a time out error.

    Here is a simple program with "bit 0" set to 1 allowing G84 to function as a rigid tapping cycle:


    (TAP 1-72)
    N14 T0808
    N15 G54
    N16 M8
    N17 G98
    N18 M5
    N19 M20
    N20 G97 S1000 M3
    N21 G0 X0. Z0.15
    N23 G84 X0. Z-0.125 R0.15 P0 F13.88889
    N24 G80
    N25 Z0.15

    I have not had any problems with the machine otherwise and it does external threads fine, so I would imagine the spindle / encoder are fine.

    Any help is appreciated.

  2. #2
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,638
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1426

    Default

    Quote Originally Posted by jj80909 View Post
    I am trying to use rigid tapping on my EMCO Turn 325. It has a FANUC 21-TB control.

    The manual for the machine says it does have rigid tapping (G84) and I can either set up parameter 5200, "bit 0" as a "0" and use a M29Sxxxx command prior to the G84 command or set "bit 0" to "1", do not use a M29, and have G84 as a default rigid tapping cycle.

    When I try either, I get the same result; the spindle turns at the commanded tapping speed, then attempts to stop at position, but slowly rotates back and forth for a few seconds and the control throws a time out error.

    Here is a simple program with "bit 0" set to 1 allowing G84 to function as a rigid tapping cycle:


    (TAP 1-72)
    N14 T0808
    N15 G54
    N16 M8
    N17 G98
    N18 M5
    N19 M20
    N20 G97 S1000 M3
    N21 G0 X0. Z0.15
    N23 G84 X0. Z-0.125 R0.15 P0 F13.88889
    N24 G80
    N25 Z0.15

    I have not had any problems with the machine otherwise and it does external threads fine, so I would imagine the spindle / encoder are fine.

    Any help is appreciated.
    Hello jj80909,
    Many will not agree, as they have not in the past, but my Japanese Fanuc Colleagues are adamant that the correct method for turning the Spindle on is via the actual rigid tapping cycle and that the immediate previous use of the spindle, for drilling the tapping hole for example, should be stopped with M05 prior to the Rigid Tapping exercise. Having said this, it is to some degree MTB dependent, but normally, having the Rigid Tap Cycle start the spindle will work irrespective.

    Just for the purpose of testing, try the following:

    1. Set parameter bit 5200.0 and parameter 5210 to Zero
    2. Run the following program

    N14 T0808
    N15 G54
    N16 M8
    N17 G99
    N18 M5
    N19 M20
    N20 G0 X0. Z0.15
    N21 M29 S1000
    N23 G84 Z-0.125 R0.15 F0.01389
    N24 G80
    N25 Z0.15

    It will not be the cause your issue, but with all the lathes with rigid tapping via the Main Spindle (not live tooling), I've encountered, the max spindle speed is 1000rpm. This is due to the considerable inertia at play with even a relatively small Main Spindle Chuck.

    A rule of thumb, if the Lathe truly has Rigid Tapping on the Main Spindle, M19 will work to orientate the spindle irrespective of whether the machine has a "C" axis and live tools or not. This is also MTB dependent, but is normally the case.

    Regards,

    Bill

  3. #3
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    75
    Post Thanks / Like
    Likes (Given)
    209
    Likes (Received)
    33

    Default

    Just because the manual describes how to do rigid tapping it does not mean your machine has the option.
    And the program sample you posted you said it was with bit "0" set to 1 which means M29 should not be used.

    Anyway, if you can't do rigid tapping and have to use a floating tap holder then this is what you should try

    G54
    T808
    M8
    G99 (stop using G98 on a lathe)
    G97 S150 M3 (yes, 150rpm)
    G0 X0 Z.15
    G33 Z-.125 F0.01389
    M05
    Z.15 M4
    G0 Z.5
    G28 U0 W0
    M01

  4. #4
    Join Date
    Feb 2018
    Country
    DENMARK
    Posts
    145
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    100

    Default

    Many fanuc dosent use g80s cycles aswell. I ridget tap by reversing the spindel with m04. Never had problems with it and I've made small and big threads in all materials.

    Sendt fra min EML-L29 med Tapatalk

  5. #5
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    55
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    8

    Default

    angelw

    I tried your program:

    N14 T0808
    N15 G54
    N16 M8
    N17 G99
    N18 M5
    N19 M20
    N20 G0 X0. Z0.15
    N21 M29 S1000
    N23 G84 Z-0.125 R0.15 F0.01389
    N24 G80
    N25 Z0.15

    The program stops at line N21 and times out without starting the spindle.

    As for the other suggestions, I don't have a floating tap holder that will fit in this tiny lathe and I'd like to take advantage of rigid tapping if I can.

  6. #6
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,638
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1426

    Default

    Quote Originally Posted by jj80909 View Post
    angelw

    I tried your program:

    N14 T0808
    N15 G54
    N16 M8
    N17 G99
    N18 M5
    N19 M20
    N20 G0 X0. Z0.15
    N21 M29 S1000
    N23 G84 Z-0.125 R0.15 F0.01389
    N24 G80
    N25 Z0.15

    The program stops at line N21 and times out without starting the spindle.

    As for the other suggestions, I don't have a floating tap holder that will fit in this tiny lathe and I'd like to take advantage of rigid tapping if I can.
    Hello jj80909,
    Again with Parameter Bit 5200.0 set to Zero, run the following program (M29 Block Omitted):

    N14 T0808
    N15 G54
    N16 M8
    N17 G99
    N18 M5
    N19 M20
    N20 G97 S1000 M03
    N21 G0 X0. Z0.15
    N22 G84 Z-0.125 R0.15 F0.01389
    N23 G80
    N24 Z0.15

    If the above program runs, your machine doesn't have Rigid Tapping. Its common for a 2 axis lathe, without live tooling, not to have the G84 Canned Cycle. If a ps10 alarm is raised when attempting to run the above program, your control is not equipped with G84.

    Regards,

    Bill

  7. #7
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Colorado
    Posts
    55
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    8

    Default

    Hey Bill, I got it working. You only missed it by this much (M3).

    I had to add a M3 to the end of the G84 command. I doesn't make that much sense to me as it's a right-hand tapping cycle

    N14 T0808
    N15 G54
    N16 M8
    N17 G99
    N18 M5
    N19 M20
    N20 G97 S1000 M03
    N21 G0 X0. Z0.15
    N22 G84 Z-0.125 R0.15 F0.01389 M3
    N23 G80
    N24 Z0.15

    Thanks for the help!

  8. #8
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,305
    Post Thanks / Like
    Likes (Given)
    790
    Likes (Received)
    2310

    Default

    Was the manual you were using a Fanuc manual or an Emco manual? Needing the M3 on the G84 line has to do with how the machine builder's ladder logic is written, not a requirement of the Fanuc control. If you were using an Emco manual, I'm a bit surprised that the M3 was not shown to be required on the G84 line.

  9. #9
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    24,952
    Post Thanks / Like
    Likes (Given)
    5198
    Likes (Received)
    7719

    Default

    Quote Originally Posted by jj80909 View Post
    Hey Bill, I got it working. You only missed it by this much (M3).

    I had to add a M3 to the end of the G84 command. I doesn't make that much sense to me as it's a right-hand tapping cycle

    N14 T0808
    N15 G54
    N16 M8
    N17 G99
    N18 M5
    N19 M20
    N20 G97 S1000 M03
    N21 G0 X0. Z0.15
    N22 G84 Z-0.125 R0.15 F0.01389 M3
    N23 G80
    N24 Z0.15

    Thanks for the help!

    Other than the M3, what in your code is determining that it is RH?



    ----------------------------

    Think Snow Eh!
    Ox

  10. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,638
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1426

    Default

    Quote Originally Posted by jj80909 View Post
    Hey Bill, I got it working. You only missed it by this much (M3).

    I had to add a M3 to the end of the G84 command. I doesn't make that much sense to me as it's a right-hand tapping cycle

    N14 T0808
    N15 G54
    N16 M8
    N17 G99
    N18 M5
    N19 M20
    N20 G97 S1000 M03
    N21 G0 X0. Z0.15
    N22 G84 Z-0.125 R0.15 F0.01389 M3
    N23 G80
    N24 Z0.15

    Thanks for the help!
    Hello jj80909,
    Are you saying that the above gave you proper Rigid Tapping, with the assumption being that Parameter Bit 5200.0 is set to "1".

    Did the Spindle start with:

    N20 G97 S1000 M03

    then stop, synchronize and start again with:

    N22 G84 Z-0.125 R0.15 F0.01389 M3


    Regards,

    Bill


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
  •