Page 1 of 2 12 LastLast
Results 1 to 20 of 21
  1. #1
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    410

    Default Fanuc 18i TA G84 & rigid tapping

    Im looking for some input for tapping with a live tool lathe. Fanuc 18i TA

    The machine has C axis & Rigid Tapping enabled,

    I am trying to use G84 canned cycle on the main spindle holding the tap in a regular solid holder, and the machine is not having it.

    Here are some of the way I have tried: Machine alarms out.


    G97
    M68 S250 <-------m68 = m29 on this machine
    G84 Z-.95 R0. F.05
    G80

    G97
    G84 Z-.95 R0. F.05
    G80

    S150M3
    G97
    G84.2 Z-.95 R0. F.05
    G80

    Has anyone else had a hard time trying to accomplish what this machine is doing at the 1:30 mark
    cnc lathe coupling rigid tapping - YouTube

    Dan-

  2. #2
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,657

    Default

    Quote Originally Posted by solidworkscadman View Post

    I am trying to use G84 canned cycle on the main spindle holding the tap in a regular solid holder, and the machine is not having it.

    Here are some of the way I have tried: Machine alarms out.

    Dan-
    Hi Dan,
    What alarm are you getting? Rigid tapping on the Main Spindle is available as an option, even when the machine doesn't have a "C" axis and live tooling. If the machine is able to execute an M19 command to orientate the spindle, not via the "C" axis but with the general drive when "C" is not invoked, then it will have rigid tapping on the main spindle.

    There are a couple of parameters that have to be set that aren't in the general parameter list; I think in the 2000 series parameters, but I'm only going by memory. These parameters are to tune the spindle for use with rigid tapping. I did one about a year ago, and I do recall that the maximum RPM allowed was only 1000. However, even without these parameters being tweaked, the machine/control still went though the motions without alarm, just that the spindle and Z slide wasn't in synch during the deceleration/acceleration phase.

    I'll dig back and see if I can find the parameter numbers, but do come back with the alarm number.

    Regards,

    Bill

  3. #3
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    410

    Default

    Hi Bill,

    I do not know the alarm that was thrown off hand, I will check it out tomorrow and respond back.

    Thanks for looing into it!

    I may have the parameter to enable the main spindle orientation, would this be the only other option parameter to enable g84?

    The machine does have canned cycle ex. g83 already.

    Thanks,
    Dan-

  4. #4
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,657

    Default

    Quote Originally Posted by solidworkscadman View Post
    Hi Bill,

    I do not know the alarm that was thrown off hand, I will check it out tomorrow and respond back.

    Thanks for looing into it!


    I may have the parameter to enable the main spindle orientation, would this be the only other option parameter to enable g84?

    The machine does have canned cycle ex. g83 already.

    Thanks,
    Dan-
    Hi Dan,
    Does the G83 cycle actually operate using the Main Spindle? As your machine has live tooling, these cycles will be available for the live tooling.

    I'm suspecting that the alarm you get with the G84 cycle being used with the main spindle is associated with the "C" axis not being engaged. Rigid tapping with the Main Spindle is an Option, and given that Main Spindle orientation isn't turned on indicates that the control probably doesn't have this option.

    Rigid Tapping with the Main Spindle, when the machine has live tooling, usually has a different "G" code as well. Okuma is the same. You will be able to determine how Rigid Tapping has been implemented via the PLC ladder.

    Regards,

    Bill

  5. #5
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,876

    Default

    Are you missing G99?


    N5T909(M8 X 1.25 TAP)
    X0Z.1Y0S100M8
    M29S200
    G84G99Z-.55F.049
    G80
    G98
    M9

    M29 is "Rigid Tapping Mode" on my 18iT

    Also - it is ass_u_med that the spindle was already running in M3 before this copy/paste.
    Otherwsie you want to add an M3 in there as well.

    The same code with an M4 will tap LH.



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

    Little 18i T&A ???
    Ox
    Last edited by Ox; 11-18-2013 at 12:29 PM. Reason: added a wee bit more

  6. #6
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,657

    Default

    Quote Originally Posted by solidworkscadman View Post

    G97
    M68 S250 <-------m68 = m29 on this machine
    G84 Z-.95 R0. F.05
    G80

    G97
    G84 Z-.95 R0. F.05
    G80

    S150M3
    G97
    G84.2 Z-.95 R0. F.05
    G80

    Has anyone else had a hard time trying to accomplish what this machine is doing at the 1:30 mark
    cnc lathe coupling rigid tapping - YouTube

    Dan-
    Hi Dan,
    With regards to specifying Rigid Tapping with M68 instead of M29, this can only be the case if a number other than "0" or "29" is registered in parameter 5210. The number can be in the range of 0 to 255. If "0" then the default of M29 is used, and registering "29" is obviously superfluous, as M29 is the default.

    Take a look in parameter 5210 for the existence of the number 68. If it doesn't appear, then M29 will be the correct "M" code, and M68 may have been implemented by the MTB for rigid tapping via the live tooling.

    Regards,

    Bill

  7. #7
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,876

    Default

    M68 on mine is a feature related to running as dual path, so if this one aint dual path, then the 68 could be used to distinguish between main spindle and live tooling as Bill says.

    ???


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

    Think Snow Eh!
    Ox

  8. #8
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    410

    Default

    Quote Originally Posted by angelw View Post
    Hi Dan,
    Does the G83 cycle actually operate using the Main Spindle? As your machine has live tooling, these cycles will be available for the live tooling.

    I'm suspecting that the alarm you get with the G84 cycle being used with the main spindle is associated with the "C" axis not being engaged. Rigid tapping with the Main Spindle is an Option, and given that Main Spindle orientation isn't turned on indicates that the control probably doesn't have this option.

    Rigid Tapping with the Main Spindle, when the machine has live tooling, usually has a different "G" code as well. Okuma is the same. You will be able to determine how Rigid Tapping has been implemented via the PLC ladder.

    Regards,

    Bill
    Hi,
    Yes, G83 does work on main spindle.
    Alarm is #197 = 197 - C-AXIS COMMANDED IN SPINDLE MODE
    Here is the description in the book
    "The program specified a movement along the Cs-axis when the signal CON(DGN=G027#7) was off. Correct the program, or consult the PMC ladder diagram to find the reason the signal is not turned on."

  9. #9
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    410

    Default

    Quote Originally Posted by Ox View Post
    Are you missing G99?



    I have tried with g99 within and before the g84 command,

    I have also tried to throw the m29, and just for the hell of it made the spindle turn G97
    s100 m3
    M68 S250
    G99 G84 Z-.95 R0. F.05
    G80

    no go

  10. #10
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,876

    Default

    What if you stop your main spindle and fire your live tool in reverse (fwd for a face tool) and see if it will cycle the code that way.

    ???

    It may require (for safety's sakes) that you are in C axis and have C programmed to some value to act as a brake for off center working.

    ???



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

    Think Snow Eh!
    Ox

  11. #11
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,657

    Default

    Quote Originally Posted by solidworkscadman View Post
    Hi,
    Yes, G83 does work on main spindle.
    Alarm is #197 = 197 - C-AXIS COMMANDED IN SPINDLE MODE
    Here is the description in the book
    "The program specified a movement along the Cs-axis when the signal CON(DGN=G027#7) was off. Correct the program, or consult the PMC ladder diagram to find the reason the signal is not turned on."
    Its as I suspected and is related to the "C" axis not being engaged. As suggested in my last Post, check parameter 5120 for the existence of the number 68. If it doesn't exist, then M68 will be implemented via the PLC (PMC in Fanuc talk). Its common for the control NOT to have Rigid Tapping on the Main Spindle when the machine is equipped with Live Tooling, as its a separate option.

    If you find where the CON signal is being turned on in the PMC (search for G027.7 in address mode), most probably by the "C" axis being engaged, then you may be able to fairly easily add an "OR" rung that tests True with another "M" code to turn the signal on .

    Quote Originally Posted by solidworkscadman View Post
    I have tried with g99 within and before the g84 command,

    I have also tried to throw the m29, and just for the hell of it made the spindle turn G97
    s100 m3
    M68 S250
    G99 G84 Z-.95 R0. F.05
    G80
    Omitting G98 or G99 is irrelevant with regards the the cycle actually executing. These are Group 10 "G" codes and relate to whether the tool returns to the Initial or "R" plane on completion of the cycle. G98 is the default when power is first turned on, and will revert to this state if G99 has been executed and the control Reset. Accordingly, if G99 is omitted, G98 is assumed by the control.

    You most definitely have to use G97 with Main Spindle tapping, Rigid or otherwise.

    Regards,

    Bill

  12. #12
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,876

    Default

    You are mixing up "milling" in this.

    G98/G99 here is feed time/rev

    He is actually using an "R" of 0 in his code, but it wouldn't be needed as 0 is the default.


    BTW - I too would have been in G97 for sure.
    (just not shown in my code sample)


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

    Think Snow Eh!
    Ox

  13. #13
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,657

    Default

    Quote Originally Posted by Ox View Post
    You are mixing up "milling" in this.

    G98/G99 here is feed time/rev

    He is actually using an "R" of 0 in his code, but it wouldn't be needed as 0 is the default.


    BTW - I too would have been in G97 for sure.
    (just not shown in my code sample)


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

    Think Snow Eh!
    Ox
    Hi Ox,
    You're quite correct, I was thinking machining centre. However, it probably still applies in the same way though. When a machine has Live Tooling, and all the general canned cycles common to machining centres are available, then "G" Code System "B" normally applies, as there are no return to Initial, or "R" plane "G" codes in System "A". In the case of "G" Code System "B", a "G" code Group 11 exists which is G98/99, and G94/95 from Group 05 specify Feed per Minute and Feed per Rev respectively.

    Regards,

    Bill

  14. #14
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    410

    Default

    Quote Originally Posted by angelw View Post
    Hi Dan,
    With regards to specifying Rigid Tapping with M68 instead of M29, this can only be the case if a number other than "0" or "29" is registered in parameter 5210. The number can be in the range of 0 to 255. If "0" then the default of M29 is used, and registering "29" is obviously superfluous, as M29 is the default.

    Take a look in parameter 5210 for the existence of the number 68. If it doesn't appear, then M29 will be the correct "M" code, and M68 may have been implemented by the MTB for rigid tapping via the live tooling.

    Regards,

    Bill
    number 68 is in the 5210 paramater

    Also I am not able to use M19 in the lathe.
    Parameter "spindle index" 9930 bit 1. would enable me to use this. Then a will have to create a separate m code for Main spindle rigid tapping

  15. #15
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    410

    Default

    Ox, I am trying to use my main spindle to rigid tap, while holding the tap in a collet not a live tool holder.

    Rigid tapping with live tools are run successfully for both face, and o.d.

    Thanks for the input!

  16. #16
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,657

    Default

    Quote Originally Posted by solidworkscadman View Post
    number 68 is in the 5210 paramater

    Also I am not able to use M19 in the lathe.
    Parameter "spindle index" 9930 bit 1. would enable me to use this. Then a will have to create a separate m code for Main spindle rigid tapping
    Hi Dan,
    As stated in my first Post, being able to execute M19 with the Main Spindle is normally a good indicator if the Machine is capable of Rigid Tapping with that spindle. If you can set the 9930.1 bit and successfully execute M19 with the Main Spindle, then you may be able to work through this and get Rigid Tapping on the Main Spindle.

    Does G84 (but without M68) work at all with the Main Spindle? It very likely that G027.7 is being set to logic "1" by the code to engage the "C" axis. You could test this out by observing G027.7 in the Diagnostic pages, when invoking and cancelling "C" axis mode. M68 is likely to be the code that's causing 197 alarm.

    Regards,

    Bill

  17. #17
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,876

    Default

    Quote Originally Posted by solidworkscadman View Post
    Ox, I am trying to use my main spindle to rigid tap, while holding the tap in a collet not a live tool holder.

    Rigid tapping with live tools are run successfully for both face, and o.d.

    Thanks for the input!

    Yes - I understand that, and I am pretty sure that the code that I posted is from a holed tapped on C/L. But as I was looking through the book on G84, all examples were shown as live tool off center.

    Near as I can figger, the only code changes between the two would be which S is turning?
    Well - I guess in your case it must be M68 instead of M29 for live tools?

    Just thought it worth trying the live tool and see what you get - and you apparently already have done that, so - I guess that works.


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

    Think Snow Eh!
    Ox

  18. #18
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    410

    Default

    Quote Originally Posted by angelw View Post
    Does G84 (but without M68) work at all with the Main Spindle? It very likely that G027.7 is being set to logic "1" by the code to engage the "C" axis. You could test this out by observing G027.7 in the Diagnostic pages, when invoking and cancelling "C" axis mode. M68 is likely to be the code that's causing 197 alarm.

    Regards,

    Bill
    G84 does not work even on its own,

    It throws the 197 alarm without the m68 or m29.

    Thank for the heads up on the G027.7 I will be looking into this tomorrow!

  19. #19
    Ox's Avatar
    Ox
    Ox is offline Diamond
    Join Date
    Aug 2002
    Location
    West Unity, Ohio
    Posts
    17,876

    Default

    Doo you have a sub spindle on this thing?

    M68 on my machine is "swap spindle commands" or something like that.
    If I had keyed that in on mine, and then tried to run in G99 on the main spindle, I think mine would prolly just sit there waiting to see some movement on the "other spindle".
    That is pretty much for a dual path unit, but .... ??? Maybe a single path with a sub spindle might use it as well?

    M69 cancels it of course....

    Since you have 68 in that param, I ??? how this all would effect it, but just thought that I would mention it.


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

    Think Snow Eh!
    Ox

  20. #20
    angelw is online now Stainless
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    1,657

    Default

    Quote Originally Posted by solidworkscadman View Post
    G84 does not work even on its own,

    It throws the 197 alarm without the m68 or m29.

    Thank for the heads up on the G027.7 I will be looking into this tomorrow!
    Hi Dan,
    In this case, check bit "1" of parameter 5200. Its likely to be set to 1, meaning that Rigid Tapping is called via G84 and NOT an "M" code. The M68, as Ox suggests, may be a code to swap spindles (in this case to the Live Tool spindles). But the fact that 68 is registered in parameter 5210 doesn't point to that. What does it say in your manual with regards to M68?

    Whats going on can be determined from the PLC Ladder, and the G027.7 address would be a good place to start. If parameter bit 5200.1 is not set to 1, but 0, then the fact that you get the 197 alarm indicates that G84 is linked to the "C" axis / Live Tools, via the PLC.

    Regards,

    Bill

Page 1 of 2 12 LastLast

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
  •