Results 1 to 6 of 6

Thread: Fanuc OT, wanna flipflop & workshift Z-.060"

  1. #1
    Join Date
    Apr 2012
    Location
    Huntsville,Texas
    Posts
    3
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Fanuc OT, wanna flipflop & workshift Z-.060"

    This 1997 Femco turning center (HL-40) uses Fanuc OT. The part is 9" long and each end is a different turned profile, 5 tools each end. The idea is to M00 in the middle of the program, flip the part and machine the other end. Sure, I could write the second half of the program an extra .06" negative in all Z moves, but certainly there exists a better method. I'm not convinced that the OT supports G54 or G52. Those codes are not listed in the manual's G-code list. I do use an M98 & M99 subroutine on another job, but that seems overkill for a simple (ha ha) Z workshift. I tried G50 Z-.060 S2000 on the first tool after the M00 but that moved the Z about 8" toward the tailstock. I tried a G52 and a G54 after the G50 and instead of the G50 only to receive an Alarm #10 - "unusable G-code command".

  2. #2
    Join Date
    Jan 2012
    Posts
    348
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: Fanuc OT, wanna flipflop & workshift Z-.060"

    Quote Originally Posted by DanTexas View Post
    This 1997 Femco turning center (HL-40) uses Fanuc OT. The part is 9" long and each end is a different turned profile, 5 tools each end. The idea is to M00 in the middle of the program, flip the part and machine the other end. Sure, I could write the second half of the program an extra .06" negative in all Z moves, but certainly there exists a better method. I'm not convinced that the OT supports G54 or G52. Those codes are not listed in the manual's G-code list. I do use an M98 & M99 subroutine on another job, but that seems overkill for a simple (ha ha) Z workshift. I tried G50 Z-.060 S2000 on the first tool after the M00 but that moved the Z about 8" toward the tailstock. I tried a G52 and a G54 after the G50 and instead of the G50 only to receive an Alarm #10 - "unusable G-code command".
    Hi Dan,
    As a P/S10 alarm is raised when G52 and G54 is commanded, your control does not support Work Shift via G Code (G54 - G59). This is typical of the early 0 Series control. As you don't mention that you use G50 to generally set the Coordinate System, most likely your control has the APRS bit of parameter 0010 set.

    You can shift the Coordinate System of your machine with the following command.

    G50 U_ W_

    The above command will shift the coordinate system as follows
    X+U, Z+W
    Accordingly, after the M00, at which point the workpiece is reversed, the above command will be executed. Obviously, you will only need to include the W address, as the X should remain unchanged, G50 W-0.06. Be certain that the opposite of the Work Shift executed after the M00 is executed before the program restarts from the beginning to machine the first end. Probably program this just prior to the M30 as follows:
    G50 W0.06
    M30

    If you happen to abort the program after the G50 W-0.06, but before G50 W0.06 is executed, and then restart the program from the beginning, the coordinate system will be out of position with respect to the first operation by 0.06 in Z. If the APRS bit of parameter 0010 set, you should be able to just execute a manual Reference Return to set things straight if you get lost

    Regards,

    Bill

  3. #3
    Join Date
    Apr 2012
    Location
    Huntsville,Texas
    Posts
    3
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Fanuc OT, wanna flipflop & workshift Z-.060"

    Thanks, Bill for the very clear explanation. I've read somewhat about the G50 code. For this system, the G50 seems used only to set the maximum spindle speed allowed. I will try your suggestions tomorrow and report in.

    Dan

  4. #4
    Join Date
    Jan 2012
    Posts
    348
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: Fanuc OT, wanna flipflop & workshift Z-.060"

    Quote Originally Posted by DanTexas View Post
    Thanks, Bill for the very clear explanation. I've read somewhat about the G50 code. For this system, the G50 seems used only to set the maximum spindle speed allowed. I will try your suggestions tomorrow and report in.

    Dan
    Hi Dan,
    G50 has a dual purpose with a lathe control. When used in conjunction with an S address it sets the maximum spindle speed when Constant Surface Speed (G96) is used, and when used with Absolute Axes addresses, it sets the coordinate system.
    Regards,
    Bill

  5. #5
    Join Date
    Apr 2012
    Location
    Huntsville,Texas
    Posts
    3
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: Fanuc OT, wanna flipflop & workshift Z-.060"

    I've been turning parts successfully, thanks. Instead of a .060" shift, I opted for a .025" shift, which was plenty to face off. This is a screen shot that I've re-typed here. Routines 100 through 500 were of the first end of the part prior to the flip of the part in the chuck.
    N536M00 (stop the chuck and flip the part end for end)

    N601G00X9.0Z8.0 (position for safe turret rotation)
    N602G50S2000 (speed only, as far as I can tell)
    N603G00T0101 (call up tool #1)
    N604G96S600M03
    N605G00X2.1Z1.0 (close in on the part, without coolant)
    N606Z.1M08 (getting close first was helpful with the math)
    N607G50 Z .125 (Z shift of .025)
    (we know that the tool is sitting at Z.1 but the program thinks it is sitting at Z.1 plus .025)
    N608G01Z0F.010 (program moves tool .125 toward chuck, calls it zero)
    ...
    N901G00X9.0Z8.0 (positioning for final tool call)
    ...
    /N907G71U.025R.04 (add a Block Delete on 3 lines only)
    /N908G71P909Q916 (B.D. allowed for a rework pass, if needed)
    ...
    N917G70P909Q916 (finish pass)
    N918 G00Z.1 (program thinks this is .1 but it is really .075)
    /N919G50Z.075(unShift Z of .025, .025 plus .075 = .1)
    N920G00X9.0Z8.0M09
    N921 T0500 (best not to place this on line N920)
    N922M30

    If I choose to run tool block 900 repeatedly, I should not unShift Z multiple times, hence the block delete (/) at N919.

    I did get lost a time or two re-working a part, so I did as Angel suggested; I simply went to machine zero and then canceled-out U and W. If you don't, the tools will creep away from the work by .025 each cycle.
    Thanks for the help, Angel and thanks for this site.
    Dan

  6. #6
    Join Date
    Jan 2012
    Posts
    348
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: Fanuc OT, wanna flipflop & workshift Z-.060"

    Quote Originally Posted by DanTexas View Post
    I've been turning parts successfully, thanks. Instead of a .060" shift, I opted for a .025" shift, which was plenty to face off. This is a screen shot that I've re-typed here. Routines 100 through 500 were of the first end of the part prior to the flip of the part in the chuck.
    N536M00 (stop the chuck and flip the part end for end)

    N601G00X9.0Z8.0 (position for safe turret rotation)
    N602G50S2000 (speed only, as far as I can tell)
    N603G00T0101 (call up tool #1)
    N604G96S600M03
    N605G00X2.1Z1.0 (close in on the part, without coolant)
    N606Z.1M08 (getting close first was helpful with the math)
    N607G50 Z .125 (Z shift of .025)
    (we know that the tool is sitting at Z.1 but the program thinks it is sitting at Z.1 plus .025)
    N608G01Z0F.010 (program moves tool .125 toward chuck, calls it zero)
    ...
    N901G00X9.0Z8.0 (positioning for final tool call)
    ...
    /N907G71U.025R.04 (add a Block Delete on 3 lines only)
    /N908G71P909Q916 (B.D. allowed for a rework pass, if needed)
    ...
    N917G70P909Q916 (finish pass)
    N918 G00Z.1 (program thinks this is .1 but it is really .075)
    /N919G50Z.075(unShift Z of .025, .025 plus .075 = .1)
    N920G00X9.0Z8.0M09
    N921 T0500 (best not to place this on line N920)
    N922M30

    If I choose to run tool block 900 repeatedly, I should not unShift Z multiple times, hence the block delete (/) at N919.

    I did get lost a time or two re-working a part, so I did as Angel suggested; I simply went to machine zero and then canceled-out U and W. If you don't, the tools will creep away from the work by .025 each cycle.
    Thanks for the help, Angel and thanks for this site.
    Dan
    Hi Dan,
    Did to actually try G50 W-0.025 (or whatever the shift needs to be)? Using this method allows the shift to occur anywhere, and there's no math whatsoever involved. If the APRS bit of parameter 0010 is set, and I suspect that it is, making the Shift with G50 W_ is the correct way of doing so.

    Thanks for coming back the Forum and reporting your result. If often helps others following a Thread to know of the outcome.

    Regards,

    Bill
    Last edited by angelw; 05-12-12 at 06:22 AM.

Similar Threads

  1. Replies: 8
    Last Post: 05-08-13, 03:14 PM
  2. Mits FA20 WEDM "EC" or "CS" setting
    By DoubleLunger in forum Programming / Applications
    Replies: 0
    Last Post: 04-19-10, 04:12 PM
  3. Robodril Fanuc α-T21i FL "Help"
    By cedares in forum Machine Repair & Troubleshooting
    Replies: 1
    Last Post: 03-24-10, 11:00 PM
  4. Replies: 1
    Last Post: 11-29-09, 10:44 PM
  5. Danichi 152 :fanuc 15T "OT007 z + overtravel (Hard) alarm" can't RESET.
    By jlpd in forum Machine Repair & Troubleshooting
    Replies: 0
    Last Post: 11-22-09, 09:58 AM

Posting Permissions

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