584,817 active members*
5,215 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Hardinge Lathes > Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)
Results 1 to 11 of 11
  1. #1
    Join Date
    Sep 2010
    Posts
    196

    Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    Sorry guys, this is kind of a noob question, but in the Hardinge Conquest T42 Programmer's manual under section 16, page 16-19 it shows an example of transferring a part from the sub-spindle to the main spindle.

    In this example, it shows setting two work offsets - the first G10 sets the Z axis (which works as expected), and the second G10 sets the sub-spindle work offset. This is so that you can command both relative to the zero-offset of the part being produced. Makes sense this way.

    Code:
    N84 (TRANSFER TO MAIN) ; Sequence Number and Operator Message
    G10 P0 Z-1.75 ; Main Spindle Work Shift
    G10 P0 Y-1.75 ; Sub-Spindle Work Shift for Workpiece Transfer
    G97 S2500 M14 ; Main Spindle 2500 RPM Reverse
    M98 P1 ; Call Safe Start Program O1
    M32 ; Sub-Spindle Sync to Main Spindle
    M21 ; Main Spindle Collet Open
    M36 ; Main Spindle Air Blast ON
    G0 Y-1. ; Rapid Part 1" into Main Spindle (Figure 16.16)
    M67 ; Sub-Spindle Axis Drive to Low Torque Mode
    G4 U.2 ; Dwell .2 Seconds
    M22 ; Main Spindle Collet Close
    G4 U.2 ; Dwell .2 Seconds
    M37 ; Main Spindle Air Blast OFF
    M56 ; Sub-Spindle Collet Open
    G4 U0.5 ; Dwell .5 Seconds
    M66 ; Sub-Spindle Axis Drive OFF
    M68 ; Sub-Spindle Axis Drive to Normal Torque Mode
    G53 Y# 5024 ; Y Axis Position Verification
    G28 V0. ; Rapid Sub-Spindle to Home Position (Figure 16.17)
    M1 ; Optional Stop
    Except... G10 P0 Y-1.75 doesn't seem to have an effect. The sub-spindle moves in absolute coordinates regardless of the work-shift offset I choose.

    I tested this using
    G10 P0 Z-5.0
    G10 P0 Y-5.0
    G0 Z0
    G0 Y5

    and both the turret and the face of the sub-spindle line up at 5" from the main spindle. This should have placed the Y-axis (the sub-spindle) 5" further out (that is, 10" from the main spindle nose.)

    Why does the Z work offset function correctly, but not the Y-axis? Can any of you provide a sub-spindle transfer example that you know works?


    Torin...

  2. #2
    Join Date
    May 2016
    Posts
    526

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    Why dont you program it using long hand using incremental values ?
    Then you can move to eject the part

  3. #3
    Join Date
    Mar 2017
    Posts
    314

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    What is this? Is there an offset besides workshift for the sub spindle? All the machines I have ran with a sub spindle have an offset for that axis.
    G53 Y# 5024 ; Y Axis Position Verification

  4. #4
    Join Date
    Sep 2010
    Posts
    196

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    Yes, on my Hardinge T42 there is an additional "Workshift" offset for each of the axes in the workshift offsets page (shown below) that is different from G53, and G54 through G59. The so-called "5024 position verification" is used for verifying the location of the spindle after returning from low torque mode. I don't know why they do it this way.

    But getting back on topic...

    The G0 P0 X_ Y_ Z_ command is a convenience function (on the T42 anyway) for setting a work shift offset for each of the axes. That way, both the turret and sub-spindle can reference the same location instead of calculating absolute positions. This is actually very convenient... if only it would work.

    I've added a pair of photos to illustrate the problem. In photo #1, I use MDI to use the G10 P0 command to set the work-shift offset for both Z (my turret) and Y (my sub-spindle).

    Attachment 391478

    In photo #2, you can see in Settings->Page Right->Page Right->WRKSHFT page that the Z offset has taken hold as expected, but the Y workshift has not. Something is preventing the G10 P0 from overwriting this value, and I want to know why. I can overwrite it manually on this page... but not programmatically. Why does it work for Z and not Y?

    Attachment 391476

    Hopefully this answers mbservice's question too; the manual says it can, but reality demonstrates otherwise, and I want to know why. Perhaps there is some other parameter blocking the Y workshift from being set? I don't know.

  5. #5
    Join Date
    Mar 2017
    Posts
    314

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    G10 Px is just generic "write to this spot" command. It is not a Hardinge thing.

    I asked about the G53 because lathes the have workshift usually dont also have work offsets G53-59 Hardinge maybe using that for your in position check.

    Does it have a work offset register? G54-59 If yes does it have a Y field?

  6. #6
    Join Date
    Sep 2010
    Posts
    196
    Quote Originally Posted by generaldisarray View Post
    G10 Px is just generic "write to this spot" command. It is not a Hardinge thing.
    Agreed. G10 P0 is a generic write parameter function, but it usually takes an L argument as well.

    I tried with L2, and it correctly wrote to the Y register but not in he workshift file. Instead it wrote to the Common (G53) Offsets file. Yes, the Hardinge has both a “workshift” file, and also has G53 through G59. They all have XYZCA and one other axis name I can’t remember at the moment.

    Hardinge, I think uses the standalone P0 in a proprietary way, modifying a work shift file. Well... for Z anyway.

  7. #7
    Join Date
    Mar 2017
    Posts
    314

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    problem solved
    jog your Y to where you want your zero to be and put that into your g54. Then call it in the program g0 g54 y0.
    Here is an example for a Mori NLX that is using the top of the sub chuck jaws or collet and the face of the part as the zero point. You can also call the gripping position zero if you would rather.
    That workshift is old school. G54 acomplishes the same thing but cleaner.I have seen that in Hardinge books before. Recommending to use G50 and stuff that is more complicated than it needs to be.
    I use this at the top of the program so the data is always relevant and present for the next setup

    (MORI-3 OFFSETS)
    (54)
    G10L2P1Z-8.6C0.B-20.2725
    (55)
    G10L2P2Z6.157C0.


    N60(TRANSFER \ CUT OFF)
    (CHECK TOOL NUMBER AND SPINDLE DIRECTION)
    (HOLDER #RF123H098-16BM)
    (INSERT #N123H-0400-0003-CR 2135)
    (TOOL SET LENGTH 2 1/4")
    G28U0V0W0
    M09
    M479
    M201
    M46
    G54 (G54 FOR MAIN SPINDLE TOOL SETTER)
    G0T1212
    M211
    G0Z.02
    M34 (SYNC BY PHASE)
    M251 (AIR BLOW)
    M252 (AIR BLOW)
    G0G54B.1 (SUB "B" G54 VALUE IS SUB SIDE WORKHOLDING TOP PLANE(Z-) AND WORKPIECE Z ZERO (Z+) INTERSECTION)
    G1G98B-.45F50. (SUB MOVING OVER PART)
    (PICK-OFF POINT)
    M210 (SUB CLOSE)
    G4U.5
    M257 (AIR BLOW OFF)
    M259 (AIR BLOW OFF)
    M11 (MAIN OPEN)
    G4U.5
    B1.095F50.(FINISH PART LENGTH IS 1.345)
    M10
    G4U.5
    G04U.5
    G97S500M4
    G50S2000
    G96S200
    G0X1.25Y0.M478
    G1G99X.95F.002
    U.005
    X.85F.003
    U.005
    X.75
    U.005
    X.65
    U.005
    X.55
    U.005
    X.45
    U.005
    X.35
    U.005
    X.25
    U.005
    X.05
    G330
    G0X2.W.02
    G30U0V0W0M479
    M36
    M5
    #501=#501+1.
    M200
    M1

  8. #8
    Join Date
    Nov 2008
    Posts
    94

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    The Y axis verify is used because of collet drawback in the Sub-Spindle and the subsequent pulling pressures on the Sub's ways. It rechecks the position to ensure accuracy after chucking..
    You should be entering into low torque mode when closing the Sub collet onto the material. Then back into normal torque. Then Y axis verify.

    Forget the G10 and work shift stuff with this machine. More importantly, (as I believe I tried to tell you before) is to use the P1 & P3 subroutines for the Main and Sub respectively. P2 & P4 are not needed. Machine your part on the main using P1 at the top and end of each tool. When your part is done on the main. Dial up with the Sub and find your closing point. Make note of the Y POS. Program that value into the Sub Program and use the Sub transfer procedure in the book. After cut off, clear the X and just G28 V0 and the Sub will rapid home. Make sure to use P3 when programing the Sub. And you may need to tweek the W(Z) value in the P3 subroutine to make it a safe index distance. This can give you fits. Too much and the machine will do nutty things. Too little and it gets too close to the Sub. And things get twisted around and values can be not what they seem when doing this. There is a sweet spot. You have to find it. I like the turret to move about .500 off (toward the Sub) from P1 when P3 is called. No more. (There MUST be a shift) That number, you will need to find by overriding and seeing what the Turret does.
    At part eject. Do the same thing. Dial up the Y to the catcher and record the Y POS value. Program it and repeat.

  9. #9
    Join Date
    Nov 2008
    Posts
    94

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    O1111(PVC BUSHING)
    G20(STICK OUT .250)
    N1
    M05
    M98P1
    T0505(BAR PULLER)
    X1.5Z.250
    G1G98Z-.125F50.0
    X0.0
    G4U1.0
    M21
    G4U1.0
    Z1.025
    G4U1.0
    M22
    G4U2.0
    X1.5
    M98P1
    M1
    N2
    G97S2000M03
    M98P1
    M08
    T1111(FTF)
    X1.2Z0.0
    G1G99X-.030F.004
    X.980
    X1.050,C.035F.001
    Z-1.050F.004
    X1.2
    M98P1
    M1
    N3
    G97S2000M03
    M98P1
    M08
    T0101(.844 DRILL F/X)
    X0.0Z.250
    G1G99Z.020F.010
    G65P9136K-1.125B.020F.003W.200C.100A.5
    M98P1
    M1
    N4
    G97S2000M03
    M98P1
    M08
    T0707(BB)
    X1.1Z.250
    G1G99Z0.0F.005
    X.890,C.025F.001
    Z-1.050F.003
    X0.0
    G00Z.100
    G97S250M03
    M98P1
    M1
    N5
    G97S1000M04
    M98P1
    M09
    T0303(.093 CUT OFF / TRANSFER)
    X1.5Z0.0
    M36
    G1X1.2F5.0
    M32(SUB SYNC)
    M36
    M07(SUB SYNC ORI)
    M56(SUB COLLET OPEN)
    G00Y3.250
    G1Y1.450F15.0
    M67(LOW TORQUE)
    G4U1.0
    M57(SUB COL. CLOSE)
    G4U1.0
    M66(SUB DR. AXIS OFF)
    M68(SUB NORMAL TORQUE)
    M37(AIR BLAST OFF)
    M08
    G1G99X.700F.0015
    G4U1.0
    G00X4.0
    S250
    M09
    G4U.5
    G53Y#5024(Y AXIS VERIFY)
    G28V0(SUB HOME)
    M36
    G4U3.0
    M37
    M98P1
    M05
    M1
    N6
    G4U1.0
    G97S2000M33
    M98P3
    M08
    T0606(SUB FTF)
    X.750Z-.250
    G1G99Z0.0F.010
    X1.048,C.035F.001
    Z.040
    X1.2
    M98P3
    M1
    N7
    G97S2000M33
    M98P3
    M08
    T0714(SUB BB)
    X1.2Z-.250
    G1G99Z0.0F.010
    X.890,C.025F.0008
    Z.030
    X.860F.005
    Z-.100F.010
    M98P3
    T0400
    M1
    N8(PART CATCH)
    M98P3
    M09
    M35(SUB STOP)
    M26(PART CATCH EXT.)
    G00Y8.125
    M56(SUB COL. OPEN)
    G4U3.0
    M25(PART CATCH HOME)
    G53Y#5024
    G28V0
    M1
    M31
    M30

  10. #10
    Join Date
    Nov 2008
    Posts
    94

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    :wee::wee:

  11. #11
    Join Date
    Feb 2019
    Posts
    38

    Re: Quick Question about Work Offset for Subspindle (G10 P0 Y-n.nnn)

    This was a HUGE help. I've figured out how to use the work shift and it's really simple to use. I think the biggest problem with these old machines is some of this stuff just takes a lot of trial and error to figure them out. I would say a little on the archaic side. Once you figure out the method to the madness, it all comes together and makes sense. These older machines are less idiot proof than today's interfaces.

Similar Threads

  1. Mazak Quick Turn, Milling, and Work offset questions.
    By driftmaster in forum Mazak, Mitsubishi, Mazatrol
    Replies: 1
    Last Post: 03-27-2014, 01:29 AM
  2. E work offset question
    By smirob in forum Fadal
    Replies: 1
    Last Post: 07-19-2012, 11:27 AM
  3. Work offset question
    By Barefootboy4 in forum Mach Software (ArtSoft software)
    Replies: 2
    Last Post: 01-25-2011, 06:07 PM
  4. Work/toolpath offset-Question..
    By CyborgCNC in forum Mastercam
    Replies: 3
    Last Post: 03-14-2010, 09:42 AM
  5. Work Offset Question
    By Cartierusm in forum Mach Software (ArtSoft software)
    Replies: 17
    Last Post: 11-29-2007, 10:50 PM

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
  •