584,800 active members*
4,349 visitors online*
Register for free
Login
IndustryArena Forum > MetalWorking Machines > Hardinge Lathes > Talent 6/45 Reference Issue Fanuc oi-T Controller
Results 1 to 5 of 5
  1. #1
    Join Date
    Mar 2016
    Posts
    9

    Talent 6/45 Reference Issue Fanuc oi-T Controller

    Full disclosure I am not that experienced with CNC but I am out of ideas as to why a certain line of G-Code is causing issues. The problem is as follows. After referencing the machine to its zero position using the controller I start a code that repeatedly wants to run the turret into the spindle if I don't hit cycle stop. The line of code causing issues is G0 X.9082 Z6.2. Which I think should be a rapid move to the start of the work. I have checked tool and work offsets however the controller always thinks the work is ~12 inches past the spindle ie there is always a foot of distance to go listed on the controller when the edge of the tool is 1" from the chuck. The only way I have prevented this from happening is to reference to machine zero engage machine lock out and in handwheel mode set the absolute z and x to zero to match the machine zero. When the same code is run again it doesn't want to crash the lathe rather it appears to reference way above (12") where the work would be toward the tailstock. If anyone needs more information I'll post the full code tomorrow when I can get access to the CNC computer. Appreciate the help at this point I'm stumbling around in the dark here.

  2. #2
    Join Date
    Dec 2008
    Posts
    3110

    Re: Talent 6/45 Reference Issue Fanuc oi-T Controller

    What offsets....( tool & work offset ) are active when that line of code is executed ?
    Put up the NC file

    Z setting
    I have set our lathe machine origin, so that chuck face is work zero origin, and the value I input on G54 Z is the distance from chuck face to the part origin ( generally the stock size )
    - tool ZERO offset is the turret face, so that any tooling offsets can be physically measured with a rule to verify that the tool has been set ( it'll be close anyway )

    X setting
    Dial indicator is held by spindle to clock inside ER32 ( must be zero T.I.R ), so that any X0.0 (zero) offset on a tool for drilling on the spindle centreline

  3. #3
    Join Date
    Mar 2016
    Posts
    9

    Re: Talent 6/45 Reference Issue Fanuc oi-T Controller

    Here is the NC file.

    Code:
    %
    O0007
    (PROGRAM NAME - THREADED PART_0304)
    (DATE=DD-MM-YY - 04-03-16 TIME=HH:MM - 17:10)
    (MCX FILE - C:\USERS\MELABUSER\DOCUMENTS\EXP2\THREADED PART.EMCX-9)
    (NC FILE - C:\USERS\MELABUSER\DOCUMENTS\MY MCAMX9\LATHE\NC\THREADED PART_0304.NC)
    (MATERIAL - STEEL INCH - 1030 - 200 BHN)
    G20
    N0101
    (TOOL - 1 OFFSET - 1)
    (LROUGH OD FINISH RIGHT - 35 DEG.  INSERT - VNMG-431)
    G97S1000M03
    G0T0G30U0.W0.
    T0101
    G0X.98017Z6.2
    G1G99Z6.1F.005
    Z2.90854
    X1.
    X1.14142Z2.97925
    G0Z6.2
    X.96034
    G1Z6.1
    Z2.90854
    X1.
    X1.14142Z2.97925
    G0Z6.2
    X.9405
    G1Z6.1
    Z2.90854
    X.98034
    X1.12176Z2.97925
    G0Z6.2
    X.92067
    G1Z6.1
    Z2.90854
    X.9605
    X1.10193Z2.97925
    G0Z6.2
    X.90084
    G1Z6.1
    Z2.90854
    X.94067
    X1.08209Z2.97925
    G0Z6.2
    X.88101
    G1Z6.1
    Z2.90854
    X.92084
    X1.06226Z2.97925
    G0Z6.2
    X.86118
    G1Z6.1
    Z2.90854
    X.90101
    X1.04243Z2.97925
    G0Z6.2
    X.84134
    G1Z6.1
    Z2.90854
    X.88118
    X1.0226Z2.97925
    G0Z6.2
    X.82151
    G1Z6.1
    Z2.90854
    X.86134
    X1.00277Z2.97925
    G0Z6.2
    X.80168
    G1Z6.1
    Z2.90854
    X.84151
    X.98293Z2.97925
    G0Z6.2
    X.78185
    G1Z6.1
    Z2.90854
    X.82168
    X.9631Z2.97925
    G0Z6.2
    X.76202
    G1Z6.1
    Z3.99811
    G3X.77Z3.98435R.02565
    G1Z3.96194
    Z3.00484
    Z2.98437
    Z2.90854
    X.80185
    X.94327Z2.97925
    G0Z6.2
    X.74218
    G1Z6.1
    Z4.00716
    G3X.77Z3.98435R.02565
    G1Z3.96194
    Z3.00484
    Z2.98437
    Z2.90854
    X.78202
    X.92344Z2.97925
    G0Z6.2
    X.72235
    G1Z6.1
    Z4.00994
    G3X.7622Z3.99795R.02567
    G1X.90361Z4.06868
    G0Z6.2
    X.70252
    G1Z6.1
    Z4.01
    X.71874
    G3X.7424Z4.0071R.02565
    G1X.88377Z4.07783
    G0Z6.2
    X.68269
    G1Z6.1
    Z4.01
    X.71874
    G3X.7225Z4.00995R.02565
    G1X.86394Z4.08064
    G0Z6.2
    X.66286
    G1Z6.1
    Z4.01
    X.70269
    X.84411Z4.08071
    G0Z6.2
    X.64303
    G1Z6.1
    Z4.99142
    G3X.645Z4.98435R.02564
    G1Z4.04119
    Z4.01
    X.68286
    X.82428Z4.08071
    G0Z6.2
    X.62319
    G1Z6.1
    Z5.00535
    G3X.645Z4.98435R.02566
    G1Z4.04119
    Z4.01
    X.66303
    X.80445Z4.08071
    G0Z6.2
    X.60336
    G1Z6.1
    Z5.00954
    G3X.6432Z4.9911R.02566
    G1X.78461Z5.06182
    G0Z6.2
    X.58353
    G1Z6.1
    Z5.01
    X.59374
    G3X.6234Z5.0053R.02565
    G1X.76478Z5.076
    G0Z6.2
    X.5637
    G1Z6.1
    Z5.01
    X.59374
    G3X.6035Z5.00955R.02565
    G1X.74495Z5.08024
    G0Z6.2
    X.54387
    G1Z6.1
    Z5.01
    X.5837
    X.72512Z5.08071
    G0Z6.2
    X.52403
    G1Z6.1
    Z5.01
    X.56387
    X.70529Z5.08071
    G0X1.005
    G97
    G0T0G30U0.W0.
    M30
    %
    From what you suggested I think the line "G0X.98017Z6.2" should be "G54 G0X.98017Z6.2" to select offset 1. From what I can tell on the controller the machine origin is the turret reference position back towards the tailstock not sure how to change this though. Also could you elaborate on how to set T.I.R? I broke a center drill one afternoon since this was not correct. Thanks for the help.

  4. #4
    Join Date
    Dec 2008
    Posts
    3110

    Re: Talent 6/45 Reference Issue Fanuc oi-T Controller

    Quote Originally Posted by hinshelwood View Post
    From what you suggested I think the line "G0X.98017Z6.2" should be "G54 G0X.98017Z6.2" to select offset 1. From what I can tell on the controller the machine origin is the turret reference position back towards the tailstock not sure how to change this though. Also could you elaborate on how to set T.I.R? I broke a center drill one afternoon since this was not correct.
    I don't think it is the G54......use MDI to change to G55, look at what is active, then hit RESET....it should revert back to G54, which is normal, but be aware that everything should be programmed in G54
    I'm thinking that you have not set the work offset correctly, or you have not got good "safety codes" at the beginning of the program

    Here is a link to my Hardinge machine & post.......I can see you are using Mcam
    ( it has a better NC program startup, goes home before any toolchange, no G54 uses G28 reference return .... checkout the Misc Integers page #1 & #3 fields


    Trueing the Turret
    Sometimes a tool may take a knock, causing the turret to be misaligned, ( a centring tool or drill is NOT laying on the X axis plane, any movement in X cannot bring that tool to the correct position, it is either above, or below spindle centre )
    - is usually means the turret needs to be placed back into its correct position, where the centring tool is inline with the spindle axis.

    To loosen the turret, there is 8 bolts & 2 dowels in the turret face, ( dowels can be removed, screws loosened to bring a drill holder onto the X plane
    - use a lever dial indicator ( mounted to the spindle, the indicator clocks the drill holder true by rotating the turret & moving the X-axis together until the holder is in correct position
    - tighten the turret screws very tight, check manual for correct torque pressure........ ( I have found that you need to go higher than specified )
    - record X absolute position, set the tool offset for the tool station you have just trued to X0.0000, activate that offset, the absolute position should be X0, if not you have to adjust the machine origin so it does read zero
    - any value that is input is not updated until you re-actives that offset
    - any tool offset that is set to X0, and if you program a tool to go to X0 should be putting that holder onto the spindle centreline

    - as you have adjusted machine X origin, you would need to re-gauge all tools again

  5. #5
    Join Date
    Mar 2016
    Posts
    9

    Re: Talent 6/45 Reference Issue Fanuc oi-T Controller

    You were right. I was not setting the work offsets correctly. On this machine I had to reference the machine on the control side to machine zero. Upload the code. Set work and tool offset. Return to machine zero then run the code. Been so busy turning parts I forgot to update the thread.

Similar Threads

  1. Fanuc reference riddle
    By MechaEng in forum Uncategorised MetalWorking Machines
    Replies: 1
    Last Post: 05-11-2019, 05:51 AM
  2. Replies: 0
    Last Post: 05-20-2014, 05:42 AM
  3. Fanuc 10T will not Zero Reference
    By serickson in forum Fanuc
    Replies: 2
    Last Post: 06-24-2011, 12:39 PM
  4. Issue with FANUC 18i-M controller
    By TeleGuy in forum Fanuc
    Replies: 6
    Last Post: 11-10-2010, 11:41 AM
  5. Harding Talent & Fanuc
    By Artitus in forum Hardinge Lathes
    Replies: 3
    Last Post: 05-15-2009, 01:42 AM

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
  •