Results 1 to 5 of 5

Thread: G78-threading cycle help please

  1. #1
    Join Date
    Jan 2007
    Posts
    42
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default G78-threading cycle help please

    Friends,

    Recently after commissioning a cnc with oi-TC controller we had G78 Threading cycle problem.

    While machining after few passes the spindle was stopping and the tips were breaking.Later we found that there was some G-CODE missing in the program like G90,G53 and G97.

    Following is the G78 threading cycle program.

    Any mistake pl identify them.

    G90 G53 T0505:
    G97 S500 M04:
    G0 X135.0 Z20.0:
    G0 Z5.0 M07:
    G01 Z20.0 F1.0:
    G78 X132.6 Z-25.0 F4.233:
    X132.4:
    X132.2:
    X132.0:
    X131.8:
    X131.6:
    X131.4:
    X131.2:
    X131.0:
    X130.8:
    X130.6:
    X130.4:
    X130.2:
    X130.0:
    LIKE THAT
    UP TO X128
    AND FROM X128.0
    X127.95:
    X127.9:
    X127.85:
    X127.8:
    X127.767:
    G0 Z20.0 M09:
    T0000
    G0 X0 Z110.0 M05:
    M01:

    Similarly while doing internal threading cycle with g78 after few passes the tool is digging.

    IAM NOT FAMILIAR WITH PROGRAMMING SO PL HELP ME.

    Thanks

    CHANDRU

  2. #2
    Join Date
    Oct 2009
    Posts
    9
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: G78-threading cycle help please

    Hello Chandru,

    For the O-T model of fanuc, you need to use G76 for a canned threading cycle. If you want to do it line by line, use G92 or G32 code. Second, do not use G53. This is a work offset. Unless you are using the same tool on different chuck, I would recommend never to use G52 to G59 on a lathe.

    Hope it helps.

    YBMach

  3. #3
    Join Date
    Dec 2009
    Location
    ca
    Posts
    16
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: G78-threading cycle help please

    Hi
    Please check this cycle for threading
    and use G54 and don't use G90. I hope that is work good.

    G76 P(m)(r)(a) Q(△dmin) R(d)
    G76 X(u) Z(w) R(i) P(k) Q(△d) F(L)

    m: Number of replication for finish maching(1 to 99)
    This command is state command.It will not change before a value is specified. FANUC system
    parameter(NO.0723)specifing.
    r: Quantity of chamfer
    This command is state command.It will not change before a value is specified. FANUC system
    parameter(NO.0109)specifing.
    a: Angle of tool nose:
    You can select 80 degree、60 degree、55 degree、30 degree、29 degree、0 degree,and specify
    it with 2 digit.
    This command is state command.It will not change before a value is specified. FANUC system
    parameter(NO.0724)specifing.For example:P(02/m、12/r、60/a)
    △dmin: Minimum of cutting depth expressed by radius.
    This command is state command.It will not change before a value is specified. FANUC system
    parameter(NO.0726)specifing.
    d: Allowance for finish
    i: Semidiameter of threaded portion
    If i=0,it is seen as normal linear thread cutting.
    k: Height of thread expressed by radius value.
    △d: Cutting depth for fist time(radius value)

  4. #4
    Join Date
    Jun 2012
    Posts
    6
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default Re: G78-threading cycle help please

    Quote Originally Posted by YBMach View Post
    Hello Chandru,

    For the O-T model of fanuc, you need to use G76 for a canned threading cycle. If you want to do it line by line, use G92 or G32 code. Second, do not use G53. This is a work offset. Unless you are using the same tool on different chuck, I would recommend never to use G52 to G59 on a lathe.

    Hope it helps.

    YBMach
    G54-G59 are work offsets on a lathe. We use G53 on a Mori SL-35 with an MF-T6 control to move the turret to a clearance point.....such as G53X-8.Z-14. G53 does not use tool geometry as part of the move. Nor does it have anything to do with a work offset. It is a machine position.

    No idea what a G52 is on a lathe. G50 is used on some old lathes. I suggest you NOT use it except as a last option. Can get in trouble if not careful. Newer lathes have much more friendly ways of moving your workshift, sorry, work offset.

    Apparently you don't program for subspindle lathes or make multiple parts with one barstop. Otherwise you would not recommend never using G54-G59.

    I am not familiar with any G78 code on a Fanuc control. This is not to say that a machine builder couldn't assign it to any option/operation.

    I can't help with the oi-TC control. We do have some O-T control lathes.
    Last edited by g-codeguy; 06-12-12 at 10:54 AM.

  5. #5
    Join Date
    Jan 2012
    Posts
    346
    Thanks
    0
    Thanked 70 Times in 62 Posts

    Default Re: G78-threading cycle help please

    Quote Originally Posted by CHANDRU View Post
    Friends,

    Recently after commissioning a cnc with oi-TC controller we had G78 Threading cycle problem.

    While machining after few passes the spindle was stopping and the tips were breaking.Later we found that there was some G-CODE missing in the program like G90,G53 and G97.

    Following is the G78 threading cycle program.

    Any mistake pl identify them.

    G90 G53 T0505:
    G97 S500 M04:
    G0 X135.0 Z20.0:
    G0 Z5.0 M07:
    G01 Z20.0 F1.0:
    G78 X132.6 Z-25.0 F4.233:
    X132.4:
    X132.2:
    X132.0:
    X131.8:
    X131.6:
    X131.4:
    X131.2:
    X131.0:
    X130.8:
    X130.6:
    X130.4:
    X130.2:
    X130.0:
    LIKE THAT
    UP TO X128
    AND FROM X128.0
    X127.95:
    X127.9:
    X127.85:
    X127.8:
    X127.767:
    G0 Z20.0 M09:
    T0000
    G0 X0 Z110.0 M05:
    M01:

    Similarly while doing internal threading cycle with g78 after few passes the tool is digging.

    IAM NOT FAMILIAR WITH PROGRAMMING SO PL HELP ME.

    Thanks

    CHANDRU
    Hi Chandru,
    The other replies you've received are based on a control that is set to G Code System A. There are three G Code Systems available with the Fanuc Control selectable via parameter.

    The G78 Code you're using and the way its implemented in your program indicates that your control is set to use G Code System B. G78 in G Code System B is the same as G92 in System A. Overwhelmingly, System A is used with Turning Centre, and unless you have some particular reason for using the control set to System B, you will gain more help from Forums such as this, by setting the control to use G Code System A. In your control, setting bit 6 and 7 of parameter 3401 both to "0" will set the control to System A. Currently, the settings of your control should be 0 and 1 for bit 7 and 6 respectively for it to use G Code System B. Bit numbers run 0 to 7 from right to left. Accordingly, its the two leftmost bits have to be set to 0.

    With regards to the problem with the spindle stopping after a few passes, there's nothing in your listed code that would do that.

    G53 is used to set the Machine Coordinate System. G54 to G59 are used to set the Workpiece Coordinate System. From a programming perspective, using G54 to G59 is a better proposition.

    G97 is correct for all G Code Systems to command constant RPM. G76 is also the correct code in System A and B for the Multi Repetitive Threading Cycle, its G78 in System C.

    Where is the Reference Return position on your machine. I note that the penultimate block is a move to X0 Z110. X0 on a lathe is generally the centre line of the machine.

    Regards,

    Bill
    Last edited by angelw; 07-01-12 at 06:11 PM.

  6. The Following User Says Thank You to angelw For This Useful Post:

    Jbanko (07-08-12)

Similar Threads

  1. Auto operation cant cycle start alarm occurs when cycle start is pushed.
    By Petro in forum General CNC & Manufacturing Discussion
    Replies: 1
    Last Post: 10-10-12, 10:28 AM
  2. g76 threading cycle (2 block g76)
    By steelman in forum Programming / Applications
    Replies: 8
    Last Post: 06-12-12, 10:11 AM
  3. Want Buy CNC Threading Machines and Setting up an API Threading Workshop
    By delta in forum General CNC & Manufacturing Discussion
    Replies: 3
    Last Post: 12-27-10, 05:26 AM
  4. Threading 2-4 1/2 thread
    By rob870 in forum Programming / Applications
    Replies: 2
    Last Post: 07-09-10, 09:17 PM
  5. Threading
    By Guest in forum General CNC & Manufacturing Discussion
    Replies: 4
    Last Post: 09-09-07, 02:02 PM

Posting Permissions

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