Results 1 to 17 of 17

Thread: machinistjay fanuc 6T parameter issue

  1. #1
    Join Date
    May 2012
    Posts
    1
    Thanks
    0
    Thanked 0 Times in 0 Posts

    Default machinistjay fanuc 6T parameter issue

    I'm having a problem with my fanuc 6T control. It lost it's parameters due to a bad board. The board was exchanged and now the machine works ok until a G02/03 is programmed. It seems the x axis isn't cutting the full radius. It will interpolate half the move in the x, then move straight up in the X until it reaches the end X position. Looks like it's not the correct ratio when interpolating. Its ok wit G00 or G01 though. Any suggestions?

  2. #2
    Join Date
    Dec 2011
    Location
    Illinois / Wisconsin border
    Posts
    190
    Thanks
    29
    Thanked 22 Times in 21 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Sounds like more testing is required to understand what is wrong.

    What happens when you command a diagonal move and return to origin?
    G01G91X5.Y5.F45.
    G01G91X-5.Y-5.F45.
    Try all four quadrants.

    What happens when you command a full circle?
    G91 G02 I2.0 F100.
    G91 G02 I2.0 F5.

  3. #3
    Join Date
    Jan 2012
    Posts
    350
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by machinistjay View Post
    I'm having a problem with my fanuc 6T control. It lost it's parameters due to a bad board. The board was exchanged and now the machine works ok until a G02/03 is programmed. It seems the x axis isn't cutting the full radius. It will interpolate half the move in the x, then move straight up in the X until it reaches the end X position. Looks like it's not the correct ratio when interpolating. Its ok wit G00 or G01 though. Any suggestions?
    Post an example of your program here.

    What you're describing is typical of what occurs when using "R" format with circular interpolation on a Series 6T, and the end coordinate of the arc is incorrect. If the end point of the arc was incorrect, the control would swing the arc as far as possible then travel in a straight path to the end coordinates. In all Servo Systems the final target is achieved one way or another.

    Are you using "R" of "IK" format? If "IK" format is used, and the end coordinates are not on the circular trajectory defined by the start point and the arc centre specified by I and K, an alarm will be raised. The situation described above for "R" format occurs when its geometrically impossible to achieve. In most cases where the error is such that an acr could pass through the start and end point, the control merely shifts the arc centre to accomodate the start and end coordinates.

    If the correct physical X and Z positions are being achieved in linear interpolation, I don't believe it will be a scaling issue of the axes.

    Regards,

    Bill

  4. #4
    Join Date
    Dec 2011
    Location
    Illinois / Wisconsin border
    Posts
    190
    Thanks
    29
    Thanked 22 Times in 21 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Good point Bill. I missed the "T" on the control completely.

    There's also the "in position window" parameter which limits the amount of arc endpoint error to give an alarm.
    Sounds like this is opened too much and the program needs to be adjusted. (??)
    However, yes - need an example for us to help. Otherwise, it's all guessing.

  5. #5
    Join Date
    Jun 2012
    Posts
    10
    Thanks
    4
    Thanked 0 Times in 0 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    i think i have same problem here

    i bought old daewoo pro6 and using control fanuc 6T (still used 7segmen for monitor)

    i use mastercam, and directly rewrite the G code to the machine.
    the error occured when execution G02/03, alarm code 022 (code 022=In circular interpolation, radius designation was performed in the NC which is not equipped with the radius designation option)

    iam very confused with this problem, i think its caused by loosing parameter (just my opinion)
    can any body solve this problem?

    sample program

    G21
    G0 T0101
    G18
    G97 S3600 M03
    G0 G54 X0. Z2.
    G50 S3600
    G96 S550
    G99 G1 Z0. F.5
    X-9.2
    G18 G2 X-20. Z-5.4 R5.4
    G1 Z-20.
    X-22.828 Z-18.586
    G28 U0. V0. W0. M05
    T0100
    M30

    regard

  6. #6
    Join Date
    Dec 2011
    Location
    Illinois / Wisconsin border
    Posts
    190
    Thanks
    29
    Thanked 22 Times in 21 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    If you can't change the machine, change your code ...

    Change your output file from Mastercam to use I,K instead of R for your radius cuts.

    Located under:
    Settings
    Machine Definition Manager
    Control Definition
    Arc (for Lathe)
    choose Delta Start to Center

    Save it and re-post your program.

  7. The Following User Says Thank You to MMMMM For This Useful Post:

    jhonyas (06-12-12)

  8. #7
    Join Date
    Jan 2012
    Posts
    350
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by jhonyas View Post
    i think i have same problem here

    i bought old daewoo pro6 and using control fanuc 6T (still used 7segmen for monitor)

    i use mastercam, and directly rewrite the G code to the machine.
    the error occured when execution G02/03, alarm code 022 (code 022=In circular interpolation, radius designation was performed in the NC which is not equipped with the radius designation option)

    iam very confused with this problem, i think its caused by loosing parameter (just my opinion)
    can any body solve this problem?

    sample program

    G21
    G0 T0101
    G18
    G97 S3600 M03
    G0 G54 X0. Z2.
    G50 S3600
    G96 S550
    G99 G1 Z0. F.5
    X-9.2
    G18 G2 X-20. Z-5.4 R5.4
    G1 Z-20.
    X-22.828 Z-18.586
    G28 U0. V0. W0. M05
    T0100
    M30

    regard
    I agree with Doug (aka MMMMM). But further, I wouldn’t, and don’t use “R” format with controls that have such an option. The reasons being:
    1. When using “R” format, the Start, End and Radius data of the arc is passed to the control via the program. This data is used by the control to calculate where the arc centre is. Accordingly, if either the Start or End data are incorrect, the control simple calculates an arc centre based on the given data. Accordingly, you can end up with an erroneous part profile without it being obvious. When I, J, and K format is used, an alarm is raised if the End point isn’t on the arc trajectory as described by the Start point and the arc Centre given by the I, J, and K values.

    2. Even Fanuc themselves state in there manual
    “When an arc having a centre angle approaching 180deg is specified, the calculated centre coordinate may contain an error. In this case, specify the centre of the arc with I, J, and K”. Therefore, even if you do everything correctly, the part shape may still be incorrect. And if the advice of Fanuc is headed, you need to know how to apply both formats. Accordingly, why would one even bother with “R” format given its limitations?

    3. The argument that it’s easier doesn’t wash with me. I, J, and K vales are byproducts of the calculations made when finding the Start and End points of an arc whether done manually or via a CAM package, and clearly there can be no argument that the “R” format is easier when using a CAM package to generate the NC code.

    Regards,

    Bill
    Last edited by angelw; 06-11-12 at 05:08 PM.

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

    jhonyas (06-12-12)

  10. #8
    Join Date
    Jun 2012
    Posts
    10
    Thanks
    4
    Thanked 0 Times in 0 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    thanks for your advice

    i'll try...and you will get the report from me later

    regard

  11. #9
    Join Date
    Jun 2012
    Posts
    10
    Thanks
    4
    Thanked 0 Times in 0 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by MMMMM View Post
    If you can't change the machine, change your code ...

    Change your output file from Mastercam to use I,K instead of R for your radius cuts.

    Located under:
    Settings
    Machine Definition Manager
    Control Definition
    Arc (for Lathe)
    choose Delta Start to Center

    Save it and re-post your program.
    it's work !
    nice tutorial..

    fyi
    i think iam beginner in lathe machine,this is my first lathe machine and i got the old one (too old i think) DAEWOO PRO G GANG TYPE, but iam familiar enough in milling machine.

    my next problem are:
    - everytime exe G18 (in first program and before G02, look at my sample prog) alarm on, also when exe the G54 command (still occure when i change to G55,56,57,58,59)
    so in sample prog above i must delete the G18 and G54
    - how to setting in mastercam (x3 ver) to use in gang type machine

    regard

  12. #10
    Join Date
    Dec 2011
    Location
    Illinois / Wisconsin border
    Posts
    190
    Thanks
    29
    Thanked 22 Times in 21 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Work offsets Located under:
    Settings
    Machine Definition Manager
    Control Definition
    Work System / Lathe
    Change the "Work coordinate selection:" to "Local work offset" or "Other".


    I'm not understanding why your machine is alarming on the G18 though??
    I'll look into this setting. It may be in your Post.

  13. #11
    Join Date
    Jun 2012
    Posts
    10
    Thanks
    4
    Thanked 0 Times in 0 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by MMMMM View Post
    Work offsets Located under:
    Settings
    Machine Definition Manager
    Control Definition
    Work System / Lathe
    Change the "Work coordinate selection:" to "Local work offset" or "Other".


    I'm not understanding why your machine is alarming on the G18 though??
    I'll look into this setting. It may be in your Post.
    iam still using default post = MPLFAN.PST
    any suggestion for my old machine?

    iam already change setting in mastercam, but nothing happen (no additinal menu) for gang type.
    which menu to selection gang type?

    sorry so many question from newbie

    regard
    Last edited by jhonyas; 06-12-12 at 12:18 PM.

  14. #12
    Join Date
    Dec 2011
    Location
    Illinois / Wisconsin border
    Posts
    190
    Thanks
    29
    Thanked 22 Times in 21 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    It looks to be attached to the Machine Configuration. (the mpflan post looks at these values in the "#Machining position turret/spindle settings" section)

    Which plane does work? You'll need to match that to the machine type.

    When you go into Settings / Machine Definition Manager, how is it configured?
    Does your machine look like the list under "Machine Base"?
    OR, do you have a bunch of stuff that the machine doesn't have?

    It is fairly simple to add and delete these componants to match your actual machine.

    After you do, save as your machine name so you can use this again.

  15. #13
    Join Date
    Jan 2012
    Posts
    350
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by jhonyas View Post
    it's work !
    nice tutorial..

    fyi
    i think iam beginner in lathe machine,this is my first lathe machine and i got the old one (too old i think) DAEWOO PRO G GANG TYPE, but iam familiar enough in milling machine.

    my next problem are:
    - everytime exe G18 (in first program and before G02, look at my sample prog) alarm on, also when exe the G54 command (still occure when i change to G55,56,57,58,59)
    so in sample prog above i must delete the G18 and G54
    - how to setting in mastercam (x3 ver) to use in gang type machine

    regard
    The Fanuc Series 6 control didn't use Geometry Offset Programming (G54 to G59) until the 6MB control was introduced, and still at that time the 6TB didn't have this feature. Your control is an early 6TA. In Mastercam you have to configure the post to output a G50 when a tool change occurs. The X, Z coordinates can be edited to the correct values during set up, or values can be calculated in the Post. With regards to the circular interpolation plane, configure the Mastercam Post to not output any plane. The 6TA does not need this specified unless the machine has additional axes such as a Y axis; rare in the day of the 6TA

    Regards,

    Bill
    Last edited by angelw; 06-12-12 at 04:47 PM.

  16. #14
    Join Date
    Jun 2012
    Posts
    10
    Thanks
    4
    Thanked 0 Times in 0 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by MMMMM View Post
    It looks to be attached to the Machine Configuration. (the mpflan post looks at these values in the "#Machining position turret/spindle settings" section)

    Which plane does work? You'll need to match that to the machine type.

    When you go into Settings / Machine Definition Manager, how is it configured?
    Does your machine look like the list under "Machine Base"?
    OR, do you have a bunch of stuff that the machine doesn't have?

    It is fairly simple to add and delete these componants to match your actual machine.

    After you do, save as your machine name so you can use this again.
    i already try to change setting from default (many time), and i hope i'll find something diffrent in the operation manager menu, something more specific regarding gang type....i still learning about this..
    thx for your advice

  17. #15
    Join Date
    Jun 2012
    Posts
    10
    Thanks
    4
    Thanked 0 Times in 0 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by angelw View Post
    The Fanuc Series 6 control didn't use Geometry Offset Programming (G54 to G59) until the 6MB control was introduced, and still at that time the 6TB didn't have this feature. Your control is an early 6TA. In Mastercam you have to configure the post to output a G50 when a tool change occurs. The X, Z coordinates can be edited to the correct values during set up, or values can be calculated in the Post. With regards to the circular interpolation plane, configure the Mastercam Post to not output any plane. The 6TA does not need this specified unless the machine has additional axes such as a Y axis; rare in the day of the 6TA

    Regards,

    Bill
    so how to configure that in mastercam? or by manual editing from nc file (before write on machine)?
    so far regarding my machine condition,all G54 and G18 manually deleted by me before write on the machine, is it safe?
    so far running well in running simulation (running without workpiece)

  18. #16
    Join Date
    Jan 2012
    Posts
    350
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by jhonyas View Post
    so how to configure that in mastercam? or by manual editing from nc file (before write on machine)?
    so far regarding my machine condition,all G54 and G18 manually deleted by me before write on the machine, is it safe?
    so far running well in running simulation (running without workpiece)
    Following is an extract from a Mastercam Fanuc Post. Mastercam can be configured to use either G50 or G54 to G59 coordinate setting systems, but it’s been a long time since I've played with Mastercam, I write my own CAM system. If I get time, I’ll reacquaint myself with Mastercam and post back the procedure, or a current user might chime in and help.

    # mi1 - Work coordinate system: (home_type)
    # -1 = Reference return / Tool offset positioning.
    # 0 = G50 with the X and Z home positions.
    # 1 = X and Z home positions.
    # 2 = WCS of G54, G55.... based on Mastercam settings.

    The way I comprehend your Posts in this Thread, it seems that you haven't used this machine much, if at all, otherwise you would more understanding of the G50 coordinate setting system. Your machine uses G50 to set the coordinate system for the current tool and program. Basically, the G50 command is used to tell the control how far the tool is from the respective X and Z Zero points of the current work-piece, when the tool is at the tool change position. As the centre line of the machine does not change (X0.0), the X G50 Coordinates for the various tools used don’t change from job to job, but the Z G50 Coordinates do. The length of various jobs can be different; accordingly, the position of the work-piece Z Zero also varies.

    As pointed out in one of my earlier posts, the control on your machine does not support Geometry Offsets for tools and it does not support Work Shift via Work Shift Offsets.

    It is safe to use the program without G54 and G18. In fact, you should get a p/s 010 alarm (illegal G code) if G54 to G59 is used. I’m a bit surprised that you get an error when you include the G18, but as stated in my previous Post, it can be omitted from your program.

    Regards,

    Bill
    Last edited by angelw; 06-14-12 at 02:31 AM.

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

    jhonyas (06-22-12)

  20. #17
    Join Date
    Jun 2012
    Posts
    10
    Thanks
    4
    Thanked 0 Times in 0 Posts

    Default Re: machinistjay fanuc 6T parameter issue

    Quote Originally Posted by angelw View Post
    Following is an extract from a Mastercam Fanuc Post. Mastercam can be configured to use either G50 or G54 to G59 coordinate setting systems, but it’s been a long time since I've played with Mastercam, I write my own CAM system. If I get time, I’ll reacquaint myself with Mastercam and post back the procedure, or a current user might chime in and help.

    # mi1 - Work coordinate system: (home_type)
    # -1 = Reference return / Tool offset positioning.
    # 0 = G50 with the X and Z home positions.
    # 1 = X and Z home positions.
    # 2 = WCS of G54, G55.... based on Mastercam settings.

    The way I comprehend your Posts in this Thread, it seems that you haven't used this machine much, if at all, otherwise you would more understanding of the G50 coordinate setting system. Your machine uses G50 to set the coordinate system for the current tool and program. Basically, the G50 command is used to tell the control how far the tool is from the respective X and Z Zero points of the current work-piece, when the tool is at the tool change position. As the centre line of the machine does not change (X0.0), the X G50 Coordinates for the various tools used don’t change from job to job, but the Z G50 Coordinates do. The length of various jobs can be different; accordingly, the position of the work-piece Z Zero also varies.

    As pointed out in one of my earlier posts, the control on your machine does not support Geometry Offsets for tools and it does not support Work Shift via Work Shift Offsets.

    It is safe to use the program without G54 and G18. In fact, you should get a p/s 010 alarm (illegal G code) if G54 to G59 is used. I’m a bit surprised that you get an error when you include the G18, but as stated in my previous Post, it can be omitted from your program.

    Regards,

    Bill
    thanks for your advice bill....its can solve my problem so far...
    btw...i am still looking for manual book for this machine, do you know where i can get (buy) it?

Similar Threads

  1. FANUC Pro 3 G68 Issue
    By Christian1029 in forum General CNC & Manufacturing Discussion
    Replies: 0
    Last Post: 10-11-12, 11:05 AM
  2. Fanuc Ot control ZRN issue
    By christate20000 in forum Fanuc Controls
    Replies: 5
    Last Post: 09-07-10, 10:09 AM
  3. Fanuc SP230 Power up issue
    By mwescott in forum Fanuc Controls
    Replies: 1
    Last Post: 10-16-07, 08:53 PM
  4. Fanuc Spindel Tapping issue
    By MisterLucky in forum Fanuc Controls
    Replies: 1
    Last Post: 09-07-07, 08:10 PM
  5. Replies: 0
    Last Post: 09-09-06, 04:41 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
  •