Results 1 to 4 of 4

Thread: Need help for using probe in CNC VMC(Fanuc series)

  1. #1
    Join Date
    Jul 2011
    Posts
    3
    Thanks
    1
    Thanked 0 Times in 0 Posts

    Default Need help for using probe in CNC VMC(Fanuc series)

    Hai friends,
    I need to check a height in my component by using the probe tool(Renishaw). need your help on macro programming for probing operation.

    Thanks,

    Any doubt on my question, pl pl pl ask me again,....... pls.............

    Regards.
    Venkatraj G.

  2. #2
    Join Date
    Jan 2012
    Posts
    350
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: Need help for using probe in CNC VMC(Fanuc series)

    Quote Originally Posted by sarvenkatg View Post
    Hai friends,
    I need to check a height in my component by using the probe tool(Renishaw). need your help on macro programming for probing operation.

    Thanks,

    Any doubt on my question, pl pl pl ask me again,....... pls.............

    Regards.
    Venkatraj G.

    What specifically do you want to know? You might also mention the make and model of the control.

    Regards,

    Bill
    Last edited by angelw; 06-30-12 at 01:16 AM.

  3. #3
    Join Date
    Jul 2011
    Posts
    3
    Thanks
    1
    Thanked 0 Times in 0 Posts

    Default Re: Need help for using probe in CNC VMC(Fanuc series)

    Quote Originally Posted by angelw View Post
    What specifically do you want to know? You might also mention the make and model of the control.

    Regards,

    Bill

    Hai,
    thanks for the response,.....
    am touching the component with the probe. i need to convert that co-ordinate to the Z work offset. for this purpose, i need programming codes....
    pls help to do so......... thanks,..............

  4. #4
    Join Date
    Jan 2012
    Posts
    350
    Thanks
    0
    Thanked 74 Times in 65 Posts

    Default Re: Need help for using probe in CNC VMC(Fanuc series)

    Quote Originally Posted by sarvenkatg View Post
    Hai,
    thanks for the response,.....
    am touching the component with the probe. i need to convert that co-ordinate to the Z work offset. for this purpose, i need programming codes....
    pls help to do so......... thanks,..............
    You still haven't specified the Series Model of the Fanuc control, so the Tool Length System variables may need changing to be compatible with your control. The example and comments I've provided should be compatible with Series16 and onwards. Also, if your control has both Geometry and Wear Tool Length Offsets, the current Wear value will need to be taken into account when updating the Tool Length Offset. I haven't considered the Wear Offset in the example I've provided.

    Renishaw actually have a Z Surface Measure Macro, but the package its included in may be expensive. The following Macro I've created for you has similar functionality as I'm assuming the Renishaw product has.

    In the following example Main Program, the Z Measure Macro (O9018) is being called with a Custom G Code. To call program O9018 with G118, the number 118 has to be registered in parameter #6058. You will have to check if this parameter is correct for your control.

    Alternatively, the Macro Program can be called with G65 as follows:

    G65 P9018 Z0.0 {M91 S1 T1}
    Where:
    1. Z = Z coordinate of Z surface to check.
    2. M = Tool Offset Number in which to store the measured error.
    3. S = Workshift Offset to be updated by the Macro Program.
    4. T = Tool Offset Number to be updated by the Macro Program.
    5. The Arguments in {} are optional. The {} are NOT included in the call block.
    6. The Z argument is compulsory.
    7. Only S or T can be included in the one call statement, NOT both.
    8. S 1 to 6 corresponds to G54 to G59 respectively.

    I have not tested (debugged) this Macro Program on a machine. Accordingly, proceed with care if you use it.

    Also, many Renishaw Probes need to be spun to turn them ON (including a M19) and spun OFF when finished. Consult your operating manual for your probe for this procedure and add if required to the Main Program before calling the Macro Program. Make sure the Probe is ON and WORKING with the Skip Function (G31), by commanding a short incremental Z move in Fresh Air, and triggering the probe by hand to ensure the G31 command is interfaced with the Probe Hardware. If its NOT, there is a strong possibility that the probe will be damaged (destroyed) if its run into something solid and immoveable.

    Post back to the Forum how it worked for you.

    Regards

    Bill

    %O0001
    (Z SURFACE MEASURE CALL PROGRAM)
    N1 G91 G28 Z0.0
    G28 Y0.0
    T20 M06
    G90 G54 G00 X0.0 Y0.0
    G43 Z100.000 H20
    G118 Z0.0 M99 S1 (CALL THE Z SURFACE MEASURE MACRO HERE) (STORE THE ERROR IN TOOL OFFSET 99 - UPDATE WORKSHIFT G54)
    G91 G28 Z0.0
    G28 Y0.0
    M30
    %

    %
    O9018
    (Z SURFACE MEASURE MACRO)
    IF[[#19 NE #0] AND [#20 NE #0]]GOTO100 (ERROR TRAP FOR BOTH S AND T ARGUMENTS BEING PASSED)
    IF[#26 EQ #0] GOTO200 (ERROR TRAP FOR MISSING Z ARGUMENT)
    #1 = #5023 (RECORD CURRENT Z MACHINE VALUE AT INITIAL LEVEL)
    #2 = [#4014 - 53] (GET CURRENT GROUP 14) ( WORKSHIFT NUMBER) (USED FOR POSSIBLE FURTHER DEVELOPMENT)
    #3 = #4003 (STORE CURRENT GROUP 3) (G90/G91)
    #4 = #5043 - #26 (GET INCREMENTAL DISTANCE TO TARGET Z)
    G91
    G31 Z -[#4 + 20.0] F2000 (USE SKIP SIGNAL FOR FAST FEED PROBE TOUCH)
    #5 = #5023 (RECORD CURRENT Z FOR FAST FEED TOUCH)
    IF[#5 LE [#1-[#4+5.0]]]GOTO300 (PROBE ERROR TRAP - NO TRIGGER)
    G00 Z3. (RAPID PROBE AWAY FROM Z WORKPIECE SURFACE)
    #3004=2 (DISABLE FEED OVERRIDE)
    G31 Z [#5 - #5023] F30 (CALCULATE AN INCREMENTAL MOVE THAT WILL ENSURE A TOUCH AT SLOW FEED)
    #6=#5063 (RECORD SKIP SIGNAL Z MACHINE COORDINATE)
    #3004=0 (ENABLE FEED OVERRIDE)
    G00 Z[#1-#5023] (CALCULATE INCREMENTAL MOVE TO RETURN TO INITIAL Z LEVEL)
    #7 = #6 - [#1 - #4] (CALCULATE THE ERROR)
    IF[#13 EQ #0] GOTO20 (CHECK IF M ARGUMENT PASSED)
    IF[#13 EQ #20]GOTO400 (CHECK IF M AND T ARGUMENTS ARE THE SAME NUMBER)
    #[2200 + #13] = #7 (STORE THE Z ERROR IN THIS TOOL OFFSET)
    N20
    (NO MORE THAN ONE OF THE FOLLOWING IF STATEMENTS SHOULD TEST TRUE)
    IF[#19 EQ #0] GOTO30 (CHECK IF S ARGUMENT PASSED)
    #[5203+20 * #19] = #[5203+20 * #19] - #7 (UPDATE Z WORKSHIFT IF S ARGUMENT WAS PASSED)
    N30
    IF[#20 EQ #0] GOTO40 (CHECK IF T ARGUMENT PASSED)
    #[2200 + #20] = #[2200 + #20] - #7 (UPDATE TOOL LENGTH OFFSET IF T ARGUMENT WAS PASSED)
    N40
    GOTO500
    N100
    #3006 = 1(S AND T TOGETHER)
    GOTO500
    N200
    #3006 = 1(Z ARGUMENT OMITTED)
    GOTO500
    N300
    #3006 = 1(PROBE ERROR)
    GOTO500
    N400
    #3006 = 1(M AND T THE SAME VALUE)
    N500
    G#3 (RESTORE GROUP 3 G CODE)
    M99
    %
    Last edited by angelw; 07-01-12 at 09:10 AM.

Similar Threads

  1. Need a Fanuc O-T series manual
    By Threeeights16 in forum Machine Repair & Troubleshooting
    Replies: 3
    Last Post: 10-24-15, 12:02 PM
  2. 15-m ge fanuc series control
    By angel1971 in forum Machine Repair & Troubleshooting
    Replies: 2
    Last Post: 09-27-12, 10:20 AM
  3. Load % - Fanuc Series 18i
    By CNC Steve in forum Machine Repair & Troubleshooting
    Replies: 1
    Last Post: 02-06-12, 08:59 PM
  4. Fanuc Series 0i-MC PWE not changing!!
    By ryaco in forum Machine Repair & Troubleshooting
    Replies: 10
    Last Post: 06-09-11, 08:34 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
  •