Renishaw RMP40 P9810 MC3086 PATH OBSTRUCTED - Page 2
Close
Login to Your Account
Page 2 of 3 FirstFirst 123 LastLast
Results 21 to 40 of 52
  1. #21
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,030
    Post Thanks / Like
    Likes (Given)
    547
    Likes (Received)
    515

    Default

    I was asked this by Renishaw,
    Can you have the customer make sure the trigger filter setting isn’t turned on. This would cause a delay in the trigger signal from the probe, which means the machine would also react slower once the stylus has been triggered.

    trigger-filter-settings.jpg

  2. #22
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,187
    Post Thanks / Like
    Likes (Given)
    931
    Likes (Received)
    2814

    Default

    Quote Originally Posted by fjs0001 View Post
    .......I tried calling Ellison all day Friday, but no one ever answered. ....
    How long before D.D. Machine jumps on this?

  3. #23
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    604
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    152

    Default

    Quote Originally Posted by LockNut View Post
    I was asked this by Renishaw,
    Can you have the customer make sure the trigger filter setting isn’t turned on. This would cause a delay in the trigger signal from the probe, which means the machine would also react slower once the stylus has been triggered.

    trigger-filter-settings.jpg
    Quite peculiar question from Renishaw. Aren't they aware, that in case in subject PATH OBSTRUCTED alarm is generated during O9810 protected move ? The clumsy (see Lock Nut's explanation above) ENHENCED FILTER option in probe setup process is meant to prevent this alarm when false trigger occurs, but they insist to turn it off ?
    Hey RENISHAW guys, nowadays, when super sensitive RENGAGE line of probes is so aggressively marketed, it's about time to update the Inspection+ with FALSE TRIGGER FILTER OPTION, which by the way is standard on all SNR routines.

  4. #24
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by PROBE View Post
    I just paid attention, that you are running the protected move on F350. feedrate (M165P9810Z-.220F350.(PROBE POSITION MOVE) This is where is faults out.), while the Renishaw's FAST FEED default, set in O9724, is 200 IPM. Too fast feedrate in O9810 can cause false trigger. Lower the feedrate significantly (F50.) and try again.
    I tried that without success. I even pulled the probe out of the machine and held it in my hand while the machine was running. it still faulted out once it reached Z-.22.

  5. #25
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by LockNut View Post
    fjs0001,
    My mistake, I just spoke with Renishaw and the PATH OBSTRUCTED alarm can only be caused during the protected positiioning move, O9810.

    I also noticed this in your previous response.
    M185
    M73
    G4X.1 (This should always be changed to X1.0) This short dwell has caused problems for us in the past)
    G5.1Q1
    M99

    This program O8501 is in memory, you can find it in the LIBRARY folder. It can be edited.This is the probe start program.

    O8501(PROBE START)
    M184(G01 INTERLOCK OFF)
    M74(OMP ON)
    G4X1.
    G5.1Q0
    M99

    This program O8503 is in memory, and can also be found in the LIBRARY folder. It also can be edited.

    O8503 (PROBE END)
    M185(G01 INTERLOCK ON)
    M73(PROBE OFF)
    G4X1.
    G5.1Q1
    M99

    There are two more for the tool setter. They give a small amount of control to users when the macro executor programs cannot be changed.
    It won't let me modify those programs, even if I changed 3202 NE9 to 0.

    Quote Originally Posted by LockNut View Post
    I was asked this by Renishaw,
    Can you have the customer make sure the trigger filter setting isn’t turned on. This would cause a delay in the trigger signal from the probe, which means the machine would also react slower once the stylus has been triggered.

    trigger-filter-settings.jpg
    The trigger filter isn't turned on.

    I did get it to work, not correctly though. If I change the tool length to be below 0.002", it works.

  6. #26
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I ran the GUI probe calibration and it set the tool length offset to the correct length. It still won't run 9810 correctly

  7. #27
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    604
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    152

    Default

    Quote Originally Posted by fjs0001 View Post
    I tried that without success. I even pulled the probe out of the machine and held it in my hand while the machine was running. it still faulted out once it reached Z-.22.
    Quote Originally Posted by fjs0001 View Post

    I did get it to work, not correctly though. If I change the tool length to be below 0.002", it works.
    1. The path is not disturbed as Z axis is achieving the target -.22.
    2. "Cheating" and setting the tool offset below 0.002 ceases the alarm appearance.
    3. Block in O9810 which checks if the machine arrived to target point:
    IF[ABS[[#5043-#116]-[#26]]GT#123]GOTO8 (ALARM PATH OBSTRUCTED)
    3.1 #5043 is Z axis position in current work coordinates. In order to verify it MDI #100=#5043 and check the #100.It should be equal to -.22 + probe tool length offset (G43 applied).
    3.2 #116 should be equal to probe tool length offset.
    3.3 #26 should be equal to commanded Z - -.22
    3.4 #123 set in O9724 as IN POSITION ZONE should be 0.002

    Check the variables. As no error is generated when offset is set to less then 0.002, it seems that there is a problem with #5043 calculation.

  8. #28
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by PROBE View Post
    1. The path is not disturbed as Z axis is achieving the target -.22.
    2. "Cheating" and setting the tool offset below 0.002 ceases the alarm appearance.
    3. Block in O9810 which checks if the machine arrived to target point:
    IF[ABS[[#5043-#116]-[#26]]GT#123]GOTO8 (ALARM PATH OBSTRUCTED)
    3.1 #5043 is Z axis position in current work coordinates. In order to verify it MDI #100=#5043 and check the #100.It should be equal to -.22 + probe tool length offset (G43 applied).
    3.2 #116 should be equal to probe tool length offset.
    3.3 #26 should be equal to commanded Z - -.22
    3.4 #123 set in O9724 as IN POSITION ZONE should be 0.002

    Check the variables. As no error is generated when offset is set to less then 0.002, it seems that there is a problem with #5043 calculation.
    We just had a power outage and when the power came back on 9810 started working again.

    I'm not sure what you meant by blocking in 9810, but this is what I tried.
    G43H36Z4.0
    M74
    IF[ABS[[#5043-#116]-[#26]]GT#123]GOTO8 (ALARM PATH OBSTRUCTED)
    M165P9810Z-.220F350.
    N8

    So I did MDI #100=#5043 and it equaled 9.4245, which is my tool length + the current position 5.4245 + 4.0 = 9.4245
    #116, #26, #123 didn't have any data stored in them, so it skipped the 9810 command.

  9. #29
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    604
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    152

    Default

    Quote Originally Posted by fjs0001 View Post
    We just had a power outage and when the power came back on 9810 started working again.

    I'm not sure what you meant by blocking in 9810, but this is what I tried.
    G43H36Z4.0
    M74
    IF[ABS[[#5043-#116]-[#26]]GT#123]GOTO8 (ALARM PATH OBSTRUCTED)
    M165P9810Z-.220F350.
    N8

    So I did MDI #100=#5043 and it equaled 9.4245, which is my tool length + the current position 5.4245 + 4.0 = 9.4245
    #116, #26, #123 didn't have any data stored in them, so it skipped the 9810 command.
    Most important - it works again. Sometimes non sequential shut down (power outage) makes miracles.

  10. Likes LockNut liked this post
  11. #30
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by PROBE View Post
    Most important - it works again. Sometimes non sequential shut down (power outage) makes miracles.
    It was short lived. It stopped working after running it a few times.

  12. #31
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    604
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    152

    Default

    Quote Originally Posted by fjs0001 View Post
    It was short lived. It stopped working after running it a few times.
    It means you will have to proceed and investigate it.
    The line
    IF[ABS[[#5043-#116]-[#26]]GT#123]GOTO8 (ALARM PATH OBSTRUCTED)
    is the excerpt from program O9810. This logic statement's responsibility is to generate ALARM if machine does not arrive to target point.
    I will repeat the explanation of the meaning of the variables used in this statement:
    3.1 #5043 is Z axis position in current work coordinates. In order to verify it MDI #100=#5043 and check the #100.It should be equal to -.22 + probe tool length offset (G43 applied).
    3.2 #116 should be equal to probe tool length offset.
    3.3 #26 should be equal to commanded Z ie. -.22
    3.4 #123 set in O9724 as IN POSITION ZONE should be 0.002

    Run once more your program. When machine stops in ALARM, DO NOT RESET IT. In order to verify the content of variables #26, #116 and #123 press PROGRAM button.This will allow you to switch to OFFSET screen and then to MACRO.
    Once done, switch over to MDI, dial #100=#5043, execute and then verify the content of #100. Now you will be able to judge, which component of the statement causes the ALARM.

    Advise.

  13. #32
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    291
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    111

    Default

    Power outage got me thinking, maybe it's the receiver on the machine and not the program/probe? That would be effected by a power reset.

  14. #33
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by PROBE View Post
    It means you will have to proceed and investigate it.
    The line
    IF[ABS[[#5043-#116]-[#26]]GT#123]GOTO8 (ALARM PATH OBSTRUCTED)
    is the excerpt from program O9810. This logic statement's responsibility is to generate ALARM if machine does not arrive to target point.
    I will repeat the explanation of the meaning of the variables used in this statement:
    3.1 #5043 is Z axis position in current work coordinates. In order to verify it MDI #100=#5043 and check the #100.It should be equal to -.22 + probe tool length offset (G43 applied).
    3.2 #116 should be equal to probe tool length offset.
    3.3 #26 should be equal to commanded Z ie. -.22
    3.4 #123 set in O9724 as IN POSITION ZONE should be 0.002

    Run once more your program. When machine stops in ALARM, DO NOT RESET IT. In order to verify the content of variables #26, #116 and #123 press PROGRAM button.This will allow you to switch to OFFSET screen and then to MACRO.
    Once done, switch over to MDI, dial #100=#5043, execute and then verify the content of #100. Now you will be able to judge, which component of the statement causes the ALARM.

    Advise.
    Unfortunately I can't get MDI to work while the machine is in an alarm state.

    Quote Originally Posted by CNC Hacker View Post
    Power outage got me thinking, maybe it's the receiver on the machine and not the program/probe? That would be effected by a power reset.
    I've been thinking of replacing the receiver, but it's nearly impossible to get purchases approved with the corona virus going on.

  15. #34
    Join Date
    Oct 2013
    Location
    Hartford, CT
    Posts
    291
    Post Thanks / Like
    Likes (Given)
    190
    Likes (Received)
    111

    Default

    If you swapped probes between machines, the macros are the same between machines, and you're still getting the issue, it would suggest to me that the receiver/interface/etc is causing the problem on this machine.

  16. #35
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    604
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    152

    Default

    I would like to make some review on what we have here and summarize the information given in previous posts:
    1. Your program is:
    O1528
    #501=2.2129
    #502=.546
    #503=.555
    #504=.22
    M20
    B0
    T36M6(PROBE TOOL CHANGE)
    T205(PRE-CALL NEXT TOOL)
    G90G54.1P44(POSITION CALL)
    G0X0Y0(RAPID MOVE TO X,Y LOCATION)
    G43H36Z4.0(TOOL L COMP, H OFFSET, Z POSITION)
    M74(TURNS ON PROBE)
    M165P9810Z-.220F350.(PROBE POSITION MOVE) This is where is faults out.
    M165P9814D1.6430S145(MEASURES BORE - S STORES G54.1 P45)
    G0Z8.0(MOVES OUT PROBE)

    2. When the program is executed, the machine goes to X0Y0, then goes down to Z4, then it executes the PROTECTED MOVE going to Z-.22. Here the alarm occurs. This is exactly the same when program is repeated over and over again, excerpt of few runs after power outage.

    3. When tool length is changed to below 0.002, alarm is not raised.

    If all above is true, there is no problem with any of hardware elements.

    As written above, you must investigate why the sentence IF[ABS[[#5043-#116]-[#26]]GT#123]GOTO8 (ALARM PATH OBSTRUCTED) is generating the alarm. In order to do it, just for investigation purpose, edit program O9810: just before this crucial line add:
    #100=#5043
    M0

    This will allow you to check all the variables of the sentence and discover which is causing the problem.

    By the way, I just recalled, that in the past I was facing quite similar problems with another Doosan, which sometimes went crazy when double G43 command was executed. I would try to add G49 command just before G43 line.

  17. #36
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by PROBE View Post
    I would like to make some review on what we have here and summarize the information given in previous posts:
    1. Your program is:
    O1528
    #501=2.2129
    #502=.546
    #503=.555
    #504=.22
    M20
    B0
    T36M6(PROBE TOOL CHANGE)
    T205(PRE-CALL NEXT TOOL)
    G90G54.1P44(POSITION CALL)
    G0X0Y0(RAPID MOVE TO X,Y LOCATION)
    G43H36Z4.0(TOOL L COMP, H OFFSET, Z POSITION)
    M74(TURNS ON PROBE)
    M165P9810Z-.220F350.(PROBE POSITION MOVE) This is where is faults out.
    M165P9814D1.6430S145(MEASURES BORE - S STORES G54.1 P45)
    G0Z8.0(MOVES OUT PROBE)

    2. When the program is executed, the machine goes to X0Y0, then goes down to Z4, then it executes the PROTECTED MOVE going to Z-.22. Here the alarm occurs. This is exactly the same when program is repeated over and over again, excerpt of few runs after power outage.

    3. When tool length is changed to below 0.002, alarm is not raised.

    If all above is true, there is no problem with any of hardware elements.

    As written above, you must investigate why the sentence IF[ABS[[#5043-#116]-[#26]]GT#123]GOTO8 (ALARM PATH OBSTRUCTED) is generating the alarm. In order to do it, just for investigation purpose, edit program O9810: just before this crucial line add:
    #100=#5043
    M0

    This will allow you to check all the variables of the sentence and discover which is causing the problem.

    By the way, I just recalled, that in the past I was facing quite similar problems with another Doosan, which sometimes went crazy when double G43 command was executed. I would try to add G49 command just before G43 line.
    Unfortunately I don't have access to 9810. I tried changing 3202 NE9, but that didn't work.

    I tried adding G49 and it still alarmed out.

    Thank you for trying to help me out!

  18. #37
    Join Date
    Jan 2003
    Location
    Tel Aviv, Israel
    Posts
    604
    Post Thanks / Like
    Likes (Given)
    83
    Likes (Received)
    152

    Default

    Quote Originally Posted by fjs0001 View Post
    Unfortunately I don't have access to 9810. I tried changing 3202 NE9, but that didn't work.

    I tried adding G49 and it still alarmed out.

    Thank you for trying to help me out!
    I attach my version of protected move routine. If program number given by me is in use already, change it but do not use 9000 numbers. This will allow you, if necessary, to single block the program and to investigate the variables despite odd behavior of the control.

    %
    O6000(SNR PROTECT)
    #3004=0
    G90
    #123=0.002
    #116=#[11000+#4111]+#[10000+#4111]
    #117=200.
    N6010
    IF[#9NE#0]GOTO6001
    #9=0.6*#117
    N6001
    IF[#24NE#0]GOTO6002
    #24=#5041
    N6002
    IF[#25NE#0]GOTO6003
    #25=#5042
    N6003
    IF[#26NE#0]GOTO6004
    #26=#5043-#116
    N6004
    G31X#24Y#25Z#26F#9
    G53
    M0
    #4=#5061-#24
    #5=#5062-#25
    #6=#5063-#116-#26
    #29=SQRT[[#4*#4]+[#5*#5]+[#6*#6]]
    IF[#29LT#123]GOTO9999
    #3000=92(PATH OBSTRUCTED)
    N9999
    M99
    %

    Of course you will have to change the line
    G65P9810Z-0.22F350.
    To
    G65P6000Z-0.22F350.

    The M00 exists already in the program. If you wish to run it to the end and see if alarm is raised, just push another Cycle start.

  19. #38
    Join Date
    Jan 2007
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    1,030
    Post Thanks / Like
    Likes (Given)
    547
    Likes (Received)
    515

    Default

    Probe,
    On Doosan machines equipped with the RENGui interface, all Renishaw cycles are embedded in the macro executor. RENGui is a graphical front end for using most of the Renishaw cycles for setting of work offsets and minor inspection routines but cannot be done from a program. Most of Inspection Plus can be used with in process inspection using M165 to call programs from the macro executor. No one has access to these programs and they cannot be viewed or edited. I work for Doosan and deal with these on a daily basis. But I have never seen this scenario. The RENGui software is good and we have had this since about 2010. It works. We even have it for Marposs.


    M165 calls programs from the macro executor as opposed to G65 which calls programs from regular memory.

    Something is not right here and I am starting to think CNCHacker might be correct and it is a faulty receiver. Intermittent good/bad operation is a good indicator. This did work at one time and now it does not except for occasional success, especially after power down. At one time this worked on both of his machines, now it only works on one.

    One thing though. If the tool length offset for the probe is set to .002, the probe would crash if you turned on G43 with the adjusted tool length offset.

    Paul

  20. Likes CNC Hacker liked this post
  21. #39
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by PROBE View Post
    I attach my version of protected move routine. If program number given by me is in use already, change it but do not use 9000 numbers. This will allow you, if necessary, to single block the program and to investigate the variables despite odd behavior of the control.

    %
    O6000(SNR PROTECT)
    #3004=0
    G90
    #123=0.002
    #116=#[11000+#4111]+#[10000+#4111]
    #117=200.
    N6010
    IF[#9NE#0]GOTO6001
    #9=0.6*#117
    N6001
    IF[#24NE#0]GOTO6002
    #24=#5041
    N6002
    IF[#25NE#0]GOTO6003
    #25=#5042
    N6003
    IF[#26NE#0]GOTO6004
    #26=#5043-#116
    N6004
    M184
    G31X#24Y#25Z#26F#9
    G53
    M0
    #4=#5061-#24
    #5=#5062-#25
    #6=#5063-#116-#26
    #29=SQRT[[#4*#4]+[#5*#5]+[#6*#6]]
    IF[#29LT#123]GOTO9999
    #3000=92(PATH OBSTRUCTED)
    N9999
    M99
    %

    Of course you will have to change the line
    G65P9810Z-0.22F350.
    To
    G65P6000Z-0.22F350.

    The M00 exists already in the program. If you wish to run it to the end and see if alarm is raised, just push another Cycle start.
    The machine didn't alarm out using your program. I don't know what that means though.

  22. #40
    Join Date
    Jun 2020
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    20
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by LockNut View Post

    One thing though. If the tool length offset for the probe is set to .002, the probe would crash if you turned on G43 with the adjusted tool length offset.

    Paul
    I moved the positions out so that the probe wouldn't crash.


Tags for this Thread

Bookmarks

Posting Permissions

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