Tool offset not working
Close
Login to Your Account
Results 1 to 20 of 20
  1. #1
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    246
    Post Thanks / Like
    Likes (Given)
    44
    Likes (Received)
    30

    Default Tool offset not working

    Havent used my lathe for a couple of weeks.

    Some reason the tool offset isnt working. Weird. I am dialing in a new program and need to change the offset slightly to hit my dimension but nothing happens.

    Everything else seems fine, just this strange issue. 3TD fanuc

    Double checked the code, and that im keying it in correctly.
    Any ideas where to look? ive run out of them!

  2. #2
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,274
    Post Thanks / Like
    Likes (Given)
    4804
    Likes (Received)
    1651

    Default

    You aren't able to change the valve in offset table? Or the control isn't applying the offset value registered? Either way odd

    Brent

  3. #3
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,274
    Post Thanks / Like
    Likes (Given)
    4804
    Likes (Received)
    1651

    Default

    I know this isn't a fix but a work around so you can run it could be to tweak the G50 by the incremental value needed to dial in size?

    Brent

  4. #4
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    246
    Post Thanks / Like
    Likes (Given)
    44
    Likes (Received)
    30

    Default

    Brent, i should have been a bit clearer.

    The control isn't applying the offset value. Keys in fine.

    I went through the parameters also, everything is as i noted. Yes i have a copy written down.

  5. #5
    Join Date
    May 2007
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    1,435
    Post Thanks / Like
    Likes (Given)
    486
    Likes (Received)
    1236

    Default

    That seems strange. The first thing I would do is check my tool call code that it's calling the tool up with the proper offset. Then I would rule out the machine by giving the tool offset and absurd plus offset like .250 and watch the cycle for that tool not even come close to the cut. That tells me the tool table is responding.

    I have had cases during set up when my rough turn tool was cutting just under the finish size and I was chasing the finish tool offset because I could not see it taking a chip.

    Good luck.

    Make Chips Boys !

    Ron

  6. Likes Bobw, TeachMePlease liked this post
  7. #6
    Join Date
    Apr 2018
    Country
    UNITED STATES MINOR OUTLYING ISLANDS
    Posts
    3,973
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1794

    Default

    Quote Originally Posted by Dupa3872 View Post
    That seems strange.
    It's not strange, it's impossible. Whenever something likes this happens, the control is correct, the human is wrong. Controls don't refuse to pick up offsets. He's doing something wrong.

  8. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,851
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1537

    Default

    Quote Originally Posted by EmanuelGoldstein View Post
    It's not strange, it's impossible. Whenever something likes this happens, the control is correct, the human is wrong. Controls don't refuse to pick up offsets. He's doing something wrong.
    Not so. Although issues such as this are predominately program and programmer centric, indeed it can be a control issue. I'm currently working with a client to resolve a very similar issue. The control is randomly not applying the X axis Geometry Offset and the program is unequivocally correct.

    When this event occurs, the error occurs repeatedly on the same tool, irrespective of any Reset or Manual Reference Return, or re-registering of the Offset as a possible fix. Recycling the power to the control has consistently resulted in a fix on the next cycle, but the same error generally occurs after the next few cycles and is random with regards to the tool the error occurs with.

    The error never occurs on the Z axis, giving further weight to the fact that the Offsets (Geometry and Wear) are being called correctly in the program.

  9. #8
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    5,082
    Post Thanks / Like
    Likes (Given)
    4634
    Likes (Received)
    3064

    Default

    Quote Originally Posted by Kenre View Post
    Havent used my lathe for a couple of weeks.

    Some reason the tool offset isnt working. Weird. I am dialing in a new program and need to change the offset slightly to hit my dimension but nothing happens.

    Everything else seems fine, just this strange issue. 3TD fanuc

    Double checked the code, and that im keying it in correctly.
    Any ideas where to look? ive run out of them!
    Can you show us a snippet of your program? Are you SURE the offset is being called up?

  10. #9
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,061
    Post Thanks / Like
    Likes (Given)
    908
    Likes (Received)
    2732

    Default

    Quote Originally Posted by angelw View Post
    Not so. Although issues such as this are predominately program and programmer centric, indeed it can be a control issue. I'm currently working with a client to resolve a very similar issue. The control is randomly not applying the X axis Geometry Offset and the program is unequivocally correct........
    Hi Bill, Can you post the model and firmware version (assuming it is Fanuc)? I'd like to look at my model-firmware info to see if it shows up as something odd.

  11. #10
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    246
    Post Thanks / Like
    Likes (Given)
    44
    Likes (Received)
    30

    Default

    No picking on it! its works, messy but been using the same layout with all my other codes.

    N30 G00 G98
    N40 G21
    N50 G28 U0. W0.
    N60 G50 X-199.00 Z420.0 S1700

    N70 (FACE5)
    N80 T0404
    N90 M42
    N100 M08
    N110 G98
    N120 G97 S1595 M03
    N130 G00 X-79.84 Z149.92
    N140 G50 S2000
    N150 G96 S400 M03
    N160 G00 Z1.334
    N170 X-59.84
    N180 G01 X-52.67 F400.
    N190 X-49.84 Z-0.08
    N200 X1.76
    N210 X-1.07 Z1.334
    N220 G00 X-79.84
    N230 Z100.
    N240 G97 S1595 M03
    N250 M09
    N260 G28 U0.

    N270 (PROFILE ROUGHING2)
    N280 M01
    N290 M08
    N300 G98
    N310 G97 S1823 M03
    N320 G00 X-69.84 Z149.92
    N330 G50 S2000
    N340 G96 S400 M03
    N350 G00 Z0.92
    N360 X-49.44
    N370 G01 Z-41.58 F400.
    N380 X-51.84
    N390 G00 Z0.92
    N400 X-47.04
    N410 G01 Z-25.964 F400.
    N420 G02 X-47.65 Z-26.173 R1.
    N430 G01 X-48.65 Z-26.673

    Just check the offset in tool 3 my centre drill running in the program, working perfect. even adjusted it .001 and re checked it, all ok there.

    Most likely something in the code, but i cant see it. Will try another offset number and reset tool 4 to see if its a code or machine prob.

  12. #11
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    902
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    326

    Default

    Quote Originally Posted by Kenre View Post
    No picking on it! its works, messy but been using the same layout with all my other codes.

    N30 G00 G98
    N40 G21
    N50 G28 U0. W0.
    N60 G50 X-199.00 Z420.0 S1700

    N70 (FACE5)
    N80 T0404
    N90 M42
    N100 M08
    N110 G98
    N120 G97 S1595 M03
    N130 G00 X-79.84 Z149.92
    N140 G50 S2000
    N150 G96 S400 M03
    N160 G00 Z1.334
    N170 X-59.84
    N180 G01 X-52.67 F400.
    N190 X-49.84 Z-0.08
    N200 X1.76
    N210 X-1.07 Z1.334
    N220 G00 X-79.84
    N230 Z100.
    N240 G97 S1595 M03
    N250 M09
    N260 G28 U0.

    N270 (PROFILE ROUGHING2)
    N280 M01
    N290 M08
    N300 G98
    N310 G97 S1823 M03
    N320 G00 X-69.84 Z149.92
    N330 G50 S2000
    N340 G96 S400 M03
    N350 G00 Z0.92
    N360 X-49.44
    N370 G01 Z-41.58 F400.
    N380 X-51.84
    N390 G00 Z0.92
    N400 X-47.04
    N410 G01 Z-25.964 F400.
    N420 G02 X-47.65 Z-26.173 R1.
    N430 G01 X-48.65 Z-26.673

    Just check the offset in tool 3 my centre drill running in the program, working perfect. even adjusted it .001 and re checked it, all ok there.

    Most likely something in the code, but i cant see it. Will try another offset number and reset tool 4 to see if its a code or machine prob.

    Your using a g50 for your x shift, then you cancel it with the g28 z0.0
    then you dont have it for the second time around. take it out and put is after then end of the tool.
    it could also be you dont have a g00 before your tool call out. IE G00T0404

    is this hand written code or form a cad system as the code looks really sloppy and confusing. I would edit your post to make the code easier to read. but tahst just me

  13. Likes Kenre liked this post
  14. #12
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    246
    Post Thanks / Like
    Likes (Given)
    44
    Likes (Received)
    30

    Default

    Bingo! You found it Delw!

    N260 G28 U0. should only be used when i change tools. Deleted it and now i can change the offset.

    Its code from Fusion360, then edited in Dnc4u to make it work with 3T.

    Thankyou very much Delw !! Legend!!

  15. #13
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,851
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1537

    Default

    Quote Originally Posted by Vancbiker View Post
    Hi Bill, Can you post the model and firmware version (assuming it is Fanuc)? I'd like to look at my model-firmware info to see if it shows up as something odd.
    Hello Kevin,
    I hope you're keeping well.

    It may be some time before I get back to see the machine, as we are just about at total lock down, due to Covid-19. Accordingly, I can't tell you the firmware version, but the Control is a 10TE-F.

    Best regards,

    Bill

  16. #14
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,061
    Post Thanks / Like
    Likes (Given)
    908
    Likes (Received)
    2732

    Default

    Hi Bill,

    Thanks. Yes I'm well and lying low till the Covid 19 blows over. Hope the same for you. Got a few boat parts to make, keeping me in the shop a fair bit of the time.

    Don't worry about the firmware info. My notes only go back to the 15 and 0 series. I'm surprised about a firmware bug, if it is one, in a 10 series. That has been around long enough and enough made that I would have thought it would have shown long ago.

    Kevin

  17. #15
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    122
    Post Thanks / Like
    Likes (Given)
    309
    Likes (Received)
    41

    Default

    Why are your X values negative?

  18. #16
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,061
    Post Thanks / Like
    Likes (Given)
    908
    Likes (Received)
    2732

    Default

    Quote Originally Posted by Fancuku View Post
    Why are your X values negative?
    Old Mori Seiki were set up that way.

  19. #17
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    2,646
    Post Thanks / Like
    Likes (Given)
    371
    Likes (Received)
    745

    Default

    If you are going to use the G50, I would suggest using a G50 return to your start position rather than the G28.
    Just the way I was taught. It's a lot easier to troubleshoot a program if you do, and you have control over where the tool goes.

  20. Likes yardbird, Larry Dickman liked this post
  21. #18
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,274
    Post Thanks / Like
    Likes (Given)
    4804
    Likes (Received)
    1651

    Default

    Quote Originally Posted by Dan from Oakland View Post
    If you are going to use the G50, I would suggest using a G50 return to your start position rather than the G28.
    Just the way I was taught. It's a lot easier to troubleshoot a program if you do, and you have control over where the tool goes.
    Dan, I agree with what you just said and that is how I was taught too. But if your going to set your G50's and run from zero return then I don't know what difference it would make?

    When running closer or from somewhere other than zero return then the return positioning G50 I see as a necessity.

    Brent

  22. Likes Dan from Oakland liked this post
  23. #19
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    902
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    326

    Default

    I have to run g50's on my citizen with a 10T control.
    well I dont have to I do to keep my offset numbers close to 0 on the x tools. I only have one offset page dont have wear offsets and geometry offsets.

    I run the g50 at the start of the tool and cancel it at the end of that tool. for every tool that needs it in the x axis. my g50s are only in 1 place decimals like g50 U0.8 U0.2 etc then cancel it with a g50 U-0.8 U-0.2 etc etc. save the other places for the offset page.
    at the end of my program I do a g28 u0.0. I have a short stroke and 2 turrets so its not huge problem to send it back.
    I have a ton of tools so all my tools are tagged with the g50 number in both U and W. when I change them out I know what U and W to use and make sure my saved program has those numbers in before I run it.

    when I was running big machines like above and bigger back in the day we used g50s the same way but didnt send the U and W home cause it was 30"- hundred inchs or so. in the am we would take the machine home and run a sub with the stored G50 u and w numbers that one time and be done with it until the machine was shut down or power went out.

  24. #20
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    246
    Post Thanks / Like
    Likes (Given)
    44
    Likes (Received)
    30

    Default

    I haven't got my head around the finer details of code. 3T uses G50 for part position as you know.
    I know the G28 U0 sends the turret up out of the way for tool changes. I can specify in Fusion the return in Z for clearance, rather important with a long drill or boring bar!

    This is the first and only CNC lathe ive ever run. Self taught with lots of help from here Im getting great parts so very happy!


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
  •