G71... Please help! What is wrong with this program?
Close
Login to Your Account
Page 1 of 5 123 ... LastLast
Results 1 to 20 of 83
  1. #1
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default G71... Please help! What is wrong with this program?

    Hello All,

    Iíve got an issue with my G71 roughing program. I have scratched my head and looked and I just donít see what the problem is? First run of this new program, everything is going just as it should until the very last roughing pass. It comes down the angle then swings the 4Ē radius then comes a cross the 1Ēdia. but instead of swinging the .38rad it plunged right into the shoulder. WTF? No I didnít run it through the graph or out in dry land first.

    Iíve attached some pictures of my drawing and the actual program and the end result. If someone could help me figure out what the deal is here I'd greatly appreciate it. At this point Iím going to go in and run the same program out in dry land and see if it does it again.

    Other than that I got nothing. I hope you can see the drawing and pictures? The exact code is at the bottom.

    Thank YouÖ.

    Brent





    help-1.jpg
    20171127_223355.jpg
    help-2.jpg


    N30(ROUGH OD)
    G0G99G40G54X14.Z10.T0
    T0303
    M41
    G97S150M4
    G0X3.5Z.1M8
    G50S700
    G96S450
    G71U.05R.05
    G71P31Q32U.03W.003F.012
    N31G1X1.4854Z.0000
    G3X1.4950Z-.0063R.005
    G1X1.2726Z-.4213
    G2X1.0000Z-1.4566R4.
    G1X1.0000Z-2.0100
    G2X1.7600Z-2.3900R.38
    G1X2.9400Z-2.3900
    G1X3.0000Z-2.4200
    G1X3.0000Z-3.3160
    N32G1X3.5
    M9
    G0G99G40G54X14.Z10.T0
    M1

  2. #2
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,070
    Post Thanks / Like
    Likes (Given)
    221
    Likes (Received)
    834

    Default

    I guess you have confirmed you have a type 2 control and can turn reducing diameters in G71?

    N31 G0 X1.485 Z.1
    G1 Z0.0 F.006
    G3 X1.495... etc...

  3. #3
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    Quote Originally Posted by jancollc View Post
    I guess you have confirmed you have a type 2 control and can turn reducing diameters in G71?

    N31 G0 X1.485 Z.1
    G1 Z0.0 F.006
    G3 X1.495... etc...
    Thanks! Fanuc 0i-td I've used type 2 roughing many times.

    The thing is I was standing right there watching it run, small DOC for fist part, it roughed down to the 1 1/2" on the end, then started carving out the concave portion, everything looking good. Multiple stabs on the .38rad, all is good until the very last pass, I watched it sweep the 4" radius and come across at 1.03". It got to the start point of the .38rad and the sumbitch just plunged right into the shoulder. WTF? I'm stumped....

    Brent

    20171127_224809.jpg
    Last edited by yardbird; 11-28-2017 at 12:59 PM. Reason: fixed stuff...

  4. #4
    Join Date
    Nov 2017
    Country
    UNITED STATES
    State/Province
    California
    Posts
    28
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    7

    Default

    I back plotted your program, looks good here

    back-plot.jpg

  5. Likes yardbird liked this post
  6. #5
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,070
    Post Thanks / Like
    Likes (Given)
    221
    Likes (Received)
    834

    Default

    Quote Originally Posted by yardbird View Post
    ...It got to the start point of the .38rad and the sumbitch just plunged right into the shoulder. WTF? I'm stumped....
    Your start of profile looks funky to me. The first line after the P address block should be a G1 Z0.0 move at the min X dia., with the feedrate for the G70 pass, and the P block should be a G0 to the X Min with to the same Z position as the start position.

    I'd make those edits and run it in air to see what it does.

  7. Likes yardbird, B-Mathews liked this post
  8. #6
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    Quote Originally Posted by Kleinfeldt View Post
    I back plotted your program, looks good here

    back-plot.jpg
    Thank you! I'm not seeing anything wrong with the tool path either.

    Brent

  9. Likes Kleinfeldt liked this post
  10. #7
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    Quote Originally Posted by jancollc View Post
    Your start of profile looks funky to me. The first line after the P address block should be a G1 Z0.0 move at the min X dia., with the feedrate for the G70 pass, and the P block should be a G0 to the X Min with to the same Z position as the start position.

    I'd make those edits and run it in air to see what it does.
    First thing I'm going to do is run the exact same program again watching it on the graph. I'm not trying to be argumentative but I've run that same roughing routine a thousand times but I'm willing to give your suggestions a shot. %99.9999 it's my fault, on very few occasions over the past 29yrs have I thought the machine had a brain fart, this is one of them. IDK? Thanks again...

    Brent

  11. Likes Kleinfeldt liked this post
  12. #8
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    @jancollc,

    Firs two pictures are the rough and finish as I had it. Changed program to like 3rd picture, results are in 4th picture. I truly don't know why but you nailed it. Thank you for your help!



    Can anyone explain exactly what the deal is here? I believe this is the second time this has happened to me and I've written hundreds of programs using this roughing template but I'm changing that today. This could have been really ugly if I wasn't close. Brain fart? Lol....

    Brent

    20171128_162609.jpg
    20171128_162837.jpg
    20171128_164814.jpg
    20171128_164729.jpg

  13. #9
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,629
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    1595

    Default

    Wow!!!

    Although I always position my tool in Z ( or X for G72 ) in the same position as the P block, but would have never thought it to be of an issue
    for the control...

    As you have gotten me very curious, in a few hours I'll load your program into an OiTC and a Haas and see if they behave the same.

  14. #10
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    Jacked up my holder also.

    Brent

    20171128_171514-1.jpg

  15. #11
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    Quote Originally Posted by SeymourDumore View Post
    Wow!!!

    Although I always position my tool in Z ( or X for G72 ) in the same position as the P block, but would have never thought it to be of an issue
    for the control...

    As you have gotten me very curious, in a few hours I'll load your program into an OiTC and a Haas and see if they behave the same.
    That would be great! Thanks...

    I had this one other time a while back using G72 but never asked about it then.

    Brent

    20151024_211133.jpg

  16. #12
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,070
    Post Thanks / Like
    Likes (Given)
    221
    Likes (Received)
    834

    Default

    Quote Originally Posted by SeymourDumore View Post
    Wow!!!

    Although I always position my tool in Z ( or X for G72 ) in the same position as the P block, but would have never thought it to be of an issue for the control...
    On the type 1 G71 where diameter is increasing, you don't even need a Z position on the P block. It will just use the Z start position. On the type 2 you need the Z position.

    In both types, the next line has to be the G1 Z-axis feed to the start of profile. It can't be a G3.

    At least, them's the rules as I understand them...

  17. #13
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    OK so I run the exact same program in post 8 the new improved version except I change the DOC from .15 to .05 and this is the results. I shit you not!

    20171128_181619.jpg

    20171128_181543.jpg

    Then change the DOC to .1 and run again and then this? What's up with that?

    20171128_182345.jpg

    OK now just for shits and giggles I changed the program back to my original program as it is listed in the OP but increase the DOC from .05 to .1 and got this.

    20171128_183838.jpg

    If anyone else besides SeymourDumore has the time and could test this on their machine it'd be interesting to see if yours acts the same as mine.

    Something funky is going on and appears to have to do with the DOC and not necessarily the start block of the cycle? IDK I got nothing...

    Brent

  18. #14
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,629
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    1595

    Default

    Yard

    I've just ran this in the Haas:

    %
    O00100
    G28
    G50 S700
    G00 G99 G40 G54
    G00 G97 T202 S150 M03
    G00 X3.5 Z0.1
    G96 S450
    G71 D0.05 P31 Q32 U0.03 W0.003 F0.012
    N31 G01 X1.4854 Z0.
    G03 X1.495 Z-0.0063 R0.005
    G01 X1.2726 Z-0.4213
    G02 X1. Z-1.4566 R4.
    G01 X1. Z-2.01
    G02 X1.76 Z-2.39 R0.38
    G01 X2.94 Z-2.39
    G01 X3. Z-2.42
    G01 X3. Z-3.316
    N32 G01 X3.5
    M09
    M05
    G28
    M30
    %

    And it ran perfectly!
    Note that Haas uses the single line G71 so that's the only difference but it should not matter.
    I've tried a few different DOC-s, all was well.
    It looks like that when your control roughs out the tapered section, it wants to ( for some odd reason ) rapid to the end of the path
    without making a final smoothing pass.
    On the Haas, after the taper is done, it rapids up-to start-X ( X3.5 ), then to start Z ( Z.1 ) and then skims the whole profile from there leaving .03 in X, .003 in Z.
    Your control looks like wants to rapid to StartX and End Z instead ....

    The Fanuc is still tied up with a job due tomorrow, but I'll plop it into it as soon as I can because I do want to know!

  19. #15
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,629
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    1595

    Default

    Quote Originally Posted by yardbird View Post
    OK so I run the exact same program in post 8 the new improved version except I change the DOC from .15 to .05 and this is the results. I shit you not!
    Dude, there IS something funky going on there!

    On the Haas I get something like this:

    Quote Originally Posted by yardbird View Post
    20171128_182345.jpg
    The only thing changes with the DOC variation is where it rapids up to Start-X before the smoothing.

  20. #16
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    Quote Originally Posted by SeymourDumore View Post
    Yard

    I've just ran this in the Haas:

    %
    O00100
    G28
    G50 S700
    G00 G99 G40 G54
    G00 G97 T202 S150 M03
    G00 X3.5 Z0.1
    G96 S450
    G71 D0.05 P31 Q32 U0.03 W0.003 F0.012
    N31 G01 X1.4854 Z0.
    G03 X1.495 Z-0.0063 R0.005
    G01 X1.2726 Z-0.4213
    G02 X1. Z-1.4566 R4.
    G01 X1. Z-2.01
    G02 X1.76 Z-2.39 R0.38
    G01 X2.94 Z-2.39
    G01 X3. Z-2.42
    G01 X3. Z-3.316
    N32 G01 X3.5
    M09
    M05
    G28
    M30
    %

    And it ran perfectly!
    Note that Haas uses the single line G71 so that's the only difference but it should not matter.
    I've tried a few different DOC-s, all was well.
    It looks like that when your control roughs out the tapered section, it wants to ( for some odd reason ) rapid to the end of the path
    without making a final smoothing pass.
    On the Haas, after the taper is done, it rapids up-to start-X ( X3.5 ), then to start Z ( Z.1 ) and then skims the whole profile from there leaving .03 in X, .003 in Z.
    Your control looks like wants to rapid to StartX and End Z instead ....

    The Fanuc is still tied up with a job due tomorrow, but I'll plop it into it as soon as I can because I do want to know!
    Thank you! It's crazy to me that regardless of how the start P block is defined the DOC seems to be the determining factor on weather it screws up or not. In my mind this should not matter. I'd be interested in how your test come out on your Fanuc control? If you should get the same results try playing with the DOC and see if that changes the nasty move on the last pass?

    Thanks again I appreciate it!

    Brent

  21. #17
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,629
    Post Thanks / Like
    Likes (Given)
    255
    Likes (Received)
    1595

    Default

    Brent

    Now that I look at your graphs, it doesn't even rapid to the end, rather into oblivion in Z!
    Almost looks like it wants to finish that 4" radius circle in full!!

    Interesting that it doesn't alarm out with a Z-overtravel.
    Don't know how Fanuc does the backplot, but Haas takes all travel limits into consideration and it throws a fit if the move
    would go beyond the limit, BEFORE!!! it even starts the path.
    Ditto in real running mode. If the programmed path goes beyond the travel limit, it will stop a few blocks ahead!

  22. Likes yardbird liked this post
  23. #18
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    Quote Originally Posted by SeymourDumore View Post
    Dude, there IS something funky going on there!

    On the Haas I get something like this:



    The only thing changes with the DOC variation is where it rapids up to Start-X before the smoothing.
    Not only funky but dangerous too, this fucked my stuff up and could have been a lot worse, I do hope you test this on your Fanuc 0i control and you get to see this shit with your own eyes. It appears by looking at the graph and seeing it running that the last jacked up move is a radius?

    I somehow feel if I was to zoom out and let it finish the roughing cycle complete you'd see an 8 inch circle on the graph? Tomorrow I'm going to rerun the cycle with the apparently wrong DOC and let it run complete, I have a feeling there will be an 8 inch circle when it finishes?

    BTW I increased the DOC so as to not have this problem on this particular run and I'm now using the tailstock to support the end.

    Brent

  24. #19
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    2,941
    Post Thanks / Like
    Likes (Given)
    4316
    Likes (Received)
    1474

    Default

    Quote Originally Posted by SeymourDumore View Post
    Brent

    Now that I look at your graphs, it doesn't even rapid to the end, rather into oblivion in Z!
    Almost looks like it wants to finish that 4" radius circle in full!!
    That is exactly how it appears. If you look at graphs you can see the changes to the P start block. I feel this is a something totally unrelated? Hell IDK?

    Brent

  25. #20
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,123
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1219

    Default

    Hello Brent,
    Re-post the program using I/K Circular Interpolation Format and test to see if you still have the issue.

    Regards,

    Bill


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
  •