584,874 active members*
5,234 visitors online*
Register for free
Login
Results 1 to 16 of 16
  1. #1
    Join Date
    Sep 2009
    Posts
    13

    G71 Errors.....

    Anybody have problems with G71 on a Yasnac LX3 Control? Here's a sample program....

    O0004;
    N001 G40 G20;
    N002 G50 S3500;
    N003 G96 S500 M3;
    N004 G41 T0505;
    N005 G0 X1.15 Z-9.5 M8;
    N006 G71 P7 Q14 U.01 W.01 D.015 F.005 S500;
    N007 G0 X.125 S750;
    N008 G1 W-.2 F.004;
    N009 G12 X1.0625 K-.09375;
    N010 G1 W-.85;
    N011 G2 X.7625 W-.15 I0.0 K-.15;
    N012 X1.0265 W-.15 I.15 K0.0;
    N013 G1 W-.975;
    N014 X1.15;
    N015 G70 P7 Q14;
    N016 G0 G40 X8.0 Z-4.0 M9;
    N017 M30;

    It runs ok till somewhere's near 'N009' during the finish cut (G70)..... then throws "Alarm 048" which is "PROG ERROR (G41-44) INTERSECTION POINT NOT OBTAINED BY INTERSECTION COMPUTATION".... What am I overlooking???

    Then on another related problem....
    Every time I try to cut a concave profile (diameter steps down then back out) on a part using G71 it takes the concave in one pass....
    Daniel

  2. #2
    Join Date
    Feb 2006
    Posts
    992
    Basicly the end point and the arc is not match, program revise is need.
    Attached Thumbnails Attached Thumbnails Untitled.png  
    The best way to learn is trial error.

  3. #3
    Join Date
    Mar 2003
    Posts
    2932
    Quote Originally Posted by drdfab View Post
    Anybody have problems with G71 on a Yasnac LX3 Control? Here's a sample program....

    O0004;
    N001 G40 G20;
    N002 G50 S3500;
    N003 G96 S500 M3;
    N004 G41 T0505;
    N005 G0 X1.15 Z-9.5 M8;
    N006 G71 P7 Q14 U.01 W.01 D.015 F.005 S500 R1; <-- Add R1 here
    N007 G0 X.125 S750;
    N008 G1 W-.2 F.004;
    N009 G12 X1.0625 K-.09375;
    N010 G1 W-.85;
    N011 G2 X.7625 W-.15 I0.0 K-.15;
    N012 X1.0265 W-.15 I.15 K0.0; <---- Should this be X1.0625 not X1.0265?
    N013 G1 W-.975;
    N014 X1.15;
    N015 G70 P7 Q14;
    N016 G0 G40 X8.0 Z-4.0 M9;
    N017 M30;

    It runs ok till somewhere's near 'N009' during the finish cut (G70)..... then throws "Alarm 048" which is "PROG ERROR (G41-44) INTERSECTION POINT NOT OBTAINED BY INTERSECTION COMPUTATION".... What am I overlooking???

    What does this shape look like?
    I think there may be a typo in N012... X1.0625 and W0?


    Then on another related problem....
    Every time I try to cut a concave profile (diameter steps down then back out) on a part using G71 it takes the concave in one pass....
    I believe you need to specify a Type II roughing by putting an R1 in the G71 block.

  4. #4
    Join Date
    Sep 2009
    Posts
    13
    Thanks abunch..... the "R1" did the trick on the 'plunging to the bottom first pass' problem....

    But it still throws the alarm code 048 about one block before the G2 area during the finishing cut (G70).... So why would the control be able the rough out the part (even the radius) and not be able to finish it???
    Daniel

  5. #5
    Join Date
    Sep 2009
    Posts
    13
    By the way..... the typo in my program was my mistake in typing here online.... it really is correct in my control.... it should read X1.0625 as dcoupar pointed out....

    I am trying to cut a full radius groove (.150" radius x .150" deep) on my shaft... not sure if this helps any.... :-)
    Daniel

  6. #6
    Join Date
    Mar 2003
    Posts
    2932
    Quote Originally Posted by drdfab View Post
    Thanks abunch..... the "R1" did the trick on the 'plunging to the bottom first pass' problem....

    But it still throws the alarm code 048 about one block before the G2 area during the finishing cut (G70).... So why would the control be able the rough out the part (even the radius) and not be able to finish it???


    Maybe I'm reading it wrong, but I would think the G41 in N004 should be G42. I believe G41 and G42 are ignored during the G71 roughing.

  7. #7
    Join Date
    Sep 2009
    Posts
    13
    Quote Originally Posted by dcoupar View Post
    Maybe I'm reading it wrong, but I would think the G41 in N004 should be G42. I believe G41 and G42 are ignored during the G71 roughing.
    The funny thing is that the program won't run any different even without tool nose comp..... still just throws the same alarm same place..... :-(
    Daniel

  8. #8
    Join Date
    Mar 2003
    Posts
    2932
    Can you punch out the program from the machine and post it here?

  9. #9
    Join Date
    Sep 2009
    Posts
    13
    %
    O0004;
    N001 G40 G20;
    N002 G50 S3500;
    N003 G96 S500 M3;
    N004 G41 T0505;
    N005 G0 X1.15 Z-9.5 M8;
    N006 G71 P7 Q14 U.01 W.01 I.005 K.010 D.015 F.005 S500 R1;
    N007 G0 X.125 S750;
    N008 G1 W-.2 F.004;
    N009 G12 X1.0625 K-.09375;
    N010 G1 W-.85;
    N011 G22 X.7625 W-.15 R.15;
    N012 X1.0625 W-.15 R.15;
    N013 G1 W-.975;
    N014 X1.15;
    N015 G70 P7 Q14;
    N016 G0 G40 X8.0 Z-4.0 M9;
    N017 M30;
    %
    Daniel

  10. #10
    Join Date
    Mar 2003
    Posts
    2932
    My mistake about the G41... it's been a while since I've programmed a Yasnac... sorry.
    Will it run through the program if you delete the G41?
    Also, the book says "The T code for tool nose radius compensation must be programmed with a sign (+ or -). Have you tried it with T+0505?

  11. #11
    Join Date
    Sep 2009
    Posts
    13
    Yup.... tried with and without plus signs.... tried it without tool nose comp at all.... always the same error code at the same place...
    Daniel

  12. #12
    Join Date
    Feb 2006
    Posts
    992
    post your part geometry, I want to see it. I see you have G12 in the program...... auto chamfer????
    The best way to learn is trial error.

  13. #13
    Join Date
    Mar 2003
    Posts
    2932
    G11 is chamfering, G12 is rounding.

  14. #14
    Join Date
    Mar 2003
    Posts
    2932
    On a general note, in your G71 block you specify finishing allowance in Z (W and K). Normally you wouldn't specify Z finish allowance with R1 type roughing, as it will shift the roughing cuts + Z, in this case 0.015 and overcut the back side prior to finishing.

    N006 G71 P7 Q14 U.01 I.005 D.015 F.005 S500 R1; <-- remove W and K

  15. #15
    Join Date
    Sep 2009
    Posts
    13
    Sorry for the delay in getting the geometry posted... been swamped in the shop and have not had time to do any computer work..... here's a pic of the part..... i was going to turn it out using a all round insert with .125 radius but may have to get a different tool as G71 does not apply cutter comp to roughing passes.....
    Attached Thumbnails Attached Thumbnails First Turning Operation.jpg  
    Daniel

  16. #16
    Join Date
    Feb 2006
    Posts
    992
    With the geometry you got...... nothing wrong with your program or idea, but G71 is not that smart like you expect, that's all she wrote and G71 have trouble with that's kind of pocket. Diffrent solution for the pocket is need, unless if you have Mazak(other brand can, I just know will) then that's possible with the way you programmed .......
    The best way to learn is trial error.

Similar Threads

  1. Errors #1,#16,#17
    By masterfabr in forum Fadal
    Replies: 9
    Last Post: 01-14-2010, 03:55 AM
  2. Errors on Arc in Mach
    By MichaelHenry in forum Tormach Personal CNC Mill
    Replies: 11
    Last Post: 10-24-2009, 12:38 AM
  3. mazatrol t1 errors
    By beno in forum Mazak, Mitsubishi, Mazatrol
    Replies: 7
    Last Post: 10-05-2009, 11:21 PM
  4. Getting 2 Errors.... Someone Please!!
    By DesKitchens in forum Commercial CNC Wood Routers
    Replies: 0
    Last Post: 09-14-2009, 02:30 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
  •