YASNAC Program Issue

Results 1 to 13 of 13

Thread: YASNAC Program Issue

  1. #1
    Member Bubby44's Avatar
    Join Date
    Jan 2020
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default YASNAC Program Issue

    Hello,

    I'm running a Kia KT-21 with a Yasnac LX-1 Interface. I'm trying to proof a program and it will not process the canned cycles I have written. I've been through it and based on other programs that have been run through the machine, I should not have a syntax error. I will run up to the G71 code of the canned cycles and then stop it dead in its tracks, or it will skip these lines entirely and continue on. The rest of the program runs through smoothly. Any Suggestions are greatly appreciated.

    Thank you

    Jake

    Similar Threads:
    Attached Thumbnails Attached Thumbnails YASNAC Program Issue-sample-prog-png  


  2. #2
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    263
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    your G42 maybe on the wrong line. try it on line 10. Also, is your Tool Tip position correct?
    CNC Lathe Tool Nose Radius Compensation - CNC Training Centre

    Last edited by machinehop5; 01-06-2020 at 08:31 PM. Reason: link add


  3. #3
    Member Bubby44's Avatar
    Join Date
    Jan 2020
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    Quote Originally Posted by machinehop5 View Post
    your G42 maybe on the wrong line. try it on line 10. Also, is your Tool Tip position correct?
    CNC Lathe Tool Nose Radius Compensation - CNC Training Centre
    I believe the tool tip position is correct. This system uses G50 codes for positioning, which I'd never dealth with before at my previous shop. The tool approach looks correct for the rest of the program.



  4. #4
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    263
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    Quote Originally Posted by Bubby44 View Post
    I should not have a syntax error.
    Line 6 & 42 looks odd to me..."G50 X5. Z5." is this possibly the syntax you spoke of ?

    Last edited by machinehop5; 01-07-2020 at 12:42 AM. Reason: 42


  5. #5
    Member Bubby44's Avatar
    Join Date
    Jan 2020
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    Quote Originally Posted by machinehop5 View Post
    your G42 maybe on the wrong line. try it on line 10. Also, is your Tool Tip position correct?
    CNC Lathe Tool Nose Radius Compensation - CNC Training Centre
    I tried moving the G42, it just skipped over the cycle again.

    Quote Originally Posted by machinehop5 View Post
    Line 6 & 42 looks odd to me..."G50 X5. Z5." is this possibly the syntax you spoke of ?
    That is the preset that BobCAD generated, we changed the X and Z to the position of the the tool at zero relative to the work. Neither of us have worked with G50 positioning before, this is our first time using this lathe. Since no one uses G50 anymore, the few instructional's I've read and videos I've watched haven't been all that clear or helpful.



  6. #6
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    263
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    Try changing Line 6 from G50 X5. Z5. to G92 X5. Z5....and change Line 42 from G50 Z5. to G92 X5. Z5. ......... add a G90 on Line7 and on Line43

    G50 is just for Spindle RPM max... How to use G50 on a CNC lathe - CNC Training Centre



  7. #7
    Member
    Join Date
    Jan 2008
    Location
    Beaverdam, Virginia USA
    Posts
    448
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    Not the same generation but I had a Yasnac X3 that was real strange when it came to cutter comp. To get it to work right every time it had to be on it's own line of code all by itself.

    Last edited by Dualkit; 01-08-2020 at 06:43 PM.


  8. #8
    Member BlueChip's Avatar
    Join Date
    Jun 2003
    Location
    Massachusetts
    Posts
    197
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    My recommendation ... take the G42 out of the canned cycle completely.
    Some generations don't accept G41/G42 in the canned cycle ... it's roughing anyway, any TNR error will be taken out during finishing ... save yourself a lot of headaches.
    To include it in finishing ... activate G41/G42 before you command the G70.

    Since this generation didn't have "geometry" offsets ... it used G50 to preset the tool position.
    Sorta like geometry offsets ... except the values are written directly into the program.
    G50 is the distance and direction from the tool tip at the index position to the X0/Z0 position on the part.
    When the G50 is read ... the position display gets preset to the X/Z values on the G50 line.
    So if you have G50 X2.0Z2.0 ... the machine will think that it is at X2.0 Z2.0 ... and then if you command G00X0Z0 ... the tool move -2.00 in Z and -1.0 (radius) in X to get to 0,0.
    Since very tool sticks out of the turret differently ... every tool has it's own G50 position.
    Old school ... but like I said sorta think of it as new school geometry offsets.

    Also ... G50 can be used as a spindle restraint ... so G50S2500 will insure the machine spindle never goes beyond 2500 RPM.

    Hope this helps ....
    Check out out Real World Machine Shop Software at
    https://www.KentechInc.com



  9. #9
    Member Bubby44's Avatar
    Join Date
    Jan 2020
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    Quote Originally Posted by BlueChip View Post
    My recommendation ... take the G42 out of the canned cycle completely.
    Some generations don't accept G41/G42 in the canned cycle ... it's roughing anyway, any TNR error will be taken out during finishing ... save yourself a lot of headaches.
    To include it in finishing ... activate G41/G42 before you command the G70.

    Since this generation didn't have "geometry" offsets ... it used G50 to preset the tool position.
    Sorta like geometry offsets ... except the values are written directly into the program.
    G50 is the distance and direction from the tool tip at the index position to the X0/Z0 position on the part.
    When the G50 is read ... the position display gets preset to the X/Z values on the G50 line.
    So if you have G50 X2.0Z2.0 ... the machine will think that it is at X2.0 Z2.0 ... and then if you command G00X0Z0 ... the tool move -2.00 in Z and -1.0 (radius) in X to get to 0,0.
    Since very tool sticks out of the turret differently ... every tool has it's own G50 position.
    Old school ... but like I said sorta think of it as new school geometry offsets.

    Also ... G50 can be used as a spindle restraint ... so G50S2500 will insure the machine spindle never goes beyond 2500 RPM.

    Hope this helps ....
    Check out out Real World Machine Shop Software at
    https://www.KentechInc.com
    Removing the G42 entirely didn't change the outcome, still got G70-76/G72-78 error. It is good to know that isn't the problem though.

    I did alter my G50 coordinates to reflect your instructions and the machine moves exactly where I want it, but it still won't read through those canned cycles.

    Quote Originally Posted by machinehop5 View Post
    Try changing Line 6 from G50 X5. Z5. to G92 X5. Z5....and change Line 42 from G50 Z5. to G92 X5. Z5. ......... add a G90 on Line7 and on Line43

    G50 is just for Spindle RPM max... How to use G50 on a CNC lathe - CNC Training Centre
    Changing the G50's to G92's got me 030: Prog Error (F/E)

    Adding G90 to line 7 and 43 caused program error 104 (Double Addrs)



  10. #10
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    263
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    I was just looking around the Net...
    https://www.cnczone.com/forums/fanuc...71-issues.html

    Last edited by machinehop5; 01-10-2020 at 10:30 PM. Reason: link


  11. #11
    Member BlueChip's Avatar
    Join Date
    Jun 2003
    Location
    Massachusetts
    Posts
    197
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    Couple more things to try ...

    (1) When using the G71 you first move the machine to point A ( these are the coords the tool is at just before you call the canned cycle ) ... in your case the last X is 1.11 and the last Z is .8187. You need to return to that point when the last N ( Q ) number is executed. In your program that doesn't happen. Make sure that X is 1.11 and Z is at .8187 before N19 ... so N18 should be G01 Z.8187 and N19 should be G40 X1.11.

    (2) On a Fanuc control an X and Z move on the P (N) line turns on Type II G71 canned cycle where non-monotonous shapes can be machined. This is an option on some Fanuc controls and will generate an alarm if the option isn't there. Maybe something like that here. I would make try taking the Z move out of the line ... see what happens.

    Hope this helps ...
    Check out our Real World CNC / Machine Shop Software at
    https://www.kentechinc.com



  12. #12
    Member Bubby44's Avatar
    Join Date
    Jan 2020
    Posts
    5
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    Quote Originally Posted by BlueChip View Post
    Couple more things to try ...

    (1) When using the G71 you first move the machine to point A ( these are the coords the tool is at just before you call the canned cycle ) ... in your case the last X is 1.11 and the last Z is .8187. You need to return to that point when the last N ( Q ) number is executed. In your program that doesn't happen. Make sure that X is 1.11 and Z is at .8187 before N19 ... so N18 should be G01 Z.8187 and N19 should be G40 X1.11.

    (2) On a Fanuc control an X and Z move on the P (N) line turns on Type II G71 canned cycle where non-monotonous shapes can be machined. This is an option on some Fanuc controls and will generate an alarm if the option isn't there. Maybe something like that here. I would make try taking the Z move out of the line ... see what happens.

    Hope this helps ...
    Check out our Real World CNC / Machine Shop Software at
    https://www.kentechinc.com
    I took the Z move out of line 10 and it final ran through. Had a couple bumps the rest of the program, but nothing major. Thank you so much for helping me sort this out!



  13. #13
    Member machinehop5's Avatar
    Join Date
    Aug 2009
    Location
    United States
    Posts
    263
    Downloads
    0
    Uploads
    0

    Default Re: YASNAC Program Issue

    define g41 vs g42 path...maybe the problem...front or rear tool charger....upside down or inside out cw or ccw realtime g41 gfourtwo....you make the call Programmer

    Never give up, to simple problem



Tags for this Thread

Posting Permissions

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


About CNCzone.com

    We are the largest and most active discussion forum for manufacturing industry. The site is 100% free to join and use, so join today!

Follow us on


Our Brands

YASNAC Program Issue

YASNAC Program Issue

YASNAC Program Issue