Issue with G85 boring cycle


Page 1 of 2 12 LastLast
Results 1 to 12 of 13

Thread: Issue with G85 boring cycle

  1. #1
    Registered
    Join Date
    May 2012
    Location
    canada
    Posts
    147
    Downloads
    0
    Uploads
    0

    Default Issue with G85 boring cycle

    Hi Tom,

    We have another little issue with planes and canned cycles. I hate to keep bothering you with these but i tried a G85 boring cycle (feed in, feed out) tonight and it rapids to R plane as it should, feeds in fine, but when feeding out it feeds all the way to the I plane instead of to the R plane.

    With the following code it rapids to 2.0, then rapids to 0.1, feeds to -.44 and then feeds all the way back to 2.0. Should be feeding out to 0.1 and rapid to 2.0.

    N8130 G00 G90 G54 X0. Y0. S1200 M03
    N8140 G43 G94 H2 Z2.0 M08
    N8150 G98 G85 Z-.44 R.1 F3.
    N8160 G80 M09

    Thanks again.

    Similar Threads:


  2. #2
    Registered Need TECH Help!'s Avatar
    Join Date
    Dec 2007
    Location
    United States
    Posts
    338
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Have you tried a G99 instead of the G98? G99 is return to R after canned cycle. Tried it here and it feeds to R plane but does not rapid back to I plane. The Fanuc examples show G98 feed to R then rapid to I. Never payed attention to it before.

    Troy

    Last edited by Need TECH Help!; 06-09-2017 at 07:40 AM.
    http://www.homecncstuff.elementfx.com/


  3. #3
    Registered
    Join Date
    May 2012
    Location
    canada
    Posts
    147
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    G99 would probably be a good work around, but the action is not right for G85 with G98 so would be nice to have it working properly.

    G98 is very helpful when working with clamps or bolts securing a part to a fixture. Allows you to hop over them without wasting much time. I do mostly prototype and one off work so its safer for me to use G98 and a higher clearance plane as a default. The extra cycle time isnt really a big deal.



  4. #4
    Registered Need TECH Help!'s Avatar
    Join Date
    Dec 2007
    Location
    United States
    Posts
    338
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Ya, G coding could get timely using G99 (without cam) if you had a lot of holes and needed to add an extra move for clearance.

    http://www.homecncstuff.elementfx.com/


  5. #5
    Gold Member TomKerekes's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    2379
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Please check if this patch for V4.34i now behaves correctly.
    http://dynomotion.com/Software/Patch...nterpreter.dll

    Copy to <install V4.34i>\KMotion\Release

    Regards

    TK
    http://dynomotion.com


  6. #6
    Registered
    Join Date
    May 2012
    Location
    canada
    Posts
    147
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Thanks Tom, I will try it tomorrow.



  7. #7
    Registered Need TECH Help!'s Avatar
    Join Date
    Dec 2007
    Location
    United States
    Posts
    338
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    It works here.

    http://www.homecncstuff.elementfx.com/


  8. #8
    Registered
    Join Date
    Apr 2016
    Location
    United States
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Quote Originally Posted by mmurray70 View Post
    Hi Tom,

    We have another little issue with planes and canned cycles. I hate to keep bothering you with these but i tried a G85 boring cycle (feed in, feed out) tonight and it rapids to R plane as it should, feeds in fine, but when feeding out it feeds all the way to the I plane instead of to the R plane.

    With the following code it rapids to 2.0, then rapids to 0.1, feeds to -.44 and then feeds all the way back to 2.0. Should be feeding out to 0.1 and rapid to 2.0.

    N8130 G00 G90 G54 X0. Y0. S1200 M03
    N8140 G43 G94 H2 Z2.0 M08
    N8150 G98 G85 Z-.44 R.1 F3.
    N8160 G80 M09

    Thanks again.
    of course it does you gave g98, use g99. it will feed back to the r plane. why do you have 94 in the line with the g43?



  9. #9
    Registered Need TECH Help!'s Avatar
    Join Date
    Dec 2007
    Location
    United States
    Posts
    338
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Fanuc G85 cycle with a G98 feeds back to R plane then rapids back to I plane. G99 only feeds back to R plane and does not rapid back to I plane. G94 sets feed per minute mode so its safe to have it with G43 line even thow it might be more kosher to have after.

    http://www.homecncstuff.elementfx.com/


  10. #10
    Registered
    Join Date
    Apr 2016
    Location
    United States
    Posts
    44
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Quote Originally Posted by Need TECH Help! View Post
    Fanuc G85 cycle with a G98 feeds back to R plane then rapids back to I plane. G99 only feeds back to R plane and does not rapid back to I plane. G94 sets feed per minute mode so its safe to have it with G43 line even thow it might be more kosher to have after.
    I have never had the need for ipr on a mill, thats why i asked. I usually see that stuff in the first line of the program



  11. #11
    Registered Need TECH Help!'s Avatar
    Join Date
    Dec 2007
    Location
    United States
    Posts
    338
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Quote Originally Posted by skywalker4 View Post
    I have never had the need for ipr on a mill, thats why i asked. I usually see that stuff in the first line of the program
    Dont know, but his spindle may be able to orientate and track for feed per revolution. Ya, thats the most common place.

    http://www.homecncstuff.elementfx.com/


  12. #12
    Registered
    Join Date
    May 2012
    Location
    canada
    Posts
    147
    Downloads
    0
    Uploads
    0

    Default Re: Issue with G85 boring cycle

    Quote Originally Posted by skywalker4 View Post
    of course it does you gave g98, use g99. it will feed back to the r plane. why do you have 94 in the line with the g43?
    As we mentioned it should rapid from R to I plane instead of feed.

    G94 is there as a safety to be sure we are in inches per minute mode. G95 is used in tapping in a normal fanuc machine. And it is a good idea to have G94 there for each tool. For example If you happen to be tapping something and a tap breaks and you feedhold and then reset machine to inspect part and the tap, you are still in G95 mode because tapping did not finish and switch back to G94. Now if you happen to decide to carry on with your part and restart on the next tool it will basically cut at rapid speed because you are still in G95 mode. Had it happen once years ago on a machine, made short work of an endmill lol. I modded post processor to add G94 for every tool as a result. No issues since.

    Good to hear the patch works. I still cant confirm, had a couple more jobs come up and dont want to mess with machine while in the middle of a job. I will post back results eventually. Thanks again.



Page 1 of 2 12 LastLast

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

Issue with G85 boring cycle
Issue with G85 boring cycle