Need Help! Error in Drilling Cycle G83


Page 1 of 2 12 LastLast
Results 1 to 12 of 15

Thread: Error in Drilling Cycle G83

  1. #1
    Gold Member amitkumar171's Avatar
    Join Date
    Aug 2017
    Location
    India
    Posts
    79
    Downloads
    0
    Uploads
    0

    Default Error in Drilling Cycle G83

    Hi all

    I made a program in CAM software for drilling operation in 3+2 Indexing mode.

    A strange error i am getting is G Code Error, R less than z in cycle in xy plane.

    How to solve this issue have anyone faced same problem, if yes then how you solved i t using kmotion CNC software. I am using KFLOP Board with KmotionCNC software UI.

    A screenshot is also attached with the error.


    Waiting for your kind reply


    AMIT KUMAR
    (+918952917319)

    Similar Threads:
    Attached Thumbnails Attached Thumbnails Error in Drilling Cycle G83-screenshot-2-png  
    Regards

    Amit Kumar


  2. #2
    Gold Member TomKerekes's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    2719
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    Hi Amit,

    My interpretation of your G83 GCode is:

    Starting Z = 75.2

    Drill down to Z = 75.2 (this is nothing!!)

    Retract Z out to R = 14.5 (this is down not up !!)

    So as the error message is saying the R value must be above the bottom of the hole not below.

    Check your CAD system and determine why it is generating GCode like this.

    Here is a good description of G83 with a diagram
    G83 Peck Drilling Cycle (Deep Hole) for Fanuc - Helman CNC

    Regards

    TK
    http://dynomotion.com


  3. #3
    Gold Member amitkumar171's Avatar
    Join Date
    Aug 2017
    Location
    India
    Posts
    79
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    Quote Originally Posted by TomKerekes View Post
    Hi Amit,

    My interpretation of your G83 GCode is:

    Starting Z = 75.2

    Drill down to Z = 75.2 (this is nothing!!)

    Retract Z out to R = 14.5 (this is down not up !!)

    So as the error message is saying the R value must be above the bottom of the hole not below.

    Check your CAD system and determine why it is generating GCode like this.

    Here is a good description of G83 with a diagram
    G83 Peck Drilling Cycle (Deep Hole) for Fanuc - Helman CNC

    Regards
    Hi Tom,

    Can you please tell me what G Code to use canned cycle (peck drilling), ?

    As I don't think G83 is supported in KMotionCNC software.

    I want to perform the above operation in 3+2 Indexing Mode.

    Waiting for your kind reply.

    Regards

    Amit Kumar


  4. #4
    Gold Member TomKerekes's Avatar
    Join Date
    May 2006
    Location
    USA
    Posts
    2719
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    Hi Amit,

    G83 should be supported. You just have to give it parameters that make sense.

    Try making one yourself by hand that drills down and retracts up to prove whether G83 works or not.

    Regards

    TK
    http://dynomotion.com


  5. #5
    Registered
    Join Date
    Jun 2004
    Location
    Scotland
    Posts
    305
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    G83 does work, however do you have your Z working the correct way?
    Z should decrease as you drill/machine into the material.

    As Tom has said, in a G83 (or any canned drilling cycle), Z should be a lower value than the retract plane (R) value.



  6. #6
    Registered
    Join Date
    May 2012
    Location
    canada
    Posts
    233
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    G83 works fine for me.

    Pretty awesome that it caught that Tom! I've made that programming error before with a fanuc control and everything looked great until my drill crashed into the part at rapid speed lol. Nice work.



  7. #7
    Gold Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    7715
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    Quote Originally Posted by amitkumar171 View Post
    Hi all

    I made a program in CAM software for drilling operation in 3+2 Indexing mode.

    A strange error i am getting is G Code Error, R less than z in cycle in xy plane.

    How to solve this issue have anyone faced same problem, if yes then how you solved i t using kmotion CNC software. I am using KFLOP Board with KmotionCNC software UI.

    A screenshot is also attached with the error.


    Waiting for your kind reply


    AMIT KUMAR
    (+918952917319)
    Your program is incorrect

    G98 Return to initial point in canned cycle ( Line # 32405 Z75.2 ) The Z axes will return to this point Z75.2 when using a G98

    32420 G98G83X-10.8Y8.1 Z 75.2 This Z move is not going to move any where, this has to be a negative number to drill into your part R14.5 Q0.5F200. this whole line is incorrect, ( so how deep do you want to drill into your part )

    G99 Return to R point in canned Cycle, This would return to the R value 14.5 if it was correct, but most likely is not correct also, this has to move the drill above your work piece to give you clearance for the next move

    Mactec54


  8. #8
    Gold Member amitkumar171's Avatar
    Join Date
    Aug 2017
    Location
    India
    Posts
    79
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    Quote Originally Posted by mactec54 View Post
    Your program is incorrect

    G98 Return to initial point in canned cycle ( Line # 32405 Z75.2 ) The Z axes will return to this point Z75.2 when using a G98

    32420 G98G83X-10.8Y8.1 Z 75.2 This Z move is not going to move any where, this has to be a negative number to drill into your part R14.5 Q0.5F200. this whole line is incorrect, ( so how deep do you want to drill into your part )

    G99 Return to R point in canned Cycle, This would return to the R value 14.5 if it was correct, but most likely is not correct also, this has to move the drill above your work piece to give you clearance for the next move
    Hi mactec54,

    I am using fusion 360 for my G-Code generation and I do not get this error when I perform 3 axis operation but as soon as I shift to 5 axis (3+2 indexing), the error arises.
    I am not able to figure out if the problem is in the post processor or in the toolpath generated in fusion 360. it will be very helpful if you could help me figure this out.

    thank you

    Regards

    Amit Kumar


  9. #9
    Gold Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    7715
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    Quote Originally Posted by amitkumar171 View Post
    Hi mactec54,

    I am using fusion 360 for my G-Code generation and I do not get this error when I perform 3 axis operation but as soon as I shift to 5 axis (3+2 indexing), the error arises.
    I am not able to figure out if the problem is in the post processor or in the toolpath generated in fusion 360. it will be very helpful if you could help me figure this out.

    thank you
    If you can simulate it in Fusion, and it is ok, then it would have to be in the post-processor

    Mactec54


  10. #10
    Gold Member amitkumar171's Avatar
    Join Date
    Aug 2017
    Location
    India
    Posts
    79
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    Hi Tom,

    I made that Drilling code in fusion 360, using post processor that is attached below, and In post processor By Turning TCP on and off two different codes are generated. both are below.

    1. TCP on drilling Code generated by fusion 360 post processor

    N31220 G0 A90. C0.
    N31225 M8
    N31235 G0 X-10.8 Y-40.
    N31240 G43 Z75.2 H1
    N31250 G0 Y-30.
    N31255 G98 G83 X-10.8 Y-8.1 Z75.2 R77 Q0.5 F300.
    N31260 X10.8
    N31265 G80
    N31270 G0 Y-40.


    2. TCP off drilling Code generated by fusion 360 post processor


    N85175 G0 A90. C0.
    N85180 M8
    N85185 G0 Z40.
    N85195 G0 X-10.8 Y75.2
    N85200 G43 H1
    N85210 G0 Z30.
    N85215 G98 G83 X-10.8 Y75.2 Z8.1 R14.5 Q0.5 F300.
    N85220 X10.8
    N85225 G80
    N85230 G0 Z40.


    And i tried running both in KmotionCNC , 1st one program is giving error R less than Z in xy plane. But When i am running 1st program in controller manually inputting the coordinates its working fine, But When i press cycle start it is giving same error.

    And 2nd program of drilling that is mentioned above is not giving that error but wrong drilling in the table itself.

    How to solve that problem. If there is anything to do in the post then let me know.

    Waiting for your kind reply

    Attached Files Attached Files
    Regards

    Amit Kumar


  11. #11
    Registered
    Join Date
    Jun 2004
    Location
    Scotland
    Posts
    305
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    I wonder if this is to do with plane selection.

    TCP is well beyond me, but how canned/drilling cycles work, depends on what plane is selected.
    G17 is XY, with drilling along the Z axis (default mode on most controllers)
    G18 is XZ, with drilling along the Y axis.
    G19 is YZ, with drilling along the X axis.

    Can you tell us the location of the hole, and what the start/finish heights of it should be?
    Or a screenshot of the item/holes in F360 showing the axis?


    I'm guessing you don't want to post the full CAD in public, but could you make a simple model with just the drill holes so we can see what you're trying to do?



  12. #12
    Gold Member
    Join Date
    Jan 2005
    Location
    USA
    Posts
    7715
    Downloads
    0
    Uploads
    0

    Default Re: Error in Drilling Cycle G83

    Quote Originally Posted by amitkumar171 View Post
    Hi Tom,

    I made that Drilling code in fusion 360, using post processor that is attached below, and In post processor By Turning TCP on and off two different codes are generated. both are below.

    1. TCP on drilling Code generated by fusion 360 post processor

    N31220 G0 A90. C0.
    N31225 M8
    N31235 G0 X-10.8 Y-40.
    N31240 G43 Z75.2 H1
    N31250 G0 Y-30.
    N31255 G98 G83 X-10.8 Y-8.1 Z75.2 R77 Q0.5 F300.
    N31260 X10.8
    N31265 G80
    N31270 G0 Y-40.


    2. TCP off drilling Code generated by fusion 360 post processor


    N85175 G0 A90. C0.
    N85180 M8
    N85185 G0 Z40.
    N85195 G0 X-10.8 Y75.2
    N85200 G43 H1
    N85210 G0 Z30.
    N85215 G98 G83 X-10.8 Y75.2 Z8.1 R14.5 Q0.5 F300.
    N85220 X10.8
    N85225 G80
    N85230 G0 Z40.


    And i tried running both in KmotionCNC , 1st one program is giving error R less than Z in xy plane. But When i am running 1st program in controller manually inputting the coordinates its working fine, But When i press cycle start it is giving same error.

    And 2nd program of drilling that is mentioned above is not giving that error but wrong drilling in the table itself.

    How to solve that problem. If there is anything to do in the post then let me know.

    Waiting for your kind reply
    Both are incorrect, there is something wrong with your drawing, the Z axes drilling move needs to be a negative number, or where you have your Tool Zero set

    Mactec54


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

Error in Drilling Cycle G83

Error in Drilling Cycle G83