G98 G99 retract plane
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 30
  1. #1
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default G73 cycle

    I'm messing with the post to get the correct format within ONECNC

    So here is the code I have currently working,

    N2680 (.422 INCH HSS 27/64 DRILL)
    N2690 G116 TOOL=28
    N2700 T55
    N2710 G15 H1
    N2720 G0 X-2.175 Y-5.025 M03 S3000
    N2730 G00 G56 Z0.5 H28 M08
    N2740 G00 X-2.175 Y-5.025 Z0.5
    N2750 G73 Z-1.2768 R0.5 Q0.5 F30.0
    N2760 X0. Y-1.595
    N2770 X2.175 Y-5.025
    N2780 G80
    N2790 G00 Z0.5
    N2800 M09
    N2810 M5
    N2820 G30 P1

    This works fine with two exceptions.
    1. This is a through hole at the bottom of a counter bore and I would like it to start feeding at Z-.700, not at the rapid plane. The Q value is set so there is no pecks I guess it doesn't like a zero value.
    2. It starts feeding at the rapid plane which isn't needed.

    How I have it set up is
    rapid plane .5"
    Plunge clearance .05"
    Material top -.700"


    It was set in the post to retract at the initial plane which I didn't catch at first but now its set to retract plane.

    g73-post.jpg

  2. #2
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Sorry about the thread title, I got that resolved and forgot to change it
    Last edited by Captdave; 02-18-2015 at 06:50 PM.

  3. #3
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,574
    Post Thanks / Like
    Likes (Given)
    4181
    Likes (Received)
    2733

    Default

    Are you looking for the right code, or asking how to change the post?

    nvm, I see you got it resolved.

  4. #4
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    I got the G98,G99 resolved, Okuma doesn't use those codes.

    I'm still working on the drill cycle.

    From what I'm gathering from the manual is there isn't a code in the G73 line for this, It may have to be a position line before the cycle is called which would be in CAM.

    G73 X Y Z R (point rapid level) P Dwell Q Peck F Feed

  5. #5
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    4,816
    Post Thanks / Like
    Likes (Given)
    3834
    Likes (Received)
    1534

    Default

    Quote Originally Posted by Captdave View Post

    N2680 (.422 INCH HSS 27/64 DRILL)
    N2690 G116 TOOL=28
    N2700 T55
    N2710 G15 H1
    N2720 G0 X-2.175 Y-5.025 M03 S3000
    N2730 G00 G56 Z0.5 H28 M08
    N2740 G00 X-2.175 Y-5.025 Z0.5
    N2750 G73 Z-1.2768 R0.5 Q0.5 F30.0
    N2760 X0. Y-1.595
    N2770 X2.175 Y-5.025
    N2780 G80
    N2790 G00 Z0.5
    N2800 M09
    N2810 M5
    N2820 G30 P1

    The Q value is set so there is no pecks I guess it doesn't like a zero value.
    I don't understand what your are asking. If you don't want a peck cycle use G81.

    G81 drill cycle
    G83 deep hole peck cycle
    G73 chip break peck cycle

    It starts feeding at the rapid plane which isn't needed.

    How I have it set up is
    rapid plane .5"
    Plunge clearance .05"
    Material top -.700"
    Are you saying the Z zero for the part is -.700"?

    Why not set the top of the part Z zero. Position the drill in x and y at the holes location. Rapid down to rapid plane .5 then G81 X Y Z(final depth of hole) R-.650 F(federate). Make sure you cancel the canned cycle and retract to a safe Z before moving to the next hole.

  6. #6
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    4,816
    Post Thanks / Like
    Likes (Given)
    3834
    Likes (Received)
    1534

    Default

    Here is a sample program from FeatureCAM. Stock is a 2 x 2 x 2 square of aluminum. Z zero is the upper left hand corner of the block. I'm drilling two 1/4" holes through the block but starting inside a .5" hole .5" deep.

    O5000(FM2)
    (FEATURECAM POST FOR OKUMA MCV4020 WITH OSP100E CONTROL)
    (OUTPUT IN ABSOLUTE INCHES 2-19-2015)
    ( BLOCK STOCK - ALUMINUM. X2 Y2 Z2 )
    ( T2 = .375 SPOT DRILL )
    ( T21 = .250 1/4 DRILL )
    CLEAR
    DRAW
    G0 G17 G20 G40 G80 G90 G94
    G111 T2 Q21
    M1
    (OPERATION - SPOTDRILL ON HOLE1)
    (TOOL NO - 2 DIAM - 0.375)
    (TOOL COMMENTS - )
    G15 H1
    S2546 M3
    G0 G90 X0.5 Y-1.0
    G56 Z1.0 H2
    M8
    Z-0.4
    G81 X0.5 Y-1.0 Z-0.63 R-0.4 F14.3
    G0
    Z1.0
    X1.5
    Z-0.4
    G81 X1.5 Y-1.0 Z-0.63 R-0.4 F14.3
    G0
    Z1.0
    M9
    G0 G17 G20 G40 G80 G90 G94
    G111 T21 Q2
    (OPERATION - .250 1/4 DRILL)
    (TOOL NO - 21 DIAM - 0.25)
    (TOOL COMMENTS - )
    M1
    G15 H1
    S3819 M3
    G0 G90 X1.5 Y-1.0
    G56 Z1.0 H21
    M8
    Z-0.4
    G73 X1.5 Y-1.0 Z-2.1001 R-0.4 Q0.25 F14.3
    G0
    Z1.0
    X0.5
    Z-0.4
    G73 X0.5 Y-1.0 Z-2.1001 R-0.4 Q0.25 F14.3
    G0
    Z1.0
    M9
    G112
    G15 H0
    M30

  7. #7
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Are you saying the Z zero for the part is -.700"?

    Why not set the top of the part Z zero. Position the drill in x and y at the holes location. Rapid down to rapid plane .5 then G81 X Y Z(final depth of hole) R-.650 F(federate). Make sure you cancel the canned cycle and retract to a safe Z before moving to the next hole.
    Part zero is the top of the part. There are 3 counter bores in each part 1.0D x .700 deep that need a through hole, 6 parts on the table. The method you posted works if there is only one hole per part or make 3 drilling cycles per part as the drill will not retract to the clearance plane before moving to the next hole. Other controls use G98,G99 to establish how the cycle functions within a canned cycle.

    The other option is to make 18 separate cycles which would suck. We make around 20 parts in this family so spending the time up front to get this right will payoff in the end. The G73 cycle was already within a proven program used on another machine so just went with it, A Q value of 0 works on the other control just fine so generally its my go to cycle.

    What I want it to do is rapid to X Y then rapid to Z-.700" Feed to Z-1.3" then rapid to the clearance plane and rapid to the next hole and repeat for the remaining holes.

    Tested G71 (Designation of return level for M53) in a line before the G73 call out and added M53 (fixed cycle return to specified point) at the end of the G73 line and it returns to the rapid plane between each hole the same as a G98 would function.

    I think this is going to be the work around for all the canned cycles but have only tested it on G73.

  8. #8
    Join Date
    Jun 2012
    Location
    Michigan
    Posts
    4,574
    Post Thanks / Like
    Likes (Given)
    4181
    Likes (Received)
    2733

    Default

    You want it to look something like this:

    G71Z2. <---- Jump height from hole to hole
    G83X1.2169Y-3.8104Z-2.R-.6Q.5F15.M53

  9. Likes Captdave liked this post
  10. #9
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Quote Originally Posted by Mtndew View Post
    You want it to look something like this:

    G71Z2. <---- Jump height from hole to hole
    G83X1.2169Y-3.8104Z-2.R-.6Q.5F15.M53
    That's what I came up with as well, now just need to modify the post to spit it out.

  11. Likes Mtndew liked this post
  12. #10
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Well that won't work after all.

    What I want it to do is rapid to X Y then rapid to Z-.700" Feed to Z-1.3" then rapid to the clearance plane and rapid to the next hole and repeat for the remaining holes.
    This will only work for getting over things like clamps that are well above the the part Z, I want to rapid to the bottom of the counter bore not go down at the F speed.

  13. #11
    Join Date
    Aug 2013
    Location
    Duluth, Mn
    Posts
    343
    Post Thanks / Like
    Likes (Given)
    47
    Likes (Received)
    103

    Default

    Can you just add your own drill cycle that will return to the plane that your looking to use?

  14. #12
    Join Date
    Aug 2013
    Location
    Duluth, Mn
    Posts
    343
    Post Thanks / Like
    Likes (Given)
    47
    Likes (Received)
    103

    Default

    Something Like

    #1=#5043 (#5043= Current Work Coord in Z on haas YMMV)
    G00 X#24 Y#25
    Z#18
    G01 Z#26 F#9
    G00 Z#1
    M99

  15. #13
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Quote Originally Posted by deljr15 View Post
    Can you just add your own drill cycle that will return to the plane that your looking to use?
    I could but there are 2 different sizes x 18 each and we have ~ 20 part in this family. That's a lot of typing

  16. #14
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    While I'm crying like a little girl, why does the spindle stop every time the control sees a G80? When you have multiple parts on the table with multiple canned cycles spindle stops at every part, heck the spindle has to stop and orient when tapping multiple parts.

  17. #15
    Join Date
    Mar 2014
    Location
    Nebraska
    Posts
    341
    Post Thanks / Like
    Likes (Given)
    42
    Likes (Received)
    214

    Default

    Quote Originally Posted by Captdave View Post
    Well that won't work after all.



    This will only work for getting over things like clamps that are well above the the part Z, I want to rapid to the bottom of the counter bore not go down at the F speed.
    It should rapid to your R plane specified in your G81 block.

    1. Rapid to first hole position
    2. G71 Z1.
    3. G81 X1.23 Y4.56 R-.7 F15. M53
    4. Next Hole
    5. Next Hole
    6. Next Hole
    7. G80

    This should drill the first hole in the pattern, rapiding to -.7, drill the hole at your feed rate, rapid to Z1, rapid to next hole, rapid to -.7, drill hole at feed rate..etc. Your Z0 is like the clamp in this circumstance, it jumps up to Z1, moves, then jumps back down.

    No help on the spindle stopping with G80. It is definitely annoying.

  18. #16
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    Tennessee
    Posts
    36
    Post Thanks / Like
    Likes (Given)
    20
    Likes (Received)
    19

    Default

    Write a subprogram.

    Something like
    ;;;
    M98 H5000 L3
    ;;;
    M30;
    N5000 G0 z-.700;
    Canned Cycle;
    G80;
    G0 z (clearance plane);
    G0 (next point)
    G99;

    half this is probably wrong, I'm drunk.

  19. #17
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Quote Originally Posted by bigjon61 View Post
    It should rapid to your R plane specified in your G81 block.

    1. Rapid to first hole position
    2. G71 Z1.
    3. G81 X1.23 Y4.56 R-.7 F15. M53
    4. Next Hole
    5. Next Hole
    6. Next Hole
    7. G80

    This should drill the first hole in the pattern, rapiding to -.7, drill the hole at your feed rate, rapid to Z1, rapid to next hole, rapid to -.7, drill hole at feed rate..etc. Your Z0 is like the clamp in this circumstance, it jumps up to Z1, moves, then jumps back down.

    No help on the spindle stopping with G80. It is definitely annoying.
    Then I must have had something wrong today because I swear I tested it the day before and it worked they way I wanted to.

    Thanks for the reply.

  20. #18
    Join Date
    Feb 2003
    Country
    UNITED STATES
    State/Province
    Illinois
    Posts
    4,816
    Post Thanks / Like
    Likes (Given)
    3834
    Likes (Received)
    1534

    Default

    Quote Originally Posted by Captdave View Post
    While I'm crying like a little girl, why does the spindle stop every time the control sees a G80? When you have multiple parts on the table with multiple canned cycles spindle stops at every part, heck the spindle has to stop and orient when tapping multiple parts.
    Try canceling the canned cycle with a G0. That works with my mills and lathes. Check my code above.

  21. #19
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Quote Originally Posted by Edster View Post
    Try canceling the canned cycle with a G0. That works with my mills and lathes. Check my code above.
    Ill be happy to give it a try, how do you know for sure that the cycle have cancelled? I assume the control alarm out if it's not?

  22. #20
    Join Date
    Sep 2006
    Location
    Atlanta, GA
    Posts
    3,054
    Post Thanks / Like
    Likes (Given)
    445
    Likes (Received)
    948

    Default

    Here is what I tried this morning.

    photo-131.jpg

    At G73 line it rapids to Z-.5 then in feeds to Z-.450 to Z-.500 and repeats over and over never feeding to Z-1.3268.

    Never made it past N230 so not sure about replacing G0 instead of G30.


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
  •