Drilling question New to the haas mc
Close
Login to Your Account
Results 1 to 11 of 11
  1. #1
    Join Date
    May 2019
    Country
    ALAND ISLANDS
    Posts
    1
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default Drilling question New to the haas mc

    Just recently started using the haas control manually to program fanuc programs.

    Also uk based.

    I have a drilling question regarding G83
    After you move say to first position i. e

    X10. Y10. It commands to drill at this position say 5mm deep

    If the next hole was 10mm deep can i use this line

    X20. Y10.,Z-10

    Without cancelling with G80 and re writing G83 with Z-10

    Thanks

    J

    Sent from my SM-G950F using Tapatalk

  2. #2
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    980
    Post Thanks / Like
    Likes (Given)
    552
    Likes (Received)
    946

    Default

    Yes (edit to add characters)

  3. #3
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,656
    Post Thanks / Like
    Likes (Given)
    294
    Likes (Received)
    1784

    Default

    Yes, you can re-specify ALL G8X parameters on the individual blocks.
    X Y Z Q R P G98/G99, even add I J K if you prefer.

    In your example though, I hope the comma ( , ) was just a typo. It is not needed and probably will be puked at.

  4. Likes bishbash25 liked this post
  5. #4
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    394
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    124

    Default

    Quote Originally Posted by SeymourDumore View Post
    Yes, you can re-specify ALL G8X parameters on the individual blocks.
    X Y Z Q R P G98/G99, even add I J K if you prefer.

    In your example though, I hope the comma ( , ) was just a typo. It is not needed and probably will be puked at.
    and even add different fixture offsets too

    like g00g90x1.0g55
    then
    g00g90x1.0g56

    etc etc

    for example

    T4M6(120 DEGREE C-SINK)
    G90 G00 G56 X-2.326Y-0.468
    T5
    S3000M3
    G43Z0.1H4M8
    G82G98Z-.106R+0.1F25.P200
    G90 G00 G57 X-2.326Y-0.468
    G90 G00 G58 X-2.326Y-0.468
    G90 G00 G59 X-2.326Y-0.468
    G80M9
    G91G28Z0M5
    M01

  6. #5
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,656
    Post Thanks / Like
    Likes (Given)
    294
    Likes (Received)
    1784

    Default

    Quote Originally Posted by Delw View Post
    and even add different fixture offsets too

    T4M6(120 DEGREE C-SINK)
    G90 G00 G56 X-2.326Y-0.468
    T5
    S3000M3
    G43Z0.1H4M8
    G82G98Z-.106R+0.1F25.P200
    G90G00G57X-2.326Y-0.468
    G90G00G58X-2.326Y-0.468
    G90G00G59X-2.326Y-0.468
    G80M9
    G91G28Z0M5
    M01
    All is good there Delw, but .... Damm is that an ugly code!!!

    How'bout this one:

    T4 M06 (120 DEGREE C-SINK)
    T5 (PRESTAGE #7 DRILL)
    G90
    G00 G43 H04 D04
    G00 G56 X-2.326Y-0.468 Z1.
    S3000 M03
    M08
    G82 G98 Z-.106 R0.1 F25. P200
    G57 X-2.326 Y-0.468
    G58 X-2.326 Y-0.468
    G59 X-2.326 Y-0.468
    G80
    M09
    M05
    G00 G53 Z0
    ...


    Or, even prettier the same thing with drill added:

    %
    T4 M6 (120 DEGREE SPOT)
    T5 (PRESTAGE #7 DRILL)
    G90
    G00 G43 H04 D04
    G00 G56 X-2.326Y-0.468 Z1.
    S3000 M03
    M08
    G82 G98 Z-.106 R0.1 F25. P200 L0
    M97 P9000
    G80
    M09
    M05
    G00 G49 G53 Z0
    T5 M06 (#7 DRILL)
    T6 (PRESTAGE 1/4-20 TAP)
    G00 G43 H05 D05
    G00 G56 X-2.326Y-0.468 Z1.
    S1800 M3
    M08
    G83 G98 Z-1.0 R0.1 F10. P200 Q.25 L0
    M97 P9000
    G80
    M09
    M05
    G00 G53 Z0
    (TAP CODE TO FOLLOW ....)
    M30
    (START SUBS)
    N9000 ( HOLE PATTERN)
    G56 X-2.326 Y-0.468
    G57 X-2.326 Y-0.468
    G58 X-2.326 Y-0.468
    G59 X-2.326 Y-0.468
    M99
    %

  7. Likes ranchak liked this post
  8. #6
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,656
    Post Thanks / Like
    Likes (Given)
    294
    Likes (Received)
    1784

    Default

    Quote Originally Posted by bishbash25 View Post
    I have a drilling question regarding G83
    After you move say to first position i. e

    X10. Y10. It commands to drill at this position say 5mm deep

    If the next hole was 10mm deep can i use this line

    To the OP however:

    G00 X10. Y10. Z100.
    S3000 M03
    M08
    G83 G98 Z-5. R2. Q100. P.1 F2.(or whatever)
    X20. Y10. Z-10.
    X30. Y10. Z-25.
    X40. Y10. Z-15.
    G80

    will be fine...

  9. Likes Chris59 liked this post
  10. #7
    Join Date
    May 2004
    Country
    UNITED STATES
    State/Province
    California
    Posts
    2,491
    Post Thanks / Like
    Likes (Given)
    882
    Likes (Received)
    1608

    Default

    I learned something today. Thanks fellas.

  11. #8
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    639
    Post Thanks / Like
    Likes (Given)
    96
    Likes (Received)
    330

    Default

    Quote Originally Posted by Delw View Post
    and even add different fixture offsets too

    like g00g90x1.0g55
    then
    g00g90x1.0g56

    etc etc

    for example

    T4M6(120 DEGREE C-SINK)
    G90 G00 G56 X-2.326Y-0.468
    T5
    S3000M3
    G43Z0.1H4M8
    G82G98Z-.106R+0.1F25.P200
    G90 G00 G57 X-2.326Y-0.468
    G90 G00 G58 X-2.326Y-0.468
    G90 G00 G59 X-2.326Y-0.468
    G80M9
    G91G28Z0M5
    M01
    Not quite. On Haas control, G00 will cancel a canned cycle.

  12. #9
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,656
    Post Thanks / Like
    Likes (Given)
    294
    Likes (Received)
    1784

    Default

    Quote Originally Posted by thesidetalker View Post
    Not quite. On Haas control, G00 will cancel a canned cycle.
    Ooops! That's correct! Any Group-1 G-code will cancel the canned cycle. Not just on a Haas, but most ( if not all ) controls.
    I've actually missed that one before cleaned up his post.

  13. #10
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    980
    Post Thanks / Like
    Likes (Given)
    552
    Likes (Received)
    946

    Default

    Gonna want to make sure G54, G55, etc. Z surface is within .100 (initial level) of each other or you’ll snap tools going between work offsets. Or make initial level bigger. ie G43 H1 Z1.

  14. #11
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    394
    Post Thanks / Like
    Likes (Given)
    25
    Likes (Received)
    124

    Default

    Quote Originally Posted by thesidetalker View Post
    Not quite. On Haas control, G00 will cancel a canned cycle.
    Quote Originally Posted by SeymourDumore View Post
    Ooops! That's correct! Any Group-1 G-code will cancel the canned cycle. Not just on a Haas, but most ( if not all ) controls.
    I've actually missed that one before cleaned up his post.
    haha I read your damn that is ugly code went back and read my post. Hell I dont even drink but it was late at night .
    Thanks guys.
    I copied and pasted the other lines forgot to edit that out.

    sorry about that Glad someone caught it before it was too late.

    Booze Daily your 100% correct have to watch the z surface.


Tags for this Thread

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
  •