Haas VF1 peck drilling trouble
Close
Login to Your Account
Results 1 to 8 of 8
  1. #1
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default Haas VF1 peck drilling trouble

    So I am new to a Haas machine and I recently purchased a 2000 Haas VF1. I am having trouble with peck drilling with G83 in that the machine errors with "Invalid I, j, k". In the book it calls I, J, and K commands optional and I have omitted them as I don't wish to use them at this time.

    This is my code section, it errors/stops after the first hole drill. Suggestions?

    Code:
    G83 X0.7385 Y-0.4375 Z-0.625 Q0.21 R0.125 F20.0 
    G83 X0.7235 Y-2.1875 Z-0.625
    G83 X3.2765 Y-2.0995 Z-0.625
    G83 X4.7235 Y-2.1875 Z-0.625
    G83 X4.7385 Y-0.4375 Z-0.625
    G83 X3.2615 Y-0.5255 Z-0.625
    G83 X7.2615 Z-0.625
    G83 X8.7385 Y-0.4375 Z-0.625
    G83 X8.7235 Y-2.1875 Z-0.625
    G83 X7.2765 Y-2.0995 Z-0.625
    G83 X11.2765 Z-0.625
    G83 X11.2615 Y-0.5255 Z-0.625

  2. #2
    Join Date
    May 2007
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    1,410
    Post Thanks / Like
    Likes (Given)
    444
    Likes (Received)
    1207

    Default

    I just posted some code to drill holes in a part for my HAAS VF-2 take a look and see if this helps. You should only need to call the G83 on the first line and cancel it at the end using a G80

    N100 G20
    N110 G0 G17 G40 G49 G80 G90
    N120 T3 M6
    N130 G0 G90 G54 X-17. Y-3.25 S2439 M3
    N140 G43 H3 Z.1
    N150 M8
    N160 G99 G83 Z-.625 R.1 Q.1 F6.
    N170 X-15. Y-.38
    N180 X-3.
    N190 X-1. Y-3.25
    N200 X-3. Y-6.13
    N210 X-15.
    N220 G80
    N230 M5
    N240 G91 G28 Z0. M9
    N250 G28 X0. Y0.
    N260 M30
    %

    Good luck

    Make Chips Boys !

    Ron

  3. #3
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    985
    Post Thanks / Like
    Likes (Given)
    554
    Likes (Received)
    958

    Default

    That's some messy code.

    G83 is modal and stays in effect until cancelled by G80. Could be the problem.
    Either add G80 in between every G83 line or delete all G83 except the first one. You could then delete all the Z-.625 as they're redundant.

  4. #4
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    Thanks for the help. That fixed it.

    This code was created with cambam so I need to figure out how to edit the post processor to make this correct code. I am now doing everything with Fusion 360, but these older designs were already completed with cambam and I need to get them running again on the new mill asap.

    Code:
    %
    O2002
    ( SMART100.1_031919_CAM 4/3/2019 8:10:30 AM )
    ( T5 : 0.0625 )
    G54
    G20 G90 G64 G40
    G0 Z0.125
    ( T5 : 0.0625 )
    T5 M6
    G43 H5
    ( DRILL1 )
    G17
    M3 S5000
    G0 X0.7385 Y-0.4375
    G99
    G83 X0.7385 Y-0.4375 Z-0.625 Q0.21 R0.125 F20.0 
    X0.7235 Y-2.1875
    X3.2765 Y-2.0995
    X4.7235 Y-2.1875
    X4.7385 Y-0.4375
    X3.2615 Y-0.5255
    X7.2615
    X8.7385 Y-0.4375
    X8.7235 Y-2.1875
    X7.2765 Y-2.0995
    X11.2765
    X11.2615 Y-0.5255
    G80
    G0 Z0.125
    M5
    M30
    %
    Thanks for your help!!!!!

  5. #5
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,662
    Post Thanks / Like
    Likes (Given)
    295
    Likes (Received)
    1791

    Default

    OK, so your problem was as follows:

    the G83 block MUST have either I, J, K, OR a Q value.
    These values are non-modal, meaning after the block is cancelled ( either by G80 or any other group command ), they are erased and must be re-defined for the next G83 call.

    In your case your post called the entire G83 cycle for each and every hole. While that is completely unnecessary, it also cancelled the previous G83 definition
    and re-called it, but now without the Q definition.
    Basically your code was equivalent to:
    G83 X0.7385 Y-0.4375 Z-0.625 Q0.21 R0.125 F20.0
    G80
    G83 X0.7235 Y-2.1875 Z-0.625
    G80
    G83 X3.2765 Y-2.0995 Z-0.625
    G80
    G83 X4.7235 Y-2.1875 Z-0.625
    G80
    G83 X4.7385 Y-0.4375 Z-0.625
    etc....

    Note that any G83 block after the first one are missing the Q value.

    R can be omitted as it can come either from the block's definition, or if omitted there is a default in the Settings page.
    F is modal, so it sticks
    P can be omitted, and if so it's assumed to be 0
    I,J and K OR the Q value however is mandatory, so one or the other MUST BE EXPLICITLY DEFINED IN EACH G83 call!

  6. Likes ForcedFour liked this post
  7. #6
    Join Date
    Apr 2019
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    1
    Likes (Received)
    0

    Default

    That makes perfect sense. Thank you!

    I added the R value because after getting it to work as above without the R value the spindle would rapid all the way up to Machine Z0 after each hole drilled. Likely a setting would fix that, but adding the R value also fixed it and got me machining today.

  8. #7
    Join Date
    Jan 2017
    Country
    UNITED STATES
    State/Province
    Oregon
    Posts
    1,988
    Post Thanks / Like
    Likes (Given)
    388
    Likes (Received)
    1508

    Default

    Quote Originally Posted by ForcedFour View Post
    That makes perfect sense. Thank you!

    I added the R value because after getting it to work as above without the R value the spindle would rapid all the way up to Machine Z0 after each hole drilled. Likely a setting would fix that, but adding the R value also fixed it and got me machining today.
    That's because you have no initial plane. If you said G43 H5 Z1.0, the retract would go to Z1.0.

    Since there is no Z position prior to reading the G83 line, it goes back to the starting point which is Z home.

    G99 is retract to R plane, so adding the R plane means it will rapid to R and retract to R for the duration of the G83 cycle.

  9. Likes rklopp liked this post
  10. #8
    Join Date
    Jan 2011
    Location
    South Florida
    Posts
    613
    Post Thanks / Like
    Likes (Given)
    62
    Likes (Received)
    116

    Default

    If your holes are all the same, then all you need after the first G83 call out is the next location. For example: X4.7235 Y-2.1875. When you call out the G83 again, it needs the Q and the R again.

    G83 X0.7385 Y-0.4375 Z-0.625 Q0.21 R0.125 F20.0
    X0.7235 Y-2.1875
    X3.2765 Y-2.0995
    X4.7235 Y-2.1875
    X4.7385 Y-0.4375
    X3.2615 Y-0.5255
    X7.2615
    X8.7385 Y-0.4375
    X8.7235 Y-2.1875
    X7.2765 Y-2.0995
    X11.2765
    X11.2615 Y-0.5255


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
  •