NCedit post modification
Close
Login to Your Account
Results 1 to 6 of 6
  1. #1
    Join Date
    Aug 2014
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default NCedit post modification

    I am trying to modify my MPost so that the work offset will be called when the x and y are called. As of right now, the work offset comes in where the z value is. Anybody have any suggestions on how to fix this?

    Here is an example of part of my program...

    (.025" X .037" LOC EM - OP. 2)
    (HARVEY TOOL P/N 823025-C3 )
    (AI LOGO )
    X5.1874 Y-0.322
    Z-0.0669
    G56 G1 Z-0.1669
    Y-0.3233

  2. #2
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,560
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1397

    Default

    Quote Originally Posted by ajfdmb27 View Post
    I am trying to modify my MPost so that the work offset will be called when the x and y are called. As of right now, the work offset comes in where the z value is. Anybody have any suggestions on how to fix this?

    Here is an example of part of my program...

    (.025" X .037" LOC EM - OP. 2)
    (HARVEY TOOL P/N 823025-C3 )
    (AI LOGO )
    X5.1874 Y-0.322
    Z-0.0669
    G56 G1 Z-0.1669
    Y-0.3233
    Hello ajfdmb27,
    I'm not familiar with the Post for that Product (I have my own Software), so no real help with your issue directly. However, you have more problems than just the initiation of the Workshift occurring after the first axes move. Unless your program only has one Tool being used and the G56 Workshift for Z is set to that Tool without any reference to a Tool Offset, then your program will fail when other tools are called if no Tool Length Compensation code is included. Even if the Tool in the above example is a Master Tool for Tool Setting purposes and therefore has a Z Zero Offset, a Tool Length Offset call should be made in the program with either G43, or G44 (most commonly with G43).

    When you get the answer you require regarding editing the Post, you need to address the Tool Length Offset application as well.

    Regards,

    Bill

  3. #3
    Join Date
    Aug 2014
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    The tool length offset is called up at the beginning. When it goes to the second op (G56), that's where it screws up. Here is another example.

    Beginning...
    N14 T11 M6
    (.025" X .037" LOC EM)
    (HARVEY TOOL P/N 823025-C3 )
    (AI LOGO )
    M1
    M3 S12000
    M8
    G00 G90 G94 G55 X5.5625 Y0.2167
    G43 Z1. H11
    ------------------------------------------------
    op.2 (g56)
    -using the same tool

    (.025" X .037" LOC EM - OP. 2)
    (HARVEY TOOL P/N 823025-C3 )
    (AI LOGO )
    X5.1874 Y-0.322
    Z-0.0669
    G56 G01 Z-0.1669

  4. #4
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    653
    Post Thanks / Like
    Likes (Given)
    100
    Likes (Received)
    331

    Default

    Surfcam?

    You'll want to add (or edit) the Upon [Work] sequence in your post template. If your template has something there, post it here, or the whole thing so we can see what's going on.

    A million ways to do it, but at the bare minimum:

    Upon [Work]
    G0 G90 G[WORK] X[H] Y[V] Z[D]
    End

  5. Likes Billetgrip liked this post
  6. #5
    Join Date
    Aug 2014
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    3
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Quote Originally Posted by thesidetalker View Post
    Surfcam?

    You'll want to add (or edit) the Upon [Work] sequence in your post template. If your template has something there, post it here, or the whole thing so we can see what's going on.

    A million ways to do it, but at the bare minimum:

    Upon [Work]
    G0 G90 G[WORK] X[H] Y[V] Z[D]
    End
    heres the post...Thanks for the help!

    name DAEWOO-WIN TAC-3 AXIS
    # Modified added RapidCode logic sequence 3/27/2014
    % 00
    / 00
    O >4
    N >4
    $ 00
    ^ 00
    & 00
    * 00
    G 2
    g 2 G
    X ->3.>4
    Y ->3.>4
    Z ->3.>4
    I ->3.>4
    J ->3.>4
    K ->3.>4
    Q ->3.>4
    R ->3.>4
    P >40
    F >3.>3
    H >2
    D >2
    T >2
    M >2
    S >4

    SbackDoor SupressHeader

    ModalLetters X Y Z F R # List of letters that are modal
    LocalOutput? Y # Machine Datum support
    ModalGs 0 1 2 3 73 74 76 80 81 82 83 84 85 # List of g codes that are modal

    Sequence#s N 0 1 1 # Char, freq, incr & start
    First#? N # Y or N 'Output 1st sequence no.
    Last#? N # Y or N 'Output last sequence no.

    HCode X # X or X U 'Horizontal char.
    VCode Y # Y or Y V 'Vertical char.
    Dcode Z # Depth char.
    FeedCode F # Feed rate char.

    Comment ( ) # Begin End comment char.

    Spindle 3 4 5 # Cw, ccw & stop m codes
    Coolant 8 9 7 61 62 63 64 # Flood, Off, Mist and Thru Spindle M codes
    DComp 41 42 40 # Left, Right & Cancel m codes
    LComp 43 49 # On & Off codes

    Feed G01 # Linear move
    Rapid G00 # Rapid positioning word
    ArcPlane G 17 18 19 # G19, G18, G17 Arc Plane selection
    ReturnPlane 98 99 # G98 G99 Return Plane selection
    Cw G2 # Circular move clockwise
    Ccw G3 # Circular move counter clockwise

    ArcToLineWarnings? Y # Small Arc Warnings

    MinArc .0001 # MinArc Default = .0099
    MinRad .0001 # MinRad Default = .005
    TOLERANCE .00005
    Inc/Abs G 91 90 #Inc& Abs char. & values

    CtrCode I J K # I J or R or I J K L
    Helical? Y
    Spaces? Y # Y or N 'Spaces between words

    Incremental? N # Y or N 'Inc or abs output
    CtrIncremental? Y # Y or N 'Inc or abs I & J
    ByQuadrants? N # Y or N 'Break arcs at quadrants

    UppercaseComments? Y # Y or N 'Require uppercase comments

    Drill # Drilling canned/manual cycle
    G81 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate]
    end cancel

    CSink
    G82 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate] P[Dwell]
    end cancel

    Peck # Pecking canned/manual cycle
    G83 G[RetPlane] X[H] Y[V] Z[D] Q[VBite] R[Vclear] F[FRate]
    end cancel

    Tap # Tapping canned/manual cycle
    if [Rigid] > 0
    M29 S[SPEED]
    G84 G[RetPlane] X[H] Y[V] Z[D] P[Dwell] R[VClear] F[FRate]
    else
    G84 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate]
    Endif
    end cancel

    LTap # Left handed tapping cycle
    G74 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate] Q[VBite]
    end cancel

    Ream # Reaming canned/manual cycle
    G85 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate]
    end cancel

    Bore # Boring canned/manual cycle
    G86 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate]
    end cancel

    Back # Back boring canned/manual cycle
    G87 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate]
    end cancel

    Cancel # Cancel a canned/manual cycle
    G80
    if [Rigid] > 0
    G94 Unlock Z if w/ rigid tap.
    endif
    End



    RapidCode #(Include 'Z safety' logic)
    Comments

    IF [D] < [LastD] #Going down?
    G0 X[H] Y[V] #XY first,
    Z[D] #then Z.
    exit
    ENDIF

    IF [D] > [LastD] #Going up?
    G0 Z[D] # Z first,
    X[H] Y[V] # then XY.
    exit
    ENDIF

    IF [D] = [LastD]
    G0 X[H] Y[V]
    exit
    ENDIF
    END

    StartCode # Start of the program
    %0
    O[PROGRAM#]
    G17 G40 G80 G90
    End

    1stToolChange # First tool change
    N[BLOCK] M6 T[Tool]
    Comments
    M1
    M[Direct] S[Speed]
    M[Cool]
    G0 G90 G94 G[Work] X[H] Y[V]
    G43 Z[D] H[Lcomp]
    End

    Infeed # Enable cutter comp
    G[Side] X[H] Y[V] D[DComp] F[FRate]
    end

    Outfeed # Disable cutter comp
    G1 G40 X[H] Y[V]
    end

    ToolChange # Secondary tool changes
    M9
    N[BLOCK] M6 T[Tool]
    Comments
    M1
    M[Direct] S[Speed]
    M[Cool]
    G0 G90 G94 G[Work] X[H] Y[V]
    G43 Z[D] H[Lcomp]
    End

    Upon [Speed] # Output spindle speed change
    M[Direct] S[Speed]
    End

    EndCode # End of the program
    M9
    M30
    %0
    End

  7. #6
    Join Date
    Jan 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    653
    Post Thanks / Like
    Likes (Given)
    100
    Likes (Received)
    331

    Default

    ajfdmb27,

    Add that Upon [Work] section to your post, that will fix it.



    BTW, do you use the multi-cut toolpath at all? MPost does not handle it properly and spits out speed/work changes before it is supposed to.


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
  •