Okuma LB15 w OSP 5000 Nose Radius Comp Help
Close
Login to Your Account
Results 1 to 7 of 7
  1. #1
    Join Date
    Mar 2018
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    14
    Post Thanks / Like
    Likes (Given)
    6
    Likes (Received)
    1

    Default Okuma LB15 w OSP 5000 Nose Radius Comp Help

    Hi all,

    New to this machine and needing help getting the nose radius comp setup correctly. Here's what I have:

    OD turning tool with .031 rad

    (in the NOSE - R COMP settings) X = .031, Z = .031, P = 2
    (The screenshot doesn't show these settings. We entered them, got the error and then removed them)

    With this code:

    G50 S2500
    G97 S1100 M42 M03 M08
    G00 X1.85 Z0.1 T020202
    G87 N0103
    G82
    G00 Z0
    G01 X1.75 G41 F0.007
    X0 F0.002
    X1.441
    G03 X1.501 Z-0.03 K-0.03
    G01 Z-0.312
    X1.625
    Z0.6

    I'm getting the following error:

    "517 ALARM - B NOSE - R COMP NOSE-R > CIRLCE-R"

    Also, the screen is super foggy. Does anyone know if this is a problem with the screen cover or the crt itself? (see pics)

    Thanks in advance!

    20180409_100004_001.jpg
    20180409_095925.jpg

  2. #2
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    Ohio
    Posts
    688
    Post Thanks / Like
    Likes (Given)
    389
    Likes (Received)
    700

    Default

    You need to use G42 for comp on an OD. With the G41 you're using it is cutting on the inside of the programmed profile. In other words, you're trying to cut inside a .030 radius with a .032 radius tool.

  3. #3
    Join Date
    Jun 2017
    Country
    NETHERLANDS
    Posts
    23
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    Plus its better get the X-step 2 time your nose radius.

  4. #4
    Join Date
    Sep 2003
    Location
    riverside, ca, usa
    Posts
    334
    Post Thanks / Like
    Likes (Given)
    31
    Likes (Received)
    76

    Default

    I’m pretty sure that when you go from X1.75 Z0 to X0 Z0 and then back up to X1.441 Z0 it’s going to make the control shit the bed. Going down you will be on the Z+ side of the contour and going up you will be be on the Z- side ( inside the part!). I could be wrong though.

  5. #5
    Join Date
    Apr 2011
    Country
    UNITED STATES
    State/Province
    New York
    Posts
    243
    Post Thanks / Like
    Likes (Given)
    162
    Likes (Received)
    137

    Default

    Change P 2, to P 3, exactly as you see in your first picture. Run your program in "Machine Lock" and see if it faults
    Best of luck,
    Chris

  6. #6
    Join Date
    Sep 2008
    Country
    UNITED STATES
    State/Province
    Florida
    Posts
    331
    Post Thanks / Like
    Likes (Given)
    26
    Likes (Received)
    86

    Default

    Well, for one thing, it looks like you're reversing your X direction in the middle of the cut. Can't do that with TNR comp.

  7. Likes johnryancnc liked this post
  8. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,065
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1203

    Default

    Quote Originally Posted by johnryancnc View Post
    Hi all,

    New to this machine and needing help getting the nose radius comp setup correctly. Here's what I have:

    OD turning tool with .031 rad

    (in the NOSE - R COMP settings) X = .031, Z = .031, P = 2
    (The screenshot doesn't show these settings. We entered them, got the error and then removed them)

    With this code:

    G50 S2500
    G97 S1100 M42 M03 M08
    G00 X1.85 Z0.1 T020202
    G87 N0103
    G82
    G00 Z0
    G01 X1.75 G41 F0.007
    X0 F0.002
    X1.441
    G03 X1.501 Z-0.03 K-0.03
    G01 Z-0.312
    X1.625
    Z0.6

    I'm getting the following error:

    "517 ALARM - B NOSE - R COMP NOSE-R > CIRLCE-R"

    Thanks in advance!
    Hello johnryancnc,
    In your example code, it would be correct to use G41 to face the part as the tool would have to offset to the Left of the Tool Path, but when reversing the direction of X travel in the X0.0 to X1.441 move, the control will still offset the Tool to the Left in the direction of travel, which would be into the Workpiece. When reversing the direction of travel, the Tool Radius Comp would have to be changed from G41 to G42. Further, if the following code:

    G01 X1.75 G41 F0.007
    X0 F0.002
    X1.441

    actually worked without error, I believe a pip at the centre of the workpiece would result.

    When facing a part where the face is perpendicular to the Z axis, there is no need to use Tool Radius Compensation and therefore, its common to face the part without using TRC and then turn it on when profiling the ID, or OD.

    The same reason applies for the Z axis as stated above when changing direction in X. With your change of direction in Z in the Z0.6 move, the TRC would have to be reversed, or cancelled.

    G50 S2500
    G97 S1100 M42 M03 M08
    G00 X1.85 Z0.1 T020202
    G87 N0103
    G82
    G00 Z0
    G01 X1.75 F0.007
    G01 X-0.062 F0.002
    G00 Z0.050
    G42 X1.441
    G01 Z0.0

    G03 X1.501 Z-0.03 K-0.03
    G01 Z-0.312
    X1.625
    Z0.6

    Regards,

    Bill
    Last edited by angelw; 04-20-2018 at 04:45 AM.


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
  •