Mori SL-25B program help.
Close
Login to Your Account
Likes Likes:  0
Results 1 to 15 of 15
  1. #1
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    72
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    21

    Default Mori SL-25B program help.

    Machine has OT control,
    My issue is call up T0101 and it rapids toward the chuck, I am not using G50,
    Use T0100 and it works(kinda, not in auto coming from previous tool. It over travels in X and Z, Reset
    Goto that line and presto it is good.(until the next tool change).
    This code works and runs, But is not how I like it, (moving to the work piece in rapid with turret moving)

    G0 T0101 X6.5 Z1.
    G97 S400 M03
    G0 G54 X6.492 Z.15 M8
    G50 S1000
    G96 S700
    G99 G1 X2.7 F.012
    X2.8 Z.2
    M9
    G28 U0. W0. M05
    M01

    (This works but not in auto)
    ( over travels during rotation)
    G0 T0100 (Reset to here, it works)
    G97 S400 M03
    G0 G54 X6.492 Z.15 M8 T0101
    G50 S1000
    G96 S700
    G99 G01 X2.7 F.012
    X2.8 Z.2
    M9
    G28 U0. W0. M05
    M01
    Was thinking it is a parameter issue
    But not sure.
    Any ideas
    Thanks in advance
    John Hudson

  2. #2
    Join Date
    Feb 2014
    Location
    Sunny South West Florida, USA
    Posts
    3,315
    Post Thanks / Like
    Likes (Given)
    11430
    Likes (Received)
    3712

    Default

    What's your Z offset in T1?

  3. #3
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,285
    Post Thanks / Like
    Likes (Given)
    73
    Likes (Received)
    230

    Default

    When you command T0101, the offset is incorporated either by moving the tool or by changing the coordinate display, depending on a parameter.

  4. #4
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    2,548
    Post Thanks / Like

    Default

    Just me, but I cancel the tool offsets before going home. I think the parameter Sinha refers to is 0013.2. 0 shifts coordinate without moving tool.

  5. #5
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    72
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    21

    Default

    Quote Originally Posted by TeachMePlease View Post
    What's your Z offset in T1?
    T1 is Z zero face of part,

  6. #6
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,061
    Post Thanks / Like
    Likes (Given)
    908
    Likes (Received)
    2732

    Default

    Quote Originally Posted by Johnhudson View Post
    ....... (moving to the work piece in rapid with turret moving.......
    By this, are you saying that the turret is rotating to the T01 position while the Z axis is moving? If so, there may be a PMC (Diagnostic) parameter that enables or disables that behavior. I seem to recall that Mori had that on the AL and CL series machines with the 0T control, but don't remember about the SL series.

  7. #7
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    72
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    21

    Default

    Quote Originally Posted by Vancbiker View Post
    By this, are you saying that the turret is rotating to the T01 position while the Z axis is moving? If so, there may be a PMC (Diagnostic) parameter that enables or disables that behavior. I seem to recall that Mori had that on the AL and CL series machines with the 0T control, but don't remember about the SL series.
    Yes exactly what is happening,
    I Am just not comfortable with
    Rapiding towards the work piece
    With the turret unlocked and moving.

  8. #8
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    5,061
    Post Thanks / Like
    Likes (Given)
    908
    Likes (Received)
    2732

    Default

    You'll need to do a read through the PMC (Diagnostic) parameters in the back of the ladder diagram manual and see if there is a bit that needs to be changed to make it not do that.

    When I helped a tier 1 auto supplier with a couple projects on Mori AL2 lathes, that function was activated so that cycle time was reduced. Typically it is set so that the turret finishes indexing before starting to move.

  9. #9
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    901
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    326

    Default

    I just code it this way then I dont have to worry about it. ot control 88 miyano twin turrets

    G50S1500
    G30
    M01
    ;
    N2700
    G00 T2700 M08
    G96 S80 M03
    G00 X-1.0 Z1.0 T2727 M28
    X-0.2299 Z0.0501
    X-0.2416
    G01 Z-0.49 F0.002
    X-0.2399
    G00 X-0.2299 Z-0.4858
    Z0.0501
    X-0.2516
    G01 Z-0.0427
    X-0.2493 Z-0.0446
    G03 X-0.248 Z-0.0471 R0.005
    G01 Z-0.49
    X-0.2416
    G00 X-0.2316 Z-0.4858
    Z0.0501
    X-0.2616
    G01 Z-0.034
    X-0.2516 Z-0.0427
    G00 X-0.2416 Z-0.0385
    Z0.0501
    X-0.2716
    G01 Z-0.0253
    X-0.2616 Z-0.034
    G00 X-0.2516 Z-0.0298
    Z0.0501
    X-0.2816
    G01 Z-0.0167
    X-0.2716 Z-0.0253
    G00 X-0.2616 Z-0.0211
    Z0.0501
    X-0.2916
    G01 Z-0.008
    X-0.2816 Z-0.0167
    G97 Z4.0
    G00 T2700
    M01
    ;
    M9
    M29
    M25
    M30

  10. #10
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    72
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    21

    Default

    Quote Originally Posted by Delw View Post
    I just code it this way then I dont have to worry about it. ot control 88 miyano twin turrets
    What does your M28 do?
    It works that way for me until the next tool change then over travels.
    Reset. Goto that line and its runs
    Until the next tool change.

  11. #11
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    901
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    326

    Default

    Quote Originally Posted by Johnhudson View Post
    What does your M28 do?
    It works that way for me until the next tool change then over travels.
    Reset. Goto that line and its runs
    Until the next tool change.
    M28 is for high pressure coolant in our case or seconary coolant in most caes.
    REASON FOR THE X- IS i AM USING BOTTOM TURRET.

    we dont send home after any tools. only time I send it home is when I start the machine up. I dont use g54 or g50s except for max spindle speed.
    my bottom line was screwed I just grabs a quick one that I hadnt used.

    Ill fix it better
    G50S1500
    G30
    M01
    ;
    N2700
    G00 T2700 M08 (CALLS TOOL UP)
    G96 S80 M03
    G00 X-1.0 Z1.0 T2727 M28 (CALLS TOOL OFFSET WHILE MOVING INTO POSITION)

    Blah Blah Blah

    G97 G00 Z4.0 (this is my tool change position as I have 2 turrets normally) I would go. G00 G97 X6.0 Z6.0
    G00 T2700 (CANCELS TOOL OFFSET)
    M01
    ;
    M9
    M29
    M25
    M30

    IF YOU SEND THE MACHINE HOME AFTER YOU RUN TOO, YOU MUST CANCEL TOOL OFFSET 1ST. IF YOU DONT YOUR GOING TO OVER TRAVEL

  12. #12
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    901
    Post Thanks / Like
    Likes (Given)
    82
    Likes (Received)
    326

    Default

    You know what Im a dumbass.
    send your machine off the switches (ie BEFORE you call up a tool offset) and Cancle it befor you go home.
    sorry
    i dont ever take machine home.

  13. #13
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    122
    Post Thanks / Like
    Likes (Given)
    309
    Likes (Received)
    41

    Default

    G50 S1000
    G54
    G00 T0100 M8
    G96 S700 M3
    G00 X6.492 Z.15
    G99 G1 X2.7 F.012
    X2.8 Z.2
    M9
    G28 U0. W0.
    M01

    That's what I do on older lathes with Fanuc controls.

  14. #14
    Join Date
    Jun 2019
    Country
    UNITED STATES
    State/Province
    Kentucky
    Posts
    50
    Post Thanks / Like
    Likes (Given)
    2
    Likes (Received)
    4

    Default

    For my own knowledge, do you to use a g00 to call up a tool with this machine?

  15. #15
    Join Date
    Sep 2016
    Country
    UNITED STATES
    State/Province
    Idaho
    Posts
    72
    Post Thanks / Like
    Likes (Given)
    7
    Likes (Received)
    21

    Default

    Update:
    Parameter 14 needs to be bit 4
    Fanuc helped me out.


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
  •