Results 1 to 13 of 13
  1. #1
    ewlsey is offline Diamond
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    5,021

    Default Setting tool lengths on an Okuma VMC

    I'm trying to get a grasp on an Okuma VMC with an OSP control (forget which model). The problem is setting the tool lengths on the machine. The control seems to set them relative to the current work offset (G15HXX I think). This is a bit different than I am used to.

    Here is what I was going to do:
    I want to make a dedicated work offset for setting tools. I will bring the spindle nose down and touch off to the table (with a gage block of some kind) and zero a work offset (say #20). Then I can use offset 20 to set all of the tools with the same gage block.

    This should give me the positive gage line offset for the tools. However, I will lose one work offset, and everyone will have to remember to use that offset when setting tools. I think that is basically what the fanuc control does, but I have to set it up manually on the Okuma.

    Is there a better way other than a pre-setter? Is there some parameter I can change to get the functionality of a Fanuc? I have seen other machines set up like this Okuma, and it seems less than ideal.

    Thanks eneryone.

  2. #2
    Edster is offline Titanium
    Join Date
    Feb 2003
    Location
    Illinois
    Posts
    3,544

    Default

    Enter G15 H0 in mdi to cancel the active work offset before you set the tool lengths.

  3. #3
    Bob Looney is offline Aluminum
    Join Date
    Dec 2006
    Location
    USA
    Posts
    69

    Default

    Quote Originally Posted by Edster View Post
    Enter G15 H0 in mdi to cancel the active work offset before you set the tool lengths.
    ditto
    G15 H0 is the machine home position, It doesn't cancel the offsets. Your program will run using H0 so make sure your code is correct.

    If you're a Fanuc guy, you'll never get a "grasp" of that control. I spent 12 years programming and running those things.

  4. #4
    ewlsey is offline Diamond
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    5,021

    Default

    Using G15H0 would not give me the gage line tool length would it? I'll give it a try. Thanks guys.

    The Okuma a little odd. The G111 tool change macro is different. And G56 for tool length. I'm used to using G10 to set the offsets, Okuma seems to have its own system.

    Thanks again.

  5. #5
    Bob Looney is offline Aluminum
    Join Date
    Dec 2006
    Location
    USA
    Posts
    69

    Default

    For work offsets you can use the VZOF x,y,z [offset number] variables. There are other variables for tool lengths.

    VZOFX[]=
    VZOFY[]=
    VZOFZ[]=

  6. #6
    mostagear is offline Aluminum
    Join Date
    Aug 2008
    Location
    alexandria, EGYPT
    Posts
    52

    Default

    here what i was doing with okuma osp 100.
    ...
    ** for the first tool use .. G15 HXX
    for the following tools use ... G56 Hxx
    the first tool setting is in the X,Y,Z measure screen.
    the other tools will be in the tool lenght offset screen.. ((in this screen the value of the first tool should be ZERO))
    like..

    N1 G15 H1 <<<<<<
    N3 T01 M06 <<<<<<
    N7 S1500 M3
    N9 G0 Z1000
    N11 G0 X0.0 Y-49.0
    N13 Z50.0 M8
    N15 G71 Z50.0
    N17 G81 X0.0 Y-49.0 Z-11 R0.0 F100 M53
    N25 G80
    N27 T02M06 <<<<<<<
    N29 G56 H02 <<<<<<<
    N31 S1500 M3
    N33 G0 Z1000
    N35 G0 X34.648 Y34.648
    N37 Z50.0 M8
    N39 G71 Z50.0
    N41 G81 X34.648 Y34.648 Z-11 R0.0 F60.0 M53
    N45 G80
    N47 G00 Z100.0
    N49 Z1000 M05 M09
    N51 Y1000
    N53 M02

    good luck

  7. #7
    dabigguy is offline Aluminum
    Join Date
    Dec 2005
    Location
    Wisconsin east coast
    Posts
    130

    Default

    What do here is call up the program, we use Z-TOOLSET.MIN. This will make it the last program in your program files.

    The program consist of
    (RUN THIS PROGRAM BEFORE TOOL OFFSETING)
    G15 H0
    G00 Z50.0
    G30 P20 (TOUCH OFF POSITION)
    M2

    Use the G30 P?? to set a area where there is no clamping or vises to touch off your tooling.

  8. #8
    ewlsey is offline Diamond
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    5,021

    Default

    Quote Originally Posted by dabigguy View Post
    What do here is call up the program, we use Z-TOOLSET.MIN. This will make it the last program in your program files.

    The program consist of
    (RUN THIS PROGRAM BEFORE TOOL OFFSETING)
    G15 H0
    G00 Z50.0
    G30 P20 (TOUCH OFF POSITION)
    M2

    Use the G30 P?? to set a area where there is no clamping or vises to touch off your tooling.
    Thanks a lot. I made my own version of this program. Instead of G30 I used the VXOF[1], VYOF[1] to set the table where I wanted. Then I used VZOF[1] to compensate for my tool setting block. Works great.

    This Okuma is so backwards from what I am used to. I think it is crazy that you can just tell it G0 X2000 Y2000 and it will just cruise up to the limits with no error or alarms. That really gets me on the lathes. Tool changes are a bit odd too with the G111 code.

    The mill has an OSP U10M control. I think it is mid 90s vintage. Does anyone know if it has graphics? The LCD is monochrome and I cannot find a graphics screen.

    P.S. I have never seen any machine where the plus sign was on the left and the minus sign on the right like the Okuma jog buttons. It's like they tried deliberately to make it backwards.

  9. #9
    rainman is offline Aluminum
    Join Date
    Sep 2008
    Location
    Orlando, FL
    Posts
    183

    Default

    Quote Originally Posted by ewlsey View Post
    P.S. I have never seen any machine where the plus sign was on the left and the minus sign on the right like the Okuma jog buttons. It's like they tried deliberately to make it backwards.
    There is some logic to this, despite it not being what you're used to. Plus on the left makes the table go left. Minus in the right makes the table go right. However, I, like you, am more used to considering tool movement relative to the table, not table movement.

  10. #10
    leocnctw is offline Plastic
    Join Date
    Dec 2007
    Location
    QLD, Australia
    Posts
    20

    Default

    Hi all! are the block numbers necessary for program body?? I am EIA ISO guy and fanuc fluent. New job needs to run okuma. Thanks

  11. #11
    ewlsey is offline Diamond
    Join Date
    Jul 2009
    Location
    Peoria, IL
    Posts
    5,021

    Default

    Why did you drag this old thread up?

    No, block numbers are not needed. Dynapath is the only control I know that needs them.

  12. #12
    leocnctw is offline Plastic
    Join Date
    Dec 2007
    Location
    QLD, Australia
    Posts
    20

    Default

    Thanks for the response ewsley.

    Mods , my apology for pulling this thread out the archive.

  13. #13
    ARB's Avatar
    ARB
    ARB is offline Titanium
    Join Date
    Dec 2002
    Location
    Granville,NY,USA
    Posts
    3,673

    Default

    Old thread or not. I would say to step away from measuring on the machine. Even using simple home grown socket and height set works so much better than using the machine to measure tools. I made the leap years ago and have not looked back..

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
  •