Results 1 to 10 of 10
  1. #1
    chet is online now Aluminum
    Join Date
    May 2004
    Location
    minnesota
    Posts
    153

    Default fanuc ot-c parts counter

    im running a bar puller to make 20 parts with G65 P9055 C20. works fine the machine runs my program 20 times. but i dont see were the parts counter is so i dont know how many cycels have run. is the counter one of the offsets or a parameters?
    -chet

  2. #2
    michael is offline Cast Iron
    Join Date
    Oct 2004
    Location
    hangtown, california
    Posts
    457

    Default

    On mine it uses an M95, each read advances the count by 1. M30 also adds to the count. That complicates things figuring the actual # of parts, especially if you end up needing to run some shorter bar lengths. Not sure of a parameter setting to disable M30 for the count. I imagine there is one that can be changed.

  3. #3
    ARB's Avatar
    ARB
    ARB is online now Titanium
    Join Date
    Dec 2002
    Location
    Granville,NY,USA
    Posts
    3,614

    Default

    Set up a simple counter using your 500 variables.

    You can set it up to count bars or parts which ever works.

    To count parts

    In your sub program
    #501=#501+1

    This will index the value of #501 by 1

    If your sub makes 2 parts then #501=#501+2

    To see your 500s
    Hit offset
    Right soft button to find Macro
    type 501 hit no.search soft key
    At the start of your run set 501 to 0

    You can have a couple different counters set up. One to count the run and one to count the day. Or what ever you might want.

  4. #4
    Kris P is offline Hot Rolled
    Join Date
    Jan 2007
    Location
    FL
    Posts
    531

    Default

    I don't know if it is the one (counter)you're looking for, but on my ot-c, the parts counter is on the second page of the main paramaters list, lower right corner. Strangely, on my machine, it counts every M0, optional stop, as one count.

    I will have to investigate this G65/M95 you guys speak of. I have always written on the Haas I ran, the whole program as a sub, and just ran a code that started the program with M98P100 L20 (20 pcs)

    I usually throw in an M1 at the end before it recycles to the top so I can stop and check a part if need be.

  5. #5
    chet is online now Aluminum
    Join Date
    May 2004
    Location
    minnesota
    Posts
    153

    Default

    Quote Originally Posted by ARB View Post
    Set up a simple counter using your 500 variables.

    You can set it up to count bars or parts which ever works.

    To count parts

    In your sub program
    #501=#501+1

    This will index the value of #501 by 1

    If your sub makes 2 parts then #501=#501+2

    To see your 500s
    Hit offset
    Right soft button to find Macro
    type 501 hit no.search soft key
    At the start of your run set 501 to 0

    You can have a couple different counters set up. One to count the run and one to count the day. Or what ever you might want.
    no macro #500. my machine has #100-148 will other numbers work?
    it is a hardinge chnc

  6. #6
    stevo1 is offline Cast Iron
    Join Date
    May 2008
    Location
    Great State Of Wisconsin
    Posts
    435

    Default

    Quote Originally Posted by Kris P View Post
    I will have to investigate this G65/M95 you guys speak of. I have always written on the Haas I ran, the whole program as a sub, and just ran a code that started the program with M98P100 L20 (20 pcs)
    G65 is a macro call. It is similar to a sub call like you are using with M98P100. Except with a macro call G65P100 this will call program 100 as a sub but you can bring variable along with it. For example you can program G65P100A10B20. Now variable #1=10 and #2=20 and your sub program can be something like G0X#1Z#2.
    Quote Originally Posted by chet View Post
    no macro #500. my machine has #100-148 will other numbers work?
    it is a hardinge chnc
    You can use these variables. If they are anything like Fanuc they will reset to null at power down. Try to make sure that you put your counter were you actually complete a pc. Don't use the M30's and M0's ect. As like Michael stated it gets confusing and don't know when things are adding on. Best spot is right after you cut off a peice.

    Stevo

  7. #7
    michael is offline Cast Iron
    Join Date
    Oct 2004
    Location
    hangtown, california
    Posts
    457

    Default

    Good idea using the variables. Gonna make use of that straight away, thank you.

  8. #8
    alphonso is offline Stainless
    Join Date
    Feb 2006
    Location
    Republic of Texas
    Posts
    1,540

    Default

    Parameters:
    0040.3: count (0) or not count (1) total number of parts M2/ M30 executed.
    219: When preset Mcode is executed total parts is counted. setting 1-255. 0 =no setting. 98 and 99 cannot be set. (?????)
    0600: number of parts required, 0-9999
    779: number of parts in total, 0-9999999

    On my machine part count shows on the Position screen. Reset to 0 by pressing P then Cancel. Also displays actual cycle time: push green button to M30.

  9. #9
    michael is offline Cast Iron
    Join Date
    Oct 2004
    Location
    hangtown, california
    Posts
    457

    Default

    My control uses different parameter #s but same functionality. Setting initial parameter with a 1 disables M2, M30 for counting. Then the following parameter is set with whatever # within the range that you wish to use. M78, M223, etc. Thanks for making me look at the manual, alphonso. :~)

  10. #10
    Boris is offline Titanium
    Join Date
    Oct 2005
    Location
    England
    Posts
    3,002

    Default

    For OM-a and OM-b
    check use of the machine parameter #3901( i think... its in the Fanuc yellow book in the macro A section)
    this is the actual value in the part counter displayed on the POS screen

    So inside you sub program you'd add
    #3901=#3901+1
    just before your M99 line

    It also stays in the machine during power off

    Boris

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
  •