545,673 active members*
2,116 visitors online*
Register for free
Login
Results 1 to 7 of 7
  1. #1

    Macro Program for Eumach VMC

    Dear Friends

    We are having Eumach VMC Model MC800P with Fanuc 0Mf control. Due to power surge All parameters & Programs lost. We re entered all the parameters M/C is Running. Due to Macro Program Deleted ATC not working. Any body having the Macro program for this machine. Pl. Help me. We are herewith attaching the photo of our VMC for your ref.
    Attached Thumbnails Attached Thumbnails Eumach.jpg  
    L. Sakthivel
    Email:info@premierengrs.com, website:www.premierengrs.com

  2. #2
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Do you not have the tool change program at all?? Or do you have it and it is not working properly? If you have the progam post the code and we will try and help. If you do not have the program which I am guessing you don't. Try to contact the MTB to see if they can get it for you. If they can not get it and no one here has it we can start writting one.

    Stevo

  3. #3
    Dear Mr. Stevo

    We are not having Macro program. We tried to contact MTB, we are unable to get the program, Thats why I posted in this Forum to get it from the user of the same machine.
    L. Sakthivel
    Email:info@premierengrs.com, website:www.premierengrs.com

  4. #4
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Your M6 logic should still work for the actual changing of your tool. All that should have to be done is the macro for the tool change position and various other codes. There is a few ways to use the variables to do this program. This is an example of the tool change macros that I write.

    O9020(TOOL CHANGE PROGRAM)
    #20=#4120--sets #20 equal to the T-code when you call a tool T2M6
    G40G80—tool dia cancel. Canned cycle cancel
    IF[#20EQ#535]GOTO1 (see note1)
    G91G28Z0M9—send tool to tool change position in Z. turn off coolant (see note 2)
    M19--orientate spindle
    G28Y0M5—send tool to tool change position in Y. turn off spindle (see note 3)
    M6—tool change
    N1G90G49Z#5043—cancel tool length offset with no movement
    #537=#[2000+#20]+#[2200+#20] (see note 4) gathers tool length data
    G43Z[#5043-#537]H#20 (see note 4)
    #535=#20 changes #535 to the tool just put in spindle
    M99

    Note 1. I choose to use a variable to keep track of the current tool in the spindle. I choose #535. You could use the system variable that tracks this. However I do not know which one it is for your control. You would have to find that out. This will skip the tool change M6 if you are calling the tool that is already in the spindle.

    Note 2. Change the Z value to your too change position Z. If your tool change position is not Z0 and you do not want to hard code it you can set up your floating reference point position in your parameters and use for example G30Z0.

    Note 3. Change the Z value to your too change position Y. Same details of note 2 if you do not want to hard code the position.

    Note 4. This is not necessary unless your tool change macro in the past set your tool length offsets. I use this so I do not have to program the G43Z3H2 in all of my programs. This automatically sets the tool length of the tool that I am calling. There will be no tool movement because the Z value is the tool length minus the machine position. If you choose to use this you will have to get the proper system variables for your tool offsets. Example #2000 on mine is the tool length and #2200 is the wear. You have to find your length and wear and change the 2000 and 2200 in the program. They might be the same system variables as above. If am not 100%

    Now in order to set this up as a macro call with your M6 code. If you have reloaded the parameters then you might have a M6 already set up. For your control:
    Parameter 203-239 sets programs 9020-9029
    Parameter 240-242 sets programs 9001-9003

    So for my program above number 9020 you would have to set parameter 203=6. Or if you wanted to use program 9001 you would have to set 240=6. If you had a macro before then check these parameters to see if any of them are set equal to 6. If for example parameter 204 is set to 6 then everytime a M6 is programmed it will call program 9021.

    There might be some other specific codes for your machine that might need to be done but can be worked out.

    Stevo

  5. #5
    Thank you Mr. Stevo for your Informations. I hope this will help all. I try this and comeback to you
    L. Sakthivel
    Email:info@premierengrs.com, website:www.premierengrs.com

  6. #6
    Registered
    Join Date
    Jun 2007
    Posts
    6
    Quote Originally Posted by L. Sakthivel View Post
    Thank you Mr. Stevo for your Informations. I hope this will help all. I try this and comeback to you
    i also have eumach v 24 , but i dont have elctrical book , so if any body kindly reply
    jaggi421@yahoo.co.in

  7. #7
    Registered
    Join Date
    Feb 2006
    Posts
    211

    Re: Macro Program for Eumach VMC

    Quote Originally Posted by jagdeep View Post
    i also have eumach v 24 , but i dont have elctrical book , so if any body kindly reply
    jaggi421@yahoo.co.in
    I have a EUMECH MC800P equipped with Fanuc OM C & Alpha servo & spindle.
    I need it's parameters, Diag. parameters & ATC Macro.
    Kindly help me somebody.

    ahe_303@rediffmail.com

Similar Threads

  1. Replies: 3
    Last Post: 03-20-2017, 01:21 PM
  2. help with sub-program in macro-A
    By landslide1 in forum Fanuc
    Replies: 2
    Last Post: 05-16-2013, 05:50 AM
  3. Please help with this macro program
    By Behnod in forum Parametric Programing
    Replies: 7
    Last Post: 03-05-2013, 05:09 PM
  4. Replies: 2
    Last Post: 03-27-2009, 09:15 PM
  5. Eumach Spindle Driver Not Ready
    By hmaxa in forum Uncategorised MetalWorking Machines
    Replies: 1
    Last Post: 10-28-2007, 10:29 PM

Tags for this Thread

Posting Permissions

  • You may not post new threads
  • You may not post replies
  • You may not post attachments
  • You may not edit your posts
  •