515,098 active members
4,230 visitors online
Register for free
Login
Page 1 of 3 123
Results 1 to 20 of 54
  1. #1
    Registered
    Join Date
    May 2009
    Posts
    393

    Question Paramteric Program

    Hi

    Wanted to know about parametric programming.

    What i want a program which will work as under -

    I will jog on to the part & after the edge finder kick, i will press cycle start. Than the machine control should capture the machine positions & store it on a memory card. The sequence of storing the locations will be the sequence of Point Pickup.


    Also wanted to know about the Spindle probe mechanism. I have heard that it automatically aligns the part to the machining centre. U don't have to break your head & hours for aligning the part to the machining centre.
    Some manufacturers like Heindan & Reinshaw have launched such product.


    Need Help...


    Ash

  2. #2
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Hey Ash,
    I finally found the post here. Anyway you got some answers to this in the PM I sent you but you still have not told me what control you are using?? This is very important as to the syntax and system variables that are going to be used to accomplish this.

    So please specify the control model you are using.

    Stevo

  3. #3
    Registered
    Join Date
    May 2009
    Posts
    393

    Cool Machine Control

    Thanks steve for your support, time & patience.

    I have an Mitsubhishi M64 control. The machine is Pinnacle 1100 Model.


    Ash

  4. #4
    Registered
    Join Date
    Dec 2006
    Posts
    49

    Parametric Programing Resource

    I am a newbie at parametric programing. Had 0 luck finding a contract programmer that could work in Fanuc Custom Macro B so I have resorted to taking an on line class. Just thought I would throw this out there for you.

    http://www.cncci.com/

  5. #5
    Registered
    Join Date
    May 2007
    Posts
    966
    Quote Originally Posted by HBFixedGear View Post
    I am a newbie at parametric programing. Had 0 luck finding a contract programmer that could work in Fanuc Custom Macro B so I have resorted to taking an on line class. Just thought I would throw this out there for you.

    http://www.cncci.com/
    What kind of machine(s) are you wanting programmed using Macro B? Rather surprised you couldn't find anyone. Steve is just one of several guys on this forum with lots of Macro B experience.

    More than one has helped me. Steve especially has been very helpful.

    Are you looking to program families of parts using Macro B, or for operations written using Macro B that can be used with any part?

    I did a Macro B lathe program a few months ago for a guy (for free) just because I really enjoy that type of programming. Unfortunately I only program for lathes. (Not by choice, however. )

  6. #6
    Registered
    Join Date
    Feb 2009
    Posts
    64

    Fanuc macros

    I learned to program macros straight out of a book. Peter Smid's Fanuc Custum Macro B was actually pretty good to get me started. Was a very quick read. Once you learn to work with the macro functions, going from one machine to the other isn't really all that complicated if you have that machine's manuals handy. There are usually only very slight variations in structure from one machine to the next.

  7. #7
    Registered
    Join Date
    May 2009
    Posts
    393

    Red face Hi All

    hI ALL...

    Thanks for your continual reply.

    But really could not any verdict over whether that type of parametric programming.

    & still fighting to know whether any such provision is there or not?

    :boxing:

    I guess i put it in a wrong fashion. I will try to put in a single sentence -

    "Can the machine positions be captured in a program file?"

    Ash

  8. #8
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Ash,
    Sorry for the late reply.

    Yes this should be possible on your machine. I don’t have much experience with Misubhishi controls so I am not going to have the right syntax for you. I will still give you an example of how you should be able to program this but you will have to fill in the proper variables.

    On my Fanucs there are variables that are the current machine position.
    #5041=current X position
    #5042=current Y position
    #5043=current Z position
    You will have to get the proper variables for your control that track the current position. Let’s say that you are going to try to find the center of a square part on the machine.

    O0001(find part program)
    M0(edge find right side then push cycle start)
    #100=#5041(sets right edge position to #100)
    M0(edge find left side then push cycle start)
    #101=#5041(sets left edge position to #101)
    M0(edge find top edge then push cycle start)
    #102=#5042(sets top edge position to #102)
    M0(edge find bottom edge then push cycle start)
    #103=#5042(sets bottom edge position to #103)
    #104=[#100+#101]/2(sets #104 to the center X of the part)
    #105=[#102+#103]/2(sets #105 to the center Y of the part)
    #5241=#104(#5241 is my G55 X variable. I don’t know what yours is)
    #5242=#105(#5242 is my G55 Y variable)
    M30

    You will have to find your variables for your workoffset or if you have the G10 function you can set it that way.
    G10L2P2X#104Y#105

    It is just a real basic program. A lot more can be added to make it do what you want.

    Stevo

  9. #9
    Registered
    Join Date
    May 2009
    Posts
    393

    Red face

    Hi Stevo

    Thanks for your time, patience & Support.

    Well, I again need to elaborate you about my requirement -

    We have parts which have a nominal tolerance & we want to inspect it on machining centre. As the geometery of the parts are round, square or rectangular shape, so it will be possible to inspect on machining centre.
    As the parts are not 3D profile & also not having close tolerance ( either customer would prefer CMM machine for the same ).
    So i want to do is edge find the part & than plot in a CAD software & then by deducting edge finder radius value & than conclude whether they reflect to the drawing tolerances.

    WELL I WANTED TO ASK, WHETHER IS THERE ANY SUCH PARAMETRIC PROGRAM WHICH CAN CAPTURE THE MACHINE READINGS IN A FILE (than the file can be transfered to Computer through Memory card ).


    Well i guess i have cleared the direction for all.


    Thanks All

    Ash

  10. #10
    Gold Member
    Join Date
    Jun 2008
    Posts
    1511
    Ok Ash I am with you now.

    Yes this is done all the time. It is the exact same concept of gathering the data points as I gave you in the previous post. This is commonly done and then the DPRNT function is used to send the data to PC/printer. Now I don’t know how to do it to the memory card because I don’t use one. I do know that it is possible. I can help you to write the program to get the dimensions of the parts into the variables on the machines but we are going to need someone else to chime in on the memory card syntax. I will also need some help with the exact code your Mits control uses.

    Do you have any books on this control or anyway of finding out what the variables are for the “current machine position”? Any examples on macro programming would also be helpful.

    The most logical thing to do is write 3 separate programs to find the points on a square, rectangle, and circle then put that data in the variables so that they can be written to the memory card.

    The “parametric” forum here does not get a lot of traffic so if we don’t see anyone chime in on the memory card or some pointers on the mits code then I will PM a few people to see if they can help out.

    Stevo

  11. #11
    Registered
    Join Date
    Feb 2009
    Posts
    64

    Output Macros

    You would be using the DPRINT like steveo was saying in addition to POPEN and PCLOSE. A very generic macro to do what you are asking would look something like this :

    O1234
    POPEN
    #33 = 0
    WHILE [#33 LE [#2-#1]] DO1
    #32 = #[#1 + [#33]]
    #31 = #33+#1
    DPRNT [VAR #3[5] ***DATA #32[57]]
    #33 = #33 +1
    END1
    PCLOSE
    M99


    Call using g65 p1234 A(lowest # variable to be sent). B(highest variable sent)

    This should store the variables into a .txt file. I will be away from the machine until tomorrow and will look further into it when I do. Also, like steveo was saying, would need more information on your machines macro variables and acceptable codes.

  12. #12
    Registered
    Join Date
    May 2009
    Posts
    393

    Smile

    oK...

    gUYS....

    I will dig it from the machine manual...

    I will let you know as soon as possible.

    Ash


    Thanks for your time, support & Patience

  13. #13
    Registered
    Join Date
    May 2009
    Posts
    393

    Question

    Hi.

    Guys did a lot of digging the whole night on the machine as well as in the manual. I Jogged the machine to a position ( X175.0 Y175.0 Z175.0 ) & was finding the value in the parameter as well as variable, but i couldn't find any such value either on the machine.

    I guess these variables values are hidden.


    :tired:

    & Basically as i am unware of variables & parameters, i guess i was digging up in a wrong fashion..

    Well luckily all the Mitsubhishi's manual are avaliable at -

    http://meau.com/eprise/main/sites/pu...FAM=0001010005

    Also if anyone provide me the mail Id i can mail the same manuals.


    I gave a wrong input previously, my Control is M60S & not M64 Magic.

    Regards,

    Ash

    Thanks for your time, support & patience.

  14. #14
    Registered
    Join Date
    May 2009
    Posts
    393

    Found it

    Hi All...

    I google down the Peter Smid Book & really its very very helpful. I found the same Parameter number embedded for my Mits Control too.

    Its 5021 - X axis
    5022 - Y axis
    5023 - Z axis


    In MDI, I commanded -

    #101=#5021 & it changed the value of the local variable to the current machine position in X axis.

    :banana:

    Now, i want to frame a program picking up 2 positions on the machines & than saving the same in a txt file (as charlie told ).

    Stevo & Charlie - Please help me out.

    Also Charlie, u gave me the program of capturing the variable data into control's memory, but can u describe the meaning of each of those codes so i can proceed further...That will be really thankful.

    Ash...

    Thanks for your continual time, patience & really thankful to all of you.

  15. #15
    Registered
    Join Date
    May 2009
    Posts
    393
    Hi James

    Well i guess u wrote down the program to output varaible data throught RS 232C Port. Well my machine does not any such provision. It has a memory card.

    Does that program needs any output storage location setting ???

    Also what we can do is write the variable data into machine control memory & than copy it on to memory card.



    Ash.

  16. #16
    Registered
    Join Date
    Feb 2009
    Posts
    64

    Sick

    Sorry I've been out a bit.. sick. I should be back at the controller tomorrow to rack my brain some more. My controller also uses a memory card so I'm trying to puzzle out the same thing. I'm thinking that it may be a setting on the controller to determine the location of variables saved through dprnt and will look into it further.

  17. #17
    Registered
    Join Date
    Feb 2006
    Posts
    1770
    I also want to know how to DPRINT on a PCMCIA memory card.

  18. #18
    Registered
    Join Date
    May 2009
    Posts
    393

    Arrow Awaited Response

    Well, its long long time now & we need to fix the Problem as soon as Possible.

    I had been through Custom Macro B programming Book (by Peter Smid). It referes to a format which outputs the Variable to a TXT file.

    Well, James L also discused it before.

    But anyone please help to let understand the Program Format & Loop Function ?


    Also it was mentioned in the book that is it not Possible to Output a Varaible Output TXT file on a Memory Card. It is only possible through RS232C port.

    We all were trying to debug the Problem for which there is no Solution.




    Also can anybody post a Varaible TXT file (output through RE232 port) ?

    Ash.

    Thanks for your TIME, PATIENCE & SUPPORT.
    Attached Thumbnails Attached Thumbnails Format.JPG  

  19. #19
    Registered
    Join Date
    Feb 2006
    Posts
    1770
    Quote Originally Posted by stevo1 View Post
    On my Fanucs there are variables that are the current machine position.
    #5041=current X position
    #5042=current Y position
    #5043=current Z position

    Let’s say that you are going to try to find the center of a square part on the machine.

    O0001(find part program)
    M0(edge find right side then push cycle start)
    #100=#5041(sets right edge position to #100)
    M0(edge find left side then push cycle start)
    #101=#5041(sets left edge position to #101)
    M0(edge find top edge then push cycle start)
    #102=#5042(sets top edge position to #102)
    M0(edge find bottom edge then push cycle start)
    #103=#5042(sets bottom edge position to #103)
    #104=[#100+#101]/2(sets #104 to the center X of the part)
    #105=[#102+#103]/2(sets #105 to the center Y of the part)
    #5241=#104(#5241 is my G55 X variable. I don’t know what yours is)
    #5242=#105(#5242 is my G55 Y variable)
    M30
    I have a confusion.
    I understand that MCS coordinates are fed into work offset system variables, for shifting the workpiece zero point to the desired location.
    If so, shouldn't #5041 etc. be replaced by #5021 etc?

  20. #20
    Registered
    Join Date
    Feb 2006
    Posts
    1770
    For the benefit for those who have never used a WHILE statement, I have attached one example with complete explanation. on Ashish's request.
    Attached Files Attached Files

Page 1 of 3 123

Similar Threads

  1. Mazatrol Program into a G Code Program
    By fuzzman in forum Mazak, Mitsubishi, Mazatrol
    Replies: 15
    Last Post: 09-25-2012, 04:27 PM
  2. Replies: 12
    Last Post: 03-15-2010, 02:19 AM
  3. Program Restart in mid program?
    By Donkey Hotey in forum Haas Lathes
    Replies: 16
    Last Post: 03-18-2008, 08:19 PM
  4. Need a CAM program
    By SteveD in forum Community Club House
    Replies: 3
    Last Post: 09-28-2006, 07:46 PM
  5. Replies: 11
    Last Post: 10-09-2005, 05:45 AM

Posting Permissions

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