Results 1 to 10 of 10
  1. #1
    SolutionEng is offline Plastic
    Join Date
    Aug 2007
    Location
    Minnesota
    Posts
    26

    Default Need help with Yasnac Mx3 basic set up procedures.

    I have a new to me Yasnac Mx3 on a matsuura mc760-v and would like some help on the basic set up, like setting zeros and tool lengths etc. This control doesnt seem very user friendly. I have the manuals but cant seem to find any info on setting work coordinates and doing simple things like setting xyz zero in the position screen. Any help would be appreciated. I found where the program memory is by searching this site.

    Thanks

  2. #2
    CPT Crunch is offline Cast Iron
    Join Date
    May 2005
    Location
    Vancouver, WA
    Posts
    452

    Default

    Measuring tools on this machine is easy. With Z in a known and repeatable position (usually home), push the "mesurement" button. A green LED should turn on. Handwheel the tool down and measure it however you want. Then push the OFS (offset) key on the keypad. Use the arrow keys to put the cursor on the tool # you are measuring (or where ever you want to store the length) and then push the "write" button. The tool height will be automatically recorded and Z will return to home position by itself. Tool lengths are stored in the table without a decimal point (4 places after the decimal is assumed), but you can use a decimal for input if you want. If you try to enter a number by pushing number keys and then wr it will be added incrementally to the current value. The only way I know to zero out the offset is to enter the opposite value.

    To enter work coordinates, push SET on the keypad. This will take you to a page that looks like parameters (that's because they are parameters). Enter 6516 and then push the down arrow. This will take you to parameter #6516 which is G54 X. Here you'll need to enter the zero coordinate without a decimal. If you want x zero to be -14.82, then you would enter -148200 (notice the 4 places after the decimal). #6517 is Y and #6518 is Z (Z will be the distance from where you measured your tools to Z0). There is a table of these parameter numbers in the manual. We have the table taped to the control for reference.

  3. #3
    SolutionEng is offline Plastic
    Join Date
    Aug 2007
    Location
    Minnesota
    Posts
    26

    Default

    Thankyou CPT, I appreciate it. I will be trying it out today and let you know how it goes.

  4. #4
    Greg White is offline Titanium
    Join Date
    Jan 2007
    Location
    Pinckney Mi.
    Posts
    2,376

    Default

    I have a MX2 on my Mat..,that was very usefull data ,thanks.
    I have been G92in everything and working with bastard numbers.

    Have you been to the Yasawa site and downloaded the manual for the control? they make the Yasnac, mine was 270 pages aboot my control.

    I been with mine maybe 2 months now,gaining confedence daily,Ill be printing your comment and taking it to machine.

    as a aside,is the way you enter data without a decimal called binary data entrey?
    Gw

  5. #5
    CPT Crunch is offline Cast Iron
    Join Date
    May 2005
    Location
    Vancouver, WA
    Posts
    452

    Default

    Hi Greg,

    Glad I could help. Remember that if you have G92'd any axis, you'll need to use G52 to cancel it before trying to use G54 etc. Otherwise, the offets will get added together. I'm not sure what the "decimal-less" data entry is called, but I'm pretty sure its not binary data entry. I think its called something like least increment entry because you're entering how many of the smallest steps to use.

  6. #6
    BudJackson's Avatar
    BudJackson is offline Plastic
    Join Date
    Jan 2011
    Location
    Baltimore, Md. USA
    Posts
    28

    Default

    Quote Originally Posted by CPT Crunch View Post
    ..... The only way I know to zero out the offset is to enter the opposite value.....
    have cursor on offset you want to zero out and just press the Origin "ORG"
    key.

    You can delete all offset in one shot buy typing, while on the offset page,
    O-9999 then press ORG.

    I perfer Yasnac controls but currently slugging it out with a Fanuc 31i X5
    and the control is winning

  7. #7
    Greg White is offline Titanium
    Join Date
    Jan 2007
    Location
    Pinckney Mi.
    Posts
    2,376

    Default

    Thanks Capt & Bud,I am not using any XorY offsets yet,just Z.


    It bothers me that the locations shown after a offset(in Z anyway) are still bastard numbers,is that changable?

    By that I mean if T1 zero(top of part) is -12.9865, the when you tell tool 1 to go to zero it displays Z-12.9865,should i just get ust to it?

    Are X&Y offsets displayed as bastard #s?


    I am still bowing to my Yasnac ,I am not yet its master.

    G92 is prolly not INTENDED to be used in a program,just in set up mode,eh???
    Gww

  8. #8
    SolutionEng is offline Plastic
    Join Date
    Aug 2007
    Location
    Minnesota
    Posts
    26

    Default Another question

    I have been running this machine for a while now and really like it.
    However, I am thinking about starting to preset tools offline and would like to know what procedures the MX3 guys are using. I am thinking I want the table top as z-zero and right now it is at z-home. I would like to get away from offsets with large negative z's. My machine came with the Matsuura presetter table and I like the idea of having each tool lenght offset the measured length from gauge line to tip of tool. Any ideas about how to get there? For starters I think I need to change the z-zero to the table top but havent a clue where to start.
    -
    Correct me if i am wrong...
    I want z-zero at the table top.
    I want tool lengths to be from guageline to end of tool.(positive number)
    I want my G54, z to be the distance from table top to top of work. (part zero)
    -
    What do I have to change in the control parameters?
    How will this affect my programming.?
    How will this work with the auto-tool measurement buttons?
    Is it all even a good idea?
    -
    How did Matsuura propose this all to work?


    thanks fellas

  9. #9
    CPT Crunch is offline Cast Iron
    Join Date
    May 2005
    Location
    Vancouver, WA
    Posts
    452

    Default

    You don't need to change the measurement reference point (z-zero). The only thing that you need to change is the G54, which will be the distance from the gage line while at the measurement reference point to your part zero. I like to think about it like this: The tool length offsets tell the machine how far to move each tool so that their tip will be at some known location (doesn't matter where). Then, the work coordinate offset tells it how far to move to get to the part Z0. Next, the machine adds the Z from the program to figure out the final position.

    TLO + G54 Z + Z in program = Final Z position

    So if you don't want the TLO to be a large negative, then you have to make G54 a large negative to compensate. Now if you wanted to make G54 the distance from the table to the part zero, there is also a parameter you can set that will add a constant value to all the TLOs. I haven't played with that, but I read about it here:

    http://www.practicalmachinist.com/vb/cnc-machining/fundamentals-tool-work-offsets-210936/#post1430821

  10. #10
    SolutionEng is offline Plastic
    Join Date
    Aug 2007
    Location
    Minnesota
    Posts
    26

    Default

    Everything has been going pretty well and I appreciate all the help.
    I have had some issues with the z going past home on a toolchange and alarming out.
    -
    Here is the end of one tool and the beginning of the next:
    N1390 G41 D1 X6.4265 Y-2.2263 F35.0
    N1400 G03 X6.5 Y-2. I-0.3115 J0.2263
    N1410 X5.5 Y-2. I-0.5 J0.
    N1420 X6.5 Y-2. I0.5 J0.
    N1430 X6.4265 Y-1.7737 I-0.385 J0.
    N1440 G01 G40 X6.115 Y-2.
    N1450 G00 Z0.2
    N1460 M09
    N1470 (END TOOL)
    N1480 M05 G40 G49 G80
    N1490 M09
    N1500 G91 G28 Z0
    N1510 (0.16INCH DRILL, 135 INC)
    N1520 T2 M06
    N1530 G00 G90 G54 X4.456 Y-1.0493 S2500 M03
    N1540 G43 H2 Z0.2
    N1550 M08
    N1560 G00 X4.456 Y-1.0493 Z0.2

    If I add a g28 line at N1455 then the machine doesnt alarm out and it toolchanges fine.

    Do any of you guys have examples of tool beginnings and endings that are known to work on a Yasnac mx3? Even a multiple tool program would be fine. My machine is a matsuura mc760-v

    Thanks

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
  •