Fanuc 3TD basics
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 32
  1. #1
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default Fanuc 3TD basics

    While i In-patiently wait for my Manuals can anyone help with some basics for this control?
    Fitted to a Mori SL3

    It the one with the LED display for everything, CRT only for the FAPT, which seems to work btw!
    Atm im unable to change spindle speed. Manual dial making no difference, i know it did work when i first looked at the machine.
    Spindle runs, but at what must be 25RPM. Need help with Keying in the speed.

    Needing a basic rundown thanks!
    Attached Thumbnails Attached Thumbnails 20190619_213843.jpg  

  2. #2
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    2,421
    Post Thanks / Like
    Likes (Given)
    246
    Likes (Received)
    644

    Default

    Try this- put control in MDI mode. press these keys on keypad "m03s500EOB enter" then hit "start" either on the keybad or the cycle start button. You may have to close the chuck jaws to get this to work, as it's probably interlocked. If that does not start the spindle, try putting a "g97" in the above command line. Also, you may or may not need the "EOB". On edit- that machine has a 2 speed gearbox. You should have a op panel button the select low, high and neutral- make sure you are not in neutral.

  3. Likes Kenre liked this post
  4. #3
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    Dan,

    Which page should it be entered in? Pos, Program, offset etc?
    ,

  5. #4
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    4681
    Likes (Received)
    1618

    Default

    Should be on the program screen. You could possibly need a gear (M41,M42) range added before your spindle command.

    M41 ;<EOB, IMPUT, THEN START
    G97 S300 M3;<EOB, IMPUT, THEN START

    After you have the spindle running in MDI turn the dial to manual then you should be able to control the speed with the STOP FORWARD REVERSE buttons and up/down speed dial.

    Did try on conversational side?

    Brent

  6. Likes Kenre liked this post
  7. #5
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,190
    Post Thanks / Like
    Likes (Given)
    4681
    Likes (Received)
    1618

    Default

    A good quality picture of the whole control panel may help spark folks memory when trying to offer help.

    Brent

  8. Likes cameraman liked this post
  9. #6
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    Thanks! got it working!

    I will try switching to manual tomorrow for the dial etc.

    I have only turned on the conversational, going through the screens it seems to be all there. Not bad considering the age, running from a cassette tape.

    Next is to work out setting the tools, i have read a bit on the G50 in here.
    What is the U and W?

    I have ordered new manuals, Takes up to 3 months to arrive, still a couple to go, dont want to wait that long lol

    I will get a better pic tomorrow.
    Attached Thumbnails Attached Thumbnails screenshot_2019-04-10-mori-seiki-sl3-cnc-lathe-ebay.jpg  
    Last edited by Kenre; 06-20-2019 at 06:19 AM. Reason: spelling

  10. Likes yardbird liked this post
  11. #7
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    2,421
    Post Thanks / Like
    Likes (Given)
    246
    Likes (Received)
    644

    Default

    Go thru your offset pages on the control and see if you have a geometry offset page. if you do have that page, there is no need to use G50 to set your tool offsets. Report back and I'll go thru how to set your tools if you have the geom offsets. U and W are incremental X and Z values respectively.

  12. #8
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    Turning it from MDI to manual the spindle stops, Manually switching spindle on its back to about 25rpm. no luck with the manual speed control.
    I i switch straight back to MDI it starts again from the previous speed set.
    Attached Thumbnails Attached Thumbnails 20190621_114230.jpg  

  13. #9
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,401
    Post Thanks / Like
    Likes (Given)
    805
    Likes (Received)
    2370

    Default

    Quote Originally Posted by Kenre View Post
    .....no luck with the manual speed control.......
    The manual speed control is just a potentiometer that controls a 0-10V analog signal to the spindle drive. If you have a wiring diagram for the machine it would be easy to trace wires and check for voltages at the pot and spindle drive.

  14. Likes Kenre liked this post
  15. #10
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    I dont think its an electrical problem, (well hope not,wiring diagram is another manual in waiting on)
    It was working when i inspected the machine.

  16. #11
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    Vancbiker,

    That will teach me to think it was something in the control i needed to set!
    Found a broken solder joint on a row of resistors behind the front panel.

    I now have manual speed control, Thanks!

    Now i can take a cut and start setting up tool offsets, Let the lessons begin!

  17. Likes solidworkscadman, Oldwrench liked this post
  18. #12
    Join Date
    Mar 2011
    Location
    MASS
    Posts
    935
    Post Thanks / Like
    Likes (Given)
    391
    Likes (Received)
    286

    Default

    This is a blast from the past, i enjoy posts like this

  19. #13
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    Dan, Vancbiker,

    Or anyone willing and patient, be able to guide me through tool offset setup.
    Yes im brand new to this Fanuc programming, i have a little g code experience with milling, but only with Mach3, so that doesnt count!
    I think i seen G50 on the LED display when playing around, but unable to find it again.

    I will be needing a step by step, button by button press guide.

    Thanks
    Ken

  20. #14
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    2,421
    Post Thanks / Like
    Likes (Given)
    246
    Likes (Received)
    644

    Default

    A G50 command in your program will always work regardless of what offsets you have available but life is much more simple if you have geometry offsets available. Have you looked for how to access your offset table(s)? Best to know that 1st.

    G50 tells the control where your tool tip is relative to the part zero and the current x and z slide position BUT there are multiple ways to make your life hell if you don't understand how to set a home position and determine x and z values for the current setup. Not understanding how G50 works can lead to nasty crashes as well.

  21. #15
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    Dan,

    I dont know how to get into the offset table. I assume its under offset in the LED display?
    Without the manual,i really do not know how to access things, not knowing what button does what hinders things!

  22. #16
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Hello Ken,
    Your control with FAPT basically has two sides, the FAPT and the NC. The Seven Segment display is for the NC component of the control and is tantamount to the configuration of very early FS6 controls that had a Seven Segment display which was just about identical to the previous FS5 control; only a very few FS6 controls had the Seven Segment display, with later controls having a CRT screen display.

    The normal mode of function of your control/machine is to create a part program using the FAPT, at the end of which, the NC program is passed to the NC Side of the control. This control, with the Seven Segment display, will drive you nuts if you try to create a part program directly by the using the NC Side of the control. Only one address at a time can be inserted and when inserting the next address, the whole of the previous code inserted is unseen.

    The FAPT Side is quite powerful and was/is one of the better Conversational Programs available; the resulting part program is readable and operational exactly like any other NC program for a Fanuc Control.

    Even when reusing an existing program at a later date, you would be well advised to get a PC connected to the control, so that the program can be easily viewed and verified as correct before uploading it to the control. Programs in memory can only be viewed address word by word.

    Even from the point of view of normal program running, you will find that running the program via DNC, with appropriate Software, will be far more convenient than running a program from memory. Following is a picture of my Software connected to a FS5T control and running in DNC Mode. The big advantage is that a whole page of the program is displayed at any one time and the Pending Block is displayed in Highlight.

    dnc1.jpg

    Regards,

    Bill

  23. Likes Kenre liked this post
  24. #17
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    Hi Bill,

    I do intend to use a PC for the part programs. Have one ready to go for it. even have the rs232 cable.

  25. #18
    Join Date
    Apr 2007
    Location
    Melbourne Australia
    Posts
    196
    Post Thanks / Like
    Likes (Given)
    33
    Likes (Received)
    20

    Default

    Great news, All my manuals have arrived!

    I think i have worked out how to set the part zero position.
    What i cant get my head around ( manual isnt very clear in explanation) is setting tool offsets.

    Eg, I Zero turret, move to part end, add the part length to Z axis for my zero point. eg, 253.100+100 = 353.100
    X axis add turned piece diameter to X geometry from zero.
    These X and Z coordinates go into my G50 in the Program for origin point on drawing.

    Manual says tool offsets are set with Eg T0401 04 being tool number(this is my WNMG for steel) which i use to set the main G50 origin
    I cannot work out the second 2 numbers. 01, 02 etc. How and what do these relate to in each tools offset from
    My original tool position?

  26. #19
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,613
    Post Thanks / Like
    Likes (Given)
    1188
    Likes (Received)
    666

    Default

    Have a look at this thread... How to use G50 on Fanuc 6T

    I have just got my mind around the whole G50 thing with the help from the folks on here and the guy I am helping out. I still make sure that every time a tool retracts it goes to the same position to the machine co-ordinates but it scares the shit out of me on a old Mazak where you cannot turn rapids down at all, only completely off or full ball. I feel like a genius on an OT or Oi but these older one's scare the shit out of me. "We" have an old takisawa that runs off a control similar to yours. Haven't had the balls to set it up yet.

  27. Likes Kenre liked this post
  28. #20
    Join Date
    Sep 2005
    Location
    Oakland, CA
    Posts
    2,421
    Post Thanks / Like
    Likes (Given)
    246
    Likes (Received)
    644

    Default

    Regarding your tool offsets. IE: T0401. I strongly suggest you keep your offsets with your tool position- T0404. Even if you use tool 4 to set your Z zero. We still don't know if you have geometry offsets or only wear offsets. Anyway, the 2nd pair of numbers in your tool call are telling the control what offset to use. The 1st pair of numbers will index the turret to that station. If you have geometry and wear offsets, the actual offset will be a combination of the two. If not, then the offset will be your wear offset.
    Calling TXX00 will index the turret but no offsets. You should always clear your offset with this command before going back to your home position. Hope you are understanding how the G50 works as this is an absolute requirement to keep from crashing your machine.

  29. Likes Kenre liked this post

Tags for this Thread

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
  •