Index position on cnc lathe
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 34
  1. #1
    Join Date
    Feb 2016
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default Index position on cnc lathe

    Hi all,
    I am getting back into setting up cnc lathes after being off them for a long time.
    can anyone tell me how to set index position closer to chuck without having to go back to
    machine zero on every index?
    I am aware of tool clearance possible issues getting closer to chuck.
    is there a simple method?
    any help would be great
    thank you

  2. #2
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,228
    Post Thanks / Like
    Likes (Given)
    350
    Likes (Received)
    566

    Default

    Lets start with what kind of lathe you're running.

    Are you talking about the Fanuc G28 U0.W0. ?

    Have you tried adjusting those numbers?

    Does this answer your question?
    https://www.cncci.com/resources/tips...28%20works.htm

  3. #3
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    86
    Likes (Received)
    19

    Default

    Quote Originally Posted by Andrew65 View Post
    is there a simple method?
    Do it in the program. Replace the block that tells the turret to go to home position with for example G00 X5.0 Z5.0 (assuming there is enough clearance for the turret to index without a tool hitting the chuck/workpiece).

  4. #4
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    It shouldn't make any difference on a Fanuc. OTOH if it's an Okuma, you need to be against the switches. (Which is brilliant).

    Why, oh why would you want to Index in an un-safe spot? Just Index, then jog, the Index, then jog. Tools caught on Chuck is bullshit and really embarrassing, when you need to tell someone. Not that I have ever done it.

    R

  5. #5
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    400
    Post Thanks / Like
    Likes (Given)
    18
    Likes (Received)
    161

    Default

    Depends on the machine and it’s control. Some older machines require each tool to be indexed at the home position. Others do not. What are you running?

  6. #6
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,678
    Post Thanks / Like
    Likes (Given)
    296
    Likes (Received)
    1796

    Default

    I for one never send SOME of my machines to home, in fact on the NL-SY I can't even do it period!

    Anyway, for indexing I just code:
    G00 G53 Xnn Ynn
    TXXX

    Where nn is a known safe position in the machine coordinate system to rotate the turret at.

  7. Likes Vancbiker liked this post
  8. #7
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    Quote Originally Posted by SeymourDumore View Post
    Where nn is a known safe position in the machine coordinate system to rotate the turret at.
    If it a "known safe position" that's great. But if a guy is just randomly Indexing the Turret wherever, it's going to end up bad eventually.

    R

  9. #8
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,056
    Post Thanks / Like
    Likes (Given)
    761
    Likes (Received)
    2141

    Default

    Quote Originally Posted by litlerob1 View Post
    If it a "known safe position" that's great. But if a guy is just randomly Indexing the Turret wherever, it's going to end up bad eventually.
    When I did field service we typically trained folks to pick a known safe position to index rather than machine zero. One customer, (tier 1 automotive supplier) wanted to eke out every scrap of cycle time so they wanted to index with the next tool just a 1/2" away from the part when going from short tool to long. Actually never really caused any problem. I do not recall ever going there to fix a crash caused by indexing close in. The nature of that type work though. High volume, low mix. ~900 parts per shift. Same old, same old, day in and day out. Offset changes not allowed unless feature measurement was using 80% of tolerance. Any kind of hiccup and the operator had to get a supervisor to deal with it. Figure out how to save a couple seconds on the cycle time and you were a hero to the department head.

  10. #9
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    I've done similar stuff, in the program.

    Not during set-up. But WTF do I know.

    R

  11. #10
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,678
    Post Thanks / Like
    Likes (Given)
    296
    Likes (Received)
    1796

    Default

    Quote Originally Posted by litlerob1 View Post
    If it a "known safe position" that's great. But if a guy is just randomly Indexing the Turret wherever, it's going to end up bad eventually.

    R
    Rob, You're correct that the guys should not just randomly index the turret wherever.

    But to the OP:

    can anyone tell me how to set index position closer to chuck without having to go back to
    machine zero on every index?
    You can initially do so by writing each and every program with a toolchange as:
    G00 G53 X0 Z0
    Txxx

    Then, during setup, the guy can move the turret to a position at which ALL tools are clear away from the part, and read the machine X and Y coordinates ( absolute mach. coords!!! )
    Then he can do a change of all values on each of those lines to the read coordinates.

    Sooner or later you will find a reasonably safe, common place to index your turret based on the machine's size and envelope and hard code it into your post.

    OTOH If/when you have a long and high qty run, just change the same values individually for each tool.
    Just as Vanc said, it can be puckerfactor close.
    With inserted tooling that never change in length or position, you might as well index the freakin' thing .05 away from the part!
    Guaranteed .05 might as well be a mile right?

    ( No joke, you can actually use a toolchange to knock off birdsnests from the part! )

  12. #11
    Join Date
    Jan 2019
    Country
    UNITED STATES
    State/Province
    Arizona
    Posts
    432
    Post Thanks / Like
    Likes (Given)
    29
    Likes (Received)
    146

    Default

    why not just program it into the bottom of every tool

    for example been doing this for 25+ years I have found
    G00G97X6.0Z6.0
    G00T0100
    M01
    for most 6 and 8" chuck machines. if your using long tools then change the Z to 8" or 10 or what ever.

    my Miyanos with twin turrets I use 4" on the Z.
    In the morning turn power on take machine home, jog off home switchs hit button and run parts
    on the z axis I could go shorter but WHY risk it.

  13. #12
    Join Date
    Sep 2015
    Country
    UNITED STATES
    State/Province
    California
    Posts
    400
    Post Thanks / Like
    Likes (Given)
    18
    Likes (Received)
    161

    Default

    I’m running Miyanos with Fanuc controls and they will allow tool indexing anywhere without requiring the machine to run to the “home” position. I always end every tool path with an M1 so that during setup I can check clearance before the next tool indexes. I also try to make all my tool lengths to match whenever possible. Especially on the “Z” tooling where I can have two tools on one station.
    My old Nakamura however, did require you to return the turret to the home position to index tools and cal offsets.

  14. #13
    Join Date
    Feb 2016
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    I believe the place I used to work at put the same numbers at the end of each cycle.
    X11. Z11. I think they used.
    Question: If each cycle used same X11. Z11. numbers and say you were using a long insert drill as well as stick tools then the turret would rapid back to a different position when going to index. is that right?
    if this is correct,
    how does the machine know its location when it indexes to next tool?

  15. #14
    Join Date
    Dec 2018
    Country
    UNITED STATES
    State/Province
    Pennsylvania
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    86
    Likes (Received)
    19

    Default

    Quote Originally Posted by Andrew65 View Post
    I believe the place I used to work at put the same numbers at the end of each cycle.
    X11. Z11. I think they used.
    That sounds like numbers that were spit out by the programming of the machine controller on older machines.
    We have that at my job.
    I changed them all to the home position. No silly numbers in my programs

    Unless you run high volume low cost parts where seconds matter, no one should index anywhere else but the home position.

  16. Likes litlerob1, StinkyDan liked this post
  17. #15
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,056
    Post Thanks / Like
    Likes (Given)
    761
    Likes (Received)
    2141

    Default

    Quote Originally Posted by Fancuku View Post
    ......Unless you run high volume low cost parts where seconds matter, no one should index anywhere else but the home position.
    So a user with a lathe with a long Z travel should always go to the home position to index when doing chucker work? Better would be to just learn how to use the control and program to use a safe index point.

  18. Likes litlerob1 liked this post
  19. #16
    Join Date
    Aug 2005
    Location
    CT
    Posts
    7,678
    Post Thanks / Like
    Likes (Given)
    296
    Likes (Received)
    1796

    Default

    Quote Originally Posted by Fancuku View Post

    Unless you run high volume low cost parts where seconds matter, no one should index anywhere else but the home position.
    It ain't about the seconds, but why on Earth would I send the turret home when 99% of the time I can index at X-8./Z-8. from it?

    And again, I challenge you to send most subspindle Y axis machines home when fully tooled up!

  20. #17
    Join Date
    Feb 2016
    Country
    UNITED STATES
    State/Province
    Massachusetts
    Posts
    7
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    0

    Default

    if you put X6. Z6. or whatever numbers work for clearance in program and say the cycle finishes and machine goes to those X6. Z6. numbers ,then machine indexes to next tool,how does machine know where it is for next tool without being at machine zero?
    thats my concern.

  21. #18
    Join Date
    Dec 2014
    Country
    CANADA
    State/Province
    British Columbia
    Posts
    1,228
    Post Thanks / Like
    Likes (Given)
    350
    Likes (Received)
    566

    Default

    Quote Originally Posted by Andrew65 View Post
    if you put X6. Z6. or whatever numbers work for clearance in program and say the cycle finishes and machine goes to those X6. Z6. numbers ,then machine indexes to next tool,how does machine know where it is for next tool without being at machine zero?
    thats my concern.
    This isn't some janky homemade 3d printer. The machine always knows it's absolute position from home unless it hits the limits and needs to be re-reference returned.

  22. #19
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,165
    Post Thanks / Like
    Likes (Given)
    1135
    Likes (Received)
    2280

    Default

    Quote Originally Posted by Andrew65 View Post
    if you put X6. Z6. or whatever numbers work for clearance in program and say the cycle finishes and machine goes to those X6. Z6. numbers ,then machine indexes to next tool,how does machine know where it is for next tool without being at machine zero?
    thats my concern.
    Fuckin' magic dude. First you need a chicken, and some candles. Some Human skulls and some incense (not incensed BTW). After you light the candles and arrange the skulls in 5 points about a Circle---you say woooo, woooo, woooo, weee, weee, weee I (insert foreign language insult here) booo, booo, booo, smeee, smeee, smeee. You have to do that 42 times in a row. Then you kill the chicken by about º350 in the oven, and eat it. (potatoes optional)

    After all that the Machine will know where it is, all the time.

    R

    You can also try; Zim Zala Bim Bombozala Dozala Dim---but I think their server is down, at least temporarily. I keep trying to use it on my wife, and she's still fat and ugly.

  23. Likes SeymourDumore, Vancbiker liked this post
  24. #20
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,557
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1396

    Default

    I'm with Seymour with regards to using G53. Even if the tools used from job to job are not changed, the coordinates used may have to be varied because of the different length of the work-piece, as the G53 coordinates are referenced from the Zero of the Machine Coordinate system, not the Work Zero.

    Quote Originally Posted by Hazzert View Post
    Lets start with what kind of lathe you're running.

    Are you talking about the Fanuc G28 U0.W0. ?

    Have you tried adjusting those numbers?
    Adjusting/varying these numbers will have Zero effect on where the X/Z axes finish at. It will be the Machine Reference Point irrespective of the values use in U and W (or X and Z).

    It's also common to just move the X axis to the Reference Return position for a safe tool change and always go to the Z coordinate with the next tool as the first move. For example (mm Mode example):

    G00 Z10.0
    G28 U0.0 M09
    M01
    (NEXT TOOL)
    G28 U0.0
    G50 T0200 S4000
    G97 S2652 M03
    G00 Z10.0 T0202 M08
    X30.0
    G96 S250
    --------
    --------
    --------
    --------
    G00 Z10.0
    G28 U0.0 M09
    M01
    (NEXT TOOL)

    Regards,

    Bill


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
  •