Lathe G76, how close can you get on Z to a wall?
Close
Login to Your Account
Page 1 of 2 12 LastLast
Results 1 to 20 of 28
  1. #1
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    2

    Default Lathe G76, how close can you get on Z to a wall?

    Trying to learn to thread on a CNC Lathe with a M70 controller, which is pretty similar to Fanuc as far as I understand. I'm trying to figure out how a G76 doesn't essentially smack into whatever is beyond the thread. An example part, 1" long, .5" diameter and on the front is a 4-40 thread that is .25" long. Just to make sure I'm getting the point down, the diameter could be 6", while the others are the same. I read that if the thread calls for .25" you could make it .249" and it would be less risky or something. I know that the tooth of the single point insert is not what the program would go by, but the face/front of the insert that it was taught off of.

    I was trying to talk to a co-worker and started 2nd guessing what I've found. If I remember right, the lathes I've watched thread take off at a 45deg angle in +X -Z (towards chuck) and then go back to Z0. Does this sound correct?

    Hopefully someone could break this down for me.
    Thanks,
    Higgins909

  2. #2
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,374
    Post Thanks / Like
    Likes (Given)
    1170
    Likes (Received)
    2400

    Default

    G76 allows the programmer to control the exit Angle. BUT I don't think that if it's programmed to Z-.25 it will go past that point. I could be wrong, I'm not a G76 expert.

    R

  3. #3
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,191
    Post Thanks / Like
    Likes (Given)
    4682
    Likes (Received)
    1619

    Default

    Like Rob mentioned the Z- is the final distance. I touch off the front of the insert then I typically thread up to a shoulder within .005" or .010" depending on the size of the thread. If it's just a straight shaft and the print calls for an 1" of full thread you need to thread a little passed to get your full distance of thread. Not too sure what you are asking.

    Brent

  4. Likes sinha liked this post
  5. #4
    Join Date
    Nov 2018
    Country
    UNITED STATES
    State/Province
    Texas
    Posts
    48
    Post Thanks / Like
    Likes (Given)
    4
    Likes (Received)
    2

    Default

    I'm trying to figure out if it would crash or not. Any example I can find, is a straight shaft that is having threads put on. I'm worried about sending the threader into the spindle jaws for this particular part that is threaded close to the jaws. In one of the videos I found, it looked like it was stopping at the end of the thread and maybe holding for a second? Then X+ and back to Z start.

  6. #5
    Join Date
    Nov 2013
    Country
    UNITED STATES
    State/Province
    Utah
    Posts
    4,374
    Post Thanks / Like
    Likes (Given)
    1170
    Likes (Received)
    2400

    Default

    Experiment with something, like plastic.

    R

  7. Likes Bluejeep, Dave K liked this post
  8. #6
    Join Date
    Jul 2013
    Location
    Indiana
    Posts
    3,191
    Post Thanks / Like
    Likes (Given)
    4682
    Likes (Received)
    1619

    Default

    Quote Originally Posted by Higgins909 View Post
    I'm trying to figure out if it would crash or not.
    Call up that tool (G0 T0101) and then hand wheel it to the absolute z coordinates in the program and see it it gonna hit. If you're gonna send it to Z-1. and the part ain't out that far you gotta problem. Don't just guess, check by moving the tool to where it's going to be before running it. This should give you confidence enough to run it.

    Maybe you should post a print so the group can see what the hell you're doing?

    Brent

  9. #7
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Quote Originally Posted by Higgins909 View Post
    I'm trying to figure out if it would crash or not. Any example I can find, is a straight shaft that is having threads put on. I'm worried about sending the threader into the spindle jaws for this particular part that is threaded close to the jaws. In one of the videos I found, it looked like it was stopping at the end of the thread and maybe holding for a second? Then X+ and back to Z start.
    Hello Higgins909,
    The Z address specified in the G76 cycle is the end of the Z travel in the Threading Cycle irrespective of the magnitude of any Exit Chamfer that may be specified in the Cycle. If you set the leading edge of the Threading Tool Holder/Threading Insert for the Z location of the Tool (Tool Coordinate System), as suggested by Brent, AKA yardbird, then you can specify a Z value that is very close indeed to the face of a shoulder, or obstacle.

    Regards,

    Bill
    Last edited by angelw; 09-14-2019 at 07:25 AM.

  10. #8
    Join Date
    May 2008
    Country
    SOUTH AFRICA
    Posts
    1,613
    Post Thanks / Like
    Likes (Given)
    1188
    Likes (Received)
    666

    Default

    So what I normally do is if the journal is 20mm long I program my G76 only 0.1mm short of that. I know I'm talking in mm but if you have a decent machine 0.1mm can be hit repeatably. I also do that so that the edge of the insert has no chance of bumping the shoulder.

    Also remember if you are using standard ISO ER/IR inserts that the tip is actually short of the edge of the insert, hence a lot of people under-cut if you need the thread to lock up on the face.

  11. #9
    Join Date
    Jan 2005
    Country
    CANADA
    State/Province
    Saskatchewan
    Posts
    10,193
    Post Thanks / Like
    Likes (Given)
    1383
    Likes (Received)
    3666

    Default

    Quote Originally Posted by angelw View Post
    Hello Higgins909,
    The Z address specified in the G76 cycle is the end of the Z travel in the Threading Cycle irrespective of the magnitude of any Exit Chamfer that may be specified in the Cycle. If you set the leading edge of the Threading Tool Holder/Threading Insert for the Z location of the Tool (Tool Coordinate System), as suggested by Brent, AKA yardbird, then you can specify a Z value that is very close indeed to the face of a shoulder, or odstical.

    Regards,

    Bill
    Damn it, Bill, you made me look up the word odstical, but I couldn't find a definition

  12. #10
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Quote Originally Posted by HuFlungDung View Post
    Damn it, Bill, you made me look up the word odstical, but I couldn't find a definition
    Hello HuFlungDung,
    Well there you go. Just another obstacle in the pathway of learning.

    Regards,

    Bill

  13. #11
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,414
    Post Thanks / Like
    Likes (Given)
    805
    Likes (Received)
    2374

    Default

    Quote Originally Posted by yardbird View Post
    .....I touch off the front of the insert.......
    Super important!

    I've had a few instances over the years where folks have claimed that there was an issue with the machine because it crashed or overcut/gouged a part after changing inserts or running a previously proven safe program. Always turned out that they had been in the habit of setting their Z offset to the center of the tip rather than the front most surface of the insert.

  14. Likes 706jim liked this post
  15. #12
    Join Date
    Jun 2006
    Location
    Thunder Bay Canada
    Posts
    1,801
    Post Thanks / Like
    Likes (Given)
    564
    Likes (Received)
    304

    Default

    Quote Originally Posted by Vancbiker View Post
    Super important!

    I've had a few instances over the years where folks have claimed that there was an issue with the machine because it crashed or overcut/gouged a part after changing inserts or running a previously proven safe program. Always turned out that they had been in the habit of setting their Z offset to the center of the tip rather than the front most surface of the insert.
    You beat me to it! Minimum Z is just that in a G76, but the 1/2 width of the insert has to be considerd if you set your offset to tool tip center.

    Like I do.....

  16. Likes Nerdlinger liked this post
  17. #13
    Join Date
    Jan 2014
    Country
    UNITED STATES
    State/Province
    Washington
    Posts
    4,414
    Post Thanks / Like
    Likes (Given)
    805
    Likes (Received)
    2374

    Default

    Quote Originally Posted by 706jim View Post
    .....but the 1/2 width of the insert has to be considerd if you set your offset to tool tip center.

    Like I do.....
    In some circumstances, that can be an acceptable method. I can see it in a one or two man operation where everyone involved is on the same page. Take that to a bigger picture when a lesser experienced operator has to swap to a different configuration of insert for some reason and doesn't consult someone that fully gets it. That's when things can go wrong.

  18. #14
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,241
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    223

    Default

    Quote Originally Posted by yardbird View Post
    I touch off the front of the insert then I typically thread up to a shoulder within .005" or .010" depending on the size of the thread.

    Brent
    Definitely a good and safe practice.

  19. #15
    Join Date
    Jun 2011
    Country
    UNITED STATES
    State/Province
    New Jersey
    Posts
    820
    Post Thanks / Like
    Likes (Given)
    491
    Likes (Received)
    318

    Default

    G76 can get within about .005" safely.

  20. Likes aj liked this post
  21. #16
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,502
    Post Thanks / Like
    Likes (Given)
    1217
    Likes (Received)
    1308

    Default

    Edit: just read more carefully and saw that you're not using a Fanuc control. What I wrote below is my experience with Fanuc controls.

    What I've found with G76 is that it will never exceed the programmed Z position, so you can safely go very close to the wall in program.

    However, it's not so great at actually cutting threads up to that point. No matter what parameters I program it always seems to retract out of the thread sooner than I'd like, compared to other (non Fanuc) lathes I've used.

    On parts with very shallow shoulders I've actually programmed Z beyond the shoulder on occasion in order to get the threads closer to the shoulder.

    Other times I've given in and used G32 instead.

  22. #17
    Join Date
    May 2006
    Location
    Burlington, North Carolina
    Posts
    379
    Post Thanks / Like
    Likes (Given)
    418
    Likes (Received)
    143

    Default

    Quote Originally Posted by gregormarwick View Post
    However, it's not so great at actually cutting threads up to that point. No matter what parameters I program it always seems to retract out of the thread sooner than I'd like, compared to other (non Fanuc) lathes I've used.

    On parts with very shallow shoulders I've actually programmed Z beyond the shoulder on occasion in order to get the threads closer to the shoulder
    In my humble experience I've found that slowing the spindle down a couple hundred RPM down gets me closer to the shoulder, at least on a Fanuc. I've coined the term "flinching", because the tool is headed toward a shoulder and acceleration/deceleration ramps pull the X-axis up sooner the faster the spindle is turning.

    ...just my nickel's worth.

  23. Likes Nerdlinger liked this post
  24. #18
    Join Date
    Feb 2007
    Location
    Aberdeen, UK
    Posts
    3,502
    Post Thanks / Like
    Likes (Given)
    1217
    Likes (Received)
    1308

    Default

    Quote Originally Posted by aj View Post
    In my humble experience I've found that slowing the spindle down a couple hundred RPM down gets me closer to the shoulder, at least on a Fanuc. I've coined the term "flinching", because the tool is headed toward a shoulder and acceleration/deceleration ramps pull the X-axis up sooner the faster the spindle is turning.

    ...just my nickel's worth.
    That's what I thought too, but I have Fanuc lathes over a pretty big range of size, speed and acceleration rates, and they all do this with G76, but not if I use G32. I can program a ramp out move in G32 and still get way closer to the shoulder than G76 will do, so it's not an axis acceleration thing, unless there are separate acceleration parameters specific to G76 (not all that unlikely, knowing fanuc).

  25. #19
    Join Date
    Sep 2010
    Location
    Victoria Australia
    Posts
    3,655
    Post Thanks / Like
    Likes (Given)
    0
    Likes (Received)
    1438

    Default

    Quote Originally Posted by gregormarwick View Post
    That's what I thought too, but I have Fanuc lathes over a pretty big range of size, speed and acceleration rates, and they all do this with G76, but not if I use G32. I can program a ramp out move in G32 and still get way closer to the shoulder than G76 will do, so it's not an axis acceleration thing, unless there are separate acceleration parameters specific to G76 (not all that unlikely, knowing fanuc).
    Hello Gregor,
    This is because G32 can be used for Continuous Threading, where the Lead and Shape of the Thread may change at various points. The system is controlled in such a manner that the synchronization with the spindle does not deviate in the joint between G32 blocks. Accordingly, programming a ramp out with G32 is seen as a change of Thread Shape at the joint between the two G32 Blocks.

    Regards,

    Bill

  26. #20
    Join Date
    Sep 2010
    Location
    india
    Posts
    1,241
    Post Thanks / Like
    Likes (Given)
    72
    Likes (Received)
    223

    Default

    Quote Originally Posted by aj View Post
    ... acceleration/deceleration ramps pull the X-axis up sooner the faster the spindle is turning...
    According to Fanuc manual, the retraction distance is not dependent on rpm.


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
  •