Results 1 to 6 of 6
  1. #1
    HelpImLost is offline Plastic
    Join Date
    May 2013
    Location
    MN,USA
    Posts
    41

    Default thread programming on lathe

    I was looking through a tooling catalog for threading tools. In the catalog they said something about the canned threading cycles on a lathe doesnt make real good threads sometimes because of the depth of cut isn't deep enough or something. It said that it is better to write a custom program for threading? Now im new to this stuff so I do not know what they are talking about. Anyone know what they are talking about and if you do can you give me an example of a custom threading program. Thanks again.

  2. #2
    bjorn toulouse's Avatar
    bjorn toulouse is offline Titanium
    Join Date
    Dec 2007
    Location
    N.E. oHIo, USA
    Posts
    2,064

    Default

    Explore the Haas programming manual, paying attention to the G76 and G92 cycles.
    Both are threading cycles that will likely work well for you.


    Rex

  3. #3
    modelmakerblue is offline Plastic
    Join Date
    Sep 2005
    Location
    Dunstable, UK
    Posts
    23

    Default

    Quote Originally Posted by HelpImLost View Post
    I was looking through a tooling catalog for threading tools. In the catalog they said something about the canned threading cycles on a lathe doesnt make real good threads sometimes because of the depth of cut isn't deep enough or something. It said that it is better to write a custom program for threading? Now im new to this stuff so I do not know what they are talking about. Anyone know what they are talking about and if you do can you give me an example of a custom threading program. Thanks again.
    From personal experience on a Haas CNC lathe there is nothing wrong with the threading cycles. As in all machining you may have to make minor adjustments to hit size.
    Tony

  4. #4
    IronReb is offline Stainless
    Join Date
    May 2011
    Location
    Shreveport/Louisiana USA
    Posts
    1,073

    Default

    G92 will give you custom threading.
    example...2''-12 thread...numbers may not be accurate but it's just for show.

    G92 X1.980 Z-3.00 F.0833 DEPTH OF FIRST CUT CAN BE AS HEAVY OR LIGHT AS YOU NEED
    \X1.960 CAN MAKE CUT DEPTH WHAT EVER I WANT IN EACH X MOVE...THE \ IS THERE FOR THE FIRST PASSES TO ALLOW ME TO SKIP THEM IF I RERUN PART TO HIT SIZE,NOT NEEDED BUT HELPS ON DEEP THREADS
    \X1.950
    \X1.940
    \X1.930
    X1.920
    X1.910
    X1.9
    X1.895 be careful on taking light cuts in a thread.sometimes you need a couple light passes for spring back.Other times it will cause chatter or shitty thread..you just have to give it a go and adjust from there.
    X1.892
    G00 X10. Z.03
    M30


    G76 can be custom to an extent.In the settings there are factors you can change to control how much it leaves for last pass and a few others,sorry I forget now because I have mine set and never muck with it much.
    G76 is like using the compound and slide to move the tool in at an angle and only cut on one side.G92 just goes straight in and cuts on both sides of tool.

    G76 A59 K.054 D.02 X1.892 Z-2. F.0833 that's it,same thread as above just less punching of the buttons.On HAAS control every thing is needed in this sample to cut.The settings in the control cover all the other stuff.

    A59 this is the angle of the thread.It is not 60 degree so it gives you just a lil clearance on the tool as it works its way down the profile of the thread
    K value is simple take depth of thread and devide by two,if book says thread total depth is .100 I add a few then devide that number
    X is the major thread diameter minus total thread depth
    D is what it will take on first pass...try to take a decent size cut here
    Z of course is how long the thread is
    F 1 / number of threads 12threads = 1 / 12=.0833" for F

    The way I do it may not be up to par with those that have much more knowledge than I do but it works and we make money and customers are happy.

  5. #5
    cajunthreads is offline Plastic
    Join Date
    Mar 2013
    Location
    Louisiana USA
    Posts
    3

    Default thread programming on lathe

    I use canned threading cycles all day long with no issues. On my Hass "ST" series lathes you can go into your setting and change depth of cut per threading pass if need be. This has worked very well for me when I clip Acme and Stub Acme threads by putting grooving insert and running threading canned cycle .010-.015" doc instead of .003-.005" doc

  6. #6
    gorrilla is offline Stainless
    Join Date
    May 2007
    Location
    Central Texas, West and North of Austin
    Posts
    1,191

    Default

    Quote Originally Posted by HelpImLost View Post
    I was looking through a tooling catalog for threading tools. In the catalog they said something about the canned threading cycles on a lathe doesnt make real good threads sometimes because of the depth of cut isn't deep enough or something. It said that it is better to write a custom program for threading? Now im new to this stuff so I do not know what they are talking about. Anyone know what they are talking about and if you do can you give me an example of a custom threading program. Thanks again.
    Most canned thread cycles will have a place to adjust the depth of cut, how much is cut on the last pass, and you can adjust the depth of the first pass either in the depth of cut or at the starting point. As to whether it cuts straight in, cuts down the angle on one side, of alternates on side , then the other, is a matter of either a parameter, or a G code in your program, at least the Okumas do, and I think the Fanucs as well. How all this works is dependent on the control you are using, and should be explained in your programming book, assuming you can make sense of THAT. It isn't usually very clear , or at least that has been my experience with programming manuals. But this should give you a place to start. As for the tool catalog saying that threading cycles don't give you good threads, if you master the different variables needed for the canned cycles, they are capable of doing as good as the "custom" type programming of the G92 type stuff, in all but a few of the most obtuse cases. IMHO.
    The vast majority of threads cut on CNC equipment, and that's the vast majority of threads cut at all these days, comes off of canned thread cycles. I can't feature where a tool catalog would get off telling you right off the bat that canned cycles won't make a decent 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
  •