Page 1 of 2 12 LastLast
Results 1 to 20 of 25
  1. #1
    TimH is offline Hot Rolled
    Join Date
    Oct 2004
    Location
    Upstate NY
    Posts
    681

    Default Multi start thread?

    Quite a few years ago I cut quite a few 3 start threads for a project. I was thinking about using a 3 start thread on a project I'm working on now. For the life of me I can't remember how to cut one. Does anyone have experience cutting these? Thanks Tim

  2. #2
    johnoder's Avatar
    johnoder is offline Diamond
    Join Date
    Jul 2004
    Location
    Houston, TX USA
    Posts
    21,935

    Default

    Set the right lead and index the part in relation to the chuck. I.E., a 3 start thread that looks like a 9 pitch will have a lead of a 3 pitch.

    John Oder

  3. #3
    PixMan's Avatar
    PixMan is offline Diamond
    Join Date
    Jan 2007
    Location
    Central MA USA
    Posts
    4,647

    Default

    Indexing the part in the chuck is very hard to repeat or get accuracy. Are you on a manual or CNC lathe?

    Manual lathe, turn the compound to parallel with the long (z axis) travel and simply move the tool over by 1/3rd if the pitch for the 2nd start, another increment for the 3rd start. On a CNC, just move the start point in Z for the thread cycle by those same amounts.

  4. #4
    RC99's Avatar
    RC99 is offline Titanium
    Join Date
    Mar 2005
    Location
    near Rockhampton, Queensland, Australia
    Posts
    3,900

    Default

    Quote Originally Posted by PixMan View Post
    Indexing the part in the chuck is very hard to repeat or get accuracy.
    You index by using the first driving gear on the gear train between the headstock and the QCGB. The gear has to be divisible by the number of starts..

  5. #5
    toastydeath is offline Hot Rolled
    Join Date
    Jan 2007
    Location
    Newark, DE
    Posts
    722

    Default

    Quote Originally Posted by PixMan View Post
    Manual lathe, turn the compound to parallel with the long (z axis) travel and simply move the tool over by 1/3rd if the pitch for the 2nd start, another increment for the 3rd start. On a CNC, just move the start point in Z for the thread cycle by those same amounts.
    This.

    Or if this isn't acceptable, drill a bolt circle with 120 degree spacing in a faceplace and use a lathe dog to drive the part. Index by changing the hole. I would do the former with smaller threads, but I'd go through the trouble of the latter if I expected trouble with plunge feeding on a larger thread.

    Never heard of the gear method. I will keep that in the back of my head and try it someday.

  6. #6
    Limy Sami is offline Diamond
    Join Date
    Jan 2007
    Location
    Norfolk, UK
    Posts
    11,958

    Default

    Quote Originally Posted by toastydeath View Post
    This.

    Or if this isn't acceptable, drill a bolt circle with 120 degree spacing in a faceplace and use a lathe dog to drive the part. .
    ... And put a little flat on the part for the drive dog screw to bite on - it'll stop any chance of slipping ......... don't ask me how I know

  7. #7
    TimH is offline Hot Rolled
    Join Date
    Oct 2004
    Location
    Upstate NY
    Posts
    681

    Default

    Quote Originally Posted by johnoder View Post
    Set the right lead and index the part in relation to the chuck. I.E., a 3 start thread that looks like a 9 pitch will have a lead of a 3 pitch.

    John Oder

    Ok for example, I set the machine to cut a 3 pitch then move the start point in z 1/3 of the pitch then cut again and repeat? What depth do I use, For three pitch or 9 pitch?

  8. #8
    PixMan's Avatar
    PixMan is offline Diamond
    Join Date
    Jan 2007
    Location
    Central MA USA
    Posts
    4,647

    Default

    You need to use the depth of a 9 pitch. Are you using a manual or a CNC lathe?

    Also, don't overlook the lead angle clearance on the cutting tool. If using a threading insert for instance, you need to grind more clearance or use a shim seat with more angle.

  9. #9
    Boris is offline Titanium
    Join Date
    Oct 2005
    Location
    England
    Posts
    3,019

    Default

    Quote Originally Posted by toastydeath View Post
    This.


    Never heard of the gear method. I will keep that in the back of my head and try it someday.

    Thats the method I was taught for doing multistart threads on the hand cranked lathe

    After a fair number of struggles and wrecked threads, my fellow tadpoles and me were shown the "multiply the leadscrew by the number of starts and offset using the compound slide for each start" method as its far easier

    Boris

    "aye... when I were a lad all we had was hand cranked machines.......

  10. #10
    stannp368 is offline Hot Rolled
    Join Date
    Jan 2003
    Location
    Philadelphia, PA USA
    Posts
    617

    Default Multi start thread

    I assume you are on an engine lathe. One way is to hold work w/ a dog between centers using a 3 jaw chuck w/ a straight shank center clamped in. Make sure you provide a flat where the dog clamp screw tightens against your work. Proceed as if cutting a single thd of req lead until thd is 1/3 the depth, then rotate the work so the dog is driven by the next jaw on the 3 jaw chuck. Repeat this to the 3rd jaw & you are downtown. Example-5 tpi triple thd. Set lathe to cut 5 tpi. Lead =1/5=3/15. Pitch=1/15. Depth=.65/n=.65/15. You will end up w/ 15 tpi but w/ a lead of 5 tpi. What you did was to cut 5 tpi 3 times. I hope this helps you

  11. #11
    Mcgyver is offline Titanium
    Join Date
    Aug 2005
    Location
    Toronto
    Posts
    2,439

    Default

    as Pix says, watch the clearance angles....3x is a big increase in the helix angle....somewhere online there is a calculator for that or you can do it manually without too much trouble

  12. #12
    Billtodd's Avatar
    Billtodd is offline Stainless
    Join Date
    Feb 2009
    Location
    Colchester UK (where the lathes used to be made)
    Posts
    1,352

    Default

    Popular Mechanics 1947 "how to cut multiple threads"

    http://books.google.com/books?id=z94...s_pt=MAGAZINES

    Some useful tips here

  13. #13
    TimH is offline Hot Rolled
    Join Date
    Oct 2004
    Location
    Upstate NY
    Posts
    681

    Default

    Thanks everyone. I had a successful day. All your help is appreciated. BTW it wan ona CNC lathe. As mentioned earlier, I have done these before maybe 12 years ago. I just couldn't remember :-) Its tough to get old

  14. #14
    blackboat's Avatar
    blackboat is offline Hot Rolled
    Join Date
    Nov 2001
    Location
    Conyers, GA
    Posts
    998

    Default

    Just release the Multi Start handle on the lathe, rotate chuck over to next correct number, re-lock handle. Pretty easy.... http://www.practicalmachinist.com/vb...es/biggrin.gif


    (Just been playing with a little Hendey that does this, thought it a nice feature.)

    On a more typical lathe, I've done the dog & chuck dividing system as the one that licked easiest with my brain. Also, smallish faceplate with holes for the dog I remember seeing somewhere; just have to have a way of dividing it into the appropriate holes/dog locators and have a set piece ready to go whenever the need arises.

    Rob

  15. #15
    locoguy is online now Hot Rolled
    Join Date
    Oct 2004
    Location
    SE Ohio
    Posts
    848

    Default

    Question about stann368 example of 5tpi, triple start: would not the correct QC setting be 1 2/3 threads per inch (5/3)?

    Cannot say that I have ever needed to machine a multiple thread. My jobs must all be of the Velveta variety.

    Once read an article on a huge width adjustment screw for a plate rolling mill for the steel industry around Gary or Chicago, that reminded one of the toe-clamp screws on the old-style roller skates: left on one end and right on the other. The finished screw was a hefty five or six tons, three or four square threads per FOOT, triple lead. Took months to manufacture on a lathe made just for this job.. Maybe another PM contributor has seen the same re-print article and can lead us to a link for all to enjoy, out of American Machinist?

  16. #16
    dp
    dp is offline Banned
    Join Date
    Aug 2005
    Location
    Puget Sound, Washington
    Posts
    3,204

    Default

    I might be tempted to use one of these hex collet holders:

    http://www.fastenal.com/web/products...v0?sku=0344213

    Set up a stop for the depth for repeatability.

  17. #17
    stannp368 is offline Hot Rolled
    Join Date
    Jan 2003
    Location
    Philadelphia, PA USA
    Posts
    617

    Default

    Absolutely not, then your lathe will give you the lead for 1.2/3 tpi when you want a lead for 5 tpi

  18. #18
    willbird is offline Banned
    Join Date
    Jul 2005
    Location
    North(very) West(very) Ohio...near exit 13 on OH turnpike
    Posts
    3,714

    Default

    The biggest PITA about the whole deal is that you will have a tough time making all starts the exact same PD, it is much tougher to go back and take a spring pass on each thread. The multi leads you can make by engaging the half nuts in the proper place will for that reason come out a lot nicer for the amount of work involved.

    Bill

  19. #19
    juergenwt is online now Hot Rolled
    Join Date
    Feb 2008
    Location
    Wheaton, IL.
    Posts
    857

    Default

    When designing parts with multiple thread starts pls. be reminded of the limitations of multiple start threads. If your part is used to exert clamping pressure a screw with 4tpi and three starts will look like a screw with 12tpi but depending on the dia will have very little clamping power because of the steep helix angle. It may actually come loose. You may be deceived by the looks of the thread.

  20. #20
    willbird is offline Banned
    Join Date
    Jul 2005
    Location
    North(very) West(very) Ohio...near exit 13 on OH turnpike
    Posts
    3,714

    Default

    One job long ago we made a lot of 3/4-5 two lead threads, they were for hospital beds.

    Bill

Page 1 of 2 12 LastLast

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
  •