What's new
What's new

Multi start thread?

TimH

Hot Rolled
Joined
Oct 12, 2004
Location
Upstate NY
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
 
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
 
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.
 
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.
 
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 :D
 
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?
 
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.
 
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.......:codger:
 
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
 
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
 
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
 
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/images/smilies/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
 
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?
 
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
 
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.
 








 
Back
Top