Threading Question

Do any of you gentlemen know a good source to explain the method of cutting multiple lead threads? I will be using an older LeBlond lathe with a 72 inch bed.

"Screwcutting in the Lathe" by Martin Cleeve.

http://www.lathes.co.uk/books.htm

Also seen on Ebay.

Regards.

Finegrain

source

Yes, me.

I’ll assume you are referring to a double lead thread as the methods for a triple and a quad are a little different.

I know of three ways, and which one you use depends on the number of threads you are cutting. Lathe type, size, etc. do not matter.

Method one

Set the compound parallel to the axis of the lathe. Set up your threading tool as usual, but instead of using cutting on the slant depth with the compound rest, you will need to use the cross slide and cut the straight depth. You will also need to set the gear box at half the number of threads.

Cut the first lead to depth.

Calculate the pitch of the thread and divide by two. Advance the compound that distance, and begin cutting the second lead starting of course at zero on the cross slide.

For example if one were cutting 20 TPI double lead you would set the gear box for 10 TPI and the distance one would move the compound for the 2nd lead is .025”

Method two

This method can be used when the TPI divided by two equals an odd number.

Set the lathe up as usual, using the compound to cut the slant depth. Like the above method set the gear box at half the number of threads. Cut one lead using the numbered lines on the half-nut dial and the other lead using the un-numbered lines.

For example for 10 TPI set the gear box for 5 TPI. Run one lead on the numbered lines and the other lead on the un-numbered lines.

Method three

If the piece can be run between centers, cut a 60 degree center in your 4 jaw chuck. You can then index the part using the chuck jaws and get double, and also quad lead threads. To do a triple lead use your 3 jaw chuck.

Stan

That was also assuming you are cutting external threads. Method One will also work for internals.

Are you using a manual lathe or NC?
If you are using a NC, you need to program twice the lead for each start. The second start would the one lead Z+ from the first start.
Your CAM system should handle all this.

Thanks, Dr Stan! Very good info. I'm cutting a five lead screw with 10 TPI. If I follow your description, cut the first lead at 2 TPI and advance the cutter for the second cut 0.02" and so on until the project is complete.

Glad to help. Now you've got my interest. A five lead! What in the world is it used on? Even the quick acting valves I repaired in the Navy only used a double lead. If I remember correctly a 10 TPI double lead was the usual.

If you are going to attempt to thread a 5-lead screw, you'd better figure out your thread helix angle and grind your tools with the special clearances to match/compensate for it, otherwise you are going to be trying to RUB the stock off instead of cutting it.

WOW! a 5 lead thread. That I'd like to see. How big is this threaded shaft? Please a picture
when done.
...lew...edit: as eKretz says that is going to be some tool shape too.

That will trasmit a fair bit of motion for sure. I make that as a half inch for each turn.

Stephen

Oh, and btw Handlebar...you want to cut your first thread at 2 TPI, then advance your tool .100" for the next pass, and so on. Not sure where the .02" came from?

P.S. well written guidelines Doc. Covered nearly every approach there. Another couple methods are to use an indexing head mounted in the lathe chuck to grip the part, another is to mill a hex or square or three- or two-flat, etc. depending on how many leads you need on the end of the part and chuck using a 3-jaw or 4-jaw, etc. indexing the grip of the jaws on the part as necessary, another is to mark the gears in the drivetrain from the chuck to the leadscrew if they have the proper number of teeth and disengage and re-engage them. There are many many ways to do this.

The correct terminology for this type of thread is 'multiple start', not multiple lead, as the lead of a thread is best described as how far a nut would travel on a threaded shaft in one revolution, in this case 5 times the pitch.

Luthor you're technically correct. It’s an example of the difference between trade lingo & the technically correct term.

I also 2nd the recommendation about the extra side clearance angle. That will be a very high helix angle.

Handlebar57:

Even if you were to set this job on a Hendey lathe, which is designed to cut multi-
start threads, indexing would be the main problem. Whenever you are cutting a thread
that is a prime number multi-start gteater than 3, I would suggest that you consider
using a double disc backing plate for the chuck indexing. I have used this simple yet
flexible method for many years to cut multi-start prime number threads in the lathe and
shaper. This method works well for cutting long leads on a planer.

I have found it easier to cut all multi-start threads to the same depth at the same
time, then reset the compound for a deeper cut and repeat the process. If any mistakes
occur during cutting because of a wrong setting or tool wear, it is usually distributed
among the threads. If you get interupted during the cutting process and have to stop
for any reason, this makes it easier to remember what you were doing.

If you are only making a few of these screws, then cutting them in the lathe is the
easiest way to get the job done. If you plan to make a large number of these, you might
want to consider setting this job on a shaper. Once you have made a few simple fixtures
the job can be run fairly fast. This method has been used to produce 6 start threads
and nuts, the bolt diameter was 9/16 of an inch, the thread was 2 to 3 inches in length
and the pitch was 2 inches. Just something to consider.

Hendeyman

All good advice from everyone! Dr Stan...it is a 1" diameter 5 helix screw that is used to move a hold down for a CNC vinyl cutter in our factory. The screw is turned by hand and has to move relatively long distances when it is time for a new pattern is to be cut. I assume it was made this way so the operator wouldn't have to stop and rest before he got to the destination point. A co-worker tried to make a replacement that was 1" x 10TPI since it appeared to be just that at first glance. Of course, it didn't work. When I took a look at the cross section of the broken piece I immediately saw the problem/solution. I couldn't believe my own eyes at first, but there it was.

Make sure your lathe is strong enough to be able to cut such a coarse thread, it puts a considerable force on changewheels and leadscrew using old machines.
MBB

Handlebar57,

You mentioned long. One of the things we did when cutting long valve stems was to use a follower rest, other wise you'll get spring in the middle of the screw from tool pressure.

Given you are cutting a thread with 5 leads, you may want to consider mounting an index head in the lathe. That might be a better way to keep track of your passes.

I have purchased Acme threaded rod from a company that is located in Minnesota. Unfortunately, I cannot remember the name nor was I able to locate it on the Net. Might be worth your time if you can find someone who rolls the thread as a rolled thread is much stronger than a cut thread.

Just out of curiosity. What is the thread form?

Stan

hendeyman said:

Handlebar57:

.... to cut multi-start prime number threads in the lathe and
shaper. This method works well for cutting long leads on a planer.

..... If you plan to make a large number of these, you might want to consider setting this job on a shaper. Once you have made a few simple fixtures
the job can be run fairly fast. ....

Hendeyman

Click to expand...

Shaper? Planer? This is new on me, can you please explain?

Troup:

To answer your question, let's start by comparing cutting a long lead on a milling
machine versus a planer. Suppose you want to cut a thread with a six foot lead on
a milling machine equipped with a long lead attachment, the limiting factor will be the
length of table travel. On a #3 or #4 miller, this will be limited to 34 inches or 42 inches.
To cut the full length thread, the job will have to be reset. There is also the problem
of supporting the outboard end of the shaft. So far we are only talking about cutting
a single start thread. For multi-start threads you will still need some form of independent
indexing in addition to the long lead attachment. The simplicity of the double disc mount
ing plate for either the chuck or a drive plate can be used on a lathe, miller, shaper or
planer.

If a planer with a stroke length equal to/or greater than the length of the lead is
available, then the job can easily be done on the planer. When a number of long leads
are to be cut, a special drive unit can be built that is usually powered by a rack mounted
along side the planer bed. When you are dealing with a one-off, an ordinary dividing
head off the miller will work just fine. The dividing head is set at the end of the platen
and usually off set from the centerline by one tee slot, this allows for mounting the
drive system. With the rack drive system, a series of gears is used to connect the rack
with the dividing head. With the one-off method a wire rope is used to supply the drive.
An upright anchor post, mount at the end of the planer bed, is connected to one end
of the wire rope, which is usually about 1/8 to 3/16 inch in diameter. The other end of
the wire rope is wound around a drum that has a partition in the middle of its length.
The drive rope is wound on one side of the partition and a counterweight rope is wound
on the other side, but in the opposite direction. With this arrangement, one rope is
unwinding while the other rope is winding, maintaining a constant pressure on the drum.
The drum shaft, which is independently supported by its own bearings, is connected to
the index plate shaft via a coupling. If necessary, a gear on the drum shaft can be
connected to a gear mounted on the index plate shaft, when this arrangement, an outboard bearing is used to support the gear on the index plate shaft. By choosing the
correct drum diameter and gear ratio, the dividing head will rotate one turn when the
platen has travelled the length of the lead. Once you have the various bits and pieces
made up, the job can usually be setup in about an hour.

With the set up checked to make sure you are getting a complete rotation, the cut
is started about two or three inches from the end of the shaft to allow for the removal
of all slop. After each pass, the tool is fed in deeper until the proper depth is reached.
On a multi-start thread, you can either cut each thread full depth and then index or
cut and index all threads before changing the depth for the next cut, thereby spreading
any errors among all the threads. While this set up and procedure may sound com-
plicated, it is really very simply and produces very good results. One more thing, I
arrange for the tool to be lifted on the return stroke just in case something goes out of
synch, I don't want to tear up a thread or break a tool.

If I get a chance later today, I will post the set-up for screw cutting in a shaper.

Hendeyman

Do, please. That would be interesting to see! I haven't got to run a planer in a good 8 years, and sorely miss it.