Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

  • Congratulations pierreick on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

Con rod threads for cap screws. 1

Status
Not open for further replies.

Tmoose

Mechanical
Apr 12, 2003
5,628
On another thread it was proposed that threaded holes with long engagement lengths are often thread milled with a progressive pitch. When a bolt with a constant thread pitch is installed it creates a more even stress distribution among the engaged threads.

I was thinking the variation in pitch on a 3/8"-24 bolt could only be on the order a thousandth of an inch ( 0.001" ) over 3/4 inch engagement lest the threads that touch first be severely strained by the time the first threads take up load.

Is anyone familiar with that technique.

 
Replies continue below

Recommended for you

I am slightly familiar with thread milling.

It's normally done with a cutter that looks like a tap with one flute but multiple teeth, and completes a nominal threaded length roughly equal to the toothed length of the cutter, in one helical trip around and along one pitch of the finished thread path, with the spindle turning very fast.

You could do a threaded hole with progressive pitch, but you'd need to use a cutter with just one tooth, and you'd lose the speed advantage of thread milling by having to move that cutter along the complete helix of the generated thread, not just one turn of the helix. I haven't heard of anyone doing it that way, but it's not impossible.




Mike Halloran
Pembroke Pines, FL, USA
 
I guess there are two choices - close-fitting threads resulting in pre-stressing of the same magnitude as the required offset - or loose thread fit with a progressive clearance as you move axially along the bolt. . . . . or a combination of the two.

je suis charlie
 
There was at least a third method attempted back in the 1960s. Pretty successfully, too.
They don't pull LeMans winners' names out of a hat.

I can attest those tri-lobed bolts had a LOT of prevailing torque.
It was not uncommon for folks to switch to a socket head cap ("Allen") screw.
If that was to be attempted today I'd want the solid shank length to closely match the stock bolt.
 
 http://files.engineering.com/getfile.aspx?folder=88c39615-3643-4dd2-9a2b-d96a315311f9&file=LeMans_427_bolt_design.jpg
Thanks to the availability of CNC milling machines with excellent precision and sophisticated CAM software tools, it is common practice to mill internal threads. Especially when the hole is blind and there is minimal length for incomplete threads at the hole bottom. Thread milling can also produce a more accurate positional location of the threads than tapping.

Here is a link to a short article that describes the fatigue benefits of "over-pitching" internal threads.

URL]
 
You do not need cam software to program thread milling. Its really very simple to program at the machine.
 
Thread milling in high volume engine manufacture is not viable from a cycle time standpoint. I can see it's use in racing or aerospace, but when the plant engineers are looking for 0.10s of a second in time on each engine, I don't it being feasible.
 
Thread milling with constant pitch using the usual sawtooth cutter should be much faster than tapping, because the head makes only one full orbit and two smaller half orbits, and advances and retracts down the hole center at top speed, while the spindle turns at a high speed optimized for metal removal.

Thread milling with progressive pitch, using a single point tool as in the sectioned illustration provided by tbuelna, should still be a little faster than tapping, as the head orbits helically down the hole while making the thread, then half-orbits to a centered position and withdraws fast, again with the spindle turning fast all the time.

Tapping still makes sense where you have to produce the exact same array of tapped holes forever, like the 4/5/6 holes around a cylinder bore, or the 20-ish holes around an oil pan, and can afford to maintain a multi-spindle tapping head, and have already bought the tooling.

If you were starting fresh from scratch, you might decide differently.



Mike Halloran
Pembroke Pines, FL, USA
 
I have no experience with production threaded hole creation, but some would say tapping is generally a faster per hole process.

"The greatest advantage of tapping is speed. High-speed tapping centers set up with a rigid tap can thread holes in a fraction of the time it would take to thread mill the same holes."

Tapping can be quite a bit faster than thread milling, particular on a machine set up for rigid tapping.
 
The single point thread mill I posted the picture of would only normally be used to produce internal threads with variable pitch or diameter. Using a conventional tap to produce constant pitch internal threads, in through holes or blind holes with adequate depth for incomplete thread runout, is likely the most efficient machining method for most common thread sizes. Multi-point thread mills are a better choice for large diameter constant pitch internal threads, cutting internal threads in materials that are hard or difficult to machine, or cutting internal threads that have limited bottom clearance.

Obviously, a conventional tap or multi-point thread mill would not work for machining variable pitch threads.

Here is a paper describing the Spiralock threadform. It uses a constant pitch internal thread with a unique cross section to achieve a more even distribution of preload between the engaged threads.
 
Status
Not open for further replies.

Part and Inventory Search

Sponsor