Three Form Thread Mill ???

Below are CNC applications:

I use machine taps in tension compression holders. Functionally like rigid tapping, but with some fudge factor for machines that do not have a C-axis. Typically I run this at 500RPM, and switch to low gear in anything harder than aluminum. I have used these on blind holes, but only if I can substantially over drill the depth. If you bottom or chip pack the hole out it will break. Works best for through holes with spiral point taps.

I use single form thread mills on the high spindle speed machines. I cut from the bottom up tracing the full thread. Blind holes. Through holes. Doesn't matter. If you start at the bottom all the chips are below your cutter.

I use full form thread mills on the slower spindle speed machines. I start at the bottom and turn 1.5 to 2 thread rotations and done. Doesn't leave the chips behind as well as the single form does, but since its only making 2 interpolations at any depth (upto its flute length) chips are not a problem. I start at the bottom anyway. Works fine in blind holes or through holes.

What exactly is the advantage of a three form thread mill?

For clarity the form is the number of teeth in a single flute. There may be multiple flutes in single form, full form, and three form thread mills.

Single form can be made in house on a tool D-bit grinder with just one "flute" with one tooth. I buy multiple flute single form thread mills from Carbide Tool Source (Rogue Systems Inc) and I usually buy full form thread mills from Lake Shore Carbide. If I find a reason to try three form thread mills I'll probably start with some "cheap" Chinese imports off Ebay to see if the concept works for me or not.

Reply to
Bob La Londe
Loading thread data ...
<snip>

Seeing you didn't get much help with this... I asked "ChatGPT" a couple questions while fooling around with it. Here is the response:

=== Me> Any insight on Three Form Thread Mill compared to single form?

A three form thread mill is a type of tool used in machining to create internal threads, or threads on the inside of a hole. It is called a "three form" thread mill because it has three different profiles on the cutting end of the tool: one for the root of the thread, one for the crest, and one for the root radius. This allows the tool to create a complete thread in a single pass.

In comparison, a single form thread mill only has a single profile on the cutting end, so it can only produce a partial thread in a single pass. This means that it takes multiple passes to create a complete thread, which can be slower and less efficient than using a three form thread mill.

There are trade-offs to consider when deciding which type of thread mill to use. Three form thread mills can be more expensive and may require more precise setup and alignment, but they can be more efficient and produce a higher quality thread. Single form thread mills are generally simpler and less expensive, but they may require more time and effort to create a complete thread.

Me> Any difference using climb cutting for a thread mill?

Climb cutting is a machining technique in which the direction of the cut is opposite to the direction of the tool's rotation. This can have a number of benefits, including a smoother finish on the workpiece, reduced cutting forces, and longer tool life.

When using a thread mill to create internal threads, climb cutting can be particularly useful because it allows the tool to enter and exit the cut more smoothly. This can help to reduce the risk of tearing or chipping on the entry and exit of the cut, which can be a problem when using a traditional threading tool such as a tap.

However, it is important to note that climb cutting with a thread mill can also be more challenging and may require more skill and experience to execute properly. The cutting forces can be higher when climb cutting, so it is important to use appropriate tool holding and workholding methods to ensure that the tool does not deflect or chatter. It may also be necessary to use a slower feed rate and/or a lighter depth of cut to ensure that the tool does not become overloaded or break. ===

I don't have a mill... hadn't heard of "Three Form" before so I was a bit curious myself ;-)

Reply to
Leon Fisk

That's funny. I just watched a video this morning about one of those Chat-AI programs and the lemon law in Michigan. Of course by a Michigan lemon law attorney. I have to say, I have as much issue with this response as he did with the Michigan lemon law response. LOL.

Some of it may be choice of definitions, but either way some of it is just not right. I make complete threads that the target machine screw will thread into with a single form thread mill in just ONE (1) pass.

One can assume with some reasonable degree of certainty that if one is thread milling (which is done by spiral interpolation) that the machine has relatively low backlash or is very heavy and climb milling is not even something one worries about. Therefore in respect to thread milling the primary relationship to climb milling is that it allows you to cut the threads from the bottom of the hole to the top avoiding any chance of chip re-cutting when cutting standard right hand threads. Even with blind holes.

As to the definition of the three form thread mills that sounds mostly like guessing. The ones I have seen just appear to have three teeth the same in each flute. This is why I can't see any benefit. At the start all three teeth cut, but than after the first interpolation only the lead tooth would be cutting. Even if a second or third pass or spring pass was required in hard material I don't see how those other same teeth would be any help. The first one does all the work.

Video single form thread milling I do everyday. 10-32 thread 0.495" deep. That particular thread mill has done hundreds if not thousands of holes.

formatting link

Reply to
Bob La Londe

One of those three form thread mills

formatting link

Reply to
Bob La Londe

[Then chatGPT says:]

Bob's already skepticized about that claim, and in web searches I didn't find any support for it. I've seen several three form thread mills where all the teeth look like the same profile, but didn't find a spec sheet or drawing that spelled it out..

Some reasons for using a multi-form (including three-form) thread mill are "They can thread faster because they cut multiple grooves in one pass" [ref 1]; they "excel in internal deep threads and hard-to-cut materials" [ref 2]; they "are designed for threading in hardened steels and difficult-to-machine materials" [ref 3].

Makes it look like production, tool life, and special cases are what make multi-form thread mills desirable.

On the con side: Unlike a single-form thread mill they cut only one pitch. Side loading and horsepower requirement are higher than for single-form.

[1]
formatting link
[2]
formatting link
[3]
formatting link
[Then chatGPT says:]

Isn't that backwards? Or ambiguous. Eg, ref 1 says of climb milling, "the tool is [fed] in the direction of tool rotation". Also see ref 4.

[4]
formatting link
Reply to
James Waldby

A full form thread mill generally has a depth limit and can cut upto that depth limit in one interpolation. (I program 1.5-2 to make sure I get a complete cut at the step over leadins. I don't say pass because I would consider making the same interpolation at multiple diameters multiple passes. Possibly also a "spring" pass. A single form thread mill also cuts the entire thread in a single pass. It just takes more spiral interpolation increments to do it. While its made up of multiple instructions it is one single continuous tool path.

I do not see how a three form could be any faster than a single form. The first tooth does all the cutting. Unless its just a three thread operation (in which case its functionally a full form thread mill) it still has to trace the entire tool path. Okay, I suppose it it were a three start thread... LOL. (I Have not yet seen that tool.) The entire tool matches the angle and pitch of the thread. There is no way it could cut three threads at once. If I am wrong please explain how.

I use full form thread mills for blind holes in slower spindle machines to save time. 1.5 interpolations takes less time than 15.

For through holes I use a tension compression tool on those machines with a spiral point tap. As mentioned in my first post TC tapping is a poor man's rigid tapping for mills that do not have c-axis control, but good consistent RPM and quick reversal.

Actually this is not correct. In practice I have found that most single form thread mills are only suitable for one thread pitch for me, but if you look on the manufacturers websites you will find most are listed for a range of thread pitches. Multi form thread mills can only cut one pitch. Whatever the spacing of the teeth is on a flute.

Reply to
Bob La Londe

Oops. I misread your comment. You said what I said. LOL.

Reply to
Bob La Londe

As a sort of off shoot on this topic. I have seen it mentioned that some guys will use a hand tap as a defacto full form thread mill by removing all but one flute. I can see the programming could be a bit tricky. You wouldn't be able to use default thread mill operations built into your CAM package since the swing diameter of the tool is the same as the finished OD of the thread, but it sounds interesting. Maybe you could use the standard op, and then re-hand-code the lead-in and lead-out.

Reply to
Bob La Londe

PolyTech Forum website is not affiliated with any of the manufacturers or service providers discussed here. All logos and trade names are the property of their respective owners.