Threadmill issues

[Michael Sullivan]

I have a set of mating parts with M22 X 1.5 threads on them made out of Delrin. I have a multi-tooth threadmill and I take the thread in one pass.

The problem I am having is :

 

On the external thread

In order to get the pitch diameter In tolerance, I have to bump the offset so much that the thread mill cuts the major diameter of the thread too small by .005 or so(out of tolerance).

I'm not sure it is a big problem since the major diameter is a nominal size and I know the fit is what's really important.

 

all I can figure is that, it is the threadmill geometry that is the problem.(Maybe they can only make the inside of the teeth so sharp so inevitably there is a small radius in it?)

 

anyone have any problems like this?

[Guest CNC Apps Guy 1]

Have you put your tool up on a comparator to check the tooth profile?

[Michael Sullivan]

Comparator.....I wish. I would have to go to a machine shop to find one of those, lol.

 

I just looked at the tool by eye though and can see a small radius in the corner

 

This is the one I have:

 

http://www1.mscdirect.com/CGI/NNSRIT?PMAKA=60024437

 

I would imagine it is tough to manufacture this type with a sharp corner.

 

Is it normal/expected to have a small radius on these kind?

[Guest CNC Apps Guy 1]

I have NEVER had a problem with Scientific Cutting tools having errant threadforms and I've been using their threadmills since I can remember...

 

I'll look in my machinist's handbook for the form specs and get back in a few...

[Guest CNC Apps Guy 1]

Looks like ther is some allowance for a radius at the root..

 

[Mike Whitten CAD/CAM Contractors]

Mike,

 

You may want to insure that the tool you are using is designed for OD threads. Here is a snip from the Scientific catalog / website:

 

----------------------------

How to Order Thread Mills

 

Thread mills must completely enter the minor thread diameter before cutting the internal thread. (See figure 2) Thus our catalog lists the smallest internal thread that each thread mill can produce. The same thread mill can also produce any larger size thread of that same pitch. Also, for small sizes, it is best to use our short series with the reduced length of cut whenever possible.

 

All of the straight flute thread mills are for internal threads only. All of the staggered tooth thread mills will cut both the internal and external threads. The helical thread mills over 0.187 diameter will also cut both internal and external threads.

 

Staggered tooth thread mills have every other tooth removed in a staggered pattern; as the tool rotates the adjacent flute fills in for the tooth that was removed. This helps to reduce side cutting pressure, thus reducing chatter. This can be extremely beneficial in small external sizes and for set-ups that lack rigidity.

 

Helical fluted thread mills are also designed to reduce side cutting pressure by distributing the cutting pressure along a helical flute. Although these tools cost slightly more, their high performance design allows for less chatter and higher feedrates.

---------------------------

 

Mike

[Michael Sullivan]

The root of the cut thread is sharp because they can grind that on the cutter, The problem is that the radius is in the root of the threadmill profile therefore, it cuts the major diameter of the (external)thread small. I guess they can only grind it so sharp.

 

the result:

 

External thread =Major dia too small

[Michael Sullivan]

You hit the nail on the head Michael. The wrong tool for the application

I guess I need the staggered tooth threadmill.

 

quote:

---

All of the straight flute thread mills are for internal threads only

---

every day is a school day!

 

Thanks a lot guys.

[Guest CNC Apps Guy 1]

DOH! I forgot about that too. Man... I need another vacation. Sheesh

[Ray Edwards]

mike

 

what i use for outside and inside thread milling is actually the boring bar for a lathe with single tipped thread cutting.. does that make sense... i just shortend the tool to fit into my BT40 tool holder..

[Mike Whitten CAD/CAM Contractors]

Ray,

 

I believe this is fine. The key is to check thread form, Major and PD. If those are good, you should be good.

 

Mike

[Michael Sullivan]

I have single point threadmilled many times before and it works great but it takes a bit longer than these multi-tooth/flute type threadmills.

 

You can really rip these things through material.

 

It works fine for internal/external threads as long as you have the right cutter

 

You have to buy the spiral flute not the straight flute.

[Greg_J]

I have that problem sometimes with Advents threadmill using the stub acme thread. In order to get my thread depth to the depth required it wants to cut my minor dia, which I don't want.

 

What I do is offset my tool up or down .001 or .002 and then it opens up the pitch dia on my thread then I have no issue with my gage going in.