Experimenting With Thread Milling - Need Help

[TTrap]

Just started messing around with thread milling but not sure if I'm on the right path. I have a hole with a .201" diameter and a depth of 1.00". I want to thread it using a 1/4-20 Thread Mill Tool to a depth of .400". I created a Thread Mill tool based on the manufactures dimensions (Cutter Dia. = .180", LOC = .500", Shank Dia. = .1875", OAL = 2.50", Flutes = 3, Pitch = .05"). The tool looks just like an end mill, not a thread mill. I created the Thread Mill toolpath (in the drilling setup). It looks o.k. but during simulation, the side of the tool moves along the side of the hole, so to me it seems it wouldn't leave any threads. Did I make the tool correctly even though it looks like an end mill? Could someone please provide some information on how they would make the tool and program the threads? I tried a search on the forum and the help menu, but not much there.  

[TTrap]

Forgot to add that it's a multi-form tool I'm using.

[Anonymous]

To actually thread-mill the hole you will need a negative offset so that the tool violates the surface (depending how they draw the hole and how you made your feature set)

[Anonymous]

The cutting edges of the threadmill need to be at the outside diameter of the threads (.250 in this case) We set the hole feature diameter on a 1/4-20 hole to be at .250 and cut to that.  We end up putting a little radial thickness (about -.004 in this case) in order to get the fit we want and account for a little wear on the threadmill.  You can accomplish the same thing using the .201 hole by putting more negative thickness into it.  (.250-.201 = .049/2 = .0245)  So -.0245 in the radial thickness and then a bit more for fit/wear.

Typically when trying out a new threadmill, I start with nothing added for fit/wear and then program it with cutter comp.  Then I run it using comp until I get the loosest fit I would ever want to know how far to go in the future without comping.  Typically the threads will end up a little tighter than that due to wear and a little cutter deflection.

[TTrap]

Thanks for the information. Just a few questions:

1) Do I add enough turns for the tool to spiral all of the way out of the hole (attachment 2) or will just a few work (attachment 1)? 

2) Is the way I created the tool correct, or do I have to I have to use the Form tool option to make it look like a thread mill? I'm not very experienced with using the Form tool option and it's seems like it would be a pain in the ....

3) The tool manufacturer has a wire frame profile available. Is there a way to get it into my tool library?

4) Would it be better to have the hole diameter in the CAD model at the maximum tap drill size (.2055") instead of (.201")? I know this depends on what kind of fit I'm trying to achieve and the type of material I'm machining, but for now this is just for practice. I'll start out with Ren Board and then eventually try aluminum.

[Anonymous]

1.) There is not much benefit in going more than one turn as long as you are not going deeper than the cutting portion of the tool.  If you want more passes, use number of passes options under the threading tab in the toolpath form.  Aluminum you probably won't need to.  Steel you might depending on what it is.

2.) The way you have it is fine.  You can use a form tool if you like for the visual effect in programming it, but it won't affect the output at all.

3.) Yes there is.  You might be able to import it directly.  See snip below.

Generally that doesn't work in my experience.  Usually I create a pattern, right click on it>Insert>File.  Then go into the curve editor, delete the shank portion if you like, select it all, right click on it>merge selected.  Then select that pattern the form tool form and use the right button in that section to create it. See snip below.

4.) I don't think the hole size matters all that much.  Just make it so that the tips of the threadmill are running out at least at a .250 diameter hole (for 1/4 threads).  Whether you get there using negative thickness or adjusting hole size doesn't really affect the end result.