I need to make a internal thread that looks like this. http://www.metalworking.com/DropBox/rockbit.jpg
The thread is called a T38 and it goes to a rock drill bit. How do I go about making this thread. Should I get a form tool made to those specs, but I worry about chatter? I don't really know. I do grinding for a living and not much turning so any help would be great, thanks. I have all the spec on the thread, I will try to post them to.

Here is the specs on the thread. It has a lead of .629 and it is 1.500" od. and this is the specs.
http://www.metalworking.com/DropBox/rockbitspecs1.jpg

If you can grind the profile, threading shouldn't really be that bad. Go relatively slow, take light cuts-.005 to .01, use oil and try to use the tailstock for support. It's a relatively shallow thread. Good luck.

p.s.
just noticed the lead--.629. That could pose a problem if your lathe cannot accomodate it. You might have to use a cnc lathe.

Yes, I would worry about chatter if I had to lathe turn it with a form tool, so I would not use a form tool, just a radius insert.

Because the lead is a little extreme, you may need to use a threading bar with angle shims beneath the insert. I am familiar with Sandvik tools which have this type of feature. Otherwise you need an insert with extreme clearance on the front to clear the flank of the thread you are cutting.

You can rough the thread with an Acme thread insert, then switch to a radius insert, and plot an offset path from the final profile. Interpolate the offset profile into short segments, then use each end point as the starting point for the threading pass. Of course you would start some distance (maybe one or two thread pitches in front of the hole before the bar engages the work. Then, program individual threading passes with G33 (which I think would be the most common standard for single pass threading cuts). G33 will call for spindle synchronization, and you are free to start at a new XZ point for each pass, once again, based on the interpolated profile I wrote about before.

This little sketch should help you get the idea. I drew in the offset path, interpolated it, then drew in some semicircles representing a radius nose tool which matches the offset of the curve. You would not actually use the semicircles for anything: only the arc centers of those semicircles would represent the start points for each G33 pass.

Of course, you might want to interpolate the curve much finer than I did to get a smoother result.

BTW, if you are doing this on a manual lathe, you can set the compound at 90 degrees and use it to get the proper Z coordinate for the starting points. That way, you can use the half nuts for threading in the usual manner, if you have a metric lathe (the thread pitch is 16 mm).

Seems the KISS program has been overlooked!
1st off what type of material are you going to be threading? Brass/Bronze?
2nd how many do you need to make?
3rd do you have any spare screws as in the picture?
It's not all science, it's art
caitolly

Oh, boy! I can hardly wait to see the simple method for doing this! ;)

Ah, a skeptic!
since my wordsmithing skills would probably be incoherent.
I'll go take some pictures of a tool I made some time ago, to do a funky thread.
Disclaimer: It may work, It may not work.
"I'll Be Back"

:stickpoke This was a one time use tool, it is actually a double lead, left hand thread, that was used to make the internal threads for a quad (4) lead, right hand thread, plastic injection mold, thats a sample from the mold on the left, for some kind of medical device. Not having access to any fancy cnc equipment at that time, I scratched a bald spot on my head trying to figure out how to make this thread in the mold. I made this tool out of D2 or A2 tool steel, don't remember which.
Which brings me to the simple approach.
As I suggested, if Donovan has an extra screw that could be modified in a similar manner, basically you would be making a funky tap, note the pilot, similar to a spot face tool, and if neccesary case harden the screw. Drill or bore the hole to the minor diameter. In this case you would have to use machine feed as HuFlugDung suggested, similar to power feeding a regular tap, otherwise you would just bore a bigger hole.
No fooling around with expensive form tools, chatter is eliminated due to the built in support opposite and below the cutting edge.
See nothing to it !! :banana:

you go hu

The guy that I am making them for wants 10 pcs. They are made out of 4140 or 4340. We do have a Mori Seiki CNC lathe but we are still learning how to use it. It have the MAPPS control on it and that is where we do the programing from. So it has all the basics that we need for every part that we have tried to program but this one is kicking me in the butt. We are a grinding shop that is learning how to use a CNC lathe.

HuFlungDung would you be willing to make a program for me and what would you charge?

caitolly I have thought about doing it your way but we have this nice lathe that I think I should beable to do it on. :cheers:

Caitolly,
I'd be too scared to turn on the lathe to tap a serious thread like this one: maybe if I could hide outside the shop while it ran the cycle :D

Donovan, it would be better if I could help you understand how to do this yourself, because you may have to modify the program a tad just to make the final part fit.

Does your lathe use a G33 cycle for threading? It may also use G76 for multipass threading, but you don't want that one because you need total control over every pass in this project.

Just post a sample of how you would use the G33 (or whatever Gcode it is) inside of a typical threading program. If anyone else wants to volunteer this info, that would be great :) It would be best to get this understanding first.

The program type I suggested is not really complex at all: just a series of XZ coordinate starting points for your radius tool, derived from a sample profile, followed by the same G33 line (which takes your tool to the far end of the hole), then a hand written tool retraction (also stays the same), and a return to the next XZ coordinate.

It is unnecessary to model the threads in the hole. All you need is the sample profile of one thread (just like you drew) maybe situated about an inch in front of the stock hole. Break the offset of this profile into tiny bits (that's what interpolation means, and I don't know what software you would be using), just for the sake of creating a bunch of segments which you can place points along. Use your software to find the coordinates of each point. Then, handwrite the program.

Okay, I think that I am understanding. It will take me awhile to get this but I will do it. I did look at the g codes today and the Mapps programs in a threading cycle and I don't remember which it is but I will find out tomorrow or Monday. Thanks again.

HuFlungDung,
Good point, ............did I mention low rpm's (chair)
caitolly