thread milling with shapeoko2?

[flashonja]

Hi,

has anybody tried it?
Is threading in aluminium with shapeoko2 something doable?

cheers
m

[cvoinescu]

I don't think thread milling is feasible with any 3-axis machine, except if you have a very special cutter that can mill it from the side. Maybe they exist, I don't know. Threads are usually cut on lathes, but a 4-axis milling machine can do it too.

If you simply mean tapping, like you'd do by hand but with a machine, then again the answer is probably no. You'd need a slow, high-torque spindle with position feedback, and control software that supports linking axis movement to spindle rotation. LinuxCNC can do that, but you still need the spindle. I'm also concerned that the machine may not be strong enough -- although it will probably work if you're tapping plastic.

[PsyKo]

Hello,

I know that some CN use this kind of end mill :


It's normally designed for boring...

You can use an helicoidal tool path tangent to your drill. I've never used such a tool. I don't know if the Shapeoko can handle it, or if it's precise enough. Maybe there is a RPM limit on this kind of tools...

It's a question I've been thinking about for a long time now, especially for specific thread (big diameter, and so on)... But never found time to actually try it.

[WillAdams]

Yes, one can do this, but you have to fall back on either special tooling, or old techniques.

Special tooling has been covered --- the old techniques are carving a threaded nut in two halves, then fastening it together. Then, one can use the threaded nut to make a thread-cutting box to cut matching threads.

Alternately, on the ShapeOko one could fasten two pieces next to each other, one half the height of the other. Mill the positive image of the threaded rod out of the full size piece, the negative out of the half. Unfasten the full-size, place it in the negative and secure it, then finish milling the rod. Creating the files to do that is left as an exercise for the reader.

[WillAdams]

For the curious, this is addressed as an FAQ on the Sherline site:

http://www.sherline.com/CNCfaq.htm

No problem. This program would do the job. The reason I switched to incremental was I could use the copy and paste edit program for each revolution of the thread.

Code: Select all

%
g90 g40 g49 g00 x1 y0 z0
x0
g91g02 x0 y0 z-0.100 i0 j0.5 f6
g91g02 x0 y0 z-0.100 i0 j0.5 f6
g91g02 x0 y0 z-0.100 i0 j0.5 f6
g91g02 x0 y0 z-0.100 i0 j0.5 f6
g91g02 x0 y0 z-0.100 i0 j0.5 f6
g91g02 x0 y0 z-0.100 i0 j0.5 f6
g90 g00 x0.5
z0
x1 y0 z0
%

This program would cut six threads at 10 TPI.

[Brian]

The big thing you have to worry about is backlash. Odds are you'll at least have to trace the hole with the proper tap upon completion.

[Enraged]

Thread mills are awesome. The only difficult thing on a budget machine is going to be the programming.

There is a manufacturer that sells a thread mill that is designed to bore, thread, and chamfer a hole. Very slick solution, and it removes the need for a tool change for each operation.

http://www.guhring.com/ProductsServices/ThreadMills/

edit: WOW just found this cool little tool on their site: http://www.guhring.com/Tech/ThreadMillCNC/CNCGenerator/

[Brian]

I favor the single point thread mill. That way one tool will work for multiple threads as opposed to needing a different tool for each thread pitch.