Multi start thread Mill

[DavidB]

Hello I have to thread mill an internal thread with 3 starts. How can I do this? Thread mill only has one start

Do I have do 3 tool paths starting at 0,120 and 240 degrees?

 

Cheers

[Aaron Eberhard]

11 hours ago, DavidB said:

Hello I have to thread mill an internal thread with 3 starts. How can I do this? Thread mill only has one start

Do I have do 3 tool paths starting at 0,120 and 240 degrees?

 

Cheers

Yep, you got it.  Threadmill doesn't currently have multi-start capabilities baked in. Your other option if it's only one hole is to use Transform, of course.

[DavidB]

I have asked the tooling reps and Im waiting for an answer.

Does anyone  know if the Internal thread mills can do a multi start thread?

Or will I have to use a single point tool.

[gcode]

I believe they can but have never tried it with thread mills

You would need a thread mill with a pitch one third of your final pitch.

For example, a 12 pitch 3 lead thread would require  a 4 pitch thread mill

You must be sure the bottom of your thread mill has the relief to clear the steep helix it will be cutting

This is an old post of mine doing a 6 lead acme thread

It was not possible to do this with a vertical tool as the helix was severe 

 

[Eric@HorsepowerInc.]

It can be done, how this triple round thread with Higby’s  look . When I get some time I’ll post what I can for you.

[BILL HUNTER]

12 hours ago, DavidB said:

I have asked the tooling reps and Im waiting for an answer.

Does anyone  know if the Internal thread mills can do a multi start thread?

Or will I have to use a single point tool.

You can single point or grind off every 2nd and 3rd tooth.

[crazy^millman]

12 hours ago, DavidB said:

I have asked the tooling reps and Im waiting for an answer.

Does anyone  know if the Internal thread mills can do a multi start thread?

Or will I have to use a single point tool.

I think you answer your own question if you break it down. It must be a single point thread tool. If you use a multi flute tool then at each lead you will get cutting above and below that thread cutting into the other leads thread wiping them out. I have always used single point tools for doing this.

Think of doing it on a manual lathe like we did 35 years ago when I learned it in trade school. 3 Jaw chuck was used for 3-6-9 lead threads. 4 jaw chuck was used for 2-4-8 lead thread. The rare 5 lead thread you could use either chuck and needed to mark off 5 places. You would then mark each jaw or each division for your start of thread. I remember many times starting at 8 rpms to get the timing down. We always used a single point tool and sometime had to grind them very extremely to get the correct rake angle to even cut the thread. I have never machined anything more than a 20 lead with a threadmill. I have done as fine as a 6 lead 96 pitch for a telescope lens prototype and only covered about .06 of thread area. I was impressed it even worked.

[DavidB]

Thread is M50 X 2 (3 starts)

I have programmed a single point insert to thread mill a 2mm pitch at 0,120 and 240 degrees.

I will cut it today and see how it goes.

Thank you

[crazy^millman]

27 minutes ago, DavidB said:

Thread is M50 X 2 (3 starts)

I have programmed a single point insert to thread mill a 2mm pitch at 0,120 and 240 degrees.

I will cut it today and see how it goes.

Thank you

David normally you program them with a 6mm pitch don't you? I have always gone by the rule the number of leads is what you multiple the pitch by to come up with the difference.

Reference Link #1

Reference Link #2

Reference Link #3

Old Thread where I said about the same exact thing 10 years ago:

Old Forum Link

[Leon82]

1 hour ago, DavidB said:

Thread is M50 X 2 (3 starts)

I have programmed a single point insert to thread mill a 2mm pitch at 0,120 and 240 degrees.

I will cut it today and see how it goes.

Thank you

[DavidB]

3 hours ago, crazy^millman said:

David normally you program them with a 6mm pitch don't you? I have always gone by the rule the number of leads is what you multiple the pitch by to come up with the difference.

Reference Link #1

Reference Link #2

Reference Link #3

Old Thread where I said about the same exact thing 10 years ago:

Old Forum Link

Thank you as always you are correct.

[DavidB]

Done! Thank you to everyone for their help.

M50 X 2 (3 start) Internal thread - thread milled using a single insert. (Lathe boring bar and Insert)

Programmed a 6mm pitch and transformed rotated the tool path twice at 120 degrees.

Cheers

[crazy^millman]

8 hours ago, DavidB said:

Thank you as always you are correct.

Cool Beans and I am wrong a lot of the time just glad I had the experience to point you in the right direction this time. Cheers Mate.

[DavidB]