[Don Clement]

I posted this on another forum about threading on a manual lathe and thought it might be useful for Tormach CNC lathe owners as threading on a CNC lathe should be the same as on a manual lathe only one could take advantage of things like infeed using the alternating flank method that is not as practical to do on a manual lathe.

This is a good article on threading with carbide on a lathe. Threading On A Lathe : Modern Machine Shop

I cut internal threads all the time in aluminum using carbide insert tooling with excellent surface finish although typically 2" to 4" diameter.

Here is how I would cut a 1" internal 24UN thread in 6061- aluminum on my lathe:. Recommended minimum surface speed is 262 FPM so minimum of 1K RPM. I use the reverse helix method with spindle running CW with feed toward the tailstock for threading at 1K RPM. Tool is facing upward on the inside wall opposite the operator. Threading tooling used :AVRC075-3CLH toolholder, 3IL24UN full profile insert, YE3-2N anvil . I would bore a hole 0.955" and if this is a blind thread also put in a 0.050" wide 0.050" deep internal slot using a Nikcole Mini-systems grooving tool as shown below. FYI Arthur Warner HSS grooving inserts fit Nikcole Mini-systems toolholders. I would feed radially in using the cross-slide. I would use 8 passes starting with 0.005" DOC and ending with 0.002" DOC. Note that when using the reverse helix method on internal RH threads infeed for the cross-slide (or compound) is in the same direction as external RH threads or as in regular turning. I use Relton A9 cutting fluid.

1K RPM is key here when using carbide for threading 1"- 24UN in aluminum for good surface finish. BTW I use radial infeed using the cross-slide for 24UN so feeding using the compound @ 29.5* is not a factor for good surface finish for me. I have gotten excellent surface finish when threading using this method and tooling on my import Chicom 12x36 lathe and even better results threading on my import Graziano SAG12.

Don Clement

Nikcole Mini-Systems internal grooving tool


Front view of insert threading toolholder


Threading tool set up for internal threading on wall opposite operator

[kirk_wallace]

In the case of the Tormach lathe, the conversational routine is very basic. It in-feeds with a compound angle of 30 degrees with the cuts approximating an equal area depth of cut keyed on the initial depth of cut.

With CNC threading, care is needed to allow the threading path to stabilize before getting into the workpiece. This gets worse at higher spindle speeds. If one needs staggered passes, this would need to be handled in CAM or g-code. The thread exit doesn't need a clearance slot, but the last bit of the last turn might not be well formed, so ending clearance may be needed if the mating thread will run past the end.

Another common issue is with the tool form and major and minor diameters. Common published values assume a 60 degree tool with the tip blunted in a standard form. It is common in hobby machining that the tool is a sharp or non-standard tip and the published values won't work well.

[Don Clement]

In the case of the Tormach lathe, the conversational routine is very basic. It in-feeds with a compound angle of 30 degrees with the cuts approximating an equal area depth of cut keyed on the initial depth of cut.

For pitches finer than 16tpi I just feed radially and have no real problems. YMMV I use Vardex TT program Vardex Thread Turning, Thread Milling & Miniature Threading | VARGUS GENius™ – NEW! to determine how many passes and the proper anvil for helix angle. When using an insert tool for each pitch the thread is stronger and there is less thread depth for the coarser pitches than when using a universal tool with a fixed sharp tip form.

The thread exit doesn't need a clearance slot, but the last bit of the last turn might not be well formed, so ending clearance may be needed if the mating thread will run past the end.

A clearance slot works well for me on the lathe. In addition to adding clearance slot I use the same insert grooving tool used for the clearance slot to square the end of the clearance slot for proper seating.

Another common issue is with the tool form and major and minor diameters. Common published values assume a 60 degree tool with the tip blunted in a standard form. It is common in hobby machining that the tool is a sharp or non-standard tip and the published values won't work well.

I use the Machinery's handbook for thread form specifications. Seems like a simple thing to grind the tip to match ISO or UN specifications for a specific pitch even for "hobby machining". For me I use a full profile lay down insert for each pitch because, in addition to producing almost perfect thread form, the O.D. and P.D. are concentric and there are no burrs or other imperfections needing another process for clean up.

Don C.

[kirk_wallace]

Don, I found your website. That's a fine product you are making. I have been working on the same 6" telescope mirror for the past 40 years. I might finish it one of these days. I live just west of Yosemite Park with pretty decent night skies. I hope your being next door to LA isn't too bad.