[UniqueMachining]

I have been asked to look at the possibility of thread milling a variable number of 3/8-18 NPT threads into a 5 sided aluminum manifold.
As this my first foray into thread milling, I could use any some advice from an experienced user. I realize I will have to make up a jig to hold the 5 sided manifold.

Machining will be done on a Torus Pro.

Thanks

John

[upnorth]

I suggest you go to google and type in "NYC CNC Thread milling". A couple of video tutorials will pop up. That guy has excellent video tutorials for beginners. I have learned a lot from his youtube videos. He has a Tormach but everything in there is also applicable to a Novakon torus pro.

Tom

[AUSTINMACHINING]

I'm using Inventor HSM for cam. I just model the hole with the taper, helical bore the hole using and end mill, and follow up with the threadmill operation. As long as the taper is in the model, the subsequent tool paths will follow.

Sent from my SM-G900T using Tapatalk

[kvom]

I have a 27 TPI NPT thread mill that I'ved use to mill both 1/16-27 and 1/8-27. The larger size won't be any different in technique. The threads are cut in a single circular toolpath. My CAM program (CamBam) has a wizard that generates the g-code. It has a tangent leadin and leadout as well.

Some people have done this using a single-point thread mill, but this requires generates a conical helix toolpath. Obviously this is a lot slower in machine time, and as well the thread form may not be precisely correct.

I calculate the F&S using the tables on the Harvey Tool website. Start with material to get SFM and chip load. Then use cutter diameter and number of cutters to determine RPM.and linear feed rate. Finally adjust feed rate for a circular toolpath (faster for external threads, slower for internal). http://www.harveytool.com/secure/Con...s/SF_71000.pdf

Since the tools are fairly expensive, I start off cutting air above the work to verify position and arc visually. I also start cutting the first test thread at a slightly smaller depth and sneak up on the proper depth, since the cutter diameter specified may be off a few thou. I also do the first trials in brass until the thread is correct, then adjust the F&S for steel.

When I thread mill straight threads with a single-point tool I take a spring pass. Haven't found this necessary with NPT threads.

[UniqueMachining]

Thanks to all.

Will check out the NYC CNC videos and other sources. I'm using BOBCAD so I'll have to see what they offer.
Seems to revolve around the choice of a single thread mill (More versatile, slower and less accurate) and a thread specific mill.

Just one more task to conquer..

Appreciate, John

[SCzEngrgGroup]

Personally, I would not be too concerned about accuracy on a tapered thread - a single-point tool will work just fine with good G-code. By definition, tapered threads will be deformed to a tight fit when tightened up, so they just need to be close. A multi-point tool will be a lot faster, but also a LOT more expensive, and typically requires a special holder, which is more $$$.

Regards,
Ray L.

[vmax549]

It will all depend on the class of fit and the pressure rating on the port you plan to tap . Also the number of holes you plan on tapping. Most thread mill manf offer teh software free of charge to program what you need using their threadmills (;-). If this is to be a reoccuring job then a multipoint single pass tool is the way to go. IF it is just a onesy twosy type of job then singlepoint would be fine. But if that were the case I would simply TAP it with a good tap (;-).

Just a thought or 2 , (;-) TP

[kvom]

I spent the morning making some 1/8-27 NPT plugs. Needed 6, made 10.

Attachment 305588

Using a NPT thread mill one decision to make is how many threads to cut. Commercial plugs I have bought use 10 threads, so that's what I did too. It's difficult to choose a minor diameter since each thread has a different one. So you have to experiment to get the right g-code arc. Same would apply with internal. These are from 7/16 brass rod and use a 3/8 wrench. The commercial ones I have use a 1/4" square head.