[brow318]

Anyone using multi profile thread mills for tapered threads?

I have the following thread mill

http://www.lakeshorecarbide.com/18-2...dmillnptf.aspx

My plan is to spot the hole then drill using letter Q drill to depth of hole.

With a tapered mill should I just use a hole drilling cycle to tap? Also does anyone have the multi profile tool in Sprutcam?

Kevin

[Hirudin]

I have that exact tool and I mill just a single spiral with it to make the tapered thread.

[Hirudin]

Sorry, I forgot to answer the other part of your question. Thanks for the reminder PM.

I do indeed start with a Q and make the machine cut the threads in three or four passes. That's three passes doing the whole depth so the tool is taking light passes. I can't say if it's the 'best' or fastest way to do it, but it seems to work. I run it at 148 mmPM @ 6000 RPM. What has worked for me is to do a thread depth of 8 mm and a "diameter" of 11 mm. (I don't really know at what point in the hole SolidCAM thinks the diameter is 11 mm, but it seems to work so... whatever.)

SolidCAM has a dedicated "thread milling" operation type, so that's what I use. I don't think a drill operation would work. Attached is a screenshot of what the toolpath looks like - just in case it helps.

By the way: although the threads get cut with the settings I'm using I'm not certain whether it's actually creating threads that seal correctly. I'd recommend putting some Teflon tape in there for good measure.

[FuriousGeorge]

Random multi-point thread milling question here. Say I have an m3x0.5 thread mill. Could I use that multi-point thread mill to cut any threads with a 0.5mm pitch and D>3mm? It seems to me that it would work fine, I would just have to go gentler on the feeds and speeds due to decreased rigidity.

[Hirudin]

That would make a lot of sense and it's my understanding. I've milled some 7/16-20 holes using my 1/4-20 thread mill.

[Don Clement]

I use multi-tooth inserts for a specific pitch. Each specific pitch insert works on a variety of diameters. For tapered threads I use a tapered thread insert: TM (BSPT, NPT, NPTF)

The Vardex TM handbook may be of interest: http://www.vardexusa.com/vardex-pdf/Hand_Book_inch.pdf
I found this excerpt from the Vardex TM handbook also interesting:
“The thread milling operation is based on three-axes simultaneous movement so the profile shape on the
workpiece is not a copy of the insert profile. In other words the profile is generated and not copied which is contrary to the
thread turning operation. This fact causes a profile distortion, especially when machining coarse pitch internal threads.
The profile distortion depends on four main parameters:
• Thread dia. • Tool cut. dia. • Thread pitch • Profile angle “

Don

BTW I modified the 3/4" shaft of the Vardex TM insert toolholder to be TTS by adding a ring and machining a groove for circlip as shown.

[Hirudin]

I randomly came across this video that talks about thread milling. I didn't really watch it intently, it was playing in the background, but it seems like it has some good information in it - including a possible explanation of why I needed to tell SolidCAM a somewhat random diameter to use.

Single Point Threadmilling Tutorial - YouTube

[rlockwood]

I randomly came across this video that talks about thread milling. I didn't really watch it intently, it was playing in the background, but it seems like it has some good information in it - including a possible explanation of why I needed to tell SolidCAM a somewhat random diameter to use.

Single Point Threadmilling Tutorial - YouTube

Im at work, so not going to watch the video now.. I also have never thread milled with solid cam. I can say though, that a good tip at least for hsmworks, is to switch a threaded feature to "remove thread" when you're going to be thread milling it. It will automatically set the ID of the threaded portion to the necessary diameter (the root dia) for the thread. Possibly helpful in solidcam as well?

[Hirudin]

Heh, I see that same video is posted in the other thread-milling thread in the Tormach forum... Oops.