[dneisler]

I have a couple parts to make for a customer that have some -10 AN tapped holes (7/8-14) and I need to find away to tap them. I am considering thread milling. I have been looking at this threadmill: Single Form Thread Mill .372 Dia X 1.125 Max Depth TiAlN Coated Made in USA MariTool

Am I understanding this right as long as the hole is big enough to get the tool in it will do threads from 14-32 TPI?

[SCzEngrgGroup]

Yes, that is correct. I use basically that same threadmill for cutting internal and external, Imperial and Metric left- and right-handed threads. So far, I've cut up to 32mm (internal and external), and down to 1/4" (external).

That's the great thing about single-point threadmills - they aren't fast, but they are VERY versatile.

Regards,
Ray L.

[dneisler]

Thanks Ray,
I have to tap a 7/8-14 what treadmill would you recommend me buy, I sure do not want to break the bank. Also, feeds and speeds as I probably can only afford 1 :-)
I have been eyeing the Maritool ones and the expensive Lakeshore Carbide ones.

[SCzEngrgGroup]

It's a trade-off. I would want the smallest one I could get by with, to give me the widest range of thread diameters I can do. But, small also means less stiff, which means slower cutting. The only one I currently own is a Maritool 0.372" diameter, probably the same one you're looking at. I've been using it for almost 18 months now. For anything smaller than 3/8" internal, I use taps. I typically cut at 6000 RPM/20IPM in 6061, and get threads that are absolutely beautiful. In most cases, I'll do two passes, rough to about 0.010" over/under, then a finishing pass at 35 IPM.

Regards,
Ray L.

[dneisler]

Wow that is flying. I assumed, we all know what that is good for, it would be like 1IPM.

You are correct that is about the size I was looking at if not the one. Any tips to look out for?
I will using Hsmworks Express or Fusion 360 for the programming.

Again, Thanks Ray for the feedback.

[SCzEngrgGroup]

No tricks really. Youll likely find you need to do a few test cuts to sneak up on the final dimension if you want a really precise fit. But, otherwise, HSMXpress makes it really painless. The .TXT file below contains my HSMXpress tool definition for the 0.372" threadmill in .CSV format. You can import it into Excel, then cut/paste it into the HSMXpress or Fusion tool library.

Regards,
Ray L.

[dneisler]

Thanks a ton Ray. I will let you know how things go. I just ordered my needed tooling so as soon as I get it I will start on these parts.

[WOTDesigns]

Ray, how do you calculate the error from the square end of the cutting edge? I'm sure I could figure it out, but on the Lakeshore carbide tools I have to add diameter to offset the lack of sharp point on the tips. Then I had to do a bunch of 1-3/8 threads so I bought a much larger (and cheaper) tool from KBC and since it had a sharp point it cut a perfect diameter thread on the first try.

Brian
WOT Designs

[SCzEngrgGroup]

The threadmill has sharp points on the cutting edges - it has to, to be able to cut small, and/or fine-pitch threads. That's part of the reason you have to sneak up on the final dimension for each thread diameter. I've had no luck calculating the correct final diameter. Calculation will get you close, but not perfect. So, the first time I do a new thread, I cut under size, then go in increments of 2-3 thou, checking the fit after each increment, until I get a perfect fit. Then I create the "production" code using that final dimension.

Regards,
Ray L.

[WOTDesigns]

The Lakeshore carbide ones don't. The end has a small flat I assumed was standard on these. Won't be ordering theirs again. I did basically what u said. I programmed for the correct size knowing the flat would cause underside then offset the wear value to get a good thread. PITA having to check the thread over and over.

What's interesting is their pictures online show it coming to a point but the actual tool had very (VERY) small flats as if they didn't want them to chip off.

Brian
WOT Designs

[SCzEngrgGroup]

The Lakeshore carbide ones don't. The end has a small flat I assumed was standard on these. Won't be ordering theirs again. I did basically what u said. I programmed for the correct size knowing the flat would cause underside then offset the wear value to get a good thread. PITA having to check the thread over and over.

What's interesting is their pictures online show it coming to a point but the actual tool had very (VERY) small flats as if they didn't want them to chip off.

Brian
WOT Designs

Brian,

There is a minimum pitch specification for each tool. I've always assumed that is why. There is also a maximum pitch, which is limited by the length of the cutting edges.

Regards,
Ray L.

[WOTDesigns]

Ah... I used the median pitch. Perhaps using the maximum would be closer with those.

Brian
WOT Designs

[BAMCNC.COM]

Good stuff, I need to try threadmilling. Wasn't sure how HSMWorks would handle it, never really looked I guess. Thanks for the link to the tool, I'll start with #8 and 1/4" threads tho.

[TurboStep]

The calculations for the diameter are just simple trig:
http://www.cnczone.com/forums/tormac...ml#post1552318
Don't forget to reduce the feed rate for internal threads dependent on cutter diameter and thread diameter.
Step

[BAMCNC.COM]

If only calculations ever worked out right, lol. Will get you very close though, and is better than winging it. I can calibrate my single point threading tool on my lathe that will hold .0005 or better, but when I have it thread a part, it never fits like "they say", and always requires a spring pass.

[TurboStep]

If calculations don't work out right, then they were not done correctly.

[LSM]

the calculations needed can be found in Machinery's handbook.
in HSMworks you just have to make a drawing of the form tool, that would be your threadmill.
key part is accurately measuring you threadmill.
your hole size is the minor diameter.
put in the appropriate values for your thread and it comes out slicker then snot on a door knob

[WOTDesigns]

If calculations don't work out right, then they were not done correctly.

LOL. what a deep statement.

Brian
WOT Designs

[TurboStep]

LOL. what a deep statement.

I didn't want to offend anyone...

[WOTDesigns]

I laughed pretty hard.

Ancient proverb say... If calculations don't work out right, then they were not done correctly.

2+2=4 unless you compensate for tool deflection, tool wear, material irregularities, machine backlash, machine flex, machine vibration, thermal expansion, etc. Then 2+2=4.0375

Brian
WOT Designs