Typical thread milling parameters? Tips?

[Garwood]

I'm new to thread milling, so far I've got great results, but I'm going conservative. 5000 RPM 25 IPM .01" stepover, 3 passes, .005 finish doing M16x1.5 in 6061

I need to do many M10x1.5 threads now. How many passes and what RPM/Feed would you threadmill M10x1.5 at? Using a .300" diameter 3 flute full form threadmill.

Do you go faster in a through hole VS a blind hole with flood coolant only?

Thanks!

 

[chad883]

I like to start at the bottom of the hole and move Z+ (so I am climb milling). I usually do it in 1 pass and 1 spring pass in 6061 with a multi lead thread mill. I will drop to depth and radius into full profile depth and mill 2 full circles from there. This does not give a spring pass on the last thread, but that is fine in my application. This is for a 32 TPI thread. The speed could go up if there is enough meat around threaded hole to prevent chatter.

 

[Booze Daily]

I'm new to thread milling, so far I've got great results, but I'm going conservative. 5000 RPM 25 IPM .01" stepover, 3 passes, .005 finish doing M10x1.5 in 6061

How many passes and what RPM/Feed would you threadmill that at? Using a .300" diameter 3 flute full form threadmill.

Do you go faster in a through hole VS a blind hole with flood coolant only?

Thanks!

Wow, that sounds aggressive. You are only interpolating an .094 circle, 25 IPM at the periphery sounds like a hell of a chip load.

 

[Vancbiker]

The only “production” thread milling I do is an M6 by 10mm deep in 6061. I start at the bottom. Feed into major diameter and then two turns out. Move to center and retract.

 

[Herding Cats]

Keep in mind when the circular path of the tool is small in relation to the tool diameter the cutting edge can be feeding much faster than the center of the tool is moving.....programed speed.

Some quick rough math shows a .300" tool moving on a .075" circle will have an outside speed 5 times the center speed. So about 125 ipm cutting feed when programed at 25 ipm.

I am not saying it should be a .075" diameter helix. Just used roundish numbers for easy math.

 

[Garwood]

Wow, that sounds aggressive. You are only interpolating an .094 circle, 25 IPM at the periphery sounds like a hell of a chip load.

You know what, I mis-typed! I was doing M16x1.5 threads with those settings and now I need to do bunches of M10's. I had M10 on my brain, that's what I bought the threadmill for. I went back and fixed the original post. Thanks.

So for M10x1.5 with a .300" tool what would you guys be running for RPM/feedrate to do it in 2 turns?

 

[Booze Daily]

I'd probably be at 3000 rpm and 6 IPM, but I'm conservative.

 

[Herding Cats]

I'd probably be at 3000 rpm and 6 IPM, but I'm conservative.

I run a .375-16 thread in SS with a similar thread mill and run it 2000 RPM 8 IPM.

So yeah, you and I are both in the same ballpark

I also get thousands of holes from 1 tool in SS

 

[Garwood]

I really appreciate the numbers. There's a lot going on with that fat corncob in a small hole so having a baseline for what works reliably is a huge help!

 

[Booze Daily]

That’s why I go conservative. I like chips to have someplace to go, coolant to stay in there and stuff to come out round.

 

[Herding Cats]

If you have TSC this type of threadmill does a great job of blowing the chips out of blind holes.

 

[g-coder05]

If you have TSC this type of threadmill does a great job of blowing the chips out of blind holes.

View attachment 943

I hate to be the bearer of bad news but I think your keyboard my have seen better days.

 

[Herding Cats]

I hate to be the bearer of bad news but I think your keyboard my have seen better days.

It's fine, the covers get jacked up from the heat cause I have the CPU and GPU overclocked

 

[Spruewell]

In 6061 I would be running as many rpm as the machine will allow. Then start increasing feed rates.

 

[SD&M]

Gotta love it-HerdingCats threadmill may cause cancer! Go Prop 65!