.010 and .015 endmills Feeds and speeds

[mike561h]

Hey any salty dogs out there got any good input. Using .015 and .010 4 flute .039 length of cut carbide endmills.

I am using A Haas TM-1 so my max rpm is 4000. Need at least 10k. I am setting my IPM at .7

to see if the cutter won't snap. .003 depth of cut.

Only bought 2 ea of cutters RATS!!!!

 

Mike

[mike561h]

ran .5 ipm and did .015 now running .01 at .4 ipm

no problems. 4k rpm

[bogusmill]

We use a speeder head on that kind of thing. It's 5X spindle with 4000 RPM max so we get 20,000 RPM. One thing to check is tool runout. One of our Haas spindles is out .0015 at the tool and on a .030 cutter it will snap off as soon as the cutter touches the material.

[Mr. Wizzard]

My TM-1 goes 6k.

He he he .......

[Mr. Wizzard]

For more rpm's and a smaller tools, we have a 50k air spindle.

How, exactly, does a speeder head work?

[mike561h]

does msc direct or mcmastercarr sell a speeder head

[GoetzInd]

http://www.airturbinetools.com/

 

http://www.macrotechnologies.com/high_speed_air_spindle_atc_mac.htm

 

We've used both and they work great.

 

Here's a vid of us running one in an old mini mill that we sold. (it's the last tool in the vid)

 

 

Mike

[CNCCookbook]

You may be work hardening if you let the chipload get too low because the tool will start to rub. Micro-milling is hard. The geometry at those scales and the shearing behavior is different, so normal speeds and feeds formulas are wrong. In addition, as was mentioned, even a little runout is a big % of the cutter diameter and hence will break cutters.

 

FWIW, G-Wizard has micro-milling feeds and speeds models based on how Makino approaches the problem and would call for as much as 4 IPM for a slot, 0.003" deep @ 4000 rpm on 0.015" EM. Several of our users are in the watchmaking world and have said they're getting good results with it. That feedrate gives a chipload of 0.0003". If you drop down 0.5 IPM your chipload drops all the way down to 0.00003". That ought to make the tool start rubbing.

 

Cheers,

 

BW

www.cnccookbook.com

[Redfire427]

For tools that small, they require rpm..............and lots of it. Even with a 30,000 rpm Makino, machining like this is a challenge depending on the material. Your run-out must be virtually zero. If you only have 4K, I would suggest an edm.

 

.003 depth of cut is way too much for a .010 or .015" endmill. You will have much better luck with a much shallower depth of cut ( read .0003" ) and a faster feed rate.

 

Carmen

[mike561h]

cnc cookbook I think 4 ipm will snap the puppy. I just machined 2 gears using .4 and .36 ipm. the end mills are still good.

[mike561h]

I ran 6 gears out of 17-4 SS .4 ipm and 4K. I had to remake 1 due to it dropped in the pan and never could find it.

Run time was under 1 hr. Used TIAN coated end mills. Used only 3 endmills. I dropped 1 .012 and 1 .015 carbide broke at .55 IPM. Gear height was .039....