Micro Machining Titanium

[nmercier]

Hey Guys,

Looking for some tips and tricks for machining Titanium. Kind of a rough setup as I'm running a 2003 HAAS VF2 SS and milling a piece that is smaller than an inch in X,Y, and Z. I've gotten good results on most of my end mills but I keep snapping a 0.035" Diameter End Mill as I'm rough/finishing a pocket that is about 0.070" deep. Running it at 5% stepover and 10% of Tool Diameter at 75 SFM. Not sure if the tool is breaking due to the coolant and I should run no coolant on this operation or if I'm leaving to much material on prior roughing steps with an 1/8" end mill and a 0.055" Diameter end mill.

Any suggestions or tips are welcome.

 

[Screwmachine]

What's your feed rate, spindle speed, how many flutes on your end mill and what material (carbide I hope)? With a quality carbide end mill, in a good holder, i.e. running very, very concentric, I would shoot for a chip load of around 0.0002" per tooth, which would be about 4 ipm with a 10k spindle. That's for a two flute mill; I'd drop the chipload 20% or so with a 3 flute.

If your machine is a little loose, you will run into problems when you come into corners and change cut direction. Any significant runout of your cutter, you will need to reduce the feed rate. Significant at this size is like more than 0.0001"...

 

[mhajicek]

First thing to check is runout (should be .0001" or better at that scale). Cutter quality could be an issue, depending on brand; I like Harvey and Redline. For a .035" cutter in Ti it should be three or four flute coated. Make sure your coolant flow is consistent; if it cuts out briefly that can kill the cutter.

 

[nmercier]

I was using a 3 FL Harvey End Mill and was running 75 SFM @ 8000 RPM. Feed per tooth was .00006 with 1.5 ipm. Got all the numbers from Harvey and lowered the SFM to be conservative.

Going to start with checking runout and re-evaluating the toolpath.

 

[Mike RzMachine]

I've used the long reach relieved shank 3 flute harvey endmills down to .015" diameter in 6/4 Ti. 10k rpm (40sfm, max speed on my mill), 0.00005 ipt. It was excruciatingly slow.
Runout at the flutes is key for sure. I tap the 1/8" diameter part of the shank with a small aluminum scrap to get the collet to shift until my runout is better than .0001" measured at the flutes. I also had to use feed optimization to slow down on inside corners to keep the cutter intact as the part had .01" R inside corners.
Are you using some type of adaptive path with the .03" cutter to clear the rest material left by the 0.055" endmill?

 

[nmercier]

Correct I had some small 0.02" radius corners that I needed to clean up. I was getting some burr like finish on the z level as well which is why I had the .055 and 1/8" leave .002" for the .035" end mill to clean up. I've reduced that now and I think that will help but still going to check runout and slow my feed rate down a little more. It doesn't add to much to my operation time.