Hi speed milling 6Al-4V titanium? 1

[ncassist]

I have an application to mill 2mm square "windows" thru 1mm thick 6Al-4V titanium. The "windows" require .5mm corner radii, so I plan to use 1mm dia carbide end mills. Quantities are 3,000 parts with 250 "windows" per part. I have CNC spindle speeds available to 30,000 rpm. Does anyone have any suggestions as to how this might be handled? Any thoughts about speeds, feeds, depths of cut, expected tool life etc...

Thanks,
Dave

 

[mrainey]

There may be some specifics about your project that get in the way, but I think I'd look for some other method, perhaps a punch press. The milling approach would, in my opinion, be extremely slow and unreliable.

But:

If you must use an end mill, you'll likely have to pre-drill a start hole in each window. Even if your end mill claims to be center-cutting, I think you'll find it unsatisfactory for that purpose, in terms of tool life. Drills are MUCH better at making holes from the solid than are end mills.

My data suggests a starting speed for the end mill around 100 SFM, which would translate to 9700 RPM for a 1mm tool. Feed of not more than .0001 IPT (and possibly much less) - a two-flute end mill would thus feed at 1.94 IPM.

I think you'd be unlikely to finish even one complete part without catastrophic tool failure.

 

[BobUXL]

I would be careful with high speed machining of Ti alloys. They do have a tendency to catch fire.

 

[TVP]

You might try reviewing some of the links that were provided in the following thread:

thread281-48509

 

[sprintcar]

I'd be talking to the designer about a round hole.....

Can Ti be cut with a water jet?

Keep the wheels on the ground
Bob
showshine@aol.com

 

[richardgb]

I would be using cobalt instead carbide EM, much more forgiving, have milled ti for years and never seen a carbide end mill being used (except to cut out broken cobalt end mills (using high rpm)).

 

[ncassist]

I thought I'd share the results of this project, started 18 months ago. I was fortunate enough to have many chances to try various combinations of speeds, feeds, tools and methods. By far the most reliable was to first pilot drill through with a #2 carbide center drill. Tool life was easily 10,000 "windows" at 100 SFM at .0007/rev feed. Then rough mill with 1/16 4fl carbide em at 100 SFM at .0007/rev feed, then finish mill with 1mm 4fl carbide em at 100 SFM and .001/rev feed. Seemed a bit time consuming, but customer required milled surfaces and the reliability was very predictable as well as the cycle time remaining within the quoted restraints. Rough end mills consistently lasted 600 "windows" and finish end mills lasted 1200 "windows. The reliability allowed us to very effectively keep all equipment running virtually non stop for the entire length of the project.
I did find exceeding 100SFM was nearly impossible.

Dave

 

[TVP]

ncassist,

Thanks for the update on your project. Which company's inserts did you use for this? Coating type? Coolant? It would be nice to have all of this together with your speeds, tool life, etc.

 

[ncassist]

Actually nothing special as far as tooling. I found the cheapest generic tools worked as well as good quality in this application. I tried various coatings (Tin, TiAiN, etc) with no improvement.

Dave

 

[icrman]

Yeah, I usually use 150 SFM for Ti, if you want better cutter life reduce it to 80 to 70%.

 

[russneff]

Are you still making these?

Is EDM an acceptable alternative for these parts?

We used to just machine the electrodes out of graphite and burn a dozen or so screens at a time.
The graphite machines quickly and a whole lot easier than Ti. On our parts the windows .187" x .187" were about .020 apart and grids of 6" x 6" at about 25 degrees.
You might have to do a thinner stack with the smaller windows
Talk to your local EDM job shop. Should be a no-brainer for for them.