Quote:
Originally Posted by techhelpbb
I did expressely mention that other people were telling me they were having issues with TiAlN in aluminum and they both stated it depends on a lot of factors like the feed rate, the coolant, the rigidity. So your mileage may well differ from mine.
|
"It might work" isn't the same as saying it's a recommended coating. If you call and ask "What tool coating is preferable for machining of aluminum?", they will not respond by saying TiAlN. That's why they don't sell it as a coating on their aluminum specific geometry tools, just uncoated or TiCN. Other companies run coatings designed for Aluminum - ZrN, TiB2, DLC, etc. Niagara and Duramill don't offer those for whatever reason, but SGS, OSG, Havey Tool, Melin, Maritool, Destiny, Lakeshore Carbide, etc, etc all do.
Quote:
Originally Posted by techhelpbb
Well if you try the calculator on the page I linked before:
1,000SFM with an 1/8" mill gets you a spindle RPM of around 30,500 RPM.
With a tooth load of 0.003 and 2 flutes you get: about 183 IPM feed rate.
I have a lot of people I've worked with that only dream about 183 IPM feed rates their systems could not achieve that.
They would be missing steps.
If you increase the diameter to 1/4" you'll get down to about 15k RPM and 91 IPM or so that's more practical for large steppers and closed loop servos.
|
Again, conflating routers and mills here. For routers - use the Onsrud single flute carbide cutters. They solve all of the issues with having high minimum RPM and limited feed rates and acceleration profiles. 1/8" end mill - 20,000 RPM @ 40 IPM. 1/4" end mill - 20,000 RPM @ 60 IPM. Doable on any junky stepper machine.
If the feed is too extreme for the router, just drop the spindle speed. If you're cutting aluminum on a router you should really skip the silly hand routers and buy a model with a VFD controlled spindle anyway. Good uncoated carbide is perfectly happy at 1,000 SFPM and up.
For mills - you're going to be spindle speed limited in aluminum on most cutter sizes, but they're able to maintain higher feeds without issue. Even the Haas TM machines are rated for 400 IPM, and that's still plenty considering the machine size/HP.
Your feeds will be much slower just based on the max RPM for the machine. 1/4" 3 flute end mill - 6000 RPM, 54 IPM @ 0.003"/tooth. 1/2" 3 flute end mill - 6000 RPM, 90 IPM @ 0.005"/tooth. You will probably get higher MRR at lower RPM just because the HP falls off on the Haas machines at higher RPM's anyway.
Quote:
Originally Posted by techhelpbb
|
Not exactly the most reputable site. Find any cutting tool company that recommends TiAlN for aluminum. Find any cutting tool company that sells aluminum specific geometry, and see what coating they put on the tool. It's not TiAlN.