Quote:
Originally Posted by techhelpbb
So you are basing this on the VMC (Vertical Milling Center) not being able to obtain those high spindle speeds in general?
What if they are using a standard shop router(19kRPM - 25kRPM) or a RotoZip (15k-30kRPM) for a spindle on a homemade gantry?
Course the price they pay is not just for the coating it's also that they will need a high feed rate.
A high feed rate most smaller steppers would have difficulty achieving.
I agree with you if you slow down the spindle and operate more in the range of 8k-12k TiAlN is the wrong coating to use.
Without knowing what sort of machines each team is trying to use it gets a bit more involved.
|
There are plenty of different coatings available if you look through a major supplier catalog. All different geometries and designs for different materials, as well as several different coatings. For aluminum - regardless of machine, TiAlN is a bad choice. The aluminum will have an affinity for the Al in the coating and will gum up. For aluminum geometry you generally want a high helix angle to help chip evacuation, a large gullet to allow plenty of space for the chips to eject, and a sharp cutting edge. Coatings that work well in aluminum are ZrN, TiB2, and TiCN. Uncoated works perfectly fine as well. Generally they make the surface harder and smoother to prevent the chips from welding to the surface of the tool. With aluminum coolant is normally used to help eject chips, add some lubricity, and keep chips from welding to the surface of the tool.
For a router in particular - the best option is using a carbide single flute tool. Carbide can run high SFPM numbers in aluminum, so that way if your router is 8-10K minimum speed you won't be burning up the tool. Single flute does two things well. Firstly, it gives a ton of room for the chips to evacuate so that they don't pack up in the gullets of the end mill and cause the tool to load up with aluminum, stop cutting, and snap. The second is derived directly from the speed and feed formulae. Say each tooth needs to be taking 0.002" per revolution so that it doesn't start "rubbing" as opposed to cutting. If you have one flute, that means you're only moving 0.002" per revolution of the tool. If you have a 4 flute tool, each tooth needs to take a 0.002" bite, so you have to move 0.008" per revolution of the tool to maintain proper chip load. On a router that can be the difference between a manageable feed rate, and something that the machine cannot achieve.
For example - you have a router that can vary from 10K to 20K RPM and you're using a 1/4" end mill to slot.
I would use a single flute uncoated carbide end mill. Depending on the specific tool, SPFM in 6061 can be anywhere from 800 to 2000 SFPM. You can run slower, but running fast will wear the tool prematurely. A 1/4" tool running 800 SFPM is 12,200 RPM. Perfect, right in the range for our router spindle. Now finding the feed rate is just (spindle speed * # of flutes * chip load). Say we're being conservative and taking 0.002"/tooth. That means our feed rate is only 24 inches/min. Any machine on the planet can do that without worrying about acceleration in curves, angle changes, etc. If we want to go faster, we can bump up to 20k on the spindle (~1300 SPFM, likely fine for carbide), and the feed rate jumps up to 40 inches/minute. Perfectly achievable numbers, the tool isn't going to burn up or rub, and we have a ton of room for chips to jump out (only one flute!).
If you like 1/8" end mills, then you can run 24 IPM at 12,200 RPM (0.002"/tooth and only 400 SFPM), or 40 IPM at 20k RPM (0.002"/tooth and 650 SPFM).
Using a two flute cutter doubles those feed rates while keeping the spindle speed the same. Three flute triples, and so on. But now you have increasingly little room for the chips to evacuate, especially with a smaller 1/8" end mill. Your previously reasonable 25-40 IPM feed is now up to 100-160 IPM on a 4 flute tool, and you'll need to be taking a shallower cut if you run out of HP in your spindle.
As for the first part - TiAlN is perfect if the situation is correct. Here's Niagara's chart:
http://www.niagaracutter.com/techinf...d_solcarb.html
Say we're cutting 300-series stainless (over 32 rockwell C). We would probably want to be using an air blast to clear chips, and let the coating do the work. We need to coating to heat up to work properly, so here we don't want to be under the recommended SFPM numbers.
So say a 3/8" 4 flute end mill - chart reads 100-150 SFPM and 0.001"/tooth. TiAlN coating adds 60-100% increase in SFPM. So we're somewhere between 160 and 300 SPFM. Let's use the high end - that gives us all of 3,000 RPM and 12 inches/minute. That's why most big VMC's don't really need insane spindle speeds unless they're running aluminum, copper, brass, etc. Even with the coatings, most jobs in steel, stainless, titanium, etc aren't going to going that fast. After that you'll have to start reading about HSM and radial chip thinning, etc, but that's way beyond the scope of this.