Slotting Saw Question - Feed and Speed

Hi,

I have a Tormach 1100 and just got the 1/2" saw arbor for slotting saws. I am using a 2" diameter, 1/16 thick blade. I am brand new to these types of cutters so hopefully someone can help me.

The following is for 6061 Aluminum.

I spoke with Tormach and they provided a RPM of 2400 and feedrate of 2 IPM with a DOC of .050. This results in a very slow cut.

With that, I have to run 3 slots on a 4 1/2" cylinder (6061) with a final depth of 0.22855" and height of 0.125". This results in ~10 passes for one slot (5x at 1/16 height and 5x at final 1/8 height).

Can I run this thing any faster? I saw some calculations which resulted in a very low RPM and a higher feed rate (180-200RPM and 5.6IPM) but this sounds like it could get immediately caught up and break in the aluminum.

Any advice is greatly appreciated!
Thanks

I would be finding out the power curve for the motor on your mill. Try and run the cutter at the best RPM for ur machine. If that mill is at least as sturdy as a Bridgeport I'd burry that saw at full depth at .0007 CPT.

RPM is a bit slow, I'd be at 3000 rpm or so, but full depth of cut and about .0005" per tooth feed rate. So if your saw is 40 tooth it would be 40x .0005=.020 per revolution, .020x3000=60ipm. That might be a tad aggressive, but not by much.

I do a 4" saw, 1/16" wide, to a depth of over 1" at 35ipm and 1200 rpm and that's baby-ing it. If you need .125 wide, why aren't you using a .125 wide saw? They don't like side cutting to widen a slot, best to use the proper width.

If there is a chance of the material moving or distorting, ensure that it can't. At that speed when one of those suckers explodes it might be exciting. I've burst a few 150/200mm ones at a couple of hundred RPM's because the material moved and pinched the blade, interesting is one of the words that could be used to describe it....

If you want a faster cut you can also get a larger blade, 2" is a fairly small saw.

I use the saws a lot. They will go harder than your intuition tells you. Rough the final diameter in one pass in the middle of the groove then you can increase the feeds and cut the top and bottom walls. 3 passes to rough, same for finish. Take it easy on the first pass, get the chips out of the groove so the cutter isn't loading on chips. The final feeds/speeds will depend on your machine, but I would ease off on the rpm, try about 750 to 1000 to start. Start by increasing your depth of cut and use your common sense to tell you whether you can do more. Ramp the cutter in helps a lot as well when starting the cut verses a plunge cut.