Tormach with Sprutcam - DOC and Speed?

[MarkWink]

Just got a Tormach with Sprutcam 2007

What depth of cut and feed rate are you guys running in Aluminum?

Any quirks or things to look out for running the machine?

Does anyone run Mach3 (not the Tormach version)?

Thanks,
Mark

[mayhugh1]

Buy a copy of ME Consultant Pro. I've found that its recommendations for feeds and speeds as a function of hp, tool diameter, depth and width of cut, for aluminum are very compatible with the Tormach. As a rule I keep the hp loading under half of what the machine is capable since I'm usually not in a hurry, it's easier on the machine, and I use a Micro-Drop cooling system instead of flood cooling. With flood cooling, I think I'd go up to 3/4 of it rated load using 3/8" and 1/2" cutters. I found the same true for mild steel. Only time I found the program's recommendations to be a bit too aggresive was with 316 stainless and even though I was using carbide I had to back the feed and speeds down to those it was recommending for use with HSS. I also use it for drilling and although it's recommendations seem a bit aggressive at times. they have always worked OK for me. -Terry

[MarkWink]

mayhugh1,

Thanks,

I've been "playing" with an CNC'd X2 for awhile and the Tormach is a big change.

I have quite a few texts on Feed and Speed/DOC, although they are dependent other factors as you metioned (coolant, matrl...)

I was looking for a real world quote i.e. '...my cuts Al with 0.25 dia @ 0.0001 @ 1 IPM and it really cooks bits with flood on'

Like you, I'm in no hurry. I was wondering what the "real" expectation of this machine are.

Thanks
Mark

[mayhugh1]

Well, in that case then I can say I'll typically machine a large aluminum part using a 1/2" inch 2 flute carbide cutter running a trochoidal toolpath at .25" depth of cut, 3000 rpm, 20 ipm, and WD-40 in the Micro-drop dispenser running rather wet. The machine is throwing a rooster tail of big chips but is still running at about half its max load. If I were running flood coolant, the trochoidal path probably wouldn't be necessary but things can get interesting in aluminum with a deep slot with no place for the chips to go especially when the toolpath suddenly makes a 90 degree turn- Terry

[Mickey_D]

OK, not running a Tormach right now, but still using sprut on a sharp and hurco. for aluminum I use either 2 or 3 flute carbide, depth is about 2/3rd with endmill diameter, and about a 75% stepover. For feed rate, I try to go .003 per flute for a half inch endmill (about 40 ipm for a 3 flute half inch em running at 4500 rpm). Cut your feed rate for smaller endmills so you don't break them, and I usually tune my feeds by looking at the finish and listening to how the machine sounds. Also, when you have a little more experience and have gotten through the brain fart endmill breaking stage, don't be afraid to buy good carbide endmills from people like lakeshore carbide, kennametal, and the like instead of what is on sale at enco. For bang for the buck, the higher quality tooling is worth it.

[redrider9112002]

I'm a fan of 4 flute end mills. For roughing, I use a .375 4 flute rougher @ .500 DOC ( it works at any depth) full cut @ 4500 rpm @ 18 ipm. For finish (profiling) I'll take 0.010 off the side @ 3750 rpm @ 27 ipm @ any depth. I use flood coolant, and it sound normal. I find that 0.500 end mills on the tormach to be to rough. 3/8 is great. I work in the machining industry full time as a Quality Inspector, so I look at parts all day. I use to be a cnc mill operator. To me the tormach is a great machine for the money. You can do quality cuts on it if you take your time and just pay attention. Andrew

[pzzamakr1980]

I was just running a pocketing and slotting run on my x3 with my spindle running at just over 6000 rpm. I was using a 1/4in 3 flute carbide endmill, the DOC was .075 per pass, and the feedrate was set to max at 25 ipm. I say max because the pocket was small, about .52 diameter, as were the slots, witdth of .32 and length of 1.25 inches. The material was 6061 aluminum. No coolant. The finish was amazing, even without coolant, and the cutter went through that metal like butter. This was a very short run. Only 4 pockets and 2 slots.
Previously I had been using a cheap 3 flute hss chinese endmill. The finish was dooodooo, even with heavy mist coolant, and they clogged and broke constantly. Even with slow feedrates. I experimented with 2 flute for aluminum, which was nice, but the three flutes designed for aluminum just work amazing. The finish is bright and shiny and smooth as butter. I use jw schultz tools. Really reasonable.