High speed machining?

JimDawson said:
In 6061, his target is 200 IPM using 3/8 cutters
Click to expand...

HSM Advisor gives me some interesting numbers with that target. If you could get 8kRPM, then the following parameters gets the MRR north of 6cu/in:
2hp spindle; 3/8" 3FL ZrN coated, .750 flute length; .625" DOC & 15% WOC, 8kRPM, .005" IPT (.0075IPT w/chip thinning) at 180IPM feed.

That's at 95% spindle load (reported). Limited to 6kRPM means giant IPT setting (like 0.008") that - I suspect - would leave a less than awesome surface finish.

Mucho interested in results!
 
We're about to find out what that new Haas will really do. :grin:
 
This week I plan to order some Alu-Power three flute end mills in the 3/8" and 1/2" diameters. I am finding that my nice rigid 4 flute end mills don't really like to do helical ramps over 3 deg in aluminum or anywhere there could be chip evacuation issues. Despite what people have told me about those 4 flute end mills, I have good success with clearing aluminum using them as long as I use plenty of water with my spray mist.

Lake Shore Carbide sells their TAS "The Aluminum Shredder" three flute end mills. I saw NYC-CNC take a 24deg helical ramp angle with that end mill and survive. They are a fair bit pricey though. http://www.lakeshorecarbide.com/tasrougher.aspx.

The way I currently run my end mills, I am only taking a .002' chip load at 24ipm and 3000rpm. But, with the planned spindle motor upgrade I imagine I could triple that chip load in aluminum and the 30 taper tooling should be able to keep up. So, I could keep the rpm the same and dial the feed up to 72IPM (for aluminum use). That would be pretty smoking fast for a 1980's knee mill :D.

That HAAS is on a completely different level. You should be able to get that thing to scary fast removal rates. Like, where the shop lights dim somewhat during the passes :grin:.
 
spumco said:
Jake - remember that regardless of your toolpath strategy, the tool RPM is generally set by tool diameter, tool material, coating, and material. Full slotting or 10% WOC adaptive - pretty much the same RPM. What changes is the WOC and DOC and feed rate based on appropriate chip thickness.

I love using HEM/HSM/Adaptive (whatever it's called). Tool life goes up, no squealing in corners, and the chip load is predictable given the right CAM software. I can clear faster this way with smaller tools as my mill is not rigid enough to take advantage of bigger (3/4") end mills due to tool side pressure. The only reason I use end mills larger then 1/2" now is for rigidity. 3/8"& 1/4" are my go-to sizes.

You can also get away with slightly less secure workholding and not fling the part since the tool will never get 'buried'. Example - I (adaptive) profiled a 4140 block using 3/8" & 1/4" roughers at 1/2" DOC and .0375"/0.025" WOC using nothing but painters tape and superglue to hold it down. Running about .0025" IPT and 400SFM + flood coolant. No way I could have pulled this off without the constant tool pressure adaptive clearing provides.

View attachment 266321

However - it is not a finishing strategy. It will leave tool marks on sidewalls and odd patterns on the floor that need a cleanup pass.

And I just tried Fusion 360's new 'both-ways' adaptive clearing today. This cuts in both directions (climb & conventional) while still keeping a constant chip load. Think back and forth arcs instead of a climb arc with a straight move back to the other side for another cut. This shaved a ton of time off a narrow pocket clearing Op and worked like magic. And the parameters for the conventional moves are editable independently from the climb passes.

Don't know how well it works for materials that don't respond well to conventional milling, but it was the bee's knees for Delrin.
Click to expand...

I also just finished trying out that both ways feature. I think they preset it to something like 80% feed rate of the climbing passes as a default for the conventional milling return pass. I had just a normal rectangular clearing pocket adaptive path and It went from 7:02 to 5:33! That was really cool to watch.

My biggest issue with my mill is that the spindle is HP limited. So, whenever I have become impatient and wanted ramp up the feed rates, I can near my spindle speed start to complain. It's a shame because the iron can handle the loads, but the spindle motor does not like it.
 
Jake2465 said:
My biggest issue with my mill is that the spindle is HP limited
Click to expand...

How many amps do you have available in your shop? 'Cause the brain trust here can probably set you up with an upgraded spindle motor...:)

The other thing to consider is if you're after max MRR, look at the spindle motor torque curve and figure out what the max RPM at max torque is. Use that speed in your F&S calculator as a target and you can take bigger chunks per tooth. As I've mentioned elsewhere on the forum, My motor & spindle can do about 7400RPM without blowing up. However, I need to keep it to around 5500RPM if I'm hogging as the torque drops off after that.

Now that you mention spindle motors, I'm considering switching my 2hp Blackmax + VFD for a big servo - mostly to cut down on the weight the Z-axis has to lift. A 35lb diet would help my ballscrew live a happier life, and I could increase the acceleration. Peck drilling would look like a sewing machine at full boogie.
 
Last edited:
spumco said:
How many amps do you have available in your shop? 'Cause the brain trust here can probably set you up with an upgraded spindle motor...:)

The other thing to consider is if you're after max MRR, look at the spindle motor torque curve and figure out what the max RPM at max torque is. Use that speed in your F&S calculator as a target and you can take bigger chunks per tooth. As I've mentioned elsewhere on the forum, My motor & spindle can do about 7400RPM without blowing up. However, I need to keep it to around 5500RPM if I'm hogging as the torque drops off after that.

Now that you mention spindle motors, I'm considering switching my 2hp Blackmax + VFD for a big servo - mostly to cut down on the weight the Z-axis has to lift. A 35lb diet would help my ballscrew live a happier life, and I could increase the acceleration. Peck drilling would look like a sewing machine at full boogie.
Click to expand...

I can probably run 5hp without a problem in my shop. So, probably around 17 amps at 220V. I have one of those R2E3 mills that has the odd motor configuration where the spindle motor is between the Varispeed belt compartment and the solid ram. I took measurements the other day and it would basically need a short, fat motor to replace what's already in there. I thought it would actually be cheaper to make a motor relocation bracket and a idler shaft to put a more common Baldor Super-E motor in it's place.

I checked the voltage and amperage figures off of the data plate of my mill spindle motor, and it's really not 2hp but more like 1.6hp. So, by the time the power gets to the end mill, I imagine I have something like 1.4hp at the tool and perhaps 1.2hp useable without bogging down the motor to the point where it wants to stall.

Here is my mill. I hear it's a fairly common machine, but I have not really seen any of them around my town. Everyone else just had the regular J head Bridgeport's.

I do plan to run a VFD, so I would need a inverter friendly motor for it. That way I can ditch the Varispeed so I can run a little higher RPM's for the small tools.

mill.jpg
 
Last edited:
You guys and your fancy high speed VMCs :D Funny I was just thinking about the high speed cutting rates because by comparison I'm going so slow that it's kinda crazy to think how fast some of the big machines really go. I run 1800rpm (2500 capable) and usually around 7-9ipm for roughing endmills/flycutter etc and 5 or so for finishing end mills. DOC is usually about the diameter of the cutter. WOC for slotting you don't have a choice, it's the full width of the cutter but for step-over in the case of pocketing etc yes I plan to use adaptive primarily to extend the life of the tool especially around the corners. However, adaptive clearing does cut air and if you don't have high rapids and feed rates you could extend the machine time quite a bit- which as a hobbyist doesn't matter to me all that much.
 
I do that too! especially when the flycutter starts doing its thing. I like your enclosure, I actually just built some shields this weekend for mine to contain the chips from flying all over the garage.
 
You must log in or register to reply here.
Back
Top