High speed machining?

Jake2465

Jake2465

Registered
Registered
Joined
Dec 27, 2017
Messages
340
I have been watching some of these guys on YouTube using their high dollar mills to machine things. I commonly see where they like to turn a real high RPM and then take the width of cut down considerably while having a full depth of cut. I am not sure if this is what people refer to as "High Efficiency Machining" or not. Part of me wonders if there is really that much of an advantage to machining that way or not. The mill has to perform tons of movements to complete it's too path. I thought "Hey, why not just drop the RPM down to something reasonable and just increase the width of cut instead of trying to make the mill run like a CNC router with a 20,000 rpm spindle?".
 
It is "High Efficiency Machining".

When cutting you generally have to make a choice between having a high WOC with a low DOC or a high DOC with a low WOC. End mills don't really like to have both a high DOC and WOC. One issue is that with a high WOC and low DOC all of the heat from cutting is put into a very small area of the tool, which will quickly dull and get ruined. You'll have to throw that tool out while 90% of it has never been used. With high DOC/low WOC you are using much more of the flutes and your heat gets spread much more evenly.
 
Right, so the advantage would be longer tool life.

So, in having a high DOC and WOC, would the end mill get too much deflection issues? I guess I am viewing it in terms of metal removal rates. If I have a mill that turns 10,000 rpm and runs a .050 WOC and manages to clear, let's say, 6ci/min, and then I take that same mill and drop it's rpm down to 5000rpm, cut the feed speed in half and increase the WOC to .100, then wouldn't the end result be pretty close to the 10,000 rpm setup?
 
Just remember that flood coolant is usually used at these high rates.
I run some high speed mills at 60k rpm. The bits are tiny at 0.012 and 0.020”. Moves are at 30-40 ipm. For cooling I use air blast for that and chip removal. The other machines all use flood coolant and they do cut fast!
 
Jake2465 said:
I have been watching some of these guys on YouTube using their high dollar mills to machine things. I commonly see where they like to turn a real high RPM and then take the width of cut down considerably while having a full depth of cut. I am not sure if this is what people refer to as "High Efficiency Machining" or not. Part of me wonders if there is really that much of an advantage to machining that way or not. The mill has to perform tons of movements to complete it's too path. I thought "Hey, why not just drop the RPM down to something reasonable and just increase the width of cut instead of trying to make the mill run like a CNC router with a 20,000 rpm spindle?".
Click to expand...
As Footpetaljones states it is high efficiency machining, commonly known as trochoidal or adaptive clearance machining. There are very significant advantages to this machining strategy as opposed to more traditional methods. Higher metal removal rates can be achieved. Lower cutting forces on the tool, spindle and machine. Far better tool life, less vibration etc. It is something worth exploring on lighter weight hobby CNC's where rigidity and stability is an issue, though on a small Chinese router anything more than a couple of mm's DOC on aluminium will have the machine bouncing and vibrating too much. A small width of cut in aluminium, about 12% of cutter width on 1/8" did (4mm) could work with up to 2 mm DOC on a 4mm cutter. Feed rates up to 300mm+ may be possible.
 
I just recently started experimenting with near full depth of cut moves with my mill. I am interested to see how much longer the tools will last.
 
I have done it just this week, high DOC and LWC works much better. Less vibration occurred as well.
 
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.

20180327_221727.jpg

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.
 
Jake2465 said:
I have been watching some of these guys on YouTube using their high dollar mills to machine things. I commonly see where they like to turn a real high RPM and then take the width of cut down considerably while having a full depth of cut. I am not sure if this is what people refer to as "High Efficiency Machining" or not. Part of me wonders if there is really that much of an advantage to machining that way or not. The mill has to perform tons of movements to complete it's too path. I thought "Hey, why not just drop the RPM down to something reasonable and just increase the width of cut instead of trying to make the mill run like a CNC router with a 20,000 rpm spindle?".
Click to expand...

Jake, my son is trying to figure this out. In 6061, his target is 200 IPM using 3/8 cutters, 1 to 1.5 D DOC. Right now he's running up to 2 D DOC at around 90 IPM and 15% to 40% stepover it's doing quite well. Maxing out the spindle at 6K RPM The goal is to maximize the material removal rate, and still leave an acceptable finish. He will be doing comparisons between different cutting strategies and tooling to try to determine the most efficient method. He'll be working with the Fusion 360 development team and tooling vendors to incorporate his findings. Oh, and doing this while making money with the machine ;)

Going to be an interesting ride. :)
 
You must log in or register to reply here.
Back
Top