High Speed Machining??

[Hellbringer]

This is going to sound weird but i will ask...

what makes a machine capable of cutting at high speeds (besides pure godliness) like the HAAS VF-4ss able to cut at 833 IPM.

is it spindle speed?
more torque in the driving motors?
higher hp on the spindle motor?

the reason i ask i am working on plans to build a mill from scratch so i want to know what i should be looking at to get higher IPM.

NOTE: i am not trying for 833IPM that is just a example.... i am looking at more like 100-125ipm.

Thanks
Mike

[LeeWay]

I don't think it's any one answer. Perhaps all the things you mentioned. Rigidity plays a large role as well as does weight or resistance to resonance.

I did build a mill with an 80/20 backbone. It turned out well. I can cut at 300 IPM, but that is if I am only taking something just proud of a polishing cut. I do cut aluminum sometimes at 50 and 60 IPM, but at .04" DOC with the spindle running 6600 RPM and using coolant.
I typically cut CRS at about 15 IPM and 2900 RPM on spindle. .025" DOC. I can cut deeper when I use a vise. I cut steel sheet using a magnetic chuck mostly though.

A lot of things to consider when designing your own, but I'm sure you know that already. I basically had an initial design. The base held true to that, but I redesigned the table and had different iterations of motors and power supplies before I was done. It has become a much nicer machine though since I first got it running.
It will be a journey for you, but for me, it's one I am glad that I took. Knowing the entire machine inside and out generally makes short work of both trouble shooting and repair.

Good luck with it and show us what you are thinking of.

[Andre' B]

Like already stated it is not any one part, it is basically have as much control as you can over everything in the process.

Cutting tools
Tool holders
Spindle RPM, and dynamic stiffness over the entire speed range
The machine slides
Servos and drives
The controller that is telling those drives were to go
The CAM software that is creating the tool paths
etc.

Here is an example of what I consider high speed machining, even though the fastest feed rate is 100 ipm. But it is very precise control of a dynamic process.

YouTube- Seal Mold Cavity Machining

YouTube- Seal Mold Cavity Machining

[LeeWay]

That is what I call just proud of a polish cut.

My machine will cut like that. No problem.

[yantra3d]

Where the heck are the chips??!?! It looks like the ball end cutter is removing the metal by magic! If that airline is blowing them out of the way I sure don't see it.

[Andre' B]

In some of the closeups you can see a few chips sticking here and there.
In that type of milling the chips are small and the speed of the cutter and the air blast move them out of the way fast.

Getting the chips out and away from the cutter is very important. When cutting hard steels recuting chips is instant death for the cutting edges.

[BobWarfield]

Turns out you can go a lot faster than you'd think, depending on your depth of cut and the materials your talking about. 100 IPM is nothing, really, though 833 IPM is pretty radical, LOL.

Let's consider what it takes to run a 1/2" endmill through aluminum 6061 at 100 IPM. We won't cheat and use a ball end (the ball shape means the effective diameter is smaller if you are less than half the tool diameter into the cut). Let's take a 1/2" 3 flute, on a mill that can do up to 6000 rpm (yes, many can't, but a lot of knee mills can). Let's even make it hard and use an HSS endmill instead of a fancy carbide.

Further, let's put aside slotting, because you have to slow down there. Instead, let's pocket. How fast can you go?

Well, if you cut 15 thousandths depth of cut with the tool 1/2" down in the pocket, that's 170 IPM right there with a chipload of 0.0032. Those numbers came out of my G-Wizard feeds and speeds calculator.

Whoa, there! How can that be? The usual chipload math says you can only go maybe 30 IPM for that cut, and that's what most people would do.

But it turns out you are really babying the cutter because of a phenomenon called radial chip thinning, and that's why I say you can go faster than you'd think. Any time you cut less than half the diameter of the cutter, and here we are cutting only 3% of the diameter, you can speed up. G-Wizard builds that math in.

How deep can you cut and still go 100 IPM? About 40 thousandths. And that cut is taking 0.4 HP, so it isn't crushing the machine and setup from a rigidity standpoint. I do cuts like that all day long with my RF-45 mill, for example.

If you want to learn more about radial chip thinning, I have an article here:

http://www.cnccookbook.com/CCChipThinning.htm

BTW, it is a technique out of the High Speed Machining world, even though we're using it on relatively low tech machines.

Now there are some considerations here when you're cruising along at 100 IPM. Probably the biggest is going to be clearing the chips. You'd better have at least a misting system or strong air blast, because they'll pile up in a hurry otherwise!

There are also crazy things you can do with the toolpath to be able to cut a lot faster than you'd think. Check out Surfcam to see some examples. Also, make sure you understand all the math (or use a tool to help you) before you just "go for the gusto." You'll have a lot of pain if you just slap in an endmill, plunge at 100 IPM to 1/2", and start cutting a slot at 100 IPM. You can only speed up once you've created some clearance. Works da bomb when helical milling a hole if you take out the center with a twist drill, for example.

Cheers,

BW

[LeeWay]

Things I cut all the time, I already have worked out to get the best tool life and quality of cut. On the mag chuck, what kills the end mills mainly is recutting chips. Most get magnetized right there. This is why I go fairly slow now. I used to go quite a bit faster, but end mills didn't last as long. I can get 10 to 15 parts with one end mill. I have been buying the Hss double end 3/16" from Enco when on sale.
10 of those were $39.50. That is 20 cutters. That lasts quite a while for me.

I like the feature in Mach that lets you bump up or down both spindle RPM and feedrate. That lets you program new stuff and bump the speeds accordingly. Very handy.