What's new
What's new

OT Theory Question: Why No High-Feed For Non-Ferrous

Joined
Nov 2, 2018
I've been really fascinated by the concept of chip-thinning high-feed cutters lately. I've read a lot about them but can't find my own answer- Why does high-feed milling seem to be exclusive to steels and harder? Is it because anything softer is already free-machining enough?
 
I've been really fascinated by the concept of chip-thinning high-feed cutters lately. I've read a lot about them but can't find my own answer- Why does high-feed milling seem to be exclusive to steels and harder? Is it because anything softer is already free-machining enough?

I don't have an official answer but I use feedmills on non ferrous when I need to reach really far or am too lazy to swap out tools since I don't do a lot of non ferrous. My best guess is you can already bury a sharp facemill and cook right along. Also the geometry of feedmills makes the inserts very durable which lends itself to more difficult to machine materials. Which makes me think....they are used all the time for titanium and that is non ferrous....
 
High feed mills insert geometery is designed for non-ferrous materials. Of course you can run them through ferrous materials. But you will have build up on the inserts reducing the inserts effective life. You can cut the same way using a tool that is designed for non-ferrous materials that has a larger radius. The large radius will have the same radial chip thinning effect, and the polished high rake inserts will not build up with the material. All that equals more chips and more money.
Noblemanufacturing.net
 
I've done it a bit, if you use stainless inserts they tend to not gum up as much. the problem I have is my machines aren't fast enough, once you turn the spindle speed up to something like I would want to run in alloy the feed rates are crazy fast.

for 99%of the time it's faster to move slower but at a bigger depth of cut in soft stuff.
 
As far as aluminum, most HF mills can be had with aluminum grade/geometry inserts. I’ve used the same mill (Seco High Feed 6) on 4140PH, and aluminum. Speeds/feeds for aluminum are usually just stupid. I was literally running as fast as the machine would feed, 600IPM. But unless you have some long reach usually a face or end mill can remove stock just as well (or better with a higher DOC). In steel or stainless they are awesome for getting a long reach on a low-rigidity machine. We’ve machined down 4” on a Haas in alloy steel, don’t even try that with an end mill...
 
I should have clarified- When I say non-ferrous I mean ISO N materials (Aloominium specifically) i.e. not ISO S titanium/super alloys, though that is an interesting gotcha. The reason I ask I guess is because I don't ever see manufacturer speeds and feeds for Al or cutters that take polished inserts

High feed mills insert geometery is designed for non-ferrous materials. Of course you can run them through ferrous materials. But you will have build up on the inserts reducing the inserts effective life. You can cut the same way using a tool that is designed for non-ferrous materials that has a larger radius. The large radius will have the same radial chip thinning effect, and the polished high rake inserts will not build up with the material. All that equals more chips and more money.
Noblemanufacturing.net

In your experience (non-ferrous specifically), is that more or less effective than low WoC high DoC tool paths as far as efficiency/MRR?
 
I should have clarified- When I say non-ferrous I mean ISO N materials (Aloominium specifically) i.e. not ISO S titanium/super alloys, though that is an interesting gotcha. The reason I ask I guess is because I don't ever see manufacturer speeds and feeds for Al or cutters that take polished inserts



In your experience (non-ferrous specifically), is that more or less effective than low WoC high DoC tool paths as far as efficiency/MRR?

I think this is the closest you'll get to a high feed cutter for aluminum.

Pro-V Mill | Products | KORLOY

To answer your question about not seeing many (or any) insert tools for milling aluminum is becasue IMO, you can do almost everything with an carbide endmill an inserted cutter would do at a cheaper price.*

* The exception being large diameters and long reach. Solid carbide gets expensive when you 'waste' 2"-3" of it because you need to reach 3.5" in a pocket or something
 
It may be due to the cutting speed needed.
Aluminum is typically run at 3-6 the surface footage of steels and likes higher chipload.
So the cutter that runs 400 IPM in steel needs 1800-3600 IPM feedrates in Al to make a decent chip.
Bob
 
I have an Ingersoll 1" indexable endmill designed for alu. That tool is balanced to 30,000 RPM and can handle .013 ipt (2 flute). (That said, my mill only goes to 8000 RPM which is where I run it.)
That comes out to 780ipm for shouldering with a .25-.35" DOC. A feedmill typically runs from .03-.1 DOC with .03-.14 ipt. So, it would have to run over 5000 ipm just to keep up with the square shoulder tool. I will also say that most tools designed for aluminum have sharp geometries with a wide wiper flat that leaves crazy good surface finishes. A feedmill would also lose there.
Good luck!
 
What Bob said.
You need to use very high spindle speeds when Milling Aluminum. So the high feed (low resistance) Milling cutters aren't being utilized. The high feed Milling cutters are for reduction of required HP. It's irrelevant when working with Aluminum. It's still feeding fast, just not the same context as Milling Steel.

R
 








 
Back
Top