Machining hard steel

Nathan the Machinist

Nathan the Machinist

KnifeMaker / Machinist / Evil Genius
Moderator
Knifemaker / Craftsman / Service Provider
Joined
Feb 13, 2007
Messages
19,152
The topic comes up, from time to time, about cutting hard steel. My default answer is," Appropriate carbide cutter, rigid setup to prevent chatter, suitable speeds and feeds for the cutter size and material, blah, blah, blah..."

I've been meaning to post an example for a while. Here is a dull Nicholson file I'm going to put in a 1/4" hole.

http://nathan.broadtime.com/hard1.JPG
hard1.JPG


I'm lining my vise jaws with aluminum because the file is harder than the jaws.

I'm using a coated carbide cutter without coolant. The mill has flood coolant and in this application it wouldn't hurt to use it, but when using carbide with certain coatings in hard steel it is often advantageous to run dry. Prevents coolant shock to the cutter.

http://nathan.broadtime.com/hard2.JPG
hard2.JPG


You'll notice the cutter is undamaged and the old file has a perfect, near mirror finished hole in it.

http://nathan.broadtime.com/hard3.JPG
hard3.JPG


Here is the data:

Full hard Nicholson file, probably around 66 HRC

4 mm carbide two flute cutter (4 flute is usually better for this, but can be more prone to squeal plunging in the hard stuff)

50 Surface Feet per Minute (SFM) spindle speed, which works out to 1,216 RPM for the .157" cutter (please note folks, running at a very slow RPM, like 300RPM, isn't helpful)

.001 chip load per tooth (because it is a small cutter in hard metal), which at this RPM works out to a glacial 2.4 inch per minute feed rate.

Helical plunge with .005" infeed per rotation, which required 50 turns through the 1/4" file.

Cycle time, six minutes (because of the small infeed and very slow feed rate, could certainly be improved some)

Beer consumed: None, it is still pretty early on a Sunday.


What is the moral to this story?

A: With proper speeds and feeds and a reasonable setup, you can cut hard steel without messing up cutters.

B: I have a job I'm supposed to be working on this morning, but I'm procrastinating.
 
I would have thought you'd use coolant. How hot did the cutter get ?
 
mete said:
I would have thought you'd use coolant. How hot did the cutter get ?
Click to expand...

I would guess probably in the neighborhood of 300-500 degrees, possibly closer to 1000 at the cutting edges. That cutter is TiAlN coated, and is designed to run dry in this application. Running coolant would actually go counter to the manufacturer's recommendations due to thermal shock.

The area around the cut felt cool to the touch immediately after machining and there is no heat discoloration on the file. 50 SFM is pretty slow.

It is becoming more common place to see this in highspeed hardmilling:

DrillSparks150.jpg


It is funny, but when I was starting out (which wasn't that long ago really) that sort of thing meant impending disaster (and possibly "industrial accident"). Now it is supposed to look like that....

I remember once having a discussion with my boss (at the time) who was not a hack machinist, but was a proper old school journeyman machinist with papers from the 60's. He had been out of it a while and was struck slack jawed the first time he saw modern carbide lathe tooling glowing red during a cut. They didn't do that in his day...
 
Thank you for the how to. Nice to know how the pros do it. Question. The chip load is the amount of metal remover by each tooth per revolution or what. Also. your saying when running carbide to run way faster than cobalt and HSS? Thanks Jim
 
ib2v4u said:
Thank you for the how to. Nice to know how the pros do it. Question. The chip load is the amount of metal remover by each tooth per revolution or what. Also. your saying when running carbide to run way faster than cobalt and HSS? Thanks Jim
Click to expand...


Yes and yes.

And in this application, you'd have to use carbide. Not because of its high speed or high heat tolerance, but simply because HSS or cobalt/HSS are no harder than the file.
 
Thats awesome nathan, thanks for posting it. Did you use a steady feed or was the cutter pecking its way through?

Is there any possibility you could show us how you would mill a 1/8" slot for a guard in some 1/4" stainless? I've tried numerous times and always end up with a broken end mill or carbide cutter ($$$), so I gave up and just design knives with bolsters instead.

Brad
www.Andersonknives.ca
 
Teknition said:
Thats awesome nathan, thanks for posting it. Did you use a steady feed or was the cutter pecking its way through?

Is there any possibility you could show us how you would mill a 1/8" slot for a guard in some 1/4" stainless? I've tried numerous times and always end up with a broken end mill or carbide cutter ($$$), so I gave up and just design knives with bolsters instead.

Brad
www.Andersonknives.ca
Click to expand...


The cutter isn't being used as a drill here. Notice the hole is almost twice as big as the bit. I'm machining in a helix, which can be done on a manual machine using powerfeed on the spindle and a rotary table. I'm using CNC here, which helps keep the beer hand free. Endmills don't plunge well and tend to wobble (and chip) when used as a drill.

If you're putting a 1/8" slot in 1/4" stainless, try this:

Drill a 3/32 hole at both ends of the cut so your cutter is plunging mostly in air. Use a 3/32" four flute end mill. Run your spindle around 1500 RPM with HSS, or 2500 RPM with carbide. Plunge .015" Depth Of Cut (DOC) and feed around 10 IPM with HSS, 15 with carbide. Rinse and repeat. Eventually you will have your slot roughed out. You can finish your slot by moving your table over about .015" in the Y axis on one side, then the other. Or you can put in an 1/8" endmill. You can take a deeper depth of cut for your finishing cuts, perhaps .030 per pass, because they're not removing much material. If necessary, reduce RPM (and feed proportionally) to eliminate chatter. These are conservative starting points for someone using a small machine.

Never try to slot all in one pass.

Remember to avoid dwelling in your cut when machining stainless. It work hardens when you do, which makes it a dog sometimes.
 
I forgot to mention. When slotting, it helps to lock any axis not being used. If you're cutting in X, lock Y and Z etc.

When you step over in Y, lift from the cut first and do it in air.

Use a coolant of some kind. I use water soluble cutting oil. WD40 works in a pinch.

Edit to add:

Good advice on a smaller machine is to never try to take it all off in one pass. And generally speaking, you always want to leave some rough stock allowance for finishing cuts.

It took six minutes to make a 1/4" hole in that file, essentially I shaved it off .005" per pass (that was the helix pitch).

Don't confuse that with going slow. It is important to maintain adequate cutter engagement. I maintained .001" feed per tooth at all times (more actually, when you consider that is centerline feedrate, not the feedrate out at the actual cut). Remember, steel is a surprisingly elastic material for its strength. If your cutter isn't fed enough the steel deflects and doesn't cut, which can lead to smearing, chatter and work hardening.

You can address machine stiffness issues and unfavorable cutter length to diameter ratios by taking lighter cuts, meaning not as deep in the Z axis (spindle axis).
 
Last edited:
That's an awesome demo of what a REAL mill can do. I don't see myself mastering that on my mini-mill. Hell, I'm lucky to mill annealed steel :D Thanks for all of you input Nathan!
 
where were you last week when i was doing a 1/4 slot in some 01. could have used your help.........
 
You must log in or register to reply here.
Back
Top