# Is It Possible To Face Mill Hardened 4140?



## Cody Killgore (Mar 30, 2015)

Hey guys,

I'm wanting to face mill the end of a piece of 5" square 4140. It is sitting at 55 HRC. Is this possible and, if so, what tool would you guys recommend?

Cody


----------



## JimDawson (Mar 30, 2015)

It kind of depends on how much material you need to remove and maybe more importantly how big is your machine.  If you have a benchtop mill then a 3/8 solid carbide endmill would probably do it.  Maybe a small insert type face mill or flycutter with a carbide bit run at low speed would work.  Reasonably high feed rates and slow spindle speed would be in in order, don't let it work harden.  If you have a heaver machine, then a larger cutter would work.

In either case, be prepared to destroy a cutter or two.


----------



## Wreck™Wreck (Mar 30, 2015)

Cody Killgore said:


> Hey guys,
> 
> I'm wanting to face mill the end of a piece of 5" square 4140. It is sitting at 55 HRC. Is this possible and, if so, what tool would you guys recommend?
> 
> Cody



Yes, you will not like the cost of the ceramic inserts however, if the rigidity of the machine is questionable all bets are off.

Do a google search for hard machining, it mostly applies to turning however, I do a 50 peice lathe part every month or so, material is RC 45-50, NO COOLANT, the finish is exceptional and holds dimension very well. It sparks a good deal and the chips are glowing a dull red when they drop.


----------



## Cody Killgore (Mar 30, 2015)

My mill is an Enco 100-1525. It is a "knee" style mill so it is heavier than the benchtop types. I want to take off about 0.035"


----------



## chips&more (Mar 30, 2015)

55RC is pretty darn hard. Does a file just zing across it or does the file dig in at all? I would grind it. Maybe even go as far as to set-up a grinding cup wheel on your mill. Wrap every part of your mill to keep out the grinding swarf/crap and try it that way…Good Luck, Dave.


----------



## Wreck™Wreck (Mar 30, 2015)

Cody Killgore said:


> My mill is an Enco 100-1525. It is a "knee" style mill so it is heavier than the benchtop types. I want to take off about 0.035"


I would not try that with a facemill, but it may work well, have never done it that way, I would try a milti-insert face mill with only one insert installed which is a fly cutter.
If .035" is all that needs to come off buy a cheap fly cutter and one or two brazed carbide tools, knock .005" off at a time, grind tool and repeat, when you get down to ,005" or so left sneak up on it.002" at a time, grind tool again and take a slow finish cut .001" big. It won't work harden because it is already hard. This should result in an excellent finish.
Do not grind the tool sharp at the point, put a bit of flat on it.
Good Luck


----------



## randyc (Mar 30, 2015)

Hi Cody, no offense but are you sure that it's at Rc 55 ?  (If it is _pre-hardened_ _4140_ hardness, it's usually considerably lower than that.)


----------



## Cody Killgore (Mar 30, 2015)

Thanks for all the tips guys! I think I may try a fly cutter and see how it goes from there.



randyc said:


> Hi Cody, no offense but are you sure that it's at Rc 55 ?  (If it is _pre-hardened_ _4140_ hardness, it's usually considerably lower than that.)


I had it professionally heat treated. They tested it after heat treat at HRC 55.


----------



## JimDawson (Mar 30, 2015)

The one tool that nobody has mentioned yet is a surface grinder.  It would take off 0.035 off in a few minutes.


----------



## randyc (Mar 31, 2015)

Cody Killgore said:


> Thanks for all the tips guys! I think I may try a fly cutter and see how it goes from there.
> 
> I had it professionally heat treated. They tested it after heat treat at HRC 55.



Sounds good   Let us know how the flycutter works - I'd be wondering if all that pounding would chip the carbide.  But might be OK for the small amount you're removing.  I machine hardened O-1 with s_olid carbide end mills_ often with no difficulties - just another alternative.


----------



## G MORSCH (Apr 1, 2015)

Another quick tip....  Fly cutter sounds fine.   And the bigger the insert radius the better.  To reduce chipping, take the widest cut possible because you will minimize entrance shock as well as exit shock.  Zero load at entrance full load at centerline and zero load at exit.  If your cut is smaller than the cutter diameter, use conventional milling to reduce shock at entrance.  This is especially successful with ceramics.  If you are able, use the biggest lead angle possible and place initial impact above the bottom tangent of the insert.  Use .002 chip load on a small radius insert and up to .005 with a 2 or 3 rad.  Depth of cut, do not use more than 30% of the corner radius.  This will allow for some chip thinning.  225 SFM to 250 SFM will do nicely for carbide, run 1,000 SFM for a AL2O3TiC ceramic.   NTK HC2, Kennametal KO90 are good for starters.

Good Luck!
Gary


----------



## Cody Killgore (Apr 2, 2015)

Some really great replies fellas. I do appreciate it.

You know, when I thought about this originally, I was not thinking about how I'm going to hold it to the table. 

Now that I think about it, I have no idea how I'm going to hold it on the table, lol.

So, just to explain a bit further. I bought this piece of steel and had it heat treated about as hard as they could get it so that I could use it as an anvil (I forge knives). Over time, it has acquired quite a few dings. I am wanting to just resurface the top in order to remove the dings that have accumulated. It is 5" square bar that is 12" long (tall). I'm actually not even sure I'll have enough room to fit it under the spindle of the mill - maybe I should go check that.

Ideas?

(don't mind the cup ring, it will get burnt off in short order


----------



## JimDawson (Apr 2, 2015)

Here's how I hold stuff that is too tall.  This is a BIG stepper motor (about the same size as your chunk of steel) that I had to drill the shaft on.  It is clamped to an angle plate that is bolted to the table.


----------



## chips&more (Apr 2, 2015)

OK then, I would get a 4 ½” right angle grinder fitted with a shallow grinding cup wheel. Then jig up the grinder to swing and arc over the top of that anvil. Move the anvil and or grinder to do all of the top. Or some similar idea with a grinding stone fitted to a router. And the router being guided by a reference surface above the anvil..Good Luck, Dave.


----------



## G MORSCH (Apr 2, 2015)

Jim:  I really like your work holding idea above.  I know I will be able to use that some time.

Thanks,  Gary


----------

