What's new
What's new

Face milling 4140 steel - how to get a good finish?

javaduke

Plastic
Joined
Jul 25, 2019
I've been trying to clean up some rough surfaces (to be specific, flats on the 1911 slide) and got a relatively cheap 3" face mill with carbide inserts on Amazon. The reviews were good and everybody was mentioning a mirror finish, but it wasn't my experience, it did cut the metal but produced some very deep tool marks which took me a lot of time to sand off. So I guess I was doing something wrong. I was taking very light passes, maybe .001" deep, moving the table very slow and spinning the mill at 150 RPM and using a lot of cutting oil.
SO what is the right technique to get a decent finish on a 4140 steel? Doesn't have to be mirror shiny, just no deep tool marks.
 
It has been my experience that 4140 machines rather well. I would have to guess there is not enough radius on your inserts or something like that.
 
Use an indicator and mag base to check all of the inserts to make sure they are at the same level. You might have one hanging down lower than the rest. Also, 150 rpm seems a bit slow to me. I'm not sure about 4140, but 4340 tends to tear and smear if you take too light of a cut or too little rpm.

Sent from my SM-N960U using Tapatalk
 
You might try using only one insert, effectively turning your face mill into a fly cutter.
 
In what condition is the 4140... That means everything, though what you were
doing would result in a shitty finish no matter what.. I'm not being that big
of dick.. I'll explain why. Why you will get a shitty finish, not why I'm not
being that big of a dick.

You've already had a bunch of people talk about insert height.. Fly cutters
are shit, but when you *REALLY* need that mirror finish, one insert in a
face mill is hard to beat..

DOC(depth of cut).. A thou, a single tiny itty bitty little thou? If you bought a cheap
facemill, you've probably got more variation than that in the heights of
your inserts, in which case you would most likely accidentally be running an
effective fly cutter with the wrong feed rate.

We're still on DOC.. A THOU!!! What is the edge hone on your insert? If you are
trying to take a thou, you had better have some ground and polished, super up-sharp
shiny inserts meant for aluminum (but work great on other stuff, in the right conditions).

Lets go back to condition of the material. 4140 annealed/normilized acts a whole heck
of a lot like a low carbon steel. 1018, A36 which shouldn't actually be called A36, the
spec should be "Unpredictable structural GUMMY steel". Up until close to a 30C (above PH
condition) 4140 still acts like a "Gummy Steel". It rips and it tears.

How do you get away from the ripping and tearing? There are a couple of ways.. SHARP,
and I mean SHARP. Ground and up-sharp inserts, the kind meant for aluminum, but that's
more of a lathe thing.. When you can't get the revs to get the surface speed, and we're
getting to that..

SPEED!!!!!!! Something to do with crystallization and blah blah blah, (that's above my
pay grade). F'n fast.. you are running 120sfm.. I've face milled 4140 at over 1400 SFM
and got good tool life, and it was nice and shiny..

DOC. For some reason, on a gummy steel, you NEED a decent DOC to get a good surface finish.
.001 is not going to do it, on almost any material.. .010 to .030" at least..

Feed, you *NEED* a proper feed rate..
moving the table very slow
So what
was your feed rate?? Just because its a manual machine does not mean that you can't
set a proper feed rate.. One Mississippi Two Mississippi Three Mississippi ETC....

DO THE MATH!!! The rules don't change just because you are in your garage, the metal doesn't
care.. The cutter doesn't care.. The RULES are the same weather you are using a
$500 POS Grizzly Mill, or a million and a half dollar high end Japanese horizontal.. The
material doesn't care if its in a Top Secret shop at Sandia labs, or in Joe Blows Garage
out in the suburbs, it acts exactly the same, the rules don't change.. If its a million$$$ part
made from a block the size of a suburban, or a bracket you are making to fix your lawnmower,
the RULES DON'T CHANGE...

There is a lot of imagination involved in machining. Its a very creative trade.. But Feeds and
speeds, those aren't very creative, they are pretty well written in stone. They do however get
creative when running long stickouts on tricky setups... But facing some 4140, nothing tricky
there..

Like the lady that wanted to make a really really good roast, instead of 1 hour at 400 degrees,
she decided 4 hours at 100 degrees would be better.. It didn't work out. Slower is not
always better.

I'm sorry if that still sounds like I'm a dick.
 
First indicate every insert. One (or more) extend beyond the others. If it is one try removing it if it won't go deeper into the pocket. The tool may not be good.

Second increase the speed to about 500 FPM. You may need to remove more than one insert for balance.

Are the inserts square with a 45 degree champher? If not what are they? Are they a steel formulation.
 
Wow Bob....unusual and interesting for you...... I was just gong to go with surface footage and maybe light DOC so no real chip formation and reweld.
I'll often set one tooth .0005 or more high so that I know which one is in control.
Sort of a proud wiper but not really.
I suspect chip weld on the inserts digging troughs at this speed. but who knows maybe it's 62 hard.
Knowing the cutter and inserts would be helpful.
no pictures ..:(..:toetap:

First post from our new member and is lost in this wild world.
Bob
 
This is a guarantee. The OP mentions cheap and Amazon. It's no mystery he's working with a POS tool. Try a real shell mill or facemill with inserts that are actually carbide and report back.

Kind of makes one wonder if he's using it on a machine-that-shall-not-be-named.
 
Kind of makes one wonder if he's using it on a machine-that-shall-not-be-named.

Yet one can do very nice finishes with crappy cutters and a HF mill/drill in 4140.
Obviously the rpm speed is low and the oil is not helping. If my guess at the tool is correct it likes speed as it is very different than a endmill.
DOC is maybe okay or not depending on the insert's edge.
With this cutter design I will do .0005 to .001 deep finishing passes and expert to hold a 30 or better which is not a mirror.
With work down under a 10 on low dollar machine at my cabin and such low dollar cutter.

It is an unskilled craftsman that blames his tools.
All good to blame the cutter or machine . That makes you proud but how to do it without cubic dollars behind you?
It can be done.
Bob
 
It is an unskilled craftsman that blames his tools.
All good to blame the cutter or machine . That makes you proud but how to do it without cubic dollars behind you?
It can be done.
Bob

Of course it can be done, there are people in Khyber Pass that are making the same 1911 that Op is with files and a drill press powered by a 1970 VW, doesn't make it economical or practical to do so no matter how much skill it takes.

Khyber Pass Copy of a Colt - Full30
 
In what condition is the 4140... That means everything, though what you were
doing would result in a shitty finish no matter what.. .

..especially with tiny depth of cuts, likely for cleanup a slide
 
There is SOFT 4140 (annealed) and there is heat treated 4140 - all the way up into the 50s for Rockwell C

Whatcha got?
 
Last edited:
Sorry, folks, I just got back and I see a lot of responses here, thanks a lot to everyone who responded (and no, you don't sound like a dick at all ;)))
So, answering all the questions - the machine is PM-25MV, and yes, the face mill is the one someone mentioned here - I guess it's no good.
I'll try to remove all inserts but one and increase the speed. The slide does feel somewhat soft, I guess it's not properly hardened.
 
many inserts dont give a mirror finish til they go fast enough. look up recommended sfpm if it gives a range like 330 - 750 and .003 - .005 ipt feed
750x4 = 3000rpm per inch so 3" dia thats about 1000rpm
.
and .003x 6 teeth - .018" per rev feed about 18. ipm feed
.
and its only mirror finish often for only 20 to 60 minutes tool life and inserts need to be for part material, wrong inserts will give a bad finish
.
mirror finish requires a lot of testing to find best parameters. not unusual to go faster rpm than recommended and less than recommended feeds. almost always coolant will help if part material is sticking to cutting edges. bue or build up edge will give a poor finish. it tends to not form as much when you go fast enough sfpm.
.
a sign of going too slow is dull finish for 0.5" from edges then its shiny once facemill is making hot chips. faster you go the less dull to shiny transition. if its throwing a lot of sparks obviously inserts are dull.
.
if you indicate, surface dull is often wavy .0004" TIR and shiny is <.0002 TIR, theirs a bit of burnishing going on when inserts cutting hot. the biggest bump or wave is at dull to shiny transition. not unusual to see .0006" height change. i think of it like a speed boat in the water. when boat goes fast enough it rides higher in the water
 

Attachments

  • ShinyMilling_cropped.jpg
    ShinyMilling_cropped.jpg
    17.9 KB · Views: 154








 
Back
Top