What's new
What's new

Newer machinist feeds and speeds question

big_i11580

Plastic
Joined
Sep 30, 2015
Hi

I know this has been hashed many times but I still haven't been able to nail settings down. I need to mill a .012" slot about .006" deep in 440C Stainless steel, non-hardened. My mill's max RPM is 2500. What depth of cut and feed rate do I need? I'll have a 2 flute end mill. I know from looking around I need about 100 fpm for free machining stainless. My pocket book will thank you, the endmills are about 20-25 bucks apiece.

John
 
If you're talking about a .012" diameter end mill at 2500, you will only see 7.8fpm.

Would the part and slot lend itself to turning it sideways and cutting with with a narrowed-up keyway type cutter?
 
Practice this first: Make a 1/2" wide slot with a 1/2" endmill, 1/4" deep, but RPM can be no higher than 61. Yes, 61 RPM. Then you'll have a feel for what you're trying to do with your .012" endmill. Except it breaks a whole lot easier.

Unless your machine has excellent motion control and you can get to near-zero runout at the end of the tool, sub this to somebody who is set up for it. If you're worried about a $25 endmill, you are not ready for this.
 
Hi

I know this has been hashed many times but I still haven't been able to nail settings down. I need to mill a .012" slot about .006" deep in 440C Stainless steel, non-hardened. My mill's max RPM is 2500. What depth of cut and feed rate do I need? I'll have a 2 flute end mill. I know from looking around I need about 100 fpm for free machining stainless. My pocket book will thank you, the endmills are about 20-25 bucks apiece.

John

I'll give you credit for thinking in terms of Surface Feet..

The answer is pretty simple.. Do your calculations for RPMs, using your intended
SFM #... If the RPM your calculation gives you is higher than you have.. Then
you use the RPM's you do have available to do your feed calculations.

It happens a decent bit of the time, where your machine can't produce the #'s your
calculations provide.. RPM's is a big one, especially on smaller endmills..

Occasionally you have to figure backwards because your machine won't provide the
feed rate you calculated..

If on a low HP machine, sometimes you have to figure backwards because the spindle
motor won't pull the cut you calculated...

And I don't think 440C is a free machining stainless.. There is a 440F which I got to
use ONCE, and it was kinda nice.. I haven't cut 440C in years (though I do have some
to do tomorrow).. If I recall, its not horrible, but its not great either.. And it
has a very distinct smell to it when you are cutting. (some people think I'm crazy with
the smell thing, but I can SMELL 440 cutting).
 
I'll give you credit for thinking in terms of Surface Feet..

The answer is pretty simple.. Do your calculations for RPMs, using your intended
SFM #... If the RPM your calculation gives you is higher than you have.. Then
you use the RPM's you do have available to do your feed calculations.

It happens a decent bit of the time, where your machine can't produce the #'s your
calculations provide.. RPM's is a big one, especially on smaller endmills..

Occasionally you have to figure backwards because your machine won't provide the
feed rate you calculated..

If on a low HP machine, sometimes you have to figure backwards because the spindle
motor won't pull the cut you calculated...

And I don't think 440C is a free machining stainless.. There is a 440F which I got to
use ONCE, and it was kinda nice.. I haven't cut 440C in years (though I do have some
to do tomorrow).. If I recall, its not horrible, but its not great either.. And it
has a very distinct smell to it when you are cutting. (some people think I'm crazy with
the smell thing, but I can SMELL 440 cutting).

This is right on the money. I would use a HSS 4 fluter if you can get it, not because it's cheaper or because you are going to F-up (both are realities though), but because it takes more of a beating. 440C is a little gummy, not terrible but...you don;t have enough RPM to utilize Carbide, so you need a tougher tool.

I would start out with 2500 RPM, 1 IPM and full .006" depth. That will be .0001" chip load per flute IF it's a 4 fluter, if not 4 then run .5 IPM. Minimize runout as much as humanly possible. I mean, get your Tenths indicator on the very end of the Endmill, take your time.

Bob, I can smell all kinds of different things cutting, 440c smells a little like clean fuel burning to me. 4140 I can smell from a mile away, Brass obviously. I'm sure others.

R
 
....I would use a HSS 4 fluter if you can get it, not because it's cheaper or because you are going to F-up (both are realities though), but because it takes more of a beating. 440C is a little gummy, not terrible but...you don;t have enough RPM to utilize Carbide, so you need a tougher tool.

+1 on this ^

The first time I had to mill some small details in Inconel, I ordered in top of the line cobalt endmills. After watching them snap off, switched to cheap regular M2 HSS endmills from the toolroom and they made it through job. IIRC ~5 SFM. :ack2:
 
Just thought I would let people know the results. I bought 2 endmills, 4 flute both. Ran at 2500 rpm and at .1ipm feed rate. I took .0015" at a pass. Did both parts without a hitch. I eventually moved to .2 ipm after 1 pass. No issues. Probably can go faster but I broke one endmill during setup and only had the other. Thanks. Always am learning new stuff.

John

Sent from my SM-G900V using Tapatalk
 
Glad it worked out for you! I just ran your settings through my calculator (just to reverse things). They amount to 7.85 surface feet per minute, at .2 inches per minute your feed load was 0.00002 inches per tooth (software reports 2E-5th! LOL).

Further, your metal removal rate was 0.0000036 cubic inches per minute (3.6E-6th) and you needed 0.000004 horse power (4E-6th) to make the cut! Pretty sure those are record numbers I just ran through my ShellerPickerCombineChopper! ;)

Good luck,
Matt
 








 
Back
Top