View Full Version : milling speeds

Frank Downey
07-29-2006, 08:06 PM
I haven't posted in a few days,but I need to know what is the milling speeds for a 3/8" Tin coated end mill that I use to cut keyways in 4140 shaft.
The problem that I have is chipping the bit at any feed or any speed.I have tried to use different brands and no luck.I've spent about $500.00 and all I have are a bow of chipped end mills.
Thanks in advance.

Mark Hockett
07-29-2006, 08:55 PM
It would help to have a little more info. Is the Tin coated EM high speed steel or carbide? What brand of EM? How many flutes? What kind of machine are you using? Whats the final width of the keyway need to be?

The problem with the chipping might be the rigidity of the machine and not the speeds and feeds your using.

Mark Hockett

07-29-2006, 09:02 PM
Is the shaft hardened?

In the absence of any other guidelines, I'd probably try about 750 rpm.

07-30-2006, 03:26 AM
Frank, just how rigid is the machine? Without more specifics...hard to diagnose. Without actually touching the machine in person, there are hundreds of combinations for tool chipping. You really should read more of the basics of tooling. Not being mean; just honest. Almost forgot...you will find people blaming all their problems on a specific alloy, not true. Any alloy can be cut, in one way or another. Knowledge makes parts; not alloys.

Frank Downey
07-30-2006, 08:42 AM
I forgot to include the most important info about the tooling. I'm using a 3/8"
Tin coated carbide endmill Kennametal,Hertel,and several other brands.The machine is a Jet 8"x36" vertical end mill brand new only about 20 hrs. on this machine.The metal is 4140 and 4150 stress relieved.I'm just getting into endmilling and milling machines,but the powerfeed on the machine don't have any settings so you don't know the exact feed that you are using,and without that the charts that I've seen can't tell you any rpm's.

J Tiers
07-30-2006, 10:28 AM
Chipping means too much feed.

Dulling means too much speed

That's in general. If the machine is not rigid, that can chip cutters also.

So I would figure you were feeding too fast.

You would probably want about 2 thou per tooth cutting depth, so for a 2 flute, 0.004 per rev, and for a 4 flute, closer to 0.008.

07-30-2006, 01:38 PM
You may do better with regular HSS end mills, too. Carbide is brittle stuff and prone to chip. You shouldn't need carbide to cut what you're cutting.

The Doctor
07-30-2006, 09:12 PM
That Jet is kinda light for a 3/8 carbide mill. Try ΒΌ" hss,maybe 2 passes to depth and 1 pass each direction to clean the sides and bring the slot to it's finished width. Make sure the cutter is sharp! No cheap Chinese hss, about 50fpm, lube well. That should produce what you need.


07-30-2006, 09:48 PM
Frank, I'm seeing a whole bunch of different problems leading to non-success in this situation.

First, the feedrates on your powerfeed. Layout a 12 or 24" long rule, or scribe a couple of lines in some dy-kem. Run the powerfeed at each setting and time it. Multiply it out, now you know what IPM your powerfeed is running at each setting. 10 seconds to cover 24" is 12 IPM. Easy.

>>>>and without that the charts that I've seen can't tell you any rpm's.

It took me while to learn this, but never ever ever think in terms of RPMs, it will just cause much heartache and roasted cutters down the road. Think in terms of Surface Feet per Minute. Every toolmaker will have all of their suggested speeds in SFM. (3.8/dia) * SFM = RPM. Write it on your monitor, you have a white machine, write it right on there, get RPMs out of your head.

Now back to the powerfeed, get the IPMs out of your head and think in terms of chipload per tooth or rev. Another easy one, chipload per rev * RPM = IPM.

Back to the mangled cutters, basically, slotting sucks. I'm assuming that you are using standard 4 fluters since your having so much trouble. Some people are saying rigidity, and I'll give rigidity a big thumbs up, but your biggest enemy in slotting is harmonics. There are a couple of ways to get around it that I've found, 1) very shallow cuts and/or very low SFM(big waste of time), 2) use a rougher to hog out the center, then finish each side, 3) since you have dumped $500 in endmills, try one of the variable flute endmills, I've never seen anything like them in my life, bury them a diameter deep in a slot, quite, no chatter, totally breaks up the harmonics. 4) you could try a HSS cutter, its still going to bounce around (why your chipping endmills to begin with), but it can just handle it a little better.

A.K. Boomer
07-30-2006, 11:40 PM
Really souldnt be the machine, i have that exact Mill and its doing great for rigidity,,, Are you locking down the quill before feeding? if you happen to have a machine with a loose quill fit this will help...

07-31-2006, 04:25 AM
Everyone keeps saying the machine may not be rigid enough, but you gotta consider setup rigidity as well...

08-09-2006, 11:25 PM
[QUOTE=Frank Downey]...what is the milling speeds for a 3/8" Tin coated end mill that I use to cut keyways in 4140 shaft.
The problem that I have is chipping the bit at any feed or any speed.I have tried to use different brands and no luck.QUOTE]
If you can, ditch the carbide and go for the cobalt endmills (M42 HSCo). My formula is about 915 rpm with the 3/8 cobalt endmill. The amount of flutes will determine the feed speed (Chipload).
I am finding that Cobalt is the way to go for most milling of hard materials. It can handle about 10% less speed than uncoated carbide, and does not chip nearly as easily. Cobalt is cheaper than carbide and still gets the job done even in high heat operations. You can even grind the cobalt easier than carbide on you grinder (wear a mask)
I use the data for speeds and feeds from the Machinery Handbook. While Cobalt is not always listed, I use the average speed of the highest HSS to the lowest uncoated Carbide. It works well for me and my applications.
Machinery Handbook, Machinery Handbook, Machinery Handbook, Machinery Handbook! A GREAT investment or request for Christmas or birthday.

08-10-2006, 05:58 AM
Chipping is a sign of excessive vibration coming from somewhere....check that your table locks are snug or maybe something is loose in the head of your machine...loose bearings maybe.Need more info if possible....a picture of your set up would help with the trouble shooting...Good Luck,Mark

08-13-2006, 12:01 PM
One of the biggest killers when using carbide end mills for slotting steel is recutting of the chips. You might try a strong air blast to get the chips out of the slot as you cut.

I probably would shy away from slotting with carbide in that application (combination of material and machine).