# Is it the end mill or the machinist??



## Jake2465 (Dec 28, 2017)

The other day I was doing some slot milling with a .250" 4 flute carbide end mill that I had purchased in a set of 5 from eBay. I believe they may have been from "online carbide" or something like that. anyway, these slots were .350" deep, .275" wide and 2.000" long. I usually have my mill running 3000rpm with a 24ipm feed rate which gives me a .002" chip load. My depth of cut was .075" deep and this material was regular hot rolled with the surface layer removed.  I had my program set to run a 2 deg ramp angle and to get my .075 depths, so no plunge cutting. With this setup I was able to make it through 6 slots before I started hearing changes in noise and a few sparks. I checked the end mill and the corners of the corners were all chipped. One of the HM members suggested that I may just be going way too fast and should try again with less chip load. Sounded like a good idea to me. 

I guess my impression was that carbide liked an aggressive cut and could handle hot rolled with no trouble. The performance made me start to wonder if perhaps those end mills are not very good or possibly just my zeal for watching end mills eject purple colored chips like a lawn mower.


----------



## Dan_S (Dec 28, 2017)

Normally you slot with a 2 flute End Mill not a 4. Also carbide usually fairs better when it has a small corner radius.

I don't have a CNC mill, but I know a lot of guys that do like to buy stuff from Lakeshore carbide.


----------



## middle.road (Dec 28, 2017)

- Were you running any coolant? 
- What was the type of material being slotted?


----------



## Bob Korves (Dec 28, 2017)

Carbide is brittle.  Nature of the beast.  Hard but brittle.  It takes a rigid machine and setup plus proper feeds and speeds to use carbide end mills successfully.  You are cutting hot rolled steel, no grade specified, perhaps "regular" means mild steel.  If it is HR mild steel, I think you would be much better off with HSS cutters for working with it.  Tell us about your mill...


----------



## Grandpop (Dec 28, 2017)

I agree with hss, and need 2 flute as well. Would never use carbide for anything less than very hard material unless in very rigid machine. 

For your slot I would drill a hole at end of slot to near final depth, put in hss 2 flute center cutting and plunge to about .345, then move over .125 and replunge, move another .125 and plunge again. Keep it up till you get to the other end, then go back and forth at full depth to clean the sides up to your. 275. Using the end mill that way if it starts to dull you can touch up the bottom on the bench grinder and keep going.


----------



## Jake2465 (Dec 28, 2017)

My mill is a Bridgeport R3E3. Basically a boss 8. It uses those Erikson NMTB-30 tool holders.

The nice thing about HSS is that it is cheaper. I guess I have not really considered it because I have concerns about tool deflection and long cycle times. I believe the material was 1018. I don't ever use cold rolled on a mill because I had too much trouble with warping.


----------



## Jake2465 (Dec 28, 2017)

middle.road said:


> - Were you running any coolant?



I was not running any coolant. I heard that running coolant could cause shock cooling and fracture the carbide.


----------



## middle.road (Dec 28, 2017)

That's what I was wondering. So much for that idea.
No shock or interrupted cut in doing keyways, so, what the devil...?


----------



## Jake2465 (Dec 28, 2017)

Another thing I noticed was that the first ramp maneuver started kicking up a burr after a couple of parts. So, perhaps the tool was getting dull for some reason?


----------



## 4GSR (Dec 28, 2017)

There's nothing wrong with running a 4-flute end mill for cutting slots unless it has to be dead on.  Then use a 2-flute end mill. In your case, running a .250" diameter end mill to cut and finish a .275" wide slot no problem using a 4-flute end mill..
In my case, I used to run .502-.505" wide slots 1.250" deep using a .500" long 4-flute end mill.  Material was 4140/45 with a 110-140K yield.  A two flute end mill would snap off in a heart beat in this material. Took five passes to get the slot to depth.
Now, if you are cutting aluminum, yes, use a 2-flute end mill.

Ken


----------



## mksj (Dec 29, 2017)

When looking at the chip load for mild steel using a carbide cutter, I usually see 0.001" for a 1/4" carbide end mill. SFM range anywhere from approximately 50-250, using 200 which may be a bit on the high side if harder material, you get an RPM of 3000 with 12 IPM, if 150 then 2300 RPM with 9 IPM. I only do manual milling, but use a power feed and set the IPM off of the DRO. With steel I use 4 flute carbide and cobalt end mills usually with some cutting oil, with a full size knee mill I usually end up milling at 1/2 the rated SFM, and usually a bit lower on the RPM. You might be a bit too aggressive in your milling parameters.


----------



## Jake2465 (Dec 29, 2017)

I will just have to try the slots again with a slower feed. No big deal, I am not running production here.

So, with that being said, could the chip loads safely go up if the diameter of the end mill went up as well? Like a 1/2" or 3/4" end mill? This reminds me of when I used a little 1/16" 4 flute carbide end mill on some aluminum a while back. a 0.0005 chip load caused it to break within about 5 minutes of use. I had to back the feed down to about 0.0002 chip load and the second end mill survived the whole cycle.


----------



## 4GSR (Dec 29, 2017)

Jake2465 said:


> I will just have to try the slots again with a slower feed. No big deal, I am not running production here.
> 
> So, with that being said, could the chip loads safely go up if the diameter of the end mill went up as well? Like a 1/2" or 3/4" end mill? This reminds me of when I used a little 1/16" 4 flute carbide end mill on some aluminum a while back. a 0.0005 chip load caused it to break within about 5 minutes of use. I had to back the feed down to about 0.0002 chip load and the second end mill survived the whole cycle.


Yep! Bigger the end mill, bigger the chip load.


----------



## 4ssss (Dec 29, 2017)

When you run a 4 flute vs. a 2 flute cutter, you're basically doubling the speed of the cutter while taking off 1/2 the amount of stock.  3000 RPM is way too fast to cut any steel. If you want to hog a part, consider back gears with a faster  feed.


----------



## Bob Korves (Dec 29, 2017)

4ssss said:


> When you run a 4 flute vs. a 2 flute cutter, you're basically doubling the speed of the cutter while taking off 1/2 the amount of stock.


With the same speed and feed, a 4 flute cutter will take twice as many cuts per revolution as a 2 flute, resulting in half the depth of cut per flute.  Nothing else changes.  As a side effect of the cutter shapes, chip clearing may not be as good with the 4 flute and tool rigidity and strength will less with the 2 flute.


----------



## magicniner (Jan 2, 2018)

If rigidity is not an issue I'd guess either re-cutting chips or material pickup on the flutes could be causing the problem, flood or air plus lube might make a difference, 
Regards, 
Nick


----------



## coherent (Jan 2, 2018)

Sounds like you figured it out. I have a small cnc mill and I wouldn't run that chip load and cut speed. The cost of good end mills usually makes me error toward the conservative side and have the job take a little longer.  I don't do production either so usualy in no rush but then again it's been a while since I've broken an end mill which I save for programming blunders and user error.


----------



## 4ssss (Jan 2, 2018)

Bob Korves said:


> With the same speed and feed, a 4 flute cutter will take twice as many cuts per revolution as a 2 flute, resulting in half the depth of cut per flute.  Nothing else changes.  As a side effect of the cutter shapes, chip clearing may not be as good with the 4 flute and tool rigidity and strength will less with the 2 flute.



I think that's what I said but in English


----------



## e189552 (Jan 7, 2018)

Are the end mills center cutting?
If not could be part of the problem


----------

