1/16" End mills are breaking

Zebradog · Mar 20, 2012

Hey everybody-

I'm fairly new to machining, meaning I've n doing it for a while, but it's mostly for small personal projects that don't require a lot of precision, I've got a 1941 Atlas 10" lathe, and a mid 1980's Bridgeport J mill. My dad's done production machining when I was a kid, and I've picked it up as a hobby in the last 3-4 years.

That being said, I decided to get a set of plans for the RG-G Gatling gun. I'm currently making the recoil pins which require a 0.062" wide slot, 0.050" deep and 1.8" long. I had a few 2 flute 1/16" end mills in the tooling I got from the last owner of the mill; those broke really fast. I also ordered a few 4 flute HSS end mills, and I have managed to make 4 complete parts, but I keep breaking the end mills

As it stands, I'm taking .010" deep cuts at a time, and my power feed is almost as low as I can go, and my Mist system is pooling cutting fluid while I make each pass. My max RPM on my mill is 2750, and I have a VFD on it running it at 82hz, so I should be in the 4k RPM Range, or just under it.

I know ideally I need above 5k, but there is no way I can get there. Any suggestions?

Thanks in advance!

jkruger · Mar 20, 2012

Put a pin on and endmill shank in the spindle and check the runout. Too much runout will ruin small endmills. What is the material?

athack · Mar 20, 2012

You need carbide end mills. 3k-5k rpm take full depth of cut and feed at 1-2ipm. If it's easy to machine material up the feed to 2-3ipm. Buy quality end mills.

John Welden · Mar 20, 2012

Use a slitting saw?

Zebradog · Mar 20, 2012

The material is CRS, nothing special.

For some reason I thought that Carbide had to be spun faster, and high speed steel was slower, that's why I never tried Carbide.

I actually had the same thoguht about the slitting saw, and I have a blade that may work too. I'll try a Carbide 4 flute end mill as well if I can get one tomorrow.

wesg · Mar 20, 2012

A stub length endmill will make a huge difference as well.

Spencer in NH · Mar 20, 2012

Carbide is only useful to improve tool stiffness, or increase SFM. Since you are RPM-limited, that's a waste of money, use HSS.

You need to look at feed rate in inches per tooth. For a 1/16-in. endmill it should be about 0.0003 (yes three tenths) per tooth. So, for 2750 RPM, that's about 1.7 inches per minute for a two-flute, double that for four. I bet you exceeded that. That's why people say you need more RPM, but you're doing this for fun, not profit, just get your feed rate correct.

For chip evacuation, a steady air blast is your best bet. If the chips don't get out of the slot ..... *tink*. Seven bucks, please.

Finally, check tool runout, as others have suggested.

jamie76x · Mar 20, 2012

Carbide 3 flute endmills are awsome! stronger than 4 flute with better chip evacuation. if you don't want to spring for carbide there is a brand called metalmonster that I got from fastenal and msc. They are HSS but I had great luck with thier small endmills. And also ... You will never get a .062 endmill to cut exactly where you want it to, and right to size due to it "walking" with the climb or convex cut. it will always veere to one side. If you have to be perfect you shound go one size smaller and run it down the middle, then run clean up passes on the top and bottom size to get both the right width and location

And i agree with every one who posted aboved me, Check run out first before you go any further.

jkruger · Mar 20, 2012

Monster tools is very close to where I work. We use a lot of their stuff and they are a pretty good company.
check them out: Monster Tool - Home Page

John Welden · Mar 20, 2012

You'll be way better off with a slitting saw. I'd go that way for sure. You could make your own arbor if you can't afford one. You can even turn it in the mill if you don't have a lathe.

There are so many variables, it's really hard to say what's going wrong with your current set up. The slitting saw will tolerate a lot more shittyness.

oldbikerdude37 · Mar 20, 2012

John Welden said:
You'll be way better off with a slitting saw. I'd go that way for sure. You could make your own arbor if you can't afford one. You can even turn it in the mill if you don't have a lathe.

There are so many variables, it's really hard to say what's going wrong with your current set up. The slitting saw will tolerate a lot more shittyness.

I agree , saws have lots of teeth and you don't need to run the mill balls out.

An arbor is super easy to make , hell you can use a bolt to make one.

Mike C. · Mar 20, 2012

"I bet you exceeded that."

Probably has no way of knowing, as I'll bet the power feed is one of those crappy variable speed Servo types. Without a gear driven properly ratio-ed feed setup, chipload and thus avoiding breaking endmills is just guesswork. The smaller the endmill, the more critical the feed rate in terms of repeatability and stability. Varispeed feed setups have neither.

9100 · Mar 20, 2012

Get a 1/16" Woodruff keyway cutter. You won't have the flex problems of a slitting saw and you just stick it in a collet and go.

Bill

Greg White · Mar 21, 2012

oh contrair,my Anilam readout on me B.port tells me my feedrate,But,its the only readout i have seen that did....
Its in I.P.M.,but its all the same,eh?
Gw

Spencer in NH · Mar 21, 2012

My Newall does, too.

Think it through, steady hand, do it.

willbird · Mar 21, 2012

9100 said:
Get a 1/16" Woodruff keyway cutter. You won't have the flex problems of a slitting saw and you just stick it in a collet and go.

Bill

Actually you want maybe a 1.5" dia "woodruff style slitter" but I agree. An actual woodruff key cutter has a pre determined dia/width ratio...and typically in a 1/16 the dia would be quite small.

Exactly how smooth power feeds are at low feedrates might be an interesting thing to check out. Another issue is if you are feeding all Left to Right, or alternating, if you are alternating you are reversing the cutter spring or flex, and it will make a wider slot, and put a lot of load on the cutter too. Making a 1/16 slot with a 1/16 endmill is never good to begin with, but in my limited experience for it to even begin to work you need to feed the same direction each cut.

Zebradog · Mar 21, 2012

Thank you to everyone. I checked my runout last night and made sure it is less than .001" left ot right and front to back, and also checked my vise. Everything is in spec.

Feedrate is a new concept to me, I've never really payed much attention to it before because I'm always using a 1/2" or 3/4" and I machin aluminum almost always. The fact that I never payed attention is feedrate shows in the condition of my 3/4" end mill

I have an Anilam 411, it may have a feed rate on it, I've honestly never explored all the features because I've never had to machine anything with so much accuracy, or anything this small.

And yes...LOL! I have one of those "Shitty servo motor power feeds with an adjustable nob. Worst case scenario, I can time how long it takes to run the mill one inch with a watch and set my power feed up accordingly. Now that I understand why it is so important I will pay more attention.

The reason I have done all this is after I put the slot in the top of the part, I have to give it a shoulder .0156" deep and .065" in, and it has to be square, so I tried to do it all in one operation. I think I'll use the slitting saw, then remove the part and stand it up and use a sharp endmill to make the shoulder. With the slot in the part, it should self level in the vise. The slot is only meant to be a pilot hole later on in the project.

Again, thanks to everyone for your replies. Without forums, I would be lost.

9100 · Mar 21, 2012

A 1/16 keyway cutter will only be around 1/2" in diameter and will be stiff enough to cut the shoulder just by raising the table and making another pass. You would not want to make it cut on the side, so you would back it out, raise the table, then feed it into the depth. Doing it in one setup will maintain the relationship without having to pick up the position in a new one. A larger slitting saw will have more teeth and last longer, but unless you are making the parts from some superalloy, cutter life should not be a problem.

Bill

gwilson · Mar 21, 2012

I want to get around to making a high speed attachment for my vertical mill. I've seen a few on Ebay that clamp around the quill and stick out sideways. They have a separate spindle,and use a belt to triple the speed. I've seen a hobby level one made from sticking a Dremel tool on a bracket that clamps to the quill,and is belted to a mini spindle.

I want to use a Dumore hand grinder mounted to a thick aluminum plate,and regulate its speed with a wood router speed control box. They are about $30.00.

If you have a Bridgeport quill master attachment,they double the speed of their spindles. I have one,but want to go faster than they will provide for very small endmills.

Screwmachine · Mar 21, 2012

Zebradog said:
And yes...LOL! I have one of those "Shitty servo motor power feeds with an adjustable nob. Worst case scenario, I can time how long it takes to run the mill one inch with a watch and set my power feed up accordingly. Now that I understand why it is so important I will pay more attention.

You can definitely time the travel, do it over several inches for more accuracy. If you are within .001" on runout and get your feed right (agree with about .0003" , maybe .0004" per tooth per rev), should be fine. But for this job you really will have less headaches going with a slitting saw or woodruff cutter.

1/16" End mills are breaking

Banned

Stainless

Stainless

Diamond

Banned

Titanium

Stainless

Hot Rolled

Stainless

Diamond

Titanium

Diamond

Diamond

Titanium

Stainless

Banned

Banned

Diamond

Diamond

Titanium

Similar threads