What's the Seceret to Long Series End Mills?

Slapstick · Mar 21, 2008

I've used long series end mills from time to time and it seems that no matter what unless you REALLY slow them down, they will chatter on you. I've had to slow down long series carbide end mills to speeds i would use for an HSS cutter just to get them to stop chattering... seems almost non productive in a way...

for instance i had to slow down a .1875 carbide long series end mill to about 800 - 1000 rpm in aluminum, in order to get a decent finish, and i was only milling 1/2" deep skimming off a few thou for a cleanup. (i needed the long series to reach down to what i was machining... had there been nothing in my way i could have used a regular length for that 1/2" doc). I had it choked up pretty well so that it was almost only the flutes sticking out from my collet.

I've also found the only luck is to climb cut at a fairly aggressive feed and you can not re-run over your cut without taking more depth, or it will chatter.

Is there a seceret to making use of them as you can an ordinary length end mill? it seems like almost anything longer than "regular length" gets this problem no matter what diameter either.

Bobw · Mar 21, 2008

You've got it, you need to load them up. I use a bunch of 2"loc 1/2d endmills. They can squeel, unless you give them something to chew on.

I had one kid, I was off at an absolutely useless production meeting. He was programming up something or other. His finish pass was like 8 minutes, he kept slowing it down(under 100sfm), less feed(he was down to .0025 per rev), less stock(he was down to .003 for the finish).

I jumped the speed back up, jumped the feed up to .010 or .012 per rev, and gave .020 or .025 to chew on. Ran beautiful.

I've also found that sometimes if you give it a little to chew on on the bottom, that can help stabalize it.

Or my latest trick, take a standard variable flute endmill, neck it way back then take multiple depth finish passes. Most times, the multiple passes blend beautifully.

cdn farmer · Mar 21, 2008

A lot depends on your machine and what your using for holders,,if your using a machine thats in reasonable condition with a decent collets, its a matter of finding the right combo of speed and feed,,cutters with a grind for aluminum would help as well ,,
Another thing is that slowing down is not always the answer,, try going the other way and cranking the rpm up to change the harmonics and don`t be afraid to push the feed and make it cut,,

fmari --MariTool- · Mar 21, 2008

I agree. Longer endmills need a constant load the stabilize the cut. Neck backed variable fluted endmils, thats a good idea. Bobw, what diameters of endmills have you done that with?

smallshop · Mar 21, 2008

BobW...I do that also. I find the long endmills to often be more than I need and you can't clamp on the flutes so I pop a standard length in my crystal lake grinder and relieve about .003 off the dia. and they work great!

I think also just having more solid shank along with less side pressure due to multiple passes makes 'em finish good. I can run them so much faster that it seems about even with a slowed chatter monster doing one finish pass against my multiple passes.
I have done this on endmills between 1/2 dia down to 3/16. I think smaller would work fine also.

I discovered this at an old shop I worked at in desperation. Didn't have a long cutter in time so I put a regular length in a drill motor and relieved it on the green wheel at the pedestal grinder. not pretty....worked great.

Bobw · Mar 21, 2008

fmari --MariTool- said:
I agree. Longer endmills need a constant load the stabilize the cut. Neck backed variable fluted endmils, thats a good idea. Bobw, what diameters of endmills have you done that with?

Maritool, what Smallshop said. Mostly 1/2" but also a bit with 1/4" and 3/8".

Just finished up a job with 1/2" variflutes relieved and hanging out 1.9". One for roughing and one for finishing. I took it easy on the rouging, it was only 4 parts, and they paid VERY well.

PBMW · Mar 22, 2008

I used to do work for a shop that was involved in fiber optics. I regularly got to do parts that has very thin walls. Like .01. Small slots that were deep. I've used necked cutters with great results. Used them as small as .062. Those situations take longer but they usually pay well.

SIM · Mar 22, 2008

I do that myself from 3/16 up to 1, it allows me to cut deep while keeping the shoulders square, if finish is important I'll take a quick cleanup pass with a new cutter to blend it all in.

fmari --MariTool- · Mar 22, 2008

Ok so for a standard variable flute endmill, for example a 1/2 X 1 inch length of cut. I can have some ground to .492 diameter for 1 inch after the flute. I would use a 4 or 4.5 inch long blank instead of a 3.5 inch blank. For a 3/8 X 7/8 length of cut I can do a .367 diameter 7/8 after the flute. So the step down length would be the same as its length of cut. Does this sound attractive to you guys?

Bobw · Mar 22, 2008

Maritool, something like that. Using a longer blank is probably a really good idea, I figure if I'm grabbing on something I'm OK(set screw holders), but then again, I don't do production, and I don't need to squeeze every little bit out of it.

Another little trick, to save yourself an endmill. A lot of times for the roughing endmill, I'll hang it out, in the first step down, I'll leave maybe .007 for a finish, then on the second step down, maybe .012. Its one endmill that you don't have to neck down, so you can still choke up on it for the next job.

Metalcutter · Mar 22, 2008

On a three flute RobbJack end mill..

I divide the diameter by 120 for milling a full diameter slot cut to get the chip load.
I also divide the tool diameter by 85 if I'm roughing, using a 65-70% set over per pass.
This gets about a 50% increase in chip load. When used at the same rpm you get a 50%
increase in feed rate.

The endmill has flute geometry which can work with a predetermined chip load. When using an extended length tool which doesn't have the rigidity, it will work better using a shallower vertical depth of cut.

Try your desired rpm and feed rate at a very shallow depth. When you get that working then begin to go deeper until it chatters and then back off.

If the endmill's extended length increases two times, it's rigidity is reduced eight times. Hence the shallower cut.

This is how I do it. However, I've seen other machinists get way more from an endmill, and I shake my head in awe. But maybe this will give you a starting point.

Regards,

Stan-

Bobw · Mar 22, 2008

Metalcutter/Stan.

I haven't heard the name RobbJack around here in a while. Me, being the cheap prick that I am, I'm wondering if they are actually worth it? I looked into them a few years ago, and they were $$$$$$$$$$$$$. I couldn't justify it. There is no way they could be that much better. How do they stack up in any type of steel? I'm guessing your running aluminum? I don't get to play with Al much.

Curious to see.

g-coder05 · Mar 23, 2008

the slots on this unit where .320 wide and around 2" deep. started roughing with a 5/15 regular length Data flute then after i hit about 1" deep i Back ground an extra long 5/16 Data flute to where it only cut on aroung the first .5 inch of the tool. ran it in multiple steps roughing and finishing. did great with very little chatter. my main problem was cutter deflection digging into the oposing wall.

smallshop · Mar 23, 2008

Fmari.....The reason these work so good is they are custom. I only make them as long as the cut is deep plus a little. Micro 100 makes relieved endmills and because they have to make them for a bunch of different uses they are a bit of a compromise. What would be cool is if you could sell a toolholder that had the id the same as the ground down portion of the shank and then you made the entire shank all the way to the flutes the same dia.. This way a guy could slide the endmill out just enough to clear the top of his part for max rigidity.

Bobw · Mar 23, 2008

Smallshop, that is a fantastic idea, give me a 1/2" variflute, on a 4 or 5 inch blank, with a .490 shank the whole way up, maybe 1/2"-1" or so of flutes.

Fantastic idea. I can just grab it in a collet, or make the cutting part metric 13mm and the shank 1/2". That is a winner of an idea and something I would absolutely buy, not a lot, but I would keep some on hand.

TonyOW31 · Mar 23, 2008

Cutters with a shank smaller than the cutting diameter are common in HSS, cant say I've ever seen carbide ones tho'.

fmari --MariTool- · Mar 23, 2008

Ok I have an idea. Smallshop I like your idea a lot. How about .5 endmills with .490 shank. 3/8 with .365 shank, etc,etc. I can offer custom ER series collets to hold these shanks perfectly.
I can offer ER16,20,25,32,40 collets that are made specifically ground for .240,.302,.365,.427,.490,.615,.740 shanks. I can offer the endmills individually on my site and also the collets individually. I can also offer an endmill and collet sold together at a discounted price.

Do you guys think .01 relief on the diameter is enough? Should it be more on the larger diameters?

viper · Mar 23, 2008

Necked cutters are the cats meow for unique pockets but I too have yet to see them in small cutters or in carbide. I just did a job last night in some cast iron. Had to helical plunge into it a depth of 1.60". I only had two mills that would do this. One was an HSS 4FL with no corner radius, the other was a carbide 4FL with a .110 radius. The first hole has a slightly interrupted cut. I started with the HSS cutter and it had almost a popping noise like the cutter was binding and then breaking free.

I bet if I had a high speed camera, it would scare me to see the deflection. Anyway, hole diameter was .490 and I used a .375 cutter. The HSS cutter lasted for 30 seconds. I tried feeds from .001-.003/tooth. After I popped that one, I went to the carbide and bored the next 35 holes with no chatter or noise. Guess my moral of the story is "carbide" for me please! I have a bunch of regrind HSS long cutters too but I think they are next to useless. many are .375 and below and some are over 4in long!! I have never found a job to use them on.

Reason I used this path instead of a drill is because half the new hole opened up into an existing drill hole I did not think I could drill it without the drill walking off center. I was not sure of feeds and speeds in cast iron so I ran with 130sfm, and .003/tooth and did great. I will probably later learn I can do 300sfm with no problem but I only had one cutter and some time to spare...

Bobw · Mar 23, 2008

Unless your hanging out 10 inches, .010 should be enough, maybe .015 or .020 to be safe, and still keep the rigidity. I really don't like the extended length, necked endmills that are out there, for the same reasons Smallshop said. They also bring the shank diameter down way too small, you really don't need much.

I can understand how the endmill itself would cost more, but for the short run stuff I do, having one endmill that I can run on 10 different jobs, sticking out 1.5", 2" or even 3" would save me a ton of money, I like this idea, Smallshop, Maritool needs to give you a royalty fee, or at least discount.

michael · Mar 23, 2008

If the shanks are ground 1/64 under on smaller and 1/32 on larger cutters they would fit standard sized collets, no? And the clearance amount would be suitable, possibly allowing for a slight regrind.

What's the Seceret to Long Series End Mills?

Cast Iron

Diamond

Aluminum

Titanium

Diamond

Diamond

Titanium

Titanium

Titanium

Diamond

Titanium

Diamond

Titanium

Attachments

Diamond

Diamond

Stainless

Titanium

Titanium

Diamond

Cast Iron

Similar threads