View Full Version : how small end mills

02-20-2003, 08:25 PM
I can't blame Murphy for this, but it seems whenever I come up with a shop project, it requires a tool or special cutter that I don't have. My stock of custom cutters is growing. Now I'm wondering what's the best way to create a slot, roughly 1/16 wide, 1/6 deep, starting from a hole. The slot needs to be full depth from the side of the hole, which is .160 dia., to the edge of the workpiece. (no room for a slotting or slitting cutter to run out) I thought I could use (make) a milling cutter to do it, but there's too much flex at this small dia. Any ideas?

02-20-2003, 09:23 PM
If a jewelers saw of 1"diameter won't do it than I might suggest a carbide circut board router they can be had down to about .035"and can be used in machines as large as a b-port mill you just have to feed them at about.001"per second at about 4000 rpm!This requires nerves of steel I admit but I have done it just be sure and lay off the coffee and use your favorite stress relieving medication first! http://bbs.homeshopmachinist.net//biggrin.gif http://bbs.homeshopmachinist.net//biggrin.gif

02-20-2003, 09:35 PM
1/16" isn't a problem either with HSS or carbide endmill. Just make multiple passes so that you're cutting about 1/32" deep at a time. Clean the chips out between passes and use lubrication especially as you mill deeper.

Feedrate of 0.001" per second is definitely too slow and you'll wear the endmill prematurely. Check the chart for the appropriate feedrate based on the material, endmill type, and depth of cut.


[This message has been edited by Rotate (edited 02-20-2003).]

02-21-2003, 12:07 AM
Smallest carbide endmill commercially avaiable is .oo5" - smallest drill is .oo40"


As noted before, your feed rates are miniscule and rpms should be maxed out (they can handle 100k+ rpm).

They do a beautiful job if you let them work and don't push them feed-wise - they cannot stand much lateral pressure - they shatter like glass when you do over stress them (trust me).

02-21-2003, 01:52 AM
Maybe make a mount for a die grinder or even a dremel to at least spin them at a more appropriate speed?

Something that can go in a collet or clamp over the quill?

Has anyone done this on the mill?

Iv'e mounted a die grinder on the lathe in the past. It worked OK for what I was doing.
(making dozens of scriber points from broken bits) http://bbs.homeshopmachinist.net//redface.gif

02-21-2003, 02:16 AM
.005 endmill? Ok, I'm going to check the one I made from a drill bit to see if I failed to get a cutting edge on it, since it should have done the job, being much larger at .063. I suppose carbide being stiffer would tend to get a better bite. My mistake also was too slow rpm. No stress reducing medication either, and I don't think I was holding my mouth right! I learn something new everyday. (serious on this part) I like the idea of a high speed attachment to the quill, is there a quality flexshaft with good radial and axial load capabilities? I wonder if a right angle air die grinder would make sense to retrofit, either with air, or modified to take a flex shaft- or, I'm thinking out loud now, can I pass a flexshaft through the spindle to drive an on-axis high speed secondary spindle, maybe built into a morse taper arbor- hmm

[This message has been edited by darryl (edited 02-21-2003).]

02-21-2003, 08:04 AM
I'd probably use a 1/16" end mill, run fast, with a jet of air to keep the chips out of the way. In those small diameters, I find coolant can tend to make the chips clog up. As per Rotate, not too deep per pass. Of course with that size end mill you can't feel a thing as to how it's cutting, so keep your eye on what's going on and feed just fast enough so it's definitely cutting; again as per Rotate, look up "reasonable" speeds/feeds for what your'e doing and use that as a guide.

If you need to finish to a precise width, make an initial cut with a 3/64" end mill and finish up with the 1/16". You say "roughly 1/16" wide" so maybe that refinement is unnecessary.....

I'm not sure I'd dare try a carbide end mill in that small a diameter (maybe I'm a coward). Carbide is so brittle I'm afraid I'd snap it for sure. HSS is bad enough!

02-21-2003, 08:22 PM
You can use a endmill just fine but keep the feed rate slow as the small ones can walk off center if they are pushed to fast.

02-21-2003, 08:40 PM
In reading your post I noticed that the material that you are cutting is not mentioned. This would certainly have an impact on the type of cutter, speeds, feeds etc. All of the suggestions are good ones and I have used them in cutting small channels in both steel and plastic. I have primarily used HSS tools and most importantly kept the chips out. The best to you on your project.

02-21-2003, 09:54 PM
How about using a Woodruf Keyseat cutter. They come in quite small diameters and widths. probably more forgiving than a 1/16 inch dia end mill. Wayne

02-22-2003, 01:02 PM
What kind of material? Steel, Aluminum, brass? I like to run around 1500 rpm's with a very slow feed. Use a lubricant. Either a few drops of oil or a mist coolant. For going 1/16" deep I would probably make 6 passes if using a 1/16" end mill at .010/pass. It takes a little longer but will leave a cleaner slot. One thing to remember that if you are using an endmill the same width as the slot, you are cutting both conventional and climb at the same time so one side of the slot will look a little worse than the other. By taking smaller depth cuts you will minimize this.


02-23-2003, 05:00 AM
It's 6061, flat bar. I played with the endmill I made, got a better result. Then I changed my philosophy and ground a suitable cutting tool from another, larger diameter drill bit, mounted it in the mill, turned the spindle to align this cutter with the long axis, then used the x axis handwheel to shove the workpiece through the cutter. The mill became a hand powered shaper for a couple of hours. If I had to make this cutter over, I'd silver solder a strip of .o5o hss bandsaw blade into a slot cut in a shaft, and grind a cutting point on it. I think that would be stiffer and would take many more sharpenings before the strength and material was gone. I didn't bother locking the spindle against rotation, since it didn't seem to be rotating at all, but I noted that my mentally modified cutter would have been easier to align. I did pull the ac plug, though, after I caught myself reaching for the on-off switch at the end of one stroke. My arm was a little sore after cranking the table back and forth till the jog was done. And my mind was hurting a bit thinking about wear on the leadscrew and nut. Overall, this process gave me by far the best results, very clean grooves. My guitar project is coming along nicely!

02-23-2003, 10:20 PM
I got a box of 50, count 'em 50, carbide endmills not too long ago from Micromart for $24.95! that go from .010" to .125". So far I haven't had the, uh, mmmarbles to spin one up and see what it can do. Anyway, keep an eye out for this type of bargain! Never know when you'll need to mill a slot to hold a whisker or two.

02-23-2003, 11:20 PM

Just a word of warning. Those carbide bit with plastic collar were meant primarily for PCB drilling/milling and engraving. They are meant to work with fibre glass and soft metal so the rake angle is relative high. In other words, just because they are carbide don't expect them to machine hardened steel very well. They are ok with mild steel, as long as you're feedrate is low.

I don't mean to dampen your enthusiasm, but the price that you quote is actually quite common. I suspect that they are either over stocked items or they have been factory reconditioned, since you have no choice over the size.

You are definitely right about their usefulness. I've machined very small brass parts using these endmills with excellent results.


02-24-2003, 03:57 AM
I've told myself many times that I wouldn't buy carbon steel drill bits, taps, or any other type of cutter if hss or better was available, except for wood or some plastics. Hss just seems to perform better overall, in any kind of material that it's capable of cutting. I wonder if my homemade endmill would have done the job for me if I started with a hss drill bit? By the way, I'm using a diamond coated disc to do the sharpening, it leaves a mirror finish on edges, so I don't think there's an excess friction problem. Carbon steel just doesn't cut it (pun). It's too flexible.

02-24-2003, 09:12 PM
I had a similar problem cutting some aluminum, .125 thick, and we had to cut it all the way through.

02-24-2003, 09:16 PM
I had to test this as its been a while since my last post.

We ended up cutting .010 to .015 thick or depth of cut, running the cnc bridgeport at 4000 rpm, and taking ten cuts to get through the material. I ended up using a two flute carbide cutter, with spray coolant, almost all air with just a thin mist on the cutter, and we also put dish detergent in the crease that we cut. We did this after each pass to try to get some lubrication on the cutting edges. We have four "sheets" to cut, each one taking 90 minutes per pass.

02-24-2003, 11:04 PM
Rotate, that's exactly what they are, and thanks for the heads up. I have no plans for them, other than the short sticks of 1/8" carbide I'll have left after I break them all. Well, I DO hope to get some use out of them first, but I expect some cheap entertainment between now and then. We've got a laser engraver at work. And you think "Laser, wow, we can cut anything!" That's how 'carbide' strikes you too, until you learn otherwise. It's almost a sure bet for woodworking, but I've found a drawer full of carbide cutters for metal are mostly good for filling the drawer.

Rich Carlstedt
02-25-2003, 12:54 AM
Hey YF
I did ! probably should write it up for HSM.

I took a piece of Aluminum 1.25 thick X 5" wide by 10" long (approx) and made it colon shaped (!)
Laid it flat in the mill and
Bored it 3 5/8" at the big end and about 2 1/4 with a web of about 2 inches between the bores. then I cross drilled the web and tapped the bottom 3/8 -16.
Then I slotted (saw cut)between the two bores.
Slipped the big bore onto the BridgePort quill and dropped a straight shank die grinder (dremal!) into the smaller bore (both are snug fits !) and tightened the unit with the cross screw...works slick..
one clamp screw and I now have a high speed tool for small cutters on the Bridgeport
and can feed it up or down etc....

One caution, NO endplay allowed on the small grinder spindle . small cutters don't tolerate it well.

I mill down to .032 without a problem.
Love Carbide...no flex.

Beware of the Boxed Deals ( 50 Cutters !!!)

I just sent 3 boxes back to a large company ( un-named here )advertised as "NEW". The 50 had one endmill, 6 router bits, one microscribe and the rest drills, mostly .0135 and .0115 in each box.
The scribes were nothing more than broken drill shanks, and mill cutters and routers were used ! Found Phenolic chips stuck to flutes and radiused/chipped corners (10 power glass)

02-26-2003, 02:19 AM
Provided you severely clamp your work piece and eliminate slop in your feed screw the PC drills and router are quite capable of drilling taps or dies. Be warned, however, that even slight side pressure will snap them like glass (especially the wee ones).

These bits do not wander unless the surface is tilted - they dig in and bite like crazy. Unless dull.

I use a stereo microscope to observe machining progress with the micro mills. My eyepiece reticle has a .o10" scale and I use it to see if the end mill is starting to flex sideways excessively so feed can be adjusted. I also use diabetic needles to directly apply minute amounts of light tapping fluid as needed.

http://www.kyoceratycom.com/ has a state of the art optical/fuzzy logic sharpener for these bits if you need them tuned up.