View Full Version : Feed Rate for 1/16th" Endmill

12-22-2008, 02:28 PM
I have to cut a some 2x2mm fins in some 6061 (tiny heatsinks) and my feed/speed chart does not go down that far. I have a couple of 2 flute stub length HSS endmills and a spindle that goes up to 8000 RPM. Anyone know a safe but efficient feed rate with full flood coolant?

Mark Hockett
12-22-2008, 02:52 PM
I use around .0005" chip load for .062" end mills at about .032 DOC at 7500 rpm. A two flute EM at 8000 rpm would feed at 8. IPM. Keep lots of coolant flowing to clear the chips.

12-22-2008, 02:55 PM

"climb" or "conventional" milling? (To assist with swarf clearance).

Mark Hockett
12-22-2008, 03:08 PM

"climb" or "conventional" milling? (To assist with swarf clearance).

Always climb on CNC mills.

12-22-2008, 04:16 PM
I have to cut a some 2x2mm fins in some 6061 (tiny heatsinks) and my feed/speed chart does not go down that far.

Mike, that's because with such a tiny endmill in aluminum, your SFPM is essentially infinite.

I.e., for a 0.0625" endmill in Aluminum, which is recommended as 650 - 1200 SFPM, you need to run at 30,000 - 60,000 RPM.
So the tooth load calculation is going to be based on essentially "infinite" spindle speed.

Bottom line: no matter how fast you run the spindle, your VMC isn't going to hit the minimum 0.001" per tooth load that's usually recommended...

12-22-2008, 04:23 PM

First off, love your signature.

I've been working with 1/8 solid carbide endmills in A2 steel suing the highest speed on my Bridgeport which is 2720 RPM's. Too slow by the book but worked great although could only do .030 at a time due to the little bugger wanting to deflect. Feed rate adjusted by eyeball.

I ran a .25 solid carbide endmill at .100 depth of cut and about 1800 rpm's and it worked great although the feed rate was probably only 2 IPM.

The 1/16 is probably a whole 'nother beast and it is sure to want lightning fast speeds.


12-22-2008, 04:49 PM
I normally try to run everything except facemills and flycutters at 7500 on aluminum when I am running coated tools. It is a lot of fun watching a half inch em running at 120IPM plus.

12-22-2008, 06:02 PM
Always climb on CNC mills.Totally unrelated to the thread, but I have found that with long series endmills I get a better finish and less chatter if I conventional mill the finish pass on the CNC. By long endmill I'm saying like a 2" or 3" cutting length 1/2" endmill. Maybe this is common knowledge, not sure, otherwise always climb like you said.

12-22-2008, 06:13 PM
I do a lot of milling with 1/8 and 1/16 solid carbide endmills. I finally stopped breaking them when it dawned on me to feed them at the same proportionate rate for their size as a much larger tool. If you were cutting the same material with a 1/2" endmill and it took 3 seconds to cut though 1 diameter worth of material the use the same rule for the small sizes too. In other words, feed it at the same number of seconds per diameter.

Your Old Dog
12-22-2008, 07:24 PM
If I was making heatsinks I'd see if I could do it with a table saw and carbide blade. I haven't done it yet but in a recent thread I started guys say it works great. I bought a blade to try it on but have not mounted and tested it out yet. You probably know if you have the heat sink black anodized it will dissipate the heat better.

12-22-2008, 08:22 PM
Question??? Why do you climb mill with CNC?

Mark Hockett
12-22-2008, 08:46 PM
There are a bunch of reasons for climb milling, one is to prevent re-cutting chips which gives you a much better finish and makes the cutter last much longer. It reduces work hardening. It pushes the cut toward the work holding device instead of trying to push it away, and less power is needed to make the cut.
The reason climb milling works on CNC machines is no backlash. If you take heavy climb cuts on a manual machine the cutter can grab and do a lot of damage.
It is also the reason I rarely use carbide on my BP. Carbide end mill cutting edges chip very easy when re-cutting chips which causes them to fail much quicker. On my CNC equipment carbide lasts much longer, to the point I will wear them out before I ever get a chip on the cutting edge.

An experiment you can try on a Vertical mill is make a conventional cut and look at the finish, then feed a couple of thou on the radial depth of cut and and make a climb cut back over the conventional cut about half way across, then compare the finish.

12-22-2008, 10:19 PM
Mark is "spot on".

Russ, for an explanation, see the text and graphics at:
"Conventional milling versus climb milling" about the bottom of the page at:

12-22-2008, 10:55 PM
Ooops..I already knew the differences between the two...I just was wondering why only climb milling with a cnc.
I "was" going to say..."Isn't milling...milling?" But now I know!
Thanks for the explanation!

12-22-2008, 11:13 PM
I have a handful of 4 flute carbide end mills, but they gum up with 6061 (been there and done that) and there were only 3 2 flute end mills in town. I would love to cut the slots on a saw, but the tolerances are just too tight. The fall back was that I could do them on the shaper, but the mill will be easier and more accurate.

On the subject of climb vs. conventional milling on a cnc, climb milling really does give a nicer finish and helps to avoid material welding to the flutes and causing tool breakage.

12-22-2008, 11:18 PM
If you keep the endmills flooded with wd40 or kerosene or ethyl alcohol in aluminum they won't gum up.

12-23-2008, 04:03 AM
Do as Forest Ady suggests
Attach a router or laminate trimmer or dremel to the quill and run at upto 30,000 rpm.

you can get a 1 hp 30,000 motor with collets for $100. that can be easily mounted on a Alu plate clamped to the quill.

http://www.trend-uk.com/graphics_cache/ee/a6/8c7444ea89538f46d9d6538ff4f4.jpg?o=TzoxMjoiRHluYW1 pY0ltYWdlIjoxMzp7czoyNDoiQmFzZUltYWdlRGlyUGh5c2ljY WxQYXRoIjtzOjMwOiIvdmFyL3d3dy9odG1sL3RyZW5kL3Jlc29 1cmNlcy8iO3M6MjU6IkNhY2hlSW1hZ2VEaXJQaHlzaWNhbFBhd GgiO3M6NDc6Ii92YXIvd3d3L2h0bWwvdHJlbmQvcHVibGljL2x pdmUvZ3JhcGhpY3NfY2FjaGUvIjtzOjIwOiJDYWNoZUltYWdlR GlyV2ViUGF0aCI7czozOToiaHR0cDovL3d3dy50cmVuZC11ay5 jb20vZ3JhcGhpY3NfY2FjaGUvIjtzOjE3OiJCYXNlSW1hZ2VGa WxlbmFtZSI7czozMjoiaW1hZ2VzL2Jhc2VfcHJvZHVjdHMvdDR fc2hhcC5qcGciO3M6NzoiTWF4U2l6ZSI7czozOiI2MDAiO3M6M TA6IkNvbnRyYWluQnkiO3M6NDoiQk9USCI7czoxNDoiV2F0ZXJ tYXJrSW1hZ2UiO3M6MDoiIjtzOjEyOiJJbWFnZUhhc2hEaXIiO 3M6NjoiZWUvYTYvIjtzOjE3OiJJbWFnZUhhc2hGaWxlbmFtZSI 7czoyODoiOGM3NDQ0ZWE4OTUzOGY0NmQ5ZDY1MzhmZjRmNCI7c zoxNzoiQmFzZUltYWdlRmlsZVR5cGUiO3M6NDoiLkpQRyI7czo xODoiQ2FjaGVJbWFnZUZpbGVUeXBlIjtzOjM6ImpwZyI7czoxM DoiRmluYWxXaWR0aCI7TjtzOjExOiJGaW5hbEhlaWdodCI7Tjt 9


12-23-2008, 07:10 AM
I note that you (Mickey) state you are cutting 6061. Do you know that for a fact?

Heat sinks are often made from 1100 aluminum as it has the best electrical conductivity. Since thermal conductivity in metals generally parallels electrical conductivity 1100 aluminum is the popular choice. The problem is that machining 1100 is the pits. It is soft as cheese and gums up the cutters badly. It doesn't saw as well or mill as well as the high strength alloys. It requires flood coolant and very sharp, preferably new cutters. A lot can be gained by using cutters specifically made for aluminum. They have greater flute depth for enhanced chip evacuation and higher rake angle on the cutting edges as well as an aggressive helix angle for chip pumping.