End mill life expectancy

I am not the person to answer your question, but I wonder if you could sense when an end mill is about to break by monitoring the stage motor current? I am presuming it breaks because it gets dull and offers more resistance to the stage movement increasing the current. Do modern CNC mills have any feature like this?

It is usually best to remove as much material as possible per rev of the cutter when roughing. The cubes may need slower cuts as you work inward due to the minimal support of the inner cubes. But, taking very fine cuts wears out the cutting edges faster for the amount of metal removed.

I started out with some Stellite cutters, and had no idea they were anything special. They lasted many years, but eventually got dull, suffered accidents, etc. When I got some new HSS bits, I was astounded at the short life, I burned some up in minutes, others lasted a few hours.

Name-brand cutters ARE better. I used to get this flyer with overstock name-brand (Hanita, Iscar, ITW, etc.) end mills for $3 - 5 each in 1/8 to

3/8" sizes. They eventually started supplying this HORRIBLE Chinese crap in blue tubes with rubber-stamped labels that looked like they were freehand sharpened on a bench grinder by a blind 80-year old guy with shaky hands. Not only was the sharpening bad, the quality of the metal was bad, too. So, I didn't buy any of that stuff again.

Since then, I have moved largely to M42 HSS with Cobalt in the larger sizes, and these are MUCH tougher. For 1/8" I use solid carbide, as they are so cheap.

Also, coolant makes a big difference. I got some TriCool some years ago, and it was awful. When I got the sample of Encool, it greatly improved the life of even the plain HSS cutters, about three times! I was very pleasantly surprised by that!

If you run carbide to where it gets hot, then the coolant can cause thermal stress fractures and shorten the life of the cutter. 2000 RPM probably is not getting a 1/4" carbide cutter hot at all. But, it could be getting the workpiece hot. Often, especially with aluminum, you want to take light cuts and keep the feedrate way up, maybe 15 - 25 IPM to prevent local heating of the workpiece.

2000 RPM on a 1/4" end mill is only 130 SFPM, quite slow even for HSS in aluminum. With a 4-flute end mill at 2000 RPM, this is .00075 inch per tooth, which is quite low. Normally, for aluminum, a chip load of .010" per inch of tool diameter is recommended, so that would be .0025 feed per tooth, or 20 IPM. (Divide by half for a 2-flute cutter.) This is a little higher than I would normally feed, but I would use 10 IPM for plowing full width, and probably 15 for half-width.

Jon

My retired cousin has a CNC Index mill in his home shop and does work for me in return for materials and tooling. I buy carbide hogging end mills (corn cobs) and "Nachi" HSS end mills. Nachi mills are preferred for their quality and life. The only thing is that the job turns into two jobs, roughing and finishing.

My cousin also has little program tips that unload the tool with direction changes and such to account for the tiny bit of slop in the ball screws. That way the stress on the tool is minimized. He makes a LOT of parts with that combination of tooling and programming. He and I use mist cooling satisfactorily.

Probably you werent flushing out the chips good enough.

In several cases here I routinely cut 6061 for several thousands of hours running at moderate removal rates using the same hss cutter on horizontals where ther is plenty of coolant and the chips generally fall freely with no heat build up in the cut zone.

Sounds like you broke it, not dulled it. Look at the tool, is it dull? Did you weld AL to it? Did you make it work in a huge pile of unremoved chips.

I go by feel. You can look at the chips. If they are fine little wispy things you got too much RPM vs feed.

Use a larger end mill if you possibly can.

With the right cutting conditions, an end mill lasts forever in AL.

Karl

Most likely too low a feed rate again. Possibly dulled, possible chip welding on the edges. Even with a 1/4" end mill you should be getting chips coming off that are a good 1/8" wide, not tiny slivers.

Also, what is your depth of cut? Depth of cut mostly relates to spindle HP requirements, but a 1/4" end mill is relatively small and a high depth of cut could be causing some deflection and stress.

The width of cut also matters, presuming you're doing a spiral pocket. The step over needs to be high enough to give a solid cut vs. just rub. Try 0.10" depth of cut, 0.010 step over and 25 IPM at 2,000 RPM.

Of course it's always possible that a bug in your g-code is giving a rapid move stress point that the end mill is handling for a while before failure.

In my manual milling I mostly use HSS end mills, and I rarely break one that is over 1/16". My go-to AL end mill is a 1/2" two flute high spiral and that will tear through 6061-T6 AL at ~2,000 RPM and something that has to be pushing 100 IPM for a side cut of .5" depth x 0.020" width.

So -- with 1/4" diameter and 2000 RPM, that gives 130 SFM.

Looking at _Machinery's Handbook, I see for end milling a speed for HSS of 165 SFM listed as optimum, and 850 SFM average. For "slit" milling, I see 1600 SFM for HSS. The feeds given are 15 and 16 respectively.

But -- the feed needs another parameter -- how many flutes on the end mill. There is typically a feed per tooth, so if this is a two-flute, you multiply by two, if a four flute, multiply by four. I've seen some 1/4" end mills which are six flute -- but those are not center cutting, so they would not be a good choice.

Since some of your cuts (the first cuts at a given level) are slotting cuts (not slitting, a different operation), I think that a two-flute end mill should be your choice.

But why are you using a 1/4" end mill for this project? What is the diameter of the smallest hole in your turner's cube? You should probably aim for an end mill about 2/3 that diameter to give you more rigidity.

O.K. The feeds given above are ====================================================================== "Avoid, if possible, using a feed that is less than 0.001" per tooth, because such low feeds reduce the tool life of the cutter."

[ ... ]

"Wider and deeper cuts must be fed more slowly than narrow and shallow cuts."

[ ... ]

"Fine chips produced by fine feeds are dangerous when milling magnesium because spontaneous combustion can occur." ======================================================================

And -- you don't specify *what* your flood coolant happens to be. What is good for steel may not be that good for aluminum, and vice versa. I usually use WD-40 for milling or turning aluminum -- just squirted from a spray bottle.

If you are not using the right coolant, you are likely to be experiencing a built-up edge, which will break the end mill long before the end of its life.

Enjoy, DoN.

Ignoramus1419 wrote in rec.crafts.metalworking on Mon, 21 Mar 2011 23:47:03 -0500:

Try aiming it from one side only. Coolant needs to flow across to carry the chips out. Pockets are a PIA for coolant flow.