End mill testing

As many people have indicated, you should not be using carbide end mills. You do not have anywhere near the spindle RPM required to take advantage of carbide end mills, they are much more brittle and prone to breakage at less than optimum feeds and speeds, and they will provide no advantages over quality HSS end mills on your machine.

This has to be scaled by cutter diameter, however. My McDonnell-Douglas slide rule gives a figure for a 1" cutter, and then you multiply by cutter diameter to scale it for the actual cutter size you have. For an end mill in aluminum, it recommends .010" feed per tooth, but multiplied by diameter. So, for 1/4", that works out to .0025"

To cut at .025" chip load, you need a cutter ground with MUCH greater back relief so the back of the flute is not rubbing on the work. There definitely are special aluminum cutters made this way, but the typical noname stuff is not ground with that much relief.

Jon

I use 4-flute end mills extensively in aluminum, with good results. Since I have limited spindle speeds, and often use small diameter cutters to get smaller corner radii, it helps to have more cutting edges per minute.

Supposedly, though, a 4-flute mill has a thicker web and is therefore stronger than a 2-flute one.

Chip welding is GREATLY alleviated by climb milling, I do almost everything in the climb direction.

Jon

That's a VERY reasonable number, in my experience. But, it ALL depends on the actual milling operation. I slow down when "plowing" at full width into material, such as making the first pass in the middle of some stock. Once there is a slot plowed into it, then I can step over and make a second pass where the cutter is mostly cutting on the side, (climb milling) and taking a much shallower cut, like maybe 0.050 or 0.1" wide.

So, the smaller chip load above might apply to the first pass, and the second value might apply to repeated passes where you can go faster. And, then for a finish pass you'd want to slow down again to reduce the scallops from each tooth.

Jon

The SFM calculation certainly takes the cutter diameter into account, but Machining Fundamentals does not indicate any adjustment to the feed per tooth based on end mill diameter. It also indicates the recommended feeds can be increased 100% or more depending on the machine rigidity and use of carbide cutters.

This is why commercial CNC controls have knobs for spindle speed and feed rate overrides so experienced operators can optimize the process for the machine and cutters in use. They are also tremendously helpful in testing your code and determining if you need to increase or decrease the parameters from the mid range of the guides where you should be starting.

I can log anything, it is a piece of cake with EMC.

halcmd show pin axis.0.f-error Component Pins: Owner Type Dir Value Name 6 float OUT 0 axis.0.f-error 6 float OUT 0.003 axis.0.f-error-lim 6 bit OUT FALSE axis.0.f-errored

I'm not sure how useful axis load is. Commercial CNC controls normally have a spindle load meter, but I don't recall ever seeing an axis load meter.

I'd start a 1/4 2 flute at 10 IPM and 1000 RPM. Then look at how the machine is running. I do it by feel, that's the advantage of manual machining for twenty years. I guess the formulas are great, but there's just too many variables. IMHO, those formulas are for optimization of manufacturing. Not so much for onesies

I do most always use HSS in AL. Mainly because I bought a two hundred plus lb. lot of cutters many years ago and still have a ton on hand.

I'm not at all like Pete, I've broke a lot of cutters over the years. I don't sweat it much unless I've got a buck big cutter in the machine.

Karl

The spindle load meter works great on my Mazak (20hp.) lathe. Not too well on the Hardinge CHNC (5hp) or the Excello mill (4hp). On the last two I find watching the spindle RPM to be the best indicator of overloading. Or at least I back off the feed when the RPM drops. I only see this happen with my large carbide insert cutters on hogging cuts. FWIW, I never tire in seeing how fast metal can be removed.

Karl

Iggy won't either once he starts using some decent feed rates...

Axis load meters will give you the information as to how sharp your tool is. I have them on every CNC mill I run in the shop. It makes it easy to see if the drill or other tool is getting dull by the increase in load.

John

Certainly not implying they don't work---they do. They're just not the right tool for the job. You'd be better served going to a three flute in the circumstances you described. Finish cuts are always taken climb milling (at least by those of us that know the difference). Roughing? Not the smartest thing you can do.

Harold

I haven't followed this thread in detail, but I can't help but wonder if, maybe, Iggy is climb milling when roughing, and there's some slack somewhere? It happens so fast you can't really tell what's going on.

Harold

That's pretty slow, Karl (only 65 sfpm). Given the opportunity, I'd run such an end mill at top speed, what ever it may be, up to 5,000 rpm. Aluminum is very forgiving of over speed, so long as you maintain a decent feed rate. Depth of cut will influence the rate.

Harold

feel, that's the advantage of manual

Then that would seem to be a better indicator of tool wear than simply waiting for the endmill to break. Y'know, you could graph loads vs speeds & feeds and calculate removal rates and total metal removed vs tool wear vs speed & feed and all sorts of neat stuff. Seems like a cool project.

In my mind.... the definition of "how much they cut."

Ergo:

The HSM... may prefer an answer based solely on the cost per unit of metal removed by the tool...

The Commercial Concern... may be more interested in the cost per unit of metal removed per unit time.....

IOW.... if I am a HSMer... I'm OK with maximizing my tool life without regard to time... it is all about the hobby, anyway...

however, if I am making chips for a living, I need a "cost per chip" analysis to assess which is the "best" tool....

Or, more germanely, the cost per finished workpiece.