High spindle speed, low tool pressure

Question

I'm building a small hobby CNC machine out of aluminium with the end goal of milling plastic, aluminium and possibly some harder stuff like steel (although if you saw the machine you'd laugh me out of the room).

The machine isn't as rigid as I would've liked in it's current incarnation. My solution to this would be to use a carbide endmill (~6-8mm or so) at high RPM (~8k) so the tool pressure is reduced and the machine doesn't flex. I've learned that HSS cutters will dull if the chip load isn't high enough, hence the use of carbide as it's a lot harder. I've tried researching this but all I can find are calculators and charts for chip loads for different brands of end mills. My spindle is 3-phase and will happily spin up to 24k RPM.

Can I use a carbide cutter at high speed to reduce chip load? Do I risk breaking the cutter by doing this?

Answer 1

Before we get into calculating the best feeds and speeds for your goals, there are a few more concepts we need to understand.

Chipload: Chip Thickness per Tooth

While feedrates are specified in length units per minute, the more important measurement is something called "Chipload". Thing of a chip as looking something like a comma in cross section, or perhaps an apostrophe. One starts big and gets smaller at the end. The other starts small and gets bigger at the end. We'll ignore that difference for a moment, though it is important as we shall see later.

Chipload is a measurement that is independent of spindle rpm, feedrate, or number of flutes that tells how hard the tool is working. That's a very useful thing, as you could imagine. Hence, manufacturers and machinists typically like to talk about chipload for a particular tool.

You can see that a tool with more flutes (cutting edges) has to be fed faster to maintain a particular chipload. Since each tooth is going to take a cut every rotation, a tooth has only a fraction of a rotation in which to cut a chip that reaches the chipload thickness. During the time it takes to rotate the next tooth to start cutting, the tool has to have moved far enough to shave off a chip that is thick enough. Hence, tools with more flutes can be fed faster. A 4 flute endmill can be feed twice as fast as a 2 flute, all other things being equal.

Why do Tools Break from Too Much Chipload?

You can imagine that forces simply become too great if a tool tries to take too much "bite" by having too much workload. This can chip or break the cutter.

But there is a second issue that comes from too much chipload--the chips get bigger and eventually can't get out of the cutter's way. Beginning machinists probably break more tools because they don't get the chips out of the way fast enough than because the force of the feed is breaking the tool. If the cutter is down in a deep slot, the chips have a particularly hard time getting out of the way. We use air blasts, mists, and flood coolant to try to clear the chips out of the way, but if they're way down a hole or slot, it makes it that much harder, and we have to reduce speed.

More exotic tools are available with 5, 6, 10 or more flutes. Experienced hands will tell you that if you're profiling (where there's lots of chip clearance) steel and aren't using 5 or 6 flutes, you're leaving money on the table. Let's run the numbers in G-Wizard. Suppose we're profiling some mild steel--1020 or some such. We're going to profile the outside of a part, so there's plenty of clearance. Cut depth will be 1/2", cut width 0.100", and we'll use a 1/2" TiAlN Endmill. Here are the numbers:

• 4 Flute: 3158 rpm, 29.8 IPM. MRR is 1.492 cubic inches/minute. A little over 1 HP.

• 5 Flute: Same rpms, now 37.3 IPM. MRR = 1.865. 1.3 HP. That's 30% faster cutting.

• 6 Flute: Now 44.8 IPM. MRR = 2.238. 1.6 HP. 60% faster than the 4 flute case.

Answer 2

High speed steel cutters dull easier because they are less resistant to heat than a carbide tool. Low feed rates tend to increase heat build up in the tool for the same amount of cutting.

Your suggestion to reduce transverse loads by slowing the feed rate will help with accuracy, but continues to run the risk of excessively heating the tool. All other things being equal, you can get better results from the carbide tooling because of their better heat resistance.

You run the risk of lowering the cut depth to the point where your tooling starts to burnish the workpiece and no longer cut the material. Some materials can work harden from repeated abrasion and localised heating with any tooling.