Aluminum Surface Speeds

[Meatloaf]

I like to try to compile recommendations for aluminum settings from different sources. I was watching the sienci video of milling a handle and they are running much faster than recommended surface speeds for roughing with carbide tooling (1981 SFM), Just cruising Amana’s recommended SFM and they list something like 600SFM for roughing.

I’ve read kind of a rule of thumb for carbide aluminum cutting is 600-1200. Are they burning up bits or is there a lot of flexibility here?

Personally I adaptive rough aluminum in the 1200SFM range but 2k seems bonkers. Feedback?

[mick_s]

You didn’t say what alloy you’re using. Aluminum can run from very soft to very hard and the correct cutting parameters vary along with it. Softer aluminum tends to gum up the tool and is trickier to dial in. Keeping the tool cool is the key.

[Meatloaf]

6061 mostly. It seems to me that if you maintain healthy chipload so heat is being removed in the chip, then you should be able to push SFM as long as chatter and spindle power aren’t an issue. My worry is that it overheats the tool even if the chip is healthy.

[mick_s]

Years ago I did some speed tests for an aircraft component part manufacturer. They sent in a few sheets of 1-⅛” 6061. I was able to cut it with a ⅜” diameter tool at 230 ipm, ¼” per pass. The chips were scalding hot (I still have scars on my arms from them landing on me) but the tool held up fine. The problem was clearing the chips out of the kerf rather than recutting them.

[gabo]

With smaller bits I have had more problem breaking them before I get to a chip load that is typically recommended. For cutting out this, I used a 1.8mm bit only cutting 0.002 depth at only 40 ipm. I probably could have gone a little more aggressive but after breaking two bits I dialed it way back.

It takes some experience to cut AL, which I don’t yet have, but working on it.

[TDA]

Usual preface, I’m with PreciseBits. So while I try to only post general information take everything I say with the understanding that I have a bias.

Surface speed (SFM) matters outside of the chipload. You can compensate some for it but you can not carry heat away from the surface speed side with a chip.

I’ll try to explain this in a non-techno babble way. However, that means it’s going to be slightly more understandable with slightly less accuracy. So take this a way of thinking of it more than exactly what’s happening and I’m not going to go over ALL parts but some critical parts.

One big place where the surface speed comes into play is at the edge of the cutter where it engages what will be the edge of your finished cut. The higher the the RPM the faster this edge is rubbing and the more heat is generated there.

Additionally, the thicker that edge is, the lower the rake, or the more tool material rubbing behind the flute, the higher again the heat gets. These also can create a non-cutting force on the tool and material. Either the heat or this force can cause chattering/squealing or damage the tool/material. That is what we are trying to control with the surface speed (SFM). It has nothing to do with the chipload (feed).

The cutting also creates heat. Assuming that you are within good surface speeds and chipload this is where most of the heat is produced. It almost all comes from the deformation of the material into the shape of the chip (inside the flute instead of outside like the surface speed). Generally speaking the thicker that chip is, the more mass is available to “sink” the heat into from the deformation. Meaning that the higher chiploads product less in general.

So to summarize and answer the original question. Yes, it was probably too fast (surface speed) and eating the tool or effecting the cut. There are times when that’s worth it though. To determine if it is too fast depends on a bunch of things you are probably not going to know (rake, relief, edge radius, carbide grade, etc.).

Hope that’s useful. Let me know if there’s something I can help with.

[Meatloaf]

I just wanted to say, that was an incredibly helpful explanation at the detail level I was searching for. Thank you for taking the time to contribute your knowledge.