Glad you got a successful cut.
In general I’d say use 6061 unless you have a good reason not to. It’s one of the better machining grades and there’s more info on it than almost any other aluminum.
It’s honestly hard in general to have any general guides with as many variable as exist between machines and tooling. I’ll give you the simplified version as best I can though.
First there’s a few things I’m going to be referencing that you’ll need a basic understanding of. These will all be simplified versions.
-
Chipload:
As I already touched on this is the size of the chip being cut per flute per rotation. It's technically the widest part of the cut as all chips are cut at an angle. This is ultimately the most important factor in any machining and what all feeds and speeds are trying to get at.
Runout:
This is how much the tool is spinning off the center axis of the machine. The spindle, collets, and bits can all have and add to runout. The reason that it’s important is that it’s basically unintended feed (chipload) that isn’t being accounted for in your parameters. In the case of single flute tooling it’s less of an issue as it’s only taking this extra amount in the initial plunge and some direction changes. In multi-flute tooling it becomes more of an issue. How much you can tolerate depends on the chipload you are using. The smaller the chipload the more the runout matters.
Chip thinning:
This gets complicated but functionally you are cutting a smaller chipload than you think when you cut with a stepover of less than 50% of the tool diameter. For the sake of starting out I would say just don’t cut less than the 50%. Chip thinning can be used to your advantage with advanced toolpaths but leave that headache for another day.
In general we have 2 issues we have to deal with in any cut. The minimum chipload that will cut instead of grind or “rub” and the limits of the tooling, machine, or material.
The minimum chipload is based on the tool geometry, carbide grade and material being cut. From the tool side there’s a thing called the edge radius that you will never find listed. It’s the first part of the minimum as we have to have an edge that can get “under” the material. After that we need a big enough chip that the material can support itself and not just fold over in the way of the cutter. In aluminum with decent tooling I’d say to start with a minimum chipload of 0.0005" (0.013mm) for grades like 6061 and double that for softer grades. To figure out a feed for this times the chipload by the RPM you want to run by the number of flutes (feed = chipload * RPM * flutes).
That will give you a starting point for feed. However, you will most likely get a better cut faster than the minimum plus obviously be machining faster. This now come down to what the tool, material, and machine can withstand. In this case you are going to be limited by either the machine or the tooling.
For the sake of argument let’s lock the tool down to the one your currently using. Now that we have a tool and minimum based on the previous section we are going to expand on it. As I mentioned earlier the forces which are what are going to be breaking our tool or deflecting our machine are cubic material removed per flute per rotation. With locking down the tool that gives us 2 functional number to play with the pass depth and the chipload. So a simple way of testing for a better cut would be to reduce the pass depth and increase the chipload. e.g. half the pass depth at twice the chipload is approximately the same cutting force. The way I usually recommend using this is to chop the pass depth down as low as you can get and take a set of test cuts and increasing feeds to look for the best cut. Then start adding depth to that feed and look/listen for chattering or deflection.
One of the other things that plays into this that you’ve found is the stepover. This is due to something call tool engagement. Which is basically the amount of time the flute of the cutter is “engaged” with the material it’s cutting. The higher the engagement time the longer the machine and tool are being pulled into the cut. This is related but separate from cutting forces as to use an example you’ve already seen the peak forces for your first pocket an contour are actually the same. However, the peak forces are maintained though the entire rotation when you are slotting. That basically makes any amount of deflection (bending) worse and when slowing or stopping for direction changes it snaps back worse.
All of the above is influenced by the tool geometry. Thing like rake, helix, relief, flute volume, end style, flute length, and carbide grades change all the above effects. This is part of what makes it so hard to have any starting number other than X tool on X machine with X runout cutting X material.
I hope that helps some. Please forgive errors and poorer grammar or sentence structure than usual. I’m covering for some people on vacation and can’t really go back through this to check.
Let me know if there’s something you want me to expand on. Or if you want to go down some of the rabbit holes in this check these: