Strategies and tools for milling pockets deeper than .75" in aluminum

I’m trying to come up with some tooling and milling strategies that will allow me to pocket as deep as 1" to 1.25" into 2" aluminum stock. Currently deeper than .75" point I know that anytime I’m near the wall of the pocket I’m going to be rubbing the shank against the wall to step down deeper. Its the same with the outer face of the shape as I move past the length of my tooling. I know that with longer tools I’m going to have to slow things down. But I’m stuck trying to figure out a tooling a milling strategy to accomplish this. Anyone have suggestions for this. I’ve found a few random 1/8" end mills that have the length of cut I might need, but would feel more comfortable with 1/4" end mills running a bit slower at those lengths.

1 Like

There seems to exist 1.125" LOC 1/4’’ endmills, e. g.

I have abused endmills by cutting a bit deeper than their LOC, and it worked reasonably well, but that felt a bit lame.

1 Like

You can take the endmill to a grinder (or a little sketchier, use a Dremel) and relieve the shank of the endmill and avoid rubbing. Doesn’t take much, just a couple thou/0.1mm will be plenty.


List of long reach endmills at:

Have you had balance issues with the endmill doing that?

Yeah I’m going to order a few and give it a shot. Any rough suggestion on how much slower these should run considering the rigidity of a shapeoko with the HDZ at those flute lengths, I don’t want to be breaking off endmills left and right trying to find the limits at those depths.

Usually one simply mounts the endmill in a drill say, and spins it and applies a stone to it to relieve it, so the material removal is uniform — just only do the area above the flutes, and don’t get up high enough so that the removed area would interfere with clamping — it only needs a tiny bit removed.

1 Like

Ok. I’ll experiment on some cheaper bits first to see how that goes.

I’ve never run them above 18k RPM, but never observed any issues. At lower speeds, the force of a cutter impacting aluminum is going to create way more force than a few grams imbalance.


Does it impact run out?

Not if you don’t touch the portion that gets held in the collet, as Will said.

1 Like

Maybe you should post a picture of your modified collet nut or endmill. I saw it in your videos but a close up may better explain.

Makes sense. I’m playing around with ordering some different tools and will experiment with adding a relief. The other thing I’m running up against is trying to manage my step downs and how to handle the adaptive clearing. No issue on our bigger machine at work, because I can helix the tool to the depth and adaptive clear with full engagement. I have gotten brave enough on this machine at any speed to remotely attempt that and have programmed everything at multiple depths. I’m kind of wondering if the shapeoko at the right speed and feed can handle adaptive with full tool engagement

I’ve pushed the machine pretty hard, even without an HDZ. But even though I know it works, I feel safer keeping my depth of cut under 1/8"


That’s kind of the ballpark I’m discovering by trial and error

Also an easy way to relieve shanks is to get some ceramic sandpaper and cut small strips. Loop it around your endmill and move from one end to the other with the router/spindle on min speed. This will ensure an even grind around the shank and provide a clearly visible collet clamp line.

It’s a good idea to check and tune the runnout before doing this.

As far as milling strategy goes, avoid load spikes like in full corner engagement with small radius. And it helps to maintain a constant load on wall surfacing with continous ramping I’ve found. If you do not want to run a reduced shank for roughing you can also set Fusion360 to pull away from the wall automatically to a set clearance after flute length.


Another great set of advice. Thanks. I’m going to goof around with Fusion360 to try that.


This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.