This might be an issue where I’m hard limited by my machine (S3 XXL with HDZ) and need to upgrade but I’m curious if maybe I can improve.
I’m milling out large pockets in aluminum (2mm deep), and the pocketed area needs to be painted. The problem is I’m spending MASSIVE amounts of time sanding these pockets, sanding large areas of aluminum is a brutal task.
So far the best method I’ve found to clean it up is a 80 grit nylon brush or 60 grit sandpaper, sanding around intricate text or graphics is generally a nightmare.
Here’s some issues I’m facing:
1/4" end mill leaving circular gouges in the pocket - most areas are decently clean, but every once in a while I assume the end mill is stopping in place for a split second and these marks are deep enough where it takes a massive amount of sanding to clear them.
Rest machining - I go from 1/4 to 1/8 to 1/16 end mill. I’m using a bitsetter. For some reason the depth of the bit isn’t calibrating properly. Lets say there’s a corner and I go 0.08" deep with each end mill, often I’ll be able to see a significant ledge (variation of depth) between the different end mills. That ledge might also happen around letters or numbers which creates major finishing problems. I’ve tried manually zeroing each bit but it doesn’t help much.
The only solution seems to be to do a finishing pass over the entire pocket with a 1/16" end mill with good step over options
Try doing the math and adjusting Depth per Pass so that the ultimate pass is only removing the thickness of a chip?
Contrived example:
chipload == 0.004"
Max Depth == 0.5"
Depth per Pass == 0.125"
4 full depth passes are being taken, but if Depth per Pass is reduced to 0.124", then 5 passes will be taken, with the last removing only 0.004" thickness.
The big thing is, always ensure that you have left a thickness of material suitable for the machine to actually cut, not rub.
Thanks I like that tip to add a bit of extra. What’s the amount you generally take off aluminum for the finishing pass? 0.004"? No need to put in a fresh end mill for that? The circular gouges are surprisingly deep in some area. I tried using perfectly new endmills and rest machining but the various cut layers weren’t lining up and that created tons of extra work. I made a project that’s 22x16 and its taken me 4-5 days to mill and sand it. I’m still having to rely on a heavy layer of primer I’m going to sand with 7000 grit to hide imperfections.
TBH I don’t ever do math, I only learned the optimal cut parameters through testing, trial and error. I could only get my S3 XXL cutting aluminum well for hours at a time if I do shallow cuts at faster movement speed.
1/4" single flute: 0.01 DOC, 60 IPM, 8 plunge
1/8" single flute: 0.004 DOC, 60 IPM, 6 plunge
1/16" single flute: 0.002 DOC, 45 IPM, 5 plunge
Any insights into why the rest machining layers aren’t lining up? Tried both doing it all through bitsetter and manually zeroing each tool. Same issue. Also strangely on one end of the project the layers might line up nicely, on the other side it’s off. My wasteboard was just surfaced and no lines.
At each operation you will want to leave enough uncut material that each remaining operation will be able to take a full chip at least, so for the 3 tools you mentioned, you would want to set up the 1/4" tool so that it both takes an ultimate pass of 0.01", and leaves an uncut thickness of material of 0.006" for the two succeeding finishing passes, then the 1/8" tool would cut a thickness of 0.004", leaving the final 0.002" to be cut by the single flute tool.
Paradoxically, larger tooling (which is more rigid) can result in better finishes, so it might be that you could try without the smaller tool.
All of this of course assumes that the belts are well-tensioned, pulley set screws securely in place, and the eccentric nuts properly adjust to hold the Delrin V wheels securely in place ensuring correct linear motion and that the carriage isn’t being shifted by cutting forces (I took some pretty heavy aluminum cuts w/ w/ decent finishes on my SO3 which has an HDZ, so this should be in your machine’s bailiwick).
I believe @wmoy has some tips on this in the videos at:
and @TDA of Precise Bits has shared some excellent information in his posts here as well.
And of course, pictures showing a freshly cut part and its workholding still in place on the machine and the matching file would be the biggest clues for us to examine.
Some (but not all) of the circular gouges are potentially caused by chips/debris on the gantry or nicks or other deformations in the V-wheels. Every time the X/Z axis has to roll over one of them, it microscopically bumps and tilts the Z-axis up or down. Other times, you’re right, a momentary stutter can cause the axis to linger. Or, even the deceleration of that pause can cause a slight disturbance to the Z-axis causing it to dip momentarily. The most obvious solution is to use linear rails on the gantry, like the Shapeoko Pro has.
The less fun solution is to block chips from reaching the gantry if possible (even a dust shoe can be surprisingly effective when cutting aluminum. And if you’re using Fusion 360 or some other software where you can “smooth” out the gcode so there are fewer opportunities for stuttering, that would also help. And before each job, I like to scrub the V-wheels and gantry rail V’s with a toothbrush to clear out any debris.
Can I ask what you’re machining, and whether you could use surface treatments like bead-blasting would help hide cosmetic defects?
So strange, I find the larger 1/4" tool creates more of these gouging issues, or maybe just more noticeable. If I run a surface pass over the entire pocket with a 1/8" or 1/16" end mill there’s much less clean up to do partially because the gouges are smaller but also because there’s no 1/4 to 1/8 to 1/16 height mismatch to clean up. The downside is it takes forever to pass over the entire pocket.
I got the machine cleaned and calibrated to the best of my knowledge and ability going over everything you mentioned, but I’m definitely missing something. The machine rails and wheels were cleaned before this job and also I use a dust boot that sucks up all the aluminum chips right away.
When I watch winstons videos cutting aluminum, it’s a spindle, so not really the most fair comparison, but my dewalt router and machine creates a lot more burs along the edges of walls. His surface finish is much cleaner.
I checked if there’s any wobble on my end mill from the collect / spindle, side to side it’s rock solid, but there’s what feels like 1-2mm of play when I move it up and down. It’s tightened firmly in place.
Is that normal? I’m going to test it with a 1/4" endmill, maybe my collet is worn down.
Can’t share the file. Since I had to run so many various clean up attempts it’s basically just a mess lol.
Hey Winston, its a 6061 aluminum sign 22"x16" with script lettering and a basic graphic. Bead blasting would be great for most normal tool marks but I don’t think they will take out the gouges fully. Rails and vwheels are super clean, I use a strong shop vac with dust boot.
That does not seem normal. Shouldn’t be any play that results in a tactile “click”.
Also, regarding surface finish, particularly on walls, are you using Carbide Create? And if so, do you have Pro? The default cutting direction is good for plastic and wood, by merely OK for metal. Using Climb cutting vs Conventional is better.
