Aluminum cutting questions

I am trying to cut 14mm x 14mm (.55 in x .55 in) holes in an Aluminum 6061 sheet that is 1/16" thick so that they can fit cherry mx style key switches.

I used 1/16" bits from Spetools to do test profile cuts and have broken 8 bits in the process of trying to find the right settings.

So far I have had success with 12000rpm (bit manufacturer recommended number), 25 in/min feed rate, 15 in/min plunge rate and .15mm (.00708 in) cut depth on each pass. Any deeper cut depth (0.20mm or 0.25mm) or faster feed rates (35 in/min) or higher rpm (18000) breaks the bit.

However I have to eventually cut around 300 holes in a 1ft x 3ft sheet and with the current settings it would end up taking nearly 10 hrs (if the bits hold up).

I’m looking for a way to bring down the time to less than 3 hrs. I’ve these options things in mind
1. Get a better 1/16" bit from another manufacturer (Amana?) which will hopefully support higher speeds and/or deeper cuts and hold up better.
2. Get a 1/8" bit to do the profile cuts with dogholes to avoid rounded corners (Thanks Danny Miller for this suggestion) - but I’m not sure if the key switches will still fit snugly.
3. Get a 1/8" bit to do the profile cuts and do a cleanup pass with a 1/16" to get perfectly square corners

Am I missing anything else? Any suggestions on which option I should go with? Also, if you can share which bit sizes/manufacturers/settings worked for you for aluminum, that’d be welcome too - I don’t want to spend too much time/money on buying/trying/breaking bits.

Does it even make sense to try to cut a sheet this big with this many holes on a CNC or should I just find a laser cutting service? Anyone knows how much laser cutting costs?

I would call Sparktech in Round Rock. They also have a Ebay store called drillman1. They sell higher quality bits. They don’t cost much more than regular Amazon bits. Are you trying to cut the al for fitting the key switches? I would go with a fiber laser/waterjet for square corners.

1 Like

I would call Sparktech in Round Rock

Thanks, I’ll check them out.

Yes, I want to fit key switches in the holes.

You may do better if you drill your holes, drilling has a much higher MRR. Or do what Danny said, or maybe even go 1/4" endmill for your roughing pass. That’ll leave 1/8" radius for the smaller cutter to clean the edges on. You’ll only have to do one tool changeout, so it’s not really that bad, and you won’t be moving the material, so you won’t have to re-zero anything.

Possibly combine all 3. Use a 1/4" drill bit to pilot your entrance holes, switch to a 1/4" endmill for roughing, and your final pass with the 1/16". I’ve found that Pilot drilling my entrance holes on sheet al seems to reduce my endmill breakage.

1 Like

Thank you. Would 1/4" drill/end mill dissipate heat well on such small holes? Last time I tried 1/4" endmill aluminum got welded on my bit - granted I hadn’t secured my stock very well and am not sure if my settings were correct either.

It’s not about heat dissipation… you have to drastically low your spindle speed. Going from 1/16" to 1/4", you’re going to have 4 times the speed at the tip of the cutter. So much closer to 1/4th the spindle speed, while keeping the same feed rate. And if you lower you feed rate, you have to lower the spindle speed as well.

I frequently used 1/8" endmills to cut that exact thickness of 6061 aluminum, and I’ve bought some 1/4" endmills to try them out.

Cutting aluminum is about cutting super slowly. A high tip speed will cause galling, which will quickly kill your bits(as you found out). Watch the chips you produce, ideally they’ll almost be like a thin fingernail shaving, though I never really was able to get those. If it looks like little squares of glitter, that’s at least acceptable. Powder means you’re going way too fast. I’m sure someone will chime in with better advice, but maybe this can be a start point. Feed/speed calculators are important with metal, the “good” window for feed & speed is super narrow. Too fast, and the metal will gall because it skips over the top of the metal, rub and generate a bunch of heat, melt the metal onto the bit, and then break it. Too slow, and you’ll try to cut out too much at once, and break the bit that way. You have to be within roughly 20% of “right” to get it to cut consistently.

Drilling your entrance holes cuts down the amount of work the endmill has to do. I use the cheap 1/8" endmills from amazon, and found pre-drilling my holes so I didn’t have to plunge or ramp make it work much better, my bits lasted much longer.

I was drilling holes in solid aluminum with a friend of mine. He was fighting left and right to get them to drill, fighting and shoving super hard to get it to cut, while I was just breezing through them. I let him dull a (cheap) drill bit before showing him how to use the exact same (cheap) bit at a very slow speed… almost the slowest my cordless drill would go, and knocked them out super fast because I was cutting “right”. (I’d gone through the same thing a few weeks earlier…). The bit needs to get a proper bite on the metal, not just rub on it.

Thanks, that makes sense. I’ll try that.

If you ultimately decide to laser this, OshCut or SendCutSend are very cost effective, I use them frequently because it’s way cheaper to have them laser a low tolerance part than it is to machine it.

I’ve used those exact endmills quite a bit and I would rough those holes with a bigger endmill and only use the 1/16 for perfecting the corners. Also, what CAM software and/or tool path strategy are you using?

1 Like

Thanks. I’m doing basic profile cuts in VCarve. Don’t know anything about tool path strategies but with the settings I tried, it plunges down to pass depth, makes the profile cut and repeats this for all passes. Haven’t used ramps or anything.

It depends upon your goal and your tools.

If I have a good flood coolant system available, I find that a 3-flute ZrN carbide mill absolutely plows through aluminum.

However, if the flood coolant system is kind of crummy and doesn’t wash the chips away fast enough, then I can easily break the mill.

As always, YMMV.

1 Like

I mostly use 3/16 bits for most of my cutting. You can go quickly with less depth of cut. 70 ipm for feed and .02" per pass. I also use smooth ramp in vcarve to reduce tool wear and ease the cut. I also use alcohol mist for cooling and chip clearing.

1 Like

On the note of flood cooling, and just machine rigidity, the tormach could knock this out in short order. 1/4” 3-flute ZrN to rough, then 1/16” to finish. You’d have no issues going full depth in one pass. You would need a sacrificial plate underneath though, since something 1x3 on the tormach would have to be attached directly to the table. If you are familiar with fusion, you could also program it as an adaptive cut instead of a full width profile cut, which would reduce tool pressure significantly. SendCutSend or equivalent sounds like it would be a good option. Or maybe asking Joe nicely :wink:

1 Like

I mostly use 3/16 bits for most of my cutting. You can go quickly with less depth of cut. 70 ipm for feed and .02" per pass. I also use smooth ramp in vcarve to reduce tool wear and ease the cut. I also use alcohol mist for cooling and chip clearing.

Thanks. I’ll try that out.

the tormach could knock this out in short order.

Oh I didn’t realize tormach could fit pieces this size. I’ll look into it thanks.

If possible, we hold pieces on the manual mill and Tormach in vises, but much larger pieces can be held down via other methods, especially the T-slot clamps. [Edited:] With 300 holes, the manual mill would be way too tedious, but the Tormach might be perfect. After all, it’s primary purpose is cutting metal, unlike the CNCs.

1 Like

Thanks. Just noticed that the travel for Tormach is mentioned as 18" x 9.5" x 16.25" in the wiki and also the manual - which is less than 1ft x 3ft. How is the cut still possible?