First Experience cutting 6061 Aluminum

[Rcnewcomb]

As FixItMike says: Good judgement comes from experience. Experience comes from bad judgement.

I got a lot of experience today.

I used WD40 as the "coolant". No real issues there.

First error(s): Had the material thickness wrong AND didn't ramp my plunge. Broke a brand new Onsrud 1/8" O flute bit on the initial plunge. Switched to a 1/4" upcut bit.

Next error: Should have done the chamfer profiling first rather than last.

Did the inner profiles at 10K RPM at 60IPM which was a chip load of 0.006 -- the recommended load for this bit. The chips seemed too large so I slowed the feedrate on the outer profile toolpath to 30 IPM.

Most of my tabs weren't sufficient. A lot of waste pieces popped out during the final pass. I either need more and/or longer and/or thicker.

Edge quality showed a lot of chatter. I attribute that to inadequate work holding. This was thinner (0.14") aluminum.

I attempted to run a chamfer with a 60° V bit. But the pieces weren't stable (poor work holding) and the V-bit ended up with a birds nest wrapped around it. Stopped it before it completely destroyed the work piece. A ball nose probably would have been a better choice to soften the edge.

Final observation. Now I have to figure out how to clean up all these aluminum chips.

I'm teachable, so I welcome additional advice. I have more 6061 in various thicknesses as well as a chunk of Mic 6.

[TReischl]

Darn good for your first go at it.

A couple of things you might want to think about:

Carbide is NOT the best choice for aluminum. My machine is probably not as rigid as yours, but I get pretty decent results using HSS. I buy the cheap chinese ones so I am not trying to run a bit past it's prime. It is darn near heresy but I run 2,3, and 4 flute bits. Today I made up a mounting plate for a Nema 23 motor. I needed two 6mm slots so I used a .125 dia carbide 2 flute on it and did a spiral profile .375 deep. Kept them pretty much flooded with WD 40. The idea behind the WD is to keep the chips from welding. The feed was 30 IPM taking a .010 depth of cut on the spiral. They turned out "ok", not noticeably gnawed out but not stellar by any means. Then I cut the clearance hole and locator pocket using an 8mm HSS bit. DOC of cut was .015 with a feed of 40 IPM. The finish was really nice.

I agree with you about holding down the work, getting a large piece of 1/8 aluminum like that to not vibrate may be an exercise in futility. I am thinking I would attempt to do a rough out leaving .004 or so on the walls and then follow up with a finish cut at full depth using a climb cut. Or maybe spiral it in fairly aggressively.

BTW, I never get the chips I would like to see. The spindle is just too darned fast.

I pretty much avoid pocketing if at all possible. I like the spiral profile routine so I will draw extra vectors so that I can use that strategy. It is the way I did the locating pocket for the Nema motor today. I offset the vectors and then used an inside cut with a spiral down feed. Sort of a PITA but it works for me.

I have NOT been very successful using any kind of V bit to cut v grooves. My thinking is that first off they are carbide and their angle of attack is about zero. (Rake for all you machinists out there), second they are not really sharp, sharp, third, at the point they cannot cut at all, fourth they are plowing. Not sure what the solution is for that. Been thinking of using something like a HSS spotting bit as a V tool. Much better rake on those.

Like I said though, I think you are doing pretty darn well for a first go.

Edit: About tabs. I rarely use them.

[Rcnewcomb]

How do you clean up the mess? My sawdust goes into compost so I don't want to use my regular dust collection system for metal.

I was thinking of using a brush, broom, and dust pan.

[BillK]

We had a Tormac Milling machine at work before I retired, and I wrote some programs for it. Obviously the slower spindle speed, flood coolant, and a stationary spindle makes a big difference. I agree with using the spot drill, that’s what we did for engraving and it worked well, on steel also.

Keep it slow and light cuts. Your ears are trained for wood, you need to re-train them for metal, I did. You’ll adjust speeds and feeds on sound more and use chip load calculations less as you go on. Good luck! Oh, and if you get to the point you need to do a lot of small aluminum parts, check out Bantam tools, they make an affordable aluminum milling cnc.

[ElevationCreations]

For aluminum plate hold down we prefer the blue tape and super glue method.

Bits we use the TiN coated carbide 3 or 4 flute and run between 10K-12K RPM. Feed and DOC depends on the size of the bit.

Lubricant we use denatured alcohol - dries and does not interfere with the waste board and recently picked up one of these mist coolant spray system which keeps the chips cleared and you can dial in a fine mist of coolant.

https://www.amazon.com/gp/product/B07X8 ... UTF8&psc=1]

For chip containment we build a wall of scraps or cauls around the machine tool path area to try to keep the chips from flying everywhere. With the air-assist the chips fly further.

For breaking the edge we use a de-burring tool similar to this one
[https://www.homedepot.com/p/Husky-Debur ... /304583908]

[kstrauss]

I seldom cut anything other than aluminum and plastics such as Delrin. A few comments on my experience:
My max spindle RPM is 10000 and that is what I mostly use

Securing thin material is very difficult. Approaches that have worked for me include using double sided paper tape (Nitto P-02 works well) combined with screws placed in waste areas, use tabs and cut mostly through the stock and then remove that in a final pass.

Realize that alloys such as 6061 cut much better than the stuff commonly at big box stores

Chip welding is reduced by using carbide bits coated with ZrN

WD40 or 95% isopropyl alcohol (available from Walmart) applied with a mister also reduces welding

For small diameters carbide bits are much more rigid than HSS and with a ZrN coating reduce chip welding

I use 2 and 3 flute bits

I break edges on most work using a carbide 4-flute 90-degree chamfer bit. I mostly use it ON a toolpath that is offset 0.05 from the edge of the stock with a 0.05 DoC

[martin54]

Dust pan & brush will work If you are going to be doing more of this then an old hoover comes in handy for clearing up. Like you I don;t want to use my regular dust extraction & mix wood & metal chips. I have an old shop hoover that I use just for cleaning up after cutting metals & plastics

Your first try went better than mine did, I had a part to make, spent time measuring & drawing up the part in the software, toolpathed it & was ready to go, cut a piece of stock to go on the machine & at the last minute changed my mind & went & made the part on the old manual lathe Later started with something a bit less complicated that just required some profile cutting

[jerry carney]

Looks really good, I like cutting alum. I never take more than .010--.015 cuts. I use most bits
end mills ball nose. Nice work Randall

[TReischl]

I see a couple of folks using alchohol. . . .

My shop is really small, 14 X 28 so I am careful not to use stuff that puts vapors in the air, especially ones that can burn.

The other thing is if someone is using a router that stuff will evaporate like crazy because most routers exhaust is in line with the cutter.

I see quite a few folks using just plain air to keep the chips out of the cut, that is sort of on one of my down the road to do lists.

Some things to consider:

"Isopropyl alcohol is highly flammable and can easily ignite. Vapors may form explosive mixtures with air, traveling to a source of ignition and flash back, and use of water spray to fight fires may be inefficient."

and.....

"Alcohol can be absorbed into your bloodstream by inhaling alcohol vapors. People who inhale alcohol vapors get drunk very quickly, because the alcohol goes straight to the brain. Also, heated alcohol vapor can injure the lungs."

That was after about a minute of searching.

So, nope, I am not going to be pouring alcohol on my parts any time soon. Definitely not going to spray it either.

[TReischl]

As far as cleaning up the mess. . . .

I made some movable acrylic shields that I position around the work area. If I screw up the machine just knocks them over.

After that? A 3 or 4 inch paint brush makes for a good machine "broom". Dustpan and into the shop trash they go.

I have been thinking about making some strips that cover the t slot openings, or at least some 1/4 inch MDF fit around the vises I typically use. I haven't done any big sheet stuff in a long time. Last time was when I built my wife's clay rolling machine a few years ago.

[kstrauss]

I don't want to start an argument about coolant. However, I would like to mention that alcohol is used by many high end industrial machines. For example, Datron (https://www.datron.de/en_gb/datron-cnc- ... ystem.html and ). They don't "pour on alcohol" but use a MQL system.

[Tailmaker]

For workholding delicate metal parts you can try fixturing wax or wax film (Mitee-Grip). I have not tried it myself but looks promising for small parts, as long as it can be kept cool.

My dust collector does not capture heavy metal chips so I take a shopvac to clean up. But aluminum or brass chips are kind of benign. Once a while I machine a piece of mild steel and the tiny sharp chips fly all over the place, mess up the machine and get stuck everywhere including the shoe soles. Obviously they cling to everything slightly magnetic.
https://youtu.be/Pl8jR2I9GGI
https://youtu.be/WuSygxzvCKM
Certain things are better not done on a wood router even if it is possible...

[Robert L]

The messy chips can be a nightmare, especially after cutting 5500 pieces. WD-40 was a good choice for lube. The sheets
are 48 x 48.

Robert

[TReischl]

I don't want to start an argument about coolant. However, I would like to mention that alcohol is used by many high end industrial machines.......They don't "pour on alcohol" but use a MQL system.

There is no "argument" about it.

The "MQL" system only controls the amount of liquid being used. It stands for "Minimum Quantity Lubricant". Turning the alcohol into a mist would seem to me to be even worse than "pouring it on".

Being used by "high end industry" does not make anything safe. Most of the "high end" cnc machines used in metal working are totally enclosed these days. It would be interesting to find out if they are filtering the air, my guess would be yes. Or maybe not.

I worked in the industrial laser business for many years. Lots of the customers would cut all sorts of stuff that gave off dangerous chemicals, the machines were not guarded or the air filtered, the operators just sucked up the fumes like human filters. So I do not give much credence to thinking something is "safe" because it is what industry uses.

All that said, I can see if one has a machine in a large shop with lots of ventilation the issue would not be as pronounced.

Well, on the lighter side, if you are using alcohol and after a few hours you are thinking your machine is looking pretty darn hot, then enjoy!

[Rcnewcomb]

cutting 5500 pieces. WD-40 was a good choice for lube.

Robert,
Thanks for helping me to see the possibilities -- 5500 pieces, and for the affirmation!