Using our HAAS TM-1P we ended up punching aluminum with holes so we could use it to make our drivetrain. For our drivetrain we used 2x1, and although not optimal we punched through holes all the way to the bottom. We face massive burrs on every face we plunge into, which requires a stupid amount of post processing. I unfortunately seem to have forgotten to take a picture, and we already post processed them, sorry about that. I can say they extended a quarter inch from each side, which took around 30 minutes to post process it
Anyone with more machining expense knows how to tackle this, I know it won’t be perfect but it will be much better than what we have. Our spindle was at 5750 RPM with / plunge rate of 40 IPM (reduced it manually to 5% to not break the bit), and we ran with no coolant. We used fairly cheap jobber #9 drill bit from greenfield industries (which is probably why we broke two of them on four tubes).
predrill with something larger than 0.125 but significantly smaller than 0.201. use a 0.125 end mill to expand each bore to 0.201 with a single pass at full depth. do each face separately. the TM1 should be able to handle this easily with no hand work afterwards.
A lot of things will effect burrs, fiddling with feeds and speeds may reduce the burrs, but that’s not what I would start with.
Sharp high quality bits: A big exit burr is usually caused by the bit pushing material out of the way rather than cutting it, sharper tools will help that.
Lube/coolant: Metal, particularly gummy metals like aluminum cut a lot better if kept cold and if the tool has lubrication. Air blast helps cool the part down somewhat but that’s it, mist coolant is more effective at cooling and adds lube without much mess, flood coolant is great but very messy.
Material: pretty much all aluminum is gummy compared to steel, but there’s a spectrum. 3003 is terrible to machine, 6063 is bad, 6061 is a bit better, and 7075 is my favorite aluminum to machine. If you are buying cheap aluminum it is likely 6063 and you will get better results if you can upgrade to a better alloy.
Machining strategies: Drills are great for speed, but not so great for precision or finish, consider using a more sophisticated machining strategy that might cost a bit more machine time but save clean up. You are using a CNC, so you could just use an endmill to bore the holes, which will usually give a much better finish. Only drill though the top face in each operation, you burn time but the burrs are mostly on the inside where they don’t matter as much. Add deburring operations in the Haas, if your work holding is good it will be much faster than doing it manually. You can even get internal deburring tools: In / Out Deburring Tools
Buy pre punched stock: If you are spending too much time drilling holes in tubes and deburring them, use pre punched stock as much as possible so you are only have to deal with the bad burrs on a few parts per year.
Reject toolchanger, embrace Omio machining strategies and choose a single endmill for every feature on the part.
Sharp drills should help too, but the exit burr through box tubing-which you can think of as borderline sheet aluminum-is always a struggle to tune for.
Fair, I can try this. The only annoying part is that since the tube is longer than the mill (it’s really annoying how they have set it up) we only have a maximum x travel of 16-17, therefore it will require 4 separate operations, but if it makes it faster and more reliable then it’s probably worth it over manual cleanup.
We will be loading in some coolant come next week, what is the concentration ratio that is recommended? All the places I look seem to have differing percentages.
To answer your first question: https://ezburr.com/ is a tool that can go in a mill and deburr both sides of a hole. They work pretty well, so long as your drill bit didn’t break the operation before and your operator didn’t notice.
To give some more info about coolant:
The different places have different percentages because they are based on the coolant you are running. Every coolant manufacturer has coolants for different materials, etc. as well. Make sure you buy a coolant that is recommended for the materials you are most commonly cutting (most likely aluminum).
Also, buy a refractometer so that you can measure the coolant concentration as you are adding to it. Adding a stock new X% every time will not work for proper coolant maintenance. Eventually evaporation or loss will catch up to you.
Contact your local Haas rep and find out what they recommend you use. I recommend making sure you let them know that the machine likely won’t be used often, and you want something with a good rust inhibitor in it. (Another reason to make sure your concentration is correct.)
Also you will eventually need to handle the waste coolant. Start looking for companies in the area that can take care of it for you. You may even be able to get a donation from a local company if you aren’t using too much, and changing it out too often, where they will take care of it for you.
The VF-4 I used to manage had a 50ish gallon coolant tank. It meant we needed to keep 55 gallon drums on hand to empty the coolant whenever it needed it. Just things to consider when working with flood coolants.
Also, some flood coolants can cause skin irritations, so make sure you have nitrile gloves available for students using the mill. I know the first coolant I used on the VF-4 I had no issues with. The first coolant we used didn’t do a great job preventing rust, so I changed brands. We started using Hocut 795-B. I had a mild skin irritation/allergy to the Hocut, and had to make sure I either had gloves on any time I used it, or that I would be able to immediately go wash my hands. Otherwise my skin would get red and itchy after about 5 minutes.
If you want to not break the bits maybe cut that feed in half to .003 feed per rev or 18in/min. But even with no burrs on the holes a prefect hole will still be sharp at the edge. Other people on here have mentioned the hole deburring tools and that’s what I would recommend. We use the Cogsdill Burraway YA-02031-M https://cogsdill.com/products/deburring-tools/burraway/ Deburred tens of thousands of holes in aluminum and no complaints. These only work for 1 inch tube though we had some special made for 1.5 thick.
As for coolant you could spend hours researching and getting varying opinions of what is best. We use Qualichem 251C. Pleasant smell and no skin irritation for us .Varying concentrations depending on material/how much we check it but 6-12%. For aluminum it can be on the lighter side you just want enough to not cause the machine to rust.
You might also play with either just pre-drilling with a very slightly smaller drill bit and then finish drilling quickly with your own size bit, or a reamer. (Edit, quantifying that, usually 2-3% under for a reamer, but depending on your size of burr I might try like a #13-#15 pre drill (0.180 to to .185)
Box tubing is fairly tough to work with in general. It tends to vibrate in all but the most well designed fixtures (something like the WCP fixture with MiteeBites is a nice style). The vibration just makes the burr worse. Everything else folks mentioned, all valid, but you might try this approach as a quicker/cheaper alternative.
The other thing you may consider if you aren’t already doing it, is tweaking your G Code output to only feed through the wall, then rapid to the bottom, and feed through the bottom. If you are fighting cycle time issues, only feeding “slow” though the 0.125" wall (x2) versus the full 2 inches, can let you go appropriately slow when needed and fast when it doesn’t matter.
Make sure to avoid 6063, it is super gummy. 6061 extrusions whenever possible.
1678 has a tool we use to deburr the inside of tubes we machine in house.
Take one of those or bigger, mill or cut a slot in the non-carbide end and cross drill it so you can mount it to a piece of bar stock.
Now you have a groove tool on a stick you can ram down your tube to knock off burrs.
Last thing, always use a high quality SPLIT POINT DRILL BIT. Don’t buy chisel tip drills, they suck. Split point is GOAT.
For slots, irregular shapes. I used this. Might need to dial in the CAM programming, but if you have lightning slots everywhere, this is way nicer than deburring manually.
Last year we started doing all our own drilling on aluminum tubing, and we got surprisingly good results, so clean that no post-processing was necessary. I see a few things your team did differently that may matter.
We used carbide bits with 0.5" flute length (from drillbitsunlimited.com). That means drilling from both sides, but it means less deflection and less rubbing. We made a jig that makes clamping/flipping fast and reliable, so we never have to worry about hole alignment issues.
We use a mister for coolant. I see people report that it is possible to cut aluminum cleanly without, but we’ve never bothered trying.
We use a chip breaking cycle (Fusion 360 for CAM), and our speeds are somewhat higher than you are using. Chip breaking reduces chances of recutting, helps a bit with cooling, and I’m guessing it reduces burrs. My basic understanding with regard to aluminum is that it’s good to cut rather quickly to avoid heat buildup. You might be better off making slightly more aggressive cuts so that you are in contact with the workpiece for less time.
