Minimizing blowout when drilling aluminum

Hello all. We are trying to do a WCD chain in tube with a ton of mounting holes as seen below (that’s the side rail). This is our first time cutting tubes on a CNC.

The problem we are having is the blowout from drilling the top face is going into the tube and getting in the way of where the chain+sprocket are supposed to go. At this point we just aren’t going to include the extra holes but we really would like to. Does anyone have any tips about how to minimize this problem? Feeds +speeds wise?

I’ll have pics of blowout and our feeds and speeds tomorrow.

Try slowing your plunge rate on those holes.

Also, I suggest a couple of deburring tools set up for doing hole insides–you’ll want to do that anyways.

Generally go slowly, it will decrease the burr on the inside. Also, we have a file on a stick that we use to deburr the inside of tubes, though it will take a while with this many holes to deburr it.

1 Like

You can also drill the holes in two stages - the first close to final size and the second at final size. This will reduce the tear out substantially because you’ll be cutting most of it away as the hole gets to final size. It doubles your drilling time but depending on your application, it might be good enough. “Good enough” here doesn’t imply low quality or hacky, it means good enough for the requirements of the design, the material, the time you want to spend on a specific operation, all that; everything is a tradeoff

Following @EricH advice of a reduced feed rate will help but it’s very difficult to prevent this problem when you are drilling unsupported like this but if you need really clean insides, you’re going to have to debur the insides in just about any case).

As you get very close to completing holes like this, the behavior of the material you are cutting gets unpredictable - some holes will be close to perfect and some will end up with burrs not matter what you do.

Finally, do you really need every hole there? Like the entire pattern? That’s a lot of time, electricity, tool wear or breakage, etc. I’ve rarely found it worth it to make things like that which are sort of “stock” parts - if you need a series of holes in a specific area, you might be much better off overall just making the holes there and leaving the rest solid. Think about whether you are making a part for a specific design or making parts that have a lot of “just in case”. It’d be a shame to spend all that effort and find out when you use it, you really need spacing that’s offset by a 1/2 or 1/3 from the existing hole pattern.

You could even make the parts with just the holes you need for the mechanism and later do a second operation for specific hole patterns once you’ve got a specific scenario in mind.

Sometimes “can” needs to weighed against “should”. I’ve spent time and money making general parts that I thought would be “good to have” and then when it really came down to it, they didn’t fit my specific scenario and I thought about all that time and material…

1 Like

You could mill the holes instead of drilling them. That should solve it.

I’ve always thought it would be neat if someone made a block with spring loaded blades that you could put in the tube and then hammer through it to shear off inside burrs.

2 Likes

Mill or use a better drill. What size holes? Looks to be about 3/16" (.191" for rivets)

I use these https://drillbitsunlimited.com/Drill-Sizes-120-and-Up-P5632986.aspx and they work really well. I don’t have many issues with

They have .191" drills (perfect for a 3/16" rivet). Super cheap and last long. They also have a 165 degree tip so if you’re doing sheets, they won’t drill into the spoilboard way too deep

I don’t have personal experience with these but this tool lets you pass the blade through and pivot it out so you can debur/countersink the opposite side of a hole.

7 Likes

The grade of aluminum will make a big difference. 6061 does not have the burr problem that 6063 has. The 2 step process mentioned earlier is the best option. Us a #4 centerdrill for the pilot hole and follow with a sharp up to size drill. Do not peck the drill and feed it .007-.01 IPR.

Here is a link to EZBURR hole deburring tools

Mr. Mike

1 Like

This is what I do. A helical bore with a finish pass leaves little or no inside burr.

Thank you everybody for your suggestions.

We ran it today with slower plunge rate, no pecking and dialed in the depth which all culminated in less blowout. There was still a burr on the inside but it was much smaller and we grabbed a 0.75" square extrusion and just shoved it through the center of the tube and it removed the rest of it. The insides look great now. Thanks!

1 Like

came into this thread to suggest exactly this