We drill a lot of holes on our Haas CNC mills and we struggle with drilling clean holes in our aluminum tubing. For most parts, we drill all the way through both sides of the tubing and there are oftentimes blow outs or rough edges (burrs) left on the inside of the tubes.
Has anyone else experienced this? Any suggestions for reducing these rough edges? We’d like to avoid deburring 100s of holes by hand.
We are researching:
Drill bit materials and points
Feeds and speeds
Right now we use standard HSS jobber bits. Very conservative feeds and speeds. Probably 1000 rpm’s and 20 ipm plunge rate.
Aside from adjusting speeds and feeds, are there other drill bit types or methods that help with this type of drilling?
In general, I think higher surface speed will help you, so faster spindle speed and higher feedrate. On a Haas SMM2, I think I normally run about 8k RPM and 40 ipm for drilling .210 holes. Some nice sharp stub-length bits will help a little, but not nearly as much as better feeds and speeds. @sanddrag?
Maybe not quite “drilling” anymore but I have found that I get a little better results in holes by just using a slightly smaller endmill and doing a helical boring operation - it’s probably slightly less efficient then drilling if I nailed the feeds and speeds but I find it’s more consistent and as a bonus I don’t need to pilot. I think a lot of this probably comes down to the fact that in an FRC style shop endmills get abused less than drills…
Use Split Point drill bits, do not use chisel tip drill bits. They cut so much better. Also the shorter you go the better the finish in my experience.
Edit: Also, get HSS Cobalt if you can. Small price increase for a big tick up in longevity.
Lastly, DO NOT, I repeat, DO NOT buy any coatings for aluminum. It is a waste of money and they almost always hurt more than help. You want Bright Finish.
One of the best things you can do is get a copy of the Machinery Handbook - even one a few generations back is a treasure trove of information on machining specific materials. You’llLimelight, an integrated vision coprocessor get solid recommendations on speeds (expressed in Surface Feet per Minute typically so you’llLimelight, an integrated vision coprocessor need to apply the math to your cutter size to get the surface speed at the OD of the tool) as well as feed rates for different materials (and you’llLimelight, an integrated vision coprocessor find there are differences in “aluminum” such as 6xxx and 7xxx materials).
Feeding slowly can often cause problems because the cutter builds up a lot of heat which is not able to get dissipated. The reason the chips coming out of the holes are so ever lovin’ hot is because that’s where a lot of the heat is going - too small chips from a lower than optimal feed rate don’t carry the same amount of heat energy and you spend time rubbing the material and mot removing it - softer materials with lower melting point can reach the point where they start to get soft and can make the burrs even worse. Sometimes it’s best to just get in and get out.
Just about any drilling operation has the possibility (maybe even high probability) to cause burrs to some degree when the cutter breaks through; @Schmools recc of going with a smaller end-cutting end mill to plunge and then clean up the hole to final size will probably result in the cleanest interior holes because the final diameter is reached from a sideways load and not a plunging load which will tend to extrude material into the interior.
@RoboChair suggestion of using shorter drills is pretty much a winner every time as well. Jobber drills are really quite long - longer than you need in a lot of cases. They can deflect and end up not moving perpendicularly through the material can end up making oversized and even non-round holes (in extreme cases). If you’re doing a lot of the same holes, getting shorter, commonly referred to as “screw machine” length, drills is a win due to their added stiffness. I pretty much use screw machine drills as the main go to when I’m out in my shop and only go with longer drills when needed.
And keep your tools sharp so you’re cutting and not wearing the material away - when cutters get dull, they generate a lot of heat and tend to shove their way through the last remaining material at exit rather than cutting but it can be a challenge to get completely burr-free holes on a consistent basis.
From your pic I’llLimelight, an integrated vision coprocessor just say I’ve seen a lot worse so you’re in the general area.
If I am going to drill with a jobber in a CNC, I never bother but still prefer shorter if I have it. Split point still will cut all the way to the center, that is why they exist. Whereas chisel tips push the material in the center out to the edges where it can finally be cut. If you are center drilling without breaking through then splits are still better.
Not sure about the validity of split point making more burr, but I know for a fact the required thrust force to cut with them is much lower than a normal bit.
If you want to be super fancy, want absolutely zero burrs, and are doing a lot of identically sized holes greater than 0.093”, you can use an E-Z Burr tool on a second pass; it is designed to deburr both front and back sides. Prices look like around $80-90.
Promotional video:
This should be a last resort though; definitely try the other things recommended above first to see if you can get burrs down to an acceptable level.
Are you center drilling through both sides of the tube at once? I think that is where the split point shines - when you are trying to drill through both sides at once like the OP is.
If you know the magic to make that work well on a drill press (especially with bearing holes), I’d love to hear it. Our MO is to scribe both sides, punch, measure again, start with a drill-point countersink for a lathe, using a zoom on a camera to make sure that it’s set right in the middle of the punch mark (I have old eyes), then move to a stub 1/4", then move to a 1 1/8" annular cutter, flipping the piece end-over-end to do the other side. Lots of cutting fluid. Lots of peering to make sure the hole is exactly where you want it.
For our 5/32 rivet holes on a Haas TM-1 we use a reamer. The rivets call for a hole between 0.160-0.164
we use a 1/4" 90 deg spot drill,
followed by a 0.152 drill,
followed by a 0.163 reamer.
We put hundreds of holes in 1/16 wall tubing without problem. Sometimes there are some small burrs inside the tube, but they don’t affect the performance of the rivets.
We have tried drill mills to plunge into the tube and then mill the hole to size. It works great for larger holes and pockets. For example, McMaster-Carr.
Once the hole is large enough for fingers to fit inside, you can try profiling with an undercutting endmill such as, McMaster-Carr to deburr the tube. Deburring these features is important for the safety of your assembly team.
We have not used the E-Z Burr, but would love to hear how well it works.
I have learned recently about special bits that are both up and down cut bits. they’re called compression bits.
I dont know much about them yet, but I know they are typically for pocket operations. however they could potentially be used for this. I also do not know if they make any for aluminum or just wood, foam, and plastic. that might be something for you to look into.
Thanks for the recommendation. Ideally, we want clean holes on the inside of the tube and the backside. We can get cleaner holes if we don’t go through both sides. We could flip and run a separate operation but we prefer to drill through all in one op.
You are always going to be left with straw hats or a burr with a twist drill in aluminum. I know it doesn’t answer your question but we finish all drilled tubes by scraping out the inside walls with a long piece of 1/4" ABS strip. Prevents any stray chips from getting places where we don’t want them.
