Drilling Holes Through Copper with Extreme Accuracy

For reference, I am a student worker at the local college with what I would expect to have the skills of a semi-skilled hobbyist. Also, I am using a Tormach 1100MX, Fusion 360, and a drilling bit with a 6in flute.

Into the problem, I am machining holes through three-inch segments of copper for use in Ph.D. experimentation; therefore, the closer to perfection the better. The end goal is to have 8 individual blocks of copper that must align perfectly with one another, all with the holes in the center. I have been using Fusion360 to model this and mill with a Tormach 1100MX, aligning the stock with a machinist square, and using a probe to find my WCS. No matter how accurately I have measured or trued my pieces up the mill cannot accurately drill through the centroids of these pieces. After realizing that the pieces I had cut were not lining up I tried several things to check my work, the addition/subtraction of coolant, using a pilot hole with a center drill bit, and slowing my plunge rate. I expected these pieces to have much higher accuracy than they were coming out. I have tried everything I know, and I am out of ideas now. If any skilled machinist can lend some much-needed knowledge, it would be greatly appreciated.

I have been pecking the drill bit through the 3-inch section of copper. I have come to the conclusion using a drill press might be best, but I would appreciate others input.

A bit better description would help. Define ''extreme accuracy''. What size holes? 3 inch thick solid copper blocks? What does not align? Is the hole in the same place on one side of the pieces and then walks off at the other side?

Pictures of your setup would be helpful.

A 6 inch flute for a 3 inch part is excessive, try a shorter tool. You can also try a carbide tool as that will be more rigid. Make sure your tool is running true, drill chucks will add a little runout which can cause the hole to walk. Also, you'd be better served machining the outer profile in the same operation as you are drilling. Probes/edge finders/squares can all add some minor tolerance to your setup. If you start with a piece of raw material and profile it and drill without moving the material in the machine, you will likely see an improvement in the positional accuracy.

Not really sure what you expect to gain from a drill press, it's going to be far less repeatable than the mill. In the end, spot drill, stub drill, through drill can help with accuracy but bear in mind the capabilities of the machine. .001-.003" positional tolerance is pretty doable on these things but you're unlikely to do better without a LOT of work.

As a final option if the parts absolutely MUST BE IDENTICAL would be to drill them all while they still have a bit of stock left to remove on the profiles. Then use a gauge pin to line them all up, stick them in the mill, and cut the profile, one side at a time, on all of them together.

If the hole on one side doesn't match the other side it's because drills rarely make straight or on-size holes, and the longer and thinner the drill, the less likely that is.. You can try and mitigate it by setting up a lot of pecks in Fusion to try, or find an on-size (preferably carbide) endmill, drill undersize the depth of that endmill, then drill with the endmill as far as possible to straighten out the hole start, then continue with an on-size drill (try coming in from both sides if mismatch in the middle isn't critical). Jig-boring is the traditional way to make holes round and straight but there's likely not one of those around. If the hole is big enough to accept a boring bar, you could do that.

hy :) a drill delivers best cilindricity if it is being used inside an existing hole

for example, if you only have a drill o10mm and expect to achieve a hole as cilindrical as possible, then use 1st a o9.8/o9.9, then change to o10 and recut only the walls

for pair parts, if possible, cut through all at once

however, this may not be enough for you, depending what tolerances you need; maybe you need a more rigid aproach than what a drill can do ? if you wish, share more stuff / kindly :)

Are you moving the table for each part or just changing the part with a fixed stop?

If moving the table, try approaching the center line from the same direction every time including probing one corner and just measure the square. (old school manual machine method.) and using G01 with a reasonable feed rate, maybe 10 or 20 ipm. This will reduce any issues with backlash or overshooting from moving mass.

I have a PNC1100 and this is not a .0001 machine even though the readout says it is.


NyCnc did some videos on tuning up an 1100 that might be worth watching if backlash is some of your problem. Downside to tightening up too much is additional wear.

Dave

Deep holes in soft sticky copper?
A PhD in itself.

You need to redesign the experiment.

Cheers
Roger (PhD)

This might be a job for an abrasive waterjet. Any drill bit that sticks out 3 inches (let alone 6) will wander a little.

I still say the experiment needs to be changed.

But if it really is a $64M thing, then start with Cu blocks of exact external dimensions (easy)
1) mount each block in the same jig, tightly. That deals with the centering bit.
2) drill each block undersize.
3) make up two 5 mm thick hard steel guide plates (use above jig) with the right sized holes in exact centre
4) buy a very long reamer (it will have to be custom, and it will be $$$, and a drill bit will NOT do)
5) mount maybe two or three Cu blocks together between the steel plates with the outside surfaces precisely aligned
6) ream the Cu blocks out guided by the steel plates
7) ask for a pay rise

Cheers
Roger

What is the actual size of the hole?
This is quite important!

If the hole is of a decent size, could you use some hard-drawn copper tubing to provide the ID, and clamp the copper blocks around the tube OD?

Cheers
Roger

Following on that suggestion, you might start with half-blocks of copper, face them off flat and mill trenches down the middle of them with a ball-end cutter to make 2 matching blocks that, when assembled, will form a straight hole. You can bolt them together or if that's not sufficient, solder them in a kiln. A reamer will finish the holes to perfect cylindricity (is that a word?).

Really precise drilling is hard to achieve with ordinary workshop tools.Would it be feasible to use a boring bar with all the segments assembled and remove the last smidgen in a couple of careful passes?It used to be a way of achieving the final cylinder dimensions for model steam engines if the only machine available was a lathe.The cylinder was mounted on the cross slide and the boring bar supported by the tailstock.

What is extreme accuracy ?

Look at the german machine tool builders for inspiration.
Hermle is a good example.

One can easily achieve 0.01 mm cylindricity and straightness..
and about 0.002 mm roundness and TIR via ball sizing and dual reaming.

But You need a Mazak Integrex or hermle for the first part, and a custom carbide tool to bore the 3" deep hole.
Or an air spindle, in a T&C cutter grinder.

Or an NSK spindle, for boring, with diamond abrasives, from both sides.
Preferably on an air bearing rotary table.

In all cases, metrology and gaging will be a challenge.
You could make custom carbide gages, my preferred approach.

They are likely to be fragile and easily snap if the holes are not straight.

Drilling say 4 mm holes to 0.01 mm true and 0.002 mm TIR, 75 mm deep, in Cu, ..
Is likely something that would cost 14.000$ per hole.

Let us know how You make out ...

Make sure the parts are squared-up accurately, and you have a fixed stop on one end.
Then, Spot Drill FIRST! To help keep your long drill from "walking".
Spot Drill one side, then FLIP the part, and spot drill the opposite side.
Next, Drill an UNDERSIZED hole, (at least .015" under final diameter), one side halfway thru (1.5" deep), and FLIP the part.
Drill the second side halfway thru to meet the first drilled hole in the middle.
Lastly, REAM the hole the way thru to final diameter.
The reamer will follow your pilot holes that meet in the middle.

Another hint: MILK is a great cutting fluid for Copper. Believe it or not, it's an old timer's trick.
Just make sure to clean-up REALLY well afterwards, or your shop will STINK!!

I haven't had to work with copper yet.. Any difference between a straight reamer or possible a spiral down reamer to push the strings out?. I suspect keeping the part cool would also help. When drilling Ampco bronze it wants to grab the drill when it gets hot.

Dave