A 16mm end mill with a 1/2 shank?

Why do you need one? Is a widening toolpath not an option?

I have a few pieces that need a precision 16mm hole sunk 5mm deep for a bearing. Since this is a production piece I can't cut any corners. I don't think that my router will be able to hold the tolerences unless it's a simple plunge down. There is possibilty of using a reamer to enlarge the hole by a few thousands for a perfect fit but the depth needs to be precisely controlled.

If what you are wanting to accomplish with the 16mm is quicker cutting time via a single pass it may not be worth the added expense since what you would save in time is minor on small RC parts. If you were machining thousands of a single part then of course this timesavings would be a real factor. Does it really make a difference if it takes a few extra minutes, I used to think so but Ward got me out of that thinking a while back, so now I just try for clean tool paths and do not get all that excited about optimizing for speed.

Ken

If I could make it work with a longer cycle that would be fine but that's not the case. The tolerence needs to be at least .001 for the proper fit. This item is a bulkhead which ties together most of the suspension so a lot depends on it.

Don't count on an endmill used as a drill to make an accurate hole. You really should try to interpolate it with a smaller endmill. If you can't use radius comp, you can just keep regenerating a new path in OneCNC until you get a fit. Keep the feedrate low, because the tool might be performing a wee tiny orbit inside the hole, while the effective feedrate is much higher out where the cutting is happening.

Most end mills I have seen are +.000 -.001 so that may work out to your benifit. Now the search for a 16mm end mill in the USA :)

BTW, reamers will not ream down to a square cornered hole bottom. You'd have to check how much fillet the bearing race has, and whether it would foul on the reamed chamfer left in the bottom of the hole.

If you can't interpolate the hole, then a small adjustable boring head would serve better.

I was looking at the indexable boring heads but my rpms might be a problem. The minimum I can spin is 10k.

By the way Hu, I really am grateful for all the advice you've been posting. Since I'm new at machining there are many little things I have yet to learn. Eventually I'll get there though with the help of this forum.

You're welcome, Andrew. :)

Have you experimented with circular interpolation of the hole to see what kind of results your machine actually gives you? Is this aluminum you are working?

Do you want to actually press fit the bearing, or just slide it in? .001" clearance is actually a loose fit, .0002 clearance will start to feel like there's some "grip" to the fit. 0 clearance is tight, and .001 interference is very tight, and in aluminum, the bearing will most likely gall the hole when you press it in with interference.

For production purposes, you might be able to get away with circular interpolation of the hole, getting from 0 to .002" clearance, then cementing the bearing in with Loctite bearing mount compound. This is actually better for the bearing than hammering it into position anyways. There are various strengths of Loctite available, depending on how much effort you want to put into getting the unit out of the hole afterwards.

I did a few test passes but right now the machine is without a controlling computer. The parents did not like the fact that I had taken the office computer to the shop for it. I'm going to buy a computer from ebay tonight but until I get it....

Slide in would be fine. There will be a very slight amount of preload being exerted on the bearings by the bulkheads so it's not critcal to have the bearing grip the part.

Here is a shot of it. The green structures holding the black diff are the bulkheads I am referring too.

You wouldn't want to Loctite the bearings into that, I guess. Disassembly would be too difficult. Boring would be the way to do it right. But at 10000 rpm, interpolation might have to be what you'd settle for.

There may be another solution, but I don't know exactly what they are called. Electric motor rewind shops use a special wear sleeve to repair light duty motor endbells that have worn out. The procedure is to bore the worn bearing seat out, then insert this special "corrugated sleeve" material (cut from a bulk roll, I believe), into the hole. The corrugated steel sleeve crushes slightly the first time you press the bearing into the hole, and creates its own correct fit. The hole tolerance is quite wide on boring the hole, because the corrugated sleeve can be crushed more or less, as required. This might be the type of thing your cnc machine could handle for accuracy. You might have to machine the hole out to 18mm or something, to allow space for the corrugated sleeve material.

By analogy, the corrugated sleeve looks kind of like the wrapper on a Reese peanut butter cup.

Andrew,

I have to agree with the guys here. I don't think you will be able to plunge a 16MM end mill at 10,000 rpm in to your part and end up with very good results as far as a bearing bore goes.

My guess would be that it would squeal like a mashed cat at that speed. Not to mention chatter.

Even under the best conditions with a rigid spindle and machine it is difficult to get a 16MM end mill to make a precision 16MM hole by plunging into the work. Pre drilling would almost be a necessity. Leaving only a couple of thousands to clean up.

At 10,000 rpm even with a good spindle and holder there is some run out. And to plunge with that, then there is the deflection that will inevitably occur as the tool fights it's way in.

But I have an Idea that might work. How about using circular interpolation as suggested. Making sure you a little over sized, for a nice slip fit.

Then as in the picture below drill and tap a set screw hole into the bearing area. And lock the bearing race from turning. That way you don't have to be as picky about your hole size.

Looks like you may be able to use one of the existing hole in your bulkhead from your picture. Just drill all the way to the bearing bore. Tap it thru and then install the set screw. Then the regular screw could go in on top of the set screw.

Looks like the assembly is captive from the design. So all you need to worry about is rotation. Just snugging up the set screw should take care of that.

Also Criterion Machine works just came out with a sub miniature boring head, about the size of a dime. I can't find it on their web site but here is a link. You could e-mail them as to info. Maybe ask if it will handle 10,000 RPM.

http://www.criterionmachineworks.com/

Squeal like a mashed cat :D

The hole might be perfectly okay if you invent a new name for the finish: "vibra-bored bearing housings" ;) Sounds like something you'd have to pay extra to get :D

Why not plunge with a smaller bit to establish the position, then drill in a drill press. Clamp your piece to a piece of plywood or similar so the drill does not break violently through. If it's not a through hole, the bearing won't matter if the bottom of the hole slants away. It will seat against the edge.

Squeal like a mashed cat

I've actually heard a mashed cat squeal (broken overhead door at our old shop). Terrifying. :)

Why not use a 1/2" endmill, do a vertical plunge to clean out most of it, then go back and do the circular interpolation? Maybe add a clean up pass if you need it.

A 1/2 end mill at 10 000 rpm in a router based CNC? Sounds like a bad idea.

I agree with the guys as I did 4>500 precision 17 mm holes for bearing pockets last year using the method you're thinking of!

I was using my manual Mill and the best results I could get were using a slow by comparison speed of around the 700 Rpm mark.

I first cut to within .25 from the finished depth with a 16 mm End mill then a finish cut with the 17 mm slot drill this gave me an exact pocket as long as I stopped the spindle BEFORE withdrawing from the workpiece.

I also agree with Hu's suggestion to try a smallish end mill around the 6 mm size with circular interpolation.

Draw your self 6 holes starting at 15.5 mm and increasing .1 each time then drill a through hole to say 12 mm in each and then run your program to cut each to size with the 6 mm end mill!

You may need to experiment with DOC and spindle speeds to get the finish you need. (I do mine with 2 mm DOC x2 for a 4 mm wide bearing leaving .25 for a full 4mm finishing pass)

Once this is done run your vernier over each hole and pick the one that's closet to the required fit and this will be YOUR 16 mm hole! ;) (This is how I'd do it in your place and how I've done it here.)

Just got back from machining some bearing mounts. I'm getting a tight press fit on the recessed 16mm hole with a brand new 1/4 carbide.

Just had to think inside the box.