Has anyone experimented with using a carbide 1.125 inch bowl and tray router bit as a final pass on your bearing holes when using a CNC router? Like the one below, thoughts? Any idea on the tolerances on a bit like this one?
A combination of the motor not having enough torque, a low enough rpm, and the router not being rigid enough means the reamer would chatter alot. We have had success making our holes around .015 inch undersized and reaming them out on a drillpress.
Ditto
We had some custom reamers made a while back. We go .015 to .01 undersize and then ream (press fit thanks to custom sizing )
For anyone curious,this is the reamer we bought off ebay. We got two of em and they’ve been great. We are lucky that our Drill Press spindle and Clausing Lathe tailstock both have Morse Taper 3, so we can use the reamer on both machines effortlessly.
-Mike
As a machinist, I would recommend an offset boring tool. You could put it in the drill press and then bore any sized hole you would like.
I used to use an offset boring head, but after a couple years I got (extremely) lazy, especially because switching to the boring head required me to drop the knee of the mill 3" or so. Now we use positive bearing retention everywhere and 1.125" holes.
My method is to drill with a 1/2" drill first (largest one we have), then go in with a 3/4" then 1" endmill. After that I finish up the hole with a 1.125" endmill. This gets some tight slip fits and a very round hole.
My dream is to own a 1.124" reamer, but the $200 cost for a custom one doesn’t suit me too well. 
Given that we use a manual mill anyway, it doesn’t hurt to use the 1.125" endmill we already own.
Im not sure if this is the exact model we have but this is what my team uses. We spent some time last offsetting setting it to exactly 1.124 and we never change it. The CNC router gets us to 1.12 ish and we manually clean it up with this:
I got my 1.124" reamer for $52 shipped on eBay. Brand new. Keep an eye out for them!
That bit is NOT a reamer, and don’t count on the tolerance to be down to 0.001".
As others have said: make the hole several thousandths undersize and use a hand reamer to make it half a thousandth (or so) undersize.
EXPERIMENT in the off season!
Boring heads are great when used on a mill, but there is no good way to use one on a drill press. There isn’t really a good (safe) way to hold your work or locate the center of a hole. The spindles in drill presses are not designed to take the unbalance load from a boring head.
Another option is to ream it to 1.125 and then use locite designed for beating retention.
You could also polish a 1.125 drill or mill slightly under sized on a lathe with Emory paper. (Run the lathe in reverse). Taking off 0.0005 should be easy with HSS.
Lapping compound is another option.
If you can chuck it in a lathe, you can bore it to half a thousandth with some care.
An experienced mentor machinist with a Starrett micrometer can achieve half a thousand on a nice big lathe that well is adjusted.
An above average student machinist on a mini-lathe using $15 digital calipers would be good to hold 0.002".
My point was either end of the machinist spectrum could take a 1.125 mill or drill and undersized it enough to achieve a snug R8 bearing fit.
I don’t think that this is what you’re looking for, but we used this step drill bit to clean up bearing holes in our waterjetted pieces this past season. It can put a 7/8" OD hole into 1/8" thick material, or run through thicker material with a 1.125" OD hole. Just the right size for the 3/8" and 1/2" bearings we all use.
Step drills are cheaper than reamers, but they can wander if you are taking off a lot of material. Our gearboxes worked great, but we had padded in an extra .003" between adjacent bearing holes to prevent gears from binding if things were off. If you want tighter tolerances, you probably don’t want a step drill.
I can get to half a thousandth without too much care on the small Taig that the woodshop teacher owns. If one is using a good pair of Brown and Sharpe calipers or Mitutoyo, those hold to 0.0005" easily. Of course, maintaining a “good pair” of quality calipers is difficult in a student’s hands. 
Ironically, I find that using a telescoping gauge and micrometer is harder for me than just trusting the calipers, although either method isn’t impossible.
Back when we used to use the boring head, all measurements would be taken on the B&S calipers, well before I was on the team. They were able to get reasonably good presses on bearings, although I don’t know what the skill level of the people were before I was there.
That being said if I tried to get that tolerance on steel, I wouldn’t have much luck.
Drilling a 1.125" hole with a drill bit I would try to avoid. Using an endmill will get those tolerances but a drill bit won’t hold the tolerances easily unless you drill undersized by 1/64" or something first, and even then I’m not sure. The largest hole I have drilled in metal was with a 7/8" drill bit, and that did not go as well as just using an endmill of the same size. What is your method to make sure it works correctly?
Most 1.125 drills have a 1/2" shank. You simply can put that in a 1/2" collet and use it in your mill.
My students could hit 0.001" easy with any lathe we have(maybe not the Grizzly) my experienced lathe students could hit that ± 0.0005" most of the time with a few pointers. But really reamers are the way to make it easy, you can make your own for cleaning up holes if you have patience, spare time, and some tool steel.
My favorite “bugdet” calipers by the way are a $35 pair of Fowler digital calipers from Amazon
I will second the step drill method! It’s super fast and easy and in my opinion is SO worth the $45 or so it costs. It will post size your holes and will be solid as long as you use positive retention like rivets or retaining compound.
My personal favorite method for making a 1.125 hole in aluminum has to be a Carpenter’s Spade Drill. I am dead serious here. It probably won’t be fantastic for gearbox plates but with a little time on the grinder to modify the bit it will make a press fit hole every time. The only major limits on this method is it can’t go through much more than 0.125 thick material and nothing tougher than aluminum. You should never try and do this by hand, not really for danger reasons, it just won’t work. Your puny meat fingers aren’t as stiff as a drill press. Below is roughly what a modified spade bit looks like.
http://i.imgur.com/YKncQJT.jpg
If you don’t believe me watch AnthonyDV drill a hole and hand press a bearing in. :ahh: 
https://youtu.be/yIonCvyEFks?t=29m40s
There seems to be a misconception of the accuracy that can be achieved on an average small or mid-size lathe with a 3 Jaw Chuck.
Most three jaw chucks have some run out, not holding the work perfectly centered. You can measure this run out easily enough, and it will be much larger than 0.0005 on almost all lathes. This is not much of an issue if you don’t move the work, and use a cut-off. As soon as you move the work in the jaws, or use some of the chucked length you will introduce inaccuracy.
Extreme accuracy requires use of a collet work holder, well-adjusted gibs, a very stiff tool post, and quite accurate measuring tools.
Runout != diameter tolerances. Although getting concentricity with a round face is affected by the runout, the bearing press fit diameter is not affected.
The freshly rebored taig jaws had around 0.0003" of runout, and have probably increased to beyond that since I last redid them.