In attempting to make a couple of hubs this year, we bored out some aluminum stock, like ya do, on our lathe. We used a 1/2" bit since the motor shafts are a 1/2" diameter. However, the holes were too press fit for our liking – we wound up having to sand down the motor shaft a bit in order to get the hubs on the motors.
In the future, I’d like to alleviate this. I’ve noticed that AM’s sprockets and some gears come with a 0.502" hole – which is great because it takes no effort to put on and remove their hubs (well…most of them ;)). However, in my searching I’ve come up blank thus far in looking for a drill bit larger than a 1/2". Any suggestions? I’d like to find a better solution than grinding down a shaft.
The process is to drill (or bore) the hole slightly undersize, by a few thousandths, then to use the reamer to open up the hole to the precise diameter.
I’m sure others will jump in here with more precise instructions.
And MSC also sells drill bits larger than 1/2". They used to have a discount for FRC teams, but I don’t know if that is still the case.
If you don’t need a precise fit, you can waller out the hole with the drill
If you do need a precise fit, a hand reamer is the way to go. You can buy them in exact sizes, or you can get adjustable reamers. We’re lucky, the fab shop we use on Ft. Huachuca has a nice set of each, from very small to an inch diameter.
Invest in a solid carbide boring bar (assuming you have a lathe). Many are available that you can use on various size holes and get the exact fit you desire. Try EBay, as I have bought some brand new at very low cost. Also make sure the shaft you are fitting to doesn’t have a burr left on the edge, as this will give you a false oversize reading on the shaft.
If you have a lathe and are willing to take the time to learn how to do precision work, you can use a **boring bar **to make the hole whatever size you want.
Btw, all kidding aside, according to my drill chart right here the closest drill size to the one you want which are standard ones are either:
the 1/2" one (.500") or a 33/64 (.5156") drill bit.
In metric the closest ones are either:
a 12.50mm (.4921") or a 14mm (.5512") drill bit.
I’d suggest that however you start, end with a reamer.
1/2" shaft is something you’ll probably be working with for a long time (And 3/8" for that matter), so you really should get the equipment to make the appropriate hub.
I suggest you actually get a .501 reamer, that’s what we use and it works just fine.
Assuming you don’t have them already, a .376 reamer and a broach set to put a 1/8" keyway in both 3/8" and 1/2" would be a very good investment.
I second…or third…or n… the idea of using a reamer…
Proper fit in a hole is made by using a reamer. You can start the hole with a drill… or bore it out…but the final thousands are taken with the reamer.
Reamers for .5, .375, and .25 should be part of any team’s toolkit…
(rather .501/.502…etc) to use with 1/2", 3/8", 1/4" shafts.
If you are looking for press fits… you may have to purchase different reamers that will make the necessary pressfits for your bearings or whatever else you want to press in…
As others have mentioned, an oversized reamer is a great way to go. You can definitely bore precise holes using a boring bar, but using a reamer is a bit faster.
I would suggest you get an over / undersized chucking reamer set. Enco’s cheapest set is currently $59.95 (china’s finest, prefer american, but these have served us well for 6 years). These sets come with 14 reamers (reamers are .001" + and - of standard chucking reamers centered on 1/8" - 1/2" sizes by 1/16th increments)
The great thing about an over/under size set, is that you can use the undersize reamers for pressing fitting pins and shafts (some bearings) and use the oversize ones for slip fits.
Also get a standard size reaming set from 1/8" to 1/2".
While we are talking about reamers, other useful reamers that we use for FRC include .874", .875", 1.124" and 1.125" which really help if you want to install 3/8" and 1/2" ID flanged bearings like the ones used in Andymark gear boxes. We use these all the time and make life a whole lot easier. Since these reamers are on the large size, we have had to turn down the shafts so a standard 1/2" chuck or a 3/4" collet could fit them.
I think we also have a .315" reamer which we use if we are installing custom gears to a CIM motor. remember, the shaft on a CIM is metric 8mm (.315) not 5/16" (3.125). Probably would be better if we had a .316" reamer.
Remember, these reamers can be used in a lathe or a mill.
Typically we bore or drill hole sizes about 1/64th" smaller and then ream them to fit. Do not run the reamer at typical drill speeds. Run them much much slower and with lubricant for best results.
Oh, one last thing. Make sure the pulley, wheel, hub or whatever slides over the shaft before you final broach it. Can’t use a straight reamer to open up the hole once it is broached although a spiral one might work if you can find one.
Question…What material is the shaft? If it’s aluminum, it will tend to be barely just too big. Steel .5" shaft fits perfectly though…at least that’s my experience. I got a flywheel machined and tried to put it on a .5" aluminum shaft and it barely wouldn’t fit. So I took it to home depot to try and find another aluminum shaft that might fit (different batch, right?). All of them gave the same result. So I tried the steel shaft, and it fit perfectly.
The two shafts are made with different tolerances.
Standard 0.5" aluminum extruded round will be somewhere in the range of ±0.005" on the diameter. It’s never going to be 0.500" even. You would need precision ground shaft. Even with precision ground shaft, you could have anything from 0.500" to 0.4998" (for example, using McMaster standards). If it’s 0.500" even, it’s not going to go into a 0.500" hole.
The tolerance on steel round stock is generally +0 and minus a few thousandths, leading to your shaft fitting nicely into a 0.500" hole.
Team 975 once had to hone out a pair of 5/8" bore flanged steel sprockets to fit a 16 mm shaft. I figure it was probably .004" or so. We used a 5/8" shaft in a drill press and a lot of valve grinding compound. It took a lot of time but the fit was beautiful. Next time that was needed, we just spun the shafts and sanded them down to fit. Much easier.
