Hi guys
Our team is currently working with our sponsor and we were wondering what size our bearing holes should be for a fr6 and fr8 bearing press fit? Should we do a .874 - .873?
Also if we anodize, our shop said its a .001 penetration and a .001 surface finish. Should be go to a .875 - .874 hole? our teacher and I don’t really know how to do this.
Thank you very much
0.873 inch is way too tight. 0.874 inch is still tight. 0.8748 is just right.
AndyMark shows bearing pocket dimensions in their plastic wheels 0.001 inch smaller than nominal bearing O.D. In those wheels the plastic gives a little when you press in the steel bearing. Aluminum will give also, but not as much.
Good practice for pressing bearings of this O.D. range into metal pockets is 0.001 mm to 0.010 mm smaller than nominal bearing O.D. – that would be 0.00004 to 0.0004 inch. That tolerance is very difficult to control using the tools of most FRC teams.
If tolerances can not be held, A bearing spacer can help solve the problem. Search Mcmaster-Carr for bearing spacer to see what they look like.
Because my team’s equipment was not more accurate, I always went 0.001" under and put a generous chamfer on the hole to help in pressing the bearing in.
You could also aim for a close fit and glue the bearings in or peen them in. I’ve had good luck peening in flanged bearings.
If you use flanged bearings and then trap them with spacers/collars/nuts/snap rings, you can get away with a pretty sloppy slip fit.
Even on a drive train with 25 chain?
We have been anodizing our robots for the past 6 years. There are two ways to deal with the press fit bearing holes.
I highly recommend going with method #1. We have had to clear away anodizing inside a bearing hole many times because the press fit ended up being too tight. Year to year, batch to batch, we just couldn’t get a consistent enough thickness on the anodize where we were comfortable using it as THE press fit.
Just my opinion based on our experiences in the world of anodizing.
-Brando
A standard Type II color anodize should not add any more than about 0.0004 inches. A hard anodize certainly would. I second the recommendation to capture the bearings, and size them for a close slip fit. Pressing them is nice simply so they don’t fall out during maintenance but it’s difficult to get the perfect fit. You’re looking for in the neighborhood of 0.0003 smaller.
Unless you have a high-end shop doing the work to your tolerances and inspecting it, be sure to give them an actual bearing they can reference to check as they’re machining the parts.
Yup.
For the last three seasons, all the sheet metal parts on 228’s robots have never had actual press fit bearing holes, simply because that would cause our sponsor to have to swap out a standard size die (0.875") for the less common press fit size in the turret punch.
We’ve dealt with this two ways: 1) use flanged bearings, stepped shafts and Delrin spacers to keep everything captured, and 2) put some Loctite around the outside of the bearing when inserting it the first time.
For a FRC robot that will literally only see tens of hours of operation, this works just fine.
Something like Loctite Press Fit Repair 660 works great in this sort of application.
Thanks for the tip Arthur. 
We just used the same Loctite 248 we use for everything else. 
// Which is also a great tip for all robotics teams: ditch your liquid Loctite and switch to Loctite 248. This is available in a “QuickStix” form (it’s basically a glue-stick) and is more or less impossible to spill or drip on things. Before 228 switched to this, our students used to constantly spill and waste Loctite. Now, one tube seems to last forever.
We make most of our press fits for bearings .0005-.0002 undersize. Even attempting this without a CNC machine is a waste of time, IMO. You’re better off just reaming it to the nominal size and using some of the green wicking loctite to retain the bearing. It’s as good as a press (and absolutely will not let go, without extreme heat).
Side topic – somewhat related I suppose –
For a 1-1/8" (or 1-1/16") Silver & Demming bit that would cut into 1/4" Polycarb and/or 1/4" Aluminum …
… would we want to get a carbide-tipped bit or would a HSS bit suffice? This assumes that S&D bits can do the 1-1/8" hole without too much slop, which also assumes we would do starter holes with a smaller drill bit first. It would also be done on a mill we’ve been able to get within 1/64" after nominal practice.
HSS would definitely suffice, though I prefer to get coated and/or carbide tooling because it is so much more durable. To quote the machinist I worked with at my college: “it costs twice as much, but lasts five times longer.”
My opinion is that for 1/4" and thinner you’d be better off with a good quality step drill, hole cutter, and/or reamer, depending on what sort of fit you wanted. I don’t like how big drill bits like that are not very forgiving. They can make ‘triangle holes’ and catch big burrs and spin parts when they’re used in thin material.
I’ll echo this as well. Bearing holes are always going to be the same sizes, 0.875", 1.125", etc. Investing in a couple of reamers that only do that job will last the team forever, and give you accurate, repeatable results.
-Brando
For Loctite, 680 is good stuff. It’s the green gap filling formula. I wouldn’t necessarily use it to hold a gear to a shaft rotationally for instance, but man, that stuff does not budge once cured. I once glued a steel gear to a steel shaft with it and it took about 5 minutes with a propane torch, a vise, and the biggest pair of channel-locks I had to get them apart. Good for holding in bearings when you mess up the press fit tolerance.
I remember Mike from 233 telling me he would have gearbox plates waterjetted with the bearing holes a little undersized and simply run a reamer through them on a bridgeport while letting the plate “float” on the table. I was surprised they could hold an accurate enough center distance that way but apparently it works.
A 1 1/8" silver and demming drill will not make a 1.125 hole, nor will it make a round hole, especially in 1/4" just due to the size of it. The tip of the drill is more than 1/4" tall. You can do it, and it will work, but the hole won’t be great. You’ll be lucky if it ends up 1.127 which is a bit sloppy. You’ll have to run down somewhere around 250 RPM too.
If you’re working on a manual mill I suppose you could drill and ream. Do something like drill 27/32 or 55/64 for the 7/8" OD bearing and then ream to .875ish and likewise (a 64th or a 32nd undersize) for the 1.125 bearing. They make reamers that are .0005 undersize.
You perhaps could try something like a TCT hole cutter to do it all in one shot. I don’t have experience with them though. I’m guessing your results would be better with a reamer.