Training the Veteran Rookie Coach: Press Fitting Bearings

Hey all,

As I’ve said in the past, I have been a coach for ten years but have only taken on the technical aspects of robot builds over the last year or two. So there are times when I have very rookie questions.

I see discussions about using bearing blocks vs press-fit bearings and for the life of me I can’t figure what it means to have a press-fit other than cutting a hole and sticking the bearing in.

Would someone please dispel my ignorance?


Press-fit just means that the hole for the bearing is very slightly undersized compared to bearing. You use an arbor press or similar to force the bearing into the hole, and then it’s held securely. The thing is, for a proper press fit, the bearing bore needs to be quite accurately made: very circular, and to the correct size within a thou or so. If the bore is slightly too large, the bearing falls out; if it’s slightly too small, you can’t press the bearing in. If you have good tooling (a CNC mill (not router) in most cases), you can machine press-fit bearing bores in your drive rails (or wherever). If you don’t have precision machining capability, you can buy bearing blocks, which come with the precision bore already machined, and which just clamp onto your tubes.

I hope that made sense.

As a follow-up question. What amount of undersized-ness should I aim for on bearing holes?

For a complete answer, any good mechanical engineering textbook should have a big section on clearance and interference.

As a rule of thumb, for FRC-standard 1-1/8" OD bearings pressed into aluminum, I usually shoot for 5 tenths under, or 1.1245".

If you can’t hold those kinds of tolerances, there are plenty of workarounds. One (in)famous technique for fitting bearings into oversized holes is to use a spring punch to make upsets on the inside surface of the bore, thus slightly decreasing the diameter. A better technique is to design mechanisms so that your bearings are geometrically constrained. This generally means using flanged bearings, and arranging them so that spacers, or steps in the shaft diameter, or something rest against the flanged side:

The idea is that if you’re not relying on the interference fit to keep the bearing in the bore, you can get away with much looser tolerances.


We aim for press fit when we can, but we ALWAYS constrain the shaft anyways. Tapping the end for a bolt and washer, along with spacers, doesn’t weigh much and it gives you that added security of having everything exactly where you want it.


You guys shoot for 5 tenths under?

We made a bearing test plate with exact, then increased from there having + and - ten thousands for ± .0001 all the way to .0003 and found -.0002 to be the best.

As a follow-up, why would a Cnc-router not work?

For making precise holes? It might work if its resolution is high enough.

-0.0005 is definitely on the “more-smaller” end of the scale. But I like to be a little conservative there: if the hole is slightly too small, I can push harder on the press, and if it’s way small, I can go in with a reamer or sandpaper. If it’s too large, then I’ve scrapped the part.

What @Amicus1 said. A router might work, if the machine and workholding are really rigid, and you have it dialed in well. But in my experience, CNC routers tend not to be able to hold better than a few thou, especially in something like circular interpolation where the axes are changing direction.

What are you guys using to machine that’s accurate to 0.0001? For that matter, does anyone know what tolerance a standard thunderhex bearing is made to?

That does seem pretty fine. Our Haas Super Minimill 2 has a resolution of one tenth, and if we’re careful with the tooling we can hold tolerances of a couple tenths. Trying to change hole diameters in 0.0001" increments, though, I’d start worrying about quantization of the motion.

Your new router should do the trick. When you have it up and running we can come over and help get it dialed in.


I’ve seen some .5in Hex bearings that dont like to fit into 1.1245 holes but with our experience this is completely solved with tunderhex.

answering the op, we typically aim for 1.1245 on all our high load, GEAR MESH, applications. This typically involves taking a roughing pass, probing the hole, and adjusting the cam accordingly. This lets us nail 1.1245 every time regardless of tool wear. I understand most teams dont have fancy CNC probes and if we didnt I think we would be shooting for something in the 1.125-1.126 area. The key thing is trying to keep your gear center to center +.002.

For the 99% of other bearings on our robot we go for a 1.127 fit. We have found this is a nice “snap fit” so repair is quick and easy but bearings dont fall out when trying to assemble things. We like to belt all our subsystems and undersize our belt lengths quite a bit (-.02) so this is well within our tolerances.

1 Like

Daniel-- don’t let these guys scare you with their tenths. You don’t need to hold tenths to make high-quality FRC robot parts. Plenty of teams, every season, make bearing bores with the crudest of tools.

Your question is asking why press fits are advantageous. I would like to suggest that they are not advantageous, because press-fit parts makes it more time-consuming to execute time-constrained repairs in the pit. We want the bearings to be installable/removable by hand. That’s why Triple Helix prefers to machine bearing bores that are a nice slip fit over the bearing… something “a few thou” over the nominal dimension. Axial retention of shaft components is accomplished using part geometry (e.g. section changes, flanges, snap rings, and axial retention screws) instead of the uncontrolled fits.

There are a wide variety of tools that could produce a bearing bore with a tolerance of “a few thou”. Yes, a cnc router table is probably one. Many others are discussed in this thread.


This is my go to reference on pin & bore tolerancing

1 Like

This thread has a lot of good discussion about different methods for machining bearing holes.

1 Like

This is an excellent video. I can’t seem to find the tool brand or link. Anyone know what brand cutter is being used?

Yes. It’s a Hougen RotaCut tool. Links to MSC product pages are in the video description. You need both the cutter and the arbor.

Agreed. We usually cut our bearing holes to 1.126" and it’s never caused a problem.