What's new
What's new

Help with milling hole for bearing press fit?

Unless it was not explicitly stated,
the reason for using a boring head
and not using interpolation, is the
boring head will make the hole as true
as the condition of the spindle bearings
of the machine. It does not compound
the inaccuracies of the ball screws and
associated parts, which themselves tend
to make for a 4 sided hole rather than a
true round hole.

--Doozer
 
I just started reading this thread and I think I'm getting as much entertainment out of reading it as Doozer. Nice practical machining tips for a home shop machinist like me. But I have another hat that is on the coat rack gathering dust these days. 15 years of mechanical and manufacturing engineering work dealing with some of the fussiest ball bearing applications you can imagine.
The discussion so far reminds me of a bunch of 12 year old boys discussing the right way to make love to a woman. Their focus is almost entirely on one aspect of the problem. And there is a general commonality to their approach.
Perhaps it's time to look at the bigger picture. First off this is a .875 dia. Doesn't sound like a precision bearing. They tend to be metric sizes. Does the OP know the actual size of the bearing? A decent 1" mike is a start. Is it a ground outer race or an unground type. A cheap bearing could be the latter. and then it may not be very round. Is .8747 something from a manufacturer's catalog or is it a dimension on a part drawing? If it has to be a .8747 (+/- 50 millionths or even a tenth) how does he plan to measure the bore?
3 point mike? Please tell me he has a class XX set ring, preferably .875 dia, to calibrate it; lest I die an early death writhing on the floor in laughter. BTW, how well is his temperature control? 20F difference in temp between an aluminum work piece and the steel measuring instrument is a hundred millionths. That's a tenth. And finally, no one has said if he needs to make one or a hundred of these things all to print. Or just one to fit a specific bearing he already has in hand. The "make", as in "If I can measure it I can make it", depends on the quantity and how the customer will know he's getting what he ordered.
OK, I've had my fun with some of you....... please don't get mad at me. In a 42 year career I've gained huge respect and admiration for any one who can put food on the table with his machining skills.
Ed Weldon, Los Gatos, CA
 
types of Boring Bars

Ok Looks like its time to get a boring head. What is a good brand and a good place to find one?

There are lots of kinds of boring bars, some are more versatile for bigger range, like criterion bars and so on.

For holding tenths, though you need one made for tight tolerances.

I suggest a Devlieg Microbore from ebay.
They are very rigid, being a solid shank down to the tip which has an adjustable ring marked in .001 on diameter (.0005" per side) and it is easy to tweak .0002" on the diameter.

They take a brazed carbide tip on a threaded shank tool bit, with dead sharp tools, which is what you need for fine boring (light radial tool pressure).

I have about 30 of these for my 4 mills, and buy straight shank ones to fit more machines.
Last ones I bought on ebay averaged about $40, and then bought a few tips for $10-12 each.
Tips last for hundreds of holes (with resharpening).

Even with that type boring bar technique makes a difference.
I would use a drill,
then make a circle with an end mill to control the amount of stock left for the boring bar to take out.
If the end mill is tapered, or mounted in a less-than-concentric collet chuck, I would probably leave .004 to .005 per side, and see how that works.
Then lastly the boring bar.

It will produce a hole like a mirror with about .003" down feed per rev and somewhere about 1100 to 1600 rpm.

Will put a smile on your face.
 
Sorry if it has been covered, as I am at work and don't have time to read all the replies. But if your getting a oversized bottom it's not tool deflection, but the tool is probably "wobbeling" and cutting bigger at the bottom. But like others have said make it a little tight and press it in. As for getting just the right size & a round hole. What I do is Interpolate CCW, Spring, then CW. I know you will be Conventional Cutting, but since you will be taking less than a spring pass it's ok. You will be helping to eliminate the Ball Screw Slop, and this will make the most round hole that your CNC can do. And start undersized, and comp it out until you reach your desired size.
 
Best bet is a boring bar, then maybe a reamer. If you have a good tight machine that can hold the tolerances and insist on interpolating the hole then try using a straight flute end mill, I use them for tight tolerance keyways to help with the taper problem. The problem with your method is there are too many variables that can effect taper like the machine, tool holder, or tool. You shouldn't have a problem finding a .8745 reamer.


I am trying to mill a hole to press fit a ball bearing with an OD of .875. I am trying to hit about .8747. I am first drilling it with a 55/64 drill bit then taking the last .015 with a .5 endmill and a pocket toolpath. First I tried using a 2 flute endmill in an endmill holder. Then I switched to a collet chuck thinking it might be a little more concentric and I also switched to a 3 flute endmill thinking it might be a little more ridgid. But I am still having trouble getting it to the right size. After hours I finally figured out how to make mastercam run endmill comp and make my machine understand it. I need to mill a through hole in a 1" thick aluminum part that gets a bearing pressed in from both sides. I finally got a part that was just about right on top but then you flip it over and the bottom of the hole is a hair too big. So I am not sure if interpolating a hole with an endmill is possible to this tight tolerance. Something I didnt think of until after I left the shop was maybe I should slow my feed rate on the endmill down to next nothing say about 2.0 imp. Maybe that would help with the tool flex issue I am having.

I am also considering investing a boring head. I have never personally used one but I think they might be the perfect tool for this job. I think I would get a lot of use out of it on similar jobs like this.

Any other ideas?
 
I'm not a CNC guy yet (I guess it's inevitable though). But I was taught to always drill => bore => ream for machining holes with accuracy in size and location. And boring with an endmill didn't cut it. I wouldn't attempt to machine for press fitting bearings any other way unless a reamer wasn't available. Then boring to finish is required. I guess things have changed.

Best Regards,
Bob
 
I have circle milled a lot of holes, typically they are not perfectly round, but it was not difficult to hold size. You could have ground the flutes of the tool down so that only the last .550 (say if the bearing was 3/8 thick) then treated it as two separate holes, circle mill the top first to dia (measure with a telescope gauge) then circle mill the bottom to size, (again measuring with a telescope gauge).

Cheap and dirty if you try it first in some scrap might be to bore the hole with an endmill. Many solid carbide endmills run .002 under nominal (because they would make a .875 endmill from a .875 blank, they use the .002 to get it sharp I think). Garr always ran -.002 anyway.

Bill
 
I've done this kind of work before. I would recommend leaving a little bit more meat to clean up. Say .030 thou. Change your program to include a roughing pass .020-.025", and a finishing pass .005-.010". Then I would interpolate in depth cuts. Say .500 then 1.030. You could break this into 3 depth cuts if need be. This worked for me. It takes a little bit longer but in the world of CNC we're talking about an extra minute. Well worth the time to avoid a headache. Other than that I would just recommend using a sharp end mill with at least 1" LOC.
 
Dont know what m/c you have acces to a bridgeport or anything with a cnc control the circular pocket canned cycle would do it,or if your a peasant like me and only have acces to a maual m/c l would simply ream it ,try it in a bit of similar scrap material,like someone suggested earlier when l do this never have a problem the bearing snaps into the hole then l put a bit locktght and lock it in/or on ,reamers in general if you want a reamer to cut tighter than it does on first attempt simply leave more stock in the hole if you want a reamer to cut bigger than it did on first attempt simply leave less stock in the pre drilled hole,obviously a micro boring head would do it but not everyone,s got one of those-B
 
I am trying to mill a hole to press fit a ball bearing with an OD of .875. I am trying to hit about .8747. I am first drilling it with a 55/64 drill bit then taking the last .015 with a .5 endmill and a pocket toolpath. First I tried using a 2 flute endmill in an endmill holder. Then I switched to a collet chuck thinking it might be a little more concentric and I also switched to a 3 flute endmill thinking it might be a little more ridgid. But I am still having trouble getting it to the right size. After hours I finally figured out how to make mastercam run endmill comp and make my machine understand it. I need to mill a through hole in a 1" thick aluminum part that gets a bearing pressed in from both sides. I finally got a part that was just about right on top but then you flip it over and the bottom of the hole is a hair too big. So I am not sure if interpolating a hole with an endmill is possible to this tight tolerance. Something I didnt think of until after I left the shop was maybe I should slow my feed rate on the endmill down to next nothing say about 2.0 imp. Maybe that would help with the tool flex issue I am having.

I am also considering investing a boring head. I have never personally used one but I think they might be the perfect tool for this job. I think I would get a lot of use out of it on similar jobs like this.

Any other ideas?

here u need to give touching cut as a ur final size. first u can interpolate rough matirial beside .1 margin and after you can done this this margin in final interpolation with high rpm of spindle also you need to use 4 flute end mill.
 
Magsightproducts

Using a boring head has always proven to give a nice round hole and using a cheap 0.001 increment boring head along with a 0.0001 indicator to make 2 tenths of an adjustment on the diameter will probably give you plenty of accuracy for most applications. It doesn't sound like you're making aerospace parts.
 
.001 boring head with the bar cutting tip adjusted way off straight so that you get .0001 per grad.
(I leave the math to you here) :)

Interpolate?
No way any 1 micron feedback cnc can make .0001 adjustments (.0002 on your dia.) let alone round even if you just laser aligned it.
The math in the computer just does not work out. (tenths do not map to microns nicely)
If you have english screws it is technicality possible at slow enough speeds but in reality never works out.
Most don't have access to the equipment to check this and lightly loaded bearings will work fine in non-round holes as long as you don't "crush" the OD.


If you use a reamer watch out for the end chamfer vs. the radius on the bearing if a blind hole.
Bob
 
An undersized endmill would solve the problem right?

So what if you took a stone to the endmill? Maybe run it backwards in the mill, or lathe and hold a stone against it for a few seconds...........

Z
 
Just to add, from a design end, I've been burned by interpolation on several occasions. A thin wall bearing needs the hole round or the bearing won't be round. A precision bearing needs the hole round no matter how thick the walls are. A precision "thumb" press needs the hole round so the parts don't rock. Holes with lobes wear quickly. I hate effing interpolation because your machine is never as good as you think it is. If I put crazy numbers on the print, you'll no-bid it or price it to the moon. If you bore the thing I know what I'm going to get and can be confident it will work, without crazy specs. Modern practice is not to put process info on a print, but I'm not always modern. I also note that you can put process info on a surface roughness callout. Maybe one could give surface roughness plus "bore" as a finish spec? [rant off]
 
QT: (Are not end mills made with back taper)

All the end mills I have made and sharpened were straight sided.
I have made taper end mills, but that is a special end mill.
End mill usually cut oversize because they are OD sharp and the slight run out will show upin the hole size.
Reamers have an OD circle land so usully cut .0002 over their size.

For .8747 make the reamer .8745. for a just go into the hole.
For a press fit
look to your Machinest hand book fo the size.
If you have +- .0001 then make the reamer .87445
The given rule is make the reamer .0002 smalLthan taget size. *But a hot part or a hot reamer cann change things.
Reamers have a back taper generally .0002 per inch, so one can make a reamer a tad big and then sharpen off an inch (or what) to make it smaller.

Reamers are not always easy to measure because some reamers don't have all flutes exactly opposite. Nowadays with CNCs flute spacing is better indexed.
For a production job one makes the reamer to produce near high limit once the job is to riunning tempature so with re sharpening you get the longest life out of the tool.
 
Last edited:








 
Back
Top