• This site uses cookies. By continuing to use this site, you are agreeing to our use of cookies. Learn more.
  • PLEASE: Read the FORUM RULES BEFORE registering!

Trouble cutting bearing pockets

RHayes

Active Member
Active Member
#1
I want to install bearings (R8 2RS) in both ends of a 1.5" piece of aluminum round bar that is 2.00" diameter.

In a 3-jaw, I face it, bore 3/4" through, then cut the first recess. Remove from chuck, reverse, cut second recess. Then install the bearings, with a light press fit,

Any tips on improving the accuracy? The .5" shafting never fits as well as the individual bearings do on the shaft. I have a Grizzly 4003G with 3-jaw and try to reverse the piece as best I can but feel this isn't the proper way to do this operation. Ultimately, the 2" round "hub" gets installed in a woodworking project not requiring high tolerance or subject to high load, but I still want to do the bearing installation as best I can, and ultimately would like to make 50 or more of these.

Thanks in advance for any suggestions.
 

Bob Korves

H-M Supporter - Premium Content
H-M Supporter-Premium
#2
The problem comes when you turn it around, and is likely mostly due to the inherent inaccuracy of the three jaw chuck. If you use a four jaw chuck and dial it in carefully for each end, you should have better results. Your piece is not very long, but you still also need to check and correct for runout from one end of the part to the other while it is chucked as well.

Edit: Another thing you can do is to accurately finish the through hole bore while doing the first side, and then turn it around and indicate the hole on the second side to get it lined up better. Still need to watch for runout from end to end while mounting in the chuck...
 
Last edited:

tq60

Active Member
Active Member
#3
Once you move the work it indeed will move.


Suggest drill slightly smaller then bore through so you have a good reference.

Flip part and 4 jaw should be used but you could test centering with dial indicator in bored hole and maybe shift in chuck until it runs true.

Sent from my SAMSUNG-SGH-I337Z using Tapatalk
 

Tony Wells

Former Vice President
Staff member
Administrator
#4
Normally, to get the best out of flipping work like that you have to at least skim cut the OD of the stock to get a round surface. If they are already cut to length you have to go another route. You also have to avoid chucking too tightly on an aluminum piece with ~7/16" wall. If you were going to make 50 and sawed them, you could forego the OD turn if you face/bore through/counterbore as a first operation, then make up a expanding stub mandrel for the other end. Then you would face to finish OAL and counterbore for the other bearing.
 

Dave Smith

Active User
H-M Supporter-Premium
#6
like what Greg said about boring all the way through--or start with a thick walled 2" OD tube if you want to make many, and use a spacer lightly pressed between the bearings---spacer can be pinned to housing after bearings are pressed in if desired.----Dave
 
Last edited:

Tony Wells

Former Vice President
Staff member
Administrator
#7
Spacer could even float a little if the bearings were tight enough. Just make sure if you go that way to make the spacer ID large enough to pass the shaft easily.
 

chips&more

Active User
Active Member
#8
I would not flip the round bar in the chuck. I would use a steady rest set-up when machining BOTH ends of the round bar. Taking a skim cut on the OD ends before you start would be a good idea as well...Dave
 

Dan_S

Active User
Active Member
#10
My first question would be did you turn the bar OD to 2.0" or is this raw bar stock? If it's just plain extruded aluminum, you can not trust that it is round.

Unless you have a really dialed in 3 jaw, the bores won't be coaxial, and that will cause binding.

The best way to hold something like this, is in a collect (unlikely at that diameter). Next would be a 4 jaw if you only have one or 2 to do. Finally would be custom soft jaws like Tony said.
 

chips&more

Active User
Active Member
#11
The way I read it, the OAL is 1.5", so steady rest is not much help. Turned OD and bored soft jaws would be the best way for me to do it.
Good point! OK then, I would bore it out all the way through to bearing OD size. Then make an internal bushing/spacer that would go between the bearings. This bushing/spacer could be a press fit or whatever. No flipping required. And no OD worries. Guaranteed perfect alignment…Dave
 
Last edited:

RHayes

Active Member
Active Member
#12
Wow, thanks for all the replies. This is very helpful for someone of my experience.

First of all, the 2" is extruded 6061 and are all short pieces from the salvage yard. After reading the replies, I'm thinking boring all the way through would be the best approach for me. I was trying to avoid turning the outside diameter, it fits nicely in a 2" hole cut in oak using a fastener bit. Will try to get a photo of the project.
 

Dan_S

Active User
Active Member
#13
Wow, thanks for all the replies. This is very helpful for someone of my experience.

First of all, the 2" is extruded 6061 and are all short pieces from the salvage yard. After reading the replies, I'm thinking boring all the way through would be the best approach for me. I was trying to avoid turning the outside diameter, it fits nicely in a 2" hole cut in oak using a fastener bit. Will try to get a photo of the project.

if you bore all the way through the bearings will align to the accuracy of your lathe, so more than good enough. If you bore all the way through turning the OD would be up to you. If the ID is concentric enough to the OD for your purposes no need to turn it true.
 

RHayes

Active Member
Active Member
#14
Thanks Dan, thats what i'm thinking.
Here is a photo. A friction drive for a compact spinning wheel.

In the photo is an empty hub with a 5/8 o.d. bearing installed in the outside diameter. This leads me to another question that should probably another thread. I plunged a 5/8", 4-flute milling cutter and the bearing fits loose. What I need to know is if I can lightly grind the 5/8" to reduce its outside diameter? friction drive.jpg friction drive.jpg
 

JimDawson

Global Moderator
Staff member
Director
#15
Trying to get an accurate hole by plunging with an end mill is problematic at best, when plunging with an endmill they tend to wobble around. It is possible to drill a pilot hole that is just undersize and then plunge with the end mill but this still may not make an on size pocket. A 2 flute would be better than a 4 flute for this operation. Reaming or boring would be a much better option.
 

Tony Wells

Former Vice President
Staff member
Administrator
#16
You could, but it's not really reasonable to expect to hold bearing fit tolerances with an end mill. That's an application for a reamer. In aluminum, a reamer would last nearly forever, especially if you spring for one that is carbide tipped.
Lightly stoning an end mill will reduce the clearance on the flutes, inducing the probability of dragging. Not good for finish or fit. I find that many, if not most carbide end mills are ~0.002 under nominal anyway, so with that and a little runout from your collet, you might get close enough, but that really isn't good practice for machine work.
 

David S

Active User
H-M Supporter-Premium
#17
Boring through the blank seemed like an awful lot of material removal, vs using say a thick wall tubing and the appropriate size bearings. However it sounds like RH is getting drops from the scrap yard so that is the starting point.

I certainly agree boring thru would be the most accurate.

David
 

David S

Active User
H-M Supporter-Premium
#19
I don't know what the speed and loads are, but just thinking out loud. This seems like it could be an ideal application for oil impregnated sintered bronze bushings. Perhaps a pair of OD 5/8", I.D 1/2" x 1/2" long. That would only require one straight through bore for a slight interference fit. Could heat the slug in the oven and slip them in from both ends.

Also with that bearing in the side, I wonder if we are running out of wall thickness if we do a straight through 1.125 " bore?

Boring the side pocket for the smaller bearing seems like and ideal application for a small boring head...or perhaps fixture to the lathe face plate and bore it that way?

David
 

Cavediver

H-M Supporter - Premium Content
H-M Supporter-Premium
#20
RHays, did you find a workable solution?

I'm in the planning stages of a DIY 2x42 belt grinder, and I would like to turn my own rollers. Since I'm working on a mini-lathe I'm very limited in terms of tooling and work space. Your issue is the same one I will face, and I'd love to know how I'm going to work around it before I start!

Thanks!
 

Cavediver

H-M Supporter - Premium Content
H-M Supporter-Premium
#22
Would a draw-bar version of something like this (plus an adapter plug turned to the ID) work as an open end mandrel?



Simplified process:
Face and bore / ream stock to the appropriate diameter
Cross-drill and thread for a set screw or two
Mount stock (on the adapter plug) and turn the OD and the bearing pocket
Flip the part, take a skim cut to check for alignment issues, face and cut the 2nd bearing pocket.

I like this idea as it has long-term versatility, but I don't know if the 5/8-16 threaded section of this 3mt blank would hold up to machining a 2"x 2" aluminum cylinder.
 

RHayes

Active Member
Active Member
#23
I've made ten so far (two batches of five) and will be making another 5 soon. Still boring from each side, and lining up a reverence mark on the same jaw. I know this isn't the most accurate way but the mechanisms have all worked well so far. I ran out of drops from the scrap yard and ended up buying a 5' length of 2" 6061-T6.
 

gheumann

Active User
H-M Supporter-Premium
#24
If you bore all the way through, even undersize, you can use a center in the tailstock to center the work in the chuck after you flip it round. Should get you very close. But as a rule, planning your work to only have to chuck a part once is always the best if possible.
 

RHayes

Active Member
Active Member
#25
Thanks. I have been boring all the way through but will make a point of bringing up the live center cone as well upon reversal.
 

Wreck™Wreck

Active User
H-M Supporter-Premium
#26
I make hundreds if rollers per year with bearing bores in each end that will be mounted on a shaft during assembly.

If possible bore soft lathe jaws to hold the parts, this has the added advantage of leaving little or no jaw marks on the part.
If possible use an adjustable chuck.
If mounting the finished product on a shaft of questionable size and roundness use what is often known as "Bearing Quality Bar" stock, turned, ground and polished, this is not to be confused with TGP material for general use.
 

MarkM

Active Member
Active Member
#27
If you need a shoulder for the bearings to butt up against and have to flip it and re chuck it. Make a pass with your boring bar through the part and when you flip it to the other end indicate off your bore and machine the second bearing pocket.