I am looking for some help please. I was running a job last night that didn't go as well as I thought it would. I need to make 64 oil impregnated bronze bushings, 1/2" od, .376 / .377 id and 1.83" long. I had faced the ends to length, and was planning on drilling and reaming the id then putting the parts on a mandrel to turn the od concentric to the id. However, after just a few parts, the reamed hole was already undersize and I thought the bronze would be a no brainer to do! I was drilling the hole at 23/64 and was reaming at 400 rpm 5"/min feed and a quick retract. If anyone has any suggestions I would appreciate it because I have to deliver this job today. Glenn McMullin.
I would make them from bar stock, holding in .500 or larger collet, drilling, boring straight, reaming to size.
If you need concentricity, using a mandrel is a poor way to go. Better to rough hole, rough OD, finish inside and then finish outside and cut off.
Drilling and reaming, instead drilling, boring straight and reaming, makes for a poor hole but is generally good enough.
You can use a small diameter and long carbide end mill as a boring bar, make your own holding
fixture for the lathe as required. Works great for me, better rigidity from four flute than a bring bar.
Use an angled cut-off tool instead a straight one.
If I would be offered a job with pre-cut to length bushings that you describe I would not take it.
I have always heard any "rubbing type" machining operation on this style of bronze tends to "wipe" the bronze closing the pores and making the oil impregnated feature generally not effective.
a new reamer cuts at the front, a good quality reamer would be needed, not a beat up old one from the bottom of the baking dish
my bet is it would be good enough to ream it thusly, but let me know if I am wrong
new reamers are for certain critical jobs, not to be used for everything else where an old one will do
re-ream them by hand, bronze stress relives like crazy and does not stay round.
you realy see it in large bronze.
Thanks for the feedback so far. The strange thing about this job is that using a new dormer reamer, I was able to get about 3 parts to size but after that, the id was getting small. I looked at the reamer through a loupe and could see wear at the tips already. After re-sharpening I had the same thing happen, 3 parts and visible wear. The composition of the bronze includes 87 - 90% copper, 1% max iron, 1.75% max carbon and about 10% tin. I am wondering if the tin is doing the damage to the reamer? As for the rubbing action of the reamer closing the pores of the bronze, I had been aware of that but the customers drawing specifies the manufacturing method so that is what I am going with first. If not successful, I can then tell them that I have wasted time trying their specified manufacturing method and they need to either change or eliminate the specification on the drawing. Keep the help coming. Glenn McMullin
Oilite or oil impregnated bronze is incredibly abrasive. Use a new dead sharp carbide reamer. Better yet, purchase suitable 2" long bushings and cut them to length.
Incidentally, I hope the customer's specified OD allowance and ID allowance work together to result in the proper shaft clearance when the bushing is pressed into its housing. Oilite is slightly compressible because of its porosity but it transfers all of its press fit allowance into ID reduction. A 0.5010" OD bushing with a 0.3770" ID pressed in a 0.5000" housing results in alightly less than a 0.3760" bore.
"Oilite or oil impregnated bronze is incredibly abrasive."
So THAT'S why this material is used for bearings
I've heard similar things about reaming oilite as John noted.
Had pretty good luck with broaching them from the tailstock. Make a broach that starts out .001 under the pilot hole. Then turn successively larger diameters, maybe .5 long or so ...
For example, if .501 bore is desired and the pilot diameter is .499, turn the broach pilot to .498 then turn successive diameters of .499, .500, .501, all about .5 long. Take care to get a sharp edge (don't de-burr).
Soft works OK for a half dozen parts or so ... harden for longer runs.
is there a close tolerance on the OD?....is there a concentricity tolerance as well?....if the ID is listed as 1/2 you should have a mile of tolerance....just use bar stock drill and bore! and cut off.....I have a carbide boring bar that is chamfered on both sides so I can face with it, and chamfer the ID and OD with the same tool!.....it cant be that much longer a cycle to bore than to ream!.... and just use the stock OD...if you need specific tolerance OD's you can trun the od at the same time!.....forget the second op on a mandrel ......bob
Funny, I had the same tolerance on some aircraft stuff once. It was AMS 4640, but for sake of argument...the same type of stuff. THe holes where undersize within a few bushings.
I was doing this on a cnc lathe, so I changed up the reaming feeds/speeds, setting the reamer .001-.002 off center. I never did get it to ream on size. I had to "polish" out the inside of the bushhings to get the id tolerance.
Next time, I have to do any bushing work with a .001 tolerance on a large qty. of bushing, I think I will burnish, or broach.
The od size is .500" / .4995". It must run within .001" TIR from the id. This material is only available in 6.5" lengths so the idea of machining and parting off from a bar results in a lot of wasted material (1/3 of total purchased). However, in hindsight, that would have been the cheaper alternative. I have spoken to my customer and he does not know why reaming was specified and because of that I will bore the id to size. I should bill them for frustration. Thanks for all of the suggestions. I really like the idea of the broach randyc. I may give that a try just for fun at this point.
i have found when you press one of these bushings
into a hole, it will be slightly undersize, and will have
to be reamed. i think this is an advantage,
because you can size the id after it is installed.
you might take this into consideration when you bore
the id. good luck with your projects.