Reamer Trouble

Comrades,

I am having trouble reaming to an accurate diameter. The situation is this:

I start with 20mm (0.79") length of 6082T6 aluminium tube of 12.7mm (0.5") outer diameter and 3.4mm (10 Gauge?) wall thickness.

I use the pre-existing hole to centre a 7.80mm (0.307") drill bit and then drill a through hole. I should say that I am holding the tube in a vertical V groove in the face of a vice, and the machine is a fairly lightweight drill press (cost ~£200 ($250) and mass 30kg (4.7 stone)). My spindle speed is ~500 RPM and the feed is very slow - I take about 15 seconds to drill the hole.

I then ream the hole using a 7.98mm (0.314") reamer. I use the same spindle speed and feed. The drill bit and reamer are HSS. The reamer is one of these (link).

When I measure the hole, I find it to be 8.00mm (0.315") in diameter, and I do not get the intended interference fit when I insert a dowel.

I do not know what the problem is.

My ideas are:
Runout on the drill press - not visible when the chuck is spinning without load, however.
Inaccurate centring of the hole w.r.t. the reamer (?)
My speed/feed is all wrong.

Can anyone shed light on the matter? Is it hopeless to achieve the tolerance I am aiming for (7.975-7.990 mm) with my current setup?

You're squeezing the part in the vise. When you remove it after drilling or reaming, it opens back up to oversize. Odds are that the hole isn't round, either. Best to do the inside then the outside by mounting on a mandrel and turning on a lathe. Barring that, you can make a near-full-circle clamp, like a split collar, and hold it that way using minimum pressure.

I'm guessing the stock is already sized for the OD, so that leaves you with figuring out a better clamping method.

You'd have better luck drilling from solid. Drilling out the existing hole in a flimsy drill press is likely giving you a hole that is off center, not round, and not straight. Plunging a reamer into that hole is just going to give bad results.

Have you actually MEASURED your hole after drilling and before reaming?

It is also worth pointing out that reamers are a crap shoot at best. They can 'wander' in hole size by as much as +/-.001" depending on feed, speed, stock left for reaming, cutting fluid, etc. You could try using oil or wd40 to lubricate it when cutting (if you are not already doing this), adjust your feed (hard to do by hand, but you can vary how hard you are on the handle), adjust your rpm. OR buy another reamer .0005" smaller and see what happens.

https://www.mscdirect.com/browse/tn...24615+4288018041+4288041671&searchterm=reamer

Do you have a 3 jaw chuck you could hold on to? Along with whats been said, feed faster. General rule of thumb is half the speed twice the feed on a reamer as you would
a drill. 500 rpm is fine for your reamer, but you should be through it in about 3 seconds. If you feed to slow the runout will allow it to go oversize.

BTW If you are in metric country using a H7 reamer(most commen) properly and m6 dowel pins (also very commen) should give you a interference fit

Peter

Guess I would take my 10x loop and look at flutes to see they all have the same waer land,and all sharp.
would add some coolant.. washing soda and water if not wishing to buy some..tap ease is good for reaming.
would measure the the reamer for back taper and resaharper it at a smalled diamerte.
likely would choose a siraight flut over a negative.
dont dwell lond at exit...might kill the rotation at exit.

chuck on about 3/8" of reamer.It might let it cut closer to size .
If that doesn't help use a hone on it .

Drilling out an existing hole in aluminum pipe or tube and then reaming it will normally lead to inconsistencies no matter what machines you use. The drill and reamer are just going to follow the existing hole. The hole in aluminum pipe isn't usually close to being concentric with the outside diameter, and often they aren't even close to round either.

Here is some of my bag of reamer tricks, and they don't all work in
all situations.

I'd leave more stock, your .307 drill is probably going over,
and you aren't reaming much of anything. In my experience, more
stock is better than less when it comes to reaming aluminum.

Slow down the reamer speed. In my experience, stupid slow
reamer speed can make up for a lot of other potential issues.
200rpm's is my GOTO reamer speed (regardless of size) when it
HAS to be right and I'm not trying to make time (sometimes
getting it right is more important than doing it fast).

You *can* adjust how a reamer cuts. These are hacks, these hacks
are not meant for long term production, and are best avoided if
at all possible. I don't like doing these things, but sometimes,
you have to do what you have to do..

If you are running a bit big, you can stone the outside of the
flutes. Perpendicular to the cylinder of the reamer. Sometimes
they'll be a burr out there that is giving you a fit. If its
cutting REALLY oversize, I've spun them slowly backwards and hit
the outer diameter with a diamond file or a fine stone.

Also, you can run a piece of carbide up the inside of the flutes,
pushing up a tiny burr, and get them to cut a bit oversize.

Somebody already said to barely chuck up on the reamer to let it float.
I've actually added grooves to the shanks of some large reamers to
give them more flex.

Feed it harder!!!

If everything isn't perfectly square and perpendicular, you may
be trying to follow a hole that is off angle a little. I've
had that problem reaming on a lathe, and the reamer wasn't quite
straight and would waller the hole out. I ground down all the flutes
except for the bottom 3/8" or so and it worked pretty good. Again,
this is a hack, and you shouldn't do this unless you absolutely have
to.


Conclusion: I'd start with more material left in the hole, slower
spindle speed and FEED IT HARDER!!! And that should fix you up,
before you have to start doing stupid stuff. Make sure she's lubed up too.

A negative flute tends to puse the cut material down, a straight flute reamer tends to more gather it in.

If all fails and your are getting good hole surface finish any local grinding shop can grind .001 from OD.

*but the reamer should make a hole about .0001-.0002 larger than thr micromerer check.

Making the reamer .001 smallr han the needed size is not logical.

How many part do you need to team? If it's a bunch I would grind a short pilot on the end of the reader that will just got the drilled hole. Grind it in a spindex on a surface grinder, toolpost grinder or if you have one a tool grinder, it will resemble a counterbore. You will have to put the cutting reliefs back on the end.

If you don't have a way to grind it accurately then you may have to resort to other methods (ball bearing trick, slightly squishing the finished tube)

Might consider the way you clamp the part. A half inch wide strap only .100 thick..with a set amount tightening may be the ticket,
The strap may be a certain thickness so it can not disform the part but the strap will bend a little if made to tight..

The strap/clamp bar and the mating vise might have a glued patch of fine abrasive so to not hurt the part surface but hold better than a smooth steel surface..

The simplest drill press should ream a hole .0002 or so larger than a decent reamer.

Might use a allen wrench to tighten and swing that wrench to a stop..or decide one finger or two finger pust to make tight.

I ream hole with not bolting down my vise..just having a bar clamped to the table to rest it from spinning. That way it finds the correct spot under the spindle..
might check the tram of the spindle with looking across a hand held right angle square..

Over all I've had best luck drilling, then boring leaving 003" to 005" for the reamer. Then ream using oil with speed very slow and feed medium to fast. Do not allow the reamer to dwell. Also be sure the part is completely cooled before reaming. Aluminum expands like crazy with heat. Hope this helps.

Best Regards,
Bob

what makes you think the hole is 8.00 mm? how big is your pin? is it h6 or m6? you will probably not get an interferrence fit with a 7.98 reamer and a h6 pin even if everything is perfect.

another hack would be to heat the piece while reaming. are you running dry? oil will decrease the size in aluminum (not in steel).