What's new
What's new

How to make a reamer cut a little smaller?

Terry Keeley

Titanium
Joined
Oct 18, 2005
Location
Toronto, Canada eh!
I have a project that uses 1/16" dowel pins in 6061, they're a couple tenths over nominal as usual.

For some reason my 1/16" straight flute reamer is cutting big, the pins fit but just go right in. I've checked and don't see any burrs on the cutting surfaces, I've even run a stone down them to make sure. If it wasn't Sunday I'd just get a new reamer.

Any way to make it cut a few tenths smaller?
 
Run a stone at about 45deg to dull a little. Don't ream any more than .005.
run slow feed fast, use cutting oil.
If that doesn't work run spindle backwards and hold a hard stone against it to make a little smaller.
 
After doing everything to make it cut smaller by how you use it then try as mentioned above stoneing a 45 on the cutting edges. I have only needed to do this on a 1/2" reamer on 6061 holes. It worked well but I was amazed at how much I had to stone the cutting edges to get it to cut smaller. This was for a finicky production job and it worked well, the reamed holes remained the same size to the end of the run.
 
I have a project that uses 1/16" dowel pins in 6061, they're a couple tenths over nominal as usual.

For some reason my 1/16" straight flute reamer is cutting big, the pins fit but just go right in. I've checked and don't see any burrs on the cutting surfaces, I've even run a stone down them to make sure. If it wasn't Sunday I'd just get a new reamer.

Any way to make it cut a few tenths smaller?

"Tenths"?

I'd not bugger-up a reamer over ignorant shiney-wood when you can simply "put the squeeze" to it and make it shrink its own holes. And/or Loctite 'em.

Not as if small steel pins in shiney-wood have all that much budget against stress loosening to begin with...


Page Two:

Put the shiney-wood in yer oven. Drill & ream it HOT. She'll cool tighter.

:)
 
Just in case you aren't doing this- stop the spindle at the bottom of the hole, and retract straight out.

Running the reamer while retracting can oversize your hole.

Also throw an indicator on the reamer and thump it in true before you run it down the hole, and drill as close to your finish size as you can..
 
All good ideas guys, thanks! I was reaming about 0.010" and pulling it out of the hole while running so I'll try a smaller cut and stop at the bottom.

I did try to dull it a little but it didn't seem to make much difference, maybe I need to go a little more as mentioned.

The pins will be pressed in and out "in the field" so I want a mild press fit, now they just slid in and out. No slop but no press either.

I think I was able to decipher your post Bill, thanks for the input. And good to have you back...
 
I think I was able to decipher your post Bill,

I don't "hate" shiney-wood, Terry - or I wouldn't have clocked a coupla million miles on airey-planes, prefer aluminium boat hulls, my 'loominum diesel-fuel tanks, nor love my all 'loominum rustfree (of course!) 2005 Jaguar.

:)

But WTH.. it is slightly less stiff or thermally stable than Bamboo, so I don't expect it to doo what it isn't good at.

Even when you get this fit to come good... With a sensitivity of less than a thou?

Your "mild" press fit of steel into raw 6XXX may not have a very long field-service life-expectancy @ a mere 1/16" diameter ++ the effects of the disparate chemistry of the two major metals.

Then again, it may not NEED to?

We've had no sight of the end-use nor how long it has to last, or under what conditions.
 
Get some hole shrinkers..

I can't find them now, but Micro-Mark used to sell a set of "hole Shrinkers".
Nothing but some ball bearings on a stick. Place bearing at top of hole
and tap with hammer.

This is of no use on a 1/16" hole, but when I make IN HOUSE (Not to ever leave this shop
as a finished product.) fixtures and I need to dowel pieces together, I just use one
reamer a, .2505, and then run a form tap down the ones I want to be a press fit.

The spin it backwards and hit it with a stone works, or I use a diamond file, usually
doesn't take long, or much to bring it in a couple tenths.

Have you tried using an endmill? They are usually a little undersize, though if
there is any run out, you're screwed.

Also, how slow are you turning it.. Laugh all you want, but I generally toss all surface
speed calculations out the window when I'm reaming.. Unless its a big reamer.. 450rpms
max (unless its a production deal, but usually its not).. Seems to work pretty consistant
that way. I'm not going to scrap an $800 part just so I can ream a hole 3 seconds quicker.
 
This is of no use on a 1/16" hole, .. and then run a form tap down the ones I want to be a press fit.
Good stuff. And yah - it can, too, be of use, 1/16" and even much smaller.

By this time of this century, most of us have Metric drills, reamers, taps around, as well as US/inch (also letter and number drills, etc.).

Lotta times the solution is a crossbreed just a skosh off .. that you already own - just in the other drawer.

Gotta love those wall-charts...

:)
 
Have you messed with the speeds and feeds yet? Sometimes dropping the rpms while increasing the feed can work. I also have had luck with grinding off half the cutting edges.
 
Are you choking up on it? I try to leave reamers hanging out much longer than drills, to let them float better. It needs to follow the hole that's already there, instead of trying to make it's own. On that same note, are you spotting the pilot holes? If the drill goes in crooked, the reamer will start out off center, making the hole big, and probably tapered. Also, make sure you're drilling deep enough. If the reamer bottoms out on the pilot hole, or on the chips, the reamer will wobble a bit. It doesn't take much.

As others have already said, try a bigger drill, a lower speed, and a higher feed. I usually spot drill to .070 diameter, and drill to #53, as deep as I can get away with. Then ream at 10 SFM, feeding at .01" per rev, no pecking.
 
Thanks again guys.

Hole is blind so burnishing with a steel ball won't do, never saw a ball that small anyway but I'm sure they exist.

Tried different speeds/feeds, cutting oil/none, they all seem to cut the same. Will trying stopping at the bottom and pulling straight out as mentioned, also zeroing the runout. Tried plain old 1/16" drills, too tight.

I'll figure out a solution and report back soon.

Oh and Bill, although there's still lots of "loominum" on airplanes these days, lots of that is being replaced by carbon fiber. What's the old saying? Boeing's are built by beer guzzling union men with rivet guns, Airbus' are built by wine sipping Euro girly men with glue guns?

But factor in the "Max" fiasco and I think I'd opt for the glue gun myself...
 
Not to be too obvious, but you could try using the correct size reamer.

dowel pin reamer sets seem to only run down to 1/8, but they are half a thou or 2 thou under. Any size you want is available from L&I

mcmaster stocks .0620, .0622. .0623

less than 20 bucks ea
 
But factor in the "Max" fiasco

Bad, one, that. But one can avoid - as I DID do for about twenny years whilst Scarebus was sorting THEIR hash. Proud member of the "If it ain't Boeing, I ain't going!" movement.

The real scare, now, is that it was effing SOFTWARE! "AI" AKA Artificial Idiot.

And we think self-driving cars and 18-wheelers are a good idea?

How d'we avoid THOSE, then?

:(
 
Not to be too obvious, but you could try using the correct size reamer.

dowel pin reamer sets seem to only run down to 1/8, but they are half a thou or 2 thou under. Any size you want is available from L&I

mcmaster stocks .0620, .0622. .0623

less than 20 bucks ea

Something tells me he doesn't want to wait for something from McMaster to show up on Tuesday.
 
I realize this isn't "in the box" thinking. But have you considered buying a Reamer that will cut the size you want? As opposed to trying to manipulate the Tool to cut under what the OD of the Tools flutes are.

R
 
Thanks for all the help guys, this place is awsome.

Tried a few more "technique" based things but it didn't make a difference.

So I chucked it in the lathe, ran it backwards and touched it with an India stone. It miked about a tenth smaller and wala, perfect fit!
 








 
Back
Top