What's new
What's new

How do I get a reamer to ream a really good hole.

laminar-flow

Stainless
Joined
Jan 26, 2003
Location
Pacific Northwest
Aluminum
Dimensions in inches
Haas TM1
Through hole depth .500
Pre-drill with short cobalt drill to .175Ø
Reamer diameter = .1875
Steel reamer four flute with carbide cutting edges
Reamer checked between centers, very straight
Reamer held in ER-16 collet, CAT 40, about 3" sticking out
Reamer run out checked in spindle with indicator
2000 rpm, F12, coolant

Hole ends up .1879 at the top and .1876 at the bottom.
Any ideas besides single point?
 
Try S/F for the first .100" depth of 500rpm, 3ipm, then go to 2K/12. You're likely getting a little resonance turning the reamer into a tuning fork (single leg) until it settles into the hole.

If you had a non-contact tool setter (laser), you could check actual size to effective size at 2K and confirm.

By slowing rpm and feed initially you'll have less vibration (unless you hit an unlucky resonance) until after engagement, at which point vibration effects (for the most part) stop. You may want to reverse the step change during withdrawal, too.

(Yes, I like parentheses (gosh bless 'em) too much)
 
I always go with Harvey tool carbide reamers indicate them and press go ....done
The price for the reamer I consider them free..
I used to spend hours fighting with hss to get the size hole I needed
 
Some of you guys are really going to disagree with me.

In aluminum, I like to leave a lot of material. .175 for a 3/16"
hole sounds pretty spiffy to me. Gives the reamer something to
do besides make an oversize hole.

Also I'd run it slower. Why? Most of the time I'm dicking around
with a small production run casting. It can't be replaced, its
not a 50 cent piece of material that can be tossed in the scrap
bucket. One oversize hole and I can be out $30 to $1200+. So slow
to make it right doesn't hurt me.

Sometimes if its something really expensive, I'll run a test hole
before EVERY PART. If its a qty thing, and I want to speed it up,
I'll toss up a piece of junk similar material and dial it in before
I hit the real thing.

My goto #'s, on pretty much any size reamer, in almost any material. 260rpms.
At 3/16 in aluminum I'd start at .0035 a rev or so, depending on how I
felt that day, and maybe push to .005 depending on how its coming out.

If I was doing 500 of that same hole in some dirt cheap bar stock, it
would be a lot faster.

Also, sometimes you get a reamer that just does not want to cooperate,
no matter what you do, it just wants to go over. That's why you always
order at least 2.


There are also a bunch of little things you can do with a reamer to
make it change its behavior. My guess is that you are hitting a
resonance since its 4 flutes, and its aluminum, and I'm guessing a new reamer.

Try reaming a few holes in some steel with it, and then go back to the aluminum,
you could be having that "New Tool" aluminum squeel going on. Proper feeds and
speed for the steel of course. Hone out the edges a bit.
 
Thanks all for al that info. I'll try tomorrow and experiment with speeds and feeds first. If I can't get it to work better I'll order a solid carbide from Harvey. I also thought that 2k was too fast but that was recommended from the manufacturer of the reamer.
 
You haven't expressed any tolerance on the diameter. But you're not happy with .0004" over, so I'm going to assume it's a +- .0005". Reamers come in .001" increments. I just buy one that is the smallest size, that still keeps me in tolerance.

R

What I meant was, you can get a .187" Reamer.
 
I think the short answer is you can't. Reamers suck PERIOD.

You can play with speeds-feeds-material removal all you want. It likely won't repeat on the next job anyways.

Besides, I think .0003" variation on a reamer is pretty darn good... :soapbox:
 
Pretty much agree with Bobw
New reamers often need some experience. IMHO either use a HSS reamer, or solid carbide. At that size in aluminum, HSS is more likely to work fine than the one you have, unless it's many thousands of holes.
As others have said, the hole you have isn't horrible, of course depends on what you need to end up with - perfection is often sought, seldom found.
With HSS, half the rpm of a drill and 2X the feed is the old school rule of thumb. (what I was told over 40 years ago, works decent)
I used to always stone the corners of a new reamer a teeny bit. It helped eliminate the new reamer chatter.
Harvey tools are always good in my experience.
good luck!
 
Reamer diameter = .1875
Steel reamer four flute with carbide cutting edges


Hole ends up .1879 at the top and .1876 at the bottom.
Any ideas

Laminar, let me be the asshole to ask this question: What is it you have a beef with?

You've managed to make a .1875 HSS shank reamer to cut +.0001 / +.0004 ....

In my world, that is a Win-Win.
 
Thanks all for al that info. I'll try tomorrow and experiment with speeds and feeds first. If I can't get it to work better I'll order a solid carbide from Harvey. I also thought that 2k was too fast but that was recommended from the manufacturer of the reamer.

Also see Harveys speed and feed charts they have them for all the tools they sell.
if you have problems you can e-mail or call for support.
No association just like their tools.
 
There are a few variable to be concerned with. Is there a lead on the reamer? Is there an adequate chamfer on the hole prior to machining. How close is the reamer indicated? Rule of thumb with reaming aluminum is to leave 2-3% of material to ream based on the finish diameter. The SFM for the drill should be in the 100-250 range for non-carbide drills. I usually stick with 150 SFM and recommended PR based on diameter of the drill of the drill (.175) is going to be in the .002-.003 range.
Inspect your drilled hole prior to reaming!! Once you get the drilled hole you want, the rule for reamers that always works for me is 1/2 the speed, 2X the feed.
 
The way we got reaming to work with us is as such:

Make a quality hole to start with. May be overboard but I drill holes with carbide drills held in hydraulic chucks. Good location and precision hole size. For 3 to 16mm I always leave .2mm (.008”).

If you can’t do that, may be best to drill smaller and skim with an end mill, at the very least the top say 1XD of the hole. If your machine makes good round holes.

I use solid carbide Morse reamers also held in hydraulic chucks for no runout. Runout is key.

Having a heavy feed is crucial. It may seem insane at first but if you jam the reamer into the hole it just seems to stay more consistent. In your case that may mean .010 to .015 IPR for 3/16 in aluminum.

Now having a steel shank reamer in your case, I would try to keep runout low or stick the reamer a good ways out, as it will flex where solid carbide won’t. Also, it may be good to chamfer the hole before reaming to help guide it in. Leaving .008 to .010 stock, feeding a bit harder and giving it a chamfer to lead into may help. We hold tolerances of .0004” total with our carbide reamers pretty consistently, in Haas mills.
 
Slow that reamer way down like 750
Leave about .015 stock to ream
Push about twice as fast as drilling
Should work nicely
Don


Sent from my iPhone using Tapatalk Pro
 
....

Hole ends up .1879 at the top and .1876 at the bottom.
Any ideas besides single point?

I just have to ask, how was this measured?
Please, please do not tell me pins or a CMM.

Since through I would expect a bellmouth at the exit also but much shorter than the entrance cone.
We are talking tenths here in a butter like material.
Is there a entry chamfer corresponding to the reamer front lead to help center the start of cut before we get to size?
No reamer, chuck, spindle runs true. What they like is that circle ground outside land that acts as a guide.
Entrance is always big which is why you push it fast to get the non-cutting sides involved in the process.
Bob
 
I suppose that machine is a mill, are you sure you don't have some runout? I have found even if they are new and clean sometimes you have to take a few cracks at them to get them to spin dead nuts in an ER collet.
 
Your ER collet is going to have some runout.

Your reamer is going to have some flex (much more if HSS).

Your hole is going to have some runout/walking.

Your machining positioning isn't going to be perfect...even if just a tenth or three off.

Some of these variables you can control, some you cannot.

Use a carbide reamer.
Don't use an ER holder, or indicate it in if you need to.
You will get a much straighter hole pecking with an endmill after you drill (undersize on the drill, peck with EM to your final pre-ream size).
Chamfer the top of the hole and make sure you're not pushing a burr into the top of the pre-ream hole.

You should be able to get better results than you are, but keep in mind nothing is perfect. How tight are you trying to make it? And how are you measuring it? Remember your measurement has a tolerance too... a few tenths from a bad measuring technique might not be any tenths at all in actuality.
 








 
Back
Top