reamer cutting oversize, what to do, and why?

Parkerbender · Nov 22, 2010

Have a couple .393 (10mm) holes on some pretty big expensive chunks of stainless. I just got done with the first hole, and the reamer cut .005 oversize. First, is there any way to fix that? I'm thinking it's too big for the ball bearing trick... I'm considering pressing a piece in there and turning the part 180 degrees. Is there any other way to fix this problem?

Secondly, what in the world did I do to made this thing cut .005 over? I pilot drilled with a 27/64, and then reamed at 220 rpm, 2.3 ipm. Cobalt drill, hss reamer.

If you have any ideas, that'd be great!

Thanks for your input,

-Parker

GM · Nov 22, 2010

27/64ths is .4219 is it not :confused:

Did you mean 25/64ths? If so are you sure it wasn't the drill that caused the oversize? Try drilling around .015 undersize then ream to under .002-.003 then finish ream to size.

GM

Parkerbender · Nov 22, 2010

Sorry about that... yeah, I meant 25/64ths... Also, they're blind holes, is there any reason not to just turn a pin for this hole?

Bobw · Nov 22, 2010

.3903 drill. .3937 reamer. You didn't ream a hole, you drilled a hole and reamed air.

A reamer needs something to do, if it doesn't have much to do (nothing or little to cut) it just wanders around and creates all kinds of havoc(like a teenager???). Drill it 3/8 and try it again.

To fix it. 10mm form tap. Though at .005" over that might be a stretch.

Making fixtures where I need 1/4 press and slips, I'll just run .2505 and form tap the press fits. I wouldn't try to sell that though, just for in-house stuff.

The ball bearing trick works only for a gage pin check. If you need a pin to actually fit in that sucker and hold position, it just doesn't work, it gets all sloppy down at the bottom, then the top bell mouths out and it ends up being a mess.

Parkerbender · Nov 22, 2010

I think i'm just going to turn a custom pin for this part. It's a blind press fit so they can't expect to change the pin out. Good to know on the form tap thing, also on the reamer needing something to eat. I had just assumed that the less the reamer had to do the better, I guess that isn't the case. Is there a percentage to figure how much smaller to go with the pilot drill? 10%?

Thanks for the help guys, this one might be a pain to fix, but at least I'll know for next time!

Any more good things to know about reaming? ...or fixing reaming mistakes? Also, twice the feed, 2/3 the speed of the pilot drill, right?

Thanks,

-Parker

Jalbus · Nov 22, 2010

I was doing a similar thing at school tonight and got really good results with a drill that was .010 under, it 'felt' right on the ream, and plenty of oil and half the speed, twice the feed-- the sizing pin hit it's mark and the finish was good too. I haven't always had the best results with reaming. Often the second best size drill is my only option, as the proper drill is missing.

Greg White · Nov 23, 2010

I will go out on a limb here and say your feeding WAY too slow,i would be feeding at maybe 10 maybe 15 ipm. with of course a dsr(dead spindle retract).

Maybe poke the hole wit a .385 2 fl.,maybe.....,dependin on what the job was.
Gw

rockfish · Nov 23, 2010

When I'm trying to hold a close reamed hole tolerance, I always sneak up on it. I will drill the hole to within .01 to .015, then use a reamer a few thou under the desired size, then finish ream.

I have not had any luck just reaming a hole to size leaving the standard amount of stock to ream. It will almost always cut oversize.

Another trick is to make sure that the reamer has sufficient "float". Do NOT choke up on the reamer shank. Hold on to the reamer shank with as little as possible to let the reamer float and cut to size.

Frank

Home

Philabuster · Nov 23, 2010

Parkerbender said:
Sorry about that... yeah, I meant 25/64ths... Also, they're blind holes, is there any reason not to just turn a pin for this hole?

If you bottomed out the reamer hard, that can also oversize the holes. CNCs have little feel when it comes to reamers.

gorrilla · Nov 24, 2010

Parkerbender said:
I think i'm just going to turn a custom pin for this part. It's a blind press fit so they can't expect to change the pin out. Good to know on the form tap thing, also on the reamer needing something to eat. I had just assumed that the less the reamer had to do the better, I guess that isn't the case. Is there a percentage to figure how much smaller to go with the pilot drill? 10%?

Thanks for the help guys, this one might be a pain to fix, but at least I'll know for next time!

Any more good things to know about reaming? ...or fixing reaming mistakes? Also, twice the feed, 2/3 the speed of the pilot drill, right?

Thanks,

-Parker

Used to be a thread in the general section on this forum, where all the old manual machinists chimed in with their "tricks of the trade". Absolutely the most fascinating pile of info about machining I've ever had the good fortune to stumble upon. In it was several suggestions about making reamers and end mills cut over or under. Some would only be good for a one time shot, others for at least limited production. Probably archived by now, at least I hope so. When you have a little time, see if you can dig them out. Probably in that archived section come to think of it, not in the general anymore. You'll be better educated and entertained at the same time. More stuff in there than you can shake a stick at. Only somebody like a machinist would give a hoot about any of it, but to us, it's a gold mine!

scojen · Nov 24, 2010

A good rule of thumb for reamers is to drill 0.015 undersize and check the reamer all the flutes for the correct dia. and check the runout of the reamer installed in the holder and in the machine. Any of these factors will affect the size of the hole. Letting the reamer float a bit in the correct holder also helps. Depending on the grade of Stainless your RPM may be a little high your feed is definitely slow enough.

Scott

voodoochld2 · Nov 24, 2010

Bobw said:
The ball bearing trick works only for a gage pin check. If you need a pin to actually fit in that sucker and hold position, it just doesn't work, it gets all sloppy down at the bottom, then the top bell mouths out and it ends up being a mess.

ball bearing trick?

Parkerbender · Nov 24, 2010

Ran the rest of the parts today, at like twice that feed, with a little slower speed... pretty much 12 speed, twice feed, like someone said, and they all came out beautiful. man, if only the first part looked like the last one... ah well. Anyway for voodoochild, the ball bearing trick is where you take a ball bearing on top of your hole, and tap it, it will make your hole read a bit undersize, but it isn't necessarily the right way to do things... and in my case wouldn't really help because these pins need to be airtight.

Thanks for everything guys!

-Parker

Bobw · Nov 24, 2010

3-PIECE REDUCING PUNCH SET

Years ago had a job, chunk of aluminum, bearing bore on a tab sticking out. Part of the assembly was pushing the bearing in and out and in and out and in and out while setting the backlash on some gears.

Well, the bearing had been pushed in and out, in and out, in and out, and the bore was oversize, and they needed a first article inspection.

4am, hydraulic press, and 2 trailer balls. 1-3/8 or so bore.

Don't tell anybody, but a countersink in a hand drill run backwards, with a bit of pressure works just as well, and it looks better.

jdj · Nov 24, 2010

scojen said:
and check the runout of the reamer installed in the holder and in the machine.

Scott

I am glad that someone FINALLY mentioned this important factor!

Jeff

jdj · Nov 24, 2010

Parkerbender said:
I had just assumed that the less the reamer had to do the better, I guess that isn't the case.

-Parker

Totally logical, however it DOES need a little bit. 10 to 15 thou. on average has been good for me on holes around that size.

Jeff

jeepnxj96 · Nov 25, 2010

first let me start by saying I hate reaming.....I would rather bore a hole for size and finish, but that is not always possible. I use to run short production runs in a job shop for about 10 years and I always ran about .01-.015" u/s on the drill and reamed with a G81 canned cyle. Almost never had a problem on press fit or slip fit sizes. If you are running a good collet and make sure to indicate the reamer to make sure TIR is good, you won't have any problems. On HSS reamers I ran around 45-55 SFM depending on dia. and about 3-5 IPM

spope14 · Nov 27, 2010

Glad you have this fixed.

Hertz · Nov 28, 2010

Philabuster said:
If you bottomed out the reamer hard, that can also oversize the holes. CNCs have little feel when it comes to reamers.

If its a CNC and the hole is not deeper than a standard Endmill length, why not interpolate the hole instead of ream. If its deep, I usually use this method. If the reamer is under 1/2", I leave .01 for finish. If over, I use .015 up to 1", then after that I try to leave at least .02. And as others have said, Twice the feed, half the speed. I don't typically have issues with reamers though as I usually buy the adjustable ones.

WILLEO6709 · Nov 28, 2010

hand sharpened or commercial sharpened drill? Never ever expect the first drill of a hole to cut closer than -0 +0.010 unless you are sure that its sharpened correctly in a precision manner ( that means you did it yourself or its a performance drill from a company you trust). That said in use of jobber drills before reaming,,, I'll pilot the hole in this case about 5/16. Then go through with a drill about 0.010-0.015 under, then ream. The second drill will center on the outer cutting lips not the point if it is off center.... but if tits running out will still cut oversize .

reamer cutting oversize, what to do, and why?

Stainless

Cast Iron

Stainless

Diamond

Stainless

Plastic

Titanium

Titanium

Diamond

Stainless

Stainless

Aluminum

Stainless

Diamond

Diamond

Diamond

Plastic

Stainless

Stainless

Diamond

Similar threads