Help with chucking reamer spindle speeds

Can anyone tell me where to find info on how fast to turn a chucking reamer. I cannot fine anything in Machinery's Handbook and I have searched this website with every term I can think of.

Thanks, John

A lot of folk say to use the speed for a similar-size drill in the same material. I personally go a bit slower than that. Sorry I couldn't actually answer your question but I'm sure someone here can do that.

General rule of thumb is half the speed, twice the feed, of a similar sized drill.

My "rule of thumb" is half the speed, the same feed (in IPM) as a similar size drill (this would actually produce a higher chipload). In mild steel that would be 50 SFM at 4 IPM, where normally I would drill at 100 SFM and 3-4 IPM depending on drill size. This only applies to ye olde high speed steel reamers.

Really the best thing is to look up the manufacturer specs. The old "rules of thumb" seem to be ebbing away as time goes on. If you are using carbide reamers, so much more comes into play. Drill runout, reamer runout, the exact right SFM and feed rate, etc..

Just what Ed said, half the speed and twice the feed.

The chip load is actually lower because most chucking reamers are at least 6 flute. My other "rule of thumb" is not to ream any more than you have to. Depending on hole condition, material, and mood, I like to keep that to 0.015 to 0.035" on diameter.
JR

From Gammons Reamers:
http://gammons.com/files/Tables/Feed and Speeds-new.jpg

Illinoyance said:

From Gammons Reamers:
http://gammons.com/files/Tables/Feed and Speeds-new.jpg

Click to expand...

Thanks Illinoyance, exactly what I wanted (a table I could print out)

John

Gammons also do a stock allowance for machine reaming table http://gammons.com/files/Tables/STOCK ALLOWANCE for MACHINE REAMING-new.jpg

Taken from their reaming hints page Reaming Hints - Gammons Hoaglund Co.

''Reaming Speeds – Speeds for machine reaming may vary considerably depending in part on the material to be reamed, type of machine, and required finish and accuracy. In general most machine reaming is done at about 2/3 the speed used for drilling the same material.''

'' Reaming Feeds – Feeds for reaming are usually much higher than those used for drilling, often running 200% to 300% of drill feeds. Too low a feed may result in excessive reamer wear. At all times it is necessary that the feed be high enough to permit the reamer to cut rather than to rub or burnish.''

I've never had any luck with the 1/2 speed 2x feed rule on any holes I actually cared about. The best advice I've found is G-Wizard's numbers which seem to favour higher RPM and a slower feedrate.

If using a sharp reamer, half the drilling RPM and double the drilling feed are good starting points, and usually work well. Other factors to consider also make a big difference in successful reaming though.

Is the reamer a bit dull and producing a torn finish? (replace it if possible). If it's all you got, try some practice holes until you get your best working process down.

Is it cutting a bit big? (Make sure you aren't trying to remove too much stock, that you don't have too much runout, and maybe try coolant instead of oil).

Is it cutting a bit small? (First, check your reamer condition, then if using coolant, try switching to oil. Too little stock or too low a feed can sometimes cause this also as the reamer will mostly rub instead of cut. You can make a reamer cut a tiny bit larger by slipping a steel shim in wrapped around the reamer that covers almost half the flutes' circumference).

(Now by "cutting big" or "cutting small" I am referring to size of hole vs. size of reamer. If the hole you're trying to ream is .250" and your reamer cuts a hole that's .252" and the reamer measures .252" you have a different problem - mainly lack of intelligence!)

eKretz said:

You can make a reamer cut a tiny bit larger by slipping a steel shim in wrapped around the reamer that covers almost half the flutes' circumference).

Click to expand...

The oldtimer trick I was taught was a wooden matchstick in one of the flutes.

There are a few, but that's the one I have the most luck with. Probably depends how you hold your tongue while doing it...

rpm and sfpm are effected by length of tool and tool holder. i see almost everyday where a longer length tool stickout and or longer tool holder will vibrate or chatter excessively and rpm has to be reduced
.
i often see a straight flute reamer ream many holes ok and some gage pin will not go in cause hole is lobed and or not straight. spiral flute reamers are for stubborn parts and give rounder and straighter hole
.
nothing worse than take a reamer that made good holes before and after a stubborn part and use same reamer in hole with hand drill and still not get gage pin in hole.
.
yes we tried leaving more or less material to ream but makes little difference. lobed holes happen but often hard to detect. my preference is having a few reamers .0005 and .0010 bigger just in case needed