Q: Drill diameter for reamed holes.
I have a few blind holes that I'm looking to drill out with flat bottoms.
Can anyone tell me what the rule of thumb is for determining the drill size prior to reaming.
I.e.
6.5mm hole reamed.
What drill bit should I use?
Additionally, I'm looking to ream 12.5 and 14.5 mm.
Thanks for any help.
Similar Threads:
How I was taught
If you are over 1/4 inch in diameter (or 5mm). Drill the hole .020 to .030 inches undersize (.5 to .75 mm).
If you are under 1/4 inch in diameter (or 5 mm). Drill the hole .010 to .015 undersize (.25 to .30 mm).
The closer the drill to the reemed size the tighter the hole will be. Do not run the reemer in and out of the hole only in and flood it. 1/2 the speed and 2 x the feed for highspeed. flood the coolant.
A rule of thumb is that a reamer can remove about 0.5% to about 1.5% of its diameter; for your 6.5mm hole this means the drilled hole will be between 6.48mm and 6.40mm. Stay closer to the larger drill size for small holes because small reamers are not as strong.
It is possible to force a reamer to remove much more than this but not good practice. Also if you are working with an adjustable blade reamer take even less per pass.
With blind holes an adjustable reamer cannot be used but even a regular reamer will not ream a blind hole to size the entire depth. The leading end of a reamer has a slight taper and does not cut full size until about 60% of the diameter back from the end.
A final note with reamers is never, never ever rotate them backwards. If they are intended to cut in a clockwise direction turn them clockwise both going in and out. And don't turn fast and go in slow; run a reamer at maybe 10% of the speed you would drill a hole, use plenty of cutting fluid and feed at up to 10% of the diameter per revolution.
An open mind is a virtue...so long as all the common sense has not leaked out.
Yea I figured the tip of the hole wouldn't get reamed.
Normally I'd use a boring bar, but 6.5mm, is a tiny hole.
Maybe I'll try grinding down a boring bar.
Thanks for the tips.
For those holes where you can get the correct size end mill, you might grind relief on all but one flute for full depth. Then grind relief above a short portion of the OD "ribbon" on the remaining flute. In effect, you have a single point boring tool for the end mill's diameter. I had a whole drawer full of those in my tool box. They are easy to mount in end mill holders or collets.
DZASTR
What about just center drilling with the correct size endmill.
Do they wander to much, or is there a problem with chips?
I was looking on mcmaster and they have most of the sizes I need in a center drilling end mill. Rated at +.001"/-.000". Where I think they reamer is rated at +.00019".
Obviously the reamer would be more accurate, but I can I actually expect to get a 6.5mm +.001" hole with an endmill.
Sorry if that is a newbish question. Traveling in uncharted waters here.
Thanks
You say "center drilling end mill". Does this mean the cutting end has an end like a spot drill? In other words it would tend to be self-centering when entering the material?
If this is the case it may be worth trying.
If it really says "center cutting" chances are it will not work. A center cutting end mill can make a hole from scratch but it will tend to wander around and the hole will not be accurate.
An open mind is a virtue...so long as all the common sense has not leaked out.
Center cutting is what I meant.
I've seen drilling_mills. But that wouldn't help me in this case.
Here is a really crude suggestion...that does work.
Get a used 2 flute end mill the correct size, but not too used, all you want is the initial really razor sharp edge taken off.
Take it to an oilstone or if you don't have this some fine emery paper held flat on something solid and hone a tiny radius on the corners of the cutting edges; tiny means a few thousands of an inch, .010 to .015.
Drill your hole undersize like you would for reaming, you should be spotting it with a spot drill and you can take this deep enough to leave a small chamfer.
Now go in with your modified end mill almost like you would with a reamer, slowish rpm and fastish feed. The dulled and rounded cutting edges hold the end mill centered in the hole. There will be a little radius at the bottom of the hole from the dulled corners but that is unavoidable.
An open mind is a virtue...so long as all the common sense has not leaked out.
What I was referring to in #5 above was substituting the modified end mill for the reamer or boring tool. Boring feeds/speeds. End mills are not usually ground flat at the tip but have a slight concave angle. That results in a slight convex shape at the bottom of the hole if bored full depth in a blind hole.
DZASTR
reamer
Hey guys. I was reading this post and though fairly inexperienced, I would like to offer my oppinion, and let you all tell me if I am wrong. lol.
I would use a fractional drill size smaller than the finall reamed hole. I would convert the metric to standard by multiplying the number by .0394. If the material was hard such as a2 or d2 I would go with the letter size smaller to take it more easy on the reamer. I don't know if I would use an enmill though I mean yes it would work but depending on speed and heat, your hole could still wind up being bigger. Depends on the tollerence, but if there was that much you propably wouldn't be reaming it anyway right. Besides why dullen your end mills when you don't have to. Drill bitts are much cheaper.
Metric - 0.3 mm under, Inch - 1/64 under.If you want a 6.5 mm reamed hole, drill 6.2, if you drill 6.48 ??- 6.4 you will most likely loose it. Don't forget to cut your speed way down and lubricate. This is gen. shop practice for use in drill press or vertical mill. In a belt driven Bridgebort for reaming speed just switch to "low speed" without changing the belt from the speed you used for drilling
Blind holes, flat bottom can not be done with a regular reamer. You need an End-reamer like for jigbore use. You will still have a small radius on the bottom. If you cut off a standard reamer you will have to stone a radius on the bottom. Do it in a vise using a triangular oilstone and tooth after tooth stone a light radius with a back up. Do not try to stone a radius on the end while the reamer is turning in a chuck.
I use a drill that is .0156"-.0312" smaller than the reamer.
The material being cut is also a large factor, as well a feeds and speeds.
Make sure that your center drill leaves a slightly larger chamfer than the reamer size.
In plain 1018 CRS steel I would use 300-400 rpm and a high feed .018" per. rev. for the larger drill size (.015") and a 4-6 flute carbide tip reamer, about 15-20 percent less feed for a HSS reamer. The higher feed insures a straighter, tighter hole size. Non-ferrous materials use abit faster RPM and about the same feed ratio.
Also, I know this sounds crazy, but I have actually reamed a dead on hole size in non ferrous materials with a spiral flute bottom tap, in a rigid collet chuck feeding at a slow feed. The teeth on th tap act like a bunch of very precision cutting edges. Works great in aluminum. Nice finish to.
And when you discovered this little tidbit, were you intending to ream the hole or thread the hole?Originally Posted by jefilomeno
It does sound like a heck of an idea, better than using an endmill, because the upper body of a tap is not relieved, so it will burnish the hole, yet the contact is minimal, and coolant flow should be good.
Plus, the rake angle of the spiral flute will give a nice positive cutting action compared to the dumb scraping of a straight flute machine reamer.
First you get good, then you get fast. Then grouchiness sets in.
(Note: The opinions expressed in this post are my own and are not necessarily those of CNCzone and its management)
Reaming with a spiral flute tap...
I was actually tapping a pretty deep hole, so I wasn't using the tapping cycle. The problem was getting coolant to the bottom and so I wrote a peck-tap cycle to reciprocate in and out but not comming out of the hole completely as to keep the threads timed correctly. Well as most of you know FEED HOLD dosen't work in a tapping cycle until the tap comes out. Not the case in just a standard G01. So, the tap stopped mid cut and just turned while inside the hole. The spiral is on a tight helix so it was like dozens of little boring bar edges polishing the hole to .250" As I investigated my screw-up, it came to end happily with a new found, as you said tidbit. And there you have it...And when you discovered this little tidbit, were you intending to ream the hole or thread the hole?
It does sound like a heck of an idea, better than using an endmill, because the upper body of a tap is not relieved, so it will burnish the hole, yet the contact is minimal, and coolant flow should be good.
Plus, the rake angle of the spiral flute will give a nice positive cutting action compared to the dumb scraping of a straight flute machine reamer.
Deviant
6.5mm converts to .256 (English) of course you can ream it. I don't see the problem.
Flat bottom the hole using a 4 flute center cutting 1/4" carbide end mill (rough the hole with a 15/64 if needed though I doubt it), go as deep as the tolerance allows. Don't use a 2 flute, use a 4 fluted end mill, it will not distort due to torque and most end mills are designed .001/.002 smaller to allow for deflection, but with a straight cut down deflection is not a problem. with the right speed and feed I doubt you could get a .2500 pin gauge into the hole.
Now, take the reamer, .2559 (.256) and grind off all but .010 of it's lead, that's plenty to guide the reamer, and if your at the top of your tolerance with the milled hole your reamed hole can be within .005 of the required depth.
It takes some finesse since reamers can cut both over and under their stated size, so practice on scrap of similar material, low RPM and as aggressive a rate of feed as the tool allows.
Now it's up to you, adjust from there.
Deviant
You mean center cutting not center drilling.
See my last reply to your question ^_^
That's good Geof
If my comments were not six years behind yours, we could have taught each other a thing or two.
Re: Q: Drill diameter for reamed holes.
Use Percentage rule IE 98% of drill size, or if bigger 96%
Reply with Quote
