What's new
What's new

Drilling a smooth hole without tool marks

Neo6

Aluminum
Joined
Mar 9, 2014
Location
Nevada
I am having a lot of trouble finding a shop that can drill a through hole in stainless steel, the though hole is about 1" deep x 3/32 I need it to be smooth free of tool marks all the way through. Could you folks please recommend a process to do this? Thank you very much in advance.
 
Drills aren't really finishing tools. I find that feeding them at .011 X diameter feedrate minimizes the chip scraping that causes most tool marks. That and 1/2 diameter pecks. Reaming is better for good finishes, and gun drilling gives an even better finish.
 
Neo6, give a little more info. All the above is good advice and will get you great holes, but what is your size tolerance? what's your actual desired finish- just free of scoring or polished? how many holes in this plate, 1, 5, 300? how straight, how perpendicular to the plate faces, and what tolerance on hole location? And maybe most importantly, what's your budget? Any half decent machine shop would know what the fellows above have said, perhaps they are working to a price for you?

Fill us in.
 
I am having a lot of trouble finding a shop that can drill a through hole in stainless steel, the though hole is about 1" deep x 3/32 I need it to be smooth free of tool marks all the way through. Could you folks please recommend a process to do this? Thank you very much in advance.

How smooth? Quantify! You may be looking for finish requirements that are out of line for what use the part is, or you may not be conveying your need in a manner that makes the shops think that you will amount to more than a low-dollar headache when there is paying work to be done. If you quantify the surface finish requirement, then you are able to accurately convey how smooth. You may think something that is nowhere near as perfect as it can get, is quite adequate for your needs. The guy that has to make it gets told "perfect" and he's starting to figure out how to get a temperature controlled room full of very expensive measuring equipment paid for... Perfect is expensive. How expensive does it need to be.
Tolerances? Again, quantify and write down.

What kind of stainless steel? Some cut better than others. Some are just misery.

That purpose is the part? Some folks won't touch anything that looks sketchy for any amount of money. Gun parts, drug paraphernalia, etc.

Cheers
Trev
 
Drills aren't really finishing tools. I find that feeding them at .011 X diameter feedrate minimizes the chip scraping that causes most tool marks. That and 1/2 diameter pecks. Reaming is better for good finishes, and gun drilling gives an even better finish.

Under 12X, gundrilling looks like it was done with an axe....ream then lap.
 
If the job was large enough a special might drill and then ream in one hit but likely too costly and increased tool length might cause location problems. Drill and ream two operations and so also time and tooling. Could burnishing or ball burnishing fit this need? The very best drill sharpening with perhaps a split point to make center better for somewhat less tool marks.. but yes a drill is not a reamer. *A second OD margin (double margin) would help... but again that is a special.
Perhaps not that special from this source.
http://www.panamericantool.com/pdf_catalogs/catalogs/double_margin_drills_PAT.pdf

Special Drill and Reamer a source for a good tool for a better price.

But Pan at $2.07 for a 3/32... SD&R might not beat that price... wow that is a good price. flute length 1 1/4 so not many re-sharps (if any) but for that price it doesn't matter.
 
Two things will leave a bad looking hole: A slightly bent drill(will leave spiral scratches,especially in large size drills),and chips will scratch the hole in deep holes. I'd suggest the shop try to get straighter drills,and do more pecking. Beyond that,you'll have to pay extra for reaming.

A straight small drill can be selected by rolling the bit against a counter top under the finger. Look at the drill to see if it has a wobble when rolling. They'd probably think that would be a PITA,though. Even "good" brand drills can have a curve to them.

How about drilling the holes with a straight flute solid carbide drill,and lots of pecking?
 
I've had pretty good luck with four flute core drills in steel, but core drills are getting hard to find. I have also heard good things about OSGs 3 flute drills for steel, but I have not tried them.
 
Bore, indeed,chuckle,chuchle

Drilling? DRILLING?

If you need a *perfect* hole you probably need to BORE the hole.

Say you drill a .086 hole 1 inch deep . What boring bar would work. In the olden days we would say a boring bar for this would look like a fly out on the end of a toothpick.
 
Last edited:
Reaming and stainless is usually a bad combination. To much rubbing on the flutes, the part work hardens and things get nasty. I'm in the single point boring camp.
 
Both boring and honing have been suggested. The OP was talking about a 3/32" diameter hole, wasn't he? Do they really make boring bars or hones in such small sizes? Can someone post a link to such a tool?

Or do you have to make your own? If so, how?
 
Both boring and honing have been suggested. The OP was talking about a 3/32" diameter hole, wasn't he? Do they really make boring bars or hones in such small sizes? Can someone post a link to such a tool?

Or do you have to make your own? If so, how?

Sure, why not. I'm away at the moment but re meme for sure that Kaiser do a micro boring head, and ism sure there would be many others. 2 mm isn't small in the micro world. I wouldn't however expect the Joe Average machine shop to have facilities to bore this small however and you'd need to ask around. Having said that, I wouldn't expect any significant tool marks for a decent drill unless it's a hack job.

To answer the OP, in stainless I would bore it, and if that wasn't smooth enough then lap it.
 








 
Back
Top