small diameter orifice machining
At work I have been asked to machine a small spray nozzle for some testing. The orifice will be machined in 316 stainless, 1/4" diameter. The diameter of the holes range from .020 to .040.
The problem is, I have been asked to machine these with concentricity and roundness specs of +/- .0003 (roundness of hole and concentricity to outside diameter).
Will I be able to obtain such precision on a lathe using a four jaw chuck and standard drill/ream processes? I know that this is very machine dependant...but I guess that I am asking that this question be answered on a "best possible machine" way
Thank you for your help
Bison makes a high precision 5C collet chuck that has adjustable centering on the backplate like the "Buck Adjust-Tru" 6 jaw chucks. New England Brass - listed in HSM sells them.
Use "Solid Carbide Printed Circuit" drills (KBC sells them) to drill the orfice as they produce a very accurate hole. Your set-up has to be ridgid or the drill will snap like glass (trust me). They produce accurate holes much like a reamer and sould give you what you are looking for.
If you have access to a Hardinge HLV-xx series lathe their spindles are extremely accurate.
I hope that helps a little anyway - good luck!
I agree with thrud, Hardinge is the way. Great machines, I used to get to run one, Boy do I miss it for those little persnickety jobs.
Another little gadjet which will really help you on a job like this is a Micro drill adapter. The good ones have a Albrecht chuck. They have a knurled ring on a bearing, by which you do the feed with your finger tips, really nice on small holes.
I am afraid everything will have to be in perfect allignment to use the carbide drill, get the indicator out and check out tailstock allignment with spindle. Might be shim time.
Run rpms high, but any vibration will likely break bit. Might have to hold down rpms because of this. Hardinge, thats the answer, maybe Monarch EE, I have never ran an EE, some say they are better than the Hardinge, if they are they sure must be good.
Good luck, and don't forget to get a center drill to match, and hold your mouth right.
The Micro drill adapter Halfnut is talking about is a sensitive feed unit. For the kind of accuracy you are hoping for it will be too sloppy. I use an ER-25 collet holder with a MT2 shank in both my tailstock and my mill. I use Lyndex Ultra precision ER-25 collets in the holder. I do use the Carbide PC drills a lot for dilling high temperature alloys. Cuts those high Nickel alloys like a hot knife through butter.
If you take reasonable care and don't force the bit (the chips will bind the drill in the hole if you do that) the .030" - .040" orfice will be easy to drill through that cheezy 316 SS. Try to keep the hole depth below 1/4". Use the highest speed on the lathe.
If you have a 1/4 HP Foredom Flexshaft machine with the HD BB Collet handpiece it could be used in a boring bar holder to drill it as well - crank it up to 20,000 rpm! A Dremel tool is too sloppy to use in this application.
If you have access to an Air turbine tool with 1/8" collets this would be the best choice - 50-90,000 RPM.
The reason I mentioned a ridgid set up is because these drills have 165* points. They will wander and break if the surface is not perpindicular to the bit. The larger bits are more tollerant of surface irregularities.
The smaller ones from a #80 and down are fragile and more care is needed in manual operations.
If you have access to a lathe with .0002" runout you should be able to just squeak it in under the wire. The Hardinge has a .000025" runout (FYI $60k Canadian LOADED).
Are you sure they REALLY need them that accurate? What the heck are you building - missle guidance systems?
Another thing you can do to help hold concentricity as well as location is to start your hole with a carbide 2 fl. endmill (this means we're off the lathe and on the mill now). This will not only help keep the drill from walking, but you can hold size better, too. But keep with carbide. With dia's that small, 316 will wipe out HSS reamers. Maybe flush the cut with something thick (my shop likes TAP MAGIC), and take tiny pecks.....everyboy's advice is good....
Have you thought about EDM, wire or ram. The ram type will keep you from having to drill any holes with small drills and will give tolerances you want and excellent surface finish.
EDM is not a bad idea - a job shop could whack em out for you cheap (sort of).
You could also get them perforated with a laser - I am not aware of anyone who does it commercially. Perhaps your Local University could help in that.