AN fitting form milling
AN fitting form milling
(OP)
Hello all,
Im currently doing a lot of short run castings(batch numbers 40-100) requiring an- fittings of various sizes. The ones Im dealing with are an-8, 10, 16, and 20. These are coming to me pre-made with an approx thread length of 10mm across all the an- sizes. Im not fully up to speed on the many types of an- adapters but these ones have all UNF threads on my casting entry side and the ends are just flat(no cone/taper). They contain an o-ring also that needs to seat against a tapered edge on the casting.
I have a cnc mill but it has not got a tool changer so as you can understand the tool changes are slowing things down even though I load ten castings into the jig at a time.
The castings at the fitting areas are just the size of the an- counter-bore at the face - as in it is like dealing with an 8mm walled tube end. There is no extra material outside the counter-bore as you would have if it was in the middle of a tank/flat surface.
Currently Im machining them in 4 steps.
The end face is milled flat with a 10mm solid carbide end mill, this totally provides the counter-bore/flat face in one move(circle).
Im then milling the inside with the same 10mm bit in two z passes, each approx 7mm deep. This provides the finish diameter for the carmex single point(s) thread mill.
I then change tools to the thread mill and machine the thread.
The thread mill then gets swapped out(again!) and an angled cutter fitted to provide the finished angled seat for the an- o-ring to seal against.
As you can clearly see, this is a lot of work.
Ive looked for an- form drills with not much luck. Im not sure if you are to spec these exactly the bore you need(possible chatter risk?), or say a third the bore size and treat them like an end mill and machine around in a circular fashion - cutting the finish bore, and counter bore in one pass.
Im also not sure if I should add the angle seat pass to this tool and cut that at the same time too. Im then wondering if I could also add a threading insert to the mix and do the entire lot in one go finishing at the bottom of the cut with a complete circle after tracking down from the thread cutting(spiral cut)
Obviously with an undersize form bit I could do all of the different sizes with one, but I wouldn't be able to add in the threading insert to the single tool as the threads are different depths in respect to the minor(internal diameter).
Im confident the thread mill could be done with the rest, as the tool could be made very short and stiff if I did go with one tool per fitting.
If I had to make a tool at this point I wouldn't mind, I could fix carbide inserts to it for long life.
So, what are peoples opinions and how the hell are these normally done?
Its worth keeping in mind that this is a ''No one will die if it fails'' sealing application - but obviously them not leaking is a plus
Sorry for the long winded post on something pretty 'simple' but the tool changing is driving me insane.
Brian,
Im currently doing a lot of short run castings(batch numbers 40-100) requiring an- fittings of various sizes. The ones Im dealing with are an-8, 10, 16, and 20. These are coming to me pre-made with an approx thread length of 10mm across all the an- sizes. Im not fully up to speed on the many types of an- adapters but these ones have all UNF threads on my casting entry side and the ends are just flat(no cone/taper). They contain an o-ring also that needs to seat against a tapered edge on the casting.
I have a cnc mill but it has not got a tool changer so as you can understand the tool changes are slowing things down even though I load ten castings into the jig at a time.
The castings at the fitting areas are just the size of the an- counter-bore at the face - as in it is like dealing with an 8mm walled tube end. There is no extra material outside the counter-bore as you would have if it was in the middle of a tank/flat surface.
Currently Im machining them in 4 steps.
The end face is milled flat with a 10mm solid carbide end mill, this totally provides the counter-bore/flat face in one move(circle).
Im then milling the inside with the same 10mm bit in two z passes, each approx 7mm deep. This provides the finish diameter for the carmex single point(s) thread mill.
I then change tools to the thread mill and machine the thread.
The thread mill then gets swapped out(again!) and an angled cutter fitted to provide the finished angled seat for the an- o-ring to seal against.
As you can clearly see, this is a lot of work.
Ive looked for an- form drills with not much luck. Im not sure if you are to spec these exactly the bore you need(possible chatter risk?), or say a third the bore size and treat them like an end mill and machine around in a circular fashion - cutting the finish bore, and counter bore in one pass.
Im also not sure if I should add the angle seat pass to this tool and cut that at the same time too. Im then wondering if I could also add a threading insert to the mix and do the entire lot in one go finishing at the bottom of the cut with a complete circle after tracking down from the thread cutting(spiral cut)
Obviously with an undersize form bit I could do all of the different sizes with one, but I wouldn't be able to add in the threading insert to the single tool as the threads are different depths in respect to the minor(internal diameter).
Im confident the thread mill could be done with the rest, as the tool could be made very short and stiff if I did go with one tool per fitting.
If I had to make a tool at this point I wouldn't mind, I could fix carbide inserts to it for long life.
So, what are peoples opinions and how the hell are these normally done?
Its worth keeping in mind that this is a ''No one will die if it fails'' sealing application - but obviously them not leaking is a plus
Sorry for the long winded post on something pretty 'simple' but the tool changing is driving me insane.
Brian,
Talk To Other Members
RE: AN fitting form milling
http://imageshotfrogin.blob.core.windows.net/compa...
Brian,
RE: AN fitting form milling
"AN Countersinks" are available everywhere.
( As I told my friend Frank Z. after he complained about having to single point the double taper on a bunch of parts. I apologized for not having told him before he started cutting. )
I think most of them also include a cutting edge to do the flat, so you can eliminate that, but your process changes to:
Drill to tap drill size.
Csk tapers and spot face.
Whirl thread.
... and start saving for that toolchanger.
Mike Halloran
Pembroke Pines, FL, USA
RE: AN fitting form milling
I was hoping you would answer.
Im failing to find a countersink with a built in counter-bore that doesn't look like it costs 50 pence but Ill look harder.
As for saving for a tool changer, try saving for a totally new machine - But something has to pay for said machine so Ill have to struggle on with the current old dog in the mean time!
Thanks,
Brian
ps, spot face is the word I meant - Im well into the small hours here.
RE: AN fitting form milling
McMaster-Carr is calling them "Mil. Spec. Hydraulic Port Counterbores"
MSCDirect.com is calling them "Porting Tools",
and lets you sort by AN/MS/SAE standard number, which is useful because there are small differences among the various specs.
The prices being asked for these low volume commodity HSS tools are in the range I'm used to paying for custom carbide tools. ... but it's been a few years since I've bought those too. You should ask for quotes from sources more local to you.
A Google search on "hydraulic port counterbores" was fairly productive.
Mike Halloran
Pembroke Pines, FL, USA
RE: AN fitting form milling
Attached is a link to McMaster Carr if you do not have it.
B.E.
You are judged not by what you know, but by what you can do.
RE: AN fitting form milling
The term we used was port cutter but not only were we making o-ring boss ports but the whole cartridge port with a form tool about 4"-5" in length.
Bill
RE: AN fitting form milling
Thanks so much for all the links and info. It seems I was searching the wrong terms and by searching the correct ones brought up this beauty,
http://www.dexport-tool.com/iso.html
Its exactly what I need and replaceable inserts too(material is Lm25 and tough on hss)so Im going to mail them in the morning,
Brian,