Here is s revision to what I want to do. Length is still 70mm, OD at 25 on the ferrule. 316 SS

• http://files.engineering.com/getfile.aspx?folder=0507de65-50d1-49ea-9c70-e3

I don't see anything terribly difficult for a turning machine to accomplish with rather typical tooling. What is the tolerance on the diameter of the through-hole - given the application, I don't imagine it is terribly critical. I don't believe 2.5x diameter is a realistic limitation for a center-hole at that diameter.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

So you're trying to drill a 14 mm dia hole 70 mm deep in relatively small OD part that results in a thin wall.

You give the largest OD, what is the minimum?

Does the hole need to be highly toleranced or for example can it be drilled from each end with a slight miss match OK?

What material?

Fundametally, assuming typical material properties etc. then drilling a hole 5X diameter is normally reasonable - I think your bigger issue is the thin wall situation.

Drill the hole before you turn the OD, KENAT.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

Sure, but depending just how thin the wall ends up you could end up still having trouble turning the OD.

I'm not a manufacturing engineer, but it looks doable. Of course, the first thing a manufacturing engineer is going to ask is can it be made from something other than 316. They would much prefer free machining brass or 303 SS. Does the ID have to be one continuous diameter? It's often easier to do with a couple of steps in the bore. In the worst case this could be gun drilled but I don't think your L/D of 5 is extreme enough to require that. I don't see any problem with the barb other than the inside corner radius is probably too small. The inside corner radii should be about 0.5 mm or bigger to allow a decent tool radius.

The second drawing with the side port adds a lot of complexity. The first part could be done on a simple lathe, now you have added additional axis.

----------------------------------------

The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

Sorry, missed the material spec in the OPs second post.

tolerance on this ID is about 0.2mm not to tight.

lol, I bit my tongue on mentioning an alternate material because I feared sounding like a broken record. 303 /will/ have a legitimate impact on the machinability though. 316 can be done, it is going to incur lots of cussing and a longer part run-time, but it can be done.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

Alternately I could weld a kind of half coupling instead of adding the NPT feature onto the part??? then you have to weld as well as machine, so not aure what to think. Smallest OD is 17.5

Honestly when I see the part, I think it's either a good part for a CNC lathe with live tooling, or for a swiss turn machine - depends on quantity of the order, really. Brass would make the swiss turn run like a dream. It will also help, in any metal, with drilling/boring and turning the OD, with a good strategy and possibly the guide bushing.

_________________________________________
NX8.0, Solidworks 2014, AutoCAD, Enovia V5

I've made similar parts and was surprised by how expensive the quotes were to CNC. When I asked one supplier if there was some way to reduce the cost, he said the parts should be made on a swiss screw machine. These days the other option is CNC with live tooling and a bar feeder. These machines can make these parts without any touch labor once they are set-up. For my parts the the cost was cut by a factor of four.

True - It is NOT a single piece, but have you considered brazing rather than welding?

If I braze it would be best to use 304 stainless, and would still need to be sent out to get brazed, and more than likely not the same place doing the machining so not sure the cost difference between machining the whole thing and making it two parts??

You make no mention of cost limitation and quantities required. Those factors will have big impact on whether to build from solid or fabricate.

Honestly, in my humble opinion, that's a really, really simple part. Everything can be cut with off the shelf tooling.
Your hole is only 5X diameter; that's a very normal ratio.

Have you considered using an "off the shelf" fitting in your design? There are literally thousands of different wigits and doo-dads available for purchase. Stuff like this:
http://www.mcmaster.com/#standard-barbed-tube-fitt...

or maybe you can simply remove the barb from your design and replace it with a thread for a stock fitting?

Lots of options.

J

Either of your renditions are not particularly difficult. Use a gundrill for the hole. L/D ratios of 50:1 and greater are not uncommon, with tremendous cycle time and accuracy.

It is better to have enough ideas for some of them to be wrong, than to be always right by having no ideas at all.

Your part is not designed for high pressure with a barb and hose clamp so having some drill walk should not cause a great deal of inacurracy. If you have great concern for drill walk then start the hole with an undersize (12mm dia.) screw machine length drill, grind an endmill to 14mm dia., plunge the endmill into the drill undersize drilled hole and bore a 14mm pilot hole and use the 14mm diameter to guide the 14mm jobber lenght drill you use to drill the remainder of the hole. You also could drill through the part using the 12mm drill and then straighten the hole with the endmill and drill.

There are some other tricks which could be used such as turning the part in the lathe one direction and powering the drill to turn the other direction which will drill the hole closer to centerline.

The question I have is how many are you going to make? This is a lot of planning for a part if you make only 300 a year.

Bill

thanks guys, I appreciate all your help.