Cheapest Way to Manufacture an Aluminum Chamber

I will take a single aluminium casting - the size is small, however not small enough to be made from a rod.

making multiple pieces means you have to join pieces say 100mm width plates or so and then machine both sides, join them, ream holes at least 4 places, put ground stud and then tighten by nut. Seems to me a too cumbersome excercise.

Simply take a casting. Mill the 4 sides in square 190. Turn the bore on lathe and then just part the 20mm opening with a parting milling cutter.

Simple, even simpler if you can get a rod or billet or anything of that size readymade, but I doubt.

There is a feature that needs to be manufactured where the 20mm meets the bore.

Could that feature be made symmetrical -- so that a shaped milling cutter could cut it?

I suppose that after everything else is done, you could make a broach that would fit the bore, and that would have an inserted cutter shaped to fit the feature. Then the broach would be advanced with a small cut, then rotated for another deeper pass, end so forth, so that in perhaps 5-10 passes you will have made the feature.

Casting aluminum may not be the best choice. As you said, it's a one of and casting requires tooling. You can get 25mm diameter round bar stock in 6061, that can be cut to the length you want and milled to size. the rest is easy. I've done similar projects before, this doesn't look that tuff.

Do you have a milling machine? What size is it?

Hmmmmm. I am wondering how he could machine a piece 190 mm across from 25mm stock.

Being only one piece I would suggest to use a d=300mm x300mm aluminum bar (which quality depends on the mechanical constrains) and machine all but the feature. After it you can cut the feature profile on a wire-cutting (electro - erosion) machine. I think it will be the most economic way to obtain the profile. Of course it is also possible to use a shaping machine with a linear movement of the cutting steel but there are less and less available. If you have not access to those technologies then only 2 parts solution can be the approach. The problem will be the stability of the assembly. In this case the interior has to be machined in assembled position and after it the 2 parts separated and the feature machined on one of the parts.

For this 2nd step a fixture which duplicates the interface with the other part is compulsory!

Hello,

Assuming that the tolerances are tight ~ +/- .001", the cheapest approach is to rough turn the through hole. Use a lathe set-up with a 4-jaw chuck and leave ~ 0.020" on the I.D. and leave ~0.010" on the diameter of the counterbores on each end. You can finish the depth of the counterbore and overall length to within 0.003". Finish both ends square to the body on the lathe.

Wire EDM the profile to its finished dimension making a pass through the outer wall first to alleviate some of the movement from cutting through the 'Hoop'. The finish may need 2-3 passes as the part may open up or close in when you cut the slot through the outer wall of the bar stock.

Wire EDM the outer faces on three sides in the same set-up to make sure that you are on center with the detail features on the inside.

Finish fly cutting the outside face that you did not wire EDM in a milling machine while holding it by the ends you squared up in the first process on the lathe.

Using the lathe again or a mill take a cleaning cut to finish the counterbores on each end. It is probably a 4-6 hour job with the right skill and the right machinery. Good luck.

I did not use the right words but it is same approach. Electro-erosion is in fact EDM. I think that you need in EDM (now the right word) 2 passes one for taking the most away and a second to finish with a thinner wire ans at a lower current density.

I would prefer to mill the slot before wire cutting to have a fully free of tensions part.

Does it need to be square?

They make Aluminium rod this size and perhaps even squares (Allro Metals in Boca Raton, FL). Producing it from many peices could come with many headaches concernings areas of sealing. You would be much more satisfied with as few piesces as possible.

Cheers

This radius is the only part I see that would be a problem . Everything else should be a snap on a mill. This to could be done .... just a pain and would take more time. Is it just an oil or grease slip?

That can be easily generated by end mill or EDM or even a fly cutter (if th profile is similar on both sides of the slot.

Similar pieces (pillow blocks) we used to machine long back, except tha parting of course and it was easy as i said in #1 - square mill, turn on VTL and then drill the grease hole (we too had one but it was at center and not at the edge also we had a grease groove there to distribute the grease along periphery.) And it was a bit more complicated, the bore was not at center of the square.