Workholding

[Swede]

Sorry to be asking so many questions lately. I just feel left behind with technology, and I really need to get better at some CNC basics.

Here's what I want to machine from aluminum stock. The ring is 0.375" thick, and about 1.4" in diameter. I want to use 1.5" wide and 0.375" thick aluminum stock. I'm having a devil of a time trying to figure out how to secure the stock, considering that as the thing gets cut out, it's going to be fairly fragile. I've even thought of super glueing the stock to a sacrificial base, and then dissolving the glue.

Ringing and chatter may be an issue. Any thoughts? It's a 60% miniature of a machine gun anti-aircraft sight.

 

[mu38&Bg#]

Glue sounds like a good option, but it would have to be some strong stuff. I recently cut a hydro foil from 1/4" stock that was .010" thick. at the leading edge. I used candle wax to hold it to a sacrificial tooling plate. In your case you have very little surface area for holding the part. I'd think about clamping it with a 1/4" aluminum plate over the sight portion and machine the outside. This requires you to machine the internal features first locate it in a tooling plate and clamp though the part.

Of course if you're were doing it like I usually do it, just clamp the stock in the vise and have at it, by leaving the perimeter for the last op it's stable. Rough and finish center bore, rough and finish crosshairs, rough outside leaving 0.5mm to the bottom, finish right through the stock. The only trouble is that you the part can make a quick exit as the last bit of stock holding the part is cut, and this can cost you a cutter. Last option is to leave a few small tabs to hold the part in the stock that are manually finished.

Gosh, I edited this post several times. I was pretty sick this weekend and my head still isn't clear.

 

[MachineTom]

Looking at the piece, assuming you have CNC mill. Mill for thickness, bore the center hole first, make a tight fitting plug for that hole, that can take a center bolt if the table has that, or just reach across with a hold down. place a hold down on the Tab feature, at all times have two hold downs tight as you move around the clamps, while milling the circle. First mill the inside of the outer circle to 50% depth, then the outside circle to 80%, then the inside to 80%, next mill out the inside features,then the mill the inside circle through, and lastly cut the outside circle through. At all times apply clamps with blocks in qradrands around the piece, leave you finsh passes at .005-.010, blow away as you mill, keep the grooves about 1 1/2 X cutter D, for chip clearance, If you are sure of your hole placement abilities drill all the radius corners before any milling begins, with that correct diameter drill.

 

[kvom]

Here's what I might do:

Drill two mounting holes, one in the center of the sight, and the other on the left in some extra stock on the "foot" (will be milled away later). Mount on a fixture block with screws/nuts and mill the outer profile, plus the 4 pockets leaving a largish roughing clearance.

Next, mount softjaws on the vise and mill a pocket to match the profile. Position the pocket so that the foot with the mounting hole, to be milled off, is outside the jaws. Then rough the center pocket and the finish passes on all 5 pockets. If you make the pocket relatively deep you'll get good support for the outer walls.

Finally mill off the extra material on the foot.

 

[steamer]

You could put some temporary screws in the "pie pieces" while you machine the outside profile and the center diameter. Then set the part on a pin inside the central diameter and with some clamps and machine away the pie pieces.

Dave

 

[shred]

I'd consider milling it into some thicker material, to the depth you want (thus leaving a block of material for holding purposes), then flipping it over and milling off the excess.

 

[bearcar1]

Not knowing much of anything about CNC, my thought was what Shred mentioned. Make the part on a thicker than needed piece of stock and then when the part is completed, flip the lump over and finish to final thickness. Thm:

BC1
Jim

 

[Ken I]

I like Shred's method.

I have done similar fragile pieces by machining the outer profile then casting it into hard polyurethane / aluminium powder mixture.

Lay it face down in a suitable "box" = steel plate coated in release agent - box formed with modeling clay - no release agent on the part - it becomes bonded in.

After curing, machine the backside flat - remove from plate - turnover - mount (drilled holes through the poly - whatever).

Do the internal machining and then drop the whole thing into methelene chloride for a few hours to break up / dissolve the poly.

Method also handy for mounting castings which have no real way of being mounted well (imagine a hemisphere that you want to bore out).

Also aluminium reinforced polyurethane makes great casting fixturing blocks for limited production. In this case you use release agent and remove the part - the "hole" now acts as a nest for subsequent parts - have used this method for fixturing CI parts in production runs of up to 1000 parts.

Ken

 

[Dr Jo]

My first rule with any part like this is try to machine it out of a piece of stock that is somewhat bigger than the part you want to end up with to allow for mounting.

As someone without any CNC equipment I would look to find a piece of durallium rather than aluminium and screw it down to a piece of steel with the screws around the outside of the required piece then I would then mount both on a rotary table.

Having machined the inside of the sight I would then machine the outside, place a piece of aluminium plate over the top of the sight and the waste original material and apply a clamp (the waste around the sight prevents over tighting and crushing the work). Then machine either side of the base, move the clamp up and finish the final edge.

Jo

 

[Swede]

Sorry it took a few days to reply - these are awesome suggestions, and have given me a lot of food for thought. I need to re-train how I do business with CNC. Something as obvious as doing the central bore first never occurred to me. I'm used to taking the g-code Visualmill delivers, and having at it, in whatever order it decides. At worst, I'll need to check it in some areas of Z to make sure the tool doesn't hit some strap or bolt. But generally, I tend to be a slave to the system, rather than forcing it to do things MY way.

My first thought was to locate the rectangular tab part within the stock, then drill and counterbore for 2 #8 SHCS which will have to be done anyhow to mount the sight on the finished base. Once the bottom is secured, that leaves the ring area, and as that gets hollowed out, it's going to want to vibrate, probably pretty badly.

I'm definitely going to re-read (slowly) all of these suggestions, and then come up with something. I'll let everyone know how it goes.

Thanks again!

 

[blighty]

or...... you could mill the part in one hit out of thicker material. then put the part in the lathe and face it to size, that's only if the "tang" on the part will fit between the jaws of a 3 jaw chuck. if not, i would go with the center hole first option.