[SRT Mike]

Ok, I am really interested in you experts feedback. Take a look at these products



They are metal accents for motorcycles. Looking at the top two, they are 2D pieces with a pair of holes in the middle. How would you guys machine such a beast? I am making something a little bit similar but for a different application. If it could be held reliably from the bottom, it could be done in one fixture. However right now I start with a sheet of 6061, drill and chamfer the holes, then use that to mount to a bottom plate that gets fixtured in a vice, then machine the exterior and the chamfer. Thats two setups. I figure I could make a fixture and maybe hold it with vacuum or tape, but tape is a PITA to get leveled perfectly and I dont want to have to do a big facing operation to keep 'em flat. I dont have vacuum right now but it may not work for such a small piece. The bottom of the part is flat.

The quicker we can make them the better. Any advice?

Also, what about finishing? I would love to have them come off the machine and just toss 'em in a vibratory finisher and have them come out with a mirror finish yet retain the sharp creases of a machined part. In other words, I think I need them to come off the machine as well finished as possible and use something like corn cob or walnut shells to polish. So whatever setup I use would need to be rigid and ideally able to let me very quickly mount the parts to the fixture.

Last but not least, if I machine them from a single sheet, there is a lot of waste around the perimeter of the part, so if I could chop them into sized bits first I could make more efficient use of the material.

Thanks for any info!

[CJL5585]

I think that for the flat pieces with holes, that I would have them punched out on a press (sub-contract). That way, the only thing left is the tapered sides and the countersink of the holes.

Countersinking could be done manually on a drill press.

I would build a custom machine which used a metal cam the same shape as the part to have the taper. I would have a motor (geared or stepper) to rotate the part slowly using the cam to hold the tolerance of the part. I would use a very fine grinding wheel to put the taper on the sides.

So far, no machining.

Setups: Vice on drillpress with countersink bit - depth preset.

Setup for edge grinding. Install metal cam with a couple bolts - grinder is spring loaded to hold a bearing (etc) against cam to hold grinding tolerance. No high dollar machining equipment required. No high dollar labor required. No knowledge required.

[SRT Mike]

Well, I already have a vertical CNC mill, and I guess what I am really looking to do is make the most efficient use of a workholder and tooling to be able to make these.

right now, we cut them from a sheet, although we only made a few. I could pre-drill and countersink the holes, then cut the stock into the individual pieces, mount them to a fixture plate (like a bunch of slightly raised cylinders with 2 holes to mount the plates) and then machine the top surface, rough and finish the outside shape, and then do the chamfer. This requires 2 setups though. Any ideas how to do it in one?

[mxtras]

Profile it from a piece of barstock stood vertically, then part it off with a slitting saw? This would be a single set-up with at least three, maybe four tools.

Scott

[MIKE JEFFERS]

2ops will be the way.buy cut billet to size drill/csk 2 holes then fixture on holes
use modded screws that sit below the (finished) top surface then machine fully
from top
i looked at some of these mirror blanks a while ago and they were diecast.
mike.

[Unabiker]

I make lots of similar parts using 3m Super 77 spary glue as the mounting.
You will need a hunk of particle board, preferably HDF, but regular ol' particle board from Lowe's will work. Get a chunk a little bigger than you bar stock, and bolt it down to your table. Surface it with a fly cutter, or the biggest endmill you can swing. Blow it off, and spray down an even layer of the glue. Coat the bottom side of your bar stock with a similar layer. Let the glue dry a minute or two, then place the bar stock onto the particle board. Get it placed right the first time, cause once it's down, it's down. Press it down good....sit on it, lay on it, stand on it, use a 2x4 under the quill and push it down in several places.
Once the stock is in place, go through and do your engraving passes first, then the holes and chamfers. Last, do your outlines and outter chamfer passes. I would reccomend cutting 90% of the way through on the outline pass, then cut the remaining 10% of material thickness during the chamfer pass.
When all the parts have been cut, you will need to use a torch to heat up the aluminum and a chisel to gently pry the parts off the board. This glue gives up at about 130 deg F. The troch does most of the work. If you get too greedy with the chisel, you'll pull parts of the board off with your parts. A trip through the parts washer will be necessary to remove the glue.
For a nice bling-bling finish, I'd hit the parts with the buffing wheel after they went through the vibratory finisher.
Looking at the parts, I would think you could do them with as few as 2 tools; a drill and a v-endmill. Maybe drill all the holes first, then engrave and do the hole chamfer and part chamfer/cutout with the v bit. Just a guess, but maybe 30 minutes of machine time for 12 pieces out of a 24" long piece of bar stock.

[Dan Fritz]

Years ago, I was visiting the IMTS show in Chicago, and saw a very clever way to hold parts like this.

In one of the small "cheap booths" downstairs, there was a guy showing off his new gadget. It used a refrigerant pump to cool an aluminum plate on a small knee mill. He would spray a bit of water on the part and stick it to the plate. After machining, he would use a heat gun to pop it free. The advantage over a magnetic chuck is obvious: Your part can be non-magnetic. I don't know if the idea is practical for you, because the fixture itself might cost more than you want to spend here.

I suppose you could experiment by taking a plain aluminum plate and cooling it in the freezer for a few hours. See if you can stick down your parts and release them easily. The problem with this is that the plate would warm up after a short while, then it's back to the freezer.

[ViperTX]

Well some of the parts appear to be domed, and you have a matte and bright finish on several of the parts, so the bright finish is another op....most likely a buffer and you'll also have a separate op for the matte finish. I personally would use a combination of all the processes mentioned so far.

For high volume I would have blanks punched or die cast, for fixturing there are so many options...you could use a magnetic chuck and use steel pins inserted through the mounting holes...you could also design a holder where the pins are drawn down and the holder is similar to the stem of a mushroom....this would also allow you to hold the items as they are machined, engraved, matte and buffer operations.

[Caprirs]

I'd consider the vacuum setup. Depending on how flat the bottom is, you might use an o-ring to help seal the part to the fixture.

[widgitmaster]

I have done similar parts, the CNC would make 4 on a flat bar, then on a second vice with softjaws contoured to hold the part upside down, the CNC would mill of the excess from the back!

Every cycle start had 4 totally finished parts!

Eric

[2muchstuff]

Machine your part out of a flat bar stock, then into a press to bend the curvature then off to buffing/finishing.

[lstool]

I would do the same as widgetmaster, it all in the fixturing

[SRT Mike]

Thanks for all the advice...

Widgit, I think you win The punching idea is a good one, but I dont do the volume to make it worth outsourcing it. Widgit, the idea with 2 vices is something I hadnt thought of before - very neat idea for ANY project that requires 2 setups.