[CadRhino]

I was curious if any of you had any thoughts on how I may want to set up a fixture for the following application.
I have a 3/8" thick 6061 Flat bar that I will need to mill out 2 1/2" and 1.9" diameter disks out of.
The disks do not have holes in them so I cannot screw them down and I do not have a vacuume table (yet).
I do have a fixture plate that I could possibly tape the flat bar to with double sided carpet tape but I do not know how well that will hold up to the machining and/or coolant.
Any thoughts would be greatly appreciated.
Best,
Nathan

[SCzEngrgGroup]

Make some small L-clamps, similar to what's used to clamp a vise to the table, and put some holes in another flat fixture plate to screw them into. If you have enough clearance around the edges, you can also just use screw-clamps to clamp the plate you're machining to another plate held in a vise. Kant-Twist clamps are especially good for this. Two of them will hold a part against all but the most aggressive machining.

Regards,
Ray L.

[WOTDesigns]

+1 what Ray said to hold the bar.

By far the easiest way to keep the parts from flying off is to leave 3 or 4 tabs. Program so u leave tabs that are 0.05 thick 0.1 wide should be enough to hold then program another pass leaving 0.003 on the wall (not cutting the disks) and leave 0.02" on the tab/floor. This will leave you with 4 tabs 0.02" thick and another 0.003" thick bit left on the part. Dikes will cut right through the tabs. Clean them up on a belt sander just enough to remove the extra material.

If u need them "perfect" round (no sanding) then machine them from 0.5" bar leaving 0.1 material leaving tabs, machine a set of soft jaws to match the disk size, flip the parts upside down and machine off the extra material leaving a perfectly flat and round disk. This also allows you to face both sides.

Brian
WOT Designs

[CadRhino]

Thanks Ray and Brian for your input.

Brian, I think your methods will work the best since I have no internal holes. I will most likely use approach #2 since I do need very clean edges and will eventually have to do ops on both sides.
Thanks,
Nathan.

+1 what Ray said to hold the bar.

By far the easiest way to keep the parts from flying off is to leave 3 or 4 tabs. Program so u leave tabs that are 0.05 thick 0.1 wide should be enough to hold then program another pass leaving 0.003 on the wall (not cutting the disks) and leave 0.02" on the tab/floor. This will leave you with 4 tabs 0.02" thick and another 0.003" thick bit left on the part. Dikes will cut right through the tabs. Clean them up on a belt sander just enough to remove the extra material.

If u need them "perfect" round (no sanding) then machine them from 0.5" bar leaving 0.1 material leaving tabs, machine a set of soft jaws to match the disk size, flip the parts upside down and machine off the extra material leaving a perfectly flat and round disk. This also allows you to face both sides.

Brian
WOT Designs

[Steve Seebold]

Start with 5/8 or 3/4 inch material, machine your part complete them flip it over, hold it in aluminum soft jaws and fly cut the back off.

[WOTDesigns]

LOL. thanks for the affirmation Steve

Brian
WOT Designs

[WOTDesigns]

All of the aluminum parts in this picture were machined on the mill in a vise from solid bar, then flipped into soft jaws, faced then if they needed work of the back I picked up center off the internal bore

Attachment 264158


Brian
WOT Designs

[CadRhino]

Cool
Very nice
Thanks for the photos

All of the aluminum parts in this picture were machined on the mill in a vise from solid bar, then flipped into soft jaws, faced then if they needed work of the back I picked up center off the internal bore

Attachment 264158


Brian
WOT Designs

[CadRhino]

Looking at these photos again, I noticed that the gear parts in the foreground has a set screw off of the side. Did you tap this before cutting the gears or did you flip it up and do that last. I guess my question is if you did it last, did you indicate off of the gear to find the center. It seems like it might be harder to indicate with the gears cut than before but maybe not.
Just curious.
Thanks,
Nathan

All of the aluminum parts in this picture were machined on the mill in a vise from solid bar, then flipped into soft jaws, faced then if they needed work of the back I picked up center off the internal bore

Attachment 264158


Brian
WOT Designs

[WOTDesigns]

Yes I drilled and tapped the set screw hole last after all other machining was done. I just set it on its edge in a vise so it was straight up/down and eyeballed the drill bit to the center of that tooth. The drill and tooth spacing were close enough that it's probably eyeballed within 0.005" or so.

If it did need to be at a specific angle to another feature (like other parts I've done) I would square the block up to that hole, drill the side feature first, then load the block in the vise with my reference based around that one feature being square to the vise, even if it means machining a square at a 45* angle to the vise.

Brian
WOT Designs

[CadRhino]

Thank you for the insight.
The eye is is amazing
Nathan

Yes I drilled and tapped the set screw hole last after all other machining was done. I just set it on its edge in a vise so it was straight up/down and eyeballed the drill bit to the center of that tooth. The drill and tooth spacing were close enough that it's probably eyeballed within 0.005" or so.

If it did need to be at a specific angle to another feature (like other parts I've done) I would square the block up to that hole, drill the side feature first, then load the block in the vise with my reference based around that one feature being square to the vise, even if it means machining a square at a 45* angle to the vise.

Brian
WOT Designs

[Bryan Turner]

Brian,

So did you make soft jaws for each unique piece? I have a similar project, but only 4 pairs of jaws.. seems like a waste to cut them up for 2-3 pieces each.

Or were you making enough pieces to recoup the cost of the jaws?

Thanks,
--Bryan

[WOTDesigns]

No these were all one or two off. If you plan ahead you can re-cut the same jaws for many different parts.

These for example held one of those and can still be re-cut to hold many others

Attachment 264440Attachment 264442

These had a very small step, and then held round and can still cut another step or round

Brian
WOT Designs

[SCzEngrgGroup]

If you're making a part with no holes, and/or an odd shape that can't be held in a vise, then soft-jaws or double-stick tape are almost your only options. If there are ANY holes, then use a flat plate with some threaded holes, and put screws through the part and into the plate. If there are only a few screws, and/or they are small, you may have to go easy on machining, but I have never once made soft-jaws for a one-off part. You'll be amazed at how well even two 4-40 screws can hold something. I can re-use the same plate for sometimes dozens of completely different parts, by just making sure the new screw holes miss the old ones. The plates eventually end up looking like Swiss cheese by the time I retire them. And it's MUCH faster than cutting soft-jaws. In fact, it's usually faster than just swapping in a set of pre-cut soft-jaws.

Regards,
Ray L.

[Steve Seebold]

Brian,

So did you make soft jaws for each unique piece? I have a similar project, but only 4 pairs of jaws.. seems like a waste to cut them up for 2-3 pieces each.

Or were you making enough pieces to recoup the cost of the jaws?

Thanks,
--Bryan

Bryan, if you machine the height of your soft jaws so the mounting holes are the same distance from the edge top and bottom, now your jaws are reversible and you can run 4 part numbers in 2 sets of jaws to make your 4 sets of parts. OR you could use thicker material, machine your part complete on one side then flip it over and cut the back side off. Then if you need to make jaws to hold your part, you start with the smallest mart and work toward the biggest one.

[WOTDesigns]

Yep... the first and second pictures are the same jaws.

Monster sells reversible jaws that can already be flipped, but I prefer the taller jaws then machine the first side down when needed to flip

Brian
WOT Designs

[Bryan Turner]

I think Ray's technique will work for me, but I've got a question. The parts are "C"-shaped, and have two holes at the 'points' of the C. I'm cutting them out of 1.25"x3" bar, slightly overlapping them like CCCCC to save material. But there's three different radii (so the holes for the different batches won't line up), and the holes are pretty small.

The holes will ultimately be tapped #8-32, but for clamping I assume a clean through-hole is better? So maybe a clear #6 hole for clamping, then widen to tap-size for #8 after profiling?
Will two #6 screws hold a piece that tall firmly enough to cut the tabs and run a finish profile?

Thanks!
--Bryan

[pickled]

I follow the same strategy Ray. A lot of times I just go to Alro and pick up a drop of precision aluminum plate just to have laying around in case I need to make a new fixture plate. Large chunks of UHMW work remarkably well too. If you use 1/4 x 20 screws and tap the UHMW over 3/4" deep I haven't had any parts pull out or shift yet. UHMW is also nice because, unlike aluminum, if you go deeper with your cut you don't have to worry about chip welding.

[SCzEngrgGroup]

I think Ray's technique will work for me, but I've got a question. The parts are "C"-shaped, and have two holes at the 'points' of the C. I'm cutting them out of 1.25"x3" bar, slightly overlapping them like CCCCC to save material. But there's three different radii (so the holes for the different batches won't line up), and the holes are pretty small.

The holes will ultimately be tapped #8-32, but for clamping I assume a clean through-hole is better? So maybe a clear #6 hole for clamping, then widen to tap-size for #8 after profiling?
Will two #6 screws hold a piece that tall firmly enough to cut the tabs and run a finish profile?

Thanks!
--Bryan

Bryan,

If it were me, I'd drill and tap the holes to 8-32 first, and mount to the plate with screws coming up from the bottom. Just reference the plate to one side of your vise jaw, or better yet, use a vise stop, so you can re-mount it in the vise quickly after mounting new stock. Or, screw in long screws, and put nuts on the bottom. Two 8-32s might not be enough for aggressive machining, or it they are both at one end of the part, but should be fine if you just go a little easier. If it's not enough, you'll know right away, because you'll get poor surface finish, and likely chatter. They'll be fine for the finish pass.

Regards,
Ray L.

[Steve Seebold]

I think Ray's technique will work for me, but I've got a question. The parts are "C"-shaped, and have two holes at the 'points' of the C. I'm cutting them out of 1.25"x3" bar, slightly overlapping them like CCCCC to save material. But there's three different radii (so the holes for the different batches won't line up), and the holes are pretty small.

The holes will ultimately be tapped #8-32, but for clamping I assume a clean through-hole is better? So maybe a clear #6 hole for clamping, then widen to tap-size for #8 after profiling?
Will two #6 screws hold a piece that tall firmly enough to cut the tabs and run a finish profile?

Thanks!
--Bryan

All the more reason to start with thicker material and run the parts complete including drilling and tapping all holes, then flip the parts over and machine off the back side.

From what you have described, I would make up a tool that uses Mitee-Bites to hold your parts on the second side.