Hey Guys,

I am going to be making PC waterblocks for watercooling, and I think I want to make a jig to hold the pieces in place.


What material should I make the jig out of?
How should I hold the jig down, with holes and bolts I'm guessing?
How much space should be in between the jig and piece? I am guessing not too much.
How would I get the pieces out?


Thanks :D
Burn

with out knowing what the part looks like or what type of cutting(profile thur hole), and if you are going to do any other operation with this jig it hard to make any useful sudjestion

Okay, it's going to be holding a piece to be milled into a heatsink of sorts, like this one: It's the top-right piece.

http://www.insanewb.com/waterblock/cpu/peltier/alvaro/images/av-tec_002.jpg

make a set of softjaws for your vise mill

If you don't want to make softjaws, you could always make a block with the appropriate clamps and such with a key on the bottom. Don't forget bolt holes to lock it to the table.

BTW: Nice parts!!!! :D

:cheers:

Well, those are not mine. They were used as an example....Mine will look much better :D

Softjaws, what are those? Google is my friend.

Ok, what you have not told us is the quantity, the state of the raw parts, and the type of machine doing the work! Are these parts in squared up blocks already? Or are you machining everything from scratch?

MY immediate suggestion ( if done on a CNC mill) would be to use two 6" vises with soft jaws!
1st vise does the top half of one part, then flip the part into the other vise and do the bottom half!

That way every cycle stop is one completed part!

This method is acceptable for all three parts!

Now, if your quantity is in the thousands, I would suggest an indexing 4th axis, with a fixture designed to hold 5-10 parts per side of a square fixture supported with a tail center. Then I would do one side and flip the parts to the other side of the fixture and finish them! This would produce 5-10 parts per cycle start, but increase loading time, and cycle time!

Your choice!
Eric

Softjaws are exactly that, vise jaws that are soft and machinable!

Okay, the raw material will be 4 by 2.5".
I will have a 4th axis rotary table set up.
CNC Taig Mill w/ IMservice servoes
Milling a pocket and drilling holes out, possibly doing full 4-axis work if need be.

because your mill so small, you should stick to two small vises!

I was thinking that too, until I realized I had to contour the outside of the piece!

That's why you need soft jaws!

After you contour the outside of the part, simply write a program to do a reverse contour in the soft jaws, creating a perfect nest for the part to clamp in! Then you can machine the opposite side to finish the part in full!

This is a common procedure in most progressive shops!
Just make a pair of jaws from aluminum, drill the mounting holes. And place a spacer between them and close the vise. Then run your little program!

Next time you do the job, the jaws are ready for quick setup!

Eric

I want to make a jig to hold the pieces in place.



The difference between a Jig and a Fixture:

A Jig guides a tool or cutter into a specific location on a semi finished part, such as a drill jig or tapping jig.
A Fixture holds a blank part in such a way to allow various machine tools to perform various operations on the part.

Eric

Thanks for the clarification! I guess I am looking for a fixture now to hold this part in place.

If you have to do this in more than one operation you have to think "how many operations can I put into one". Example: If you have to square the block up and drill holes on the outside profile and you have a 4th axis, I would hold the block against the 4th with a floating center to push the part against the 4th axis. Then mill all four outside edges and drill the apropriate holes, then put the part in soft jaws for the remaining operation which would be the inside interior of the part and mill across the top surface to bring it into print for the height.

....But that is how I would do it!

See ya!

Thanks for the clarification! I guess I am looking for a fixture now to hold this part in place.

Fixtures are usually made by the machinist who plans on making the parts!
Finding one to do exactly what you need is impossible, so grab a block of metal, a notebook, pencil, calculator, and start drawing different ideas! Usually the simplest ones are the most efficient! I have designed my own fixxtures for over 20 years, and have found it to be the best part of making the finished products!

The best place to start is with the x/y zero datums, because everything is measured from those surfaces!
Eric

Is there any way you could show some of the fixtures you've done and how they hold/operate? Thanks :D

Because I'm retired, and have made only a few milling fixtures in my new shop, I no longer have access to all that I made! Not to mention they did not belong to me, but the company that signs the checks!

You need to do those little blocks in a vise, but you should use a set of soft jaws with a step milled in them just deep enough to do the entire top side first, along with the top section of the outer edges!

Remember, the secret to production is to do the same thing to ALL pieces first, then move on to the next thing!

After you have one side done, then you will have a better idea of what to do next, and how to hold them!

Eric

Yeah, there won't be any work done on the reverse side (bottom), just because I want to keep it simple...And there won't be much point. Thanks for the tips :D

let us see what that blokks will be lookin like

let us see what that blokks will be lookin like


Here...Hopefully this will help to explain what I'm machining. It's 4" by 2.5".

Remember, the secret to production is to do the same thing to ALL pieces first, then move on to the next thing!
Eric

True if you have a manual machine, or have to do manual tool changes. Otherwise you want to do as many operations to the part as possible without removing the part from the fixture. I think the best suggestion was two vices, making a finished part every cycle.

-edit
now that I see your part...
are those through holes? if so I would drill the holes and face the part in a vice in the first operation, then move the parts to a fixture which you made with a threaded hole pattern to match the part, put a few screws in it, then you can finish machining. It would be best if you could afford to put a couple dowel holes in the backside to locate the part to the fixture.

Two vises holding 2 parts to be machined?

Also, RE the piece, it is outside contoured as well as the pocket done inside.

see edit above

Yes, those are through holes, and the big middle thing is a pocket.

When I transfer the part to the fixture from the vise, I lose all my zeroes...What can be done to regain all the zeroes?

Burn,
If you have stock that is 1/8 extra thick, you hold it in vise #1, do the entire part, then flip it into vise #2 and remove the 1/8 extra!

Eric

Well, That's why I would keep all the pockets and blind holes drilled with more distance than needed so I can lap/sand the base flat, optimising thermal transfer.

Still wondering about post 25.

You would need to have a reference location on the fixture to find the zero.

Aaron

Hmm...So would that just be a spot where I re-set the zero while in teh middle of the program? If I use DeskCNC, can I set zeroes mid-way through a program? Thanks a lot :D

My idea would be a block of steel with the shape of the outside contour milled in it and the holes drilled and tapped to line up with the holes in the part. The contour in the fixture would be recessed slightly so that the cutter doesn't touch the fixture. The fixture would be a few inches deep and clamped in a vise. You would just hold the part (still a square chunk) in a vise and set a progam to drill all the holes, then tranfer the part to the fixture, bolt it down with the newly drilled holes, use a dial indicator around the head of one of the bolts to find your 0-0 location and then cut the outside contour and all the rest of the operations on the part. If you had a lot of parts drilled you could just swap them in and out and you would't lose your 0-0 location either.
PS: I am the guy who made the prototype blocks for Burn on a CNC Bridgeport. :D

Hmm...So I would have to write 2 separate programs, one to drill all the holes, the second to mill the pocket and contour the piece?

That sounds like a good idea.

You would have a seperate work offset set up for the fixture. When you make the fixture, you should know the distance from one corner to the holes. Zero off the fixture and set that as one work offset, zero off the vice and set that as another.

Oh okay, I gotcha. And I would use, say, calipers to figure out the distances?

If you make the fixture to a drawing then you don't need calipers, just do the math. Bolt your fixtures to the table, move you spindle to the zero point of the fixture, then enter coordinates into G54 or whichever. Do the same for the vice or other fixture.

No, I meant to find the zero of the fixture....How would I go about doing that?

No, I meant to find the zero of the fixture....How would I go about doing that?


Use an edge finder

Aaron

Should this be what I'm trying to make? 4 holes on the outside to bolt it to the table and then 4 holes on the inside with the pocket to bolt it to?

Not exactly, reverse that pocket so it sticks up above the plate and then you have it.

Okay, how far up should it come? The piece is 0.500 tall.

Just enough for the cutter to pass below the edge of the part, so maybe .5625" tall. I would recommend not making a big base like that since it would take forever to mill all that material away around the part that sticks up. Just clamp it in a vise since you will probably already have a vise on your table.

Okay, so like this? The inital part is 0.4375", then the top part is 0.0625" to keep the overall height 0.5 to make buying metal easier.