Can this part be cut on a Taig CNC mill with a 4th axis?

[drclawscat]

Hi All, I'm new to these boards; I've just started lurking around this week and learned a ton. Right now I'm considering a Taig 4 axis CNC mill. It's been a while since I've been in the industry and used to use a HAAS mini-mill to prototype and build production parts for a small business about 7 years back, so I'm a bit rusty.

Anyhow, I was wondering if anyone could advise if something like the attached could be cut fairly easily on this mill? It's a basic u-joint shaft from 3/4" aluminum rod. The only strict tolerances I'd need are the holes where the sleeve bearings would be pressed in (.25") and the angle symmetry would have to be quite exact.

I'd figure you'd cut the roundstock to approx length first (>1"), then mount it in the rotary table, have the mill cut the hole for the bearing (.25") and the side contours in the first part of the operation, then have the rotary table rotate the part 90 degrees, and cut the center slot (.5")? Or you could do 4 90 degree operations where half the depth of each side would be cut to complete the part. The top hole I could imagine I can cut using the tailstock and rotary or a separate lathe. Could a 1/8" endmill be used for the whole operation? or would a tool switch using a 1/4" be advantageous? Would the mill spindle have enough clearance to cut that close to the rotary jaws or would you need to leave the roundstock extra long and cut it after the operation?

I'm sure there's someone with more experience that has some thoughts on this. Thanks, this site has been a wealth of information.

[quazga]

Let's see, if I were going to make that the first thing I would want to know is how many need to be made. If it's just a one off then the steps involved are no big deal, but if making a lot of them then the steps involved would be critical.

Here's what you need! http://video.google.com/videoplay?do...38628683391433

If there are any wealthy manufactures in the forum who would like to donate to charity, THEN BUY ME THIS!

HAHAHA! JUST KIDDING!

Ok let's see, back to reality. I don't have a Taig, but I'm sure you could pull this off with a Taig being that the part is so small. I'll assume you want to make a lot of them. I'd use this end mill:

http://www1.mscdirect.com/CGI/NNSRIT...MT4NO=94721801

That keeps you from having to make tool changes. As for clearance, humph! Well, I went to their site and they don't give any detailed specifications for their machines! That's strange. Oh well, in any case that end mill I'm recommending, or something similar, should be long enough and stiff enough to get around the clearance concerns associated with the chuck in the Z axis. Also, you'll have plenty of room to hold it in the chuck and still have clearance in the X axis. You'd be doing four operations at 90 degrees as you proposed.

They are stating 0.0005 inches repeatability! Ok, if that's true then you won't have to ream those holes out for the press fit bearings. But you could play it safe and leave 0.0015 inches of material and hand ream them to size. Or instead of making round holes you could make holes with undulating side walls varying by 0.0001 to 0.0005 inches from the 0.250. That would be a little harder to press the bearings in but it would work.

As for the center hole, yeah, I would do that separately on a lathe. I would start it with a center drill, then drill slightly smaller than the 0.275 and at a depth of about 0.250 and then I would use a 0.2756 or 7 millimeter end mill to square off the bottom and bring the ID to 0.2756.

Once the drilling was done I would part it off a little longer than 1 inch.

I'd also make an appropriately sized slightly smaller OD end stop to reside in the chuck to keep your 0.750 solid round bar stock in the same position for each operation.

Things I'm wondering about are:

What RPM will this turn?

How many do you need?

How strong does it have to be?

It's so tiny I'm thinking that it's not going to encounter very large forces. And there may be the possibility that you could make a silicone mold using the lost wax process and then centrifugal cast them in a low temp metal alloy or even a strong plastic casting resin. Also, along this line of thinking is the possibility to cast them in situ and have the whole assembly already assembled right out of the mold.

[lsces]

quazga Is quite right.

I'd certainly do the job with a long nose cutter like the one he identifies, and 1/8" would be fine for all of the machining. Not having a suitable lathe here, I'd set up a jig to hold the part vertically to surface and mill out the end using the same tool. Finishing a little under size and reaming out the holes, although at this size, a little lock-tite is probably all that is needed to secure the bearings? Running a large number, do all the rotary table end and then re-align for the vertical jig.

[drclawscat]

Guys, absolutely excellent responses. I've learned a ton just from your post, Thank you! In response to your Q's quazga:

What RPM will this turn?
Extremely slowly, it's not intended for high rotational speeds, mainly isolating movements between two bodies.

How many do you need?
A small batch, I would be just be prototyping parts on the machine.

How strong does it have to be?
It would be set in a vertical configuration and assume a max load of about 10 lbs.

This joint would be designed more for angular clearance rather than strength or speed and would face merely minute rotational and lateral forces.

I'll start a fund for your Tsugami, here's two cents in the jar, *plink* *plink*

[FranH]

Why does it have to be round?

If stock were machined square it could be clamped in a vise, indicated for center and machined. A ninety degree rotation to cut the clearance, another ninety for the pin to be straight through.

After the fact it could be chucked and turned round. The end radius (Concentric to the holes) could be hand formed on a belt sander.

Of course not as much fun as programming and cnc.

[FranH]

To be ABSOLUTELY sure that the bearings are inline,....after the first hole is done.

make a work plate, machine the top to be flat, drill and ream to size the pin hole. Indicate the hole to be exactly on center.

Put a slipfit pin thru the first hole on the part and into the workpiece, ( no vise) clamp down, and without moving the table drill and ream the second hole. They will be inline as good as the machine and the stock top and bottom surfaces parallel.

[quazga]

Thanks for the Tsugami donation! HAHAHA!

In addition to everything else, including Fran's clever way of making them without budging a single electron , there is also the CV option. With 4 axes you can make CV joints and not have to bother with pressing in bearings. You can also make flexible shaft couplers like these.

And don't overlook all of the 3D printing options that are becoming more and more readily available. A good place to start when looking into 3D printing is Shapeways' materials page.

[drclawscat]

Fran, quazga, good points and excellent suggestions. The shapeways site is really pretty amazing for additive rapid prototyping at really fantastic prices. I will probably order some parts of there for fitment testing before investing in a mill!

Both the CV option and block joint are interesting concepts which I hadn't considered before. I'm going to keep reading and absorbing to learn more.