Milling Softjaws of 3-Jaw hydraulic chuck in VMC

Hey guys,

Require a little help.

I need to cut square pocket (6" x 6" square with 1" corner radii) in CNC-lathe soft jaws. Plan to do it in VMC (I don't have turn-mill setup yet!).



I would be putting a slug in centre ofcourse while milling. I am concerned with ensuring that softjaws remain in clamped condition and not vibrate/move while milling.

Need ideas how to ensure softjaws don't move?

Take a light boring cut on the inside, measure, then turn a slug to fit. Demount the jaws and clamp them in the VMC vise around the slug, mill to your profile. You may need shims between jaws when boring and milling to keep registration.

Ed.

How do I clamp jaws in vice ?

I am not gonna use pie jaws.

Will be welding ring segments to soft jaws in this case. (Since there is just a boss in square plate which we need to turn in lathe; and it's centricity w.r.t outer square is not that critical).

How about buying a cheap 4 jaw scroll chuck and chucking that in your 3 jaw? Quite a bit more universal in application than going to a lot of trouble making these special jaws and trying to get them mounted accurately, from lathe to mill back to lathe again. When I think about the distorting aspects of welding ring segments onto soft jaws and then trying to figure out where the hell everything is, all I get is "does not compute"

Another way to do it would be to make your 4 cornered ring as a form of collet which you chuck in your 3 jaw. You would split this ring on one side, the side that is positioned midway between the jaws aligned with the single corner radius.

If you think you will be doing this more than once on different jobs make a threaded plug the size of your draw bar. put a big flange on it. then use spacers to put in between the back of chuck and your threaded plug with flange.
as you screw the threaded plug in this will tighten the jaws on the spider( like a manual drawbar.
if you think ahead you can tighten the jaws from the top in the chuck through hole whiles its mounted on the mill.

also done it with big hose clamps around the outside of the jaws that works too

Vishrut said:

I am not gonna use pie jaws.

Click to expand...

The attachment you show is/are "Pie Jaws".

If you are not using Pie Jaws, I would try drawing it up in your software again, with regeler jaws. If your square fits into regeler jaws, there isn't a great way to get good repeatability, unless you take the whole Chuck off the Lathe and put it in the VMC. (which may not be a bad idea...?)

The location of the jaws is based on the Position and Parallelism of the serrations to the Masters.

R

turn a disk, weld on the jaws (probably have to tack them while bolted to the chuck), mill the pocket, then split it into 3 segments.

Remove the chuck and mount it in the VMC to mill the jaws in situ.

It will be quicker than any of the alternatives.

You'll need to turn and thread a disk that you can screw into the draw nut, and then clamp down onto the table to close the chuck.

Depending on the chuck, and if you buy good soft jaws (Monster Jaws) I have had good luck just picking up off the outer/flat edge of the jaw. Had a job where we had to bore and groove an existing hole in a rectangular block, and the hole was not centered on the rectangle either. I modeled up the pockets to make sure the whole thing would be concentric, then made three mill programs for it. Y0 was center of the jaw, X0 the left edge - in this case the outer flat side of the jaw. Milled them without compensation, ended up with about .002 TIR without any adjustments.

At the shop I worked at in the 70s and early 80s we ran a lot of castings and had lots of sets of jaws that had strange profiles cut in them. We made a fixture plate to bolt the jaws to so the fixture guy could cut the pockets as needed. Basically it was a 1" thick plate flame cut round with 3 slots in it for bolting the jaws to the plate. There was a bored hole in the center of the plate to dial it in on the mill.

This next part is gonna be hard to describe....

To locate the softjaws, rather than mill in the serrations, there were 2 shallow vee-grooves cut in the plate across each jaw hold down slot. We used pieces of 1/16" diameter wire (tig welding filler rod)laid in the shallow vee-grooves to locate the serrations in the soft jaw blank. Bolt down the blanks and cut away.

Lots of ways to skin this cat. Let me tell you how we make jaws to hold on square that isn't super important, runout-wise.

Mill, or turn, a round boss on a piece of square material (6" in your case) so you can hold it in a set of soft jaws. Don't worry about having material with 1" radius on it, you don't need that.

Orient the square in such a way that jaw 1 is normal to one face of the square and clamp on the diameter you made.

Now scribe a nice line around the profile of the square. With any luck, the bottom corners of the square will be somewhere within jaws 2 and 3.

Take it to the mill, use a wiggler to line the scribed lines up straight in x, and clamp it to the table. Endmill it to eyeball precision; that is all you probably need. If you were running material with square corners, drill the corners out with an endmill.

You do not need to mill the 1" corner radius into your jaws, you really don't. No, really.

With care, you can get really close this way. And if you needed it even closer, you could even figure out the runout, do some trig or draw it in cad, and figure out which jaw(s) needed more material removed, if necessary. But for us doing 3" square shafts with 1" diameters on the ends, this has always been good enough to get within .010" runout.

HuFlungDung said:

How about buying a cheap 4 jaw scroll chuck and chucking that in your 3 jaw? Quite a bit more universal in application than going to a lot of trouble making these special jaws and trying to get them mounted accurately, from lathe to mill back to lathe again. When I think about the distorting aspects of welding ring segments onto soft jaws and then trying to figure out where the hell everything is, all I get is "does not compute"

Another way to do it would be to make your 4 cornered ring as a form of collet which you chuck in your 3 jaw. You would split this ring on one side, the side that is positioned midway between the jaws aligned with the single corner radius.

Click to expand...

We've been doing that, but have to run machine slow parametere...(4-jaw chuck in 3-jaw chuck method).
We have several such jobs, some rectangle and some square. Trying to establish a routine here for future.

I thought of ring-splitted-in-chuck method, but seems ring itself will have significant weight posing ergonomics issue.

lumley32 said:

turn a disk, weld on the jaws (probably have to tack them while bolted to the chuck), mill the pocket, then split it into 3 segments.

Click to expand...

"Welding inside CNC Lathe"....I'm afraid poses a bit of danger and prevents me from doing that!

Vishrut said:

I thought of ring-splitted-in-chuck method, but seems ring itself will have significant weight posing ergonomics issue.

Click to expand...

Here is a thought for making a split bushing:

put a groove on the OD of the split ring, and when you bore your jaws, turn them so they have something sticking out to catch the ring. This way,the split bushing can't come out of the chuck, even when unclamped.

You'd have to install 2 of the jaws, put the ring in, then install the 3rd jaw.

Alternatively, you could drill and tap some screw holes in the jaws and put some screws in it to catch the groove. This would probably be an even better method than turning the jaws like i said above.

this way you wouldn't have to worry about the thing falling out every time you unload a part.

Okay, firstly thank you all for your suggestions..

Here's what I ended up doing: Made custom pie jaws, milled (rather, shaped) teeth in it, mounted on Chuck. Bingo!

Attached videos/images. Tapatalk Cloud - Downlaoad File VID_20190418_102312.mp4

Sent from my Redmi Note 4 using Tapatalk