6-jaw chuck for holding awkward castings question

I have a job offered to me that involves machining several aluminum castings. One of them is a bracket for mounting a fluid pump. It weighs about 15 lbs. In short, I will be grabbing it by its "small" end, likely in my 10" 3-jaw Bison, machining the "big" end, then flipping it 180 degrees to grab the machined big end to in turn machine the small end.

The big end will be machined to result in a 10" OD "ring" about 5/8" deep. Put another way, what I will have to grab is a clean, round, machined feature, about 10" OD, with a depth-of-grab of around 5/8".

My question is this. My plan is to EITHER cut soft jaws for my 10" 3-jaw Bison to grab this, OR to use a chuck that came with my lathe but I've never used: a 10" Buck Adjust-Tru 6-jaw. Important: the Buck has fixed jaws, so soft jaws are not an option.

This is an out of balance load for the chuck. The part will also be protruding from the chuck face about 12". So, it'll put some forces on whatever is grabbing it.

Is this a good application for a 6-jaw or would i be better off making steel soft jaws for the Bison 3-jaw? I simply don't really understand the pros/cons of 6-jaw chucks.

This would be ongoing work with some significant volume so whatever is the best way to hold these things, is what I want to do.

Thank you!

Have you got a 4 jaw independent? that would be my go to.

If not and you have to use self centreing , stick with 3 jaws, any more and you run in to the old milking stool scenario.

Don't forget castings can vary special jaws might fit 1 but not the next.

Don't forget faceplates either

Soft jaws for OP2 are really the only way to do it I can see. Any other way will be inaccurate or waste a bunch of time.

I guess I'm assuming you are making more than 2 of these and the cost of jaws is justifiable. Otherwise 4 jaw makes sense to me.

Long Tom said:

I have a job offered to me that involves machining several aluminum castings. One of them is a bracket for mounting a fluid pump. It weighs about 15 lbs. In short, I will be grabbing it by its "small" end, likely in my 10" 3-jaw Bison, machining the "big" end, then flipping it 180 degrees to grab the machined big end to in turn machine the small end.

The big end will be machined to result in a 10" OD "ring" about 5/8" deep. Put another way, what I will have to grab is a clean, round, machined feature, about 10" OD, with a depth-of-grab of around 5/8".

My question is this. My plan is to EITHER cut soft jaws for my 10" 3-jaw Bison to grab this, OR to use a chuck that came with my lathe but I've never used: a 10" Buck Adjust-Tru 6-jaw. Important: the Buck has fixed jaws, so soft jaws are not an option.

This is an out of balance load for the chuck. The part will also be protruding from the chuck face about 12". So, it'll put some forces on whatever is grabbing it.

Is this a good application for a 6-jaw or would i be better off making steel soft jaws for the Bison 3-jaw? I simply don't really understand the pros/cons of 6-jaw chucks.

This would be ongoing work with some significant volume so whatever is the best way to hold these things, is what I want to do.

Thank you!

Click to expand...

It is 2018, now. For an asymmetical casting not easy to grasp, the entity you would be competing with - if there is any competition yet - probably won't be using a lathe, nor anything manual. He'll be moving the tool around the work, not the reverse.

Otherwise? Got a bit of volume?

Subplate on faceplate. Fixtured. Very! Powered clamping, even.

And in two flavours. One for each end. Batch the ops. "Live" cutterhead at the TP if it cuts the time.

Second choice: 2, 3, or 4 jaw, powered, NOT scroll, top-jaws tooled to suit.

Now you are a factory. Not just a "machine shop".


NB: Hang-out is too great to "make time" with a 4-J, AND the risk of scrapping castings is too high. The two scroll-operated chucks you mention are not even relevant.

Based on tool marks, the shop that has been doing these (for decades) uses a lathe. FWIW.

Are you guys advocating 4-jaw independent for the holding power? I do have a 12" 4-jaw.

Long Tom said:

Are you guys advocating 4-jaw independent for the holding power? I do have a 12" 4-jaw.

Click to expand...

Yes, because they have much greater holding power and variation in size etc can be easily accommodated ..... and still have the part run true on the surfaces to be machined.

On production work, set up and mark two jaws with paint, and either avoid or only use those two for changing parts, .....once you've done a few you'll have it down to seconds.

Long Tom said:

Based on tool marks, the shop that has been doing these (for decades) uses a lathe. FWIW.

Are you guys advocating 4-jaw independent for the holding power? I do have a 12" 4-jaw.

Click to expand...

No, not at all.

Holding power is not an issue with what you have there. # of jaws doesn't matter.

What matters is not marring the shit out of the customers parts and getting both ends concentric. making money on the job would be a swell thing too.

Soft jaws on a 3 jaw will be preferred here.

Ideally, you cut one set of jaws that will do ID and OD in one shot that way you save money and time.

No to the 6 jaw, because the slightest out of roundness in the part, material deflection in the part, or irregularity in clamping position of the 6 hard jaws can result in only 2 jaws holding the part, and then be ready to duck. If you want full circumference holding for max contact or for max holding power, use pie jaws on a 3 jaw. You can make them by welding pieces onto your std. soft jaws if you don't like the bulk of commercial pie jaws.

Long Tom said:

Based on tool marks, the shop that has been doing these (for decades) uses a lathe. FWIW.

Click to expand...

Surely. They may have fixtures. Or plenty of patience.

As "general purpose chuck" work? Probably no longer the fastest and most economical means.

Are you guys advocating 4-jaw independent for the holding power? I do have a 12" 4-jaw.

Click to expand...

At 12" for the 4-J, tall jaws according? It could work. Most especially in steel, CI, or a strong bronze.

If, OTOH, the casting is plastic or light-metal? Grip should be expected to distort the part right about the time it is good enough to hold the off-end stable enough to machine well. You'd want bespoke jaw tops or at least "overshoes".

What doe the PRINT say about the (2) bores & faces ?

Monarchist said:

You thinkin' what I'm NOW thinkin?

Hollow or through hole casting, internal mandrel, fixtured if need be, pick it up and do both ends, same clamping, essentially one op?


D

Click to expand...

Well, ussualy I see rough jaws
(they leave little dimples in the casting outside, maybe what the OP is seeing)
for the first op.

3 jaw, or other self centering holder to "balance" the material
of the rough casting. Custom made soft jaws with tilting pad rough inserts sometimes are used (see Jergens, carr lane catalogs)

First Op, lathe cycle will face, bore & turn the available surfaces, sometimes reaching down deep in to pick up the second bore (the one close to the chuck).

I have even seen some shops go so far as, making up
special tools to reach in and face off the surface against the chuck
(the part being held up off the face on stepped jaws).

All in pursuit of doing the most work possible in the first chucking.

Sometimes the first bore (the one away from the chuck) will be held
to a much tighter tolerance than the final part needs to be (for proper operation).

To be used in the second op as a "In process tolerance".

The second op, might use a precision plug to locate on that
first turned dia. On larger diameters using a short ring,
usually hardened and ground, set into a mild steel faceplate,
called a "Rabbet ring".

Where this system has it's limits, is when the in process plug/ring,
has a slip fit of under .001 (to hold the alignment of the 2 bores
tightly) applying and removing the part's on that plug is difficult.
The tool designer needs to get creative with an expanding, centering
plug/ring.

You haven't said whether a center can be used on the small end. That would take care of your problem.

Tom

digger doug said:

What doe the PRINT say about the (2) bores & faces ?

Click to expand...

I don't have the luxery of a print. I'm reverse-engineering the bleepin' things. It's a long story involving production being shifted to China with some overflow going to a shop in the USA.... and now maybe I'm yanking it all back! It's more complicated than that but that's the gist. It's a lot of business. Worth hustling after for sure. I want an offshore boat, you see.

There's two bearing fits; those will be critical of course. There's several seals that are part of the assembly; doubt the fit there is "bearing fit" critical. Then there's some clearance-grade machining and assembly bevels and mounting holes and so on. Nothing complicated, really, other than the fixturing. Oh, THAT little detail!

Aight guys, get out your whack-a-noob sticks because I've got a dumb question. One bearing pocket is about 6" deep in the sucker. What do you guys use to measure a critical ID way deep in a part?! My ID mics won't reach. I don't trust those little expanding thingies, though I do have a set. All I can come up with is a plug gauge... which sounds dicey... or simply to cut the pocket in a piece of scrap, lock down the dials, and "assume" the Webb will adequately repeat. I have other parts I make with bearing fits where the machine repeats like a champ; but I hate ass-u-ming.

Air gage comes to mind.

As you are reverse engineering, I would make up a drawing, and
the tolerances are gonna be tighter than originally, as
you don't know all the needs.

FWIW (and I'm working blind here) that deep bore might
be best done as the 2nd OP.

Reach down in on the first op, drilling the center junk out, make the bearing bore, and reach in behind it to clean up the face.

Hole the other bore really tight (within .001 tir) for a rabbet ring
on the second op.

2nd op working into that 6" deep bore, no tight work, just hogging
clearance to expose/dig down to the bearing fit you did on the first OP.

Long Tom said:

Aight guys, get out your whack-a-noob sticks because I've got a dumb question. One bearing pocket is about 6" deep in the sucker. What do you guys use to measure a critical ID way deep in a part?! My ID mics won't reach. I don't trust those little expanding thingies, though I do have a set. All I can come up with is a plug gauge... which sounds dicey... or simply to cut the pocket in a piece of scrap, lock down the dials, and "assume" the Webb will adequately repeat. I have other parts I make with bearing fits where the machine repeats like a champ; but I hate ass-u-ming.

Click to expand...

Sunned bore gauge or equivalent, like Federal. Anything less is a toy when doing ±.0002.

There's other stuff like air gauges, I'm not the guy to ask about those.

I think without a photo of the part everyone that has posted so far is guessing.

moonlight machine said:

I think without a photo of the part everyone that has posted so far is guessing.

Click to expand...

Why do I take the time to write up these things for the OP ?

The all knowing and all seeing Moonlight has spoken, and we know
nothing at all.