Machining rings out of high tension aluminum.

Hello all I'm new to the forum and my name is Jon. Im only a few years into the industry and work at a training aerospace shop. We don't have engineers. I turn a lot of heat treated 7075 aluminum and a lot of aluminum nickel bronze. The reason I am here is because no one at work has an answer to my problem. Every time I turn a ring style part with a diameter over 3 inches, it springs inconsistently once you unclamp the workpiece. I'm currently trying to bore out a ring with an OD of 3.750" and an ID of 3.250" and an OAL of .530". The material is 630 Aluminum Nickel Bronze AMS 4640. My clamping pressure is 100lbs. It starts out as a .600" thick slug of 3.760" diameter material. I face it and turn half the OD, flip it and face and turn the other half while only clamping onto .200" of the length of the part. Run-out to the jaws is within .0003". Then I insert drill a 1.750" hole, take it out to remove the slug left by the drill, and re-indicate the part back in. Then boring out the ID from 1.750" to 3.250" I tried to take passes with a .050" Depth of cut per side. Then I tried .025" per side passes. Still after unclamping, the part springs inconsistently from part to part. Some parts will be .001" out of round and some will only be .0003" out of round. Without programing a U taper move the part cones out about .001"-.002" larger on the clamped side of the part. But it doesn't repeat within that difference. I have to leave material on the ID, take the part out and measure it's unique taper, and adjust my U move accordingly from part to part. My boss wants me to get this part running on a production level and I'm stuck. Does anyone have experience making larger diameter rings? Every time I bore rings out of high tensile aluminum they spring inconsistently within a .002" margin. My tolerance is usually + or - .001" but I like to keep it a lot tighter than that. Any ideas or suggestions would be appreciated. Thanks God bless.

Try one piece using a longer piece of stock. Cut your material long enough to be able to get a good grip
in the chuck and leave enough hanging out to machine your part and part it off. No guarantees but there's
a good chance your tolerances will be tighter if you machine the entire part from one position. All you'd
have to do is face off the back side after parting...

I agree with Keith. If you want a consistent/production run then cut it long enough to do all your machining outside of the clamp. When you are thin walled the order of material removal and how much is coming off the ID/OD can change a finished part a lot.
My plan assuming you have the extra stock to cut longer would be :
Face
Rough ID using your indexable drill as a drill/boring bar. Forget about the slug. All chips.
Rough OD
Finish OD
Finish ID
Part

Might get you a better part. You never know how the thin wall is going to act sometimes


Sent from my iPhone using Tapatalk

Rough the ring blanks, finish with bored pie jaws and an arbor to suit. Do them in batches to minimize swapping of arbor and jaws.

Rough the blanks out oversize on both the OD and ID dimension. (I usually like to double the finished wall thickness)
Build a fixture plate that will go into your chuck with clamp holes on the OD / ID
Put clamps on the OD pushing the face of the part straight down against the fixture plate and bore the ID.
Add clamps on the ID pushing the face down and remove OD clamps.
Cut OD.

Try to think of it this way...when the material was formed it was forced into shape and kinda glued there by the surrounding material. Once you remove the material holding it in place the balance of material springs back to the shape its most comfortable.

So, rough, release from machine or part off from solid...let it spring (as if you really have a choice) then go back and finish.



I do one job after where after I rough one side, I bench them (straighten), rough second side, flip and finishing the first side. If I didn't I'd have to go up another material size which adds considerably to the cost.

Some materials really move and you have to account for it or anneal material.

OP 1: Bored pie jaws. OD clamp. Face/drill/bore
OP 2: Turned pie jaws. ID clamp. Turn/ face.

Or.............do what I do on a ton of ring shaped parts I make.............Cut your blank to make 2-3-4(or more) + cut off+ 1/2" or so to clamp. Face/turn/drill/bore all parts. ID grove to ID chamfer. Part each off. Throw away the 1/2" ya clamped on.............might even get away with less than a 1/2".

I just finished 400+ pcs outa 7075. I make a few thousand of these a year. 4.75"ODx3.50"IDx.375" long rings. I get 6 parts/3.35"x5"Ø blank. I do these a little different from above. I clamp 1/2" with hard jaws and make 5 complete parts. Leaves me with around a .75" drop. I then clamp on that by .200" and make one more part. I never drill/bore through the material I'm clamping onto. Since it's still solid, I get hardly any spring/deformation....................

That's how I make these large nuts............they drop off the lathe in one OP(minus the spanner wrench slots).................. 4" material....................long blanks...........face/turn/drill/bore/ID chamfer & thread relief/ID thread/OD groove and part off.......................




..........................

Thank you all for the replies. I agreed machining the part at once while clamping on extra stock is the way to go. Unfortunately the blanks are cut already. We can cut them longer next time or even use rolled stock with most of the bore already gone. But I have to try to save this material. Do you guys think if I trued up all the blanks, bored my pie jaws to .500" deep instead of .200" and clamped on the whole OD of the part it might help control that springing? We don't have a fixture plate to clamp the part to like dstryr suggested. Once the part springs it doesn't change after the second op which just clamps on the ID and faces/ID chamfer.

David N that is a great idea. How do you part off the rings without dinging them when they fall?

Bulletsnatch said:

Thank you all for the replies. I agreed machining the part at once while clamping on extra stock is the way to go. Unfortunately the blanks are cut already. We can cut them longer next time or even use rolled stock with most of the bore already gone. But I have to try to save this material. Do you guys think if I trued up all the blanks, bored my pie jaws to .500" deep instead of .200" and clamped on the whole OD of the part it might help control that springing? We don't have a fixture plate to clamp the part to like dstryr suggested. Once the part springs it doesn't change after the second op which just clamps on the ID and faces/ID chamfer.

Click to expand...

Rolled stock? You mean tube? Don't do that or your problems will only get worse...................

And by pie jaws do you mean full pie jaws or just soft jaws?.................I think pie jaws on the the whole 1/2" would be the ticket......................

Bulletsnatch said:

David N that is a great idea. How do you part off the rings without dinging them when they fall?

Click to expand...

Very very technical and expertly engineered apparatus ...................................





......................................

can't you use an emergency collet make it specific to the job for a good hold and it won't add stresses in. I don't know, don't they have that for CNC?

david n said:

Or.............do what I do on a ton of ring shaped parts I make.............Cut your blank to make 2-3-4(or more) + cut off+ 1/2" or so to clamp. Face/turn/drill/bore all parts. ID grove to ID chamfer. Part each off. Throw away the 1/2" ya clamped on.............might even get away with less than a 1/2".

I just finished 400+ pcs outa 7075. I make a few thousand of these a year. 4.75"ODx3.50"IDx.375" long rings. I get 6 parts/3.35"x5"Ø blank. I do these a little different from above. I clamp 1/2" with hard jaws and make 5 complete parts. Leaves me with around a .75" drop. I then clamp on that by .200" and make one more part. I never drill/bore through the material I'm clamping onto. Since it's still solid, I get hardly any spring/deformation....................

That's how I make these large nuts............they drop off the lathe in one OP(minus the spanner wrench slots).................. 4" material....................long blanks...........face/turn/drill/bore/ID chamfer & thread relief/ID thread/OD groove and part off.......................


..........................

Click to expand...

I wouldn't exactly say those were thin rings that would be tough to hold roundness on tho...
OP is doing .250 wall which isn't that bad. I just finished a 5 axis part that had a .100 wall thickness tube on it that was 4" tall. The key is clamping the material on the face down instead of trying to clamp on the OD / ID

woodchuckNJ said:

can't you use an emergency collet make it specific to the job for a good hold and it won't add stresses in. I don't know, don't they have that for CNC?

Click to expand...

The part is a bit large for a collet.

Here's just one more idea in case you don't already have enough options to try out. Drill a 1/2" hole in the middle of your blank. Chuck up on a piece of stock with a 1/2"-13 hole down the middle. Bolt the blank to that. Then, turn the OD, face the front, back-face the back, and trepan (face groove) the bore. Do your trepanning such that it almost breaks through to the back face. Then, you can just punch the slug through once you get it out of the machine. You would just need one more operation to do the back chamfer. The bores will be perfectly concentric, and as long as the material doesn't have any internal stress, the part will be round. If it's still springing on you, you could try rough trepanning the part before doing the turning and facing to allow it to relax while still attached to the slug. Then just clean up the bore one more time before taking it out of the machine.

Wmpy that's a great idea. David N I'm using aluminum pie jaws. What we ended up doing for this time is leaving .025" on the ID and we're gonna finish bore on a machine with lighter clamping pressure while clamping on the full .500" OAL next time we make this were going cut the blanks .250" longer and part the ring off like most of you guys suggested. And yeah tube stock. Not too sure what it's called. I've only used it once. Some one here suggested that most of the tension is already relieved.

For parts like this I have cut blanks long enough for 2 parts, plus enough for facing and parting off between them. I then hold one half of the blank in soft jaws, finish the ID, OD, and face of the side hanging out, but put an M30 before the part off and skip it. Then after running one side of all the blanks like that, bore your OP2 jaws and hold the finished half of the blank in them, delete the M30 before the part off, and run OP1 on the half of the blank you initially were clamping on. You will have to do something like the photo above, catch them in a non-OSHA approved way, or hand them off to a sub chuck, but then you will have two parts fully done with OP1, and your jaws for OP2 are already in the machine and good to go after re-setting the work shift.

Hope that makes sense the way I explained it. It has worked great for parts that must be blanked out but are a challenge to hold for the first op without excessive material waste.

Redd

mhajicek said:

The part is a bit large for a collet.

Click to expand...

I don't know, I have an emergency collet that's about 4 1/2 inches across. And its for a 3C not even a 5c..

wish I knew why my images never attach.

[url]https://i.imgur.com/rEcKjMm.jpg[/URL]

This is a link to my imgur , I can't get the image uploaded...
This emergency collet is uncut, it's the business end, the stub is removed when you cut your