Concentricity machining Allowances 1

[deangardner]

Hi all,

I'm about to start the manufacture of a large ceramic disc (263mm in diameter) which will currently be turned on a lathe. The disc has an inner bore as well a bit like a large scale polo mint. The bore diameter is around 95mm.

Can anybody tell me what they think the best geometrical concentricity that i can achieve will be using a conventional lathe or do you think it would be possible put this on a grinder and machine it to a higher degree of accuracy.

I'm currently specifying a diametric tolerance of 0.05mm from the axis of the inner diameter to the axis of the outer diameter - A maximum permissible deviation of 0.05mm.

Any help would be greatly appreciated. Unfortunately the trusty old machinists' handbook can't help me on this occasion...

 

[desertfox]

Hi deangardener

From memory if you grip in a three jaw chuck your accuracy
on concentricity particulary if you have to remove or turn round your component in the lathe will be about 0.003".
If you use bored soft jaws you can probbably be within 0.001".
However the tolerance you should use is that which gives you the maximum allowable without affecting the function of the component

desertfox

 

[drawoh]

deangardner,

Can you cut the bore and the outside diameter on the same setup? Perhaps you can chuck the part using a pitch circle.

If concentricity really mattered to me, I would not cut one diameter then rechuck the part to make the other diameter. This is a design issue.

JHG

 

[BobM3]

Length of the part is another consideration. If the part is not square in the chuck then the far end will be more non-concentric. So, how long is the part and are you also turning the OD of the part?

 

[ushang70]

Are you going to machine face also? if it is, then in any condition you have to machined in two step,machine inner,outer diameter with face all three operation at same time, and another face in next step.
however objetives are also there, like accuracy of machine, type of tooling etc.


ushang

 

[MartinSr00]

I think it depends on how tight the lathe is. If you've got .05mm (.002"), that seems in order.

Make sure you put the necessary form controls on your hole.

.05 mm is agressive if you want to do it in multiple setups, because parts can be very hard to re-center. A check with a dial indicator checks both hole form (variation in the diameter) and position (where the center is). So, in theory, you could perfectly center align two holes that are each .05 mm out of round. But in practice, finding those centers with a dial indicator could be a bit of a challenge.

Eliminate the problem by one setup if you can. If the part doesn't move, then any mis-centering would be related to deflection during machining and accuracy of the lathe's bearings.

 

[vc66]

What kind of ceramic?

V

 

[KENAT]

Maybe a silly question but look at it the other way.

Functionally, what do you require?

I'd spec the loosest I can tolerate. Then if the manufacturing method I'm looking at can't meet that, I'd think again.

Posting guidelines faq731-376

http://eng-tips.com/market.cfm?

(probably not aimed specifically at you)
What is Engineering anyway: faq1088-1484​