Tolerance Validation

In my experience -- and I think this is true for most companies -- the drawing furnished by the buyer should have all of the requirements for the part, without telling the supplier how to make the part. If a manufacturer can meet the drawing's requirements using a lathe, drill press, Dremel tool or even a hammer and anvil, it shouldn't matter. If a part meets the drawing, and ALL of the requirements are on the drawing, then both supplier and buyer should be happy.

Your component - the hub is shrunk on a shaft

First question- your tolerance of ±0.0015 is OK? As per our experience and also the normal procedures, the hole should have unidirectional tolerance ie may be it should be 15.4135 + 0.003" It falls in between the grades H7 and H8 for the diameter (almost exactly in the center)

As you are aware that we specify the tolerancing for fits based on grades eg H7p6, H7n6 etc.

The lathes have a perfect capability to hold a tolerance of this (H7+) and we regularly achieve it in our lathes- but the question arises is the condition of the machine- guideways, lead screw backlash et all.

Only where the tolerance is grade 6 or fimer or there are special requirements for finish (<1.6 micron, sorry for talking in metric) we go for these processes (grinding for us, honing we don't own the capability)

The whole problem about the process cabability study is that it is for a process. To calculate the process cabability you should go for at least a large batch production if not continuous. Considering the size of the component, it looks unlikely that your supplier would be doing it. In on off line these become too complicated. I have done a study on this a few years back- though statistically questionable, where I tried for relating the machine capability with the diameter. Surprisingly a pattern is followed. But then the process was a relatively stable- CNC Center lathe, Same set of operators, Turbine rotors of a bit different size but more or less same profile.

In your case, unless sufficient ressearch is done at vendor works, the Cpk may be only of academic interest not of a practical significance. Since in this type of cases, the operator (at least in our plant) takes a cut, emasures, does the tool offset correction and passes the finishing cut (keeping fingers crossed) though for this wide tolerance we don't even cross that. Just for an example, in batch productions on vertical lathes we machine hubs of diameter approx 15" (that is nearest to your size) with a tolerance of +0.0015"/-0.00 and no deviations (and that is too shrink fit with p6 shaft).

Your approach is technically correct for a process ruled by random variations which all statistical processes calculations demand. Check if the conditions satisfy, but off the hand, this wide tolerances are perfectly achievable by a lathe.

Great information, thanks for the comment back on this topic. I am beginning to think that the issue is more about the part than the process. The part is a casting with multiple features around the outside of the part (flange, mounting boss, cored holes, etc....). I believe that residual stress may be the problem. I'm having the machine shop try to measure the part while it is in the constrained condition and then again after being removed from the lathe to see how much it may be changing due to the relief of the internal stresses of the part.

I believe the picture is becoming clearer with your comments and additional information from the vendor showing that there is also a roundness issue with the part. The vendor supplied roundness measurements the other day that the parts are out of round as much as .137mm (.0054"). I believe this points to part distortion if you say that the lathe op should be able to hold this tight of a tolerance. I think it is at least worth investigating.

Thanks for your help.

In case it is a thin casing -

Our procedure is two folds

a) Stress relieve with approximately 3mm tool point allowance (pl convert it into inches)

b) If it is too thin - stress relieve with a bit more allowance or in our case we do not do a thermal relief - we allow it to rest for approx 2-3 days before taking the finishing cut

c) Ensure clamping stresses during machining - we usually use different fixtures and supports for ensuring that the stresses are as far as possible not allowed to distort- eg in quiite large thin casings after the rest period - these are mounted on vertical supports - machined just prior to mounting on chuck, vertically clamped with u clamps. The vices are used to center and then pressure released , veritcal clamped, check the radial run-out. Ensure the axial face-run-out (shouldn't get disturbed between the free condition and the tight condition.

Usually it takes 4 to 5 settings to finish - 2 settings side-1, side-2 in roughing.

side-1 finishing face- (this face would be now almost perfect)

Side-2 finishing face and bores

Side-1 finishing face and bore.

Though it is a bit complicated and time consuming but considering the complicated component it is worth. It is very thin section and very large casting to gas turbines.

For you most likely thismuch won't be necessary- the basic concept is after roughing ensure that the clamping doesn't distort- that is ensured by the run-outs before and after clamping. But as mentioned- note that the clamp do not stress the component unless the zone is rigid enough to take the stress. Ensure supports so that the clamping load is transfererd to the chuck without stressing the component. use clamp for clamping purpose only. We have seen the U clamp between two parallel plates also distoring the flange so we put the clamp exactly where the plate is, over the plate so thet the friction - clamp to job to plate -holds the item. The jaws only supports against accident.

Check the run-outs both axial and radial in clamps just hand tight and full tight conditions, no significant variations should occur between the two- it would signify the clamps distorting the job piece.

In case the quantity is sufficiently large, special clamping fixtures need be designed.

Do you ever find the need to use a torque wrench to set the clamp pressure? I wonder if variation in the clamp pressure due to just wrenching down the clamps leads to variation from one part to the next?

Would .500" wall be considered thin?

How much material are you leaving for the final cut?

Torque wrench may be advisable, but we normally (or our machinists rather) do it by the feeling of the hand.

0.5" is 12.5mm is really thin. I have problems in the bushings of this thickness of diameter as low as 300mm (12") , but it is a long bushing. of approximately 20".

This one we do by clamping the flange and 4 setting machining with approximately 3mm material left on tool point for final. More than this may result in distortions due to machining stress. how much you should leave have t be found by trial and error. Say you leave this much or a bit more in first piece and then find the distortion due to relieving (ie before the final machining) then minimise it depending upon the minimum machining allowance that you need and also the sistortion. As per our experience if properly dione this (2 to 3mm on tool point) is almost optimum and we take care during roughing to control distortion to the maximum.

leave the job aside after roughing for at elast 1 day (we go for batch so it is left for at least 3-4 days)