Effect of Datum accuracy on the controlled feature 3

[sluzzer]

Can the controlled feature be more accurate than the datum?
For example, if the positional tolerance is called with reference to a flat datum with the flatness control (say, 50 microns), then can the positional tolerance be less the the flatness value of the datum (that is less than 50 microns)?

 

[3DDave]

It depends a lot on the geometry, too much to make a universal rule.

 

[Belanger]

In general, the answer to your question is yes.

But to be a wise guy... technically the controlled feature can't be more accurate that the "datum." (That's because a datum is by definition a theoretically perfect plane/axis/point. Your position tolerance can be more accurate than the "datum feature," though.)

 

[axym]

Sluzzer,

I agree that the answer is yes. The tolerances on the controlled feature can be smaller than the tolerances on the datum feature(s). I am not advocating this approach, but it doesn't violate any rules or concepts. For example, a parallelism tolerance of 50 microns could reference a datum feature with a flatness tolerance of 1 mm. This would be a risky practice, but it isn't fundamentally incorrect as per Y14.5 rules.

Evan Janeshewski

Axymetrix Quality Engineering Inc.

http://www.axymetrix.ca

 

[drawoh]

sluzzer,

A crude rule of thumb is that your fabrication and inspection fixtures should be ten times as accurate as the controlled feature. This is not a rule in any of the standards to the best of my knowledge. This applies to feature of size (FOS)[ ]datums.

This is a practical problem. For example, let's use bolt holes as secondary and tertiary datum features, and let's locate some dowels accurately. The holes are [⌀]6.5[±]0.4mm in size. Our positional tolerance on the pins is [⌀]0.1mm. My fixtures for these are a pair of carefully made expanding collets, which will account for the sloppy diameters. This is dumb.

IF your FOS datums are called up at MMC, a fixture with a couple of dowels will work, but the resulting parts may not comply with your design requirements. It is way better to use the accurate dowel holes as datum features.

If your datum feature is a surface far enough out of flat to compromise your positional tolerances, consider specifying datum targets.

--
JHG

 

[sluzzer]

Thanks for the answers!
Let's consider a practical scenario.
1. A dowel is required with 10 microns positional tolerance with respect to datum A (Flat datum) and datum B (Cylindrical datum).

2. Now do we need to control the flatness of datum A and cylindricity of datum B within 1 micron?

3. Can we give flatness of datum A and cylindricity of datum B as 50 microns and still call for positional tolerance of 10 micron with respect to datum A and datum B?

We received a drawing as per point no. 3 for manufacturing. Now my process planner asked this question "when datum itself 50 microns, how can we achieve 10 microns positional tolerance? Please grid the datums to 1 microns"

Now is it drawing mistake? Whether the question of my process planner is correct?

 

[3DDave]

Is it possible to make a part that meets the requirements? Yes.

Do large variations in the datum features make that more difficult? Maybe.

Do large variations mean the inspector might have to do some work to fit the feature to the tolerance zone? That's the thing that's being complained about.

They can't just slap the part onto the CMM, click their heels three times, and be done. They might have to shim the part, maintaining contact with the datum feature simulator per the ASME Y14.5.1 requirements and they don't want to do that.

Now, if datum feature A is a 1000 mm diameter flat and the thickness of the part is 0.0001 mm, how much rocking of the part will there be that they are worried might happen?

Knowing only the zone and not the actual sizes of the part means not being able to calculate for you the amount of rocking that might occur.

It also means that if datum feature A is 0.01 mm diameter flat and the part is 20 meters long, then rocking might be a huge problem. But no information means no applicable answer.

Which is why all the dimensions are important and not just the allowable tolerances which, by themselves, are nearly meaningless in making a decision.

 

[drawoh]

sluzzer,

Dowel pins make excellent Feature Of Size (FOS) datums. The smart thing to do is call up the dowel pins as datum features, and position everything else with respect to them. The next drafting strategy would be to call up datum targets.

It sounds like these are not your drawings. You have two choices. You can work out a fixturing and fabrication process to achieve your customer's tolerances, and then quote the price. Your other option is to call your customer and explain them your interpretation of their drawing. It sounds like people can be flexible, and the cost of functional parts can be drastically reduced.

Do you have the relevant ASME[ ]Y14.5 standard in house? You want to read carefully the section on datum features.

--
JHG

 

[mfgenggear]

sluzzer
to the rules per ASME yes
in real life no, I would machine the the flatness in order to maintain the positional tolerance. (for tooling purposes)
What a process engineer does in the first operation it will effect the following post operations.
it is not un common to tighten the tolerance to maintain the the following operations.
and to add makes their life easier. It's experience

 

[sluzzer]

Thank you everyone!
@drawoh yes this is not my drawing. I am a CNC shop manager. Yes do we have asme standards. Ok thank you.

I could understand better from all the answers. Had I uploaded the drawing, it would have been better. But I couldn't do it because of the company policy.

For further better understanding, I like to explain the part.
It is a jet engine casing. The geometry is a hollow cylinder with flanges at both the ends. There is a spighot (thin cylindrical projection at the inner ID of the flange) on both faces. The flange has a dowel hole and a pattern of bolt holes.
Next assembly parts on both side of this casing is similar. The casing axis is located by the spighot and its orientation is fixed by the dowel and then comes the bolt holes.

Now, the flange face is the datum A with 50 microns tolerance and datum B is spighot axis with 50 microns. Now with these datums, the dowel hole is located with 10 microns tolerance.

Now with these extra details whether all our previously discussed answers remains same?
Thanks a lot.

 

[3DDave]

No chance of sketching the schematic of this part? I see lots of pictures from Google of jet engine parts, so it's not a secret.

But it sound much like the first example I gave. If the casing is one meter in diameter and the flange is 3 mm thick, then the ratio is 50 microns/1000mm vs 10 microns/3 mm.

Which is the tighter requirement?

Hint: 0.05 microns per mm is tighter than 3 microns per mm.

It's up to you to use the values on the drawing you alone have access to.