GD&T Datum Selection

[Jieve]

Hello,

I am new to GD&T and have been reading books, websites, etc. on the topic trying to educate myself. Couple of questions:

1)Say I have a cylindrical flat part, like a spacer on a shaft, and want the ends to butt up against 2 other flat surfaces, say a spur gear on one side and a ball bearing inner race on the other. It seems to me that using the outer cylindrical face as the datum and specifying a perpendicularity tolerance of say 0.1mm, on each face would result in a better “mating” of the adjoining parts than a flatness tolerance of 0.1mm on one flat face and calling it a datum surface, then using a parallelism tolerance of 0.1mm with respect to that datum to the other side. Using the cylindrical face as a datum, each face would ultimately only be off max 0.1mm from horizontal (or vertical if mounted on a horizontal shaft). Using the face as a datum, the opposite face could theoretically be a max 0.2mm off from horizontal, making the “mating” to the neighboring surfaces more poor, although the second surface would be only 0.1mm with respect to the first face. Is this correct?

2)I have a number of very simple parts that I am trying to apply GD&T to and despite knowing what I want, I am not experienced enough to know under what circumstances I should use one specific feature as a datum feature with corresponding controls as opposed to another. One example is what I mentioned above. There are two ways of solving the problem, presumably depending on the application. Another example, if a shaft spacer is going to be interference fit on a shaft, are there “better” controls and datum features to use to keep the ends “flat” than if the spacer were clearance fit to the shaft? Despite reading the datum sections from about 5 different textbooks, I have yet to come across anything more useful than essentially “datum features/surfaces should be selected depending on the importance or function of the features/surfaces.” They are always incredibly vague on under what circumstances specific features/surfaces should be selected as datums. Maybe my question is somewhat vague, but can anyone with some experience give me and others in the same boat some guidelines on what to use when?

Thanks!

 

[drawoh]

Jieve,

The biggest problem I had understanding GD&T was understanding that the datums primarily are a fixturing specification. Ask yourself how the part will be fixtured for fabrication and inspection. Also, ask yourself how the part will be located on the assembly. The fixturing ought to reflect this.

On a short spacer between a gear and a bearing, my primary concern would be the parallelism of the two end faces. On my drawings, one face would be datum[ ]A, and the inside diameter would be datum[ ]B. The second face would be parallel to datum[ ]A.

I would use the inside cylindrical face as datum[ ]A if the spacer was long, and the inside diameter fairly accurate. One end face would be datum[ ]B. I would specify both faces perpendicular to datum[ ]A. Probably, I would specify a ±[ ]dimension between the faces. I could use a profile tolerance on the face opposite datum[ ]B.

How does that sound?

JHG

 

[Jieve]

Hi Drawoh,

Thanks so much for the response. Your description sounds pretty much exactly like 2 examples of what I did on 2 of my drawings, so it's good to have that confirmation.

Another thing I still find slightly confusing is when to use multiple datums on a drawing. For example, in both of the drawings I just finished (both of cylindrical parts), one used the outer cylindrical surface as the primary datum, and the other used one flat face as the primary. In both cases, the controls were only related to that primary datum, so it is the only datum I included in the drawing. Is it always necessary to use enough datums to constrain the part completely, even if the extra datums are not used for controls? For a cylindrical part that is designed for one face to be flat against something, it seems to measure flatness of the opposite face, no other datums are needed. Am I right about this?

When specifying controls with multiple datums, I understand the datum priority in each case to be order in which the parts should be located on inspection. If I have 2 different features that have different datum priorities, would the part then be re-situated according to the datum priority of the second feature control frame to measure the second feature? This may be a simple question, I just want to make sure I understand this fully.

Thanks!

 

[Slowpotato7]

Jieve,

It always helps me to think of GDnT as basic instructions for inspection- something you hinted at in you last post. The point is to make sure that two people inspecting the same part to the same drawing will take measurements the same way.

All of that is to say no, it is not always necessary to fully constrain the part with datums. In the case of your spacer, you only need the one on the bottom. Since you are only concerned in the parallelism of the two opposing faces, does it matter if you, say, rotate the spacer on the primary datum?

The answer to your last question is yes, any good inspector will realign the part to the datum hierarchy called out in the second feature control frame. Just because a datum is labeled "A" does not make it the primary datum. You can label all of the datums as whatever you want and then control which is the primary, secondary and tertiary in the control frame- you don’t even have to use “A”, “B” or “C”. If you are really creative/have lots of spare time you can leave little messages for inspectors, spelling phrases such as "CAN" "IT" "JIM" in the control frames :

 

[Jieve]

SlowPotato7,

Thank you for the very clearly explained answers to my questions.
One more question regarding datums of features of size and of surfaces. I have a simple cylindrical part that has a screwdriver slot cut across the top center, and I would like to specify a symmetry tolerance for the slot. The primary datum is the outer surface of the cylinder. I have read that when placing the datum symbol, if the symbol is on the surface of a cylindrical part and not inline with the dimension, then the datum is the axis. If it is placed inline with the dimension, then the datum is the midplane and corresponds to the feature of size (a description that I find somewhat confusing). In another book, I read that there really is no axis datum, when the datum symbol is placed on the cylindrical surface, it is understood that it is referring to two perpendicular planes that cross at the center axis of the part. In my case, for the symmetry control, since the symmetry is technically about a midplane, is it correct to put the corresponding datum inline with the cylinder dimension, or on the cylindrical surface itself? I’m still not entirely sure what the difference is.

On a related note, I came across some examples of using datums on rectangular parts. For a datum on a flat face, it’s totally clear; when you inspect the part lay it on that face (assuming primary datum). However, there was an example where the dimension of a face was specified, and the datum symbol was placed as an extension to the dimension line. This was to denote that the datum was related to the “size feature” of that side. I don’t understand the relevance of this and how this relates to inspection. Is the part still just measured from that same face where the datum symbol is located? BTW I am working to ISO standards, not ASME, not sure how much of a difference there is between the standards regarding this topic.

Thank you so much again for the informative answers.

 

[Belanger]

You can place the datum feature symbol pretty much anywhere on a cylindrical part and it always means the same thing: the axis is the true datum. The business about having it "placed inline with the dimension, then the datum is the midplane and corresponds to the feature of size" is true for rectangular features of size (unless the datum derived from the cylinder will be used as a tertiary datum).

You can't really use symmetry in this situation. Symmetry must reference a center-plane datum, not an axial datum. Position is probaby what you want.

For a rectangular part (your second paragraph), it is true that there is a difference between having the datum feature symbol be in line with a feature-of-size dimension and having it be offset from the dimension. As you stated, a simple surface datum is simulated by setting the part down on a gage table. But the feature-of-size datum is simulated by sandwiching the part from top and bottom in order to derive a center plane. Thus, there is a difference between having all subsequent measurements originate from the center plane versus the table.

John-Paul Belanger
Certified Sr. GD&T Professional
Geometric Learning Systems

http://www.gdtseminars.com

 

[PaulJackson]

Jieve,

You said,

Despite reading the datum sections from about 5 different textbooks, I have yet to come across anything more useful than essentially "datum features/surfaces should be selected depending on the importance or function of the features/surfaces." They are always incredibly vague on under what circumstances specific features/surfaces should be selected as datums. Maybe my question is somewhat vague, but can anyone with some experience give me and others in the same boat some guidelines on what to use when?[\quote]


The primary emphasis for selecting features used as datum features should be their function, in other words... their role in constraining the three orientation degrees of freedom and the three translation degrees of freedom. There are other influences like measurement stability that may supplant the purely functional when it cannot enable a repeatable conformance assessment but reasons other than that hold little significance over that of the function. Many will say that fixturing and gaging influences in manufacturing should drive the datum feature selection but that is a flawed strategy that often enshrines a given process and fails to link the measured variation to its affect on the function. Generally (not-always) the one that constrains the most orientation degrees-of-freedom in its function will be primary.

In your spacer example... Drawoh captured the functional criteria by offering the two scenarios of choosing whether the ID cylinder has sufficient depth (and I would add fit) to perform the role of primary. The question I believe that will guide you to the functional selection is... Is the depth and fit of the spacer's ID sufficiently deep enough and/or limited by fit to constrain the two rotational degrees-of-freedom that it must if it functionally serves as the primary datum feature over that of the surfaces? At the one extreme where the cylinder's length is infinitesimally shallow compared to the cylinder's diameter the spacer surfaces will always win in constraining the orientations perpendicular to the surface. At the other extreme where the cylinder's diameter is infinitesimally small compared to the cylinder's length... the cylinder will likewise win. In between fits and forces in function should guide you in selecting which features functionally constrain the six available degrees-of-freedom.

While I am an advocate of manufacturing process control monitoring, variation reduction, and process improvement... the product design's functional variation and it's related measurement strategy should be detailed on the drawing over that of the manufacturing strategy. If the two can be the same then all-the-better but I have experienced many operations where they cannot. Sometimes the feature that serves as the functional primary is the last feature finished in the process. Measuring functional variation from it rather than its substitute selected via the process will always be different... how much depends on orientation and location inequities between them.

Paul

 

[CheckerHater]

John-Paul,
On the matter of placing the datum feature symbol:
As Jieve pointed out, he is working to ISO; and even though ISO generally agrees that feature of size (or “size dimension”) produces “derived” datum as median of some sort, it is also more strict when it comes to placing the symbol.
They still insist that you have to align your symbol with the dimension even if there is no other interpretation.
Either way, isn’t it better to promote straightforward way of doing things, rather than obscure technicality?

 

[fsincox]

I disagree with your statement (1) a direct parallelism tolerance will hold it closer, the indirect way (perpendicular to an intermediate diameter) adds the sum of the two tolerances when then looking at the parallelism of the two faces to each other. So I agree with drawoh.
Frank

 

[drawoh]

... Is it always necessary to use enough datums to constrain the part completely, even if the extra datums are not used for controls?

If your spacer is round, with a hole in it, you should call up one diameter as a primary or secondary datum, and then locate the second diameter, somehow. If the spacer is short, you use a positional tolerance to A and B. If the spacer is long and accurate, you can use concentricity or runout.

If my part is round and has no more then one asymmetric feature, I don't worry about clocking.

Your drawings should define your part completely.

JHG

 

[Jieve]

Thanks all again for the informative responses.

Belanger: thanks for the info about the midplanes. interestingly i came across an example in the metal trades handbook (german version of machinerys handbook) that uses a symmetry control for a keyed slot on a shaft. It uses a datum specified with the symbol inline with the diameter dimension-line viewed from the face end of the shaft and says that symmetry in this case is a zone with two planes the tolerance apart symmetric to the shaft centerline (I guess plane in this case?). That's where I got the original idea. You're saying this would be better with a position tolerance?

Drawoh and pauljackson: thanks for the datum info, the more I think about it the more it makes sense.

CheckerHater: you're right about iso's pickiness, iso says that a datum placed inline with the dimension on a circular feature (at least when viewed from the side) means the axis is the datum, and when the symbol is placed on a surface of a circular feature, the datum is the surface line, this again from the metal trades handbook.

Fsincox: you're absolutely correct, i realized this later while i was thinking about it after i posted. I was assuming the diameter would be locating the part but since it is a clearance fitted spacer, the flat end acts as a functional primary datum.

I feel like I'm starting to get a grip on this stuff. So if I have a circular part, regardless of if I specify the inner or outer diameter size-feature as a datum (aka datum axis), the axis location will still be derived using a chuck or mandrel and the specified tolerance related to that datum will be measured from that axis, is that correct? I'm wondering what it actually means to specify the surface line of a circular feature as a datum ( again iso differentiates an axis and surface line on cylindrical features).

Thanks for the awesome discussion!