Help With GD&T Interpretation 1

[fineout]

Hi everyone,
I am just starting in Quality engineering and am just getting started out with really getting into the meaning of GD&T Callouts, I've programmed CMMs but always just used the builtin GD&T functions on PCDMIS and never got really into the meaning of everything, so I'd like to ask for a quick explanation of this callout, I made this general layout since I can't show the real part but my questions are:

1. With datum B, first off it is created by a mid plane of the two side planes on the width, right?
2. Being refrenced to A, I'm unclear what actual meaning that is, basically showing its perpendicularity or something? It doesnt make much sense to me because it doesnt actually have a Z location.
3. Datum C doesnt have a X or a Z location either if it is a mid plane created by the two planes on the top and bottom, so that position callout also seems to be confusing me.

These may be way over my head and I need further training, but if anyone can shed any light on this I would really appreciate it.

 

[KENAT]

1. Yes

2. & 3. One of the folks on here that do training etc may be able to give you the more complete answer but yes the references to the other datums is about perpendicularity.

Posting guidelines faq731-376

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

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

 

[EMorel]

Assuming this is in accordance with Y14.5

Datum A is defined by a surface, the shoulder inside the part shown in the section view.

Datums B and C are intended to be the mid-planes of the rectangle, B being the horizontal mid-plane and C being the vertical. The top feature control frame is stating that there is a position tolerance of "xxx" when the dimension is at Maximum Material Condition (MMC) (when the dimension is at low-limit in this case) in reference to the Datum A surface. That means that the shoulder defined as datum A must be in contact with the gauge (part sitting on the shoulder defined as A) when the position of that width is checked, and it must not be farther out than "xxx" when the part is at MMC, and the tolerance grows as it moves away from MMC.

The second feature control frame states mostly the same thing, and adds the requirement that the Datum B center plane be simulated at MMC as well. So your simulation gauge will have to contact the shoulder defined as datum A and have an extruded piece coming up simulate datum B at MMC. Essentially, your gauge will look like a solid in the shape of the internal section that is empty in the part.

These two position tolerances pretty much ensure that the short sides of the rectangular hole are perpendicular to the long sides, within reason, to allow whatever the mating part is to fit into the hole.

I would suggest getting yourself a GD&T textbook. Sometimes, reading the standard(s) by itself can be confusing and does not give examples to clarify certain things. I learned from (pretty recently actually) "GD&T Application and Interpretation, 5th Ed." By Bruce Wilson, ISBN 978-1-60525-249-0. About $65 on Amazon.

 

[EMorel]

I should also add that I am a young and new designer so my explanation might need to be altered by a more seasoned individual.

 

[Belanger]

This might seem (by some) to be nitpicky -- but the perpendicularity symbol should really be used here, not position. Use verbal words to describe to yourself the relationship of these various items. Notice that the verbal description is always "perpendicular" or "orientation," but never "located..." or "distanced from..." So your inkling expressed in question #2 is correct.

To check the feature control frame on datum feature C, datum B would be simulated not at MMC, but rather at its virtual condition (or MMB).
Finally, we'd have to see where datum C is referenced in a feature control frame, but most likely datum C will not really be the midplane of the short sides of the rectangle (unless it's referenced without B), but rather the midplane of those short sides as we close down with a gage which is exactly 90 degrees from datum B. This last sentence may seem confusing, but it's just that datum C always has to be perpendicular to datum B if they are referenced together, even if the actual sides of the rectangle are not.



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

http://www.gdtseminars.com

 

[fineout]

Belanger,
would the correct method of creating datum C then be to find a midpoint of the two planes and create a perpendicular plane to B with that as it's midpoint?
Thanks so much for all your help, I'm glad to know that I wasnt totally wrong in getting confused by the first callout.

 

[Belanger]

Yes, datum C is created from the midplane of two parallel planes contacting those two sides at their highest points while staying perpendicular to B's midplane.
But again, this is assuming that you're creating datum C for some callout that has datum B mentioned ahead of it. If there's a callout on the print that uses C as the only datum reference, then it would be the midplane of two parallel planes contacting the two short sides wherever they are. (And if datum C isn't referenced anywhere on the drawing, then it really shouldn't be identified here anyway.)

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

http://www.gdtseminars.com

 

[pmarc]

To make it a more complicated, two parallel planes that are going to be used to derive datum C may but do not have to contact two sides of the slot. It all depends on how datum C will be defined in FCF(s) using C as a datum reference. If C is defined at RMB (meaning no modifier after datum letter) these two planes will always be in contact with sides of the slot. However if C is defined at MMB (meaning M modifier after datum letter), the two planes will be at fixed distance from each other but may not contact datum feature C surface at all.

 

[Belanger]

Righto -- good point pmarc! Finout, is C mentioned in any feature control frame on the print?

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

http://www.gdtseminars.com

 

[fineout]

so here is a more complete "drawing", youll have to excuse the sloppiness as this was drawn in MS Paint and not a cad software.

Since it has a modifier, I guess it falls under the not being able to contact the datum feature c surface Im not sure what you are saying by they may not contact the planes at all? If it is made from them, something needs to be refrenced and therefore contacted with the others, doesnt it?

 

[pmarc]

fineout,
It would be good if we had some values especially for datum features B & C sizes and the two positional callouts that you already asked for (the ones that should be switched to Perpendicularity).
I think this would pretty much help in giving you understandable answer.

 

[fineout]

here it is with numbers that are fairly close to the real ones

 

[pmarc]

Saying as short as possible - without going deep into datums, physical/theoretical datum feature simulators, gagemaker tolerances stuff - datums are derived from datum feature simulators (inspection equipment, fixtures, soft or hard gages) and not from actual datum features. In your case, due to presence of (M) modifier following B and C in feature control frames, datum B will be a center plane of simulator consisting of two parallel planes spaced .26 apart (.265-.005) perfectly perpendicular to datum A and datum C will be a center plane of two parallel planes spaced .52 apart (.525-.005) perfectly perpendicular to datums A and B. The two datum feature simulators and in consequence the 2 datum center planes are perpendicular to each other, but the part features do not have to contact the simulators.

Imagine that the height of the slot = .535 and the width = .275 and the width is almost perfectly perpendicular to datum A, whilst the height is almost perfectly perpendicular to both A and B. In such case you will have a certain loose available between actual surfaces of datum features B and C and their simulators, so the part when mounted on the simulators may not contact them at all.

If there was no (M) modifier in FCFs, the simulators B and C would have to expand until maximum possible contact between datum feature simulators and actual datum features was achieved and then the loose (also known as "datum shift") would not be available.

 

[fineout]

Hey guys,
first off i realized that I copied the C datum callout on the other true positions, C is really the .525/.535 width.

We ended up sending the part out to be inspected and my job will now be to try inspect it and try and bring it in house. So now I will need some help, This will probably be measured with a CMM and/or a Smartscope Flash Optical Measurement System. When it comes to the measurement, I am still having trouble grasping how this needs to be measured to be acceptable.

The drawings are to conform with ASME Y14.5M-1994...
-The method I was planning on using for the datum setup would be a plane on the A surface to create that datum
-then lines around the "box" create intersections of them and use the midpoint of bottom intersection as my X,Y origin and then rotate the axis to the midpoint of the top intersections. This will give me a width and the angle of the center line that is datum B
-Take the midpoint of the top and bottom lines and shift my Y origin to this spot

as far as I have been trained, I believe this to be an acceptable setup/alignment, however if there is any major problems with it I would be happy to hear.

Now my dilemna comes to this. If B will be a line, there is no Z offset to have a TP to A.
If C is to be a point there will be no Z offset to have a TP of the .525/.535 width to A and no X to have a TP to B.
This will also be the same when I measure the .590/.600 width, that will end up as a point, so it will really only have an X location, and should only be able to be reported as .010(m)/B/ right?

I feel like this drawing is all sorts of wrong and asking us to measure it is really forcing us to send it out to a company that I'm not really sure are doing it right either.