Datum Shift ? 1

[par1]

I have one dwg which has 3 holes on the plate.
In a dwg, they defined a

datum point A1, A2,A3 as the centre point of the hole.

datum B is defined as centre plane of one of the hole
In a feature controlled frame for datum B

block 1 has 0.5 positional tolerance with 0.5 MMC
block 2 has mentioned datum A

Datum C defined as centre plane of one of the hole & there is attached Featured controlled frame
blcok 1 (In feature control frame) has 0.5 MMC of positional tolerance
In block 2 there is only mentioned datum A
block 3 has datume B with MMC condition

Now my question is

1, There is nothing like datum A defined but only the datum points A1, A2, A3 so how could i define the datum B& datum C using reference from datum A?

2. While defining the datum C ; what does the mean of block 3 in feature controlled frame " datume B with MMC condition" ( I think it is a datum shift - but not sure about the understanding or how to calculate tolerance stack)

could you explain me in detail.

Thank you very much in advance,

 

[ewh]

Datums B and C do not appear to be correctly defined. What exactly is "the center plane" of a hole. How is it oriented? How is it inspected? The part may be acceptably dimensioned if it weren't refering to those center planes. Datums B and C should be the hole features, not some arbitrary planes along their centerlines.
If your part consisted of irregular surfaces (as opposed to a flat plate), then datums B and C need to reflect flat planes. Datum A is correct in as it defines the primary datum plane consisting of three points. Datum B should be the secondary datum consisting of two points, and should be perpendiculat to datum A. Datum C should be the tertiary datum, consisting of one point and mutually perpendicular to datums A and B.
As to your second question, datum C is being defined as having 0.5 MMC relative to datum A (regardless of the material condition of datum A) and datum B (at MMC of datum B). This allows additional tolerance to be added to the positional tolerance of datum C as datum B approaches LMC.
Here is how I would approach it (others may have better suggestions). If your part is a flat plate, and you are only trying to control the hole pattern and aren't concerned with its location relative to the part edges, I would define datum A as one of the surfaces. Make one hole datum B and control its perpendicularity to datum A. Make the second hole datum C, true position relative to datums A and B. The third hole would be true position to datums A, B and C.

 

[ewh]

A couple of additional comments...
Datum A would have no modifiers as it is a plane.
Datums B and C can be defined using the points that established datum A because those points in and of themselves are not datums. Datums B and C are relative to the plane established by those points, not the points themselves.

 

[ctopher]

Having datums A1, A2, A3 is confusing. I have never seen that before. Which one is the primary datum?

Chris
Sr. Mechanical Designer, CAD
SolidWorks 2005 SP0.1

 

[ewh]

Pts A1, A2, and A3 are not datums. They define datum plane A.

 

[ctopher]

thanks for clarifying

Chris
Sr. Mechanical Designer, CAD
SolidWorks 2005 SP0.1

 

[par1]

Thank you very much for your post,

Let me define datum again as I did little bit mistake last time:

Datum points A1, A2 & A3 are the centre point of Hole
But, all the holes are at different level (means at different height)


datum B is attached the hole dia of one of the hole
block 1 has perpendicular toelrance
block 2 has diametric symbol, 0.5 with MMC
block 3 has mentioned datum A

Datum C is attched to the one of the hold dia
block 1 has positional tolerance symbol
blcok 1 (In feature control frame) has 0.5 MMC
block 3 there is only mentioned datum A
block 3 has datume B with MMC condition

1. Now, my question is as you mentioned that datum B is perpendicular to the datum A which is not the case b'coz all datum points A1, A2 & A3 are at different height ?

2. Generally, I didn't see modifier with Primary datum plane - does any reason for that?

3. Also, if you able to understand the datum B & C - could u explain & also let me know if they are appropriate?

4. I understand primary, secondary & tertiary datum plane, but when I see the product its difficult to say anything so if you could give info about how to recognize datum & how to define datums while designing?



Thank you,

 

[type26owner]

That person has used their imagination of how the GD&T works instead of being actually knowledgable and fluent. I see this silly stuff all the time. Found the best approach is ask them to point out the relevant sections of the ASME Y14.5-1994 book that justifies their technique of application, which they can't do. Usually I find if they even have a copy of the ASME book it's sitting on a bookshelf collecting dust but otherwise in pristine condition from never having been opened. Unfortunately applying it poorly is apt to be more confusing then not using the GD&T system at all.
-Keith

 

[ewh]

I have to agree with type26owner that this tolerancing scheme is apt to add confusion.
If datum hole B is to be perpendicular to datum A, and the points defining datum A are at differing heights on your part, then it cannot be normal (perpendicular) to the part surface. This means that your holes are angled relative to the part surface.
Primary datum planes do not require a modifier. Modifiers are limited to features of size, such as your datums B and C. Your datum A is not a feature of size, but a perfect plane through 3 points.
If the intent is to have the holes skewed, then datums B and C are called out properly.
The best approach to defining datums while designing is to use the primary, secondary and tertiary scheme, while considering how the part will be made and inspected. It is also very important to recognize the function of the part itself. If you establish A, B and C using features that are easily made and inspected, you can always add additional datums to control features which are critical to the parts function (such as controlling runout on a drive shaft or the position of mounting holes relative to a pattern center).
I hope this helps you to understand GD&T a little better. The best way to understand it is to use it, either with hands-on machining experience or inspection experience. Design experience is also a good way to learn it, as we don't all have the opportunity to get our hands dirty.

 

[type26owner]

I don't know if you folks are aware of the Appendix E section of the ASME book. There is an extremely handy condensed tool there that's called the 'Decision Diagrams for Geometric Control'. It should help here somewhat. Suggest you peruse Fig E-7 for the essence of Datum Selections.

I've copied those seven pages and have them hung up above my monitor because I got tired of opening up the book.
-Keith

 

[drawoh]

par1,

Let's see if I can interpret this datum scheme properly and work out an inspection fixture.

Datum A is a plane defined by the three datum targets. A1, A2 and A3 are called datum targets. These would be modeled by three pins, slightly bigger than your holes, sticking up out of a base, each with its own elevation apparently. Your part would sit on top of them, oriented to the same orthogonal coordinates as your drawing.

Datum B is the hole. Since it is inclined with respect to datum A, the actual datum point is the intersection of the hole's cylinder with the datum plane. This is actually not an issue, since a vertical pin models it correctly. This locates your part in X and Y.

Datum C is the other hole, which keeps your part from rotating. This would be modeled by a vertical diamond pin.

The only deficiency of your drawing is that the datum targets ought to be specified with a diameter. The actual contact point, the centre of your hole, does not exist, at least, not in the sense of possessing material. Your drafter needs to define the diamter of the A1, A2 and A3 pins.

JHG

 

[ewh]

drawoh,
How can a vertical pins at differing heights be used to inspect datums B and C when those datums are to be perpendicular to datum A? The datum point is not the feature, only a defining point of datum A and the centerpoint of datum B (or C).

 

[drawoh]

ewh,

ASME Y14.5M-1994 explicitly describes non-orthogonal datums. You project the angled features to the points or lines where they intersect the higher level datums.

Orthogonal datums certainly are desirable, but they are not absolutely necessary.

I am guessing that par1's datum surfaces and holes are orthogonal to each other, making the fabriation of a fixture fairly simple. If the datum surfaces are not orthogonal, the fixture is more complicated, but still manageable. Datum_A is a surface located at some weird 3D angle from your orthogonal drawing coordinates, but you do not care, as long as you can locate to it.

This part may be the product of very bad drafting, or it may be a casting. One of the advantages of a casting is that you can produce a very complex form for almost no additional effort, once you have your tooling. Now you have to machine it. You have to inspect the casting, and you have to inspect the final machined part. You want datums that will be present throughout the process. You plan to machine flat the bottom surface of the casting, which otherwise, would be a good datum.

Your datums become whatever features are available to be jigged to. Foundries recommend designing in datum points, but my boss would not let me do this the last time I prepared a casting drawing. The worst case is that your convenient jigging points are not in a plane, which brings us to the point of this discussion.

A complex weldment could get you here too.

JHG

 

[ringman]

My best guess (experienced and educated) is that the drafter intended to use tooling balls to locate the holes which would be used in the establishing of Datum plane A. I believe this would be quite doable in compliance with Y14.5. From there, the datum features B and C should serve to complete the reference frame necessary for the inspection of the specifiied dimensions.

I DO NOT believe pins of any sort would work to establish A as previously suggested. Also there are some misleading statements concerning the establishment of datum reference frame.

 

[ewh]

drawoh,
I understand your scheme for jigging datum A. Datum A though is not a surface of the part, but the combination of datum points. What confuses me is how do you inspect datums B and C, which are defined as perpendicular to datum A, using vertical pins at varying heights? Your jig only locates the center points of those features, but does not allow for the inspection of the features themselves.
I agree with you as to castings. On complex parts, it is common to have orthogonol spotfaces machined into raw castings to establish these datums.

ringman,
Please elaborate on the misleading statements concerning the establishment of datum reference frame.

 

[ringman]

Misleading statement/s for one: 'Primary datum planes do not require modifiers.' (part of ewh post) Datums, whether planes, points or lines are assumed perfect and are not subject to modifiers. It is the Datum FEATURE of size that requires addition of a modifiier.

 

[par1]

Thank you very much for your valuable post, & sorry for late reply,

The part was under the development & i didn't have information but now i could explain little bit batter way as getting some info!

1. The part i am talking is Automotive part under the hood - Injection molded plastic part

2. The A1, A2 & A3 is mounting datum points & the reason for different elevation due to the limited space.

Now,

1. I think i can hear better information about datum planes, & rectify if necessary

2, As Ringman stated that datum which is any plane, point, line doesn't require any modifiers but in my case datum B & datum C which is attched to the hole dia has modifiers in their Feature controlled frame. why?


&

 

[ringman]

Datum features B and C are features of size. Therefore they require modifiers. They are not the same and the A1, A2 and A3. Again, as I understand your problem, A1,A2 and 3 are intended to be points ONLY. Whichever one of them is B, differs in that it is the axis of the circle, which has a size associated with it. Therefore it requires a modifier

 

[ewh]

ringman,
I still do not understand how my statement "primary datum planes do not require modifiers" is misleading, as you seem to concur with your statement "datums, whether planes, points or lines are assumed perfect and are not subject to modifiers." We seem to be saying the same thing. Granted, I was only addressing primary datum planes, but the statement still stands. Perhaps you felt it misleading because I said that they do not require modifiers, as opposed to not being subject to modifiers? This seems a small point to quibble about, but I agree that not only do they not require modifiers, modifiers would be incorrect in that useage.
I do take issue with your statement that datums B and C, because they are features of size, require modifiers. They do not, as it is to be assumed that RFS applies if no modifiers are present. Granted, RFS is a modifier, but it does not need to be noted in the feature control frame.
Please do not feel as if I am being obstinate. I am trying to better understand the correct application of GD&T myself, and may sometimes seem arguementative. I do appreciate and look forward to your comments.

 

[ringman]

EWH,

Perhaps, as you say it is a small point, but Y14.5 contains numerous small points. "Primary Datum planes do not require modifiiers" might better have been worded "Datum planes do not require modifiers". Or Datum features not associated with size do not require modifiers".

I will agree that it is difficult to understand, apply and/or interpret much of the standard. As to B and C they require modifiers. They require consideration as to wshich should apply. I believe that 'assumed" should have read 'defaults to' in your previous statement.

Hope this is of some benefit and not just argumentative.