datum reference frame and profile

[DoogieP]

Greetings All,
I hope someone can clarify an ongoing debate on interpretaion of a print.The attached print is a basic representation of an actual part and shows the features in question. As I see the part the datum reference frame is established by A, P3 and P4 since hole P1 has no positional tolerance and notes on the drawings indicate as such. The debate is on the .019 profile of a surface to datum C and how it is referenced to the .002 profile callout and the 5.250 +/-.005. Our Process engineer who also controls our OGP SmartScope says that you cannot have a profile of .019 on datum c because it violates the +/-.005 tolerance. I don't see it this way, the print specifies "dimensioning and tolerancing IAW asme y14.5m-1994. I said it is possible because the 5.250 will move with any deviation of this surface and the 5.250 is a secondary control of form. Our second debate is, he is establishing datum C from the part itself but, I see datum C as being "implied" and should be established using basic dimensions to create theoretical plane because it is there to establish location of the tolerance zone. pleas chime in, any and all feedback is greatly appreciated.

Thanks In Advance,
Doug

 

[Belanger]

Before getting to the debate about profile, we have to sort through the mess of the datums. None of the datum callouts are IAW ASME Y14.5M-1994.
If using datum targets (i.e., A1 through A4) they can't be referenced as individual targets in a feature control frame; the datum reference must be just A. And if referencing these targets, there's no possibility of using the "M" modifier after the datum letter.

Perhaps this was redrawn from the original to present this question. But maybe verify for us if this is really how the datums are called out?

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

http://www.gdtseminars.com

 

[DoogieP]

Hi John-Paul,
Thank You for the responce. Yes, this an accurate (even though basic) representation of the drawing and this is how all these features are called out. I am unable to publish the actual drawing. The only exception is on the drawing P3 is labeled as P1P2 and P4 is labled as P1_P2. P1 and P2 are dowel pins and I think they labeled them solely to generate datums P3(P1P2) and P4(P1_P2). All basic dimension are from P1 which is the intersection of P3 and P4 and there is no positional tolerance applied to this location. Can you explain why P1 though P4 cannot be referenced as individual targets in a control frame? How can you only reference one datum in a feature control frame if you are tolerancing something like true position or profile of a surface? How come you can't have an "M" modifier when referancing P1? It's a dowel pin and has a MMC (FYI, they had an MMC callout to P3 on the .019 profile too). I ask these question for my own personal knowledge and would not like to have this spin off in another direction. For argument sake lets say A,P3 and P4 are the frame of reference and go from there, since I cannot ask the individual who made the drawing 10 years ago, why.

Thanks,
Doug

 

[Belanger]

Think of it this way: A datum doesn't exist on a part. A datum is defined as a theoretically perfect plane, axis, or point from which measurements will be made. So the datum feature symbol (the triangle thing) that we display on a print doesn't really point to a datum, but from the physical aspects of a part that a theoretical datum is derived from.

This is why we can't put P1, etc. into the last portion of a feature control frame -- because the feature control frame is referencing a datum, not a datum feature. There is no such thing as "datum P2." But rather, "datum target P2" is supposed to be part of a group of datum targets that will together create a perfect plane, axis, etc.

That may sound like semantics, but it's a key concept of GD&T and I think the designer lost sight of this concept. And that, along with numerous other deviations from the Y14.5 standard, is what makes the drawing so confusing.

At any rate, here's how I extract the intended meaning of the GD&T: The four corner pads establish a primary datum plane. The pin CLs are meant to lock down the other directions of space. Once that's all locked into place, the top edge of the part is to be checked for profile of a surface to within .019. This edge then creates a datum C, which helps to tolerance the outline of the inner pocket (unilaterally outboard). Finally, the pin labeled as P2 is to be checked for position within .019 at MMC, and this is measured relative to the established plane A and while locking down the other pin (called P1 right now).
BTW, if that's the intent for P1, then it is permissible to have the "M" modifier after the datum in the feature control frame, but it can't be referenced as P1, as mentioned in the paragraph above.

I know you say this is from 10 years ago, but this really should all be cleaned up. Is my description of the design intent correct?

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

http://www.gdtseminars.com

 

[DoogieP]

So if I'm reading this correctly, datum C is actually derived from the part itself? (Then it's not theoretically perfect or am I misreading what you wrote) If it is the part, being the tertiary datum how do you establish one point of contact? Otherwise, wouldn't the .002 profile move with datum C? That seems to be the biggest area of confusion, is datum C theoretical or is it the part itself. Yes, the drawing is an absolute mess and I don't think datum C should even be referenced with regards to this pocket, I think the profile of the pocket should be referenced to A, P3 and P4 . The function of the pocket is to accept a cover which is then welded or brazed in place and they want a predicable gap between these two components. I have asked why we haven't gone to the customer for clarification and the responce I get is that the customer didn't design the part and they don't want to change it but, there name is on all the drawings, they state they are the owners of the design in a disclaimer and they sent us all ECN's showing the rev history.

Thank you for sharing your knowledge,

Doug

 

[Belanger]

Datum C is a theoretically perfect plane formed by contacting the highest point, after the primary plane A is established and after the axis of P3 is locked in. (Datum C's only job is to stop rotation.)

So I think I see the main question now: If "datum feature C" has a profile tolerance of .019, does that number get carried through to the other tolerance of .002 position.

Answer: No. The profile tolerance of .002 on the pocket is looking to the perfect plane C. So any bumps along the top are not noticed when measuring the profile of the pocket.

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

http://www.gdtseminars.com

 

[DoogieP]

Ahha! I see what your saying, so datum C's alignment is still perfect relative to A and P3 at 30 degrees from P3, the only thing that changes is its relation to the .3750 basic dimension which would be the highest measurement(point) from this basic dimension. The way I originaly interpreted datum C was, a theoretically perfect plane that was generated from the basic dimension, regardless of the actual part surface. This is only part true because datum C can still move with respect to basic dimension ".3750". One of the issues we are having is QC is saying our profile is out in certain areas using an OGP smartscope using a vision system along with touch probe and we are trying to validate this using a Tesa Micro-Hite and they are saying we can't do that. From what you are saying is, we can. We first need to establish datum A, in this case would be making sure this surface is square to our surface plate. Then we need to align and establish datum P3, if we do this with datum C in contact with the surface plate we have established datum C and can then measure profile dimensions which come from P1. Unfortunately they see the OGP as some infallible god that doesn't make errors but, the old adage "garbage in garbage out". I think they are aligning datum as an average of contact points which is scewing the plane but, they won't tell me exactly what they are doing.

Doug

 

[pmarc]

DoogieP,
You seem to be focusing on how to establish datum plane C from top surface, but the thing is this datum feature reference to C in profile callout for pocket is not needed. I am veeeeery far from saying that this drawing has been done in accordance with any GD&T standard, but I think it gives enough idea to say that it is not the top surface that stops rotation of the part. Looking at what P3 is, it seems that the intent is to stop the rotation using the hole currently marked as P2 or P1 and P2 simultaneously. If that is true, you do not need to reference to C, because the part is already fully constrained by A and P3 (datum plane established from centers of P1 and P2).

 

[DoogieP]

Hi pmarc,
I don't see how datum C is relavent to the .002 profile either and I'm hoping to gather enough info so I can go to my boss and say we need to sit down with the customer and discuss these issues because there are too many things that are "open to interpretation" on this part and has done nothing but caused fruitless debate and lots of money. I hoping to get feedback as to how this part should be dimensioned and post a marked up drawing for a consensus and go to the customer from there. Any and all (constructive) comments are welcome, it's all about continuous improvement and moving forward. Thanks pmarc for the input, if you have anything else to add please do. There are a few other issues with this part I would like to clarify but, this seems to be the biggest bone of contension right now. Any one have any thoughts on the .019 profile not being possible because it would viotlate the 5.250 +/-.005 dimension? please refer back to my original thread.

Thanks,
Duog

 

[Belanger]

Good stuff -- yes, I missed the fact (using that term loosely, given the shakiness of this print!) that P3 was meant to include both corner holes. Then the rotation is indeed stopped already.

I think you've got plenty of ammo to go to your boss and suggest that this thing needs to be redrawn.

As for the .019 stepping on the toes of the 5.250, that's a negative because the profile tolerance only applies to the top surface. If they had meant for the profile to wrap around all four sides of the part, then they would have indicated that by the note or symbol for "all around." In that case, then the 5.250 would have to be a basic dimension to avoid taking on a ± tolerance, otherwise the ± would contradict the profile tolerance.

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

http://www.gdtseminars.com

 

[pmarc]

Any one have any thoughts on the .019 profile not being possible because it would viotlate the 5.250 +/-.005 dimension? please refer back to my original thread.

Profile tolerance applied to top surface controls not only its orientation and location to other datums, but also its form. That means the allowable flatness or straightness error of the surface can be .019 maximum. This is in conflict with Rule # 1 saying that for 5.250 height any form error of top (or bottom) surface of the part cannot be greater than .010 (twice .005).

 

[Belanger]

Pmarc, I don't think it's necessarily true that there's an automatic conflict between the .019 and any general tolerance of .005 on the 5.250. The profile controls form, location, and orientation of that top surface, and the 5.250 is a dimension controlling local size and envelope size of top-to-bottom.
Suppose the entire outside rectangle shape is simply shifted up by .008. It would still be within the profile tolerance zone, as measured from the intended datums, and the height dimension would still be satisfied. You just might have portions of the profile or the ± .005 that are unusable.
Just thinking out loud...

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

http://www.gdtseminars.com

 

[pmarc]

I am also thinking out loud...
What if as-produced top surface occupies whole .019 wide profile tolerance zone, in a way that the contour looks like flattened V in main view (that is, in top-left and in top-right corner the surface touches outer profile boundary and in the center it touches inner profile boundary). Surface meets its profile requirement, but is there a possibility that all local two-point measurements and Rule #1 for dimension 5.250 will be met in such case?

 

[DoogieP]

My last thread didn't seem to post.any who...
I think John-Paul and I are thinking the same (i could be wrong). Wouldn't rule #1 take priority then, as long as that deviated form lie within the .019 profile it would be good? (just trying to learn something )

 

[pmarc]

I have thought about it more.
You are right, there is no conflict between profile .019 callout and size tolerance for dimension 5.250. Rule #1 is there to make sure that the situation with flattened V as I described can't happen.

 

[DoogieP]

I've made some changes to my original drawing, any feedback is greatly appreciated

 

[DoogieP]

Could someone chime in on my post where jmarc joined in? Not with respect to the messed up drawing but, to validate methodology for setting the part up to inspect with a Micro-Hite. The engineer that is in charge of the OGP claims I cannot inspect this part (with the Micro-Hite) because I cannot establish my datums to which I replied "We can. We have been making this part for several years before we got the OGP and never had issues". He couldn't explain why I cannot establish my datums, he just insisted I cannot do it.

 

[pmarc]

Doug,
Perhaps I should not be doing this (you should get to it on your own with our assistance only), but since I created a confusion with the dependency between profile callout and size tolerance for dim. 5.250, I feel obliged to give something in return, especially that your recent changes to the original drawing did not really make things better.

In the attachment you can find a drawing that shows one of possible ways of dimensioning the part.

http://files.engineering.com/getfil...-82cb-ec7f3931d8d9&file=plate_with_pocket.pdf

I made some assumptions that may not necessarily be functionally justified (like for example both profile callouts applied all around, or datum features B and C called out at MMB, or profile tolerance zone for the pocket being unilateral), but I think this may help you in a discussion with your boss. I do not know how far you can go with print modification, but if you just compare it with my version, you will easily notice that quite a lot must be reconsidered.

 

[DoogieP]

pmarc,
thanks for the drawing let me digest it and get back to you. FYI, the .002 does apply all around (my bad) but, they have it as out bound to the profile so they can insert a cover piece to weld or braze in. The outside profile is a mess too! You have datum c from my drawing as .019 profile, then the 5.250 +/- .005, there are intersecting arc segments at the corners of the outside profile with a profile of .009 and the ends (you have dimensioned as 8.500 basic) that have an inbound profile of .019 from each end. I'd like to work through this in stages, starting with establishing datums. I'm not sure how far I can go with this since I do not know fully what the design intent is, and will probably never know because of security reasons. If nothing else, I can get the customer to clairify several areas of confusion.

Thanks for the help!
Doug

 

[DoogieP]

Hi pmarc,
I had a chance to look at your drawing, datums P3 and P4 seem to be redundant on my drawing and datum C isn't even needed. I think I will do a redraw with a little more detail

Doug