Angle Basic Dimension

[J.Powell]

This is my rendition of a print I received. The problem is that the customer is not happy because the bottom 90 deg angle is at 90.02. I'm no pro at GD&T, but something don't seem right. It's a basic dimension so I would think that the inspection report would not include it. Should they have omitted it and only recorded the true position? Can someone help me?

[Kelly_Bramble]

This is my rendition of a print I received. The problem is that the customer is not happy because the bottom 90 deg angle is at 90.02. I'm no pro at GD&T, but something don't seem right. It's a basic dimension so I would think that the inspection report would not include it. Should they have omitted it and only recorded the true position? Can someone help me?

Yes, the specification requires that the derived axis from the as-built hole fall within the cylindrical tolerance boundary.. Reporting the angle is interesting however not required.

[J.Powell]

If my true position was measured at .028mm out of tolerance and I know that my 17mm dimension was 17.05mm could I remove .05mm and improve on the true position?

[JFleck]

I'm not fond of the GD&T in this drawing. As shown, it relates to datum A only; this means that there is no actual reference to the top surface (as shown in the right hand view). The basic dimension if [17] effectively has no tolerance on it because it doesn't relate to a control frame. The drawing should at least call out this top surface as datum [B] and then refer to it as a secondary datum reference in existing FCF's. The datum [A] hole is not currently positioned relative to anything either but I expect the customer also wants it to be positioned relative to that top surface.

Instead, I would suggest the customer should mark the top surface as datum [A] (this ensures the desired distance) and the Ø260 as datum [B] (this ensures the holes are perpendicular to the tangent of the profile). Then all three holes may use the same FCF callout.


That said, it's of course all about what the customer wants (there's been a couple threads like this lately) regardless of what there current document technically states. They will likely appreciate your effort to clarify the intent.

Lets assume for the sake of discussion that the customer wants the position of all the holes to be as I suggested (which sounds similar to your interpretation). Since you know the distance is currently at 17.05mm, then the angle would need to be exactly perfect - which it is not (however small the difference is). This must be why the customer is not happy.

If my true position was measured at .028mm out of tolerance and I know that my 17mm dimension was 17.05mm could I remove .05mm and improve on the true position?

To answer your question, we would have to know the location of the other holes... If they are also 17.05, then your solution is perfect. But if they are 16.95 from the top surface, then you will mess up their locations while fixing the other. If that was the case, then your hole pattern is titled relative to the top surface and you would have to machine on an angle.

Last: I'm not sure how you are measuring your true position value... based on your other measurements I find that your position is currently about 0.135mm.
Since I forgot to write it on the image, the grey circle is the position tolerance zone of Ø0.1mm

[J.Powell]

I think if it had been dimensioned as JFleck suggested I would not have such a hard time understanding what was needed. I can go from here and get all three holes' measurements and maybe I can remove some material from the face of the parts. Thanks for the help. It is truly appreciated.

[Kelly_Bramble]

If my true position was measured at .028mm out of tolerance and I know that my 17mm dimension was 17.05mm could I remove .05mm and improve on the true position?

?.... Maybe, however there is not a modifier (MMC) or a size shown on the engineering drawing to make that assessment..

[Kelly_Bramble]

I'm not fond of the GD&T in this drawing. As shown, it relates to datum A only; this means that there is no actual reference to the top surface (as shown in the right hand view). The basic dimension if [17] effectively has no tolerance on it because it doesn't relate to a control frame. The drawing should at least call out this top surface as datum [B] and then refer to it as a secondary datum reference in existing FCF's. The datum [A] hole is not currently positioned relative to anything either but I expect the customer also wants it to be positioned relative to that top surface. forgot to write it on the image, the grey circle is the position tolerance zone of Ø0.1mm

You're making assumptions about the functionality of the component.. There is insufficient information on which feature is applicable as a datum..

Changing datum A and adding datum B may alter the relevancy and function of the feature tolerances.

[JFleck]

You're making assumptions about the functionality of the component.. There is insufficient information on which feature is applicable as a datum..

Changing datum A and adding datum B may alter the relevancy and function of the feature tolerances.

I agree that there is insufficient information on the example drawing and that I was making assumptions. The assumptions were necessary for assessing why the customer rejected the part as described (otherwise the original, physical part may have already been within tolerance). Without the (top) face being a datum, the [17] basic dimension is pointless. I was hoping my intent was clear by stated:

Lets assume for the sake of discussion that the customer wants the position of all the holes to be as I suggested ...

I apologize if this was not clear - I thought it was.

I also agree that changing & adding datum's may change the relevancy. However, the original datum and control frames were insufficient. I was just trying to offer my interpretation of what was originally drawn and what could be drawn so that an educated discussion could happen with the customer.

I am just trying to help, and I feel confident in my answer.