Tolerance Analysis - Bonus consideration on chained basic dimensions

[Luis Ernesto Quiroz]

Hello,

In Alex Krulikowski Workbook Unit 11 Example #1 basic dimensions 20 (1) and 20 (2) are add up and considered as 40 basic ignoring the position and bonus of the central hole and only considering the position and bonus of the initial and final holes (condition 1B):

However, in Unit 12 Example #6 dimension 20 (2) does considers the position and bonus (condition 1B) and again neither basic dimensions 20 (1) nor basic dimension 8 (3) considers the position and bonus of the hole between 8 and 20 (condition 1B).

My questions are:

1. considering note #5 in Bonus/Shift Chart "Stacks using chained position callouts must include a location tolerance for each callout" does an additional feature control frame for the hole between basic dimension 20 and basic dimension 8 need to be add to consider its position tolerance and bonus on the tolerance stack up?

2. Would everybody agree that this drawings are only for academic purposes and real drawings should show basic dimensions for each hole against datums B and C and not between features?

Thanks a lot for your comments on this post!!!

Luis Ernesto Quiroz
Mechanical Designer.

 

[3DDave]

The second example is to see if the user was paying attention to the importance of datum feature references. The basic dimensions don't change; the datum feature reference for the 8.6/8.2 diameter holes aren't the same as for the other holes, particularly the one identified as datum feature D.

Real drawings are just like this, but it's less common that anyone cares about the remaining thickness to do such a calculation. It's also not clear why anyone would define a part in the second manner as variation accumulation is often unwanted but, again, it's mostly to see if the reader/student was paying attention. I say variation because the variations can accumulate; the tolerances don't.

 

[Belanger]

There's nothing wrong with chaining basic dimensions together, even if the dimension is touching off of something that isn't a datum.

For your question 1: "Does an additional feature control frame for the hole between basic dimension 20 and basic dimension 8 need to be add..." No, because they don't have chained position callouts (the position callout of the large center hole references a different datum reference frame than the position callout of the 4 small holes).
But actually... While it is given as Note 5, that is actually a triangle #1, which tells us that there is "No shift when planar datums are referenced." (From page 12-3 of that textbook.)

For question #2: I wouldn't say that, because there may be a reason to have an intermediary basic dimension (for some other GD&T callout). Also realize that basic dimensions are not required at all, because designers are allowed to add a note appealing to CAD data for basic/nominal locations.

 

[drawoh]

Luis Ernesto Quiroz,

In answer to your second question, the [box]40[/box] basic dimensioning shows design intent. This all gets programmed in CNC. It is a little inconvenient for the inspector. Before CNC, it would have been inconvenient for the machinist, and I would have dimensioned from the datum, as you note.

--
JHG