Taper only in one direction

[bxbzq]

I have an irregular internal feature machined through on a block with bottom face being datum feature A. Now I want the internal feature to be perpendicular to datum A nominally and allow the feature tapered in one way, but not the other way, ie, opening of the feature at bottom being larger than at top is ok, but the other way is not ok. Is there a clean and clear way to specify the requirement on the drawing?

 

[Catbug]

I think the most straightforward thing to do would be to simply dimension both openings and specify tolerances on each that do not overlap each other; only one of the openings can be larger than the other and not the other way around. This would be if you only care about the top and bottom openings of the taper - the entire taper can be controlled using an angularity or surface profile tolerance with a tolerance zone sized such that only one of the openings may be larger than the other.

Perpendicularity may be controlled separately with position or perpendicularity.

 

[bxbzq]

One more try. See attached pic. How to call out the internal feature?

 

[bxbzq]

I'm thinking to use conventional angle callout, 90^o(-2, 0), for example.

 

[Tarator]

what is the purpose/function of the hole? why can it not be taped the other way?

 

[Catbug]

I would do it like this.

Does it make sense? Not writing a, b, x and y literally of course, but using whatever are the required predefined values.

 

[pmarc]

Since this is IRREGULAR feature, I would first consider applying profile of surface FCF wrt A all around the feature (the contour would have to be dimensioned by basic dimensions of course). This will control perpendicularity of surface of the hole relative to datum plane A plus size and form of the hole. However, it will not be able to control direction of taper (as a matter of fact, by default geometric tolerances are not able to control "behavior" of toleranced surface inside tolerance zones).

Therefore something extra is needed.

And I think the idea with directly toleranced 90deg angular dimension may work in this case, but with some modifications:
1. Replace one of dimension line arrows - the one starting at datum A - with origin symbol (see fig. 2-18 in 2009). This will clearly indicate the feature serving as an origin for angle measurements.
2. Change the dimension value to 90deg MAX. There is no need to control the lower limit of the angle, because it is already indirectly controlled by profile tolerance zone.
3. Put SEE NOTE # (or similar) under the angular dimension and clarify in notes area what the "SEE NOTE #" is about. And this is, of course, the trickiest part. In my opinion the note should somehow state that the angular dimension applies to each TANGENT LINEAR ELEMENT of the surface of the hole. This will work similarly to an orientation tolerance modified by (T) and applied to each linear element of the surface (imagine fig. 6-16 in 2009, but with (T) modifier after 0.02 inside the FCF, and with EACH ELEMENT notation beneath the FCF). The only difference between directly toleranced angle approach and geometric tolerance approach will be the shape of tolerance zone - two non-parallel lines vs. two parallel lines.

Does it make sense?

 

[bxbzq]

As pmarc pointed out, since it is irregular feature, Catbug's idea won't work.
But pmarc, I don't get TANGENT LINEAR ELEMENT part. Why would I need to control tangent linear elements, not just the surface?

 

[pmarc]

Why would I need to control tangent linear elements, not just the surface?

Well, in my opinion the main problem is that Y14.5 is silent on intepretation of directly toleranced angular dimension requirement applied to contours like holes or pins. Does the requirement apply to whole surface of hole simultaneously or just to each single linear element of surface separately? How would the tolerance zone look like in case of your irregular internal hole? Or for simplicity, how would it look like if your hole was regular? Would it be a space between two non-parallel cones or a collection of spaces between two non-parallel lines? I am not able to tell with certainty, and that is why I decided to use a note precising which feature(s) the requirement applies to.

Why did I choose to control linear elements instead of whole surface? Because then I would not be able to use concept of tangency, I believe.

And why did I use the concept of tangency? Because it would give me the idea about inclination (taper) of hole surface in each cross-section without going into details about actual form of the surface. The actual surface would still be controlled by profile requirement.

 

[bxbzq]

What about using draft symbol in a machining drawing?

 

[CheckerHater]

How about just using a verbal note?

 

[bxbzq]

CheckerHater,
If we don't figure out a straightforward symbolic way, note would be the option.

 

[CheckerHater]

I would appreciate if you tried to visualize how your tolerance zone looks like.
Is this what you are trying to achieve, tapered surface being just “somewhere”, or taper will have its own tolerance zone like straightness?

 

[bxbzq]

Now I think the wall of the internal feature does not need to be perpendicular to datum surface A. I can model it to be say 88^o and specify a all-around profile tolerance, making sure the outer boundary at top smaller than inner boundary at bottom. In this case the tolerance zone would be the space between two cone-like shape, but the xsection is not a circle.