Position Tolerance, Basic Dimension, and Aligned Features 2

[YNIEH]

I need assistance resolving this dilemma I've run into on a few occasions now. I have a series of holes that are vertically aligned. Typically, the dimension to locate the holes from the datum would be shared by all the holes. Two out of the five aligned holes need to be very precise. The remaining holes are clearance holes so precise control isn't necessary... I'd like to leave the shop plenty of leeway with these.

My dilemma: what is the most appropriate way to get the precision I need, leave leeway where appropriate for machinists, avoid unnecessary clutter on the drawing, and satisfy ASME?

Right now I see two options.
Option 1: Two locating dimensions - one basic and one with the title block tolerance. The clearance holes wouldn't have a position tolerance in this instance.
Option 2: Make all locating dimensions basic. Add position tolerances to each hole callout even though the clearance holes don't need precise control.

How would you handle this situation? Would your approach change depending on the size of the part and number of different holes in alignment? I can't find where ASME covers something like this.

Thank you for your feedback.

https://files.engineering.com/getfi...4f8e-9ae0-e8a5ef4283f9&file=hole_position.JPG

https://files.engineering.com/getfi...8-db9873418313&file=hole_position_option1.JPG

https://files.engineering.com/getfi...9-07112dbf16a5&file=hole_position_option2.JPG

 

[Belanger]

I suggest a modified form of your Option 2.
Since you mentioned ASME, the Y14.5 standard actually discourages Option 1 -- see paragraph 5.1.1.1, where they say that "tolerances on dimensions that locate features of size are specified by the position tolerancing method described in Section 10" (Section 10 being the GD&T method of positioning). In previous versions of Y14.5 they allowed for some wiggle room to use traditional +/- tolerances for locating holes, but that's always been fraught with problems.
So make all locating dims basic. But instead of having a position callout for each hole, perhaps give the tighter position callout a note saying "all holes marked X" and then put an X near those holes. Then give the more generous position callout a note saying "all holes marked Y" with those non-critical holes labeled with a Y.

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

 

[Burunduk]

The remaining holes are clearance holes so precise control isn't necessary... I'd like to leave the shop plenty of leeway with these.

Clearance holes have function too - they need to maintain clearance.
You can leave the most leeway if you apply position at MMC to the clearance holes. If the diameter tolerances and the position at MMC tolerances are carefully applied, you can provide the most tolerance to manufacturing while being safe that no interference will occur.
Location by title block tolerances is ambiguous and can be somewhat risky, and if you focus just on the tolerance value, most chances that properly applied position at MMC will allow the manufacturer bigger total variation.

 

[Belanger]

Burunduk, based on the paragraph I quoted from Y14.5, would you say that location by title block tolerances is ambiguous, or forbidden?
That's one of the few times where they don't say "should" or "shall" -- they merely say "are."
Strange!

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

 

[Burunduk]

John Paul,
I think the Y14.5 standard now almost forbids it.
Directly toleranced dimensions for location of features of size are not explicitly forbidden, but probably more clearly unsupported than before.

What I find important for everyone to realize is that, as you know, directly toleranced distance locating hole axes or slot/tab center planes have no single defined meaning. And while metrology equipment and software have ways to cope with them, those ways may vary greatly.

Certainly, there are those who don't mind when controls of those part features that are considered non-critical to function remain fuzzily defined, but a better approach would be to use loose enough geometric tolerances that are precisely defined. The latter approach lowers the risks of both acceptance of bad parts and rejection of good parts.

 

[YNIEH]

Great info and perspectives, guys! Thank you for getting me lined out!