Is this datum hole callout correct? - ISO

[Jieve]

Hello,

Quick question - the way I have the hole diameter labeled as datum B dimensioned, with 2x Diam 9 and the Datum referring to the axis of the left hole, is it clear that the LEFT and only the LEFT hole is datum B? I would like to dimension the 9mm hole only once with a 2x callout, but not sure if this is ok when only one of those holes is a datum.

Thanks!

 

[pmarc]

Yes, it is OK to do it this way. Since datum feature symbol is attached to the contour of left hole, it is clear that only left hole serves as datum feature B.

 

[SeasonLee]

Yes, you may use the left hole as secondary datum feature unless you made the following changes:

1. Remove the quantity 2X from the left hole callout, otherwise we will consider it’s a hole pattern and the callout will be different.
2. Add dimension (Ø 9) callout on the right hole, both holes need to be called out separately; even they are the same size.

Besides, 60.50 should be a basic dimension.

SeasonLee

 

[pmarc]

1. Remove the quantity 2X from the left hole callout, otherwise we will consider it’s a hole pattern and the callout will be different.

I do not consider it that way .

 

[SeasonLee]

Oh, I didn't notice its an ISO drawing, what I said is based on ASME standard, I am not quite sure are there any differences between the two standards here, pls correct me if I am wrong.

SeasonLee

 

[Jieve]

Thanks for the replies.

Does the 60.5 need to be a basic dimension according to ISO? The right hole is being measured from the left hole (datum B), and since there is an assumed 0 dimension (vertical) between the holes (they are on the same line horizontally) I left 60.5 as a non-basic dimension. The 60.5 actually only directly relates the the left hole to the bottom (datum C). In this case, Datum C was simply being used to stop the final rotational degree of freedom.

Pmarc, does this reasoning make sense to you, or do I need to make 60.5 a basic dimension?

Thanks!

 

[powerhound]

I think ISO follows the same rules as ASME in regards to positioning features of size. In order to position the right side hole, you must have a basic dimension. It makes no sense to use a positional GD&T callout while also having a tolerance on the locating dimension.

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2010
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[Jieve]

The tolerance is only on the left hole. The right hole is GD&T toleranced relative to the left hole. Relative to the left hole, there is an assumed zero basic dimension, therefore not specified on the drawing. But maybe I'm missing something here.

 

[powerhound]

It doesn't work that way. If you call out relative to datum C, you must be able to get back to datum C via basic dimensions. This is per ASME. I'm not up to snuff on ISO though, so maybe what you're trying to do is okay per ISO.

Powerhound, GDTP S-0731
Engineering Technician
Inventor 2010
Mastercam X6
Smartcam 11.1
SSG, U.S. Army
Taji, Iraq OIF II

 

[pmarc]

Jieve,
In my opinion 60.50 dimension should be basic (as well as 48.25), but not due to positional tolerance requirement on the right hole. And this statement applies regardless of a standard governing the print.

Now, being more specific - I agree with you that basic 60.50 is not needed in case of positional tolerance. Datum C serves only as a constraint of rotational degree of freedom that Ø0.1 tolerance zone is having relative to datum axis B. Location of the zone relative to B is defined by basic 238.75 and if that rotation is stopped, that is all what has to be done in order to fully define true position of right hole.

60.50 dim. should be basic because of something else - assuming that datum B is of higher functional importance than datum C (this assumption is based on the sequence of datum references specified in Ø0.1 positional FCF; |A|B|C| and not |A|C|B|), datum feature C (bottom surface) should be located relative to datum B. There are at least two options to achieve this: 1) profile of surface tolerance refering to |A|B| applied to surface C - and this method is applicable in ASME Y14.5 standard, or 2) positional tolerance refering to |A|B| applied to surface C - a method recommended by ISO standards. Regardless of which one is chosen, both require 60.50 dimension to be basic.

Similar applies to 48.25 dimension. Left surface of the part needs to be somehow located relative to a datum reference frame. If DRF is the same as for location of right hole, |A|B|C|, profile (ASME) or position (ISO) should be applied to that surface and that requires 48.25 dimension as basic.

And last remark: it is in general not recommended in ISO to use directly toleranced dimensions (in this case 60.50 and 48.25) to locate centers of features or other features relative to those centers. Annex B of ISO 5458:1998 clearly states that the meaning of such method is not standardized and that basic dimensioning + geometrical tolerancing should be used instead.