How to make a hole pattern a datum reference for GD&T?

[lwestlake]

I want to make my hole pattern datum C and reference it in a feature control frame. How do I do that in Creo?

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[lwestlake]

I should say, how do I attach a datum tag to a hole pattern...

[dschenken]

A datum reference symbol is typically attached to the diameter dimension of the holes in a pattern. Create an axis through one of the holes (never use an axis that's part of a feature unless you want to make things more difficult) and then choose "IN DIMENSION" or whatever is right for the version of PTC software you are using.

[RonSt.Pierre · Accepted solution]

David,

In all due respect, it is the axis of the pattern, not an axis of one hole of the pattern, as I understand y14.5 1994

Ron

[dschenken]

The axis of a pattern is never identified on a drawing. To get PTC to show the datum reference symbol it needs a feature, typically a model axis. The model axis could be anywhere because the datum reference symbol is never shown on a drawing attached to it; it will be attached to a surface or to a dimension.

There is specific direction prohibiting attaching datum reference symbols to centerlines for drawings.

[RonSt.Pierre]

Lori Westlake‌, to your question, David is correct when one is producing a drawing to denote a pattern datum (see my reference to the Y14.5 spec for how this looks like.)  It takes human understanding that the pattern can revolve about the pattern axis.

However, when dealing with MBD parts, I question the selection of an individual feature of a pattern to describe a pattern datum in a model.  How does this get described?  Is it the full annotations that must get applied to the model?  Is there a different way?

Just wondering....

[RonSt.Pierre]

I would refer you to visit ASME Y14.5M-1994, paragraph 4.5.8 and figure 4-22. (I don't know/have 2009 yet - assuming it's the same)

Once you understand that, you should be able to answer your own question.

Sorry for being vague, but there is no way I'm going to try to explain this one here

Edit:

I assume you are making a radial pattern with the holes.

If it is linear, I'll be lost to explain.

-r

[lwestlake]

When you use a hole pattern as a datum it establishes 2 mutually perpendicular planes at the center of the pattern ...and since I'm locating the pattern to a datum plane that keeps it from rotating.  I just wanted to know how to create the datum tag in Creo and I figured it out by trying the suggestions given here.  Thank you!  I'll probably be visiting this forum more often!

Thanks for all the quick responses.

Lori

[Dale_Rosema]

Don't forget to mark an answer as correct, even if it is your own, so that those following behind will know that an answer has been found.

[lwestlake]

My pattern happened to have been 2 holes so I created a datum plane thru each holes' axis and named it "C".  Then as David said I chose "IN DIMENSION" and attached it to the 2X dia. dimension of the hole I am calling out on the drawing.  Because the datum tag is attached to a 2X dimension - this indicates the pattern is the datum.

Cheers!