How to add a model datum to a dimension

[fgallagher]

I want to add a datum B to the .813 diameter dimension to start my hole sequence. How can I add this datum?

I was able to add datum A to the surface shown below without any issues.

[StephenW]

1.Right click on the axis for that hole you want to specify as "b".

2. select properties

3. select the datum symbol

4. select "in dim"

5. pick the dim you want "b" to show up under.

[fgallagher]

Stephen,

Thank you for the response, everything worked except when I tried to pick the dim I wanted "b" to show up under I keep getting the error "Selected part in not active. Select again". How can I select the dimension I want to use?

[StephenW · Accepted solution]

The dimension you are picking has to be in the model your axis is in. Also, it can't be a created dimension, it has to be a shown dimension.

Your screenshot looks like an assembly. If the hole is in the part (not assembly) and you are adding GD&T to the assembly, it won't work.

Is the holes assembly features or are they in the part?

[Lalo_T]

That works on CREO 3.0 but doesn't seem to work on CREO 4.

[StephenW]

This is a post from 2014 so Creo 4 wasn't there yet.

Try this one maybe or post a new question.

 https://community.ptc.com/t5/Creo-Modeling-Questions/Unable-to-access-set-datum-tag-in-creo-4/m-p/494567#M114257

[rmix]

Create the datum in the part, set datum in the part.

In the drawing go to datum feature symbol under "annotate" - then it asks where to put it. I was afraid it wouldn't align with the diameter dimension, but it did.

[StephenW]

And is that old school pro/e blue background? Man, you're going back to the golden ages!!!!

[fgallagher]

Stephen,

Thanks for the last response, the dimension was a created one and not a shown one so that fixed it. My IT department defaulted the blue background for us, so I just kept with it!! I've only been a Creo/Pro E user for a little over a year now, but I'm getting there. Thanks again for the help!

[fgallagher]

Stephen,

One last thing, when I select the model driven annotation to use on the drawing, creo places this on a different hole than what it is on the model. Is there any way to change this location? On the four hole bolt pattern, I want the dimension on the lower right hole and not the upper left.

[StephenW]

It's a true pro/e Pattern right? Not a single sketch with all 4 holes.

In the drawing, right click on the hole dimension and DELETE.

Go to the show annotations box and select to show dimensions and pick the specific hole you want the dimension shown on. It'll show the dimension on any of the holes in the pattern.