Created a feature referencing the leader of a patterned CSYS. The datums were created on the fly off the CSYS. Tried to pattern the feature but the reference pattern option is greyed out??
It simply doesn't recognize the previous pattern as related. I've put a feature between a referenced pattern and the reference failed.
Often I avoid reference patterns because in Creo 2 M040, they are seriously unreliable. Even in Creo 3 they are not overly reliable.
I've used ProE since the early 90's, I think it was vers3. Stopped using it about 10 years ago. Recently started using it and am surprised that the functionality is seriously lacking. It used to be much better!
I doubt a software bug is a culprit here.
Reference patterns work just fine - if you keep your references tidy...
It seems like you know this, but it's always easy to miss something. Specifically, you seem to imply that since the feature datums were created "on the fly", there should be no problems, which just does not sound right.
If you posted a screenshot or better yet - the example model, the mistake would probably be quickly spotted by someone here.
Attached is the 3D model and the reference viewer associated with the extrude 13 feature.
Aha, I see. You are trying to reference pattern Extrude 13 because CS1 is the leader of Pattern 1.
Fair enough, but the problem is that reference pattern requires that your feature to be pattern is based directly on the leader of another pattern.
And your Extrude 13 is not directly dependent on CS1... It is actually dependent on Sketch 11 (which is dependent on CS1).
Try reference patterning Sketch 11, then see if reference patterning of Extrude 13 works. (It does for me in a toy example I made up in Creo 2.0)
Alternatively, do not use a stand-alone sketch as the section of Extrude 13 - instead, unlink its section from Sketch 11, then try to see if reference pattern works.