Trying to make a circular pattern with multiple features selected

[Tilen]

Coming from SW to Creo...

I am Having problem when trying to pattern this 1/4 part around Y axis. In SW I would simply use combine option and then making pattern around Y axis with 4 parts at 90 degree option. It really is an elementary thing but it seems I am stuck on this one. Is there a way to do this similarly in Creo?

Pattern option seems to be dimmed if nothing is selected. Can I somehow select all the features in the model tree with pattern option being enabled? I tried to pattern one feature at a time but I get errors in the model tree. Then again I doubt that this is the right way to do it. 

[StephenW · Accepted solution]

Couple of things.

Group your features...select them all, right click, group

Your axis (probably a_5), needs to be before the group in the model tree.

Use the "axis" option in pattern.

[Tilen]

After fiddling around I managed to pattern all the features. 

Thanks again.

pattern around axis

[dgschaefer]

An alternative way to do this is to pattern the geometry only.

I'm using Creo 2, the steps might vary slightly in newer versions.

1. Set your filter to "geometry" and select any surface on the model.
2. Right click and select "solid surfaces" in the pop up menu. That should select all the solid surfaces of the model.
3. On the model tab, select the drop down under pattern and select "Geometry Pattern".
4. Select axis pattern and your axis and pattern increment.

This makes a copy of the geometry and patterns that rather than  patterning the features themselves.  Any changes to the solid geometry made ahead of the pattern will be reflected in the pattern as well.