I think I'd use planes. If you want to keep your tree tidy, I think you can create planes 'on the fly' while assembling components...
If the rectangle is likely to change size and you want the placement to update, then use a relation to set the plane offset.
Someone else may come along shortly with a better method, though!
As a novice user, can you elaborate on how to use the plane?
I will be deleting the rectangle once the component is in the right position. I just need it in the correct location before I do delete it. With other components, I've just been setting coincident constraints and doing well - but the round vs. square geometries are throwing my basics off...
Well... I'm assuming that the circular part has some planes already, and that two of them pass through the centre.
Create a plane (or two planes) in your assembly, referencing parallel surfaces; then when you assemble the component, you can do so by selecting a component plane and an assembly plane in turn, which will then become coincident.
If this isn't clear, maybe see whether you can find some tutorials on building assemblies.
Incidentally, if you're going to delete the rectangle afterwards then make sure you don't reference it to assemble the component, either directly or to define the assembly planes. 'Deleting things later' isn't really how Creo works - you need to choose references that will continue to exist.
Hi, if you think of deleting the rectangle after having placed the circular part, that means you need references to place you model. You shouldn't draw that rectangle but instead place references, such as points, axes or planes in order to get your part in the place you want. And don't forget that you might have to move that component, so create your references to give you this possibility.
I'm on the relations bandwagon by using measurement parameters.
That way you can "center" planes with a simple equation "dn=measurement/2" on a plane offset.
And, even better, you don't have to go back to older models to add reference geometry.
And of course, construction geometry (curves) that one can use in an assembly as assembly constraints is not unheard of either.
There are many options of how to do it, but you need construction geometry in each part to align them properly.
In the tan part, I'd make sure you have datum planes through the center in all 3 directions. Ideally, that's where the default places would be. The best modeling practice is to put your three default planes through the preferred or logical origin of the part.
In the part with the rectangle, add datum planes that pass through the center. I'd avoid offset planes driven by a relation, but that will work (and it better than offset planed NOT driven by a relation). Relations are sort of buried drivers to your design intent, one has to go looking for them and then you have to dig to find which feature the dims that drive them belong to.
I suspect that rectangle is an extrude feature. By placing a geometry point centered in the sketch you will end up with an axis at the center of your rectangle. That can be used to create 2 of the 3 planes that will stay centered if the rectangle changes size. The third is harder to do without relations and would depend on how the model is built. That one may need to be relations driven.