It surprises me that, while running through the different PTC forums, I did not find the answer to a lack in Creo Parametric that seems so obvious to me and to other users who have worked with other CAD systems like SOLIDWORKS, Inventor, NX...
In all these CAD systems, it is possible to create a Symmetrical constraint between parts in an assembly. In Creo Parametric, this simple functionality isn't available at all. Or am I wrong?
Any comment is appreciated, as long as it is polite!
Without understanding the specifics I would suggest that the mirror component function may support symmetric placement of components. This requires that a mirror plane be available for selection to work.
The other option when using skeletons is to create symmetric placement reference features in the skeleton model to deal with this if the mirror is not appropriate.
A possible use could be like in the picture above, where you want to put the red line of the upper part nicely positioned between the two small red lines from the lower part.
Of course, I know that with a good design intent you would create your parts symmetrically around the standard datum planes (as is the way I do most of the times), but sometimes it isn't so so you need another way to position components quick and easy...
Midplane datum should address this. In the scenario you describe adding the symmetry plane takes but a few seconds.
You are correct that Creo doesn't have a constraint that does what you're asking. @tbraxton suggested a fine workaround that I would have also recommended. Just wanted to chime in and mention that symmetric constraints (width mate in SW), can decrease model performance. We try to guide our users to create simpler mates (like a mid plane coincident) to keep performance high. Advanced mates take longer to regenerate as they are dependent on more features. Probably not the most scientific explanation but hopefully helpful.
thanks for your reply! Yes, you're right and I also tell people the same explanation you just provided.
In addition to what Philip has posted I would like to post another example where I feel that Creo Parametric falls short. I have two assemblies that are similar but not symmetric so no possibility to use the mirror. Both assemblies are positioned symmetrically around a center plane and I want to control the overall width.
Really something very common in machine building. With any other CAD system I have worked with I would use the symmetric constraint together with a constraint defining the distance between the two assemblies. So just one parameter controls the width. In Creo I have not really found a decent and easy way to do so.
The only way I can think of is placing the overall distance constraint, and then creating another distance constraint from one end to the center plane controlled by a parameter (through relations) that is half the value of the first and overall distance. This way there is only one parameter to control and symmetry is maintained but for me personally this feels far too complex. Moreover this way of working is not allowing me to use this assembly in a flexible manner on a higher level; if I want to change the width on a higher level I have to change the parameter but if I just want to link the position of one end to another component I have to disable the distance constraint and by doing that I am loosing the symmetry again because it's controlled by the very distance parameter.
Any help here will be kindly appreciated.
No relations required to do this and you can use the mirror functionality.
They will then always be equidistant from the symmetry plane. A single linear dimension controls the distance between the components and you can create a dimension for the full distance between components for reference. Creo 7 models enclosed for reference.
There are of course other ways to manage this in Creo such as skeleton models and layouts (Notebook file).