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Relations in Assembly should change the parts parameteres by using family tables


Relations in Assembly should change the parts parameteres by using family tables

Hello everyone, 


I am relativly new to PTC Creo and I am having a big problem that I don't get solved by my own.


I want to make a assembly of different parts, which should be variable in height and length. So I decided to put every part in the assembly and drive them by the relation tool. 

I defined paramters in the assembly (LENGTH and HEIGHT), and set in the relation tool every part length connected to my parameters (e.a. d6:01 = LENGTH).

Also I set some distances between the part connected to the paramters (d10 = LENGTH)


After defining all relations I wanted to make a family table to create every product with (length x height) that I want to. 


The only problem is that the part parameters don't change when I open the family member of the table. It's only changing the direct assembly relations, means that all relations connected to parts (e.a. dXX:XX) don't change in the new family member.


I hope you could understand my problem and even more that you can help me. 


Thanks a lot for your efforts.




You seem to say that you are changing a dimension which belongs to a feature inside of an assembled part by assigning it a value of an assembly parameter via an assembly relation - e.g. "D6:01 = LENGTH".  You then vary value of LENGTH in different instances of the assembly family table.


As an aside, a part assembled into an assembly will have an even number for its session ID, so I'd expect something like "d6:2 = LENGTH" for the relation.  Anyway, if my assumptions are right about what you are doing and trying to achieve, then you will not be having much success (although what you are doing seems quite logical)


Basically, you should be aware that the assembly level relation you are using actually changes the sub-component model upon regeneration.  Say your sub-component is a bar that is 100mm long.  Then you put this bar into your assembly and craft the above relation - upon regeneration, the bar will (permanently) become LENGTH mm long.



So what's missing in your modeling is specifying (in the way PTC intended) the various lengths of bars you will be using.  You do that by making the bar be a family table part.  In its family table, you vary the D6 dimension.  You then assemble the bar generic into your assembly and then you build the assembly family table and use "component" as the variable item.  For a given assembly instance, you specify the bar instance (see Tools->Replace Using->Family member function in the assembly family table editor).


In other words, Creo will not auto-generate the bar "variants" from assembly level relations.  Well, you can if you use flexible components, but that's another can of worms 🙂

Community Manager



Did pausob answer your question?  If so, can you please mark as the "Accepted Solution."


just for you reference, I use notebook to transfer golabl parameter to all level assembly or part. all they can synchronizate the global parameter. for your case, you can put LENGTH_BAR in notebook and all related assbly or part. after declaring, they all change to your notebook setting data.

however for your pre setting a table of the gobal parameter and clike to synchronizate to whole assembly, I remebly some example, but can not remember it.

just show you another way to transfer parametr to whole assembly.