How to make relation parameter in mother assembly with all sub part in model tree

Question

DearI want to make somes parameter in assembly file, if i change this parameter in mother assembly other all part in model tree automatic change together (Normal Creo, not Windchill)Ex:I want to make 2 parameter: Project, local show in the picture => when i make this parameter in mother assembly => all part or subassembly will be add two paramater tooThen when I change this parameter in mother assembly => all part...drawing will automatic change.Or if possible this parameter collect with notepad file... then mapkey to do replace This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

KenFarley · Answer

I have done something like this in some assemblies. Specifically, as follows:

(1) The parts and assemblies all have a parameter called "Title2" that is used on drawings. It is the second line of the title block, usually the project description.

(2) When I set the parameter for the top level assembly, I want it to be set for the subcomponents (except for common hardware like screws, dowel pins, etc).

(3) Once the assembly is put together, I use relations to set the "Title2" for the parts to the assembly's "Title2". For example, I'll have something like this:

Title2:22 = Title2

The ":22" added to the end of the parameter name is the session ID for the part. Each part in an assembly is given a number when it is put in the assembly. One number for each part, no matter how many times that part is in the assembly (i.e. if you have a block included in your assembly 50 times, it still only gets one session ID). The second "Title2" in the relation, since it doesn't have a ":##" suffix, is the assembly's value.

(4) Session IDs for parts or assemblies are found by entering the relations editor (Tools->Relations), then via Show->Session ID.

(5) The Session ID for a part will change every time you start up Creo (i.e. today it might be 22, tomorrow it might be 4), but it's not something to worry about. The relations you define will be updated automatically.

You should try this out with something simple to get a feel for it. We don't use Windchill, so I don't know if this type of thing causes any problems with it.

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