Display 3D Annotation with Parameter of Subassembly Inside Larger Assembly (Creo Parametric 7.0)

[TE_11078759]

Hello,

I'm currently attempting to display the "&DESCRIPTION" parameter of a subassembly within a larger assembly model, but am having issues. Here is what I've currently tried:

Typing "&DESCRIPTION" into a leader note attached to the subassembly displays the description for the overall assembly, which is not what I'm looking for.

I'm aware of some modifiers that can be added to these commands to change how they display. When I type "&DESCRIPTION:att_mdl", I get the parameter for the specific PART within said subassembly. I'm combing the list on PTC but none are jumping out as the solution (but maybe one of them is).

Is there a way to acquire this parameter for the intermediate subassembly? I can access it while searching around the parameter lists, but I don't know what command to type to display it. I have several subassemblies in this assembly and would like to show the name/description for each of them in one view.

[KenFarley]

If you are writing relations in an assembly, you can reference dimensions from a specific part by appending the parameter used in the relation with the session ID that corresponds to the part/assembly of interest. For example

lengthAssembly = length:14  /* sets the lengthAssembly to the value of length in the part with session ID = 14

lengthAssembly = length:5   /* sets the lengthAssembly to the value of length in the assembly with session ID = 5

Unfortunately, this doesn't work on drawings. When I need the value of a parameter or dimension from a subcomponent, I usually define a parameter in the assembly to contain the value. I then use a relation in the assembly to obtain that value from the subcomponent. Once I've done that, I can use that top-level assembly parameter in the drawing for that assembly. It's a pain, but it works.

[MartinHanak · Accepted solution]

Hi,

to display Parameter of Subassembly using &DESCRIPTION:att_mdl you have to select feature which belongs to this subassembly. For example default coordinate system.

Suggestion: If you need to attach the note to specific location, create datum point in subassembly and place it to the requested location.

[TE_11078759]

This was ultimately the method I used to display what I wanted to display, thank you for the response. I wish Creo Parametric had functionality to perform this without having to create a datum in the subassembly; it makes it harder to place the annotation somewhere else if it has to be moved. But for now, this works as a good stop-gap.