DRIVE PART DIMENSIONS FROM ASSEMBLY

How can I control a part dimension from the assembly mode? I want to insert the parameter in the assembly family table and be able to control this dimension.
Edited by: Tesla77

You need to drive part dimension with assembly relation.


d12:34 = 50


Where d12 is the dimension and 34 is SessionID of the compoent.
To find Session ID, Tools > Relations > Show > Session ID > Part > Pick the part.


Charles
(WF2)

That woks awesome!!


Now how do I create a parameter to drive thisrelation in the assembly family table? I want to be able to change this dimension in different instances using the parameter.
Edited by: Tesla77

dig in the help files and in the PTC knowledge base for layout. If you dont have AAX, you can use a 3D note instead.
Basically you create a parameter and a 3D note like dimension=&parameter. Then you write al relation like d12:34=parameter. You dont need family tables for this.
You edit the parameter by RMB #value in your note

Edited by: ReinhardN

I do it this way...


Create a sketch in an assembly (You may call it Top Down Approach) to represent the parameters.


Drive the assembly thru the parameters of the sketch (Family Tables.... Configuration...)


A thorough study of Help on Family Tables is required under Proe/Fundamentals. It is very difficult to put the same in a forum post.


This is a very effective way to create families of Assemblies and Components...from the General Assembly.