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urgent please..:))

john666

New member
i want to know how can we create different configurations of the assembly in proengineer wildfire.

and i want to show differerent configurarions of the same assembly in the detailing section.

can anyone help me please??????????
 

skraba

New member
Use Simplified Representation feature. You can exclude parts from the assembly and so "create" new configuration of the assembly. Those SimpReps can be then shown on the drawing.
 

dr_gallup

Moderator
Family tables are another way. You can have different instances of table driven components as well as exclude/include components. Then you add the different instances of the assembly model to your drawing.
 

SSLaser

New member
From a BOM standpoint: Are you trying to create different views of the same assembly, or are you trying to create slightly different assemblies? In my experience, simplified rep is suited to the former, family tables for the latter.


For showing family table instances, you have to "add model" (i.e., one of your instances) then "set model"the newly added instance. Any view you add after that is of the new instance model. To switch back, just "set model" your original model. In this way you canshow multiple assemblies (or parts, etc.) on a single drawing. They don't even have to be related by family tables.


To add model for WF 2.0: Right click on the drawing field (not in a view) and choose Properties>Drawing Models>Add Model


To set active model for WF 2.0: Right click on the drawing field (not in a view) and choose Properties>Drawing Models>Set Model


I hope this helps.
 

skraba

New member
For WF2.0: to set active model or active rep you can double-click model or rep description text on the bottom of the screen (beside scale and format description). The drop-down menu is shown so you can simply select the desired model/rep.
 

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