two representations in one drawing

[Tudor]

Is it possible to use 2 representations in one drawing ?


For instance master rep. in some views and another simplified rep. in other views ?


Thanks!

 

[PRStockhausen]

Right cliick on the drawing outside of any view or table. Select properties, then set/add rep and add the second rep. Or create your view, select the view, right mouse button and select properties. Then goto view states and set the simplified rep. (These selections are for WF3, they may be different in other versions.) Note one thing I did not expect, if you have a section of rep a, you can show the arrows in a view of rep b (assuming they are of the same assembly). Also note that views of simplified reps can only be made of assemblies not parts.

 

[Tudor]

I've done this in the pastin WF 2 with assemblies.


Now, I'm using WF 3 but I'm trying to do the same with one part and the window View States from view properties in not active (as below).


View attachment 3347


I'm trying to eliminate one feature from one view and to have it on other.


Is it other way to doit ?

 

[PRStockhausen]

One way would be to create an assembly with the part as the only component. Then create an simplified rep of the assembly and use the simplifed rep from the part in that simplified rep. Then use that assembly simplified rep in the drawing. Or you could create a family table and show the instance in the drawing for the simplifed view.

 

[dr_gallup]

About Creating Views of Part Simplified Representations
You can use part simplified representations as
representations of drawing models to create general views. Child views such as
projection views, detail views, and so on use the general view of the same part
simplified representation as the parent view.
When you display dimensions in the view, only dimensions of
features included in the part simplified representation are displayed.
Displaying annotations in the view of the part simplified representation is
similar to displaying annotations in a view of a family table instance. For
example, a view of a part simplified representation shows a note even if the
parent feature of the note is excluded from the part simplified representation.
If a note belongs to an annotation feature and the parent feature of the note is
excluded from the part simplified representation, then the note is not shown in
the view of the part simplified representation.
Note: Driven
dimensions are stored with the part, and not with the part simplified
representation.
You can set the part simplified representation as the
representation of a drawing model for a new drawing by selecting the required
representation from the Open Rep dialog box. This dialog
box opens when you create an empty new drawing for a model that has part
simplified representations that you can use to create a drawing.
You can set the part simplified representation as a
representation of the drawing model for the active drawing by clicking File > Properties > Drawing Models and clicking Set/Add Rep on
the DWG MODELS menu.
Note:

You must convert the part simplified
representations created in Pro/ENGINEER Wildfire 2.0 and earlier releases to
Pro/ENGINEER Wildfire 3.0 part simplified representations to make them usable as
models for creating drawings views. You can perform this conversion through the
View Manager dialog box, that can be accessed, in the 3D
mode.

After you convert part simplified representations
from the Pro/ENGINEER Wildfire 2.0 or earlier releases to Pro/ENGINEER Wildfire
3.0 part simplified representations, these conversions cannot be undone

You can create drawing views of user-defined part
simplified representations only.[/list]
See Also
About
Simplified Representations in Drawings
To Create Drawing Views
of Part Simplified Representations in an Active Drawing
To Create a New Drawing
of Part Simplified Representations
< ="1.2" ="text/">