Part Simplified Rep

[warmwinds]

Can anyone confirm this quirk? In 2001 youcan notcreate a simplified rep of the 3-D part but in the 2-D drawing you can use the 'View-Represent' feature to create a simplified representation by excluding certain features in certain views. In Wildfire II you can create a simplified rep of the 3-D part but you can not show this in the 2-D drawing (simplified rep options are greyed out in the view properties and drawing models box). This gets especially nasty when using wildfire II toopen up 2001 part drawingsthat havesimplified representations. Am I missing something here?

 

[cpodom]

You are only missing what we are all missing, component simplified reps in drawing mode.


We will have to wait for WFIII for this functionality.

 

[Cheesewhiz]

If you right click in the drawing, then go to properties, drawing models, you can select any simplified rep you want .. in WF2 that is and i think in any version of pro/e

 

[cpodom]

Cheesewhiz,


I would love for you to prove me wrong, but that works for assembly drawings not for component drawings.

 

[Cheesewhiz]

cpodom .. u r right .. I miss understood the question


The only way to do it is with family table of the part .. But that is no help for 2001 version .... Could you enlighten me on the application

 

[warmwinds]

The company I work for has recently switched from 2001 to WildfireII. I am modifying a welded part which has a drawing consisting of two sheets, the firstsheet showing dimensions of the simplified piece before welding. The original drawing in 2001 used the 'View-Represent' feature to do this. In Wildfire II, the drawing looses it's simplified view after I modify the part. The SAP inventory system rules out creating two parts.


My solution has been to create an assembly with just the one part. The part alreadyhas a simplified rep definedand one also has to be definewith the assembly. In the assembly, I usedthe 'Substitute' feature in the 'Edit-Redefine' box and clicked on the part and the accept button in just the right order. The drawing of this assembly now allows for selecting the simplified rep in the 'Drawing Models - Set/Add Rep' box.


Unfortunately this means a complete redraw of several drawingsand replacing the part with the new sub-assembly in all the main assemblies. Ouch!

 

[dr_gallup]

You would be much better off in this case to make the part into a family table. Then you could show the simplified instance in the drawing views and you would not have to amek any change to your assemblies. All Pro/E 2001 did with the part simplified reps was make a hidden family table and do the work for you with smoke & mirrors.

 

[kdmgooner]

I have had this problem recently trying to show a part in its fabricated state and then in its machined state. I found this issue in the PTC knowledge base and they say that the only way to do it is by turning the part into an assembly (as done by warmwinds above in this topic). The family table approach works too I hadnt thought of that and I think it is better than the assembly approach. As far as WF3 is concerned, I hope that they are going to introduce it but its not in the pre production version that I have.