Simplified Representation in Part drawing

[AnkurAggarwal]

Hi all Can we use simplified representation in a part drawing? Ankur

[ptc-313948]

As far as I know, NO. This is a major problem. It sucks! PTC should address this issue in future releases. As an alternative, I use a family table instace, making sure not to include any undesired parent/child dependencies. I hpoe Wildfire 5.0 solves this problem. I cannot see why PTC could not offer this fuctionality in future releases. Good luck

[AnkurAggarwal]

u r right. family table may solve d problem, but not in every case. anywayz thanx.

[eric.mills]

You have received the wrong answer, yes you can use a simplified rep in your drawing. Under the view properties box select view states next select the rep you want.

[AnkurAggarwal]

But the drop down menu of simplified rep is always deactivated.

[CBenner]

Did you already create a simp. rep. in the model? that needs to be done first.

[AnkurAggarwal]

yes, i first created simp rep in model. then i tried to use it in drawing using View Properties dialog box and view states tab, as described by u. but its doesnt activate. I m using wf 4.0

[WillyC]

I get around the grayed-out Rep Box by adding each Rep separately to the drawing. You should be prompted for a Simplified Rep Name when adding it (or placing first view - I forget) The parts are then treated as unique and individual parts in the drawing. Does make you wonder what use the grayed-out options are, though. Hope this helps, Willy

[AnkurAggarwal]

I tried that also. It do not prompt for Simplified rep while adding the first view. Thanx. Ankur

[Kevin]

The intended use of changing view states with simplified reps is with assemblies. If you want to be able to change the rep using the View States option, add the part to an assembly and create assembly reps that display the part using the part simplified reps.

[CBenner]

Kevin, That seems to be the case, it is greyed out on part drawings, and not so on assembly drawings. Why then (rhetorical) does PTC allow you to use reps at the part level to exclude/include features, surfaces etc... if you cannot then show them in that state in the part drawing?

[ptc-313948]

I hope PTC addresses this issue in future releases. I fail to see the logic of why you can do it with assemblies and not with parts.

[Kevin]

From my experiences that is the way they present it both in the classes I've taken and in writing as the workflow. The option use to be called Assembly Simplified Representation so maybe they will or are headed in that direction. The other way to do what you want might be to create a family table for the part and exclude the features you don't want. You then use Replace under the Drawing Models menu.

[ptc-1972305]

Ankur, YOu can first create Simp rep in part mode by giving name, say for example TEST. Now open drawing then Right click/ Properties/ drawing models/ set/add rep and select your Simp rep (TEST)/ Done. Now when you place new view it will be from your Simp rep not from original model. Hope it will solve your problem. Best of Luck. Regards, Vimlesh

[AnkurAggarwal]

Hi It works. Great vimlesh. We finally got the solution after a long discussion. Thanks everyone. Ankur.

[ptc-4767562]

It is ok when you start drawing from zero.

I can't change existing view's reps from master rep to user created rep.

It is painful.

[haåman]

See my reply here, hope it helps. I'm using Creo 2.

[haåman]

Hello,

I don't know if you are still wondering, seems as if you have solved the problem, but here's what I do in order to have both a Master rep view and a simp rep view in one drawing:

1. Create a simp rep of the part

2. Create a drawing, place a general view, and choose Master rep when you get prompted to choose a rep. As you can see the Master rep is the active model rep if you look at the bottom left corner (REP: MASTER REP)

3. Add the simprep model to the drawing by going to Drawing Models > Add model. Choose your part and now choose the simprep when you are prompted with the rep question. Click on Set/Add model and see that both Master rep and simprep are listed. Choose simprep if needed.

4. See that the active rep is now REP: SIMPREP. Place a general view and it's the simprep view that is placed.

5. If you wish to change back to placing Master rep views you only need to go to Drawing Models > Set/Add rep and choose Master rep instead.

Hope it helps. Think this way is easier. Don't know why one can't choose representation in the Drawing View dialog box under View State for parts...

[cdmorris11]

I created a user defined representation of a part and was able to create another user defined representation in the assembly using that part calling out that part representation. I now have the representation in a view on my drawing but I'm unable to dimension it. Any ideas why that might be?