simplified reps

[John.Pryal]

Hi all, is it possible to create a simplified rep of a part in the same way you can with assemblies. I want to show a drawing view with some features not showing, hiding features or putting them on layers does not work, it does for some features such as curves & surfaces, but not solid geometry. This posting is linked to my earlier one about copying geometry. What i am ultimately trying to do is show a sketched curve that drives a revolve feature without showing the revolved solid geometry, i just want the curve visible in a drawing view. Hopefully, this will make sense to someone out there. Regards John
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[sschroeder]

You can make simplified reps of parts. Use the view manager while the part is up. Notice there is a simp rep tab. There's a few options for how to create one in a part. If you select the "Features" option from the menu, then you can turn on/off any features in the model without worrying about parent/child relationships.

[John.Pryal]

Hi Steve, thanks for the reply, that is exactly what i wanted to do, but now i have another problem. How do you create the drawing view with this sim ref active? When i bring in the part onto my drawing, its the full part with all features present. I edit the properties of the view & can see that under view states category there is a simplified rep tab, but its greyed out, i don't appear to be able to select the sim ref i created on my part. Kind Regards John

[timb]

For parts: Go to Drawing Properties> Drawing Models> Set/Add Rep, then just add or set the rep you want. I don't know why you can't just change the "View State" like you can with an assembly. Tim

[John.Pryal]

thanks for the replies guys, i figured it out this morning. it would appear you can only add new views, you cannot modify an existing view & impose a sim rep upon it, that is why i was struggling. Regards John