create a part in the assembly mode

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Is it possible in pro/e 2001 to redesign a part component in the assembly mode ( create a protrusion) having as references surfaces of other parts of the assembly, and simultanuisly to see the changes in the prt file of the part??????



Or can you create a new part in an already full constrained assembly in an assembly file??

 

[bem]

You can do both, but be aware of the parent/child relationships you are creating.



To bring up your modified part, you'll need to load the assembly as well.



A better approach would be to create a copy geometry feature in the part and do all the modifications at the part level

 

[nemecek]

Hello,



You can create a new part and add a new feature to existing part.



1) Add a feature:

In the model tree click a right button on the part, witch you want to edit. Choose a insert feature and next you work like in part module.



2) add a part to assambly

Choose a component -> create in the menu

Choose insert feature in the model tree.



Best regards

Ladislav Nemecek

CAD Designer

 

[jabbadeus]

Regarding question 1, as bem stated, yes you can. That's called designing with External References. You want to be very careful how you go about doing that, because also as bem pointed out, you create dependencies between the part and the assembly. A lot of places shun designing with external references, but if you use Data Sharing features (like Copy Geoms, also as bem pointed out), you can control change propagation by toggling dependency on and off, and you won't have to check out the whole darn assembly to open a single part.



Creating a part in the context of an assembly is a very common operation, but again beware of creating dependencies between the new part and your assembly. When prompted for creation method, the best bet is the first choice (IIRC) which allows you to specify a default template or start part. Create First Feature and Locate Default Datums make the part dependent on the assembly.

 

[scottm]

I'm still new to Pro-E and maybe I'm overestimating what it can do (compared to Boolean modeling).


If I have a curved surface and I need to put maybe a dozen curved braces on that surface - what is the best way to ensure that the braces match the curve on the base?


I was tinkering with creating parts in assembly mode, but I can see how that is problematic. I tried copying the sketch geometry from the curve - but its not associative. Can I reference geometry in another part without referencing its location? Or do I just need to use relationships to link the defining dimensions of the surface to define the brace dimensions?


Thanks,


Scott

 

[donha]

Start your new part with default datum planes. You can then insert shared data (copy geometry from other model). Please note, when you copy geometry from other models, if the other models change, you must have them active in memory and regenerate the part with the copied geometry. In your case, the copied geometry would be the curved surface you are placing the braces on.