insert part in part

[ptc-2208978]

dear frnds, i have a part file, which i have created for casting. i want to create a machining model. so i want to insert that casting model in a new empty part file. y because, after removel of material in machined model, if suppose i made any change in casting model it must reflect in machining model. pls any of u can ans me?
This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[NIGELHAYWARD]

Sounds like you need to use Inheritance. You need a full pro/E licence for this functionality. I think it is not avaliable in Pro/Foundation. Set up a new part file, just with default planes/axis etc. This represents your machined from casting part. With your existing casting part open use Insert tab then select Shared data and then Inheritance from another model. browse to & select your new part & locate- thats it your casting model.prt is inserted into your m/c from casting.prt. hope this helps

[DavidButz]

vinose, The common Pro/E technique for doing what you want is as follows: Create a new assembly. This will be a "dummy" assembly used only for passing geometry to your new part in a connected, dependent manner. In the assembly create a new part (Three Datums or Empty). With the part active, select Insert--Shared Data--Merge/Inheritance. You have the choice of References/Copy Datums and will want to leave Options/Dependent. Done. Now you can do machining on the new version, and changes to the original casting will be passed (through the medium of the dummy assembly) to the machined version. David

[NIGELHAYWARD]

No need to create an assembly as you used to in older versions of pro/E when using the MERGE command. The process is much simplified now using INHERITANCE. Nigel

[DavidButz]

Nigel, The description of the "old" technique was a follow-on to your earlier post. If you don't have Inheritance capability at the part level, you can still do it with the Assembly technique. David

[nkakulte]

Hello Nigel,

As David mentioned that, I am able to make Inheritance featured by using Component operation in the assembly in foundation licence. Also I have deleted created assembly then also there is inheritance feature is working.

Nilesh