Create new part in Assembly 1

[rocket100]

Hi Guys,

I am working with assembly and want to create new part inside the assembly. that new part will be made through projecting curve from the another part in assembly.

After I create that new part, please advise how will I be able to save it as a separate model.

I hope it make sense.

Thank you

regards

Rodney

 

[RhysMog]

Hi rocket,
If you're modeling within the assembly (not within the existing part), just use Project Curve and create your model geometry, then use "Create Component" within the 'Assemblies' application toolbar. Just select any geometry you want to be included in your new part and give it a name/number. Done.

Hope this answers your question.
Rhys

 

[rocket100]

Thanks Rhys, Thats exactly what I was looking for.

If I was to make new part within the existing part using project curve, what will be the possible way to create new part as a separate model without removing its parameters ?

Thank you

Rodney

 

[JohnRBaker]

OK, while in the Assembly but BEFORE you project any curves or create an models, use the 'Create New Component' function to create your new part file, but just ignore the step where it asks you to select objects to be included in the new Component and simply hit OK. Now you've a got your new Component in your Assembly but there is nothing in it yet. Now set this Component to be the WORK Part and while this part is the WORK Part, you can go into Project Curve and when the dialog appears set the 'Selection Scope' (just to the Right of the 'Type Filter' widget) to 'Entire Assembly' and toggle ON the 'Create Interpart Link' icon (just to the Right of the 'Selection Scope' widget). Now create your projected curves and then create your features. Now when you save the New part file and your Assembly, the features in the new part file will still be fully parametric and they will ALSO be linked to the other models so that when they are modified your new model updates as well. Now if you DIDN'T want those interpart relationships, back when you were creating the Projections, while using the 'Selection Scope' of 'Entire Assembly', simply LEAVE the 'Create Interpart Link' icon toggled OFF. Your subsequent model will still be fully parsmetric, just that the the projected curves used to create your models will NOT be linked back to models in other part files.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA
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