I would like to know if any of you knows, for a fact, the answer to this:
Is it faster to rebuild and/or more stable (meaning less crashes) to draw, with one of the following methods
A- Work with baseparts
- Draw a bunch of sketches in your base part, and use them to define most of your part’s shape
- Then, insert the basepart into a new part, and reuse the original unabsorbed sketches defined in the base part, to create all the links and relations with the other parts of the assembly.
-This allows for parts that have literary no context defined featured or sketches, and everything comes from the basepart
B- Work with independent parts
- Start drawing one part
- When more parts come to the Assy, link the new part’s sketches to the sketches on another part (i.e, offseting, converting entities, etc)
- This makes parts that have lots of features that are defined in context…
Thanks all for your input!
Here’s the thing in either method chosen, the more external relations created across files, the more rebuild time and checking to make sure everything is “kosher” is going to happen. This can be somewhat offset based on the power of your computer (i.e. 64bit)
Also, doing drawings, if all dims are in the master file, then the subsequent “linked” or “children” files will not be used for drawings.
You can also do your layout sketches in an assembly file to start with, then insert new part files for each.
Stability wise…good file management, keeping external references in check (i.e. Keeping them to only necessary items and break others when not needed)
Hope this helps…
To reiterate part of what cadjunkie said, keep external references in check, as in keep them to a minimum. External references can be extremely powerful and a great feature, but they do complicate things and, as you know, make them less stable. They cause me most trouble on models that have a lot of rework or are otherwise in flux, which is unfortunately one of the times when they’re most useful.
As for whether to work with base parts or independent parts, I do both. Generally, if the parts have only a few areas where they need to reference each other I do independent parts. If I don’t need to severely link the parts, I won’t, just in case something with the design changes and one of the parts is eliminated, has to be totally rebuilt, highly modified, etc. If it’s really simple geometry I might not do any references. If the parts are relating in many areas and highly dependent on each other, especially if it is a surface that is going to be split (two halves of an outer shell, etc), I do a base part and split it. It does create a better tie, but that comes with always having to open and edit multiple parts instead of one. In the past I’ve used one base part to spawn most other pieces in the product, but that became quite a headache. However, I might consider doing it again if the parts were all very dependent on each other at areas of complex geometry, especially since SW has made improvements with managing their “Save Bodies” feature (esp. being able to relink to an existing file).
But either way, as cadjunkie said good file management is key. In SW making use of the “references” button when doing a “save as” can be useful.
This modeling technique you describe has been called Top Down design and has been used to develop products. Multiple parts with moving or non moving components alike can leverage ‘insert part’ functionality and usually require more than basic knowledge of surfaces. Post some pictures.