There are quite a few presentation that you can pull down on these, among others, to choose from “Solidworks world presentations”.
That said good file management is paramount is going to key no matter which method is chosen. Top Down, Bottom Up, or Master Model. Some tips to keep in the back of your head…
- Always overbuild and trim back to what you need.
- Better to build a whole surface then break it up rather than build pieces to create the whole.
- Don’t mirror if you can build the whole shape.
- Keep an eye on the “Performance Evaluation” to see what features are taking “a long time” to rebuild.
- “Enable the Freeze bar” (Systems Options---->General) but don’t just use this as a crutch for bad modeling techniques. Just because you can doesn’t mean you should.
- If you “have” to have a pattern of 1000 holes create it but make a configuration with it suppressed and an alternate version with a possible graphics texture version of it.
- Generally save fillets towards the end of the modeling.
- Use features and not sketch fillets if possible. A lot more levels of functionality and can always suppress/unsuppress features.
- Generally larger fillets first then smaller ones.
- File “Pack and Go”…this gathers up all files associated with the model, drawings, renderings…etc.
- Give names to features that are important. (we’ve all had extrude 15 at least 100 times and no one knows what that is)
Short and Sweet Snap shot…keep in mind you’re never limited to just one method. Any or all of these can be used in combination but generally not recommend if sharing with others or even for the sake of your own sanity and not creating circular references.
Master Model - one thing to consider is that you don’t have to just take the multi body model right into an assembly. You can also leave out certain details in that first master part file and insert the bodies into a second tier of part files and add the additional details there and then throw these into the assembly. Keep in mind that all dimensions with this method are contained in the master part file and not in the 2nd tier or assembly so if that’s needed for down stream then you’ll have to add in the drawing…possibly use some MDB if applicable. SW HQ would benefit greatly if they’d added this kind of functionality where dimensions can be added to the 3D model to drive it. There’s also no way to make a body within a part file “light weight” or “SpeedPak” which is huge in terms of making larger files easier to work with.
Top Down - Virtual Parts are “great” but confusing if you’re really not paying attention to if a file is or not. Upside is that one part files can drive one, ten, all or on an as needed basis. Generally not a good idea to reuse models made in this way unless it’s saved out as a different file name and all external references are broken. (once broken this can’t be undone). Because the other files can be loaded as light weight or even SpeedPak this “can” ease up on the strain on your CPU. But again KNOW what’s weighing down your computer through the performance evaluation, what you think it is and what it could be can sometimes be different. For ever external reference made just know that it adds to overall rebuild time.
Bottom Up- The most straight forward method. A lot of this is really product, company, and workflow dependent. Also downstream vendors consideration is always nice. Most “flexible” in terms of possible reuse of models in other projects and also for the creation of drawings if needed. Though the other models can’t be seen, once inserted into an assembly the ability to edit there is totally possible. (POKE POKE…hey SW HQ if you’re reading this, allow for more than one part file to be edited at once).
This really is only scratching the top of the modeling method ice berg but hopefully it’s a start…