Normally when it's just a matter of hiding some components in certain views I'd recommend display states instead of configurations, but as of now you can't set a BOM to exclude hidden components. I'm always hesitant to use configurations just for hiding components because when a component is suppressed any mates that involve that component are also suppressed. Obviously, if other un-suppressed components are mated to the suppressed component that can cause problems.
You might try using display states, and balloon all visible parts in the drawing view. You can then expand the left side of the BOM to get the tiny balloon icons to show which components have balloons. Move all the other rows to the bottom and hide them.
Someone else may very well have a better option, but if not this might be worth a try.
Olivier Gandou wrote:
So I have this design, for which I have a detailed model.
I need to develop one set of drawings for this design with what I would call a low level of details. Some of the parts should not even be shown. I want to show a few key dimensions but not much... this is just to show the basics of the design. Let's call this set #1.
Then I need another set of drawings with a little more details (set #2). Some of the parts not shown on the previous set (#1) should be shown here. More dimensions should be shown... this set #2 will be used as basis for detailed design calculations.
Finally I need another set (#3), which will have the greatest level of details. Everything needs to be shown in this one. It will be used for fabrication of the design.
Optional: I'd like to develop one last set of drawings (#4) for a mockup of the design. Ideally it'd be based off of the same model the other sets are based on, but some features may be slightly different. Level of details to be somewhere between sets #2 and #3...
All of these sets should have their own BOMs of course, and the items not shown in set #1 for example should also be hidden in the BOM.
Definitely use configurations (but stay away from "Derived" configurations in my opinion).
If this is an assembly, then create multiple configurations with the parts that you DON'T want shown as suppressed.
If this is a part, then create multiple configurations with different features suppressed. (You will need to build your model with these suppression states in mind).
Then just create your 3 drawings and link them to the proper configurations.
Olivier Gandou wrote:
Using configurations? We use them at work but find them unstable...
If you are finding configurations unstable, I would like to know HOW you are using them.
Can you share an example of how they are unstable? It might be a simple fix or a workflow change that will make them more stable for you.
Applying multiple configurations in a large assembly that experiences frequent changes to the design has to be done very carefully. The configurations should be named clearly, and I recommend using folders to organize the components by their configurations if navigating in the model becomes a challenge. Eventually you're going to have a bunch of parts and subassemblies suppressed and hidden, and it's important to be able to discriminate between parts quickly if you use non descriptive file names, such as [product#]-XXX. If another person doesn't understand the structure of the assembly, then it's difficult, if not impossible, for them to predict the effects one change has over the entire assembly. The drawings could have unintentional changes in the views or the BOM. The user must also understand the options found in configuration properties because they affect how configurations behave by default or when they rebuild. Not understanding those options could lead to "Solidworks has a mind of its own" syndrome. It's also possible that the model may be passed to another user who is not that familiar with configurations, so it's important to be aware of how wieldly your cad models are especially if your assemblies are large and is shared between multiple users, groups, or even companies. You don't always have control over the competency of the users.
You could create multiple configurations or make three separate copies of the model to create three drawings. Of course, with the latter, you lose the advantage of being able to create a change in one assembly and having it propagate to all three drawings, but you have three relatively simple assemblies versus one potentially unwieldy one. Also three cad users can work on all the drawings simultaneously, which might be important to you if the drawings have to be developed in parallel. On the downside, if you have three separate copies, it will be more challenging to maintain three drawings. It's a tough decision.
Another thing you might consider with one model controlling three drawings is, are you ok with indirectly revising the other two drawings if one drawing is being revised? For example, if you revise drawing 1 and fix the broken annotations and dangling dimensions in drawing 1, should you fix the annotations and dangling dimensions in drawing 2 and 3 as well? Some companies require design change documents to drive changes in drawings and you can't simply make changes to drawings. Document control will also play a role.