Configuring multiple instances of the same sub-assembly in different ways

[jorgmungandr]

I am trying to configure a top-level assembly consisting of multiple instances of the same sub-assembly. The sub-assembly in question has its outside dimensions controlled by a global variable in a way where I can change the length (the primary dimension) of the sub-assembly by changing a single value. I have tried to make multiple configurations of this part with different lengths. Whenever I put multiple instances of this sub-assembly in a top-level assembly and try to set them to different configurations, changing one of them to a different configuration automatically changes all of the others to the dimensions of that particular configuration, instead of just the one.



Am I doing something wrong, or are configurations not the way to achieve my goal? I have never worked with configurations before so there's a valid chance I am just doing it wrong... I was hoping to get a table/list where I could edit the variables of the different individual sub-assemblies in one place, but I have not found a way to achieve this yet. What I am trying to avoid is having to model and save different versions of the sub-assembly with different dimensions every time I need a specific size, as I sometimes need upwards of 25 variants of the same sub-assembly at once...



tl;dr I am trying to find a way to set different variables for multiple instances the same sub-assembly in a top level assembly, cant seem to make individual changes and just keep changing all of them at once.

[SPerman]

Are you using configurations in the part as well? The part needs to have a configuration that represents each length. And then each configuration of the sub assembly will reference the appropriate configuration of the part.

[Tom G]

There is another way to achieve this, in addition to configuring the part. Configuring the Part, without knowing other things about the design, is the more widely applicable solution.

If an object's length within the assembly is intended to vary with configurations, AND IT IS SIMPLE, then you can create the part as a virtual component saved within the assembly. This allows you to define its length with internal relations from the assembly, whether by sketch relations or by extrude to face or plane. The problem with this method is that you cannot control configuration specific properties for that part (or at least it is more difficult to represent). So, its body can have a length variable such as from a cut list of a weldment, but it does not get a unique description for each part length as needed to manufacture. This is why configuring the part to use in a configured assembly is a more thorough and widely applicable solution with additional advantages.

I do this often, because I do not instruct my assemblers how long a pipe should be. I tell them where it needs to go to, and provide them with enough to do so. It does not meet all needs to all users.

[jorgmungandr]

Thank you @Tom G and @SPerman for your replies. I did not know about having to make configurations of the parts within the assembly, I assumed making the variable that controls the parts configurable would do the trick. I'll have to look into that and do some experimenting. For now I think I'll try the "virtual component" trick, as the main parts that need to differ in length are basically just plates with some minor machining done at the end. The end goal here is creating STEP files to send to our supplier, no BOM required at this point. For context: I am the intern who was asked to see how we can get this all done more easily, and also the only person in the company who has ever used Solidworks before (even though I've never had formal teaching after getting my CSWA)...

For how easily/intuitively equations work I didnt expect it to be such a hassle to get this all done. I was really hoping to just get a list of equations for each part/subassembly that I could edit to my needs. I guess I'll keep dreaming, and keep learning. Any other hints and tips are much appreciated!

[TooTallToby]

Just adding on here - but basically saying the same thing:
Using traditional configurations, you can only have one geometric representation of a configuration loaded into computer RAM at one time.

If you want to show 2 different geometric representations of your part, whether its in a higher level assembly or in a drawing, each geometric representation has to have it's own configuration (using traditional configurations).