SolidWorks Assembly Question

Try saving each sub assy with a different name i.e. sub1: sub2......etc.Then for each new sub assy go to File Menu and 'Select References'. Then from the drop down menu 'Break all references'. This should disassociate all the sub assemblies from each other and you should be able to insert them one by one into the assembly.

Im not guaranteeing this will work but its worth a try

Regards, Cadman

If you break the references, your sub assemblies will not update when you make changes in the future. This is a bad thing, because then you will have to modify your total assembly all over again

You can do as the previous post suggested and create separate sub assemblies, or do as the error message said and make new configurations for the single sub assembly. The second option is generally the best because it only requires you to keep up with one subassembly file.

To do this, open you sub assembly and then, over at the feature manager, click on the configurations tab. Make as many configurations as you need subassemblies by right clicking and selecting "add configuration". There are options where you can make the colors, mates, and even suppressions apply only to a single configuration in case you want to make the flexible one a different color from the rest or you want to suppress components from only one sub.

Go back into the top level assembly and find one of the sub assemblies in the feature manager. Right click the sub assembly's name and I think you want to look for "properties" (right now I can't remember because I am not at a CAD station). This should be the same dialog where you can select to make the sub flexible. I think you can click on the subassembly configuration you want in the window. Do this for each sub if you want them to all behave independently or select a new sub for the one you want to be flexible.

If you decide to go the multiple file route (saving multiple copies of the same sub assembly), then in the main assembly right click one of the assemblies you want to replace, hit the double down arrows at the bottom of the menu to show more choices, and then select "replace entities". This should let you drop in a new assembly and as long as the files are similar it will translate the mates to the new sub.

I hope this helps. And in case this doesn't work, call your VAR and they should be able to walk you through it. That's what you pay them for anyway.

Thank you "Guest" (Post #2) for your very good reply. That helped me too.

Thanks for your replies. I'm new to SolidWork and the other 3D software I've used in the past allowed me to bring multiple sub assemblies in, independant of each other.

You shouldn't have to create multiple config's, Each part or sub-assembly inserted already has its own reference name when inserted this sounds like a problem with your software and I would either contact my SW rep or Solidworks themselve and get the problem fixed. From personal experiences, I have done as you are trying with no problems. When you insert a sub then right click on it in the feature tree and go to component properties and make flexible. Should work.

Yes each inserted assembly has its own reference name, but they are actually the same file. If you try to change one, it will change all the subs. Remember that when SolidWorks sees a change in an assembly, part, or drawing file, it tries to reconcile that in ALL references of that file. That is why it doesn't like the whole flexible thing when you have multiple instances of the same sub. If it was four separate files, then your comment would hold true. I've been through this and did ask a VAR about it.

This is actually a legitimate question, even if you're not new to SolidWorks. Here's my quick tutorial which is partially a restatement of several of the aforementioned replies. If you disagree with any of these steps, I don't care, this is how it works.

1. You will need a separate configuration for each instance to be able to make one instance flexible.
2. Open the subassembly in its own window.
3. Insert a design table with Auto Create selected. (It is just the fastest way, hands down).
4. If you have angle mates or distance mates, you can set up loads of different positions while you're in the table. If you are truly going for flexible configurations, then don't worry about the parameters, just create a bunch of configs. The names are not relevant, but must be unique.
5. Now, here's the often missed step. If you simply drag a component with your mouse, SW will attempt to move the same component in all of the other configurations if it is able to. Not all 3D softwares are smart enough to be ABLE to do this. SW gives you the OPTION to move only one configuration. To do this, you need to click on the Move Component button and select the check box under Advanced Options for "This Configuration." Should be self-explanatory. In case you're wondering, yes, you will have to remember to use this every time you move one of the components.
6. And I know you'll hate this step. Go back to the top level assembly and turn off Flexible Subassemblies. The issue here is that it is hard to use the function I stated in Step 5 when you're not editing the sub.
7. Instead of flexible, you can now use Edit Sub-Assembly from the top level assembly and you can use the Move Component command as I detailed in Step 5. You'll still need separate configurations so that you can choose which one is going to move. This should be better than multiple copies of the sub assembly, but that method is also valid (although not my first choice).
   

Hope this helps. If it is not clear, call your VAR and tell them what I've written above. If you are not current on subscription, then shame on you. If your VAR doesn't understand this, then shame on them. Either way, please log an Enhancement Request telling SW how you would prefer this to work based on your experience with other softwares.