topic Re: Problem with imported solid components linked in Fusion Design, Validate & Document Forum

Problem with imported solid components linked

kltdave — Wed, 14 Oct 2020 13:18:39 GMT

I have a model with several components and sub components. This was imported from solid edge part and assembly files. When importing I selected the assembly and all parts that go with it. Import went fine model is correct with all components shown and listed in the tree as individual or sub components, just like I would have set it up if I was drawing from scratch in fusion.

My problem is the model has several components that are identical or mirrored parts and for some reason fusion has them linked together, for example I have 2 welded frames they are identical but represent 2 separate doors. They imported as 2 separate components (not a sub component), but I can't change one without the changes being automatically applied to the other. I don't see any way to break the link, It does not show linked anywhere? I can't share as this is a customers file and there is a NDA on this project. I have done enough work to this trying to get through that starting over would not be a option at this point. I have another file from them that was not imported yet so if it's something that can be fixed at the import level I have that option with that file just not this one.

Thanks

Dave

Re: Problem with imported solid components linked

jeff_strater — Wed, 14 Oct 2020 14:45:52 GMT

I understand about this being customer data under NDA, of course. What you are describing sounds like these components are instances of the same component. That should be the only condition under which modifying one will modify the other, because instances share the same geometry data.

By default, Fusion imports data into a Direct Modeling design. In your case, this is good, because Direct Modeling supports the "Make Independent" command on components. So, as long as you have not yet turned on design history, you should be able to select a component in the browser, right click, and choose "Make Independent" from the context menu:

This should create a new component with independent geometry.

Re: Problem with imported solid components linked

kltdave — Wed, 14 Oct 2020 16:17:34 GMT

Jeff,

Thanks, Looks like that is the problem. Unfortunately capture history is on for this project, and as frustrating as it is I think I can work around it. Unless you have a work around for after design history is on? I will keep this in mind going forward.

Is this a Fusion thing it does on import or does it have something to do with the file pre import?

Thanks for your help

Dave

Re: Problem with imported solid components linked

jeff_strater — Wed, 14 Oct 2020 16:42:39 GMT

there is no great work around, unfortunately. Make Independent is not available in a parametric design. The reason is: it is hard... I suspect we will get to it some day, but we are not there yet. Until then, the only ways that I can see to do this are:

Save Copy As. You can make a parametric copy of an individual component by selecting it and saying "Save Copy As". That mostly works, but there can be some lingering bugs in that approach. You should be able to avoid those, since this is an imported component, so should not have too complex of a timeline. Then, insert the copy, and use Remove on the original (you might be able to use Delete, depends on the design). But, then, you will need to repair any references (say Joints) that used to point at the old component, and point them at the new one.
Similarly, you can use Derive. You can Derive a new design which only includes that component. The difference is: Derive is associative, so will update with changes to the original (Save Copy As will not), and the result will not have its own timeline. The rest is the same as the above (insert the new version, fix up joints, etc)