Create linked component out of a normal component

[Coscor_NPL]

Hi all

I'm missing the abbility to create a linked component out of an normal component... is it even possible to do?

workflow:

- open empty design

- create 2 seperate bodies

- right click body 1 and select 'creaty components from bodies'

- right click body 2 and select 'creaty components from bodies'

- now I want to open the component seperately, but can't... it needs to be a linked component for me to open it in browser or project browser OR to add that component to another design as a linked part

Which leaves me to my second question: how to make a new design and then add a component from another design (within the same project) to that new design as a linked component... in many ways, it's the same question...

Why?

because If I have made a complex tool design consisting of 100+ different components and need to make CAM on every one of them.

I would like to add the vice and possible the whole machine plan to the part that needs to be milled/CAM.

So if I open my 100+ design, and isolate a component and add a vice to it... in the end I would have a very cluttered 'tool design'

I really dont want my tool assembly to be dragged down by a lot of vices and mill lines...

In an old project I created a new file for every part, made an assembly and insert all of them, and therefore they were all linked parts in my big assembly.

from there I made a new file and dragged one of the linked files into it and also dragged the machine/vice into the design and saved the new design as 'CAM - Part xx'

BUT I want to use the 'new' way of designing with bodies directly in the design and all that, because I think this is maybe the 'new correct and in future smart way to do it' but as of right right now, it's just in my way with this issue...

unless somebody knows something I don't? 😉

[James.Youmatz]

Hi @Coscor_NPL,

I think I can help here! To put this in the simplest of terms, let's say you are designing a bicycle, and you create the frame and tires in it's own file within your project. Then you want to create the "assembly" of the bike, so you create a new model called bike. In here, you would insert the components for the frame and the tires (I will explain how in a second), and once they are inserted you can design things off of them such as brakes, handlebars, etc. So, the "new way" that you were describing can still be utilized here in that you have your basic parts that you want to leave referenced to its original file for efficiency, such as the frame and tires, so you create a new model, assemble it and then model based off of that. That is just one workflow, no need to take that as the exact way you have to do things!

To insert a component, expand your data panel. Here is where you would right-click the "tire" or "frame" model and select "Insert into Current Design" to get it to be referenced in your "bicycle" assembly (assuming that is the open tab in your model space). 

From what it sounds like you went ahead and created all the parts in one file and made them components, which is fine, but now they just all exist in that one file. If you want to isolate those and have them be their own separate file, you can just right-click the component in the browser tree and then select "Save Copy As" and this will create its own independent file of just the one component. From there, you can build an "assembly" model and insert that component and it is now externally referenced.

Let me know if you have any other questions!

Thanks,

[Anonymous]

Hmmm...First, you can link components by right clicking a file in your data panel (with the design you want to link the components to open and saved) and choose "insert into current design". If there are components in the linked file you don't need, use the lightbulb to hide them.

But for your wrokflow, the way you describe this is exactly the opposite to how I would do it. (But my workflow is also a little wierd).

You want to create all your parts in one file, then link them individually to seperate files? I'm not sure of how to do this besides linking the entire file and hiding the components you don't want.

It may be easier to create them in seperate files first, then bring them together.

Or to create a linked file just for your cam (this is what I do).

So, these two workflows would be:

- Create each component or component set seperately

- Create CAM in each file for each part

- Link together in one design (linking does NOT bring along CAM data)

Or

- Create all parts together in one design

- Link to a different design to CAM them all at once in one file.

Heres a screencast.

I show how you can -

1. Take a file with 2 components in it and import to another file for CAM operations only. You can turn on / off linked components for ease of use.

2. Import seperate components (with CAM data on them) and see the CAM part doesn't get linked with the component.

Let me know if this helps. Thanks!

[TrippyLighting]

I know precisely what you wnt to do and currently that's a little more complex than necessary. I've creatred an Idea in the Idea Station to get that behavior improved.

To export a component from a design/assembly you can highlight it in the browser and "ave as", which saves it as it's own independent copy in the data panel. That however does not automatically keep it linked to the current design. You would have to delete the components in your desirgn and (re) insert it into the design from the data panel. Then it'll be linked and changes to the component in the data panel will be refleced in the design it was linked to.

[Coscor_NPL]

Hi @James.Youmatz

Many thanks for the reply, really appriciate it, but I do not think this really help, I know of the 'save as' function (but then will loose referances) and also that I could make files first and then add them to an 'new assembly' but then i'm not really builing from the 'buttom and up' or the new way as i call it 😉 I would still have a lot of vices in each 'sub assembly'

Please let me know if I misunderstood something...

[James.Youmatz]

Hi @Coscor_NPL,

Ah, I see what you are saying now (thank you @TrippyLighting for the heads up! I see what he is trying to accomplish now).

Like he said, we don't currently have that functionality, I believe, of creating an in-model referenced file. His workflow of saving it out and reintroducing the piece into the model, would be the only workaround I can think of. Definitely give his Idea Station a vote (I know I will!) and hopefully we can get that implemented. 

Thanks,

[Coscor_NPL]

Hi @Anonymous

Thanks for the reply! I also used to do it this way (your way) making a lot of seperate files and then add them to a new big assembly, actually this is 'preferred way of thinking' since i have come from traditional CAD software like SolidWorks

But since Fusion is both 'buttom to top' and 'Top to bottom' I wanted to use this functionality, since it seems to be 'the way to do it' in the new way to design in CAD

But your post made me think that I could do a tricky mix or at least a variation of what you suggested... I could make a new file 'CAM - Part xx' and insert the whole assembly and hide all the parts I dont want... this does not affect the assembly and this also means that if I update the part in the assembly that it will update in the CAM file...

Thanks, I will try this, not as great or simple as it should be, but it can work... i think 🙂

[Coscor_NPL]

Hi @TrippyLighting

Thanks for you Post

Must admit, i'm not a fan of the 'save as' option because then i loose my 'design referances up to that point', but yes it seems to be the only 'clean' solution

Can you write a link to you solution here... because then I will defintly take a look at it!

a thing like this is needed to make both 'buttom to top' and 'top to bottom' design possible... as of now it seems like both are a little broken

Thanks!!

[Coscor_NPL · Accepted solution]

Hi All

After I read all the replies, I tried some things out, and it seemed to work out well, not the best solution, but it works.

1. made a lot of bodies in one file, saved it, named 'Design assembly' then made them all into components

2. made a new file, saved it, named it 'CAM of Design - Part A', and then inserted the 'design assembly'

3. Hide alle the parts I don't need, and insert the vice

4. mate it together and then it all seems to work out...

Thanks for all the answers, It has helped me to be able to continue this way...

[jeff_strater]

For what it's worth, this is on our list, although likely a ways out.  We call this "externalize".  The idea was to allow you to define components locally, then "externalize" that component to an independent design.   Which would be a "Save Copy as", but one where the local component is automatically replaced with a linked external component, all while maintaining references to things inside the component (sketches, bodies, faces, work planes, etc).  Harder than it sounds, though...

Thanks for the post, and the discussion.

Jeff Strater (Fusion development)

[Coscor_NPL]

Hi Jeff

I sounds great that you're looking at it at least... I can imagine it is more difficult to implement that me as a user can... well imagine 🙂

Sometimes it's just hard for the user to see if it's a design choice, a bug, a coming feature or just because seen as not important or not thought of or never used...

Thanks for the reply!

[Anonymous]

Has this been made a feature yet? I would love to be able to export components in to their own file but keep them linked to the original file.

[jeff_strater]

Nope.  Unfortunately, other priorities got in the way, as well as, this is a complex feature to implement.  It has bubbled up in the planning discussions again, but I'm not sure that will translate into actual delivery any time soon.  Sorry...

[TrippyLighting]

Well... I would disagree with about 15% of @jeff_strater "no".

You can derive a component of ut an assembly into its own files. That file will maintain a link to the component in the original assembly design. But just like everything, this comes some tradeoffs.

If you make modifications in that derived component they won't link back to the component in the originating assembly. etc. This is a pretty deep topic.

[Anonymous]

@TrippyLighting and how do you do that?

[TrippyLighting]

Create->Derive

[Murray.Industries]

This actually seems like the answer to the problem... at least as I read it and have my own use for it.  I had completely forgotten about this despite having learned it from Lars at one point... 

Thanks for the reminder!

[Anonymous]

Not really sure if this approach would work in all scenarios but this i what i do:

1. Make a sketch of the component you need to make in the main assembly file itself, taking in the dimension or clearance you need for that particular component.
2. Open a new file and copy paste the sketch you have made before in the main assembly file.
3. Create your component as a separate part and then insert it in your main assembly file

That way it stays linked and help you with the initial sketch of the component, you can also use "Edit in place" afterwards to refine the component in the main assembly file.

Hope this helps!