Component Added Without Bodies

[Anonymous]

I have successfully made a model with components. I have designed a component. When trying to bring this separate component into my model, it comes in but without the bodies. The component looks like a blue ghost when selected, when not selected it's just not there. What is going on here?

[Anonymous]

Where did the screencast go???

[xander.luciano · Accepted solution]

Hey There! Welcome to the Forums!

Quick note - I would recommend creating all your "part files" inside of one single file. I'm working on a writeup and video tutorial right now that I'll share with you to help you get accustomed to that. It's a better workflow with fusion.

But onto your real issue, on the front panel file, on the toolbar, click "finish base feature" then try it again!

Best!

[Anonymous]

And so it works now! Thanks for the fast reply. Somehow this needs to find its way into component creation. What is the significance of "finishing base feature"? I have read a number of articles on components, bodies, assemblies etc. but never once saw any reference to completing the base feature. What's interesting is I made another part (the main panel cutout that shows in maroon) and did not have to complete the base feature.

[Anonymous]

Creating all features in one file gets confusing. It also makes it more difficult to use one component in many designs because you have to remember what design you had it in...

[xander.luciano]

No problem!

Stuff like that is what I'm going to try and cover in my tutorial. Especially for solidworks users (I being one), the assembly workflow isn't identical. Though you can do it the way you are, you lose a lot of cool features doing it that way - and things can get confusing when it comes to moving bodies/components and then trying to edit sketches.

As per the base feature - at least the way I think of it - is that it's exactly what it's called. You create your initial geometry that you expect to remain constant with it. So if you are working on making saying an engine block, you could create a new component, then create a new base feature like this:

And the advantage is that you can create a fairly complex base feature without having it clutter the timeline. Then you can add features to the base feature after you finish it, but as you see below, all the extrudes and chamfer features I created in the base feature are not visible. Only the holes that I added after I finished the feature are visible.|



If you ever want to edit it though, you can right click the the "Base Feature" in the timeline, choose edit, and all your operations are right here:

So it's just a way to keep things a little more organized inside fusion without losing the design history. 

Also, the reason you didn't need to finish the base feature for the red part is because that part was made in the file that you are dragging everything else into. Instead of just creating a sketch and extruding it right off the bat, if you know you are going to be making an assembly I would recommend creating a new component first (this is like creating a new part inside solidworks) and then making all your sketches, extrudes, etc. in that component. Then when you are ready to create the next part, create a new component again, and then sketch in there.

Then your file tree would look more like this:



And the cool thing about that is you can reference the geometry from your other components! If you ever need to hide everything else, just right click the component you are working on and choose isolate. This will give you a clutter free view!

And lastly, by activating individual components you can further reduce timeline clutter. 



Note the difference in timelines



Well that ended up being a little longer than anticipated! But hopefully that gives you a good general idea. If it's a lot all at once, don't worry - I'll be doing a full tutorial that should hopefully make more sense.

Happy modeling!

[xander.luciano]

I will agree in the case of having a component in multiple designs then a separate file is better. Though components specific to a single assembly (I find) work best in a single file. Everything updates quicker, I still have a good perspective on what the whole assembly looks like, and I can visualize changes while editing sketches when I can see surrounding components. In the end it truly is all personal preference! There is no "right way" 🙂

Do whatever you like best! You are the designer after all.

Best,

[TrippyLighting]

The workflow Xander describes is part of Fusion 360's R.U.L.E #1 and you should follow the link and review it.

Usually a common or re-usable component originates in a particular design/assembly. My recommendation would be to finish developing the component in that dsdesign, unitil it really  is ready to be used in another design. Working with too many linked/external components can really slow the design workflow down and make it quite cumbersome.

The only current disadvantage is that when you export it that it will be a standalonde design and will not remain linked to the originating design. You'll basically have delete it in the originating design and then re-insert it. This will change as Fusion 360 develops.

Also, don't go overboard on cross referencing between too many components/assemblies. This can make designs very compicated and problems can be hard to track down and fix.

[Anonymous]

The Rule #1 video is great. I learned a lot from it, wish I had known about it before beginning. I've hit innumerable training video broken links. The main page http://fusion360.autodesk.com/learning/learning.html?guid=GUID-FB809CBA-4C97-4367-8E68-67B0483F81AF has lots of links, nothing to this. I'dl like to view the other training videos in this series. Please let me know how to find them. Thanks!