F360 export errors in slicer - Adjacent component-bodies which are not merged?

[Lacathedrale]

I've been modelling an LBSCR Guards Lamp as my first project and had some success, where each major part (lamp, bulb, body, handle) are separate components. This works fine in Fusion360 and as I understand is the preferred method of creating designs of more than one piece -  but when I export as STL and then I import it into my slicer (Lychee) it shows up as containing errors.

 

I believe I know what the problem is: when component bodies are in contact with each other, they are both rendered separately with faces touching each other - rather than merged as a single entity. Because these are If I preview the slices I can see artefacts, as shown below:

 

 

If I pull all the bodies into a single component and then Modify > Combine before exporting to STL, then those faces are removed and the model imports fine:

 

 

If I import my STL into MeshLab and choose Cleaning & Repairing > 'Remove Duplicate Faces' then 'Merge Close Vertices' then 'Remove Mon-Manifold Edges' - the file also imports fine - but it feels like this has got to be a simple fix in F360 rather than having to either a) move all the bodies into a single component then merge them, or b) Rely on Meshlab to clean up the file?

 

Does anyone have any insight that might be able to help me, please?

[billbedford]

Are you using joints between the components? I've not had a case where components with  joints have failed.  

[Quarryscapes]

There is no error here, this is exactly how it's meant to be. If you want two touching bodies to become one, then you have to use a combine operation, otherwise you'd never be able to create moving assemblies of parts. However, it's also a none issue - it will print as one solid lump even if theoretically they are separate bodies as long as there really is no gap between them. 

[Lacathedrale]

Thank you @Quarryscapes - so basically in this case I should ignore my slicer’s protest?

[Quarryscapes]

Yes, you can comfortably ignore it provided the parts are touching. 

[Lacathedrale]

5 hours ago, billbedford said:

Are you using joints between the components? I've not had a case where components with  joints have failed.  

I am not - I'm using one component's sketch or body as the basis for another's -  presumably a rigid joint?

[billbedford]

That seems to be a very odd way of proceeding. The usual workflow would be either:

 

Have all the sketches in one component and join each body to the existing ones as they are produced. This gives you a single component with one body and mesh if converting to STL.

 

Have several components each, with its sketch(es) and join all the components with joints. This allows you to draw the sketches for each component at its origin. Also, components can easily be used in other assemblies. 

Edited October 12, 2023 by billbedford
typo

[TM2201A]

12 hours ago, Lacathedrale said:

I've been modelling an LBSCR Guards Lamp as my first project and had some success, where each major part (lamp, bulb, body, handle) are separate components.

 

 

 

 

 

 

Does anyone have any insight that might be able to help me, please?

That's a nice bit of modelling.

 

A few thoughts from 24 years of swearing at CAD software...

 

If for some reason sketch geometry fails to produce a new feature that intersects an existing feature most modern CAD systems will produce a new separate body; this can be useful in some circumstances (and is better than just throwing a fit and crashing like they did 15-20 years ago)  but can give rise to multi-body parts like you appear to have experienced. It's worth checking the model or feature tree/menu (usually up the left hand side of your screen) for the part to see if an additional body has been created.

 

As a tip model the part in its most basic condition first, so leave any tapering of surfaces, chamfers on edges or radii in corners until last; by doing this you can be confident that any geometry copied from one feature to the sketch of the next always intersects. If you think that a sketch edge may break away from the edge of a parent feature (for example if the feature is drafted) most CAD systems now have an option to use copy geometry with an offset which will force the system to understand that you want to merge the new feature and keep to a single body part.

 

Although it seems like tedium get into the habit of manually fully dimensioning or constraining each sketch, ideally to either the part origin or known fixed features such as the centre vertical axis or bottom face of your lamp; the discipline helps avoid wandering sketches that then produce errors or wacky features if something gets changed in a parent feature.

 

[Lacathedrale]

Thank you - I wasn't very clear in my explanation - but I understand what you're getting at!

[F2Andy]

I use Blender and Chitubox, so this may be different, and I am not sure exactly what the issue is, however...

 

After exporting the STL file, I always load it up in Microsoft 3D Builder. It will check for errors in the model, and repair them for you. Then save it - I suggest to a new file or folder that flags this is the repaired version. It can be slow with very complex models, but I have yet to have a model fail because of a bad STL files (plenty of other failures...).

 

It is free too!

 

 

[Lacathedrale]

Thank you @F2Andy - as detailed above F360 is doing exactly as I ask it (exporting the design) and Lychee is doing exactly as I ask it there (validate the model can be printed).

 

The error arises because Lychee doesn't know that my model consists of multiple components/bodies and so detects faces exactly against each other as an error, but the model actually prints out fine.

 

[billbedford]

On 12/10/2023 at 14:41, Lacathedrale said:

I am not - I'm using one component's sketch or body as the basis for another's -  presumably a rigid joint?

 

How many yellow squares do you have in the time-line?

 

[Lacathedrale]

Hi @billbedford I have three: one on the sketch for the handle, and on each of the two revolves for the lamp shade. I've not 'got to' assemblies yet so haven't looked at joints.

[billbedford]

I think it's worth going back to basics. Fusion is written for engineers and manufacturing, so if you wanted to produce a full-sized version of your lamp, drawings of each part would be needed as they would each be made separately and assembled. This is the thinking behind the components and assemblies in Fusion component can have their drawing for manufacture, and there can also be an assembly drawing. 

 

For modellers, all that is needed is a single file that can be converted to STL. 

 

I've had a go at drawing your lamp and put the f3d file on my Dropbox. 

 

https://www.dropbox.com/scl/fi/20blmenxg13cwvkaigyhm/Lamp-v1.f3d?rlkey=tah5pui6fv6wcushwttjg0b7e&dl=0

 

You should be able to follow the steps in the timeline to get an insight into a better way of working. 

 

There are two caveats in this file. First, I guessed all the dimensions and the fins on the lamp top are a hack. There is another way of doing these, but it's not intuitive and uses two sketches.