Losing body reference when changing a parameter

[vectorzero]

I've built a fairly simple model using a sketch and then extruding the features of the sketch.

When I came to modify one of those features, I seem to lose a stack of the other features on the model.

I'm not (to my mind) doing anything overcomplicated, but I must be breaking a dependency of which I was not aware.

I've created a video to show the behaviour here.

The model can be found here.

Can anyone tell me what I'm doing wrong?

[joel.palioca]

Hello,

Thank you for sending this through.  I am investigating with our team, but looking at things initially this should be in the realm of something Fusion 360 can do.  The failure looks to be a bug on our end where the sketches chosen for the cuts or extrudes aren't being picked up correctly after the edit.

While we investigate the problem, you can go through the extrudes that you have created and edit the feature and reselect the profiles that have gotten lost.  This way you can continue to leverage the file.

Please let me know if you have any additional questions, I will try and update things on here as we continue our investigation and any potential resolution that comes from it.

Cheers,

[innovatenate]

Can you try using the Sketch > Break command to break up the circle sketch entities in the profile? I suspect that Fusion 360 is losing its reference to an adjacent profile in the sketch upon being recomputed.

I will report this to development for further investigation, but for now...  Using the Break command to help break up the sketch entities from a single circle into small circular arcs may resolve the issue altogether for you.  I hope this helps. Let me know if you have any questions.

[gautham_kattethota]

Hi,

The extrude should not be losing one of its profiles when you make that dimension change to the sketch.  While we investigate why this is happening, you could try another way of changing the sketch dimension without having downstream problems with extrude.

Go to the Parameter table (Modify > Change Parameters) and under the parameters for Sketch1, change the "Diameter dimension-7" to the required value.  This updates your model properly.

Regards,

Gautham 

[jeff_strater]

I think this is just a bug in Fusion.  It should be a perfectly OK to do that edit and have the model update correctly.  We are investigating this.

In the meantime, you can repair the model, even after the change, by editing Extrude1.  This is actually the source of the problem.  Extrude1 should have two profiles selected, but after the edit, there is only one.  So, to fix it, just edit Extrude1, and select the missing profile.

Here's a screencast:

Hope this gets you past this problem until we can fix this.  Thanks for reporting it, this is very helpful.

Jeff Strater (fusion development)

[vectorzero]

Thanks for the very fast responses. I'll use the workaround. BTW there are more issues than just Extrude 1.

[gautham_kattethota]

Hi,

Please do let us know what the other issues you are experiencing are.  Do they all relate to features losing part of their profiles when you make sketch changes?  

Also, could you let us know whether you imported the sketch from some other software through a dxf/dwg file, or is it natively built in Fusion360?  We found that there are some issues in the sketch.

Thanks

Gautham

[vectorzero]

Hi

Extrudes 3, 4 and 12 are also disappearing. There may well be issues with the sketch as I'm still learning about the correct way to achieve the right result. Please bear with me!

Regards

Neil

[vectorzero]

Sorry

Forgot to say that this was created natively in Fusion 360.

[jeff_strater]

Hi Neil,

Thanks for pointing out the other failures - I did not notice those at first.  We'll investigate those, as well.  Hopefully they have the same root cause.

By the way, thanks again for sharing this model.  We have tracked down the problem with the first extrude, and have a fix for it.  It was not a case we had seen before, so you did us a great favor by reporting it. 

Thanks,

Jeff

[jeff_strater · Accepted solution]

I spent some time today with your model.  I think that the main problem with these features is some missing sketch coincident constraints, to make sure that the sketch profiles stay intact.

For instance, for Extrude 3,

here is what it is supposed to look like:

but, after the edit, this is what it looks like:

to fix it, I had to add some coincident constraints, and edit a couple of features:

Feature 4 is a similar story:

should look like:

but actually looks like this:

So, I had to do a similar repair job to add some coincident constraints:

after that, as near as I can tell, the rest of the design computes correctly.

Hope this helps,

Jeff

[vectorzero]

Thanks Jeff

I've looked again at the design, and I can see where I went wrong in not ensuring some of the lines were coincident on the arcs. On this basis I have accepted your answer as the solution.

I very much appreciate the time and effort on this issue, and I'm seriuosly impressed with the level of support Autodesk have for their products.

I think the other major issue with the issue is that I created one sketch to begin with and then extruded various features at differing heights. The final object is a decorative insert that will fit into a slot on another component. My method was to extrude all features to 1mm or greater, which implicitly creates a 1mm thick base to the object upon which all the other features stand. That way when its printed it stays as one solid piece.

Perhaps the smarter way to do this, is to create a simple sketch, extrude that to 1mm thick, and then sketch the additional features separetely on the new plane that I have created.

That way there is less likelihood of leaving a void, and the amount of geometry on the base plan is reduced leaving it less likely that I forget a constraint. I'm very much a beginner to 3D design, so being able to distinguish how to use the tools from what the best practice in their use is (for me) the tough part. As the former becomes easier, the latter can be more easily grasped.

I will try this differnt method and report back.