Warning for reference failure should explain what constraint uses the reference

[jarkman]

This warning tells me the name of the point it *can't* find, but that's not useful to me in working out what to fix, since the point is no longer present.

What I need to know is what depends on that point. Perhaps the affected constraints or sketch objects could be highlighted when I click on the warning.

Even more helpfully, as it clearly knows where that point used to be, perhaps it could offer to recreate a suitable point for me ? 

There's also a mismatch here, where the warning refers to the point by name, but the rest of the sketch UI takes care to never show names of sketch objects, and (as far as I know) there's no way for me to set or see these names.

This would all be a lot easier to use if (eg) the selected object description in the bottom right of the screen could show the name of a selected object. it could also show the names of the objects involved when a constraint was selected.

[pawel.potyrala]

Hello @jarkman,

thanks for posting and for the feedback! I noticed that the following point is causing trouble:

Deleting the point and re-drawing the features that were centered around will allow you to get rid of the warning (see the fixed model here). While there is no direct way to follow the errors in the sketch geometry, which might make it problematic especially in complex sketches, the icons and the color coding for the constraints might give you some hints of how to proceed with the warnings.

In this particular case, it led me to the center points of the d12 and d36 circles. They were both fixed to a point from "base" sketch and cocentric.

I encourage you to post your idea in our Fusion 360 Idea Station - I'm curious to know how many users struggle with this issue.

Please accept as solution if my post resolves your issue, or reply with additional details if the problem persists.

Best regards,

[jarkman]

Paweł - thanks! 

So, to fix it, did you have to actually destroy and re-draw the affected circles ? You can't destroy and re-make the constraint ?

I'm afraid I find the constraint colour coding is not terribly helpful, and when a bunch of elements are co-located I find it utterly impenetrable. A bit of additional text added to the object description in the bottom right would go a long way to making this less painful.

Thanks again for your help, I'll go post in the Idea Station.

[pawel.potyrala · Accepted solution]

Hi @jarkman,

I admit I destroyed three of the d3 circles created with the circle pattern to make sure I do everything correctly. One circle (to the right) was left in peace. What I did after that is as follows:

1. Deleting the center point of d12 and d36 circles with all the constraints
2. Fixing the circle to the left side temporarily to prevent it from moving
3. Moving away both d12 and d36 circles
4. Adding coincident constraint between d12 circle and the point from "base" sketch
5. Adding concentric constraint between d12 and d36 circles
6. Unfixing the circle to the left
7. Creating the circular pattern with the d3 circle.

I hope it helps. Thanks in advance for posting in the Idea Station!

Best regards,

[jarkman]

Paweł - thanks - what a dance! 🙂

So, by way of feedback (I don't want to seem ungrateful for your help), this is a terrible, terrible experience for a new user.

I've done something slightly unwise, that I did not understand the unwisdom of at the time. And my content is all there, stuff is in the right place, it's pretty much done. Only there is this little warning, which it seems tidy to fix.

If the only solution is to delete and rebuild all the affected parts - not so many in this case, but this is a simple part - I'm going to be extremely discouraged. Throwing away work should be a last resort, reserved for disasters, not the only solution to a small error.

I'm not sure why Fusion 360 is so brittle, but I'm fairly sure it doesn't need to be.

[Anonymous · Accepted solution]

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@jarkman wrote:

Paweł - thanks! 

So, to fix it, did you have to actually destroy and re-draw the affected circles ? You can't destroy and re-make the constraint ?

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no need to destroy and re-draw -> break link to invalid reference and then fix the point -> see screencast (might take some minutes, Autodesk servers are pretty busy right now)

[jeff_strater]

@jarkman, just FYI - we have started work on a project that will let you re-associated any "sick" projected sketch geometry with a new entity.  While this may not address all of your concerns (it still can be painful to find which sketch objects are broken, especially if they are points), and it might not address your "new user confusion" concerns, it will help you fix broken sketches without having to delete and re-project new sketch entities, and all downstream references should be OK.  I can't promise exactly when this will be released, but rest assured, we see this workflow concern and are working to fix it.

Jeff

[jarkman]

@jeff_strater - thanks, that is good to know.

Just in case it helps, I feel like what I want to see is an informative list of sketch objects, a bit like the list of bodies. That would provide me a lot of context. I could see all of the objects that were present, see what constraints were connecting which features, see what each features was called, and select things in an unambiguous way.

I feel like the UI at the moment is trying very hard not to need that list, but the consequence is that many operations that should be very simple are needlessly obscure, and (to a new user) quite maddening.

That may be a very naive perspective, but it is what it looks like to me.

[jarkman]

@Manfred.Steinbach - thanks, that's a huge help. I would never have found that on my own!

Richard