2D Sketch No Longer Allows Any Modification Of Elements Including New Ones

[jaykinzie]

Hello Support Team,

I am having an issue where I can no longer make any modifications to a sketch. New elements seem to be having an issue as well. I have attached a video and the file in question.

Thank you for your time and energy!

-Jay

[dsouzasujay]

Hi @jaykinzie ,

Thanks for reporting this issue! Reported as FUS-80815 in internal issue tracking system.

Are you able to reproduce this bug in other existing sketches or just this one?

[HughesTooling]

This is a great example of why you should keep sketches simple, you have way too much going on in one sketch and you're overloading the sketch solver. The problem is caused because you have 2 Fixed lines at the bottom of the main rectangles, this really should flag as over constrained because your dimension for the top line in the rectangle can not change it's size because the other side is fixed.

When you unfix the 2 bottom lines you can add more to the sketch but it's painfully slow because there's too much info for the solver to work with. Also when you unfix the rectangles show unconstrained, they look like they should be constrained top the origin by there centre points but they are not. No way to actually fix this because again too much info to work with the sketch.

Keep your sketches simple, don't fillet in the sketch for the cut outs, keep the corners sharp and fillet the extruded body. An unfilleted fully constrained rectangle has 10 constraint, a filleted one has 26 and a lot more calculations need to maintain the 4 fillet rads. Make sure you sketch is fully constrained each time you add a feature, add a rectangle fully dimension it's position and size. Leaving stuff unconstrained is like building a house of cards, this sketch in more like a house of cards built on a table with rubber legs in a earthquake! 

Mark

[jaykinzie]

Yes I was able to reproduce this bug. This is actually the second version of this file I created because I encountered this issue while working on the first file.

[jaykinzie]

@HughesTooling@dsouzasujay 

I appreciate your advice of keeping things simple, but this really seems like something that ought to work correctly. I can accept that the software might operate slowly due to the number of constraints, but I don't think it is reasonable to dismiss this issue as a bug because the behavior is not correct.

Originally, I encountered the bug where when I would add or delete an unrelated constraint or geometry; The whole sketch would go unconstrained when I know it should have remained constrained. This might also be due to the solver being "overloaded". Reading the forums, the advice given was to go through the sketch and apply the geometry as fixed until it was constrained. This is why the lines on the bottom were set as fixed because it then showed the rest of the sketch as being constrained.

I see how applying the geometry as fixed might over-constrain a portion of the sketch, however, it doesn't seem reasonable for one over-constrained and unrelated portion of a sketch to prevent any further unrelated sketch operations to unrelated geometry.

So really we have multiple bugs here working together:

1) The sketch solver gets "overloaded". This sketch isn't really that complicated, and have made much more complicated sketches in the past with Fusion 360 and other CAD software packages; A 2D layout like this should be within the reasonable scope of the software. I am willing to accept that the solver might operate slowly which is another issue, but the solver having incorrect behavior as the complexity grows is not acceptable in a reasonable production context. In addition, the relationships are not overly dependent. For example I am thinking of geometric situations where there is a lot of tangencies occurring and changing a dimension might make the sketch unsolvable. This is not the case here. This is essentially a series of rounded rectangles that are just spaced off eachother's edges; there really isn't any magic going on here. Also this actual sketch is just meant to be a 2D layout which will become a dwg. Extruding and filleting solids is a very round-about solution to what should be a regular 2D problem.

2) The sketch solver shows elements as unconstrained when they really are constrained when an unrelated piece of geometry is added or removed. When this happened to me, I did the regular ritual of rebooting my computer to make sure it wasn't something related to the computer's immediate state. I also did ctrl-b to try to see if recalculating the sketch would solve, but that solution didn't work either. This led me to create the second version of the file where I encountered the same issue. At that point it became clear to me that this was a deeper issue and not a one-off. Being a software developer myself for my day job, I wanted to reach out to the Fusion 360 team to try to provide some good information on this issue so that you can improve the product in the future.

3) When the user applies a fixed constraint to the falsely "unconstrained" sketch, it then shows the rest of the sketch as constrained when in reality it is over constrained and then prevents further geometric operations on additional unrelated elements.

[jaykinzie]

@HughesTooling @dsouzasujay 

I am adding another video and file so you can see part of the root issue. I talk about it in the video. You can see how deleting some unrelated geometry is causing the main area of the sketch to become unconstrained.

Thanks for your time.

-Jay

[TheCADWhisperer]

Why all of the unnecessary repeated sketch geometry?

That is a lot of extra work?

I say - get lazy.  Don't do extra work.

[jaykinzie]

@dsouzasujay 

Do you have enough information to process this bug?

-Jay

[dsouzasujay]

Hi @jaykinzie ,

Yes, i have enough information, If required we will contact you.
I have passed the bugs that you added in the post.