Dimensioning and Constraint Problem Since Update

[docara]

Hi

Only just noticed this (v2.0.2383).

Just started a new very basic sketch to work something out and I'm in the process of dimensioning and added constraints. And something strange has started to happen.

If you notice in the enclosed Screencast I have an unconstrained sketch - all the lines are blue. I am unable to dimension or align certain parts of the Sketch even though no dimension value is showing. There can also be a long delay before a message appears (if at all) 

Interestingly, reviewing the Screencast the delay in warning messages appearing seems to be much quicker than in real life

 Have I missed something or has a bug crept in?

Matt

Screencast will be displayed here after you click Post.

f74b3012-2680-4b9d-9773-2d8ee6e28303

[TheCADWhisperer]

Why are you not using the Origin to lock down your foundation geometry?

I recommend sketching one line or one circle or one rectangle and fully define it immediately - do not continue until this is done.

I see a lot of duplicated dimensions in your sketch.

I recommend not duplicating dimensions, but rather either use equal (=) constraints or use Pattern (if appropriate).

I recommend creating Splines with as few points as possible.

I might use reference sketch points to visualize the scope of a curve, but these are for reference only - within the tolerance of the actual manufacturing process.

If I double click on some of your dimensions - I see magnitudes that cannot be measured out on the shop floor?

I recommend simplifying to dimensions that can actually be measured.

[docara]

Hi,

No this profile does not need to be on the origin. It's final position of the profile will be away from it, there are other things which will need to be on the origin. Also this profile is going to be mirrored around the origin.

If you notice in the Screencast I am trying to dimension the profile with reference to the origin but unable to do so.

This is a quick and dirty sketch from an onsite cardboard template, the levels of precision are only there because I tweaked the lines from the originals to match up to the spline. The Spline originally was constructed using only two points - beginning and end, an the nodes adjusted to best fit the original measured line values. As mentioned above the lines were just trimmed or extended to touch this new spline this is why you at seeing the values you do.

Other than for producing a basic cutting list nothing is going to be produced with machinery. 

Duplicating values is a fair point but as mentioned quick and dirty

[TheCADWhisperer]

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@docara wrote:

1. Because this profile is away from the origin, there are other things which will need to be on the origin 

2. If you notice in the Screencast I am trying to dimension the profile with reference to the origin but unable to do so.

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1. That is fine - I would have started with 2 dimensions to give absolute X and Y distance from the origin - just the way I work.  The two dimensions would lock the foundational geometry in position relative to the Origin and match my Design Intent.

2. I think you must have edited your original post.  Unfortunately with this new and improved forum experience rolled out several months ago  - editing a post causes loss of Screencast link.

In any case, I would start over from scratch.

Would you like for me to create example?

[docara]

Hi TheCADWhisperer,

Will repost Screencast

Yes I did edit my original - .....this new and improved forum experience is ..... an experience borderline annoying!

Thank you SO much for you kind offer but I'm fine - when I got home I only then realised I had forgotten to measure the distance from the origin when I constructed my template onsite, so I did the basic shape first with a view to locking it down later.

That not withstanding - I still should not be getting behaviour that I am seeing which is why I posted to the forum. The only thing I can think off is dimensioning values are either not being properly deleted or not being displayed properly. It is interesting that the lines which are misbehaving are the lines for which I interred values during the line command itself and NOT via the dimensioning tool.

As you suggest I am going to start from scratch to see if I can see a pattern for what is going on.

Matt

[jeff_strater]

@docara, you can still get the over constrained message, even if the sketch is not already fully constrained.  It just means that the geometries you picked for the dimension are already fully constrained with respect to each other.

I did not see the delay that you experienced, but I have a snazzy brand-new Mac, so it's probably not a fair comparison.  Are other operations slow, or is it just the dimension on that sketch?  I do know that it can take some time for the sketch solver to realize that the geometries are over constrained (it is usually slower than a valid dimension), but it should not be overly slow, in my experience.

[chrisplyler]

@docara  I know this screencast is long, but it will be very educational for you.

@jeff.strater  Please watch at least from the 12 minute mark to the 15 minute mark. A bug?

[docara]

Hi ChrisPlyer,

Many thanks thanks for the Screencast and yes I did watch all of it! I think it was good advise about locking a shape down to the origin whilst constructing it - I will steel that little snippet from from you my friend. And the other nice piece of info was the ability of locking down the handles of Splnes (something I didn't know)

For the record the horizontal construction lines were just that - lines to construct an approximate curve (spline) . 

Now, viewing my original Screencast I realised two things

1) Of the 2 versions I recorded I uploaded the wrong one

2) Because I was trying a few things out - to try to get things working before posting to the forum and recording the Screencast,  a number of the constraints which you suggested I hadn't reinstated, which probably threw you a bit of a curve ball. Sorry about that.  I certainly had vertical and horizontal ones present as those are my usual 'goto' ones before the any others. 

I have found the problem to be with coincident construction lines and Splines.

I have manage to do a Screencast with audio and you will see the issues I was having. My machine really struggled producing the video and encoding the audio so I'm afraid the quality is not good!

If you delete the construction lines from my original uploaded Sketch and add constraints and dimensions it becomes functional. You should be able to see on this Screencast why I originally posted fusion was pretty much inoperable.

Thank you again for spending the time sorting out the video for me , it was very much appreciated.

Matt

[jeff_strater]

Thanks for the screencast, @docara.  Very helpful.  I think there are two issues here.  1) the performance issue of adding a dimension to this sketch, and 2) the fact that those dimensions even return an error, and the general behavior of this sketch.  I think 2) is the more important issue, and 1) is probably related.  I think you have hit the issue spot on - the problems all stem from those horizontal lines.  It doesn't matter that they are construction - the same bad behavior happens if they are "normal" lines, and more, even if there is only one of them.  This is a solver issue for us to investigate.

here is my screencast explaining what I found out with this sketch:

[jeff_strater]

this is being tracked as FUS-42837.  Thanks!