Where to find a list of unconstrained sketch elements

[rickseiden]

Hello,

I've seen this question asked before, but everyone gets into the specifics of the sketch in question.  I'd like to ask it at a generic level.

If Fusion 360 is telling me my sketch is not fully constrained, is there anyplace I can go to get an idea of what isn't constrained?

I don't have a specific sketch in mind, or a specific issue.  It's just that in the past I've had a sketch show that it's not fully constrained when all of the normal attempts at figuring out why have failed.

I know that black means constrained and blue means unconstrained and sometimes it can be tricky things like the endpoints that are the issue.  I'm hoping that someone can say, "Click on this menu, select this option, and a list comes up of what isn't constrained."

Thanks

[davebYYPCU]

I don’t know of any such utility or function, certain sketch checkers may have that function.

However, if you don’t have a red padlocked sketch icon, it is not fully constrained.  Things like spline and ellipse segments are difficult to fully constrain, but the other articles should be black, without white dots.

Might help....

[chrisplyler]

I've gotten so that I can pretty readily just look at a sketch and figure it out. But there is one thing that annoys me.

Why does a LINE turn black if one of its ENDPOINTS is still white? Sure, maybe one end of it is constrained, and maybe it even has an angle dimensions, or vert/hori constraint or something, so it's ALMOST fully constrained. But if that other endpoint is free, and thus the length of the line can vary, then IT'S NOT FULLY CONSTRAINED itself.

[TheCADWhisperer]

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@rickseiden wrote:

...in the past I've had a sketch show that it's not fully constrained when all of the normal attempts at figuring out why have failed.

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Next time this happens - File>Export and then Attach your *.f3d file here.

[rickseiden]

Thank you everyone for your replies.

I get when everyone is saying.  I know all about how to constrain it, and how things look.  It's frustrating, however, that when something has slipped by you, there is nothing that tells you what has slipped by you, and why.  And while I appreciate the offer of help, I shouldn't have to run to the forums every time some little detail is off in one of my sketches.  Experts would be spending years debugging noob sketches if that was the only way to resolve this.

After the switch in plans, I looked into alternatives to Fusion 360. Specifically FreeCad.  It was good, but it lacks some basic features that Fusion 360 has, and it is more difficult to use in most things.  It does have the feature that it tells you in what ways your sketch is not constrained.  It tells you in how many ways, and what exactly is not constrained.

If Fusion doesn't have that, it looks like a much needed feature request to me.

Again, thank you for your replies.

[jeff_strater]

@chrisplyler - starting religious debates again, are you?  Sigh...

First, I agree that it is misleading.  However, this is how all constraint solvers work.  They deal with infinite geometry.  A "line" is not a line segment, but an infinite line that happens to have 2 points constrained to that line, that the graphics system decides are the times to start and stop drawing pixels for that line.  So, from the solver point of view, a line is fully constrained when its direction is fixed and its position is fixed.  It cares nothing about those measly points that are constrained to it.  If they are free to move, that is a different entity entirely.

What I wish Fusion would do is to draw the points in a different color if they are under-constrained or fully constrained.  That would help.  Part of the problem, though, is we don't always draw those points (if they are shared by two or more lines).

So, yeah, it's confusing, but I think all CAD systems work in basically the same confusing way.

[chrisplyler]

Thanks Jeff. That makes perfect sense.

I would like to point out though, that we, the users, perceive ourselves, when we click on a starting point and then an ending point, to be sketching a line segment. The fact that Fusion only shows that segment, and not the infinite continuation of the line off both sides of the screen, reinforces this perception.

We perceive it as a segment. Fusion displays it as a segment. So it is not unreasonable to assume Fusion would also display its constrained condition as if it were a segment.

[ritste20]

I think this has been proposed before but I would very much like to see an option that shows/hides the unconstrained degrees of freedom for all sketch entities similar to how Inventor can display the red arrows.

Regards,

[wmhazzard]

Just a FYI Freecad does require 3 constraints on a line segment before it changes color. 

Go to the 8:00 mark in this video. https://www.youtube.com/watch?v=gbNg3mzm84s

[steveEQC6U]

This is the single most maddening feature of an otherwise spectacular piece of software.  I've spent *hours* even on simple sketches looking for the unconstrained elements.  I know about looking for the white circles and all that, but some of these can be really hidden.

Example: if I have a long line that's fully constrained, but a spurious smaller collinear line with disconnected endpoints, that spurious line - which was surely my mistake - is essentially invisible. I lost an hour on one of these this morning.

I'd love to see "animate unconstrained elements" feature that would wiggle whatever objects in whichever degrees of freedom are unconstrained.

Please?

[rickseiden]

I don't mean to say that FreeCad is better or worse at how it handles or enforces constraints.  But FreeCad does have a feature that tells you what isn't constrained.  Fusion just says the entire sketch isn't constrained. I was hoping for a feature that said what isn't constained so I can fix it easily.  I have started checking after every single action (where I expect it to be constrained), and if it's not, I undo it and try again, being more careful.

[mrakomo]

To be able to find the list of unconstrained items would be awesome.  I just spent 3 hours by searching no longer needed (unconstrained) construction line hidden under regular constrained line. And possible "zoom to the element" would be a really great feature. 

[jeff_strater]

I hesitate to expose text commands, because some of them can be dangerous, and are really intended for internal use.  But, this one seems useful enough that it's worth putting out there.  The command is "Sketch.ShowUnderconstrained".  This command will select any geometry that is under constrained.  Worth trying.

We are discussing how best to expose this capability in a more official UI.

[steveEQC6U]

YOU ARE A HERO! Thank you.

It seems this works only while the sketch is being edited - which makes sense - and the highlighting appears to be really subtle by showing a small circle endpoint on an unconstrained line that's under a fully constrained one, so one has to look really close.

I did figure out what was causing some of my unconstrained items: sometimes when drawing a line, a "single" line segment is actually like 1/8" of tiny segment at the beginning, followed by the rest of the line, and collinear without the intermediate endpoint jumping out at me. I don't know if I'm clicking funny - probably - but this has been incredibly frustrating.

Having this Sketch.ShowUnderconstrained is a YUGE win. Thank you.

[mrakomo]

This is a huge thing! Considering the amount of threads about this topic in the forums it may be a good idea to add this to the standard sketch menu.

[TrippyLighting]

No, it isn’t. In 6 years and thousands of hours using Fusion 360 I haven’t need that a single time 😉

[TheCADWhisperer]

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@jeff_strater wrote:

We are discussing how best to expose this capability in a more official UI.

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Here is how the remaining sketch Degrees of Freedom are shown in Autodesk Inventor Professional.

https://help.autodesk.com/view/INVNTOR/2021/ENU/?guid=GUID-B06FA7B7-5CD5-4D58-B1C5-0C5ABAFFD84E

DoF

DoF

Ah, finally got it.  This forum reminds me of the early days of Fusion.

Anyhow - I use this frequently in Inventor, perhaps because most of my day (thousands of hours) is diagnosing/evaluating the (unconstrained) work of other users.

[perisoratis]

File -> View -> Show Text Commands

On the bottom of the screen there will be a TEXT COMMANDS panel.

Go to the text field where it says "Type Text Commands Here" 

Enter the command: Sketch.ShowUnderconstrained 

[johan.rutgeerts]

I just have to bump this.  🙂

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@jeff_strater wrote:

First, I agree that it is misleading.  However, this is how all constraint solvers work.  They deal with infinite geometry.  A "line" is not a line segment, but an infinite line that happens to have 2 points constrained to that line, that the graphics system decides are the times to start and stop drawing pixels for that line.  So, from the solver point of view, a line is fully constrained when its direction is fixed and its position is fixed.  It cares nothing about those measly points that are constrained to it.  If they are free to move, that is a different entity entirely.

What I wish Fusion would do is to draw the points in a different color if they are under-constrained or fully constrained.  That would help.  Part of the problem, though, is we don't always draw those points (if they are shared by two or more lines).

So, yeah, it's confusing, but I think all CAD systems work in basically the same confusing way.

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Well, I know from personal experience that not all CAD systems work in that same confusing way, on the contrary.

I understand that the solver calculates with infinite lines.

But the solver does not decide about the line colour; the graphics system does. And the graphics system does indeed know the start and endpoint of each line, as well as their constraint status.

So the graphics system has all the info that is needed to decide if a line segment is fully constrained or not, irrespective of status of the solver's infinite line. So it's perfectly possible for the graphics system to draw the line segment in blue, even though the solver indicates that the corresponding infinite line is fully constrained.

The way partially constrained line segments are displayed in Fusion is the result of a management decision, and not the consequence of a technical necessity.

I think the importance of such details is underestimated, especially when scaling to larger design teams with multiple designers. It's already difficult to motivate everyone on a team to adhere to design rules (e.g. to ensure  that every sketch is fully constrained), and ever more so if the CAD tool adds to the confusion.

My two cents...

Regards,

Johan

[jjharbaughx]

I just started learning Fusion 360 and this command saved me hours of frustration trying to figure out why a simple sketch was unconstrained. Even as a learning tool this functionality is very helpful.

To fix my particular problem, all I had to do was "fix" one point and then the entire sketch was constrained (I know, rookie error). Using the Sketch.ShowUnderconstrained helped me figure out what I was missing.