Method To Find Missing Constraints

[GoremanX]

I've done a search in these forums and come up empty. Other people have had a similar question before, but the answers were unsatisfactory.

I find that I spend a lot of time looking for missing constraints in sketches. It LOOKS like my sketch is fully constrained, every line is black, and yet the lock icon still doesn't show up for the sketch. This happens very frequently. Sometimes it's because of an extraneous point that's hiding behind another point. Sometimes it's because of a construction line way off the screen somewhere. Sometimes something is constrained "enough" to be black, but still have 1 degree of freedom that I need to discover by pulling on the right point at the right angle. Finding these things is a massive waste of time. There must be a better way than to yank every **** line and point in a sketch and hope to find the missing link.

Another issue I'm having is figuring out which constraint icon refers to which constraint. If I highlight a point, it can have multiple "coincident" constraints. But which one refers to the constraint that joins two lines together, and which one refers to the one that keeps a point locked to another point? So far, the only method I've figured out is to randomly delete a constraint and hope for the best, then if I picked wrong, click "undo" and try again. There has to be a better way...

In FreeCAD, I have a list of all my sketch lines in a pane on the left, and I can select each line from the list and figure out whether it's constrained and how. It also keeps track of how many degrees of freedom remain in the sketch, and allows me to highlight any or all of them with the push of a button. Is there something similar in Fusion 360 that I haven't learned about yet?

[shahriarsifat1802164]

Hi,
When your sketch is fully constrained it turns into black and you can not move your sketch. That's it.
Thank you.

[shahriarsifat1802164]

Constrained can be made by adding dimensions and relations. 

[shahriarsifat1802164]

You can see perpendicular or linear or concentric and other relations are shown on your sketch. I hope this would be your and for 2nd query.
Thank you.

[GoremanX]

Thank you for your reply, but unfortunately that's not helpful in this case. I already know those things, as I explained in my original post.

[etfrench]

Another way to narrow down the problem is to Fix/Unfix geometry until the sketch shows fully constrained. 

Another is to change dimensions to see what moves.

Fusion 360 really needs to address this issue.

[g-andresen]

Hi,

I don't know anything to that effect.
But I can understand that the desire for a tool of this kind is all the greater when one is always desperately searching for the culprit of an incompletely determined sketch.
But even if various people repeatedly complain about the missing constraints, one should not elevate their importance to a dogma.
Since I work with splines very often, I have gotten out of the habit of wanting to define them 100 % with constraints. In my view, such a definition makes no sense because splines are a means of visually controlled design.
If I am satisfied with the result in a "spline phase", I fix it (even temporarily).
Nevertheless, I would also welcome having such a tool, if it is not to the detriment of the workflow or the development of Fusion in terms of stability and functionality.

günther

[GoremanX]

My issue isn't so much with the desperate need to have everything constrained as it is about having a missing constraint wreak havoc later on when I change a fixed measurement and the unconstrained line causes a bunch of issues with the change (and all the components that were subsequently dependent on that line). I've had this happen so many times, especially on designs with dozens of complex components. It's infuriating. And my time gets wasted when I go back and try to find that culprit. I swear, hunting down missing constraints makes up a solid 25% of my time lately as designs get more complex.

I don't understand how a design software like this can allow us to define countless lines and constraints and yet not give us a list of all of them to keep track of everything. FreeCAD has its (very serious) deficiencies, but at least as far as this specific issue, it offers a much better solution. And it's free. I pay for Fusion 360...

[etfrench · Accepted solution]

I agree.  One should not have to guess at the properties like degrees of freedom, constraints, dimensions, xyz coordinates, fixed/unfixed, etc. of sketch items.  Using only colors doesn't work very well when you're color blind.

[GoremanX]

So what I'm gathering from this is that there is no facility to view these things? I was really hoping it was just a feature I hadn't learned about yet. This is really disappointing

[davebYYPCU]

While I agree there is no checker utility, and it could be better,

it is about having a missing constraint wreak havoc later on when I change a fixed measurement and the unconstrained (blue / orange?) line causes a bunch of issues with the change (and all the components that were subsequently dependent on that line)  

It's strange that the last change that you just made (breaking the model) can not be tracked down or even fixed with UNDO.  No timeline would be worse than with the timeline, do you use a timeline?

Could be your sketches are over complicated.  (No example yet)

We teach one sketch per feature for new people.  Very robust and easy to trouble shoot, but that dissipates with experience.

[GoremanX]

Of course I can undo. That doesn't pinpoint where the missing constraint is, especially if it's in another component.

So what you're saying is, my problem isn't an obviously missing feature (that's available in other design software), it's that I don't build my designs with this deficiency in mind? Now we're back at the beginning. Either waste time looking for missing constraints, or waste time restricting my workflow.

I mean, what's the point of parametric design if a sketch feature from 5 components ago prevents me from making a small revision. I literally cannot currently find the missing constraint that's giving me a headache right now. I've been beating my head against it for hours. It's the most basic sketch ever, there's nothing fancy about it, and the missing constraint is laughing at me. In FreeCAD, I could just click a single button and BOOM! There would be the missing constraint. But in Fusion 360, I have to yank on every line and dot like a monkey and hope I come across it by dumb luck.

This is stupid.

[davebYYPCU]

You are changing something.  It breaks something, and you don't know where to look, but undo fixes it.

However you have to have the change - one dimension, has two referenced articles, would be good place to start.

No file - Screencast or pic to allow us to assist, is - just text.

I think it's been said, could be better but for now it what it is.

[GoremanX]

That one specific instance I'm currently dealing with is not what this post was about. This post was about asking if there's a facility to find missing constraints, so that I can learn the software better. The replies imply that there isn't any such facility. The end.

If I had to depend on this forum to find a missing constraint every time this happens, my work would come to a standstill. I'll find it myself and learn yet another new method to tease them out... again. Why you're defending this is beyond me. If you feel like I'm belittling your beloved software and that insults you, I'm very sorry about that. This question has been asked and answered to my satisfaction. There's a missing feature in Fusion 360 that's present in competing applications. Whether you think that feature would be useful to you is a whole other issue.

[DaveGadgeteer]

I too waste time trying to fully constrain my sketches. 

There ought to be a tool to help us with this.

[etfrench]

There is😂  Open Text Commands.  Enter "Sketch.ShowUnderConstrained" without the quotes.  It's also not case sensitive.

[DaveGadgeteer]

It must be necessary to do something else to set it up?
I view a sketch, then enter the command:
Sketch.ShowUnderConstrained
and I get:
Sketch.ShowUnderConstrained
Traceback (most recent call last):

File "", line 1, in

NameError: name 'Sketch' is not defined

[davebYYPCU]

Edit the problem sketch, 

then run the text command, and the response will highlight where they are in the window.

Might help....

[DaveGadgeteer]

Aha, I hadn't checked the txt button on the far right, so it was set to python.
Now it works.
However, it doesn't offer any clues about which motions are not constrained, it just shows the offenders in color, which is what it does already in Sketch editing.
I'd like some clue as to motions that are still possible, something to help me figure out what I've forgotten.

[jhackney1972]

While in the sketch, you can use you left mouse drag on entities to observe the lack of sketch constraints.  This should give you a good clue as to the constraint you want.