2022 OVER CONSTRAINED SKETCH WARNINGS?

[jchancegreen!]

This is my second day trying out IV 2022, and I seem to constantly get warnings after placing dimensions that my sketch is over constrained?  The problem is that they are clearly NOT constrained.  I can freely move the sketch in the picture attached, but as soon as I place a dimension it gives me that warning.  I started this skeletal sketch over this morning just to see if the bugs magically worked themselves out over night, but no luck.  Are other people experiencing this issue?  The sketch is attached as well.

[WHolzwarth]

Most of your geometry is already constrained, but visible only behind the lines.

Do that:

- Edit Sketch1
- Press F8 on keyboard
- Now constraints show up. Only lines with different color need additional ones or further dimensions.

[jchancegreen!]

I think you are missing what I am asking...I'm aware that most of my sketch is already constrained or defined, the question I'm asking specifically involves the image I attached in my original post.  If you open my layout sketch and go to the left side there is a "ridge beam tail" rectangle (shown in attached image), when I edit that sketch I can freely move and widen that rectangle (and endplate rectangle) about the center line of the building.  I have put a symmetric constraint so that the rectangle is always centered but I need to add a width dimension to fully constrain the sketch.  When I do this the program gives me the warning (attached image)  that "adding this dimension will over constrain the sketch"...I shouldn't be getting this message when the rectangle in question is clearly not fully constrained, otherwise I would not be able to click and drag the width of said rectangle, correct?

[WHolzwarth]

Hmm. I've seen this message only once. But now I could place a horizontal dimension and a vertical one for finished constraining at this region.

[JDMather]

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@jchancegreen! wrote:

 I started this skeletal sketch over this morning just to see if the bugs magically worked themselves out ...

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Can't you use Equal (=) Constraints (see Attached)?

[jchancegreen!]

The issue with this is that sometimes the ridge beam tail is not the same size as the other tail beams.  Does this not seem like a bug though?  Should it be giving me that message?  I can clearly still freely move the sketch.

[jchancegreen!]

I plan on eventually making a form so the individual member sizes can be typed in and the sketch will flex.  I need that tail width to be separate from others.

[JDMather]

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@jchancegreen! wrote:

 I can clearly still freely move the sketch.

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Try dimensioning this one (I didn't look deep into the issue).

Hmm, looks like one for @johnsonshiue 

[jchancegreen!]

That works just fine, what did you do differently?

[jchancegreen!]

@JDMather I did notice that in your sketch, you changed the end plate thicknesses to be equal.  If this was your fix to be able to dimension the width of the rectangle tail then it will not work for my particular problem...those plates will need to have individually controlled dimensions.

[JDMather]

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@jchancegreen! wrote:

That works just fine, what did you do differently?

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There is something fishy going on, it didn't exactly work fine on my second dimension.

That is why I pinged @johnsonshiue to take a look.

In the meantime - I recommend breaking this up into multiple sketches (Project Geometry appropriate reference points).

[DavidTunnard]

can you try dimensioning to the points at the end of the line? That worked for me.

[jchancegreen!]

That does work.  I've always been a subscriber of dimensioning to lines and edges instead of points when possible so there is less possibility of dimensions not controlling exactly what you want...but I'll take what I can get for now.  Thanks for the band-aid fix:)

[DavidTunnard]

Yeah me too. I tried a couple of other ways but haven't been able to get it to work by dimensioning between the lines.

No idea what could have caused it.

[DavidTunnard]

another way I got it to work was to remove the symmetry constrain and then add the dimension (d2) I then added a dimension (d1) to the centre line it wants to be symmetric about and always made that half of d2. Hope that makes sense.

[jchancegreen!]

That works as well...It's just a bummer that its throwing errors for something that simple.  Morale killer:)

[jchancegreen!]

@DavidTunnard @JDMather @johnsonshiue   Here is another head scratcher for me:  When I delete the same "band-aid" dimension as suggested by David, it all the sudden turns pink and gives me a warning.  Why would deleting one dimension in a fully constrained sketch all the sudden do that?  I'm not adding anything to it...at the most I would think it would just change the color of the sketch to show me it is not fully constrained anymore?

[jchancegreen!]

here is the dimension to delete:

[johnsonshiue · Accepted solution]

Hi! I see the behavior and I think I have seen it before. This is indeed related to symmetric constraint. In this case, there are multiple symmetric constraints applied. The problem with symmetric constraint is that it reduces multiple degrees of freedom. When the constraints are placed, the symmetry conditions are met. But, when you try to add a dimension forcing the sketch to solve again, the required degrees of freedom are not available.

Strictly speaking, it is a bug. But, the thing is that it depends on the constraint type and geometry. It is usually case specific. I don't think there would be a quick fix unfortunately.

Many thanks!

[jchancegreen!]

Well if there is limitations and bugs its good to know them.  Thanks for being honest at least:)