3D sketch over-constraint error

[clamuro-IPEC]

I have a platform frame sketch where I am trying to add 45° braces to the vertical legs.  I get half(ish) way around the frame adding the 45s and then it starts giving me an over-constraint error when adding the angle constraint to the newly created lines.  I also can't add a length to the 45° line.

This sort of issue seems to arise when 3d sketches grow in size.  It would be nice if I were able to use the same 3d sketch for an entire frame without it bugging out on me randomly.  Frame generator using solids doesn't work well with the types of frames we typically make, so that option isn't practical.

I have attached the sketch in question. This is in Inventor 2017-R2.

[EvanGu]

Hi, could you please point out where you are going to add the line with 45° in a snapshot?

[clamuro-IPEC]

any of the exterior vertical members.  I was attempting to add an angle dimension between the two members shown in blue.

[SBix26]

I don't know why you're seeing the errors.  But I would suggest a different technique which could make your frame more robust, easier to edit, and would probably avoid these errors, too.

If I were designing this frame, I would be using a series of 2D sketches, probably starting with the top.  Add workplanes as needed, tied to top frame geometry and sketch legs and stiffeners on those workplanes.  All of that will be much easier to manage, even though the tree looks a lot more complex.

Sam B

Inventor Professional 2017 R2
Vault Basic 2017.0.1
Windows 7 Enterprise 64-bit, SP1
Inventor Certified Professional

[clamuro-IPEC]

Thanks for the suggestion.  I am aware that combining multiple 2D sketches is an option.  For this application, it would be a viable option.  For the vast majority of the frames I design, it is a much less appealing option.  The number of planes I would be making increases dramatically, along with the time it would take to draw the frame.

It would be nice if Autodesk fixed a broken component of their software instead of relying on their user base to find work-arounds.

[johnsonshiue]

Hi! I have seen this behavior before. This is model specific behavior. Usually, it means the constraint solver could not find a solution possibly due to implicit ground or multiple solutions. I need to take a look at the model in order to understand the behavior better. If you could post it here or send it to me directly (johnson.shiue@autodesk.com), I would like to take a look and get back to you.

Many thanks!

[clamuro-IPEC]

@johnsonshiue Model is attached in the first post.

[EvanGu]

Thank for your update information.

If you still want to create the frame in 3D sketch, try this workflow as the snapshot

1. locate your start point of the 45 degree line (I start from the center of the horizontal line segment in the snapshot)

2. click the orange plane, that means the line you are going to create will be in this plane

3. you will see 2 input boxes, press TAB to switch to Angle, input 45

4. press TAB, back to Distance input field

5. click the vertical line to snap on it

[clamuro-IPEC]

@EvanGu were you able to apply a length dimension to the 45° line?

[TheCADWhisperer]

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@clamuro-IPEC wrote:

Thanks for the suggestion.  I am aware that combining multiple 2D sketches is an option. .

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It would be difficult to convince me that (primarily) 2D sketches wouldn't always be the best option.

[clamuro-IPEC]

Coming from SolidWorks where the 3D sketch works, I feel like this is something that shouldn't be an issue.

I'm not saying using planes, 2D sketches and projected geometry isn't a more robust modeling technique (in Inventor).  However, if you have a frame with multiple off-shoots and awkward hooks/hoops, it is a much more time consuming process than simply putting them all in a single 3D sketch.

[JDMather]

I spend half my day in SolidWorks.

You would have a difficult time convincing me that it would be easier to do all 3D sketch rather than a couple or a few 2D sketches controlling my 3D sketch.

In the file you attached - it appeared to me that you are doing way too much work, especially if any editing (changing of dimensions) is required down the road.

[clamuro-IPEC]

I completely agree that this particular frame, which is atypical, is better served using 2D sketches and planes.

The error issue seems to be something everyone is glossing over.  @johnsonshiue said he has seen the behavior before.  I'd like to know the actual source of the error.

I'm not trying to be difficult.  I do appreciate the comments and solutions offered as alternative methods/better ways to make the frame sketch, but I am really more concerned with why this issue happens.

[johnsonshiue · Accepted solution]

Hi! Yes, I have seen similar behaviors before when constraint system is severely under-constrained. I took a look at this part but this case is different. I think I might have found where the problem is. There are 4 short segments overlapped longer segments. The coincident constraints are not applied appropriately, creating confusion to the constraint solver. Please see attached files for more detail. I am able to apply the desirable dimensions after I delete the overlapped segments and reapply coincident constraints. Let me know if you have any question. Many thanks!

[johnsonshiue]

Files attached.

[Anonymous]

100% agree. 

[SBix26]

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@Anonymous wrote:

100% agree. 

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With what? Or with whom?

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Sam B
Inventor Pro 2019.0.0 | Windows 7 SP1
LinkedIn

[Anonymous]

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@SBix26wrote:

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@Anonymouswrote:

100% agree. 

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With what? Or with whom?

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Sam B
Inventor Pro 2019.0.0 | Windows 7 SP1
LinkedIn

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Hi SBix26,

Thanks for reaching out.  I really appreciate it.

In a moment of frustration I was replying to clamuro-IPEC's comment on 31Oct2016 that having come from SW, this shouldn't be an issue.  I didn't realize my post wouldn't be filed underneath.

I also am coming from 12 years of SW with now 6 months of Inventor under my belt and, as unemotionally as I can put this, I find the 3D sketch environment almost unusable.  I'm a custom one-off machine designer and design custom frame weldments in all sorts of contortions for almost every project.  3D sketches in Inventor (2016) get inexplicably over-constrained; are undimensionable?; dimensions that were changeable all of a sudden are not;  there's no Equal, along X, along Y, along Z constraint; dragging under-contrained (green) sketch features to see what is still free almost never works; and half the failure error messages, of which I get plenty, have no constructive feedback as to what's wrong. 

I've been doing this for 14 years.  I used to fly through this.  Bottom line is now frame design stresses me out and significantly holds me back.  I've seen others post about only using 2D sketch planes but I find that a cumbersome, imo should be unnecessary work-around, and often impractical approach for my designs.  

At this moment I'm working on a relatively simple frame and just want to change the 12in dimension (circled in red below) to 49/3 or 16.333; file attached.  The dimension to the left that is now 16.333 I tried changing several times with no luck and then it just did it.  I tried to just repeatedly change the 12in dimension but can't get it to budge.  I'd love some help.  It seems so buggy.  Thanks for letting me vent a little.

[johnsonshiue]

Hi Tim,

This is a very good case! There are no overlapped lines or corrupted sketch constraints or redundant constraints. This is a case of too many degrees of freedom. I am able to avoid the error by grounding a point (see attached file; it is the lower-left corner in isoview). After that, all dimensions can be edited and there are no errors.

The question is why the point needs to be grounded. It may have something to do with the 3D constraint solver. Inventor 3D Sketch uses the same constraint solver as in Assembly Constraint. In Assembly, it is indeed preferable to have a grounded component so the solve result is more predictable. Although it is logical to have a grounded component or grounded geometry, the requirement is not apparent and not explicit. It is because sometimes it simply works fine without grounding, while sometimes it does not.

I will work with the project team to see if there is room for improvement.

Many thanks!

[Anonymous]

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@johnsonshiuewrote:

Hi Tim,

This is a very good case! There are no overlapped lines or corrupted sketch constraints or redundant constraints. This is a case of too many degrees of freedom. I am able to avoid the error by grounding a point (see attached file; it is the lower-left corner in isoview). After that, all dimensions can be edited and there are no errors.

The question is why the point needs to be grounded. It may have something to do with the 3D constraint solver. Inventor 3D Sketch uses the same constraint solver as in Assembly Constraint. In Assembly, it is indeed preferable to have a grounded component so the solve result is more predictable. Although it is logical to have a grounded component or grounded geometry, the requirement is not apparent and not explicit. It is because sometimes it simply works fine without grounding, while sometimes it does not.

I will work with the project team to see if there is room for improvement.

Many thanks!

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Thank you, thank you for your quick response, Johnson!  Fixing that point definitely helped.  I generally don't like leaving any sketch under-constrained and tried to constrain a few line midpoints to a plane in attempt to locate the whole sketch in space but got the same failure error.  I will fix a point on my first 3D sketch feature in the future.  

Thanks again for your support.