topic Re: Error in Sketch: Dimension could not be solved. in Inventor Forum

Error in Sketch: Dimension could not be solved.

achintya_bhatnagar — Tue, 17 Oct 2023 09:11:02 GMT

I have this attached Sketch, and when I try to add even a simple line into it, I get this below error:

Problems occurred while solving sketch. Use Edit Sketch to change sketch geometry or constraints.
Dimension could not be solved. Change its value or remove some sketch constraints to allow the dimension to be solved.
Dimension could not be solved. Change its value or remove some sketch constraints to allow the dimension to be solved. [Repeated several times]

What is going on here?

Also, when I was creating this Sketch, I saw that when I used 'Mirror', a few lines used to turn blue even though the Sketch was 'Fully Constrained'. The lines turned back to black when I changed a few dimensions and they remained black when I changed those dimensions back to their original values.

Overall, Inventor seemed to behave a bit unpredictably when I work on this Sketch.

The overall dimension of this Sketch is in the range of 100 meter by 70 meters. Could it be because we are supposed to be working only on small parts (a few meters maximum, maybe) and not tens or hundreds of meters? This is a rail track layout. Would you recommend some other approach or another method for defining the layout of a rail track system?

Thank you!

Re: Error in Sketch: Dimension could not be solved.

JDMather — Tue, 17 Oct 2023 11:55:02 GMT

@achintya_bhatnagar wrote:

Also, when I was creating this Sketch, I saw that when I used 'Mirror'

In my opinion you are making this sketch unnecessary complex.

No need to use Mirror.

Does Manage>Rebuild All return any unresolved issues?

Edit: Also - I recommend modeling with symmetry about the Origin.

Edit2: It is best to work within a +_100 cube of the Origin, by working primarily in one quadrant you are approaching this limit.

Edit3: I haven't dug deep into this sketch yet, but I would not expect to see repeated dimensions like this in one of my sketches - especially the 14 and the 0.5 dimensions.

What are you attempting to model? Do you have a picture of something similar that already exists in the real world?

It is better to pattern (and Mirror is a pattern) features rather than sketch elements.

I suspect a thin feature or shell technique along with Mirror of Feature would dramatically simplify the computational efficiency of this design.

Also, iProperties would seem to indicate that you have not installed the Update for 2024.

As I start to reconstruct your sketch from scratch - the first thing I notice is a dimension that does not make logical sense to me...

Re: Error in Sketch: Dimension could not be solved.

achintya_bhatnagar — Tue, 17 Oct 2023 15:05:05 GMT

> What are you attempting to model? Do you have a picture of something similar that already exists in the real world?

I'm modelling the layout of a railway line track. It has two stations (the rectangles at the opposite vertical ends of 14 meter by 2 meters).

The three parallel curves (the dotted line in the middle of two solid black lines) going all around is the layout of the railway line. The dotted line in the middle is the centerline of the track and and the solid lines are the two parallel rail lines. As the track approaches a station, it branches out from the mainline and runs along the station for 14 meters, 0.4 mm away from it.

When the line curves (at the four corners and when the track branches out and merges at the stations), it first curves gently in a radius of 17 meter (the centerline radius of curvature) and then after some distance (as specified), the radius of curvature becomes sharper, at 8.5 meters. Since the two rails are 1 m apart, the radii of the curvature for them are 8 m and 9 m at sharp curves and 16.5 m and 17.5 m at gentle curves.

I will not be developing a part out of this sketch. The sketch is the visual representation of the layout. I have the square section pipes as part files, which I will lay out as per this sketch. I don't know at the moment how I will do it. So if you think that there is a better way for me to model a railway track of this shape and size, please let me know.

I first developed the lower left corner of the railway track layout. I then mirrored it to make the lower right corner part of the sketch. I then drew a horizontal line, as you show it in your picture (although vertical in your picture), at 45.837 m from the station side edge of the track, and then mirror the lower left and lower right part around that line to to draw the upper half to make the complete loop.

I hope this clarifies what you asked. I am still not clear how best to do this. Now the file has become practically unworkable as Inventor generates errors when I try to add new lines to it.

Thanks.

Re: Error in Sketch: Dimension could not be solved.

JDMather — Tue, 17 Oct 2023 16:09:14 GMT

Try the Attached file.

The key is to get within the +- 100 Meter of the Origin.

I converted the geometry to a Block.

Moved the center to the Origin.

I deleted some sick dimensions that you will have to re-establish if you need to Edit Block.

You might have to start over if you need to edit the sketch and it doesn't work. (For me this would be faster than digging deeper into the sketch.)

I would be sure to model with symmetry about the Origin.

All geometry must initially be created within +- 100 M of the Origin...

Re: Error in Sketch: Dimension could not be solved.

achintya_bhatnagar — Tue, 17 Oct 2023 20:01:38 GMT

Thanks to your reply, I learnt about the Blocks. They are a very useful feature. I am still exploring them. (I am trying to figure out if a particular instance of a placed block can be edited separately or how it can be flipped).

The blocks helped solved my problem.

Thank you!

Re: Error in Sketch: Dimension could not be solved.

johnsonshiue — Tue, 17 Oct 2023 23:45:15 GMT

Hi! The issue with invisible body when the profile is placed more than +-100m from the origin, is a bug in 2024. It has been resolved on our internal 2024.2 update. It will be available some time in November.

Many thanks!

Re: Error in Sketch: Dimension could not be solved.

achintya_bhatnagar — Wed, 18 Oct 2023 12:44:08 GMT

Ok, thank you for letting me know. I will keep this in my mind when designing.

Re: Error in Sketch: Dimension could not be solved.

s.bayat — Mon, 16 Mar 2026 10:58:08 GMT

Hey Achintya,

I have had this issue today with a small block gemoetry of a few parts sketched in a single block. It is drawn just near the origine. That was not the problem with my sketch. When you have a few part geometry with a random closed profile not perpendicular to the ground plane and drawn rectangeluar parts which overlapping the same boundaries, multiple boundry line on top of each other is the main cause. I solved it by adding the three side of the rectangle against the main part. That solved the problem. I have had also no constrain or dimensions errors.

I hope this helps you.

KR,