Learning Forum

[joepa_2017]

I have a 2D model which consists of three layers. The layers are bonded together. I am applying a 3 displacement boundary conditions (ux = 0 at x = 0, uy = 0 at y = 0, and ux is variable at the right edge of the model) to simulate tension.

I want to use the mesh convergence tool in my results to make sure that my mesh is sufficiently refined. However, I get this error that I don't see how to resolve: "There are no candidate nodes or elements available for adaptive refinement. Check that results with convergence are not scoped to singular boundary conditions."

Any suggestions to resolve this issue and be able to use the mesh convergence tool?

Thanks

[Sandeep Medikonda]

Hi,

  Are you aware of the limitations of using the convergence tool? Please make sure that your model isn't following these limitations suggested in the help:

Note:

To use Convergence, you must set Calculate Stress to Yes under Output Controls in the Analysis Settings details panel. However, you can perform Modal and Buckling Analysis without specifying this option.

Convergence objects inserted under an environment that is referenced by an Initial Condition object or a Thermal Condition load object, will invalidate either of these objects, and not allow a solution to progress.

When performing an out of process solution asynchronously, wherein the solve may finalize during another Workbench session, the application performs only one maximum refinement loop. As necessary, you must manually perform additional loops. To solve with a single user action, solve synchronously.

Results cannot be converged when you have a Mesh Connection object.

You cannot use Convergence if you have an upstream or a downstream analysis link.

Convergence is not available when you:

Import loads into the analysis.

Activate the Nonlinear Adaptive Region condition in the analysis.

Convergence is not supported for:

A model with Layered Sections.

Design Assessment.

Solution Combinations.

Mixed Order Meshing

If the above suggestions do not help. Please reply with images of the analysis settings, model, error etc.

Regards,
Sandeep

[peteroznewman]

I prefer to have direct control over the element size so I can plot the mesh convergence data myself.

Regards,
Peter

[joepa_2017]

Do you mean, you simply run the analysis multiple times with, for example, twice the number of elements as the previous run?

The only issue I see with doing something like that is that it would refine the entire geometry instead of only refining locations of interest (e.g. curves) and could take a very long time to solve. I am certainly willing to do that. But, would the mesh convergence tool take into account that the mesh would not be uniform size for the entire geometry?

Or, perhaps equally useful, is there a way to refine a mesh more than what is allowed by the refinement setting? I have refined an edge with a refinement level of 3 (the highest level). If there was a way to refine the edge even further to look at mesh convergence, I assume that would be helpful.

Thanks

[peteroznewman]

The analysis is run multiple times, but the element size is reduce locally in the Sphere of Influence where the peak stress is located. The mesh is not reduced in size for the whole model. You can see and read about that in the link I provided above.

The multiple runs can be automated by using a Parameter Set that is created when you click the P button next to the element size input.

[joepa_2017]

I hadn't realized that there was a link. I will try to use that advice.