incompressible simulation steady state

Submitted by pcaste12 on April 2, 2012 - 04:36

Questions

Hi,
I am currently evaluating the PRO version, I am impress by the easiness of the product, I have build in a couple of ours what took me days using blockMesh!! Unfortunatly when I want to run ithe simulation it doesn't work
Warning:
volume_7 [www.1313.5] RANS Flow: Failed
Solver singularity: smoothSolver: Solving for epsilon, Initial residual = -nan, Final residual = nan, No Iterations 100

After 3.5 hundred simulations. My pressure is growing to billion of pa!!
Juste a question, is their a way to see all the model parameters and the initial data that are send to openFoam?

Many thanks,
Pierre.

Check mesh metrics

Submitted by symscape on April 2, 2012 - 07:59.

Have you check the mesh metrics? If not review "How do I fix mesh and solver failures?".

To see the entire OpenFOAM case setup, first initialize your simulation by requesting a flow field (e.g., Vector Fields->U) and then use File->Export, Save as type: OpenFOAM (*.ofm)

Thanks for your fast answer.

Submitted by pcaste12 on April 2, 2012 - 10:02.

Thanks for your fast answer. Yes I've reviewed the mesh (almost all parts) and it is all correctly defined. But I didn't try the relaxation factor..
Btw i will also review the export.
Pierre.

Correctly defined does not always equate to a good mesh

Submitted by symscape on April 2, 2012 - 10:22.

Correctly defined does not always equate to a good mesh i.e., your geometry can be topologically correct and the meshing tools can succeed, but the quality of the mesh elements can be poor. A poor mesh will then cause the solver to fail.

You specifically should check the:

Surface mesh element quality with Scalar Fields->E Ratio
Volume mesh element quality with Scalar Fields->Vol Ratio

If you find clusters of poor elements around a certain edge/face then you need to apply the Accuracy tool to either an edge or face in that region to improve the mesh.

I often find that modifying relaxation factors just delays the solver failures for a mesh with poor elements.

If you are confident that you have a good mesh then try setting Substance->Solver->Turbulence Model = K-Omega SST, if you haven't already, before you try modifying the relaxation factors.

Working on it

Submitted by pcaste12 on April 4, 2012 - 02:09.

Thanks again for your answer, and I can see that my sim (with very small relaxation factor) didn't work well (convergence after 5000 iterations), the results didn't behave as I expected.
I will try your suggestion.
Pierre.

E and Vol

Submitted by pcaste12 on April 4, 2012 - 03:51.

What do you think of having an E-ratio between 0.37 and 0.99?
And having a Vol-ratio between 0.12 and 0.82?
With no warning and "Tetulator: Complete: 1063954 elements"?
Thanks in advance.
Pierre.

Model and sim

Submitted by pcaste12 on April 4, 2012 - 09:05.

Many thanks, I reduce the number of cells to 142k and use the k-omega SST model, it converge faster (it is probably the fact that I didn't reduce the relaxation factor ;-) ).
I will move to compressible case.
Pierre.

Cell Values

Submitted by symscape on April 4, 2012 - 07:52.

I'm guessing the volume values are smoothed (node values), you want to examine actual cell values to view the cells, so for the volume you need to set the View Properties:

Style = Flat
Transparent = unchecked (off)

Then use the View Legend sliders above and below the color bar to focus on the lower quality elements - if they are clustered around edges or faces try improving the mesh there using the Accuracy tool.

Assuming you are satisfied your mesh is ok, then other likely causes of problems could be:

Substance->Properties->Reference values - do they reflect your case (e.g., U, Omega:Turbulent Length Scale)?
Initial Values - do you have initial values close to the main bulk of the flow? It maybe the Reference option for U isn't a good choice, so try specifying a Fixed Value
Boundary Conditions - are all your walls covered with Wall conditions? The most robust combination of inlet and outlet are the defaults, but are you sure the outlet is far enough away from flow gradients?

If you are still having problems then upload your Caedium project file (.sym) to a file sharing service, such as Dropbox, and use our contact form to provide a link so I can take a look.

Symscape