I have a problem with Ansys CFX. My runs aren't converging. I have attached a screenshot of a previous run.
Any ideas on how to resolve this?
I think it has to do with the mesh. Check the aspect ratio and the skewness.
Mesh transition from the boundary layer mesh to the volumetric tet mesh most likely leads to larger jumps in cell volume. Usually CFD solvers do not like that very much....
But this is just a guess. Inherent transient behavior of the flow in certain regions can be another reason for not leading to a converged (steady-state) solution. Would require more in-depth investigations and more information about what has already been done.
Regards,
Dr. Th. Frank.
Thomas Frank I had tried a double box with refinement in around the wing and the wake area. But this didn't work.
The growth ratio is 1.2 (as default).
I have uploaded the runs here: https://drive.google.com/file/d/1JN68Je-LS49mQktAuc3o3ke0jn_G3IfQ/view?usp=sharing
Thu Ya Win : 1.2 is the growth are within the boundary layer mesh from layer to layer. What I meant is the observable cell volume jump from the outermost prismatic cell of the BL mesh to the first tetrahedra cell layer on top of them.
Regards,
Dr. Th. Frank.
E.g. by using a different meshing method. I.e. ICEM/CFD Hexa to construct a mesh, which is entirely structured (hex).
In ANSYS 2020.R2 ANSYS SpaceClaim has a blocking mode for creating structured meshes (it is basically ICEM/CFD technology behind it, with a contemporary graphical user interface). But I have not yet used it.
With ANSYS Meshing one can only play around with bodies of influence and local mesh scales, which is not sufficient control in order to achieve a smooth volumetric transition.
But as I mentioned - inherent transient flow behavior detected by the underlying turbulence modle can be another reason for not converging solution. Not everything is or can be controlled by the mesh.
Design Modeler is a kind of a CAD program for geometry modeling. It does not has an own meshing component.
You can find out whether your flow is transient, if you run it for a certain period of time in the CFD solver in transient solution mode and by analyzing e.g. transient results (e.g. monitoring points for velocity/pressure over time and being placed in the wake of the airfoil or on its rear suction side).
How long should I run it in transient mode?
Also, what option in Space claim would block mode fall under?
Regarding Spaceclaim and Blocking Mode: There was only recently an ANSYS Webinar regarding this new exposed feature in Spaceclaim 2020.R2. You probably find it either in ANSYS Youtube channel or in ANSYS own mediathek. cannot repeat the 1 hour video here.
Regarding transient: depends on characteristic frequencies of vortex shedding (if there is such a transient phenomenon in your case). Not simple to be forecasted. Give it a trial.
Dear Thu Ya Win
Let me explain the foundation and why this is happening to you. In Ansys Fluent and CFX, the mesh non-orthogonality is a key in the convergence of results. It should be near to one, so what is non-orthogonality? it is the angle between the vector passing through cell centroid and the normal vector of adjacent cells share surface. It should be near to zero, to make cosine in dot product 1. however, in the diffusion term, the resultant vectors divide into two constitutional vectors, one is parallel with the straight line passing through centroids, and it goes to the implicit term for making the matrix of coefficients diagonally dominant, while the orthogonal term goes to the explicit part which increases source term value in Navier stocked equation and makes the solution unstable. in this order, we need to increase the parallel vector value by decreasing non-orthogonality between cells for giving many contributions to the implicit part and attain stability. Consequently, you may need to refine your meshing by a trimmer or hexahedral mesh method, while decreasing the skewness angle as well.
Then you may decrease the under-relaxation factor, to give higher weight to the previous values for stabilization. However, it must be noted you can make your run getting started with an upwind differencing discretization scheme after stabilization of results switches it into linear upwind differencing (second-order). For meshing, you can make use of Gambit and Ansys design modeler. Finally, more details about your simulation are required, if is it transient or steady-state? how much in the Mach number? which scheme are you using for the solution of the flow or velocity field?
Hope it can be useful.
regards
It is in steady-state with a speed of Mach 0.215.
The control is based off Britten-Norman BN2B Islander.
I plan to do a wing optimization study so I can't rely on the one-off mesh. Making a model, re-optimizing the mesh, and running will take a long time..
Any suggestions of how to speed this up?
- Badges
- Science topic
- Similar topics
- Biological Science
- Kinesiology
- Running