[dancoelhoptr]

I was hoping for your help. I'm doing a multiphasic simulation with free surface of a Wigley hull. I started doing mesh convergence (comparing with experimental results) and when I do a finer mesh (maintaining the same mesh quality) the solver generates the "floating point error overflow", or it just converges from 1e-3 to 1e-8 in only one iteration which makes the results extremely strange.

I'm generating the mesh on ICEM CFD with hexaedral elems., SST turbulence model (in BC the turbulence intensity is 5%) and steady state. Here are the boundary conditions used:

-Inlet: Velocity inlet with Volume Fraction calculated with a step function;
-Outlet: Static pressure (hydrostatic pressure varying with coordinate z height);
-Top surface: Opening pressure with Entrainment option and pressure equals to 0 Pa. Pressure option: Opening Pressure. Turbulence: Zero Gradient.
-Symmetry

Initial conditions: Hydrostatic pressure varying with coordinate z height, Volume Fraction with step funcion and Velocity in coordinate x.

On Solver Control, I'm using High Resolution for both Advection Scheme and Turbulence Numerics. Volume Fraction Coupling: Coupled. And I tryed to change Timescale Control, to see if I could make the model convergence, but without success.

Here is the BC picture:
http://imagizer.imageshack.us/a/img913/3354/YieJiS.png

And the result for waterheight on the hull for the last mesh (you can see that the waterheight profile oscillates too much from 0.4 to 0.8 and I tried to get this better with a mesh convergence):
http://imagizer.imageshack.us/a/img537/3369/IPcDLt.png

And below the CCL file with the CFX-Pre options:

fig1.PNG

RESULT.png

CCL-file.txt

[ghorrocks]

Are you using double precision numerics? You will probably need it for the fine mesh cases.

Also: Are you running this steady state? Free surface models often need transient simulations to resolve the free surface perturbations as they have very little damping. Steady state cannot handle these very well with fine meshes.

[dancoelhoptr]

Thank you for your reply, I'll try to use that!

[dancoelhoptr]

Using double precision did work, but not for all meshes so, I raised the distance between the free surface and the top surface of the domain and changed the opening BC to free slip, and I don't have anymore convergece problems.
But, the waterheight profile remains almost the same even with a finer mesh.

Here is the waterheight profile:
figggg.PNG

I want something like this (someone knows the ANSYS wigley domain size or BC?):
ansys.jpg

[ghorrocks]

Those charts look pretty similar to me. What is not correct about it?

But now this sounds like a question on general accuracy: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

[dancoelhoptr]

I've seen that FAQ dozens of times already. From what I've seen, everything is correct and I already tryed a lot of suggestions from other posts and the results remain the same.

[ghorrocks]

When you are close but a bit off the expected answer there is no substitute but a careful analysis of all the key parameters. Have you looked at:
* domain depth, width, height
* free surface modelling parameters (smoothing etc)


And how much are you off by?

[dancoelhoptr]

What could you suggest for free surface parameters? I cannot find enough information on ANSYS HELP.

[ghorrocks]

All of them

I find the free surface model can be tuned for specific cases quite a bit, and some changes to the defaults can give significant improvements. But my method of finding the necessary changes is crude: Set up a quick benchmark case of your model and give every free surface option a try and adjust all tuneable parameters. Most will not do anything (so just leave them at defaults), some will wreck it, but a few will be a step forwards. If you have a good benchmark simulation and script all these permutations up you can run them quickly and sort out the ones worth investigating.

[dancoelhoptr]

I solved my problem. Now I am using Fluent with the following BC: pressure-inlet, pressure-outlet (in Fluent you can select pressure for both inlet and outlet BC in a VOF case because you set on the inlet a velocity for the fluid). For the external boundaries I am using wall BC.

The mesh must have numerical beach. The "numerical beach" is basically a very coarse mesh, with big jumps in cell size, near the external boundaries. It helps avoid wave reflection at the boundaries of your domain and therefore convergence issues. And now I get a smooth wave profile for the Wigley hull