[i000e]

Hello guys,

I am currently doing a grid independence study on an underwater towed vehicle. My problem is that the value for the lift does not seem to converge when I increase the number of elements. The towed vehicle has two larger wings on the front side, which should permanently generate a negative lift. The following picture shows the basic system:

overview.jpg

The underwater towed vehicle has a total length of 600 mm. The mesh is constructed in such a way that face meshing is used on most surfaces of the body and a fixed element size is set on all surfaces of the body. The element size of the meshing is set to 0.2 m and the maximum element size is set to 0.5 m. The rest is all set to default from ANSYS CFD. Below are two images of the meshing (element-size of body set to 2 mm):

mesh_1_2mm.jpg mesh_2_2mm.jpg


To perform a net independent study, I varied the element size on the entire surface of the body from 10 to 1 mm in 1 mm increments and from 1 to 0.7 mm in 0.1 mm increments. Then I plotted the relevant values for the simulation, which is mainly the lift, against the number of elements from the entire mesh network.My expectation was that if I greatly increase the number of elements, then the relevant values will also converge. The drag seems to do that but the lift does not. Below is the graph of lift/drag to number of elements.

graph_lift_drag.jpg

For every single calculation there is a nice co convergence and the scaled residuals set to 10e-5.

What could be the reason that the values just keep decreasing (linearly) instead of converging? What suggestions do you guys have on what I can improve about the mesh network?

Best regards
Rasmus

[mluckyw]

I had encounter this problems with using Tetra as a volume mesh. Some of my question and suggestions:
Have you set an inflation layer for the boundary layer?
Have all of the residual converged to 10^-5 RMS wise?
How is the mesh quality after it is generated by ANSYS Mesher?
What are the settings of your simulations? (steady or transient, turbulence model, and so on) this also can affect your results

On my experience using Tetra with flow over a wing, my PC can not handle more than 15 mill tetra.
So I mesh it by using a structured hexahedral mesh (yes it took quite a long time with big learning curve), but the result speaks for itself. The hexahedral mesh converges nicely with smaller elements count than tetrahedral.

CL CD CY with tetrahedral mesh
CL CD CY with Hexahedral mesh

[i000e]

there is no inflation layer set at the moment. All of the residuals have converged to 10e-5.

The mesh quality is:
- orthogonal quality: 0.76613
- skewness: 0.23246

The settings for the simulation are:
- velocity 2 m/s (fluid: water, solid: aluminium)
- steady
- model: k-e standard

thank you very much for your opinion!

[mluckyw]

Yes I think you should add the inflation layer for boundary layer properties and maybe try SST as the turbulence model

[i000e]

Thank you very much, it seems to converge now. I added some boundary layers (theory: Frank M. White's Fluid Mechanics 5th edition, page 467) and stayed at k-e model