[androm]

Hello,

I am trying to do heave mode on airfoil using CFX. I used structure mesh using sizing and bias, I did make the bias too high in the y-direction to get the Yplus 1, however, when I do that it give me a negative volume in the solver or fatal overflow. How can I solve this problem?
I tried to increase the time step but still these errors come out to me. I tried increasing the coefficient loop instead of using 5 I used 7 and I even used 10 but It is still not working. I found out this is a common error if I used the mesh deformation, and the only way to overcome these errors is to make the first boundary layer far from the Yplus 1, If I used 2, or 3 I will be get result but the solution does not seem right compare to the paper that I am studying. If I used Yplus near 15, it gives me solution near the right result that is in the paper. Is there any explanation for that? I am doing laminar, and for heat transfer, I am using thermal.


Another question, I know if I used dynamic mesh option instead of mesh deformation, I may get better solution according to what I have read from several previous threads, Can anyone guide me with reference to read or tutorials that could help me?

Thanks In Advance,

AM

[ghorrocks]

I don't quite understand your question, but you appear to be getting negative volume errors when you have a y+=1 mesh but you are concerned about accuracy if you decrease the mesh size.

My comment on this is that you should not assume that you need y+=1. Many simulations run fine with a much coarser mesh than this. Also I would do some validation on a simple model before starting your complex heave model.

I would recommend you do a fixed mesh simulation of your airfoil shape and do a mesh sensitivity study. This will determine what mesh (and time step and convergence criteria) you require for an accurate solution. Once you know these parameters you can do the more complex heave simulation in the knowledge that your approach should be accurate. It might tell you a coarser mesh is OK, which means the negative volume element error you are currently getting is not relevant.

[androm]

Yes, I am concerned about the accuracy. When I did the steady state case to check the lift coefficient and drag coefficient, they seems have the same response even if I used Yplus 15 and not 1.
For the mesh Sensitivity (time step and convergence). For the steady state case, the residuals reach the convergence value (1e-6). For the time step, how to check its sensitivity.

I have attached the residual for the steady state and transient, the Cl and Cd convergence, and Cl and Cd during the heave motion, please, can you look at them and give me your feedback. Thanks.

[ghorrocks]

Mesh size - so it looks like you can use y+=15. In that case you won't get the negative volume elements error, so you don't need to fix that problem.

Time step - it is only of significance for transient simulations. You double or halve the tiem step and see if that changes your results.

Your transient results looks good so far. There is nothing obviously wrong there. But now the issue is to do sensitivity studies on anything you have not done yet (for instance time step size) to check that is OK.

[androm]

I did time step checking for the transient case, I used time step equal to periodic time divide by 100 and the other one is divide by 250 and they are almost the same, this means that time step has no effect if I used 100 time step, is that time sensitivity test?

Do I get the same result if I used dynamic mesh instead of mesh deformation?

[ghorrocks]

Yes, that is a time step sensitivity check.

There is no fundamental between dynamic mesh and moving mesh. When a new mesh is generated with moving mesh the previous step results are interpolated onto the new mesh, which is exactly the same process as dynamic mesh. The difference is dynamic mesh can be an entirely new mesh, whereas moving mesh is just the same mesh distorted a bit.

You normally only consider dynamic mesh when the motion is too large for moving mesh to work well on. If you are getting negative volume element errors this is a sign dynamic mesh might be a good thing to consider.

[androm]

I am doing low frequency in this case, but when I increase the frequency to higher value, I get negative volume, that means I need to use dynamic mesh. Please, can you recommend a reference to read or video tutorial to watch that could help me to do dynamic mesh for airfoil or cylinder or any shape? Thanks.

[ghorrocks]

There are dynamic meshing tutorial examples in the ANSYS customer page. I think they are under ANSYS workbench rather than CFX.

I don't think these examples are available in the ANSYS student page. Stuff this complex is beyond what they support for students.

[androm]

Thank you for your replies. I am doing my thesis and I need to learn this stuff to finish it so I will try to contact them and see if they have tutorial video or book for dynamic mesh.