[Islam Abdelghafar]

I am working on CFD simulation of a wind turbine blade using STAR CCM+. I am using overset meshing; I made my mesh in Pointwise for the background (180 deg. segment with degenerate line "axis") and the blade (O-grid). Then I imported the volume meshes to STAR CCM+. I used sliding mesh technique to let the blade mesh (O-grid) rotate alongside two rotational periodic faces have a common line "axis". I checked the overset cell status and it was very nice as shown in the attached snapshots after switching the overset interpolation option from "Linear" to "Distance Weighted" as Linear gave an error when I initialized the interface. However, after one time-step (1 deg.), I got an error message telling me that 50 in-active faces are found in the background region. Do anyone here can help me to solve this problem ?

By the way, I set "axis" boundary condition to the degenerate line of the background mesh with the 180 deg. slice. Is that correct or not?

I uploaded some snapshots to help anyone to figure the problem out.

Thank you in advance.

[Islam Abdelghafar]

These two snapshots illustrate the error message after only one time step (1 degree of rotation)

[dmirel]

Hello Islam,

I had the same problems and fixed them following these steps.

For transient problems with moving bodies, set the time step such that the movement of the overset region within one time step meets the following conditions:
*When the time integration is set to the 1st-order Euler scheme, the maximum movement is the smallest cell in the overlapping zone.
*When the time integration is set to the 2nd-order implicit time integration scheme, the maximum movement is half the smallest cell size in the overlapping zone.

Hope it helps.

dmirel

[Islam Abdelghafar]

Hello dmirel,

Thank you so much for your reply. I am very grateful for your help. I agree with your answer but the problem in my case was in the definition of the motion as I have defined a motion for the blade mesh only. However, when periodic boundary conditions is employed, one should define the motion for both, the background and the blade.Now, the problem is solved after I set the motion to the background mesh too.

Kind regards,
Islam

[Marium]

MR. ISLAM,
I'm also trying to import volume mesh from Pointwise to star. The problem is I have no parts, so I can't progress further. I don't know how to go further. it will be helpful for me if you can guide me on how to progress after importing volume mesh in star.

[Islam Abdelghafar]

Originally Posted by Marium

MR. ISLAM,
I'm also trying to import volume mesh from Pointwise to star. The problem is I have no parts, so I can't progress further. I don't know how to go further. it will be helpful for me if you can guide me on how to progress after importing volume mesh in star.

Hello Marium ;

In my case, I haven't face any problem during importing my volume mesh from Pointwise to STAR-CCM+. I suppose that you choose your Solver in Pointwise to be STAR-CCM+ before exporting your volume mesh.

Hereby, I am attaching some snapshots for my steps from 1 - 5, I hope that could help you to solve your problem. It is supposed that every thing could work correctly after you followed the mentioned steps.

[Marium]

Thank you so much for your reply.
I have imported and run the simulation. The new problem that I faced is that i can not fathom the origin of the ship and that's why i can not set the isosurface for free surface view. As you can see, the free surface is quite lower than the draft line. 1.PNG
Can you share some insights on how I can change the isosurface in draft line? or how I can change the origin of the ship?

[Marium]

Mr hashem I am having negative volume problem when importing mesh from pointwise starccm+. After running 40 mins/252 iterations it shows error implying that there is non-positive volume cell and the expanded error message shows reversed flow and matrices problem. I have used the mesh diagnostic before running, it shows the mesh has no negative volume. I have examined the mesh volume component in pointwise too and it shows a few negative cells
Can you suggest me what to do?

[ping]

if you are using a flat wave to apply the vof physics then you simply change the point on the water setting to move the water level.
or you can transform the whole mesh in either parts or in regions.
i would recommend you should be meshing in star for any ship type cfd to make use of the special mesh refinement features

[kncujo]

Originally Posted by Islam Hashem

Hello dmirel,

Thank you so much for your reply. I am very grateful for your help. I agree with your answer but the problem in my case was in the definition of the motion as I have defined a motion for the blade mesh only. However, when periodic boundary conditions is employed, one should define the motion for both, the background and the blade.Now, the problem is solved after I set the motion to the background mesh too.

Kind regards,
Islam

Hi Islam Hashem,
I have a very similiar problem.
What do you mean by “define the motion for both”?
By assigning a motion to the background region, won’t it rotate together with the blade? I’m a bit confused.
I have a problem when the blade pass through the periodic boundary of the background region.