Meshing wind turbine including tower in AutoGrid
 

Hello,

I'd like to simulate the complete wind turbine including tower. My idea is to use rotor/stator interface with two rows - one for the blade and another one for the tower. However, in the Row Wizard of AutoGrid, when I select the "Wind Turbine" for the blade row type, I get a message which says "Wind turbine wizard not available for multistage".

Is there a way to add a tower to a wind turbine in AutoGrid? Thank you in advance.

Instead of defining a row for the tower, I would recommend you to make the mesh for the blade with the outlet at the desired location of the rotor/stator interface and then to add the mesh for the tower as a 3D effect.

Hi Colinda,

Thanks for your suggestion. It sounds like a good idea. I'll definitely try that one and will let you know. What I've been doing up to now is using FINE/Open instead for the simulation by connecting the rotor mesh created in AutoGrid with the tower mesh in HEXPRESS.

Many thanks,
Shine

Meshing tower in AutoGrid5
 

That works as well and may be easier to set up. The only advantage of making it in AutoGrid5™ as a 3D effect would be:

• one template to run to get the complete grid

• a structured grid with an advantage in speed of calculation

• more control over the grid points distribution

Making it in HEXPRESS™ is easier to set-up and putting the meshes together can be scripted to counter the first advantage listed above.

With OMNIS™ all this will be even easier with the full integration of AutoGrid5™.

Best regards,
Colinda

Well noted and thanks a lot for that. Yes, it is easier to set it up in HEXPRESS but I'll also try the 3D effect in AutoGrid as the fully structured mesh and FINE/Turbo are preferred. I don't have OMNIS™ and I'm not sure if I have access to it.

Many thanks,
Shine

In the Admin Tool you can see whether you have access: in the License server tab click on the server name to see all the features. If there is a feature with OMNIS in the name, you have access.

For example, if you have an active free student license, OMNIS™/HEXPRESS is included. Meshes created in OMNIS™/HEXPRESS can be combined with AutoGrid5™ meshes and run in the FINE™/Open solver. The integration of AutoGrid5™ inside OMNIS™ GUI is not yet available.

Best regards,
Colinda

Hi Colinda,

Thanks once again for that. We have academic license here at our university. The license has been installed on the university server and our IT department is taking care of that. Anyway, I also have the student version on my computer, so I believe OMNIS is included. I'll certainly give a try.

Thank you very much for your help.

Best regards,
Shine

Hi Colinda,

I’ve decided to solve this in FINE/Open connecting the rotor mesh with the tower mesh in HEXPRESS. I’ve done two steady simulations – one with the rotor-alone model and the other one with the rotor-tower model. Please see the two figures below. In Fig. 1, with the rotor-alone model, the solution seems to have converged well in terms of residual and torque. However, in Fig. 2, with the rotor-tower model, there seem to be some fluctuations in terms of global residual on the finest grid but the torque seems to have converged well. Can I presume that the solution has converged with the tower as well?

Thanks in advance,
Shine

Attachment 71923

Attachment 71924

Dear Shine,

At first sight, the simulation with the tower seems indeed converged. You show the residuals for mass conservation, how about the other ones?
What does the convergence in the control points as defined in the Output page look like?

Best regards,
Colinda

Hi Colinda,

Thanks for your reply.

The simulations are run for 1000 iterations with the convergence criteria of -6. The residual which I’ve shown in the figure previously was Global Residual Fluid. It’s not actually Residual Continuity. However, Global Residual Fluid, Axial Thrust and Torque are the only monitor points added for Steering during the run, so I can only check those three. Please see axial thrust in the image attached, which seems converged as well.

I’ve quickly verified the pressure coefficients. It seems okay despite a little higher pressure noticed on the pressure side.

Do the residuals have to be smooth? Or, are the kinds of fluctuations seen in the Global Residual Fluid figure normal?

Thanks,
Shine

Attachment 71935

Dear Shine,

The "Global Residual Fluid" is based on the residuals of the mass conservation. You can change this (see the User Guide) but you can also look in the Monitor to see the convergence of the residuals of the other equations.

With control points I mean the points added in the Outputs page under the Advanced tab. Once you have defined such points, you can add an independent quantity like the pressure or velocity to the Steering and you'll see the convergence plot for this quantity at the chosen point(s). But this needs to be done before starting a computation.

Best regards,
Colinda

Hi Colinda,

I now understand what you mean. Thank you very much for that. I’ll have a look at them.

Many thanks,
Shine

Hi Colinda,

Having obtained the satisfactory steady state results, I’ve moved on to the next phase of the project which is to run a flutter simulation using modal coupling approach with NLH method. I’ve done that using the rotor-alone model in FINE/Turbo. The goal now is to run such an analysis on the complete wind turbine model including the tower which I’ve set up in FINE/Open. I’ve just realised that the coupling module is not compatible with the NLH method in FINE/Open. It seems that I have to give up on FINE/Open if I want to run the modal coupling simulation using NLH method. Would you have any suggestion?

Thank you very much in advance.

Best regards,
Shine

Dear Shine,
Indeed, the wind turbine wizard is limited to a single row.
However, you can perform the row wizard on the blades and, then, add a second row that would be your pylon. The pylon will be meshed as another row without any difficulty. For this, you can use the CROR wizard. The only limitation is that the height of the pylon will be limited to the height of your blade.
If you want to extend the mesh of the pylon further then I recommend you to create two projects: one for the blades and one for the pylon. They must have in common their boundaries. This means that the outlet of the blades should be at the same location as the inlet of the pylon project and, of course, the maximum radial limit should be the same but, for the pylon, you can set the farfield limit wherever you want. You even remove the farfield limit and only mesh the pylon between the hub and shroud curves but, in this case, the shroud should be at the same radius as the maximum limit of the farfield of the blades. Then, once you have generated the two meshes, you can import them in IGG and change the boundary conditions. For instance, you will need to change the outlet of the blade and the inlet of the pylon to ROT boundary condition. Do not forget to change also the boundary in the far field in order to have a full rotor/stator interface between the two meshes.
This two options allow you to generate the mesh of the pylon with the structure technology without manually defining the blocking in IGG or in a 3D effect.
I hope that I have helped you.
Best regards,
Alban

Hi Alban,

This is indeed very helpful. Thank you very much for that. This is also very similar to what I have done so far.

What I have done is – I meshed the blade row first with the outlet placed at the desired rotor-stator interface location, and then I meshed the tower separately in expert mode. Then I connected the two meshes (projects) in IGG changing the boundary conditions as required, and it worked. I’ve successfully run the steady simulation with that. The only thing I’m not entirely sure with this mesh is the grid distribution on the tower side (please see the close-up view of the rotor-stator interface on the tower side of the mesh in the figures below). I expected the grid to be equally spaced on the rotor-stator interface but I believe this is something to do with the solid boundary condition of the tower. On the other hand, this also makes sense that I need the fine grid near the tower to capture the flow around the tower. I also needed to activate the “Singular Line” option in the “Outlet Bulb Mesh Topology”. Please also have a look at the grid quality report of the tower mesh.

What you have suggested is also interesting to me and I’ll try that one as well. However, I don’t seem to know about the CROR wizard. Is that another wizard other than the Row Wizard?

Thank you very much for your help.

Best regards,
Shine

Attachment 72261

Attachment 72262

Attachment 72263

Dear Shine,
The CROR Wizard is just another wizard that allows to insert a far field region without the constraint to be single row. You could, for instance, use the wind turbine wizard for meshing the blade alone and, then, add a new row for the pylone and use the CROR wizard on this row. But, please, note that in this configuration, the shroud must be continuous between the two rows so the pylone cannot be greater than the blade.

Regarding the point distribution, it is highly dependent on your blade-to-blade mesh. In the attached picture, you will see the numbers of points that have an impact on your tangential distribution. You can also try the option "Relax Inlet Clustering" in the Mesh tab of the window "B2B Mesh topology control". This option impose an uniform point distribution at the inlet of the mesh. However, according to the distance between the leading edge and the rotor/stator interface, this can induce a low orthogonality.

Best regards,
Alban

Hi Alban,

Thank you very much for that. Indeed this has been really helpful. I adjusted the grid point distribution as well as applied “Relax Clustering” option for both inlet and outlet to have the uniform point distribution. The mesh seems good and this is something I wanted. However, the only problem is the low orthogonality as you mentioned. I have the orthogonality of around 1.3. Please see attached images for the entire mesh, the close-up view and the mesh quality report. I’m not sure with the mesh in the transition from the row mesh to the inlet or outlet. Do you think this will affect the results?

Thank you for your help.

Many thanks,
Shine

Attachment 72537

Attachment 72538

Attachment 72539

Dear Shine,
This is expected and, since there are located close to the inlet and the rotor/stator, they may disturb the convergence. Howver, from the pictures that you sent, I would say that you have some fixed Z cst lines. If you select a Z cst line, right click on it and select "Properties", you can access to different parameters of the Z cst lines. One of them is at the bottom of the "properties" window and it is a check button named "Fixed Geometry". When it is activated, AutoGrid5 does not smooth the blade-to-blade mesh downstream the Z cst line (if it is located downstream the blade) or upstream the Z cst line (if it is located upstream the blade). In the picture in attachment, you can see the difference. The upstream Z cst line is not fixed while the one downstream is fixed. Of course, some Z cst line are fixed and cannot be unfixed like the rotor/stator interface and the Z cst line separating the blade domain from the bulb domain. These Z cst line are used for splitting different domain for the mesh generation.
I hope that I have answered your question.
Best regards,
Alban

Hi Alban,

Yes, this is very helpful. Thank you very much for your help. Much appreciated!

Many thanks,
Shine