Learning Forum

[Jan Walschewski]

I'm trying to simulate a vertical axis wind turbine using Dynamic Mesh in Fluent. However, the turbine barely moves and does not accelerate despite the moment being positive. The folowing pictures show this behaviour:

I put many hours into fixing this problem without success. I would be thankful if anyone has knowledge on this problem and is willing to share how to fix it. The following screenshots share details on my setup. If it is suspected that the problem lies somewhere else, I'm glad to share more information.

Geometry:

Dynamic Mesh:

Six DOF:

Fluid:

Run Calculation:

[mpowens]

Is the  rotation axis in the geometry/mesh at (0,0,0)? What is reported in the dynamic mesh form for the dynamic mesh zone "surface" after 0.4s. It should be reporting an updated rigid body orientation and angular velocity.

[mpowens]

Have you got a non-conformal mesh between the "rotating_space" cell zone and exterior cell zone? Have you specified a mesh interface at the cylidrical interface and top and bottom circular end caps? You don't need one on the bottom if it is at the bottom of the flow domain but I can't quite tell from the picture.

[Jan Walschewski]

The Geometry is centered at (0,0,0) and the orientation and anglular velocity are updating:

[Jan Walschewski]

I need interfaces on all sides and there are interfaces on all sides. I created the "rotating_space" and the exterior cell zone using boolean operations in DesignModeler. The interface was generated automatically and I assume they're good. Do you suggest adding them manually?

[mpowens]

If you put the solids in different parts in DesignModeler then the mesh will be non-conformal/disconnected between the parts which is what you want in this case. Ansys meshing will automatically create contact regions. When the regions are read into Fluent then Fluent will automatically create mesh interfaces for those regions. It should have worked. I guess you could try deleting the contacts from Ansys meshing and manually creating the mesh interfaces in Fluent. You will have to ensure that you have named selections set up for the faces on each side. Something strange does seem to be happening. The angular velocity should be higher based on the torque plot and moment of inertia. Is the torque plot for the torque on all the active rigid body surfaces and only the active rigid body surfaces? Can you add a picture for the report definition for the torque plot. Can you  add a picture of the rigid body surfaces? Are they all the surfaces inside the rotating_space zone or just some of the surfaces. If they are just some of the surfaces then there could be fluid drag on the other surfaces creating a counter torque.

[Jan Walschewski]

Manually creating the contact regions did not change anything. 

The torque plot should be only on the active rigid body surfaces:

"surface" is all the surfaces inside of the "rotating_space":

 

[Jan Walschewski]

I tried to set up the geometry differently so that the rotating space goes through the entire exterior space, without needing contact zones at the top and bottom. The turbine rotates much faster with this setup, but it still behaves as if a huge load torque is being applied, even though it should spin freely.

[mpowens]

It all looks good.  Are there any warnings in the console/transcipt when you open the case or run a timestep?  When running you should see reported "Updating mesh at time level N... done.". Any errors reported here?

In the main dynamic mesh panel do you just have Dynamic Mesh and Six DOF turned on? Anything else? If you have Implicit Updated ticked on it will significantly under-relax the motion and require many more iterations  per time step.

Is the Y-coordinate in the geometry also the Y-coordinate in Fluent?

Do you have any UDFs?

[mpowens]

Are you running in double precision? You should run in double precision.

[Jan Walschewski]

The "Updating mesh at time level N... done." is reported. There is not one warnings unless this is a problem:

It comes up, when I start Fluent.

 

Six DOF is turned on, Implicit Update is turned off. I tired it with and wihout smoothing, it does not changhe anything.

 

The coordinate systems line up.

I'm not using any UDFs.

Yes, I'm running in double precision.

[mpowens]

The message for the  sliding interface could be for the non-overlap wall part of the sliding inteface which in this case should be empty. Although I don't see that in a test case here.  For dynamic sliding mesh interfaces Fluent will create a  wall for the non-overlap region which can dynamically have faces added to it and removed from it over time.   I suspect in your case it will have no faces all the time. If you try to dsiplay it you should see the message "Creating empty surface".  What mesh interface method are you using? In Fluent 2025R2 the method defaults to one-to-one paring.  You can run the TUI command /define/mesh-interfaces/one-to-one-pairing? and it will report in square brackets what the current setting is. What does that report? You can right mouse click on the interface in the tree and sellect list to get a print out of the components of the interface. What does that report?

 

[Jan Walschewski]

List and Display are greyed out. 

The TUI command returned the following:

[Jan Walschewski]

Where do I define the mesh interface method?

[Jan Walschewski]

I just installed the 2026R1 Student version on my personal laptop. The setup was identical, and the simulation works perfectly there. The only difference I noticed was that the turbine was loading in along the z-axis, not the y-axis. 

[Jan Walschewski]

I need to get it working on my university PC tho.

[mpowens]

The mesh interface  in the picture is the many-to-many style of mesh interface which is not the default. The setting of [no] for the one-to-one pairing is not the default setting. Try changing it to [yes].  Instead of getting the list from the GUI you can get it from the text command /define/mesh-interfaces/list.

When you said the simulation works on the student version on your laptop with the axis in z,  I presume you changed the axis definition in the  rigid body setup or transformed the mesh. What does the mesh interface look like in the  laptop version? Perhaps the config settings are different on the university PC. They are likely to be at default for a brand new  installation. You can reset the Fluent configuration on the university PC  by  starting the Fluent launcher outside of workbench from the start menu, select the reset button, then close Fluent. You can also reset the Workbench configuration by deleting %appdata%Ansys. That has been know to get corrupted occasionally.  %appdata% when you type it in the address bar of a file manager typically resolves to  AppDataRoaming under your home folder.

[Jan Walschewski]

I tried setting one-to-one-pairing to [yes], nothing changed. I deleted configs in %appdata%Ansys nothing changed. I rotated the Geometry, so that the z-axis is the rotation axis and it finally works on the university-PC. This is a really weird problem, but at least it finally works🫠

[Jan Walschewski]

Thanks for the help, I learned a lot 👍