Learning Forum

[erwin]

Hello, I have a question regarding this 3D streamline of my turbine simulation. To give some context, I have two domains, one stationary and one rotating (turbine). I did my meshing using Fluent Meshing and have no problems with the actual simulation. I've been trying to apply a streamline to see how air flows around the wind turbine, however when I do try applying a 3D streamline this is the result. It looks like the air flow is "avoiding" the wind turbine and not showing the streamline around it.

[KR]

Hello This is alright. Fluent meshing will recognize all volumes in your domain. This is the reason why you are seeing the 'Turbine' volume. If you don't need it in your analysis, you can simply mark it as 'Dead'.
Regarding the 3D streamline plot, is this a MRF simulation? Is this a steady run? When the streamline touches the solid walls of the turbine, the streamline should end. This is the behavior you should be seeing.
If this is a Fluent run, can you try plotting the pathlines in Fluent post-processing to understand the flow field? Can you also plot the velocity contour or vectors in Fluent to understand the flow?
Karthik

[Rob]

Can you check the surface between the turbine volume and the free stream volume. I suspect you have a wall there. In Fluent meshing there's an option to set fluid:fluid boundaries as walls, don't do that.

[erwin]

Hi Sir Rob, thanks for replying.
Correct me if I am wrong, but the option to set fluid:fluid boundaries as walls is found in the "Describe Geometry" portion of the workflow in Fluent Meshing right?
If I remember correctly, the option for that was to keep it as a "Wall" or convert the boundary to "Internal". I left it as a "Wall" since I am not that familiar with what Internal does. In that case, I would have to change it into Internal and see if it the flow changes.
Thank You!

[erwin]

Karthik. Thanks for clarifying my question regarding Fluent Meshing, I understand better now.
For the simulation, I was trying to do a MRF, and yes, a steady run. Regarding what you said about "when the streamline touches the turbine, the streamline should end" does this mean that I would not be able to see how the air flows at the turbine's outlet?
Lastly, I am doing the simulation in Fluent and have tried to plot pathlines on the turbine, but I get a similar plot of pathlines to the picture I posted above. As for the velocity contour, I Have also tried this but the flow does not make sense. I think it has to do with what Sir Rob mentioned about fluid:fluid boundaries being set to wall. Here is a sample velocity contour:
As you can see, I can't really assess the flow around the turbine. I will have to try changing the fluid:fluid boundary from Wall to Internal in Fluent Meshing to see if it changes.
I truly appreciate your input on this matter
Regards Erwin

[Rob]

Yes, you need to have it set for Internal. In the above image it's clear there's a wall in the way so no flow reaches the turbine. An internal boundary is a labelled surface in the mesh that doesn't have any effect on the fluid flow. If you didn't use inflation in the mesh you can just convert one of the wall wall:shadow pair to interior (near enough the same as an internal) via the boundary conditions panel in Fluent.

[erwin]

Thanks Rob and Karthik!
I have resolved the issue

[hinarani]

Hello erwin, apologies for bringing up an an already resolved topic but may I ask how you were able to resolve yours? I'm running a similar simulation with another type of spiral turbine and have run into this same issue.
I'm just doing a transient analysis. I set the rotating domain to dead zone and kept the turbine and outer domain as fluids as per this guide [CFD ANSYS Tutorial - Wind Turbine Simulation Using Dynamic Mesh and 6 DOF - YouTube] at about 53:08.
The construction of the geometry was a turbine made in solidworks, then brought to design modeler for creating a cylindrical rotating enclosure and a larger rectangular stationary enclosure. I did the meshing in fluent in accordance with the guide above (used face sizing on the inner rotating domain, generated surface mesh with some tweaking, no inflation layer, shared topology, polyhedral with growth of 1.4 instead of tetrahedral).
What could I be doing wrong?

[Rob]

You need to deactivate/suppress the metal turbine and bring in the outer & rotor volumes as fluids.