[Carlos_lboro]

Hello everybody, this is my first post in this forum so I'll try to be concise:

I'm simulating the near wake of a wind turbine by designing an actuator disc, in the simulation I have made the actuator disc as a subdomain porous medium with a momentum loss.
https://goo.gl/photos/1MSUACnsA8D1vZCt9
https://goo.gl/photos/e9bsYd3Si4SH4aBp7
That model worked perfectly fine, no issues there, but then I tried to make it a bit more complex by creating several concentric discs (or rings) each of those being as well a porous subdomain and with different loss coefficients because the energy taken form the wind is different in different parts of the wing.
I found out that the program was not able to calculate de solution, throwing at me an error 2.
Pictures of the second model:
https://goo.gl/photos/TLbbWVTYMZVSeXxTA
https://goo.gl/photos/szG4kNFt66aW75B16
https://goo.gl/photos/3dpiw3YEVVB5JQPe8

Thank you very much for any help or hints that you can give me.

[ghorrocks]

Your images are not attached.

But I do not recommend you use a porous model to model a turbine. I have never seen a wind turbine which looked like a sponge. You should use a general momentum source term for this, then you will have much more control over the source term.

And finally: If you are trying to model different amounts of momentum being applied to different parts of the wind turbine disk then I think you are pushing the source term approach too far. If you want to see the effects of different loading across the turbine disk then I recommend you model the wind turbine properly and get the full, complete 3D flow field.

[Carlos_lboro]

momenumloss.jpg

Is this what you mean by general momentum source?

Thank you!

[ghorrocks]

Yes, but do not use a loss model and a general momentum source at the same time. Remove the loss model.

Also note you need to correctly set the source term coefficient to get convergence - read the documentation on how to configure that.

[Carlos_lboro]

I have read this:

https://www.sharcnet.ca/Software/Ans...fxBasiMomeIsot

but it doesn't really clarify anything about convergence or correct values, it randomly throws a 10^5 coefficient that I cannot understand.

In this other one they talk about the convergence:

https://www.sharcnet.ca/Software/Ans.../i1300063.html

But I still can't understand the partial derivation of Sm vs U...

I'm sorry, I'm sure this must sound super easy for you but for me is a lot of fluids theory in a really short amout of time and with a very brief explanation by anyone.

[Carlos_lboro]

Doing what you said of avoiding the loss coefficient and just using the general momentum loss does not "take" any energy from the flow, therefore the velocity at both sides of my "actuator disc" are the same. Any ideas of what could have gone wrong?

[ghorrocks]

You will not get a velocity increase from one side of the actuator to the other as this does not conserve mass. Rather you get the flow accelerates into the actuator, passes through the actuator at a high velocity and then dissipates into the surrounding lower velocity fluid.

The source term coefficient is just there for convergence. If you are converging OK then you might not need it. Note the page you quote explains source term coefficients, but in section 1.3.2.1.1.

Have a look at the units of the source term and the units of the momentum your turbine removes from the flow. That might help you understand how they are linked together.

[Carlos_lboro]

Hi Glenn, thank you for your answer, it wasn't showing to me.

I want an actuator disc as a sink of momentum, I need it to drain momentum from the flow thats going through it and therefore change the pressure (and velocity).

I understood from the documentation and other forum posts that I have been looking at that the source term is only for convergence and that usually is a large number, in several posts I've seen used 10000-100000.

The units I get on ANSYS of the momentum source are [kg m^-2 s^-2] and the ones from the turbine are [kg m s^-1] or that is what I've found... But still dont get how they relate to each other.

I need to eventually get the thrust so I would need to calculate:
F = (m dot * V)e - (m dot * V)0 + (pe - p0) * Ae
being e the exit and 0 the undisturbed flow before the actuator.

Again thank you very much for your help, my apologies for being so slow learning this kind of things.

[ghorrocks]

Hi Glenn, thank you for your answer, it wasn't showing to me.

Can you PM me with what happened? I would like to know why my post was not showing.

I understood from the documentation and other forum posts that I have been looking at that the source term is only for convergence and that usually is a large number, in several posts I've seen used 10000-100000.

You are getting confused with the source term coefficient, but you mean the source term. I recommend for now you do not worry about the source term coefficient. Get the source term right first and see if you need a source term coefficient. Not all cases need a source term coefficient.

The units I get on ANSYS of the momentum source are [kg m^-2 s^-2] and the ones from the turbine are [kg m s^-1] or that is what I've found... But still dont get how they relate to each other.

If you divide the momentum source by the turbine figure you quote you get [m^-3 s]. That is the inverse of the volume flow rate. Hopefully that is a clue for you.

F = (m dot * V)e - (m dot * V)0 + (pe - p0) * Ae

You can simplify this. m(dot) and V is the same at the inlet and exit plane as mass is conserved. This means it just comes down the pressure difference.

[Edgar Alejandro Martínez]

Look at my YT video in which I generalized Erik Svenning's actuator disc. You can calculate the pressure drop in ParaView and the solver gives you the thrust.
https://www.youtube.com/watch?v=MbqbgGLJRso

Link to the solver: https://github.com/EdgarAMO/multipleDiskSimpleFoam

Link to the case file: https://github.com/EdgarAMO/actuator-disk-farm