[AhmadHij]

Greetings,
I am new to this forum.
So I am working on a 2D transient simulation of a vertical axis wind turbine. I tried first to run the simulation at tip speed ratio (TSR 2.58). Things were fine, but when I moved to TSR 1, I am getting a very low results in comparison with experimental results in terms of comparing the power coefficient Cp. I am using the coupled pressure-velocity solver (it is pressure based type) so I noticed that in the solution control panel, there is a flow courant number that is 200 by default. I changed it to 1, and run the simulation. I got close results to experimental.
I then tried to change this Flow courant number to 0.5, I got different results than the 1 flow courant number case.
My question is what is the recommended flow courant number that can be used, and is using a 1 courant number wrong ?
thank you in advance.

[LuckyTran]

The recommended flow Courant number in the coupled pressure-velocity solver can be anywhere from 0 to infinity (it can be anything). It depends on what is your time-step size and "Courant number" that you achieve with this time-step size and number of iterations you perform per time-step to achieve convergence.

Without knowing the details of all these other parameters, I'm going to warn you that you need to make sure your results at each time-step are converged, because setting the Flow Courant number setting to 1 generally means you need 2x more iterations to converge in that time-step compared a Flow Courant number of 200. If the only change you made was changing the Flow Courant number to 1, that was probably not a good idea. And if changing the Flow Courant number to 1 improves the quality of your results, I instead recommend you to lower your time-step size and simply calculate more time-steps with the same Flow Courant number of 200 unless you have a mysterious illness that causes you to get cancer if you lower the physical time-step size.

[AhmadHij]

Originally Posted by LuckyTran

The recommended flow Courant number in the coupled pressure-velocity solver can be anywhere from 0 to infinity (it can be anything). It depends on what is your time-step size and "Courant number" that you achieve with this time-step size and number of iterations you perform per time-step to achieve convergence.

Without knowing the details of all these other parameters, I'm going to warn you that you need to make sure your results at each time-step are converged, because setting the Flow Courant number setting to 1 generally means you need 2x more iterations to converge in that time-step compared a Flow Courant number of 200. If the only change you made was changing the Flow Courant number to 1, that was probably not a good idea. And if changing the Flow Courant number to 1 improves the quality of your results, I instead recommend you to lower your time-step size and simply calculate more time-steps with the same Flow Courant number of 200 unless you have a mysterious illness that causes you to get cancer if you lower the physical time-step size.

I lowered the time step size (previous one was 0.25 degrees, new one 0.05 degrees) but I am still getting very low result in comparison with the experimental data. Once I set flow courant number to 1, It is giving me better results and also residuals are converging to 10^-3. So can I work with flow courant number of 1 or I am building my work on wrong setup ?

[LuckyTran]

Again... need to know a lot of things.

If lowering the time-step size did not help then lowering the Flow Courant number should not have helped unless your convergence is being limited be outer coupling. How many iterations are you doing per time-step? What is your Courant number?

I agree that lowering the Flow Courant number cause the residuals to be lowered, but residuals alone don't mean much. You need to check the convergence. If you've read the other thread, lowering the Flow Courant number is like lowering the underrelaxation.

If this is too difficult to understand then I suggest a more easy-to-understand scheme like SIMPLE.

[AhmadHij]

I am doing 20 iterations per time step which I think they are enough.
I checked the cell convective courant number, it is lower than 1 for both blades.
Results are fine at TSR=2.58 with flow courant number=200. But at low TSR=1, results are bad.
I tried the SIMPLE scheme, it also gave low results at TSR=1.
I dont know if the solidity of the turbine has an effect (solidity=0.265).
Dimensions:
Diameter =2
Chord=0.265
Number of blades=2
pitch angle=6
airfoil: NACA 0021
Boundary conditions :
inlet velocity=8 m/s
turbulence intensity=0.5%
Here are the main inputs that I am using.
The mesh is fine, I am using inflations layers to make sure y+<1.
So at flow courant number 200, I am getting cp=0.004 while experimental is 0.025 which is very different. when I use flow courant number=1 I get close results.
Thank you very much for taking the time in helping me.

[LuckyTran]

Hi, I get that you are freakin out that results do no match, but there is a laundry list to take care of before you can worry about that.

So 20 iterations per time-step... For a Flow Courant number of 200, at which iteration does the solution converge? 2, 10, 18, or never? Whatever is that number, multiply that by 2 and that's the iteration that you should converge at when you switch to a Flow Courant number of 1. Unless you were already converged after 1 iteration, in which case you might still converge in 1.

For a convective courant number of 1, you should be using using very large Courant numbers like 10000 or more. Lowering the flow Courant number will artificially lower the residuals and stall convergence because your flow won't advance in time and appear frozen.

[AhmadHij]

for a flow courant number= 200, It takes about 10 iterations for the residuals to converge, and at flow courant number of 1, it takes 20 iterations to converge.
I dont have issues at high tip speed ratios, My problem is when I go to low tip speed ratios.
In your opinion, what is causing this issue if I am sure from the mesh and I am using the same setup as the high TSR. The only thing I am changing is the rotational speed of the turbine and time step size.
That is why I tried to play around with the flow courant number and see how results are changing. What I understood is that setting flow courant number to 1 is wrong even though it is giving me better results, so what could potentially be causing the results to be so low when using flow courant number= 200 ?
thank you again for the help, really appreciate it.