[alimea]

Hi all

I am simulating "flow around a cylinder in Re=1-1000"

for divergence of velocity, which scheme is better?
I have used central, 1st order upwind and 2nd order upwind for that and I have gotten more accuracy (according to other numerical papers not experimental) for central!
for example for Re=100:

numerical paper: CL=0.15 and -0.15
central: CL=0.1461 and -0.1461
linearUpwind: CL=0.123 and -0.1293

thanks

[AliE]

Hello,

In my opinion a classical 2nd order scheme should work well, so i will go for central difference. LinearUpwind is equally good and usually more stable. In your case I will play more with the time step and the domain dimensions.

Good luck,

Alie

[FMDenaro]

Originally Posted by alimea

Hi all

I am simulating "flow around a cylinder in Re=1-1000"

for divergence of velocity, which scheme is better?
I have used central, 1st order upwind and 2nd order upwind for that and I have gotten more accuracy (according to other numerical papers not experimental) for central!
for example for Re=100:

numerical paper: CL=0.15 and -0.15
central: CL=0.1461 and -0.1461
linearUpwind: CL=0.123 and -0.1293

thanks

what do you mean for that??

[alimea]

Originally Posted by AliE

Hello,

In my opinion a classical 2nd order scheme should work well, so i will go for central difference. LinearUpwind is equally good and usually more stable. In your case I will play more with the time step and the domain dimensions.

Good luck,

Alie

Thank you
So your priority is central, after that linearUpwind.
Could you plz explain more about working on time step and domain dimensions? What's relation between these parameters and most accurate scheme?

[alimea]

Originally Posted by FMDenaro

what do you mean for that??

Divergence of velocity? I mean advection term of momentum eqn.

[FMDenaro]

Originally Posted by alimea

Divergence of velocity? I mean advection term of momentum eqn.

Ok, now I see (the divergence of the velocity is in the continuity equation).
Central (second order and higher) are generally better owing to the absence of numerical dissipation. However, depending on the combination with the discretization of the diffusive term, you need to have Re_h=O(1) to prevent wiggles. Have a look to the book of Peric and Ferziger.

[alimea]

Originally Posted by FMDenaro

Ok, now I see (the divergence of the velocity is in the continuity equation).
Central (second order and higher) are generally better owing to the absence of numerical dissipation. However, depending on the combination with the discretization of the diffusive term, you need to have Re_h=O(1) to prevent wiggles. Have a look to the book of Peric and Ferziger.

Thanks

Excuse me! I think st is wrong. the divergence of the velocity is in momentum eqn, in advection term.
According to your statement "Central (second order and higher) are generally better owing to the absence of numerical dissipation." you would ratter central scheme.
I didn't get " However, depending on the combination with the discretization of the diffusive term, you need to have Re_h=O(1) to prevent wiggles"

what are wiiggles?
Re_h is the same Peclet number?

[FMDenaro]

Originally Posted by alimea

Thanks

Excuse me! I think st is wrong. the divergence of the velocity is in momentum eqn, in advection term.
According to your statement "Central (second order and higher) are generally better owing to the absence of numerical dissipation." you would ratter central scheme.
I didn't get " However, depending on the combination with the discretization of the diffusive term, you need to have Re_h=O(1) to prevent wiggles"

what are wiiggles?
Re_h is the same Peclet number?

You are wrong. The convection in the momentum is the divergence of the teonsorial product of the velocity, that is a vector. The divergence of the velocity is a scalar.
For the other issues, you need to read the textbooks of CFD.

[alimea]

Originally Posted by FMDenaro

You are wrong. The convection in the momentum is the divergence of the teonsorial product of the velocity, that is a vector. The divergence of the velocity is a scalar.
For the other issues, you need to read the textbooks of CFD.

Ok, thanks

[AliE]

Originally Posted by alimea

Thank you
So your priority is central, after that linearUpwind.
Could you plz explain more about working on time step and domain dimensions? What's relation between these parameters and most accurate scheme?

Hello,

FMDenaro has provided you good advices, so follow them and read the textbook by Ferzinger and Peric .

yes, I will use the central scheme which is a standard option. My favourite for more complex problem is however linearUpwind which is usaully more stable (central is known to generate wiggles).

The time step is important since you are trying to capture the vortex shedding with a good precision, so put a constant time step, get the result, then divide the time step by two and perfom again the simulation to see the difference!

The domain size is important in measuring the Cd and Cl, that's why in literature you will find very large domains. This is due to the effect of the boundary conditions on the results (especially outlet!). Be sure to put your outlet far at least 20 diameters from the cylinder and use the advective boundary condition.

[alimea]

Originally Posted by AliE

Hello,

FMDenaro has provided you good advices, so follow them and read the textbook by Ferzinger and Peric .

yes, I will use the central scheme which is a standard option. My favourite for more complex problem is however linearUpwind which is usaully more stable (central is known to generate wiggles).

The time step is important since you are trying to capture the vortex shedding with a good precision, so put a constant time step, get the result, then divide the time step by two and perfom again the simulation to see the difference!

The domain size is important in measuring the Cd and Cl, that's why in literature you will find very large domains. This is due to the effect of the boundary conditions on the results (especially outlet!). Be sure to put your outlet far at least 20 diameters from the cylinder and use the advective boundary condition.

Thanks
1- please tell me the chapter that you point to (include wiggles, false diff and what you think that I should read). I have read some parts of Peric, Versteeg and completely Patankar.

2- Yes, I changed time steps and schemes seperately. these are the results:
for scheme study:
Re=100, Wi=80, residuals=1e-6, dt=0.01 :
As a result, I selected linear for div(phi,U) and Upwind for div(phi,tau).

for timeStep study:
Re=100, Wi=80, residuals=1e-6, div(phi,U): linear, div(phi,tau):Upwind:



As you can see, by decreasing the timeStep, lift coeff approaches to exact value but drag coeff's error increasd!
According to these values, which of these timeSteps do you select?

3-I know about the importance of domain size and put 25D from cylinder to outlet, 10D from cylinder to up and 10D from cylinder to down boundary. Is it enough?

[AliE]

Originally Posted by alimea

Thanks
1- please tell me the chapter that you point to (include wiggles, false diff and what you think that I should read). I have read some parts of Peric, Versteeg and completely Patankar.

2- Yes, I changed time steps and schemes seperately. these are the results:
for scheme study:
Re=100, Wi=80, residuals=1e-6, dt=0.01 :
As a result, I selected linear for div(phi,U) and Upwind for div(phi,tau).

for timeStep study:
Re=100, Wi=80, residuals=1e-6, div(phi,U): linear, div(phi,tau):Upwind:



As you can see, by decreasing the timeStep, lift coeff approaches to exact value but drag coeff's error increasd!
According to these values, which of these timeSteps do you select?

3-I know about the importance of domain size and put 25D from cylinder to outlet, 10D from cylinder to up and 10D from cylinder to down boundary. Is it enough?

1- In chapter IV Ferzinger's book explains both CDS and UDS for convection-diffusion equation. If you want something more "numerical", then I suggest you this book : "The Finite Volume Method in Computational Fluid Dynamics. An Advanced Introduction with OpenFOAM® and Matlab". This is not for beginners, but I have found it great, if the numerics is in your interest (see chapter 11 to 13 in particular);

2- Your results look ok. At the end of the story you are very near to reference's results and nobody is the holy bible so, in my opinion, your setup is good.

3- Domain size looks good.

I have forgotten to mention the non-orthogonal corrections. If your mesh has not a "O" topology, then put them at least equal to 2.

[alimea]

Originally Posted by AliE

1- In chapter IV Ferzinger's book explains both CDS and UDS for convection-diffusion equation. If you want something more "numerical", then I suggest you this book : "The Finite Volume Method in Computational Fluid Dynamics. An Advanced Introduction with OpenFOAM® and Matlab". This is not for beginners, but I have found it great, if the numerics is in your interest (see chapter 11 to 13 in particular);

2- Your results look ok. At the end of the story you are very near to reference's results and nobody is the holy bible so, in my opinion, your setup is good.

3- Domain size looks good.

I have forgotten to mention the non-orthogonal corrections. If your mesh has not a "O" topology, then put them at least equal to 2.

Thank you
The non-orthogonality of my grid is 14 degree. So I think that's ok and it doesnt need correction.