[wchen]

Originally Posted by byrong

Hello Winson,

I assume you already got a proper mesh. However, to obtain a proper perturbation, I kind of cheated because I tried thousands of times using the perturbCylinder, and it did not work. In fact, the sine waves always became laminar. Therefore, what I did was the following:
1. Create a square channel with only two plates at the top and at the bottom which fits within the pipe you have.
2. Generate an initial perturbation using the boxTurb utility. Check a tutorial to use boxTurb first since the mesh must be divided in powers of two in each direction.
3. Run the case with the same velocity and viscosity parameters as the ones you will use in your pipe maybe for 5 to 10 cycles within the flow domain, or until you reach constant turbulence.
4. Once you got the turbulence map the velocity field of the squared channel to the pipe geometry with developed flow as an initial condition (both geometries should have the same length). To do this you require to use the mapFields utility, and create a mapFieldsDict within the system directory (there are plenty of tutorials of this online).
5. Run your pipe case. At the begining, the initial condition will look weird, but as long as the flow develops, you will get some nice turbulence. Run the case through the pipe domain for at least 10 complete cycles. Then use your last time step as a new initial condition, and run your case again for another 5 cycles. By doing this I got really nice statistics. Indeed, my statistics were very close to some DNS statistics that my supervisor gave me.

I hope it helps.

If you still need to use perturbCyl, you might have to write to Eugene de Villers, since he coded that utility, but in my case it did not work. And if you make it work properly, please let me know.


Cheers,

Byron

HI Byron,

Thank you for your quick and detailed reply. I will try your way and let you know the outcome later.

Have a nice weekend.

Winson

[wchen]

Originally Posted by byrong

Hello Winson,

I assume you already got a proper mesh. However, to obtain a proper perturbation, I kind of cheated because I tried thousands of times using the perturbCylinder, and it did not work. In fact, the sine waves always became laminar. Therefore, what I did was the following:
1. Create a square channel with only two plates at the top and at the bottom which fits within the pipe you have.
2. Generate an initial perturbation using the boxTurb utility. Check a tutorial to use boxTurb first since the mesh must be divided in powers of two in each direction.
3. Run the case with the same velocity and viscosity parameters as the ones you will use in your pipe maybe for 5 to 10 cycles within the flow domain, or until you reach constant turbulence.
4. Once you got the turbulence map the velocity field of the squared channel to the pipe geometry with developed flow as an initial condition (both geometries should have the same length). To do this you require to use the mapFields utility, and create a mapFieldsDict within the system directory (there are plenty of tutorials of this online).
5. Run your pipe case. At the begining, the initial condition will look weird, but as long as the flow develops, you will get some nice turbulence. Run the case through the pipe domain for at least 10 complete cycles. Then use your last time step as a new initial condition, and run your case again for another 5 cycles. By doing this I got really nice statistics. Indeed, my statistics were very close to some DNS statistics that my supervisor gave me.

I hope it helps.

If you still need to use perturbCyl, you might have to write to Eugene de Villers, since he coded that utility, but in my case it did not work. And if you make it work properly, please let me know.


Cheers,

Byron

Hi again Byron,

I am using you method to generate some turbulence firstly in a channel. However, I have a couple of questions regarding the channel I need to generate:

1. Is the channel going to have top and bottom planes as walls and inlet and outlet as cyclic? In the boxTurb tutorial 6 planes are all cyclic.
2. In order to run the flow at the same Re in the channel (for my case it is Re_tau = 180), I have to mesh the channel very fine ( even finner than my original pipe to meet the CFL condition). Is it like this in your case too?
3. Do you by any chance know whether grading is allowed for the channel mesh?

Thanks in advance!

Winson

[usv001]

Dear Foamers,

I am trying to run a compressible turbulent pipe flow using rhoCentralFoam. I have already implemented two synthetic turbulence generator boundary conditions:

• Synthetic eddy method (SEM) - superimposing turbulent structures
• Harmonic turbulence generation (HTG) - using an energy spectrum (similar to src/randomProcesses/turbulence/Ek.H)

Both methods are producing 'turbulence' (see image) with the correct mean and covariance, but the turbulence decays quickly without developing into eddies as it should. I am at a loss as to why. Has anyone faced similar problems or have any idea as to how I can prevent the decay?

Many thanks,
USV

P.S. I am not using a cyclic inlet/outlet arrangement since I would later need to apply these methods for more complicated geometries.

[gu1]

Originally Posted by usv001

Dear Foamers,

I am trying to run a compressible turbulent pipe flow using rhoCentralFoam. I have already implemented two synthetic turbulence generator boundary conditions:

• Synthetic eddy method (SEM) - superimposing turbulent structures
• Harmonic turbulence generation (HTG) - using an energy spectrum (similar to src/randomProcesses/turbulence/Ek.H)

Both methods are producing 'turbulence' (see image) with the correct mean and covariance, but the turbulence decays quickly without developing into eddies as it should. I am at a loss as to why. Has anyone faced similar problems or have any idea as to how I can prevent the decay?

Many thanks,
USV

P.S. I am not using a cyclic inlet/outlet arrangement since I would later need to apply these methods for more complicated geometries.

Did you find the solution to your problem?

I would like to know of the others present in the topic if, the model used to describe the velocity in the fvSchenes (div U) can influence the laminarization of the fluid when related to the spacing of the mesh in streamwise direction?

I'm having a problem with laminarization (LES - pipe), and my question is justified for this reason, because only the 'Gauss cubic' model manages to maintain the perturbations imposed by the perturbU. I do not know if it is related to the spacing in the streamwise direction.

Thanks

[usv001]

Hello Guilherme,

I did manage to find the reason behind it. In my case, the shock capturing schemes TVD scheme in rhoCentralFoam were simply too dissipative to preserve the eddies. However, when I attempted to use rhoPimpleFoam (which does not use any shock capturing scheme), the eddies made it all the way to the end with little dissipation. Check out this post for further details:

Link: Question about rhoCentralFoam and rhoPimpleFoam?

[spalartallmaras]

Originally Posted by alexeym

So I guess, you've tried channel395 mesh and it does have grading. If you'd like to have grading in your mesh and initialize it with boxTurb, you can initialize flow on the uniform mesh and then use mapFields utility to interpolate between meshes (uniform and graded).

Hi, I have a similar problem. With uniform grid the simulation works well. My time step is 0,0025 s. So I started my simulation with uniform grid only one time step.

Now I have the result of time 0,0025 s. So, with this result I did mapFields

mapFields <source> -consistent

and I changed the folder of the uniform gird to another folder "polyMesh" which has grading. But it doesnt work... What will be the reason?