[fatirishman53]

I started trying to develop turbulent flow within a channel, in order to simulate the findings of Kim, Moin, and Moser in 1987. However, I am getting some unexpected pressure readings (rapid fluctuations, between -5e-12 and 2e-12 and an overall oscillating behavior). This is unexpected because I have set a pressure gradient within fvOptions, based off a mean velocity. I expected fluctuations, but not an overall oscillating behavior.

Here are the parameters of my case:

Dimensions: 6m x 1m x 3m (x,y,z)

The mesh matches that of Kim, Moin, and Moser from 1987:
(192 x 128 x 160) in x, y, and z respectively with a 10:1 reduction in cell size toward the upper and lower boundaries

Solver = pimpleFoam

turbulenceProperties:
simulationType = laminar

transportProperties:
nu = 1.0e-5
Ubar = 0.033 (used for fvOptions)

Wall boundary conditions:
upperWall and lowerWall = type wall
velocity = uniform (0 0 0)
pressure = zeroGradient
(all other walls are cyclic)

fvOptions:
type = pressureGradientExplicitSource
active = on
selectionMode = all

pressureGradientExplicitSourceCoeffs
fieldNames = (U)
Ubar = (0.033 0 0)

So far I have about 1000s of simulation. Perhaps I'm just not giving the flow enough time to develop?

Also, I wonder if the solver term from uEqn "+ turbulence->divDevReff(U)" is not providing the necessary information to properly solve the momentum equation without an actual turbulence model.

Any helpful input would be appreciated. Thanks.

[amir.mofakham]

Hi,
I just started simulating a turbulent channel flow through the pimpleFOAM solver. I am wondering if you could get any promising results?
Thanks.

[Santiago]

1. Any reason Why you use PIMPLE for DNS?

2. The 'fluctuations' in pressure seem more like to round-up errors coming from the linear solver used. Most probably your flow is still laminar, so the 'dynamic' pressure inside the domain is zero, if you set the reference pressure as zero.

3. DivDevReff() is a pointer to the laplacian term plus the SGS fluxes. If no LES model is used, and the simulation conserves mass, then the latter are off.

[amir.mofakham]

Originally Posted by Santiago

1. Any reason Why you use PIMPLE for DNS?

2. The 'fluctuations' in pressure seem more like to round-up errors coming from the linear solver used. Most probably your flow is still laminar, so the 'dynamic' pressure inside the domain is zero, if you set the reference pressure as zero.

3. DivDevReff() is a pointer to the laplacian term plus the SGS fluxes. If no LES model is used, and the simulation conserves mass, then the latter are off.

Hi Santiago,


Thank you for your response.

I guess you replied to fatirishman53 questions, but your answer is helpful to me too. My goal is to solve a turbulent channel flow by the DNS approach. I appreciate if you can help in this regard.
I just found out OpenFOAM has been used for the DNS study, so I decided to start with the channel395 example of the LES pimpleFOAM tutorial and just changed the simulation type to "laminar".
I picked pimpleFOAM, just because I thought it is more stable than pisoFOAM. Please let me know if you have any other suggestion.

I am trying to simulate a square turbulent channel with the size of (0.1, 0.15, 0.15) (m) and (160, 128, 128) number of grids. The grid is staggered toward the walls with the growth ratio of 1.06. The cyclic boundary condition is imposed in the x-direction.

The flow was initialized with perturbUChannel and used 3e-6 s for the time step. I know that this should be run for a very long time to get turbulent features, and it is possible I get laminar flow after a long simulation.
I appreciate if you can help me to make sure that I am on the right track.

[Santiago]

Originally Posted by amir.mofakham

Hi Santiago,


Thank you for your response.

I guess you replied to fatirishman53 questions, but your answer is helpful to me too. My goal is to solve a turbulent channel flow by the DNS approach. I appreciate if you can help in this regard.
I just found out OpenFOAM has been used for the DNS study, so I decided to start with the channel395 example of the LES pimpleFOAM tutorial and just changed the simulation type to "laminar".
I picked pimpleFOAM, just because I thought it is more stable than pisoFOAM. Please let me know if you have any other suggestion.

I am trying to simulate a square turbulent channel with the size of (0.1, 0.15, 0.15) (m) and (160, 128, 128) number of grids. The grid is staggered toward the walls with the growth ratio of 1.06. The cyclic boundary condition is imposed in the x-direction.

The flow was initialized with perturbUChannel and used 3e-6 s for the time step. I know that this should be run for a very long time to get turbulent features, and it is possible I get laminar flow after a long simulation.
I appreciate if you can help me to make sure that I am on the right track.

Some questions/comments:

1. I guess by stability you mean 'robustness' of PIMPLE comapred to PISO. In any case, if your grid is OK, I don't see why you would need to run an over-dissipative solver like PIMPLE in order to get this channel going. If you need PIMPLE (OuterCorrectors or nonOrthogonalCorrectors) for such a simple case, then you have something really wrong with your case.

2. your time-step is extremely small! Going so small in the time-step using PISO solvers forces the local term (ddt(U)) to be balanced by convection (div(UU)), instead of the pressure gradient, which renders the solution first-order accurate. I'm not going into the details of this, but if you want a quasi-DNS using OpenFOAM (note the 'quasi'), you'll have to increment that dt a bit. What's your Re_tau?

3. Get used to run your simulation in non-dimensional scales! specially if you're solving for archetype flows. Like that you're solving for a very specific case, whereas for a non dimensional case you'll be solving for a family of channels!

[amir.mofakham]

Originally Posted by Santiago

Some questions/comments:

1. I guess by stability you mean 'robustness' of PIMPLE comapred to PISO. In any case, if your grid is OK, I don't see why you would need to run an over-dissipative solver like PIMPLE in order to get this channel going. If you need PIMPLE (OuterCorrectors or nonOrthogonalCorrectors) for such a simple case, then you have something really wrong with your case.

2. your time-step is extremely small! Going so small in the time-step using PISO solvers forces the local term (ddt(U)) to be balanced by convection (div(UU)), instead of the pressure gradient, which renders the solution first-order accurate. I'm not going into the details of this, but if you want a quasi-DNS using OpenFOAM (note the 'quasi'), you'll have to increment that dt a bit. What's your Re_tau?

3. Get used to run your simulation in non-dimensional scales! specially if you're solving for archetype flows. Like that you're solving for a very specific case, whereas for a non dimensional case you'll be solving for a family of channels!

Thank you so much for your helpful comments and suggestions.



1- Sure, I will switch to PISO, but I was using PIMPLE with nOuterCorrectors and nCorrectors equal to 1. So I guess I was already using PISO, right?



2- I made the time step small to capture the fluctuations with large frequencies. I though the smaller the time step is, the more accurate the fluctuations can be captures. Re-tau is 300 based on the height of the square channel.


3- Sure, I will make the size and velocity of the channel dimensionless.

[Santiago]

Originally Posted by amir.mofakham

Thank you so much for your helpful comments and suggestions.



1- Sure, I will switch to PISO, but I was using PIMPLE with nOuterCorrectors and nCorrectors equal to 1. So I guess I was already using PISO, right?



2- I made the time step small to capture the fluctuations with small frequencies. I though the smaller the time step is, the more accurate the fluctuations can be captures. Re-tau is 300 based on the height of the square channel.


3- To run the simulation in dimensionless scale, I should only change the size of the channel and the velocity? Right?

Responses:

1. I guess, I don't know. Does the PIMPLE algorithm reduce to PISO, exactly, when given the right parameters (whichever they are)?

2. Small frequencies? You mean High-frequencies, with small time steps! Besides, what kind of high frequency pressure fluctuations you expect to capture? At such time-scales you seem to be going towards the dissipative range, where no sub-harmonic should be present.

3. You have to scale velocities, viscosity, dimensions.


One last note, and probably one for which they could kick me out of this forum: but, Why you deem to use FVM PISO (OpenFOAM) as a proper algorithm for DNS?

[amir.mofakham]

Originally Posted by Santiago

Responses:

1. I guess, I don't know. Does the PIMPLE algorithm reduce to PISO, exactly, when given the right parameters (whichever they are)?

2. Small frequencies? You mean High-frequencies, with small time steps! Besides, what kind of high frequency pressure fluctuations you expect to capture? At such time-scales you seem to be going towards the dissipative range, where no sub-harmonic should be present.

3. You have to scale velocities, viscosity, dimensions.


One last note, and probably one for which they could kick me out of this forum: but, Why you deem to use FVM PISO (OpenFOAM) as a proper algorithm for DNS?

1- I prefer to discuss the other questions and leave understanding the difference between the PISO and PIMPLE solvers for future. Thanks for the answer though.


2- You are right! I meant fluctuations with high frequencies! I will increase the time step to see if I can get better results or not. Thanks.


3- I should make the parameters dimensionless in wall scale, right? So the dimensions will be L/(Nu/U*), and the velocities U/U*. But I am not sure what I should pick for viscosity!

That is a good question! I would like to simulate a turbulent channel flow by the DNS approach to capture the near-wall coherent structures and also study the turbulent features including the Lagrangian and Eulerian time scale. Then I would like to simulate particle motion in the turbulent flow! I was running a spectral code with point particle simulation, then I found out people have used OpenFOAM. The good thing about OpenFOAM is that it is coupled with LIGGGHTS code which makes possible use the Immersed Boundary approach to more accurately study particle motion in turbulent flows. So I decided to try OpenFOAM to see what I can get by this code, but I am not sure if I can get promising results or not!

[Santiago]

Originally Posted by amir.mofakham

1- I prefer to discuss the other questions and leave understanding the difference between the PISO and PIMPLE solvers for future. Thanks for the answer though.


2- You are right! I meant fluctuations with high frequencies! I will increase the time step to see if I can get better results or not. Thanks.


3- I should make the parameters dimensionless in wall scale, right? So the dimensions will be L/(Nu/U*), and the velocities U/U*. But I am not sure what I should pick for viscosity!

That is a good question! I would like to simulate a turbulent channel flow by the DNS approach to capture the near-wall coherent structures and also study the turbulent features including the Lagrangian and Eulerian time scale. Then I would like to simulate particle motion in the turbulent flow! I was running a spectral code with point particle simulation, then I found out people have used OpenFOAM. The good thing about OpenFOAM is that it is coupled with LIGGGHTS code which makes possible use the Immersed Boundary approach to more accurately study particle motion in turbulent flows. So I decided to try OpenFOAM to see what I can get by this code, but I am not sure if I can get promising results or not!

Responses:

1. Fair enough! Although I would suggest you to clear that up, I meant the question to be rhetoric: It is very important what kind of equation you're solving when using PISO, i.e. what do you recover from the linearized problem. There is people that have used PISO for DNS, but the question is not whether the results are correct but whether the results correspond to the solution of the INSE, or just to a 'relaxed' version of it. A simple inviscid laminar test should show you what I'm talking about.

2. REad the paper of Le & Moin (1993?) it might give you some insight.

3. In that case viscosity becomes equal to 1/Re, no-brainer!

well, try to reproduce the KMM 1987 paper first! And use a constant pressure gradient to drive the flow (not a constant UMean) and check the velocity RMS, and the integral force balance.

I would even go a step back and try to validate the PISO code using some limiting cases: Taylor-Vortex, transition to turbulence, etc. Validating with a channel flow is a "cheap shot": the flow is highly diffusive at low-Re, so it's difficult to see the non-linearities in action!

[calf.Z]

Originally Posted by Santiago

Some questions/comments:

1. I guess by stability you mean 'robustness' of PIMPLE comapred to PISO. In any case, if your grid is OK, I don't see why you would need to run an over-dissipative solver like PIMPLE in order to get this channel going.

2. your time-step is extremely small! Going so small in the time-step using PISO solvers forces the local term (ddt(U)) to be balanced by convection (div(UU)), instead of the pressure gradient, which renders the solution first-order accurate.

3. Get used to run your simulation in non-dimensional scales!

Thank you for your excellent response.

I want to use DNS to investigate the heat transfer of supercritical CO2 in the heated pipe by using OpenFOAM.

Is pimple also over-dissipative when solving pipe flows? I have heard that pimple is also suitable for DNS.

If I use DNS, the time step should be small enough, is it right?

I want to simulate the case of the experiment, what is the result if I don't run it in non-dimension scales?

Regards,
Calf.Z