[vsammartano]

Hi there,
I'm quite new to OpenFOAM and I am working on a CFD simulation of a Cross-Flow water Turbine. I have created the OpenFOAM case and the simulation seems to work fine. BUT, during the simulation, in the terminal I can't read the residual of the velocity components. I know that the solver computes those unknowns, I want see these residuals during the simulation.
How can I do that!?
Thanks in advance!
PS: I am using the interDyMFoam solver

[Bazinga]

how do you start the solver? I just tried a tutorial and the residuals and simulation information were shown in the terminal after I just typed the solver name.

[wyldckat]

Quick answer: Check the file "system/fvSolution", search for the block "PIMPLE" and check if this line exists:

momentumPredictor no;

If you have it defined like this, then this means that the velocity (momentum) equation isn't solved directly.

[vsammartano]

Originally Posted by wyldckat

Quick answer: Check the file "system/fvSolution", search for the block "PIMPLE" and check if this line exists:

momentumPredictor no;

If you have it defined like this, then this means that the velocity (momentum) equation isn't solved directly.

Dear Bruno, I'm so grateful to you for helping me out! I was stucked! it was such an easy solution ... tomorrow I'll modify the fvSolution file as you told me! YEP!
thank you again!

[vsammartano]

Originally Posted by Bazinga

how do you start the solver? I just tried a tutorial and the residuals and simulation information were shown in the terminal after I just typed the solver name.

Dear Bazinga, thank you for your suggestion. Obviously I started the solver typing the name of the solver in the terminal. I think this is the only way to start a simulation in OpenFOAM.
In my case the problem was that in the fvSolution file, located in the system folder, the momentum equation was not solved directly...thus I caould not find the residuals of the velocity components.

Thank you again!
cheers!

[vsammartano]

Dear Bruno, I modified the fvSolution file as you suggested....it works! Could you please suggest me some reference where I can read how does this solver work? Thank you again,
cheers!

[wyldckat]

Originally Posted by vsammartano

Could you please suggest me some reference where I can read how does this solver work?

Quick answer: Unfortunately I'm not familiar with any reference documentation for interDyMFoam.
Nonetheless, there is some about interFoam: https://openfoamwiki.net/index.php/InterFoam
The "DyM" part means "Dynamic Mesh" and is a mechanism that is mostly common to all solvers that have this tag in their name. Google:

OpenFOAM dynamic meshing explained

[Carno]

I also have exact same problem. My velocity components are not getting printed on screen to monitor. Here is a log,

Create time

Create mesh for time = 0


SIMPLE: convergence criteria
    field p      tolerance 0.0001
    field U      tolerance 0.0001
    field "(k|omega|epsilon)"    tolerance 0.0001

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
    alphaK1         0.85;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.856;
    gamma1          0.55555556;
    gamma2          0.44;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    b1              1;
    c1              10;
    F3              false;
}

Creating MRF zone list from MRFProperties
    creating MRF zone: MRF1
Creating porosity model list from porosityProperties

Porosity region porosity1:
    selecting model: DarcyForchheimer
    creating porous zone: rad
Using pressure implicit porosity
No finite volume options present


Starting time loop

Time = 1

GAMG:  Solving for p, Initial residual = 1, Final residual = 0.0229096, No Iterations 1
time step continuity errors : sum local = 0.16611452, global = -0.013244094, cumulative = -0.013244094
smoothSolver:  Solving for omega, Initial residual = 0.0074746818, Final residual = 1.6552667e-005, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0020565579, No Iterations 1
ExecutionTime = 393.767 s  ClockTime = 394 s

Time = 2

GAMG:  Solving for p, Initial residual = 0.99980948, Final residual = 0.028042093, No Iterations 1
time step continuity errors : sum local = 1373.7404, global = -115.04725, cumulative = -115.06049
smoothSolver:  Solving for omega, Initial residual = 0.001862281, Final residual = 2.6651327e-006, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 0.99999977, Final residual = 0.00054471924, No Iterations 1
bounding k, min: -30136.2 max: 40949627 average: 31.478273
ExecutionTime = 547.618 s  ClockTime = 548 s

The part of my fvSolution is as below,

SIMPLE
{
    residualControl
    {
        p               1e-4;
        U               1e-4;
        "(k|omega|epsilon)" 1e-4;
    }
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
    nUCorrectors    2;
    momentumPredictor   yes;

}

Kindly help..I am using porousSimpleFoam solver

[kmefun]

Originally Posted by Carno

I also have exact same problem. My velocity components are not getting printed on screen to monitor. Here is a log,

Create time

Create mesh for time = 0


SIMPLE: convergence criteria
    field p      tolerance 0.0001
    field U      tolerance 0.0001
    field "(k|omega|epsilon)"    tolerance 0.0001

Reading field p

Reading field U

Reading/calculating face flux field phi

Selecting incompressible transport model Newtonian
Selecting turbulence model type RAS
Selecting RAS turbulence model kOmegaSST
Selecting patchDistMethod meshWave
kOmegaSSTCoeffs
{
    alphaK1         0.85;
    alphaK2         1;
    alphaOmega1     0.5;
    alphaOmega2     0.856;
    gamma1          0.55555556;
    gamma2          0.44;
    beta1           0.075;
    beta2           0.0828;
    betaStar        0.09;
    a1              0.31;
    b1              1;
    c1              10;
    F3              false;
}

Creating MRF zone list from MRFProperties
    creating MRF zone: MRF1
Creating porosity model list from porosityProperties

Porosity region porosity1:
    selecting model: DarcyForchheimer
    creating porous zone: rad
Using pressure implicit porosity
No finite volume options present


Starting time loop

Time = 1

GAMG:  Solving for p, Initial residual = 1, Final residual = 0.0229096, No Iterations 1
time step continuity errors : sum local = 0.16611452, global = -0.013244094, cumulative = -0.013244094
smoothSolver:  Solving for omega, Initial residual = 0.0074746818, Final residual = 1.6552667e-005, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 1, Final residual = 0.0020565579, No Iterations 1
ExecutionTime = 393.767 s  ClockTime = 394 s

Time = 2

GAMG:  Solving for p, Initial residual = 0.99980948, Final residual = 0.028042093, No Iterations 1
time step continuity errors : sum local = 1373.7404, global = -115.04725, cumulative = -115.06049
smoothSolver:  Solving for omega, Initial residual = 0.001862281, Final residual = 2.6651327e-006, No Iterations 1
smoothSolver:  Solving for k, Initial residual = 0.99999977, Final residual = 0.00054471924, No Iterations 1
bounding k, min: -30136.2 max: 40949627 average: 31.478273
ExecutionTime = 547.618 s  ClockTime = 548 s

The part of my fvSolution is as below,

SIMPLE
{
    residualControl
    {
        p               1e-4;
        U               1e-4;
        "(k|omega|epsilon)" 1e-4;
    }
    nNonOrthogonalCorrectors 0;
    pRefCell        0;
    pRefValue       0;
    nUCorrectors    2;
    momentumPredictor   yes;

}

Kindly help..I am using porousSimpleFoam solver

Hi
you can set nUCorrectors 0;
to use pressure explicit porosity and then it will go through the block that solving momentum equation. More details can be referred to the files createPorousZones.H and UEqn.H which located at applications/solvers/incompressible/simpleFoam/porousSimpleFoam/
Hope this could help you.

[Carno]

Thanks ... It works

[saeed sangchooly]

Originally Posted by wyldckat

Quick answer: Check the file "system/fvSolution", search for the block "PIMPLE" and check if this line exists:

momentumPredictor no;

If you have it defined like this, then this means that the velocity (momentum) equation isn't solved directly.

dear Bruno,
I'm working with multiphaseEulerFoam solver with 3 phases
I did set momentumPredictor to yes and I've also tried setting nUcorrectors to 0; but still I can't see the velocity component residuals. why is that?
how can I fix this?

[YanaLolux]

same problem here...

[MarioM]

Originally Posted by saeed sangchooly

dear Bruno,
I'm working with multiphaseEulerFoam solver with 3 phases
I did set momentumPredictor to yes and I've also tried setting nUcorrectors to 0; but still I can't see the velocity component residuals. why is that?
how can I fix this?

I face the same problem. Could you solve it?

[saeed sangchooly]

Originally Posted by MarioM

I face the same problem. Could you solve it?

Apparently they've daisabled the momentum perdictor in this solver since it does no good in the sake of stability and acuracy in multiphase cases.
From what I've understood so far, Velocity whould be obtaind by solving momentum algebraically immedirely after solving poisson for p_rgh and updating rho (based on the equation of state specified for each phase) .

In that case, there whould be no velocity residuals which we can monitor

pls correct me if i'm wrong