[walakaka]

Hi everyone,

I am currently working on a two-phase laminar flow through a pipe. To check my mesh, I ran a simulation with only air through the pipe (alpha = 0) using the interFoam solver and the results matches the hagen-poiseuille equation.

However, I am currently trying to plot the residuals using help from the forum in the following link:
plot residuals

The residual plot was successful in the past when I was using the simpleFoam solver. However, using the interFoam solver, I am getting an error message stating the following

• warning: skipping data with no valid points
• unable to open display
• x11 aborted

Does anyone have any idea of what I am doing wrong?

p/s: I also notice that in my log file, they are only solving for the p_rgh term and no ux,uy or uz term

Kind regards
Shaq

[Tobi]

Hi,

you don´t solve for p, thus you have to grep for p_rgh if you want to get the residuals for p_rgh. In most cases there is no need to solve the momentum prediction. In your fvSolutions you momentumPredictor is false. Thats why you don´t see Ux, Uy and Uz residuals.

[walakaka]

Originally Posted by Tobi

Hi,

you don´t solve for p, thus you have to grep for p_rgh if you want to get the residuals for p_rgh. In most cases there is no need to solve the momentum prediction. In your fvSolutions you momentumPredictor is false. Thats why you don´t see Ux, Uy and Uz residuals.

Hi Tobi,

Thanks for getting back to me. I had a look in the fvSolution folder and it is true that my momentumPredictor is set to "no".

Could you kindly explain the following please:

• Why is there a momentumPredictor option in the interFoam solver compared to the simpleFoam solver (which has no momentum Predictor option and plots out ux, uy and uz residuals)
• Would my residual plot be fully legitimate in showing that my simulation has converged if it only contains the plot for the residual of p_rgh?

Kind regards
Shaq

[Tobi]

Hi,

• in steady-state solvers the calculation (estimation) of the velocity field helps to go to the solution. Transient normally have the momentumPredictor flag. Its nothing than estimating the U field.
• Yes, if p_rgh is converged, the fluxes are converged as well and thus the U field. Normally the momentumPredictior is needed if the viscosity ratio is large (e.g. in two phase flows). If one does not activate the momentum predictor, the tolerance for the pressure has to be set very strictly

[walakaka]

Originally Posted by Tobi

Hi,

• in steady-state solvers the calculation (estimation) of the velocity field helps to go to the solution. Transient normally have the momentumPredictor flag. Its nothing than estimating the U field.
• Yes, if p_rgh is converged, the fluxes are converged as well and thus the U field. Normally the momentumPredictior is needed if the viscosity ratio is large (e.g. in two phase flows). If one does not activate the momentum predictor, the tolerance for the pressure has to be set very strictly

Thank you Tobi!

I have another question:

When not activating the momentum predictor, the solver only solves the residual for p_rgh. However, every time iteration has 3 p_rgh residuals, Which one should I take from each iteration?

Also, if one does not activate the momentum predicture, what are the recommended tolerance for pressure residuals? Will it have to be below 1e-7 or will a residual of magnitude below 1e-5 be reasonable?

Regards
Shafik

[walakaka]

Originally Posted by walakaka

Thank you Tobi!

I have another question:

When not activating the momentum predictor, the solver only solves the residual for p_rgh. However, every time iteration has 3 p_rgh residuals, Which one should I take from each iteration?

Also, if one does not activate the momentum predicture, what are the recommended tolerance for pressure residuals? Will it have to be below 1e-7 or will a residual of magnitude below 1e-5 be reasonable?

Regards
Shafik

Has anyone got any info on this matter please?

[walakaka]

Originally Posted by walakaka

Has anyone got any info on this matter please?

For example, the logs below, Which residual do I grep for? The first, second or final one? Or do I grep for each of them in succession (even though they are the resultant value from 1 particular iteration)



PIMPLE: iteration 1
smoothSolver: Solving for alpha.water, Initial residual = 0.000529543, Final residual = 2.66809e-11, No Iterations 2
Phase-1 volume fraction = 0.517887 Min(alpha.water) = 0 Max(alpha.water) = 1.06837
MULES: Correcting alpha.water
MULES: Correcting alpha.water
Phase-1 volume fraction = 0.517887 Min(alpha.water) = -8.72144e-07 Max(alpha.water) = 1.06794
DICPCG: Solving for p_rgh, Initial residual = 1, Final residual = 0.880426, No Iterations 1001
time step continuity errors : sum local = 0.00204219, global = -2.39327e-05, cumulative = -4.39327e-05
DICPCG: Solving for p_rgh, Initial residual = 0.270516, Final residual = 0.753417, No Iterations 1001
time step continuity errors : sum local = 0.00579181, global = -2.39253e-05, cumulative = -6.7858e-05
DICPCG: Solving for p_rgh, Initial residual = 0.510678, Final residual = 0.1488, No Iterations 1001
time step continuity errors : sum local = 0.00170815, global = -1.19552e-05, cumulative = -7.98132e-05
ExecutionTime = 12.26 s ClockTime = 12 s

Regards
Shaq

[walakaka]

Originally Posted by Tobi

Hi,

• in steady-state solvers the calculation (estimation) of the velocity field helps to go to the solution. Transient normally have the momentumPredictor flag. Its nothing than estimating the U field.
• Yes, if p_rgh is converged, the fluxes are converged as well and thus the U field. Normally the momentumPredictior is needed if the viscosity ratio is large (e.g. in two phase flows). If one does not activate the momentum predictor, the tolerance for the pressure has to be set very strictly

Hi Tobi,

I have used your advice and greped for p_rgh successfully, is there a command to only grep the final residual in every outer loop iteration?
Because at the moment, my residual plot is plotting every single iteration (inner loop and outer loop) as shown in the attached file.

Yaxis: residuals
Xaxis: Iterations

Kind regards
Shafik

[saeed sangchooly]

Originally Posted by Tobi

Hi,

• in steady-state solvers the calculation (estimation) of the velocity field helps to go to the solution. Transient normally have the momentumPredictor flag. Its nothing than estimating the U field.
• Yes, if p_rgh is converged, the fluxes are converged as well and thus the U field. Normally the momentumPredictior is needed if the viscosity ratio is large (e.g. in two phase flows). If one does not activate the momentum predictor, the tolerance for the pressure has to be set very strictly

dear Tobi
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?

[Tobi]

Can you provide use the solver log file?
If you have the momentumPredictor activated, you have to see it. Maybe its related to the solver and the residual control function object (don't know how you are extracting your data) should give the velocity field. Otherwise, its a feature we would / could be implement in newer versions.

[saeed sangchooly]

Originally Posted by Tobi

Can you provide use the solver log file?
If you have the momentumPredictor activated, you have to see it. Maybe its related to the solver and the residual control function object (don't know how you are extracting your data) should give the velocity field. Otherwise, its a feature we would / could be implement in newer versions.

that's the point. there is no solving message for velocity in the log file:
this is what I get in log file:


(RAS bubble column tutorial in multiphaseEulerFoam):

PIMPLE: Iteration 1
MULES: Solving for alpha.air
MULES: Solving for alpha.water
air fraction, min, max = 0.293331 -2.33203e-178 1
water fraction, min, max = 0.706669 0 1
Phase-sum volume fraction, min, max = 1 1 1
MULES: Solving for alpha.air
MULES: Solving for alpha.water
air fraction, min, max = 0.293331 -6.74315e-178 1
water fraction, min, max = 0.706669 0 1
Phase-sum volume fraction, min, max = 1 1 1
Constructing momentum equations
smoothSolver:  Solving for e.air, Initial residual = 0.000387688, Final residual = 1.57809e-08, No Iterations 1
smoothSolver:  Solving for e.water, Initial residual = 1.45421e-06, Final residual = 4.86519e-11, No Iterations 1
air min/max T 300 - 350
water min/max T 300.159 - 350
GAMG:  Solving for p_rgh, Initial residual = 3.32827e-06, Final residual = 8.8626e-09, No Iterations 5

it seems that momentunPredictor can not be actually activated in multiphaseEulerFoam. because the solver gave no error that for example UFinal is undefined in fvSolution like other solvers.

thank you so much for your answer btw.

[Tobi]

You mix up a few things here. However, you are right, the momentum-prediction is not implemented: https://develop.openfoam.com/Develop...erFoam/UEqns.H

So probably, there is a reason why its not implemented or why we cannot use a prediction step prior to the pressure-equation. I am not familiar with multiphase flows.

However, UFinal, if you don't set the "*.Final" Relaxation, it is commonly 1. It should be a <lookupOrDefault> value. So I never had issues that "*.Final" is not defined in terms of relaxation factors. Furthermore, in the UEqns.H file, you can see that the relaxation of the matrix is commented. Hence, not used at all.


Note. In the Foundation version, there you have the relaxation included:

https://github.com/OpenFOAM/OpenFOAM...oam/pU/UEqns.H

[saeed sangchooly]

Originally Posted by Tobi

You mix up a few things here. However, you are right, the momentum-prediction is not implemented: https://develop.openfoam.com/Develop...erFoam/UEqns.H

So probably, there is a reason why its not implemented or why we cannot use a prediction step prior to the pressure-equation. I am not familiar with multiphase flows.

However, UFinal, if you don't set the "*.Final" Relaxation, it is commonly 1. It should be a <lookupOrDefault> value. So I never had issues that "*.Final" is not defined in terms of relaxation factors. Furthermore, in the UEqns.H file, you can see that the relaxation of the matrix is commented. Hence, not used at all.


Note. In the Foundation version, there you have the relaxation included:

https://github.com/OpenFOAM/OpenFOAM...oam/pU/UEqns.H

you mean it's a bug in openFOAM8 (that momentum-prediction can not be implemented in multiphaseEulerFoam)?
is there any chance that other versions don't have this bug?