[a.mahmoud]

I have a problem where I am required to simulate the flow through a reconstructed geometry of a human vessel (pipe flow), where the pressure at the inlet and at the outlet is known, in order to find the resultant flow rate.



My question is how should I set up a case in openFoam using the simpleFoam solver, where the pressures are the input and no velocity is specified. I have tried doing this by setting the velocity boundary condition to zero gradient at both ends, and the pressure as fixed value for both values, but the results were usually unstable and did not converge satisfactorily. I have tried with k-epsilon turbulence models as well as k-omega SST and even fully laminar, but none of them would converge.


What appropriate boundary conditions should I use and how can I improve the stability and convergence of the problem?


Thank in advance!

[frantov]

That seems correct. Check the file attached, which is a microchannel (100microns x 20) the velocity is generated correctly with pressure. This case is laminar.

microch_vel.png
microchannel100x20Pressure.zip
Perhaps you can try laminar first and then add turbulence later?


What issues are you having?
Cheers
Francisco

[AndreasPe]

Maybe you can try the pressureInletUniformVelocity instead of zeroGradient for one side. This sets velocity to a constant value over the whole inlet in one direction, which made simulations stable in my case...

https://www.openfoam.com/documentati...d.html#details

[a.mahmoud]

Originally Posted by AndreasPe

Maybe you can try the pressureInletUniformVelocity instead of zeroGradient for one side. This sets velocity to a constant value over the whole inlet in one direction, which made simulations stable in my case...

https://www.openfoam.com/documentati...d.html#details

What value would I set i to. Note that I do not have vales for the velocity or the flux, that is the value i am after.

[AndreasPe]

The "value" field ist just a dummy field for this boundary condition, that will be overwritten by the calculation of the boundary condition. So you can just set it to 0.

[Tobermory]

Another suggestion is to apply a total pressure boundary condition at the upstream end; the ESI documentation page (https://www.openfoam.com/documentati...tions-subsonic) suggests that this gives good stability ... my experience is a bit mixed though. Let us know what ends up working for you.

[dlahaye]

Aha!

What has your experience with subsonic cases been?

I am working on a jet-in-co-flow with transonic jet to (hopefully) clarify convergence issues. What are in your experience are point to look into?

Would pressure-velocity coupled solver help in these cases?

Thx, Domenico.

[zyliao]

Originally Posted by a.mahmoud

I have a problem where I am required to simulate the flow through a reconstructed geometry of a human vessel (pipe flow), where the pressure at the inlet and at the outlet is known, in order to find the resultant flow rate.



My question is how should I set up a case in openFoam using the simpleFoam solver, where the pressures are the input and no velocity is specified. I have tried doing this by setting the velocity boundary condition to zero gradient at both ends, and the pressure as fixed value for both values, but the results were usually unstable and did not converge satisfactorily. I have tried with k-epsilon turbulence models as well as k-omega SST and even fully laminar, but none of them would converge.


What appropriate boundary conditions should I use and how can I improve the stability and convergence of the problem?


Thank in advance!

Hi Ahmad,
Have you solved the problem yet? What boundary conditions are appropriate?
These days I met the same stability and convergence problem when I simulated the plane-Poiseuille flow (plane-parallel plates with pressure gradient).
I chose the simpleFoam solver, and set simulationType as laminar in the turbulenceProperties file, and the boundary and initial conditions are showed in the followed figure.

According to my result, it didn’t converge even after 200000 time steps (attached figure 2).

But, one good point is the simulated outlet flux is matched quite well with the calculated flux by the theoretical equation (Cubic law: v=－△Pw^2/(12μL) (m/s)).

[zyliao]

Originally Posted by zyliao

Hi Ahmad,
Have you solved the problem yet? What boundary conditions are appropriate?
These days I met the same stability and convergence problem when I simulated the plane-Poiseuille flow (plane-parallel plates with pressure gradient).
I chose the simpleFoam solver, and set simulationType as laminar in the turbulenceProperties file, and the boundary and initial conditions are showed in the followed figure.

According to my result, it didn’t converge even after 200000 time steps (attached figure 2).

But, one good point is the simulated outlet flux is matched quite well with the calculated flux by the theoretical equation (Cubic law: v=－△Pw^2/(12μL) (m/s)).

I uploaded one of my OF case to the GoogleDrive, maybe someone can have a look? Thank you!
https://drive.google.com/drive/folde...Th?usp=sharing

[Tobermory]

If you look at the log file that you posted, you'll see that it is doing zero iterations on the solvers for Ux and p ... which means that it has stopped solving. You need to adjust the solver tolerances to force it to solve to a tighter residual level, or add a minIter line in the solver instructions to force it to always do at least 1 iteration. That will keep it solving ... up to the limit posed by your grid design. Hope that helps.

[zyliao]

Originally Posted by Tobermory

If you look at the log file that you posted, you'll see that it is doing zero iterations on the solvers for Ux and p ... which means that it has stopped solving. You need to adjust the solver tolerances to force it to solve to a tighter residual level, or add a minIter line in the solver instructions to force it to always do at least 1 iteration. That will keep it solving ... up to the limit posed by your grid design. Hope that helps.

Hi Tobermory,
Actually I conducted some other cases by setting different tolerances. As you can see from the attached figure, if the tolerances are bigger (cases name highlight by yellow), it can converge very fast, but the outlet flux didn’t match the theoretical value well (the theoretical averaged flow rate v = 0.4464 m/s); while if the tolerances are smaller, it’ll converge very hard.

And how to add a minIter line in the solver intructions?
I also a little confused about the exact meaning of “No Iterations X” in the log file. As you can see in my results, X can equal to nonzero in the converged cases.

BTW, I wonder what’s the difference between the “tolerance” and “residualControl”?
What are the exact meanings of “tolerance”, “relTol” and “residualControl”? What do these three values control? What settings are appropriate for them? Are there any tips or rules for people to obey?

[zyliao]

Originally Posted by AndreasPe

Maybe you can try the pressureInletUniformVelocity instead of zeroGradient for one side. This sets velocity to a constant value over the whole inlet in one direction, which made simulations stable in my case...

https://www.openfoam.com/documentati...d.html#details

Hi AndreasPe
I tried the pressureInletUniformVelocity type for the inlet (cases name highlight by green), it indeed converges very fast, but the calculated outlet flow rate didn’t match the theoretical value (v = 0.4464 m/s) well.
I also tried the pressureInletVelocity type (cases name highlight by blue), it seems still has the stability and convergence problem.

[zyliao]

Originally Posted by frantov

That seems correct. Check the file attached, which is a microchannel (100microns x 20) the velocity is generated correctly with pressure. This case is laminar.

Attachment 86086
Attachment 86087
Perhaps you can try laminar first and then add turbulence later?


What issues are you having?
Cheers
Francisco

Hi Francisco,

I wonder which solver did you use for your case? simpleFoam, pisoFoam or pimpleFoam? I'm a little confused because I see seetings for PISO, SIMPLE & PIMPLE in the fvSolution file.

[Tobermory]

Originally Posted by zyliao

Hi Tobermory,
And how to add a minIter line in the solver intructions?

In fvSolution, just add a line for each variable you want to apply it to, eg.:

    p
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.01;
        smoother        GaussSeidel;
        minIter         1;
    }

Originally Posted by zyliao

I also a little confused about the exact meaning of “No Iterations X” in the log file. As you can see in my results, X can equal to nonzero in the converged cases.

The log file is showing you how many inner iterations the linear systems solver is taking to reach the tolerances you have set in the fvSolution file. This should generally be nonzero (an exception is a diagonal solver that does not have to iterate to solve), else the solver is not doing any work. In your case that you shared above, the Ux and p equations showed 0 inner iterations, which is a sign that your tolerances needed to be lowered.

BTW, I wonder what’s the difference between the “tolerance” and “residualControl”?
What are the exact meanings of “tolerance”, “relTol” and “residualControl”? What do these three values control? What settings are appropriate for them?

You need to do some homework on this - see the user guide, and perhaps have a read of https://doc.cfd.direct/notes/cfd-gen...iples/contents. Suffice it to say that tolerance and relTol controls the inner iterations, and determine when the linear solver has "converged" sufficiently, whilst residualControl controls when the whole simulation has "converged".

[zyliao]

Originally Posted by Tobermory

In fvSolution, just add a line for each variable you want to apply it to, eg.:

    p
    {
        solver          GAMG;
        tolerance       1e-08;
        relTol          0.01;
        smoother        GaussSeidel;
        minIter         1;
    }

The log file is showing you how many inner iterations the linear systems solver is taking to reach the tolerances you have set in the fvSolution file. This should generally be nonzero (an exception is a diagonal solver that does not have to iterate to solve), else the solver is not doing any work. In your case that you shared above, the Ux and p equations showed 0 inner iterations, which is a sign that your tolerances needed to be lowered.


You need to do some homework on this - see the user guide, and perhaps have a read of https://doc.cfd.direct/notes/cfd-gen...iples/contents. Suffice it to say that tolerance and relTol controls the inner iterations, and determine when the linear solver has "converged" sufficiently, whilst residualControl controls when the whole simulation has "converged".

Hi Tobermory,

Thank you very much for your patience!

I have gone through the User Guide, it didn’t introduce much about the “No Iterations” and tolerance. I’ll refer to the book you recommended.
According to my limited understanding, the values of “No Iterations” will lower from a high value towards to 0, right? So, when the values of Ux & p equal to 0, does it means Ux & p have converged (i.e., stopped solving/iterating)? So a better result maybe that when the whole simulation is converged, all the “No Iterations” values equal to 0? I mean, each variables (Ux, Uy, p) converged, then the whole simulation converged?

And I have run some cases by adding the minIter and lowering the tolerances, hope they will show better results.

[Tobermory]

The main issue is that although the residual values are normalised, their magnitude can vary from problem to problem, so a solver tolerance value that works for one problem may not be effective in another. That's why you need to keep an eye on your log file and adjust your solver settings from case to case.

According to my limited understanding, the values of “No Iterations” will lower from a high value towards to 0, right? So, when the values of Ux & p equal to 0, does it means Ux & p have converged (i.e., stopped solving/iterating)?

Umm - no, I don't think that that is the case. I don't think that the number of iterations for any of the solvers should ever drop to zero since otherwise the solution for some variables is not progressed in that iteration and my experience is that the solution then goes to junk.

For most SIMPLE simulations, you should have a small number of velocity and turbulence inner iterations (maybe even just one) and rather more pressure iterations - sometimes a few hundred. This should be the case all the way through to "convergence", i.e. until you decide that the solution is not changing significantly and you can stop the run. To decide the latter, use the residuals of course, but also monitor quantities that are of interest to you (eg velocity in a key point in the flow, macro quantity like drag on a wing, etc etc).

[joshwilliams]

Originally Posted by zyliao

Hi AndreasPe
I tried the pressureInletUniformVelocity type for the inlet (cases name highlight by green), it indeed converges very fast, but the calculated outlet flow rate didn’t match the theoretical value (v = 0.4464 m/s) well.
I also tried the pressureInletVelocity type (cases name highlight by blue), it seems still has the stability and convergence problem.

In my experience with pressure driven flow, it is best when the inlet is pressureInletVelocity and the outlet is pressureInletOutletVelocity. See attached figure where the flowrate calculated by OpenFOAM shows excellent agreement to the analytical flowrate I design the pressure BCs to replicate.

[zyliao]

Hi Tobermory,

You're right, the number of iterations do not need to drop to zero, I misunderstood this point.

Thank you very much for your patient and careful reply!

And I found that for my cases, if I set tolerances to 10e-8, residualControls to 10e-6, they can converge much better.

[zyliao]

Hi Josh,

Thank you for you advice!

According to my newest result, if I set inlet is pressureInletVelocity and the outlet is zeroGradient, and set tolerances to 10e-8, residualControls to 10e-6, it can converge better and match the theoretical value well.

I'll try to set the outlet to pressureInletOutletVelocity to see if it can perform better!

[joshwilliams]

I am working on something similar; flow in human airways taken from CT scans, with time-varying pressure defined at outlets. For a simple one bifurcation case, the BCs I mentioned above work very well (as I showed). But when the geometry gets more complex it fails (timestep gets very small as few cells at the outlet have big courant number).


Is your geometry complex like this? What fvSchemes are you using? I think my velocity BCs and pressure BCs are okay, so I think there is something else causing this.