[engineerJAM]

Greetings,

I have a time step continuity error appearing after p_rgh. The residual and number of iterations keeps increasing until it breaks. I've been trying to figure it out for awhile now. Any help would greatly be appreciated.

Here is what I have tried so far:

- increasing and decreasing the mesh resolution
- decreasing deltaT down to 1e-9
- change the p_rgh solver
- reviewed boundary conditions
- using a different geometry
- decreasing temperature delta between the fluid and the wall
- decreasing the velocity of the fluid (makes it take longer to break)

About the model:
Looking at the heat transfer through the wall of a single pipe. It consists of an inlet, outlet and pipe wall. The pipe follows a half circle in shape.

OpenFoam files
https://drive.google.com/drive/folde...usp=drive_link


Error Example:
Time = 8e-05

DILUPBiCGStab: Solving for Ux, Initial residual = 0.0496474, Final residual = 0.000320209, No Iterations 1
DILUPBiCGStab: Solving for Uy, Initial residual = 0.0613424, Final residual = 0.000501452, No Iterations 1
DILUPBiCGStab: Solving for Uz, Initial residual = 0.0483784, Final residual = 0.000280833, No Iterations 1
DILUPBiCGStab: Solving for T, Initial residual = 0.0223053, Final residual = 0.000718434, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 0.0799987, Final residual = 0.00549111, No Iterations 2
DICPCG: Solving for p_rgh, Initial residual = 0.0139417, Final residual = 0.00126615, No Iterations 6
DICPCG: Solving for p_rgh, Initial residual = 0.00491635, Final residual = 0.000490945, No Iterations 20
time step continuity errors : sum local = 2.23732e-07, global = -4.54896e-08, cumulative = 2.71372e-07
DILUPBiCGStab: Solving for epsilon, Initial residual = 0.172514, Final residual = 0.00040205, No Iterations 1
DILUPBiCGStab: Solving for k, Initial residual = 0.132612, Final residual = 0.00172569, No Iterations 1
ExecutionTime = 16.35 s ClockTime = 17 s

[Yann]

Hello Jacob,

Just to make sure we are on the same line, the time step continuity check is part of the resolution process. You will see it in every solver, for every time step.

In the snippet you posted, continuity errors are in the order of 10^-7, which is pretty low. This what is expected.

If continuity errors start increasing, this would indicates there is a problem in your simulation. (often related to boundary conditions)

Yann

[engineerJAM]

Not sure why my reply did not post but I'll try again.


Correct the keeps growing until it breaks. Here is what it shows when it breaks;


Time = 0.01338

DILUPBiCGStab: Solving for Ux, Initial residual = 0.0294298, Final residual = 0.000228221, No Iterations 1
DILUPBiCGStab: Solving for Uy, Initial residual = 0.0234604, Final residual = 0.000125468, No Iterations 1
DILUPBiCGStab: Solving for Uz, Initial residual = 0.0223239, Final residual = 0.000150431, No Iterations 1
DILUPBiCGStab: Solving for T, Initial residual = 0.000473069, Final residual = 4.52044e-05, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 0.0289488, Final residual = 0.00274625, No Iterations 2
DICPCG: Solving for p_rgh, Initial residual = 0.00567332, Final residual = 0.000556981, No Iterations 10
DICPCG: Solving for p_rgh, Initial residual = 0.00350916, Final residual = 0.000349147, No Iterations 6
time step continuity errors : sum local = 2.08409e+30, global = 9.4385e+29, cumulative = 1.18906e+31
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 ? in /lib/x86_64-linux-gnu/libpthread.so.0
#3 Foam::scalarProduct<double, double>::type Foam::sumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&) at ??:?
#4 Foam::scalarProduct<double, double>::type Foam::gSumProd<double>(Foam::UList<double> const&, Foam::UList<double> const&, int) at ??:?

[Yann]

OK then must probably there might be an issue with the mesh and/or boundary conditions.

I can't access your files so I cannot help more

Yann

[engineerJAM]

Yann,


Thank you for being patient with me. The link to the google drive folder should work now.


https://drive.google.com/drive/folde...usp=drive_link

[Yann]

Thank for the re-upload.

After a quick check:

1. You cannot impose a fixed value on p_rgh on both inlet and outlet, especially not with the same value (you cannot have a flow satisfying those conditions)
2. Pressure BCs have to be defined on p_rgh, while p has to use calculated BC (check the buoyantBoussinesqSimpleFoam tutorials)
3. Use fixedFluxPressure BC rather than zeroGradient on p_rgh (zeroGradient leads to flux issues on buoyant solvers)

These changes should fix your issue.

Cheers,
Yann

[engineerJAM]

Yann,



Thank you so much. I changed those boundary conditions and now it converges.


Jacob