# buoyantBoussinesqSimpleFoam time step continuity error

 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 26, 2023, 22:59 buoyantBoussinesqSimpleFoam time step continuity error #1 New Member   Jacob Join Date: Apr 2023 Posts: 5 Rep Power: 3 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

 October 27, 2023, 03:43 #2 Senior Member   Yann Join Date: Apr 2012 Location: France Posts: 1,140 Rep Power: 27 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

 October 28, 2023, 23:05 #3 New Member   Jacob Join Date: Apr 2023 Posts: 5 Rep Power: 3 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::type Foam::sumProd(Foam::UList const&, Foam::UList const&) at ??:? #4 Foam::scalarProduct::type Foam::gSumProd(Foam::UList const&, Foam::UList const&, int) at ??:?

 October 29, 2023, 03:03 #4 Senior Member   Yann Join Date: Apr 2012 Location: France Posts: 1,140 Rep Power: 27 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

 October 29, 2023, 22:30 #5 New Member   Jacob Join Date: Apr 2023 Posts: 5 Rep Power: 3 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

 October 30, 2023, 03:52 #6 Senior Member   Yann Join Date: Apr 2012 Location: France Posts: 1,140 Rep Power: 27 Thank for the re-upload. After a quick check: 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) Pressure BCs have to be defined on p_rgh, while p has to use calculated BC (check the buoyantBoussinesqSimpleFoam tutorials) 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

 October 30, 2023, 22:38 #7 New Member   Jacob Join Date: Apr 2023 Posts: 5 Rep Power: 3 Yann, Thank you so much. I changed those boundary conditions and now it converges. Jacob Yann likes this.

 Tags p_rgh, time step cont. error