CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

buoyantBoussinesqSimpleFoam time step continuity error

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

Like Tree1Likes
  • 1 Post By engineerJAM

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 26, 2023, 22:59
Default buoyantBoussinesqSimpleFoam time step continuity error
  #1
New Member
 
Jacob
Join Date: Apr 2023
Posts: 5
Rep Power: 3
engineerJAM is on a distinguished road
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
engineerJAM is offline   Reply With Quote

Old   October 27, 2023, 03:43
Default
  #2
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,140
Rep Power: 27
Yann will become famous soon enough
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
Yann is offline   Reply With Quote

Old   October 28, 2023, 23:05
Default
  #3
New Member
 
Jacob
Join Date: Apr 2023
Posts: 5
Rep Power: 3
engineerJAM is on a distinguished road
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 ??:?
engineerJAM is offline   Reply With Quote

Old   October 29, 2023, 03:03
Default
  #4
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,140
Rep Power: 27
Yann will become famous soon enough
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
Yann is offline   Reply With Quote

Old   October 29, 2023, 22:30
Default
  #5
New Member
 
Jacob
Join Date: Apr 2023
Posts: 5
Rep Power: 3
engineerJAM is on a distinguished road
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
engineerJAM is offline   Reply With Quote

Old   October 30, 2023, 03:52
Default
  #6
Senior Member
 
Yann
Join Date: Apr 2012
Location: France
Posts: 1,140
Rep Power: 27
Yann will become famous soon enough
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
Yann is offline   Reply With Quote

Old   October 30, 2023, 22:38
Default
  #7
New Member
 
Jacob
Join Date: Apr 2023
Posts: 5
Rep Power: 3
engineerJAM is on a distinguished road
Yann,



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


Jacob
Yann likes this.
engineerJAM is offline   Reply With Quote

Reply

Tags
p_rgh, time step cont. error

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
courant number increases to rather large values 6863523 OpenFOAM Running, Solving & CFD 22 July 5, 2023 23:48
Undeclared Identifier Errof UDF SteveGoat Fluent UDF and Scheme Programming 7 October 15, 2014 07:11
Upgraded from Karmic Koala 9.10 to Lucid Lynx10.04.3 bookie56 OpenFOAM Installation 8 August 13, 2011 04:03
Problem with compile the setParabolicInlet ivanyao OpenFOAM Running, Solving & CFD 6 September 5, 2008 20:50
Could anybody help me see this error and give help liugx212 OpenFOAM Running, Solving & CFD 3 January 4, 2006 18:07


All times are GMT -4. The time now is 00:56.