|
[Sponsors] |
What is wrong with my pressure? buoyantBoussinesqSimpleFoam |
![]() |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
![]() |
![]() |
#1 |
New Member
Andreas
Join Date: Jun 2015
Posts: 3
Rep Power: 11 ![]() |
Hello,
My pressure ends up like this all the time, I have tried so many different BC's but nothing seems to help. The velocity and temperature fields seems fine though. xD.jpg I am using the solver buoyantBoussinesqSimpleFoam. Thanks for help! |
|
![]() |
![]() |
![]() |
![]() |
#2 |
Member
Join Date: Nov 2009
Posts: 56
Rep Power: 16 ![]() |
It is better to be more clear when posting questions. Which pressure are you visualising in the figure above, p or p_rgh? Your solver uses the Boussinesq approximation and introduces a modified pressure term, so you really have two pressure definitions that you can visualize (p and p_rgh). Definitions are p=p_rgh+rhok*gh, so p includes the buoyancy contribution.
|
|
![]() |
![]() |
![]() |
![]() |
#3 | |
New Member
Andreas
Join Date: Jun 2015
Posts: 3
Rep Power: 11 ![]() |
Quote:
Sorry for the lack of information, I simply just thought it was an ordinary error that you could solve quite fast. In the figure i visualise p but p_rgh shows only the same value in the entire volume. My BC's are: p_rgh: outlet - fixedValue 101325; all other boundaries - fixedFluxPressure; p: calculated on all boundaries. I really appreciate your help! |
||
![]() |
![]() |
![]() |
![]() |
#4 |
New Member
Mateo
Join Date: Jun 2019
Posts: 3
Rep Power: 7 ![]() |
did you solved your problem?
i am simulaing the same case but i am having troubles with the convergence of the simulation. Could you please tell me which were your BC for the velocity? Thank You |
|
![]() |
![]() |
![]() |
![]() |
#5 | |
Member
Mahmoud
Join Date: Nov 2020
Location: United Kingdom
Posts: 43
Rep Power: 5 ![]() |
Quote:
Could you please share your experience if you've made any progress on this thread? Cheers |
||
![]() |
![]() |
![]() |
![]() |
#6 |
Senior Member
Yann
Join Date: Apr 2012
Location: France
Posts: 1,169
Rep Power: 27 ![]() |
Hi,
The thread is quite old so I do not know if the original author will answer. I experienced something similar with buoyantSimpleFoam and in my case it was related to the writePrecision setting in controlDict. By default writePrecision is set to 6 which means data will be written with 6 significant figures. When working with absolute pressure, this leads to rounding up pressure values to the nearest Pascal. For natural convection, the pressure difference is usually quite small and writePrecision needs to be increased in order to write pressure values with a precision fitting the actual pressure gradient in the flow. Please note this is a matter of write precision so it does not affect the simulation by itself. But it can cause issues when restarting a simulation since the solver will read the latest time step / iteration. I hope this helps, Yann |
|
![]() |
![]() |
![]() |
![]() |
#7 |
Member
Mahmoud
Join Date: Nov 2020
Location: United Kingdom
Posts: 43
Rep Power: 5 ![]() |
Dear Foamers,
It’s been a while that I’ve had the same problem in setting the correct BC for similar problems. Here is the review of how I solved this issue: Problem: steady state open channel flow simulation. In this scenario, normally the simpleFoam is employed. The BCs are given by: BCs: inlet, outlet, wall, topWall U: inlet { type fixedValue; value uniform (0 0.1589 0); } outlet { type zeroGradient; } wall { type noSlip; } atmosphere { type slip; } p: atmosphere { type zeroGradient; } inlet { type zeroGradient; } outlet { type fixedValue; value uniform 0; } wall { type fixedFluxPressure; //remember that we cannot use Drichlet and Neuman BC at the same time value uniform 0; } As one can see, selecting fixedValue BC for the outlet pressure is physically incorrect even though one can get result. To resolve this issue, I decided to use the hydrostatic pressure as the outlet BC for the pressure. To this end, one need to either define gravity in the governing equation or else use a steady state solver that has gravity in the equations. I went for the second approach. The only available solver for incompressible fluids that has this feature is buoyantBoussinesqSimpleFoam. When this solver is selected, the BCs needs to be defined for the U, p, and p_rgh. Generally, p_rgh=p-rho*g*h. I have searched a lot and finally could find the correct way of setting BC for the foregoing parameters. U: inlet { type fixedValue; value uniform (0 0.1589 0); } outlet { type pressureInletOutletVelocity; value uniform (0 0 0); inletValue uniform (0 0 0); } wall { type noSlip; } atmosphere { type slip; } P: atmosphere { type zeroGradient; } inlet { type zeroGradient; } outlet { type calculated; value $internalField; } wall { type zeroGradient; } P_rgh inlet { type fixedFluxPressure; } outlet { type fixedValue; value uniform 0; } wall { type fixedFluxPressure; } atmosphere { type fixedFluxPressure; } let me know if it is not clear. Keep Foaming |
|
![]() |
![]() |
![]() |
|
|
![]() |
||||
Thread | Thread Starter | Forum | Replies | Last Post |
[ANSYS Meshing] Help with element size | sandri_92 | ANSYS Meshing & Geometry | 14 | November 14, 2018 07:54 |
Does star cd takes reference pressure? | monica | Siemens | 1 | April 19, 2007 11:26 |
Pressure Inlet yields wrong velocities | Ben | FLUENT | 0 | November 21, 2004 01:47 |
Gas pressure question | Dan Moskal | Main CFD Forum | 0 | October 24, 2002 22:02 |
Hydrostatic pressure in 2-phase flow modeling (CFX4.2) | HB &DS | CFX | 0 | January 9, 2000 13:19 |