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

buoyantSimpleFoam with equationOfState rhoConst crashes

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   December 7, 2017, 08:44
Default buoyantSimpleFoam with equationOfState rhoConst crashes
  #1
New Member
 
Moa Miche
Join Date: Sep 2017
Posts: 3
Rep Power: 6
Moa_miche is on a distinguished road
Hello,

I wanted to calculate the hydrodynamics and heat transfer of a stirred tank with the buoyantSimpleFoam solver. For this i merged the cases of buoyantCavity and mixerVessel2D with a MRF for the rotor of the stirred tank. If I am using the equationOfState perfectGas it is working fine and I get the velocity and temperature field. Now I wanted to use the equationOfState rhoConst and therefore changed my thermophysicalProperties-file like this:

thermoType
{
type heRhoThermo;
mixture pureMixture;
transport const;
thermo hConst;
equationOfState rhoConst;
specie specie;
energy sensibleEnthalpy;
}


In addition I inserted rho:

equationOfState
{
rho 10;
}


If I start the solver now I get the following error in the laminar and turbulent case:

Starting time loop

Time = 1

DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 0.00404327, No Iterations 1
GAMG: Solving for p_rgh, Initial residual = 0.996177, Final residual = 0.00740903, No Iterations 5
time step continuity errors : sum local = 2.42478, global = -7.73459e-15, cumulative = -7.73459e-15
#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::sigFpe::sigHandler(int) at ??:?
#2 in "/lib64/libc.so.6"
#3 Foam::dimensioned<double> Foam:perator/<double>(Foam::dimensioned<double> const&, Foam::dimensioned<double> const&) at ??:?
#4
at ??:?
#5 __libc_start_main in "/lib64/libc.so.6"
#6
at ??:?
Floating point exception
gott@master:~/OpenFOAM/gott-2.3.x/run/buoyantCavity> ICE default IO error handler doing an exit(), pid = 240390, errno = 11

Why is my simulation crashing? Is it not possible to use the equationOfState rhoConst with the buoyantSimpleFoam-Solver? Or how can i calculate with an incompressible fluid a heated stirred tank else?

Help is really appreciated I trust in your knowledge,

kind regards,

Michael
Moa_miche is offline   Reply With Quote

Old   December 8, 2017, 01:24
Default
  #2
New Member
 
Moa Miche
Join Date: Sep 2017
Posts: 3
Rep Power: 6
Moa_miche is on a distinguished road
After some research i found the answer myself. I used OF2.3.x and there is a bug in the source code. In the pEqn.H at the end you find this:

if (closedVolume) { p += (initialMass - fvc::domainIntegrate(psi*p)) /fvc::domainIntegrate(psi); p_rgh = p - rho*gh; }

For incompressible equations of state the compressibility psi is zero and therefore you get an error for closed volumes. The bug is already corrected in the new OF5.

if (!thermo.incompressible() && closedVolume)
{
p += (initialMass - fvc::domainIntegrate(psi*p))
/fvc::domainIntegrate(psi);
p_rgh = p - rho*gh;
}

With the additional condition !thermo.incompressible() you are not entering the loop for incompressible flows.

Michael
Moa_miche is offline   Reply With Quote

Old   March 12, 2019, 21:10
Default
  #3
Senior Member
 
Jianrui Zeng
Join Date: May 2018
Location: China
Posts: 157
Rep Power: 6
calf.Z is on a distinguished road
Quote:
Originally Posted by Moa_miche View Post

[/SIZE] if (!thermo.incompressible() && closedVolume)
{
p += (initialMass - fvc::domainIntegrate(psi*p))
/fvc::domainIntegrate(psi);
p_rgh = p - rho*gh;
}

With the additional condition !thermo.incompressible() you are not entering the loop for incompressible flows.

Michael
So you men that for compressible flows, it should enter the loop and adjust the pressure level to obey overall mass continuity?
calf.Z is offline   Reply With Quote

Reply

Tags
buoyantsimplefoam, floating point exception, mixervessel2d, rhoconst, thermophysicalproperties

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
buoyantSimpleFoam for Natural Ventilation Manuel CFD OpenFOAM Running, Solving & CFD 15 February 15, 2020 04:42
a problem with convergence in buoyantSimpleFoam skuznet OpenFOAM Running, Solving & CFD 6 November 15, 2017 12:12
flo-efd v11.0.0 crashes YoavF FloEFD, FloWorks & FloTHERM 3 June 21, 2012 12:37
Running buoyantSimpleFoam with oodles data as initialisation samulu OpenFOAM 5 November 19, 2009 11:49
BuoyantSimpleFoam solver crashes prashant24983 OpenFOAM Running, Solving & CFD 6 October 28, 2008 06:03


All times are GMT -4. The time now is 02:31.