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

buoyantSimpleFoam and watertank

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

Like Tree9Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   January 14, 2014, 16:28
Default
  #41
New Member
 
Bernhard
Join Date: May 2012
Location: Freiburg/Germany
Posts: 7
Rep Power: 7
BernhardS is on a distinguished road
Unfortunately I do not get beyond 0.07 seconds before the pressure blows up. If have attached the new version with the modified Allrun script. Switching off the turbulence does not make any difference...
Attached Files
File Type: gz ts_v1.gz (38.2 KB, 9 views)
BernhardS is offline   Reply With Quote

Old   January 15, 2014, 12:32
Default
  #42
New Member
 
Bernhard
Join Date: May 2012
Location: Freiburg/Germany
Posts: 7
Rep Power: 7
BernhardS is on a distinguished road
I am able to run that case if I change the BCs for p_rgh for bottom and wall to buoyantPressure and the one for top to fixedValue. Additionally I use funkySetField to initialize p. I have to use a lot of outerCorrectors (~30) at the beginning and underrelaxation, especially for p_rgh.

The velocity profile at the wall, due to the heat loss, is not as distinctive as before with buoyantBoussinesqPimpleFoam (see post #36). While the velocity profile is well developed in the lower region (after 360 sec), there are some disturbances in upper region probably caused by the BC for the top face.
UY.jpg T1.jpgThot.jpg Tcold.jpg
At least the temperature distribution is stable and quite uniform in radial direction (except at the outer wall with the heat flux) which was previously not the case.

Does anyone have an idea which BCs might be as well appropiate for a closed tank?
Even though the case is running with the current BCs, it is probably a wrong setup since there is still some velocity (see Fig. 2, UY) at the top face where it should actually be zero...
BernhardS is offline   Reply With Quote

Old   January 15, 2014, 17:07
Default
  #43
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,806
Blog Entries: 6
Rep Power: 32
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Hi Bernhard,

I tryed several options.

- changing 0/ files
- changing initialization
- changing thermodynamicProperties (with air its working)

- test case with cht
- test case with buoyant
- test case with boussinesq

- testings with diverent meshes
- testings with several fvSolution options

- changing pEqn.H in buoyantPressure

- checking with laminar and turbulent flow characteristics

Summary:

- most simulations have a continuity problem (U_x,y,z) blow up and p_rgh too
- re-coarse the mesh did not solve the problem
- thermodynamics changing to perfectGas with air is working
- changing p_rgh (top) to fixedValue is working but the results are bad.

At the moment I am out of ideas - sorry.
Tobi is offline   Reply With Quote

Old   January 16, 2014, 05:13
Default
  #44
New Member
 
Bernhard
Join Date: May 2012
Location: Freiburg/Germany
Posts: 7
Rep Power: 7
BernhardS is on a distinguished road
Thanks for all your efforts, I also think that the thermophysical model is the problem. If I set the second coefficient for rho to zero the case is working...
BernhardS is offline   Reply With Quote

Old   January 17, 2014, 08:18
Default
  #45
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,806
Blog Entries: 6
Rep Power: 32
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Quote:
Originally Posted by BernhardS View Post
Thanks for all your efforts, I also think that the thermophysical model is the problem. If I set the second coefficient for rho to zero the case is working...
Additionally you can set g to (0 0 0)^T - it should give the same possibilty to solve the case but you need gravitation.
Tobi is offline   Reply With Quote

Old   March 3, 2014, 16:00
Default
  #46
nsf
Senior Member
 
Nicolas Edh
Join Date: Mar 2010
Location: Uppsala, Sweden
Posts: 119
Rep Power: 11
nsf is on a distinguished road
Quote:
Originally Posted by jherb View Post
Add the following line to your thermophysicalProperties:
Code:
dpdt no;
see:

[/code]
Hi all,

I might have an explanation of why the solution diverges when the density is non-constant and dpdt is on. I am hoping for your comments.

By using icoPolynomial we are setting the fluid as incompressible, i.e. \rho(p,T) = \rho(T). So we have, by definition:

\frac{\partial\rho}{\partial p} = 0

Which is what icoPolynomial returns when the function psi is called. For an ideal gas \frac{1}{RT} is returned. The compressibility can be expanded to

\frac{\partial\rho}{\partial t} \frac{\partial t}{\partial p} = 0

or

\frac{\partial\rho}{\partial t}\left[ \frac{\partial p}{\partial t}\right]^{-1} =0

So if we have non constant density, \frac{\partial\rho}{\partial t} \ne 0 and hence \frac{\partial p}{\partial t} must diverge?

Perhaps we would need and compressiblePolynomial class where the compressibility can be set even though it's really small for water?

Any thoughts?

Cheers
Nicolas
nsf is offline   Reply With Quote

Old   October 31, 2014, 09:33
Default
  #47
New Member
 
Ezequiel Fogliatto
Join Date: Aug 2012
Posts: 1
Rep Power: 0
efogliatto is on a distinguished road
Hi Bernhard,
I'm facing a similar problem when I try to use icoPolynomial in a closed cavity. Could you solve your case?
efogliatto is offline   Reply With Quote

Old   December 4, 2014, 04:59
Default
  #48
MK.
New Member
 
MK
Join Date: Oct 2014
Posts: 6
Rep Power: 4
MK. is on a distinguished road
Hi,

What kind of boundary conditions did you use? Could you be so nice and tell me which BC you used for the simulation with buoyantSimpleFoam, specially p and p_rgh. I am confused about these BC. I have changed the solver as recommended by Tom in the post.

Have a nice weekend,

MK.
MK. is offline   Reply With Quote

Old   December 26, 2014, 09:49
Default
  #49
New Member
 
a
Join Date: Nov 2013
Posts: 29
Rep Power: 5
minaret is on a distinguished road
Quote:
Originally Posted by Tobi View Post
Hi all,

now the pressure fields are the same (buoyantSimpleFoam and chtMultiRegionSimpleFoam) .

I had to change the schemes to get the same results


Now I am going to check if its working wit a bigger domain.
hi
I have continuity error with buoyantSimpleFoam
how did you change the schemes?
thanks
minaret is offline   Reply With Quote

Old   February 7, 2017, 10:48
Default BuoyantPimpleFoam crashes when using polynomial thermophysical properties
  #50
New Member
 
Antoine
Join Date: Jan 2016
Posts: 3
Rep Power: 3
antoine_hub is on a distinguished road
Hi everyone,

I am using OpenFOAM 4-1 and I would like to run the buoyantPimpleFoam tutorial "hotroom" with the polynomial properties. The problem is the same as many of you got earlier which is that the solver crashed after few iterations (here 1 ...) and which is the following:

Quote:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 4.1
Exec : buoyantPimpleFoam
Date : Feb 07 2017
Time : 14:27:43
Host : "workstation"
PID : 29230
Case : /home/antoine/OpenFOAM/antoine-4.1/run/heatTransfer/buoyantPimpleFoam/hotRoom
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


PIMPLE: Operating solver in PISO mode

Reading thermophysical properties

Selecting thermodynamics package
{
type heRhoThermo;
mixture pureMixture;
transport polynomial;
thermo hPolynomial;
energy sensibleEnthalpy;
equationOfState icoPolynomial;
specie specie;
}

Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type laminar

Reading g

Reading hRef
Calculating field g.h

Reading field p_rgh

Creating field dpdt

Creating field kinetic energy K

No MRF models present

Radiation model not active: radiationProperties not found
Selecting radiationModel none
No finite volume options present

Courant Number mean: 0 max: 0

Starting time loop

Courant Number mean: 0 max: 0
deltaT = 0.0012
Time = 0.0012

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 1.6982e-14, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 5.23806e-14, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 0.999992, Final residual = 0.00742046, No Iterations 8
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 4.1936e-08, global = 8.41042e-10, cumulative = 8.41042e-10
DICPCG: Solving for p_rgh, Initial residual = 0.971329, Final residual = 1.36506, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 5.85951e-07, global = 8.41042e-10, cumulative = 1.68208e-09
DICPCG: Solving for p_rgh, Initial residual = 0.97777, Final residual = 0.00967648, No Iterations 83
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.06797e-07, global = 8.41042e-10, cumulative = 2.52313e-09
DICPCG: Solving for p_rgh, Initial residual = 0.986932, Final residual = 8.90563e+07, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 9.63673, global = 8.41042e-10, cumulative = 3.36417e-09
ExecutionTime = 0.3 s ClockTime = 1 s

Courant Number mean: 9.24507 max: 26.4701
deltaT = 2.26671e-05
Time = 0.00122266707585703

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0.0532814, Final residual = 8.28644e-08, No Iterations 2
DILUPBiCG: Solving for Uy, Initial residual = 0.046897, Final residual = 7.8823e-08, No Iterations 2
DILUPBiCG: Solving for Uz, Initial residual = 0.0402159, Final residual = 1.72421e-10, No Iterations 3
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 4.72054e-08, No Iterations 3


--> FOAM FATAL ERROR:
Maximum number of iterations exceeded

From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hPolynomialThermo<Foam::icoPolynomial<Foam:: specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hPolynomialThermo<Foam ::icoPolynomial<Foam::specie> >, Foam::sensibleEnthalpy>]
in file /home/antoine/OpenFOAM/OpenFOAM-4.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam:olynomialTransport<Foam:: species::thermo<Foam::hPolynomialThermo<Foam::icoP olynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::calculate() at ??:?
#3 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam:olynomialTransport<Foam:: species::thermo<Foam::hPolynomialThermo<Foam::icoP olynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::correct() at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6 ? at ??:?
Aborted (core dumped)
I have followed the different advices given in this thread like:
*refining the mesh
*changing the pressure initialization in the solver or using funkySetFields to initialize the pressure
*modifying the relaxation factors in the fvSolution as well as increasing the number of inner and outer correctors
*using dpdt off/no

However, none of these solutions was solving my problem.

Has someone already had this problem before and solved it? Or do you have other any trick I could try to make it work?

Many thanks,

Antoine
antoine_hub is offline   Reply With Quote

Old   February 7, 2017, 11:01
Default
  #51
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,806
Blog Entries: 6
Rep Power: 32
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Dear Antionio,

please start with dt = 1e-7. You first time step is too big and therefore the courant number explodes already: Courant Number mean: 9.24507 max: 26.4701. That would be my first guess. Especially because you run in PISO mode
Code:
PIMPLE: Operating solver in PISO mode
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   February 7, 2017, 11:21
Default
  #52
New Member
 
Antoine
Join Date: Jan 2016
Posts: 3
Rep Power: 3
antoine_hub is on a distinguished road
Thanks for your quick answer Tobi.

Yes I tried this as well and the solver crashes during the third time step. Here is the log file.

Quote:
/*---------------------------------------------------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 4.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
Build : 4.1
Exec : buoyantPimpleFoam
Date : Feb 07 2017
Time : 15:16:35
Host : "workstation"
PID : 30239
Case : /home/antoine/OpenFOAM/antoine-4.1/run/heatTransfer/buoyantPimpleFoam/hotRoom
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0


PIMPLE: Operating solver in PISO mode

Reading thermophysical properties

Selecting thermodynamics package
{
type heRhoThermo;
mixture pureMixture;
transport polynomial;
thermo hPolynomial;
energy sensibleEnthalpy;
equationOfState icoPolynomial;
specie specie;
}

Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting turbulence model type laminar

Reading g

Reading hRef
Calculating field g.h

Reading field p_rgh

Creating field dpdt

Creating field kinetic energy K

No MRF models present

Radiation model not active: radiationProperties not found
Selecting radiationModel none
No finite volume options present

Courant Number mean: 0 max: 0

Starting time loop

Courant Number mean: 0 max: 0
deltaT = 1.2e-10
Time = 1.2e-10

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for Uy, Initial residual = 1, Final residual = 1.66064e-19, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0, Final residual = 0, No Iterations 0
DILUPBiCG: Solving for h, Initial residual = 0.0546701, Final residual = 1.0306e-22, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 1, Final residual = 0.00887971, No Iterations 77
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.05398e-16, global = 3.9305e-17, cumulative = 3.9305e-17
DICPCG: Solving for p_rgh, Initial residual = 0.491793, Final residual = 0.00240797, No Iterations 75
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.4897e-16, global = 4.3335e-17, cumulative = 8.264e-17
DICPCG: Solving for p_rgh, Initial residual = 0.57848, Final residual = 0.00314953, No Iterations 75
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.4878e-16, global = 4.3335e-17, cumulative = 1.25975e-16
DICPCG: Solving for p_rgh, Initial residual = 0.586074, Final residual = 8.47746e-09, No Iterations 155
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.38492e-16, global = 4.4141e-17, cumulative = 1.70116e-16
ExecutionTime = 0.12 s ClockTime = 0 s

Courant Number mean: 5.2325e-16 max: 2.01354e-14
deltaT = 1.44e-10
Time = 2.64e-10

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0.375238, Final residual = 5.06174e-17, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.425447, Final residual = 1.02992e-16, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.376789, Final residual = 9.52503e-17, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.109804, Final residual = 2.35794e-17, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 0.95771, Final residual = 12.2972, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.12464e-13, global = -7.97004e-17, cumulative = 9.04156e-17
DICPCG: Solving for p_rgh, Initial residual = 0.969428, Final residual = 0.00897822, No Iterations 8
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.06168e-14, global = -8.09331e-17, cumulative = 9.4825e-18
DICPCG: Solving for p_rgh, Initial residual = 0.725705, Final residual = 0.00585134, No Iterations 11
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.01544e-14, global = -8.03642e-17, cumulative = -7.08817e-17
DICPCG: Solving for p_rgh, Initial residual = 0.705409, Final residual = 1.3606, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 7.04522e-14, global = -8.13598e-17, cumulative = -1.52242e-16
ExecutionTime = 0.36 s ClockTime = 0 s

Courant Number mean: 8.14634e-14 max: 2.0581e-13
deltaT = 1.728e-10
Time = 4.368e-10

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0.389284, Final residual = 6.39416e-16, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.374786, Final residual = 6.94543e-17, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.636027, Final residual = 1.45355e-16, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 0.996707, Final residual = 6.67237e-16, No Iterations 1
DICPCG: Solving for p_rgh, Initial residual = 0.808542, Final residual = 1.16481e+09, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 0.000418179, global = -2.55172e-13, cumulative = -2.55324e-13
DICPCG: Solving for p_rgh, Initial residual = 0.999999, Final residual = 0.00614212, No Iterations 13
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 2.56852e-06, global = -2.55169e-13, cumulative = -5.10493e-13
DICPCG: Solving for p_rgh, Initial residual = 0.99982, Final residual = 0.00569006, No Iterations 14
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 1.46772e-08, global = -2.55171e-13, cumulative = -7.65664e-13
DICPCG: Solving for p_rgh, Initial residual = 0.96881, Final residual = 4.72076, No Iterations 1001
diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
time step continuity errors : sum local = 7.21886e-08, global = -2.5517e-13, cumulative = -1.02083e-12
ExecutionTime = 0.61 s ClockTime = 0 s

Courant Number mean: 1.41177e-07 max: 3.2514e-07
deltaT = 2.0736e-10
Time = 6.4416e-10

diagonal: Solving for rho, Initial residual = 0, Final residual = 0, No Iterations 0
PIMPLE: iteration 1
DILUPBiCG: Solving for Ux, Initial residual = 0.376711, Final residual = 2.2168e-15, No Iterations 1
DILUPBiCG: Solving for Uy, Initial residual = 0.412434, Final residual = 2.2696e-15, No Iterations 1
DILUPBiCG: Solving for Uz, Initial residual = 0.420672, Final residual = 2.49295e-15, No Iterations 1
DILUPBiCG: Solving for h, Initial residual = 1, Final residual = 6.01906e-15, No Iterations 1


--> FOAM FATAL ERROR:
Maximum number of iterations exceeded

From function Foam::scalar Foam::species::thermo<Thermo, Type>::T(Foam::scalar, Foam::scalar, Foam::scalar, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar, Foam::scalar) const, Foam::scalar (Foam::species::thermo<Thermo, Type>::*)(Foam::scalar) const) const [with Thermo = Foam::hPolynomialThermo<Foam::icoPolynomial<Foam:: specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hPolynomialThermo<Foam ::icoPolynomial<Foam::specie> >, Foam::sensibleEnthalpy>]
in file /home/antoine/OpenFOAM/OpenFOAM-4.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.

FOAM aborting

#0 Foam::error:rintStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam:olynomialTransport<Foam:: species::thermo<Foam::hPolynomialThermo<Foam::icoP olynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::calculate() at ??:?
#3 Foam::heRhoThermo<Foam::rhoThermo, Foam:ureMixture<Foam:olynomialTransport<Foam:: species::thermo<Foam::hPolynomialThermo<Foam::icoP olynomial<Foam::specie, 8>, 8>, Foam::sensibleEnthalpy>, 8> > >::correct() at ??:?
#4 ? at ??:?
#5 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6 ? at ??:?
Aborted (core dumped)
Many thanks,

Antoine
antoine_hub is offline   Reply With Quote

Old   February 7, 2017, 11:29
Default
  #53
Super Moderator
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,806
Blog Entries: 6
Rep Power: 32
Tobi has a spectacular aura aboutTobi has a spectacular aura about
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Your p_rgh solver has problems:
Code:
DICPCG:  Solving for p_rgh, Initial residual = 0.95771, Final residual = 12.2972, No Iterations 1001
  • You should use GAMG solver for pressure (speed up)
  • However, this will not solve your problem
  • Mesh problem
  • But I think you have a BC problem


Good luck,
__________________
Keep foaming,
Tobias Holzmann
Tobi is offline   Reply With Quote

Old   February 9, 2017, 08:51
Default
  #54
New Member
 
Antoine
Join Date: Jan 2016
Posts: 3
Rep Power: 3
antoine_hub is on a distinguished road
Thanks for your advice Tobias. I will investigate.

Cheers,

Antoine
antoine_hub is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On



All times are GMT -4. The time now is 20:23.