[miquelvinya]

Hi all,

I have made a geometry that is basically a cube with an inlet of fresh air (298K) and an outlet of wasted hot air, walls at 303 K, ground at 298K and ceiling at 308K. I fix the inlet velocity as 1 m/s and gravity in environmental properties. All I want is to simulate the profile for the air between inlet and outlet.

Here there are 2 pictures of the case:



When I run the case I obtain:

#0 Foam::error::printStack(Foam:stream&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xffffe420]
#3 Foam::compressible::turbulenceModels::kEpsilon::kE psilon(Foam::GeometricField<double,> const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenceModels.so"
#4 Foam::compressible::turbulenceModel::adddictionary ConstructorToTable<foam::compressible::turbulencem odels::kepsilon>::New(Foam::GeometricField<double, > const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenceModels.so"
#5 Foam::compressible::turbulenceModel::New(Foam::Geo metricField<double,> const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenceModels.so"
#6 main in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/buoyantFoam"
#7 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#8 Foam::regIOobject::readIfModified() in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/buoyantFoam"

Is there anything that I forget?

Thank you!!
Miquel

[prashant24983]

I believe there is something wrong with the internal field that you have initialised in k epsilon file... Make sure that they are not initialised to zero

[miquelvinya]

Thanks Prashant,

I tryed your option because I forgot k and epsilon values for the internal field, but the problem persists with the same message...

#0 Foam::error::printStack(Foam:stream&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xffffe420]
#3 Foam::compressible::turbulenceModels::kEpsilon::kE psilon(Foam::GeometricField<do uble,> const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenc eModels.so"
#4 Foam::compressible::turbulenceModel::adddictionary ConstructorToTable<foam::compr essible::turbulencemodels::kepsilon>::New(Foam::Ge ometricField<double,> const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenc eModels.so"
#5 Foam::compressible::turbulenceModel::New(Foam::Geo metricField<double,> const&, Foam::GeometricField<foam::vector<double>, Foam::fvPatchField, Foam::volMesh> const&, Foam::GeometricField<double,> const&, Foam::basicThermo&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libcompressibleTurbulenc eModels.so"
#6 main in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/buoyantFoam "
#7 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#8 Foam::regIOobject::readIfModified() in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/buoyantFoam "

Wha can I try now? Thanks in advance,
Miquel

[prashant24983]

Check the R file in the 0 directory, just like in the buoyantFoam tutorial set the internalField likewise

dimensions [0 2 -2 0 0 0 0];
internalField uniform (0 0 0 0 0 0 0 0 0)

followed by the patches, I believe the zeroGradient patch should work.

If the problem persists I believe the problem is with the implementation of boundary conditions.

Can you post the case or mail it at prashantojha@gmail.com

[miquelvinya]

I would specially thank to Prashant for helping me.

I changed intitial conditions such as k, epsilon and pressure. With this there is no zerodivision problem. And then I reduced timestep to 0.05 s.

Here there are the results:


=)
Miquel

[miquelvinya]

The next step was to create a more complex case based in the above described. When I try to run the case the solver shows me this message:

Create time

Create mesh for time = 0


Reading environmentalProperties
Reading thermophysical properties

Selecting thermodynamics package hThermo<puremixture<consttransport<speciethermo<hc onstthermo<perfectgas>>>>>
#0 Foam::error::printStack(Foam:stream&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#1 Foam::sigFpe::sigFpeHandler(int) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libOpenFOAM.so"
#2 Uninterpreted: [0xffffe420]
#3 Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hc onstthermo<foam::perfectgas> > > > >::calculate() in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysicalMo dels.so"
#4 Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hc onstthermo<foam::perfectgas> > > > >::hThermo(Foam::fvMesh const&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysicalMo dels.so"
#5 Foam::basicThermo::addfvMeshConstructorToTable<foa m::hthermo<foam::puremixture<f oam::consttransport<foam::speciethermo<foam::hcons tthermo<foam::perfectgas> > > > > >::New(Foam::fvMesh const&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysicalMo dels.so"
#6 Foam::basicThermo::New(Foam::fvMesh const&) in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/lib/linuxGccDPOpt/libbasicThermophysicalMo dels.so"
#7 main in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/buoyantFoam "
#8 __libc_start_main in "/lib/tls/i686/cmov/libc.so.6"
#9 Foam::regIOobject::readIfModified() in "/home/mvinya/OpenFOAM/OpenFOAM-1.4.1/applications/bin/linuxGccDPOpt/buoyantFoam "

What can I do now? Thank you!!
Miquel

[prashant24983]

are you trying to add aother specie in the previous case? What complexities are you talking about?

[miquelvinya]

Hello!

The geometry is more complex and there are surfaces up to T = 473 K. Is the buoyantFoam thermodynamic package prepared for these temperatures? Must I change the solver?

Thank you!
Miquel

[girogirozakk]

Excuse me.

I want to know what type of boundary aer there?
Now , I try same-type calculation.
But , I cannot understand what type of boundary "Inlet Hole" & "Outlet Hole".

I tried "freestreem" or "atmosphere" , but cannot calc.
So , I cannot understand to set U,p ,etc..

Please teach me the setting.


Sorry,I'm not good English-speaker , my sentence is Hard to read...




Thank you!
Giro.

[miquelvinya]

Hello,

The values used for my first buoyantFoam simulation were:

INLET

- Type: inlet
- U_y = 0.1 m/s
- k = 0.1
- epsilon = 0.01
- P = 1.0E5 Pa
- T = 295 K

OUTLET

- Type: outlet
- U = 0.0 m/s
- k = 0.1
- epsilon = 0.01
- P = 1.0E5 Pa

WALLS

- Type: fixedTemperatureWallFunction
- U = 0.0 m/s
- k = 0.1
- epsilon = 0.01
- P = 1.0E5 Pa
- T = 303 K

INTERNAL FIELD

- U = 0.0 m/s
- k = 0.1
- epsilon = 0.01
- P = 1.0E5 Pa
- T = 298 K

My simulaion has 90.000 tetrahedra and I fixed dt=0.001 s.

My new simulation crashes. Probably is because wall temperaturea are above 373K.

Is air thermodynamic package prepared for properties at that temperature (hThermo...)??

If not, why my crash report shows me a sigFpe message??



Thanks for your attention,
Miquel

[prashant24983]

Please check your thermoPhysicalProperties file.

Try this for Air instead of previous form... Hope this helps.

mixture air 1 28.9 1000 2.544e+06 1.8e-05 0.7;

[girogirozakk]

Thanks !
I could get some result for my calc.

Giro

[miquelvinya]

Thanks Prashant,

The case is correctly running.

Regards,
Miquel

[ep4]

Hi,

i'm trying to use the solver buoyantFoam for natural convection and having some difficulties: temperatures increasing untill the simulation crashes.

I would like to make a simple test. I have a flat plate case wich gives satisfying results with turbFoam. I would like to reproduce these results with buoyantFoam, setting g= (0 0 0) in the envireonnemental properties (no buoyancy effects) and using constant temperature boundaries, equal to the initial intern field (no heat transfer phenomenons). However, it doesn't work. I have also tried with adiabatic boundaries. For each case, i obtain after several time steps temperature of order of 10000000 K !!

It makes me think to stability problems. Using the Euler or backwrd time schemes which are implicit (User Guide U-112), i don't understand, with my theoritical knowledge of CFD, why i encounter problems of stability.
I have similar problems with buoyantSimpleFoam.

Could someone say me what i'm doing wrong?

Thank you

Eric

[prashant24983]

Use "fixedFluxBuoyantPressure" for the flat plate boundary at "p". I think the problem is in getting the boundary conditions right. Can you paste your "p" boundary condition here?

[ep4]

Hi everybody,

i have changed the intern initial velocity field by (10 0 0) in place of (0 0 0). It is more stable, i mean, the really high temperatures appear later...

Any idea to help me?

Thank you

[prashant24983]

Hello Pattyn,

I have realized that the code for buoyantFoam and buoyantSimpleFoam has changed considerably from version 1.4.1 to 1.5. Even though, I am not very clear about the declaration of pd and p in version 1.5, I can help you with some basics based on how I understand the buoyantFoam from version 1.4.1.

pd is dynamic pressure. In the simple form is 0.5*rho*V^2. In your declaration of pd you provide a '0' value to fluid coming in and going out. Which I must say is not right. For inlet and outlet provide a zeroGradient boundary condition.

Also make sure that you are not providing a fixedValue boundary condition for inlet and outlet patches in 'T'

Most times your solution may blow up because of the courant number.Check the courant number as your iterations progresses.

I have few questions, What is Up? is it wall? if its not then your pd should look something like this.

internalField uniform 0;

boundaryField
{
WallDown
{
type fixedFluxBuoyantPressure;
value uniform 0;
}

Inlet
{
type zeroGradient;
}

Outlet
{
type zeroGradient;
}

Up
{
type zeroGradient;
}
frontAndBack
{
type empty;
}
}

[prashant24983]

If your boundary conditions are not right, this leads to wrong calculation of the pEqn which eventually results in irrational p values, and irrational velocities.. so your maximum courant number eventually will make you worry!

[prashant24983]

Hello Eric,

Its really difficult to say what might be the exact trouble!

If you are using turbulence do you observe bounding errors? Just switch off turbulence and see if the error remains.

If possible send your case to me prashantojha@gmail.com

Though, I can look at it only tomorrow.

Regards,

[ep4]

Thank you for your help. I'm going to search a solution this afternoon and if it doesn't work i will send the case to you.

I have the impression that the problem could come from the T file given that the case runs well with turbFoam.

It appears me logical tu use a fixed temperature at the inlet and the plate, a zeroGradient condition at the boundary Up (infront of the plate).
And i'm wondering if it would be possible no to impose anything at the Outlet. It is not logical for me to impose a temperature or a gradient at this boundary.

Any comments?

Thank you