[JaimeFdz]

Hi guys,

I am new in CFD online and also in multiregion problems in OpenFOAM, so I hope it doesn't sound stupid my problem.

The problem I'm facing is a 2D aerothermal problem, which I already simulated in Fluent (y+ obtained is 1.6, the maximum) and now I'm triying in OpenFOAM. The geometry is a NACA profile in air domain with inlet, outlet and ciclic conditions in top and bottom; with subsonic velocity and two holes in the profile with cte temperature.

This are the steps I followed:

• fluentMeshToFoam
• change boundary in polymesh to make cyclic the top and bottom; make mappedWall the interfaces of metal and air
• checkMesh
• splitMeshRegions -cellZones -overwrite

I have the next problem:

--> FOAM FATAL ERROR:
Negative initial temperature T0: -243006.5

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::hConstThermo<Foam::perfectGas<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::per fectGas<Foam::specie> >, Foam::sensibleEnthalpy>]
in file /home/luiscssz/OpenFOAM/OpenFOAM-6/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 54.

FOAM aborting

#0 Foam::error::printStack(Foam::Ostream&) at ??:?
#1 Foam::error::abort() at ??:?
#2 Foam::species::thermo<Foam::hConstThermo<Foam::per fectGas<Foam::specie> >, Foam::sensibleEnthalpy>::THs(double, double, double) const at ??:?
#3 Foam::heRhoThermo<Foam::rhoReactionThermo, Foam::SpecieMixture<Foam::singleComponentMixture<F oam::constTransport<Foam::species::thermo<Foam::hC onstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::calculate() at ??:?
#4 Foam::heRhoThermo<Foam::rhoReactionThermo, Foam::SpecieMixture<Foam::singleComponentMixture<F oam::constTransport<Foam::species::thermo<Foam::hC onstThermo<Foam::perfectGas<Foam::specie> >, Foam::sensibleEnthalpy> > > > >::correct() at ??:?
#5 ? in "/home/luiscssz/OpenFOAM/OpenFOAM-6/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam"
#6 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#7 ? in "/home/luiscssz/OpenFOAM/OpenFOAM-6/platforms/linux64GccDPInt32Opt/bin/chtMultiRegionFoam"

I also fixed the temperature in fvOptions

limitT
{
type limitTemperature;
active yes;
min 100;
max 450;
selectionMode all;
}

but I don't know what can I do now, any hep is wecome
I attach the log file, and the rest of files.

Thank you for your time,

Jaime

[Bloerb]

Your settings seem reasonable, some error messages in the log file for some missing uniform keywords in some boundary files here and there but that shouldn't matter.

You could try to solve the flow with a nonThermal solver like simpleFoam and initialize the flow field (U) with that calculation.
Does it work without the cyclic conditions? with slip walls or noSlip walls?

What was the result form checkMesh?

Maybe check the defintion of the residuals in fvSolution. I am not using the foundation version a lot, since your time step and courant number are crazy high. Since you are running it in simple mode this should however work.

This might however just be because of your turbulence conditions. The intensisity seems extremly low 0.001. You might want to solve it with simpleFoam and get reasonable estimates for k and omega to set as initial values for the internalField

[JaimeFdz]

Thank you very much Bloerb, I'm going to try with your suggestions.

This is the checkMesh:


Mesh stats
points: 4801112
internal points: 0
faces: 9563135
internal faces: 4761923
cells: 2387526
faces per cell: 5.999959
boundary patches: 9
point zones: 0
face zones: 0
cell zones: 0

Overall number of cells of each type:
hexahedra: 2387428
prisms: 98
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Cell to face addressing OK.
Point usage OK.
Upper triangular ordering OK.
Face vertices OK.
*Number of regions: 2
The mesh has multiple regions which are not connected by any face.
<<Writing region information to "0/cellToRegion"
<<Writing region 0 with 49032 cells to cellSet region0
<<Writing region 1 with 2338494 cells to cellSet region1

Checking patch topology for multiply connected surfaces...
Patch Faces Points Surface topology
ns_metal_to_air 2002 4004 ok (non-closed singly connected)
ns_o_inlet 567 1134 ok (non-closed singly connected)
ns_o_outlet 572 1144 ok (non-closed singly connected)
ns_a_top 1372 2746 ok (non-closed singly connected)
ns_a_bottom 1372 2746 ok (non-closed singly connected)
ns_a_inlet 170 342 ok (non-closed singly connected)
ns_air_to_metal 19935 39870 ok (non-closed singly connected)
ns_a_outlet 170 342 ok (non-closed singly connected)
frontAndBackPlanes 4775052 4801112 ok (non-closed singly connected)

Checking geometry...
Overall domain bounding box (-0.3 -0.08460433 -0.02356084) (2.05 0.08460433 0.02356084)
Mesh has 2 geometric (non-empty/wedge) directions (1 1 0)
Mesh has 2 solution (non-empty) directions (1 1 0)
All edges aligned with or perpendicular to non-empty directions.
Boundary openness (5.992487e-17 5.677612e-16 -4.039284e-19) OK.
Max cell openness = 3.09335e-16 OK.
Max aspect ratio = 6.629027 OK.
Minimum face area = 6.711132e-11. Maximum face area = 0.0002820796. Face area magnitudes OK.
Min volume = 3.162398e-12. Max volume = 2.807682e-07. Total volume = 0.01871278. Cell volumes OK.
Mesh non-orthogonality Max: 45.64205 average: 9.439424
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 0.8797299 OK.
Coupled point location match (average 0) OK.

Mesh OK.

[peterhess]

In p_rgh fluid.

Replace:

ns_air_to_metal
{
type zeroGradient;
}

with:

ns_air_to_metal
{

type fixedFluxPressure;
value uniform 44000;
}

And:

ns_a_outlet
{
type inletOutlet;
value uniform 44000;
inletValue uniform 41504;
}

with:

ns_a_outlet
{
type fixedValue;
value uniform 44000;
}

------------------------------

In T fluid.

Replace:

ns_a_outlet
{
type zeroGradient;
value $internalField;
//inletValue uniform 280;
}


with:

ns_a_outlet
{
type inletOutlet;
value uniform 300;
inletValue uniform 300;
}