[Tobi]

Dear Carno,

• Please use code tags (the first post)
• Is your problem related to the problem described here?
• What problem do you actually have? Providing all files is senseless

Good luck,

[Carno]

Sorry for the confusion. Again thanks for the reply.
Please find attached the picture of the problem. In this the inlet and outlet of the wind tunnel are seen.
Inlet and outlet atm. total pressure.
Fan speed: 2400rpm
if required I can upload the case also.
My problem is the error as pasted below after just 3 iterations,

$ rhosimpleFoam
/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3                                   |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
/*   Windows 32 and 64 bit porting by blueCAPE: http://www.bluecape.com.pt   *\
|  Based on Windows porting (2.0.x v4) by Symscape: http://www.symscape.com   |
\*---------------------------------------------------------------------------*/
Build  : 2.3-7bcdf589cfaa
Exec   : E:/PROGRA~2/BLUECF~1.3/OpenFOAM-2.3/platforms/linuxmingw-w64DPOpt/bin/rhosimpleFoam.exe
Date   : Jul 05 2016
Time   : 11:09:43
Host   : "SP-005"
PID    : 9248
Case   : 
nProcs : 1
SigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

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

Create mesh for time = 0


SIMPLE: convergence criteria
    field U      tolerance 0.0001
    field omega  tolerance 0.0001
    field k      tolerance 0.0001
    field h      tolerance 0.0001
    field p      tolerance 0.0001

Reading thermophysical properties

Selecting thermodynamics package
{
    type            hePsiThermo;
    mixture         pureMixture;
    transport       const;
    thermo          hConst;
    equationOfState perfectGas;
    specie          specie;
    energy          sensibleEnthalpy;
}

Reading field U

Reading/calculating face flux field phi

Creating turbulence model

Selecting RAS turbulence model kOmegaSST
kOmegaSSTCoeffs
{
    beta1           0.075;
    beta2           0.0828;
    c1              10;
    F3              false;
    betaStar        0.09;
    b1              1;
    alphaOmega1     0.5;
    gamma2          0.4403;
    a1              0.31;
    alphaOmega2     0.85616;
    gamma1          0.5532;
    Prt             1;
    alphaK2         1;
    alphaK1         0.85034;
}

Creating finite volume options from fvOptions

Selecting finite volume options model type MRFSource
    Source: volume_rotor_RotatingFrame
    - applying source for all time
    - selecting cells using cellZone volume_rotor
    - selected 718966 cell(s) with volume 0.6299373


Starting time loop

forces forces:
    Not including porosity effects

Time = 1

DILUPBiCG:  Solving for Ux, Initial residual = 1, Final residual = 0.001208181, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 1, Final residual = 0.001165042, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 1, Final residual = 0.001168873, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.5087361, Final residual = 0.0005684527, No Iterations 1
GAMG:  Solving for p, Initial residual = 1, Final residual = 0.004860938, No Iterations 14
GAMG:  Solving for p, Initial residual = 0.80171, Final residual = 0.007509924, No Iterations 2
time step continuity errors : sum local = 0.3719482, global = 0.0004397649, cumulative = 0.0004397649
rho max/min : 2.044925 1.054925
DILUPBiCG:  Solving for omega, Initial residual = 0.006431888, Final residual = 7.051876e-006, No Iterations 1
bounding omega, min: -97.3309 max: 10887.77 average: 336.3591
DILUPBiCG:  Solving for k, Initial residual = 1, Final residual = 0.001160957, No Iterations 1
ExecutionTime = 28.967 s  ClockTime = 29 s

forces forces output:
    sum of forces:
        pressure : (-899605.5 1591.197 82.94594)
        viscous  : (-7.870473 0.08385379 -0.01845338)
        porous   : (0 0 0)
    sum of moments:
        pressure : (302652.8 384.7494 7704.933)
        viscous  : (65.02162 0.08545086 0.3926327)
        porous   : (0 0 0)

Time = 2

DILUPBiCG:  Solving for Ux, Initial residual = 0.5047674, Final residual = 0.001111357, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.7303689, Final residual = 0.001712937, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.7270983, Final residual = 0.001712452, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 1, Final residual = 0.001870025, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.2711847, Final residual = 0.002301069, No Iterations 8
GAMG:  Solving for p, Initial residual = 0.1710556, Final residual = 0.0008337344, No Iterations 3
time step continuity errors : sum local = 0.1683412, global = -0.002403294, cumulative = -0.001963529
rho max/min : 2.840433 0.9594328
DILUPBiCG:  Solving for omega, Initial residual = 0.05179233, Final residual = 9.097313e-005, No Iterations 1
bounding omega, min: -21.0178 max: 4.475544e+007 average: 1380.209
DILUPBiCG:  Solving for k, Initial residual = 0.6845529, Final residual = 0.0008470325, No Iterations 1
ExecutionTime = 47.062 s  ClockTime = 47 s

forces forces output:
    sum of forces:
        pressure : (-918968.3 1524.961 103.2043)
        viscous  : (-6.779444 -0.293652 -0.4734017)
        porous   : (0 0 0)
    sum of moments:
        pressure : (306471.3 294.5037 7422.213)
        viscous  : (64.44063 1.755617 -0.8498381)
        porous   : (0 0 0)

Time = 3

DILUPBiCG:  Solving for Ux, Initial residual = 0.1646682, Final residual = 0.0003629798, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.2946895, Final residual = 0.0006918891, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.2940873, Final residual = 0.0006919726, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.3497916, Final residual = 0.000794688, No Iterations 1


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

    From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const
    in file P:/OPENFO~1.3/OpenFOAM-2.3/src/thermophysicalModels/specie/lnInclude/../thermo/thermo/thermoI.H at line 76.

FOAM aborting

Thanks a lot.

[Tobi]

Hi,

as you can see, your rho is somehow starting to blow up and I think it is due to your turbulence settings or somehow related to that. I hope that you have under-relaxation for omega too (omega is blowing up too).

Another way to check out the problem is to save each iteration and check out the results. If you want more than 3, you have to reduce your relaxation factors.

Good luck

[Carno]

Ok. I have managed to do up to 70, but did not save results. I will do now and let you know.

[Carno]

Please find attached some plots before blowing up after 77th iteration. I am planning to change to k-e turbulence model. The forces output is also not practical (axis of rotation is x axis). Under-relaxation are at 0.01, this is also something I am not happy with.

Below are some the few iterations before blowing up:

Time = 74

DILUPBiCG:  Solving for Ux, Initial residual = 0.0016068, Final residual = 2.942787e-008, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.02447367, Final residual = 4.696535e-007, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.02484658, Final residual = 4.818262e-007, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.007868051, Final residual = 1.453934e-007, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.8710183, Final residual = 0.005953933, No Iterations 5
GAMG:  Solving for p, Initial residual = 0.2143385, Final residual = 0.001296351, No Iterations 3
time step continuity errors : sum local = 0.06567112, global = 0.0004610975, cumulative = 0.001395762
rho max/min : 5.425856 0.6043491
DILUPBiCG:  Solving for omega, Initial residual = 0.0001321104, Final residual = 2.229225e-009, No Iterations 1
DILUPBiCG:  Solving for k, Initial residual = 0.001264901, Final residual = 2.230363e-008, No Iterations 1
ExecutionTime = 1790.409 s  ClockTime = 1790 s

forces forces output:
    sum of forces:
        pressure : (-119495.8 -8.68136 37.04536)
        viscous  : (0.9753639 -0.1774745 -0.06073789)
        porous   : (0 0 0)
    sum of moments:
        pressure : (39797.91 7.085947 137.5878)
        viscous  : (2.52183 0.3243306 -0.815964)
        porous   : (0 0 0)

Time = 75

DILUPBiCG:  Solving for Ux, Initial residual = 0.0014298, Final residual = 2.611228e-008, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.02205032, Final residual = 4.2032e-007, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.02281876, Final residual = 4.409009e-007, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.008515087, Final residual = 1.584947e-007, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.8703139, Final residual = 0.006404774, No Iterations 5
GAMG:  Solving for p, Initial residual = 0.2276821, Final residual = 0.001520347, No Iterations 3
time step continuity errors : sum local = 0.07802001, global = 0.0004286407, cumulative = 0.001824403
rho max/min : 5.471597 0.5993056
DILUPBiCG:  Solving for omega, Initial residual = 0.0001324695, Final residual = 2.243347e-009, No Iterations 1
DILUPBiCG:  Solving for k, Initial residual = 0.001219343, Final residual = 2.153197e-008, No Iterations 1
ExecutionTime = 1812.054 s  ClockTime = 1812 s

forces forces output:
    sum of forces:
        pressure : (-109906 0.06622584 52.64534)
        viscous  : (1.080065 -0.1744566 -0.05967288)
        porous   : (0 0 0)
    sum of moments:
        pressure : (36503.47 -20.19777 193.9374)
        viscous  : (2.53353 0.3219708 -0.802274)
        porous   : (0 0 0)

Time = 76

DILUPBiCG:  Solving for Ux, Initial residual = 0.001280855, Final residual = 2.329567e-008, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.01984538, Final residual = 3.752663e-007, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.02087654, Final residual = 4.009792e-007, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.009183481, Final residual = 1.719931e-007, No Iterations 1
GAMG:  Solving for p, Initial residual = 0.8691126, Final residual = 0.007156285, No Iterations 5
GAMG:  Solving for p, Initial residual = 0.2411567, Final residual = 0.001989359, No Iterations 3
time step continuity errors : sum local = 0.1029002, global = 0.0003322396, cumulative = 0.002156642
rho max/min : 5.516881 0.5943126
DILUPBiCG:  Solving for omega, Initial residual = 0.0001322716, Final residual = 2.247858e-009, No Iterations 1
DILUPBiCG:  Solving for k, Initial residual = 0.001177052, Final residual = 2.078855e-008, No Iterations 1
ExecutionTime = 1833.554 s  ClockTime = 1834 s

forces forces output:
    sum of forces:
        pressure : (-99363.48 21.30831 61.30617)
        viscous  : (1.174318 -0.1747786 -0.05766641)
        porous   : (0 0 0)
    sum of moments:
        pressure : (32896.46 -12.13509 304.8201)
        viscous  : (2.543182 0.3170202 -0.8048378)
        porous   : (0 0 0)

Time = 77

DILUPBiCG:  Solving for Ux, Initial residual = 0.001152901, Final residual = 2.088103e-008, No Iterations 1
DILUPBiCG:  Solving for Uy, Initial residual = 0.01782562, Final residual = 3.336711e-007, No Iterations 1
DILUPBiCG:  Solving for Uz, Initial residual = 0.01907107, Final residual = 3.635077e-007, No Iterations 1
DILUPBiCG:  Solving for h, Initial residual = 0.009829574, Final residual = 1.854111e-007, No Iterations 1


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

    From function thermo<Thermo, Type>::T(scalar f, scalar T0, scalar (thermo<Thermo, Type>::*F)(const scalar) const, scalar (thermo<Thermo, Type>::*dFdT)(const scalar) const, scalar (thermo<Thermo, Type>::*limit)(const scalar) const) const
    in file P:/OPENFO~1.3/OpenFOAM-2.3/src/thermophysicalModels/specie/lnInclude/../thermo/thermo/thermoI.H at line 76.

FOAM aborting

[Tobi]

I am not sure about transonic problems but are your BC for p and U, k, epsilon are correct? What you have for U? IF you have totalPressure you should use adjusted fluxes there (pressureInletOutletVelocity). If I get your simulation correct you set a fixedValue for the velocity at the inlet. Normally you should set p to zero here (but I am not sure if you do it in transonic and I am to lazy to check the numerics for this ?elliptic? problem).

For k and omega / epsilon I would use turbulentIntensity... and mixingLength... BC.

Even k-Omega is not a good choice for far field flows.

[Carno]

Do you mean this for U?

inlet
	{
		type	pressureInletOutletVelocity;
		value	uniform (0.0 0.0 0.0);
	}
	outlet
	{
		type	pressureInletOutletVelocity;
		value	uniform (0.0 0.0 0.0);
	}

k BC

	inlet
	{
		type	turbulentIntensityKineticEnergyInlet;
		value	uniform 1.0;
		intensity	0.05;
	}
	outlet
	{
		type	inletOutlet;
		inletValue	uniform 1.0;

omega BC

inlet
	{
		type	compressible::turbulentMixingLengthFrequencyInlet;
		value	uniform 1.0;
		mixingLength	0.001;
	}
	outlet
	{
		type	compressible::turbulentMixingLengthFrequencyInlet;
		value	uniform 1.0;
		mixingLength	0.001;

[Tobi]

Yes,

for the outlet you can also use inletOutlet or zeroGradient (if you have no recirculation).

If you set up U and p like you did, then I do not know where the driving force is for the flow? (:

p equal inlet / outlet
U based on p , no pressure gradient -> no flow. In other words, I guess that your BC are somehow different to that one you posted.

[Carno]

I have pasted the BCs from my working directory. The fan is creating the flow. It is rotating at 2400 rpm.
Do you think this is wrong modelling? In other CFD software this is typical.

[Tobi]

Aaa I am sorry (to many things in my mind)... I was thinking that you have a flow around something

In that kind of simulation, it should be fine. But totalPressure at the outlet can be changed to zeroGradient (finally totalPressure should act as zeroGradient there). For numerical stabilisation you also can check the following:

Set the rotating speed to 1/3 of the official or even less. Start calculating and after 500 iterations check the result (I would use k-epsilon for the first start). Then use the latest solution and increase the RPM's.

[Carno]

Thanks for the suggestions. I am trying slowly ramping the speed now. Apart from that I am trying Gauss vanLeerV for div(phi,U)