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

From Laminar to Turbulent FLow

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 23, 2019, 09:35
Default
  #21
Senior Member
 
Ruiyan Chen
Join Date: Jul 2016
Location: Hangzhou, China
Posts: 156
Rep Power: 6
cryabroad is on a distinguished road
I think the controlDict should be right now, because for steady-state simulations we set deltaT to 1, and endTime to the max number of iterations you want the solver to run for.

I took a brief look at your file, and still you have min/Max rho equals to 2.0 at the very beginning of the iterations. This value of 2.0 is what you set the maxRho to be. Therefore, this tells us that the actual density in your flow is already larger than 2.0. Any particular reason you are still bounding the densities? Since you are using rhoConst for the equation of state, what density did you set to your fluid?

Also, after you ran checkMesh, note that you have high non-orthogonal regions, please improve your mesh as well.
cryabroad is offline   Reply With Quote

Old   May 23, 2019, 10:59
Default
  #22
Senior Member
 
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 3
Raza Javed is on a distinguished road
I am sorry I couldn't get exactly where I am bounding my density, because in the thermophysical properties of fluid, I set it to 1000. I am attaching my thermophysical properties of fluid below:


Code:
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    location    "constant/fluid";
    object      thermophysicalProperties;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

mixture
{
    // Water

    specie
    {
        nMoles          1;
        molWeight       18;
    }
    equationOfState
    {
        rho             1000;
    }
    thermodynamics
    {
        Cp              4181;
        Hf              0;
    }
    transport
    {
        mu              959e-6;
        Pr              6.62;
    }
}

// ************************************************************************* //
Raza Javed is offline   Reply With Quote

Old   May 23, 2019, 23:38
Default
  #23
Senior Member
 
Ruiyan Chen
Join Date: Jul 2016
Location: Hangzhou, China
Posts: 156
Rep Power: 6
cryabroad is on a distinguished road
In the SIMPLE entry of your fvSolutions file, you have rhoMin of 0.2 and rhoMax of 2.0. I think if you get rid of these your case should run smoothly. One more thing, in the same entry you have set pRefCell and pRefValue (we need these for incompressible flow, otherwise the solver doesn't know what pressure to use), I personally would recommend using pRefPoint instead of pRefCell, unless you know your reference point for the pressure is indeed in cell 0. for pRefPoint you can set the coordinate of the reference point, like (0.0 0.0 1.0).

Btw just out of curiosity, what fluids are you simulating, looks to me to be liquid water?
cryabroad is offline   Reply With Quote

Old   May 24, 2019, 04:14
Default
  #24
Senior Member
 
Raza Javed
Join Date: Apr 2019
Location: Germany
Posts: 183
Rep Power: 3
Raza Javed is on a distinguished road
Thank you for your reply.


I removed these two entries of rhoMin and rhoMax from fvSolution file, and then the solver runs for 76sec, and before it was running for 35sec.


Then I changed the pRefCell to pRefPoint, but after that the solver still RUNS only for 76sec, and after that the same error comes.


The log file is given below:




Code:
Time = 74


Solving for fluid region fluid
DILUPBiCG:  Solving for Ux, Initial residual = 0.626649, Final residual = 0.04759457, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 0.5895491, Final residual = 0.03011316, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 0.4690052, Final residual = 0.03334807, No Iterations 2
DILUPBiCG:  Solving for h, Initial residual = 0.5372248, Final residual = 0.01909215, No Iterations 2
Min/max T:175.3879 319.9405
GAMG:  Solving for p_rgh, Initial residual = 0.601514, Final residual = 0.005827719, No Iterations 5
time step continuity errors : sum local = 76870, global = 3725.554, cumulative = -1018.419
Min/max rho:1000 1000

Solving for solid region box
DICPCG:  Solving for h, Initial residual = 0.01015602, Final residual = 0.0002773318, No Iterations 2
Min/max T:294.9693 301.3153

Solving for solid region plate1
DICPCG:  Solving for h, Initial residual = 0.01482085, Final residual = 0.0001559468, No Iterations 2
Min/max T:300.1433 300.905

Solving for solid region plate2
DICPCG:  Solving for h, Initial residual = 0.01324452, Final residual = 0.0001238401, No Iterations 2
Min/max T:300.146 300.9248

Solving for solid region plate3
DICPCG:  Solving for h, Initial residual = 0.01349652, Final residual = 0.0001322007, No Iterations 2
Min/max T:300.1422 300.9191
ExecutionTime = 41.95 s  ClockTime = 42 s

Time = 75


Solving for fluid region fluid
DILUPBiCG:  Solving for Ux, Initial residual = 0.5524515, Final residual = 0.03745622, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 0.514814, Final residual = 0.02340077, No Iterations 2
DILUPBiCG:  Solving for Uz, Initial residual = 0.410066, Final residual = 0.02328914, No Iterations 2
DILUPBiCG:  Solving for h, Initial residual = 0.4178126, Final residual = 0.01453362, No Iterations 2
Min/max T:-34.34473 332.0189
GAMG:  Solving for p_rgh, Initial residual = 0.7237737, Final residual = 0.005526134, No Iterations 4
time step continuity errors : sum local = 98527.33, global = 5650.649, cumulative = 4632.229
Min/max rho:1000 1000

Solving for solid region box
DICPCG:  Solving for h, Initial residual = 0.01065494, Final residual = 0.0004797391, No Iterations 2
Min/max T:285.1992 302.3668

Solving for solid region plate1
DICPCG:  Solving for h, Initial residual = 0.01462008, Final residual = 0.0001537349, No Iterations 2
Min/max T:300.1448 300.9088

Solving for solid region plate2
DICPCG:  Solving for h, Initial residual = 0.01308332, Final residual = 0.0001222664, No Iterations 2
Min/max T:300.1475 300.9285

Solving for solid region plate3
DICPCG:  Solving for h, Initial residual = 0.01334374, Final residual = 0.0001307139, No Iterations 2
Min/max T:300.1437 300.9227
ExecutionTime = 42.52 s  ClockTime = 43 s

Time = 76


Solving for fluid region fluid
DILUPBiCG:  Solving for Ux, Initial residual = 0.5800244, Final residual = 0.03650541, No Iterations 2
DILUPBiCG:  Solving for Uy, Initial residual = 0.5799028, Final residual = 0.009888277, No Iterations 3
DILUPBiCG:  Solving for Uz, Initial residual = 0.4281356, Final residual = 0.005665427, No Iterations 3
DILUPBiCG:  Solving for h, Initial residual = 0.5357228, Final residual = 0.01507815, No Iterations 2


--> 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::hConstThermo<Foam::rhoConst<Foam::specie> >; Type = Foam::sensibleEnthalpy; Foam::scalar = double; Foam::species::thermo<Thermo, Type> = Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy>]
    in file /home/ubuntu/OpenFOAM/OpenFOAM-4.1/src/thermophysicalModels/specie/lnInclude/thermoI.H at line 66.

FOAM aborting

#0  Foam::error::printStack(Foam::Ostream&) at ??:?
#1  Foam::error::abort() at ??:?
#2  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy> > > >::calculate() at ??:?
#3  Foam::heRhoThermo<Foam::rhoThermo, Foam::pureMixture<Foam::constTransport<Foam::species::thermo<Foam::hConstThermo<Foam::rhoConst<Foam::specie> >, Foam::sensibleEnthalpy> > > >::correct() at ??:?
#4  ? at ??:?
#5  __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#6  ? at ??:?
Aborted (core dumped)
Raza Javed is offline   Reply With Quote

Old   May 25, 2019, 05:16
Default
  #25
Senior Member
 
Ruiyan Chen
Join Date: Jul 2016
Location: Hangzhou, China
Posts: 156
Rep Power: 6
cryabroad is on a distinguished road
I don't think the errors you are getting now is related to the fluid dynamics part of your problem, everything (velocity, pressure) looks good. The min/max density is 1000, which is the value you set. During every iteration, it takes about 1-2 iterations for the velocity to converge, and more iterations for the pressure to converge, which is typical. I think the problem is more about heat transfer, as you noticed in the output for Time = 75, you are getting negative temperatures. Also, your continuity errors are quite large, that's not good. The means your velocity field doesn't satisfy the divergence free condition.

As I mentioned, I'm not familiar with this particular solver you are using, but normally heat transfer involving only fluid and solid under normal conditions should be easy. I would start from lowering the URFs, especially for pressure (I normally use ~0.3). Another thing is, your mesh has cells that have very high non-orthogonality, you should refine your mesh as well (or use at least 1 nNonOrthogonalCorrectors).

One way to check the problem is visualizing the results before the solver crashes, and identify suspicious locations. For example, which part is having negative temperatures? Another thing I would do is, instead of having 3 solid regions, how about we start from only 1?

Hope others who are familiar with this solver can check out your case. I've never used this solver so maybe this solver needs some special tunes?

Good luck,
Ruiyan
cryabroad is offline   Reply With Quote

Reply

Tags
fluid, laminar, openfoam, turbulent

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
Laminar and Turbulent flow of transient analysis gbrajtm Main CFD Forum 0 February 8, 2019 00:19
Issues on the simulation of high-speed compressible flow within turbomachinery dowlee OpenFOAM Running, Solving & CFD 8 October 25, 2016 20:48
Turbulent or laminar flow yansheng STAR-CCM+ 4 July 1, 2016 18:53
Do formula for Laminar and Turbulent Flow Calculation formulae change with Fluid Parag Gadgil FLUENT 0 June 19, 2012 08:07
Can I use turbulent model to solve a laminar flow? nikhil FLUENT 5 February 1, 2011 11:42


All times are GMT -4. The time now is 15:42.