CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Fluid Flow and Heat Transfer in a Mixing Elbow (http://www.cfd-online.com/Forums/openfoam-solving/60205-fluid-flow-heat-transfer-mixing-elbow.html)

atzaru May 14, 2006 14:59

Hello Foam users i am tryin
 
Hello Foam users

i am trying to simulate Fluid Flow and Heat Transfer in a Mixing Elbow (a problem similar with the one in fluent tutorials).

the file can be downloaded here

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif MixingElbow.tar.bz2


hen i run the case i obtain always:


BICCG: Solving for Ux: solution singularity
BICCG: Solving for Uy: solution singularity
BICCG: Solving for h: solution singularity
ICCG: Solving for pd: solution singularity
time step continuity errors : sum local = nan, global = nan, cumulative = nan
rho max/min : 0 0
ExecutionTime = 0.34 s ClockTime = 0 s


Can anybody have a look on my file and give me a hint?
thanks
Atzaru

gschaider May 15, 2006 11:52

Try checkMesh . MixingElbow
 
Try

checkMesh . MixingElbow

Amongst other things it says

--> FOAM Serious Error :
From function primitiveMesh::checkClosedBoundary(const bool report) const
in file meshes/primitiveMesh/primitiveMeshCheck.C at line 91

And for 800 cells it says

High aspect ratio for cell 0: 1.59475e+197

IMHO you'll have a hard time to simulate anything on that mesh.

gschaider May 15, 2006 12:00

One more remark: blockMesh com
 
One more remark: blockMesh complains about negative volumes (which is a strong indication for problems)

I think the problem is somewhere in your blockMeshDict

atzaru May 17, 2006 08:07

Bernhard thanks a lot for your
 
Bernhard thanks a lot for your sugestions. I corrected the geometry but it seems there is another problem

I attached again my case

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif MixingElbow.tar.gz

Here is what the openFoam reports when stops iterating after only 4 time steps:

Time = 4

BICCG: Solving for Ux, Initial residual = 0.331866, Final residual = 8.91692e-07, No Iterations 6
BICCG: Solving for Uy, Initial residual = 0.223996, Final residual = 8.35056e-06, No Iterations 6
BICCG: Solving for h, Initial residual = 0.274355, Final residual = 1.56448e-06, No Iterations 6


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

From function specieThermo<thermo>::T(scalar f, scalar T0, scalar (specieThermo<thermo>::*F)(const scalar) const, scalar (specieThermo<thermo>::*dFdT)(const scalar) const) const
in file /home/dm2/henry/OpenFOAM/OpenFOAM-1.3/src/thermophysicalModels/specie/lnInclude/specieThermoI.H at line 83.

FOAM aborting

Foam::error::printStack(Foam:http://www.cfd-online.com/OpenFOAM_D...part/proud.gifstream&)
Foam::error::abort()
Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hconstthermo<foam::per fectgas> > > > >::calculate()
Foam::hThermo<foam::puremixture<foam::consttranspo rt<foam::speciethermo<foam::hconstthermo<foam::per fectgas> > > > >::correct()
buoyantSimpleFoam [0x805cf48]
__libc_start_main
__gxx_personality_v0

Anybody had a similar problem?

atzaru

gschaider May 17, 2006 10:53

Hi Atzaru. Try what I alway
 
Hi Atzaru.

Try what I always do: write out the solution at every timestep and look for strange pheomena. In your case that means: negative temperatures near the outlet at t=3 (which might cause problems for the perfect gas ...)

However. When I looked at the velocities at t=1 they were even stranger: velocities of up to 180 in the straight part that leads to the oulet, and they drop just before the bend. So I suspect there is still a problem with your blockMesh (but I'm not using that very often so I can't help you there, sorry)

atzaru May 17, 2006 13:35

Thanks again Bernhard for your
 
Thanks again Bernhard for your answer.

I suspect a bug in the solver because i have done a test using the same geometry and i just change the solver from buoyantSimpleFoam to the transient one buoyantFoam and it works ....the results looks as expected (so the geometry and mesh is good). I will try also to run my case in the OpenFoam version 1.2 and see if it runs or not.

In the buoyantSimpleFoam i keep receiving:






BICCG: Solving for Ux: solution singularity
BICCG: Solving for Uy: solution singularity
BICCG: Solving for h: solution singularity
ICCG: Solving for pd: solution singularity
time step continuity errors : sum local = nan, global = nan, cumulative = nan
rho max/min : nan nan
BICCG: Solving for epsilon: solution singularity
BICCG: Solving for k: solution singularity
ExecutionTime = 0.66 s ClockTime = 1 s

Can it be a bug in the solver or i am doing a stupid mistake?

Does anybody had similar experience with buoyantSimpleFoam ? Or does anybody have a similar working example and can email it to me?


http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif MixingElbow_tr.tar.gz -transient case works

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif MixingElbow.tar.gz -steady state case does not run

Atzaru

gschaider May 17, 2006 14:34

OK. I did two minor modificati
 
OK. I did two minor modifications (to the case from your 6:07am posting):

Change the IC for U from (0.2 0 0) to (0 0 0) and set g in the environmentalProperties to (0 0 0).

Now it runs and the result looks reasonable. But don't ask me why (maybe someone who knows more about the buoyant-solvers can tell you about the problem)

atzaru May 17, 2006 17:47

Hi Bernhard You are right,
 
Hi Bernhard

You are right, if i change the case to the particular one u have suggested it will run and the solution is believable. This is verys strange ...

I try also to switch from laminar to k-eps model and again the error appears.

Maybe Mr Hrvoje Jasak have some suggestions (or is a bug in the code?)?


Any suggestion will be appreciated
Atzaru

hjasak May 18, 2006 08:33

Well: (I don't feel obliged
 
Well:

(I don't feel obliged to answer all these questions because my time is very much in demand, so please go easy on calling out names. Also, it's been more than 10 years since I've meed a Mister) :-)

Of course, no bug in the code. I get:

Exec : buoyantSimpleFoam /home/hjasak/OpenFOAM/hjasak-1.3/run/support MixingElbow
Date : May 18 2006
Time : 08:33:59
Host : wooster
PID : 14907
Root : /home/hjasak/OpenFOAM/hjasak-1.3/run/support
Case : MixingElbow
Nprocs : 1
Create time

Create mesh for time = 0


Reading environmentalProperties
Reading thermophysical properties

Selecting thermodynamics package hThermo<puremixture<consttransport<speciethermo<hc onstthermo<perfectgas>>>>>
Floating exception


and that would be because your internal field for the temperature is set to zero!!!!.

Do yourself a favour and set the following in the .cshrc (or equivalent) - it will help you.

setenv FOAM_SIGFPE 1
setenv FOAM_SETNAN 1


Until next time,

Hrv

atzaru May 19, 2006 02:06

Thank you for your kind answer
 
Thank you for your kind answer. I will be more careful next time

Atzaru


All times are GMT -4. The time now is 00:06.