Hi all I am trying to simu
 

Hi all

I am trying to simulate the standing wave formation in rhopsonicfoam solver. I am applying a timevaryingFixedVaalue patch at inlet for pressure and fixed value patch for velocity (with value v=0.001m/s). My simulation is going smooth if velocity is zero. but when velocity is some value like 0.001m/s the simulation crashes with high courant number at around 0.06 sec.
i m using vanLeer div scheme. and deltaT = 1e-5. can anybody suggest something?

Nishant

Hi Nishant rhopsonicFoam i
 

Hi Nishant

rhopsonicFoam is not using adaptive time stepping, thus try to follow the guidelines in the following thread to make the solver time adaptive (do not panic, it is rather straight forwardhttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif):

http://www.cfd-online.com/cgi-bin/Op...how.cgi?1/7583

Best regards,

Niels

Niels, Thanks for the prompt r
 

Niels, Thanks for the prompt reply.
I am rather not using the turbfoam solver. so the headers are not similar. I can not see courant.H header in my rhopSonic.C file.
However my case is still runing well with only changing the controldict file, WITHOUT recompiling the source.

The results are also not very encouraging and it also failed in a similar fashiion!

Nishant

Hi Nishant I meant that you
 

Hi Nishant

I meant that you should add the header files inside the time loop as suggested in the thread. That would give you the possibility of basing the time step on the Courant number. I do not believe that simply changing the controlDict will yield any differences at all.

Best regards,

Niels

Nishant Singh, look in to yo
 

Nishant Singh,
look in to your solver source, it should be like this:
int main(int argc, char *argv[])
{

# include "setRootCase.H"
# include "createTime.H"
# include "createMesh.H"
# include "readThermodynamicProperties.H"
# include "createFields.H"

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

Info<< "\nStarting time loop\n" << endl;

for (runTime++; !runTime.end(); runTime++)
{
Info<< "Time = " << runTime.value() << nl << endl;

# include "readPISOControls.H"
scalar HbyAblend = readScalar(piso.lookup("HbyAblend"));

# include "readTimeControls.H"

scalar CoNum = max
(
mesh.surfaceInterpolation::deltaCoeffs()
*mag(phiv)/mesh.magSf()
).value()*runTime.deltaT().value();

Info<< "Max Courant Number = " << CoNum << endl;

# include "setDeltaT.H"

if you can't find line #include "setDeltaT.H", than you must add it, otherwise, your task is given wrong

My rhopsonicFoam.c file is sam
 

My rhopsonicFoam.c file is same as shown above. (and i think this comes with OpenFoam-1.4.1 )But the result obtained is not encouraging. So I suspect there is some other problem.
I kept the initial internal field for U as (0 0 0). Do I need to keep some other initial value for U as this is a transient problem. Can anybody comment?

Nishant

Is your case internal/external
 

Is your case internal/external?
What BC's are using for U/p?

What is min/max cell volume?

Its a internal case. flow is i
 

Its a internal case. flow is inside the rectangular duct.
BCs are
p: internal field uniform 1;
Inlet- timevaryingfixedvalue
outlet - fixedValue 1

U: internalfield (0 0 0)
inlet - fixedvalue (0 0 0.001)
outlet - zerogradient

CheckMesh Reports:

Mesh stats
points: 169781
edges: 499380
faces: 489600
internal faces: 470400
cells: 160000
boundary patches: 6
point zones: 0
face zones: 0
cell zones: 0

Number of cells of each type:
hexahedra: 160000
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 0

Checking topology...
Boundary definition OK.
Point usage OK.
Upper triangular ordering OK.
Topological cell zip-up check OK.
Face vertices OK.
Face-face connectivity OK.
Number of regions: 1 (OK).

Checking patch topology for multiply connected surfaces ...
Patch Faces Points Surface
inlet 1600 1681 ok (not multiply connected)
outlet 1600 1681 ok (not multiply connected)
side1 4000 4141 ok (not multiply connected)
side2 4000 4141 ok (not multiply connected)
topWall 4000 4141 ok (not multiply connected)
bottomWall 4000 4141 ok (not multiply connected)

Checking geometry...
Domain bounding box: (0 0 0) (4 4 10)
Boundary openness (7.43763e-17 -3.33392e-18 1.76418e-16) OK.
Max cell openness = 8.67362e-17 OK.
Max aspect ratio = 1 OK.
Minumum face area = 0.01. Maximum face area = 0.01. Face area magnitudes OK.
Min volume = 0.001. Max volume = 0.001. Total volume = 160. Cell volumes OK.
Mesh non-orthogonality Max: 8.53774e-07 average: 0
Non-orthogonality check OK.
Face pyramids OK.
Max skewness = 8.82696e-14 OK.
Min/max edge length = 0.1 0.1 OK.
All angles in faces OK.
Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 1
All face flatness OK.

Mesh OK.

End

This is a laminar case and no
 

This is a laminar case and no turbulence model has been used.

Nishant

Hi Nishant Have you tried t
 

Hi Nishant

Have you tried to see what happens, if you as a first approach skip the timeVarying BC on p and put dp/pn=0. That would give you a nice channel flow, and if that succeeds, then you know your attention should be on your boudnary conditions.

I have a hunch which tells me that specifying Dirichlet on pressure in both ends and Dirichlet on the U at the inlet some what over-determines the system. The short story is that you have a pressure gradient which will be able to drive some net flux, but on the other hand you specify the flux by U: uniform (0 0 0.001), which makes it inconsistent.

Good luck and best regardshttp://www.cfd-online.com/OpenFOAM_D...part/happy.gif
- Niels

try using pressureInletVelocit
 

try using pressureInletVelocity for U at inlet

or outletInlet for pressure at inlet