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

Simulating standing wave in rhopSonicFoam solver

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 7, 2008, 10:02
Default Hi all I am trying to simu
  #1
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 7
nishant_hull is on a distinguished road
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
__________________
Thanks and regards,

Nishant
nishant_hull is offline   Reply With Quote

Old   May 7, 2008, 10:19
Default Hi Nishant rhopsonicFoam i
  #2
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,528
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
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 forward):

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

Best regards,

Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   May 7, 2008, 12:20
Default Niels, Thanks for the prompt r
  #3
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 7
nishant_hull is on a distinguished road
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
__________________
Thanks and regards,

Nishant
nishant_hull is offline   Reply With Quote

Old   May 7, 2008, 16:09
Default Hi Nishant I meant that you
  #4
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,528
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
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
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   May 7, 2008, 16:21
Default Nishant Singh, look in to yo
  #5
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7
mkraposhin is on a distinguished road
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
mkraposhin is offline   Reply With Quote

Old   May 7, 2008, 17:55
Default My rhopsonicFoam.c file is sam
  #6
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 7
nishant_hull is on a distinguished road
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
__________________
Thanks and regards,

Nishant
nishant_hull is offline   Reply With Quote

Old   May 8, 2008, 02:12
Default Is your case internal/external
  #7
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7
mkraposhin is on a distinguished road
Is your case internal/external?
What BC's are using for U/p?

What is min/max cell volume?
mkraposhin is offline   Reply With Quote

Old   May 8, 2008, 07:33
Default Its a internal case. flow is i
  #8
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 7
nishant_hull is on a distinguished road
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
__________________
Thanks and regards,

Nishant
nishant_hull is offline   Reply With Quote

Old   May 8, 2008, 07:59
Default This is a laminar case and no
  #9
Senior Member
 
Nishant
Join Date: Mar 2009
Location: Glasgow, UK
Posts: 165
Rep Power: 7
nishant_hull is on a distinguished road
This is a laminar case and no turbulence model has been used.

Nishant
__________________
Thanks and regards,

Nishant
nishant_hull is offline   Reply With Quote

Old   May 8, 2008, 08:17
Default Hi Nishant Have you tried t
  #10
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Rotterdam, The Netherlands
Posts: 1,528
Rep Power: 23
ngj will become famous soon enoughngj will become famous soon enough
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 regards
- Niels
__________________
Please note that I do not use the Friend-feature, so do not be offended, if I do not accept a request.
ngj is offline   Reply With Quote

Old   May 8, 2008, 10:48
Default try using pressureInletVelocit
  #11
Senior Member
 
mkraposhin's Avatar
 
Matvej Kraposhin
Join Date: Mar 2009
Location: Moscow, Russian Federation
Posts: 172
Rep Power: 7
mkraposhin is on a distinguished road
try using pressureInletVelocity for U at inlet

or outletInlet for pressure at inlet
mkraposhin is offline   Reply With Quote

Reply

Thread Tools
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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
SonicTurbFoam Vs rhopSonicFoam vishal OpenFOAM Running, Solving & CFD 0 January 29, 2009 00:58
RhopSonicFoam reference abhishek OpenFOAM Running, Solving & CFD 0 November 5, 2006 22:43
Viscous rhopSonicFoam didomenico OpenFOAM Running, Solving & CFD 0 February 9, 2006 02:29
RhopSonicFoam didomenico OpenFOAM Running, Solving & CFD 0 October 3, 2005 10:53
Standing Cylinder Garvin Forrester Main CFD Forum 1 June 15, 2001 14:28


All times are GMT -4. The time now is 08:08.