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

Pressure instability with rhoSimpleFoam

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

Reply
 
LinkBack Thread Tools Display Modes
Old   September 18, 2006, 15:52
Default We have a need to run a pressu
  #1
New Member
 
Daniel Mills
Join Date: Mar 2009
Posts: 13
Rep Power: 8
daniel_mills is on a distinguished road
We have a need to run a pressure\density based compressible steady state solver. I have been fighting with rhoSimpleFoam for a few weeks now.

We would like to be able to specify:
2 inlets with TotalPressure using a fixed pressure.
2 outlets with possibilty of reverse flow and fixed static pressure.

I am currently using totalPressure with fixed values for the inlets and outletInlet for the outlets in the p file. I am using pressureInletVelocity for the inlets and inletOutlet for the outlets with the values set to 0 for the U file.

The flow field will develop a swirl as this runs.

The geometry checks fine using checkMesh.

This also runs fine in simpleFoam developing a fully converged solution.

For some reason when we run it with the pressure\density solver like rhoSimpleFoam we get an instability in pressure\density after a few hundred steps.

I have been able to change the instability by playing with the "phi -= pEqn.flux()" statement in the the code, but never actually get rid of it. I think the problem may reside pressure\density equation for the SIMPLE solvers.

Is OpenFoam capable of solving this type of problem?

HAS ANYONE BEEN ABLE TO SOLVE A PROBLEM SIMILAR TO WHAT I HAVE DESCRIBED WITH A STEADY STATE SOLVER?
daniel_mills is offline   Reply With Quote

Old   September 19, 2006, 15:03
Default I have noticed when someone as
  #2
New Member
 
Daniel Mills
Join Date: Mar 2009
Posts: 13
Rep Power: 8
daniel_mills is on a distinguished road
I have noticed when someone asks a question about stability problems in rhoSimpleFoam or density correctors in steady state solvers they are never answered. Here are two other posts posing similar questions from other users that never got further response. If there is a problem with rhoSimpleFoam thats alright, but it would be nice to get some sort of response?

Just tell me there is a problem and no one currently has a solution.

http://www.cfd-online.com/OpenFOAM_D...es/1/2068.html

http://www.cfd-online.com/OpenFOAM_D...es/1/2718.html
daniel_mills is offline   Reply With Quote

Old   September 19, 2006, 15:57
Default There's no problem in the solv
  #3
Senior Member
 
Hrvoje Jasak
Join Date: Mar 2009
Location: London, England
Posts: 1,758
Rep Power: 21
hjasak will become famous soon enough
There's no problem in the solver. What you are seeing is that compressible flows are much more sensitive to solver setting, initial field, time-step and boundary conditions. Unless you get all the components right together, the solver will blow up in your case.

All in all, this just requires lots of care.

Hrv
__________________
Hrvoje Jasak
Providing commercial FOAM/OpenFOAM and CFD Consulting: http://wikki.co.uk
hjasak is offline   Reply With Quote

Old   September 20, 2006, 09:48
Default Alright I can easily believe t
  #4
New Member
 
Daniel Mills
Join Date: Mar 2009
Posts: 13
Rep Power: 8
daniel_mills is on a distinguished road
Alright I can easily believe that the problem is in my setup somewhere. Maybe someone would be so kind as to spot where my potential problems are. I will post my checkMesh, fvSolution, fvSchemes, and my 0 files. Please anyone with any ideas let me know what else I should try. No matter what I try I seem to get what looks very much like a low wave mode pressure instability after about 500-600 steps.

Remember this mesh converges in simpleFoam. I also get much more stability by decreasing the pressure drop or increasing viscosity.



checkMesh:

Number of points: 124105
edges: 649440
faces: 979095
internal faces: 920158
cells: 453762
boundary patches: 19
point zones: 0
face zones: 0
cell zones: 0

Checking topology and geometry ...

Point usage check OK.

Upper triangular ordering OK.

Topological cell zip-up check OK.

Face vertices OK.

Face-face connectivity OK.

Basic topo ok ...

Checking patch topology for multiply connected surfaces ...

Patch Faces Points Surface

Periodic-Center 816 875 ok (not multiply connected)
Periodic-Combustor 16178 10957 ok (not multiply connected)
Periodic-Holes 328 204 ok (not multiply connected)
Periodic-Plenum-2 2792 1522 ok (not multiply connected)
Periodic-Plenum-1 2046 1095 ok (not multiply connected)
SmallTubes-2 2538 1324 ok (not multiply connected)
LargeTubes-2 3107 1707 ok (not multiply connected)
SmallTubes-1 2078 1092 ok (not multiply connected)
LargeTubes-1 6047 3191 ok (not multiply connected)
Wall-6 1032 687 ok (not multiply connected)
WallSet-5 7102 3751 ok (not multiply connected)
WallSet-4 3742 2016 ok (not multiply connected)
WallSet-2 4455 2328 ok (not multiply connected)
Wall-3 860 957 ok (not multiply connected)
Wall-1 742 409 ok (not multiply connected)
BC-PressOut-center 95 113 ok (not multiply connected)
BC-PressOut-1 3088 2180 ok (not multiply connected)
BC-PressInlet-2 1048 568 ok (not multiply connected)
BC-PressInlet-1 843 461 ok (not multiply connected)


Patch topo ok ...

Topology check done.

Domain bounding box: min = (-1.42109e-17 -2.75474e-51 0) max = (0.0757305 0.0245345 0.0245345) meters.

Checking geometry...

Boundary openness in x-direction = -4.32336e-18
Boundary openness in y-direction = -8.77453e-18
Boundary openness in z-direction = -3.35318e-18

Boundary closed (OK).

Max cell openness = 4.27239e-22 Max aspect ratio = 2.58574. All cells OK.

Minumum face area = 1.86851e-09. Maximum face area = 1.79996e-06. Face area magnitudes OK.

Min volume = 3.02777e-14. Max volume = 1.42021e-09. Total volume = 1.34424e-05. Cell volumes OK.

Mesh non-orthogonality Max: 65.6633 average: 17.5979

Non-orthogonality check OK.

Face pyramids OK.

Max skewness = 119.41 percent. Face skewness OK.

Minumum edge length = 5.08262e-05. Maximum edge length = 0.00214438.

All angles in faces are convex or less than 10 degrees concave.

Face flatness (1 = flat, 0 = butterfly) : average = 0.999994 min = 0.999846

All faces are flat in that the ratio between projected and actual area is > 0.8

Geometry check done.

Number of cells by type:

hexahedra: 19560
prisms: 44800
wedges: 0
pyramids: 285
tet wedges: 0
tetrahedra: 389117
polyhedra: 0

Number of regions: 1 (OK).

Mesh OK.


fvSolution: (note I update the relaxation values to .2 on p and .6 on everything else after about 150 steps. It continues to run fine for another 400 steps)


solvers

{
p AMG 1e-06 0 100;
U BICCG 1e-06 0;
h BICCG 1e-06 0;
k BICCG 1e-08 0;
epsilon BICCG 1e-08 0;
}

SIMPLE

{
nNonOrthogonalCorrectors 0;
pRefCell 0;
pRefValue 0;
}

relaxationFactors

{
p 0.05;
rho 0.05;
U 0.3;
h 0.1;
k 0.05;
epsilon 0.05;
}




fvSchemes:

ddtSchemes

{
default steadyState;
}

gradSchemes

{
default Gauss linear;
}

divSchemes

{
default none;
div(phi,U) Gauss limitedLinearV 1;
div(phi,k) Gauss upwind;
div(phi,epsilon) Gauss upwind;
div(phi,h) Gauss limitedLinear 1;
div((muEff*dev2(grad(U).T()))) Gauss linear;
}

laplacianSchemes

{
default none;
laplacian(muEff,U) Gauss linear limited 0.5;
laplacian((rho|A(U)),p) Gauss linear limited 0.5;
laplacian(alphaEff,h) Gauss linear limited 0.5;
laplacian(DkEff,k) Gauss linear limited 0.5;
laplacian(DepsilonEff,epsilon) Gauss linear limited 0.5;
laplacian(mut,U) Gauss linear limited 0.5;
}

interpolationSchemes

{
default linear;
interpolate(U) linear;
}

snGradSchemes

{
default corrected;
}

fluxRequired

{
default no;
p;
}


Epsilon: (note I crash almost immediately when I run laminar. I also get increased stability by fiddling with viscosity.)

dimensions [0 2 -3 0 0 0 0];

internalField uniform 1.5;

boundaryField

{
Periodic-Center
{
type cyclic;
}
Periodic-Combustor
{
type cyclic;
}
Periodic-Holes
{
type cyclic;
}
Periodic-Plenum-2
{
type cyclic;
}
Periodic-Plenum-1
{
type cyclic;
}
SmallTubes-2
{
type zeroGradient;
}
LargeTubes-2
{
type zeroGradient;
}
SmallTubes-1
{
type zeroGradient;
}
LargeTubes-1
{
type zeroGradient;
}
Wall-6
{
type zeroGradient;
}
WallSet-5
{
type zeroGradient;
}
WallSet-4
{
type zeroGradient;
}
WallSet-2
{
type zeroGradient;
}
Wall-3
{
type zeroGradient;
}
Wall-1
{
type zeroGradient;
}
BC-PressOut-center
{
type inletOutlet;
inletValue uniform 1.5;
}
BC-PressOut-1
{
type inletOutlet;
inletValue uniform 1.5;
}
BC-PressInlet-2
{
type fixedValue;
value uniform 1.5;
}
BC-PressInlet-1
{
type fixedValue;
value uniform 1.5;
}


k:

dimensions [0 2 -2 0 0 0 0];

internalField uniform 0.055;

boundaryField

{
Periodic-Center
{
type cyclic;
}
Periodic-Combustor
{
type cyclic;
}
Periodic-Holes
{
type cyclic;
}
Periodic-Plenum-2
{
type cyclic;
}
Periodic-Plenum-1
{
type cyclic;
}
SmallTubes-2
{
type zeroGradient;
}
LargeTubes-2
{
type zeroGradient;
}
SmallTubes-1
}
type zeroGradient;
}
LargeTubes-1
{
type zeroGradient;
}
Wall-6
{
type zeroGradient;
}
WallSet-5
{
type zeroGradient;
}
WallSet-4
{
type zeroGradient;
}
WallSet-2
{
type zeroGradient;
}
Wall-3
{
type zeroGradient;
}
Wall-1
{
type zeroGradient;
}
BC-PressOut-center
{
type inletOutlet;
inletValue uniform .055;
}
BC-PressOut-1
}
type inletOutlet;
inletValue uniform .055;
}
BC-PressInlet-2
{
type fixedValue;
value uniform .055;
}
BC-PressInlet-1
{
type fixedValue;
value uniform .055;
}


p: (note I have also tried totalPressure and fixed value for the outlet)

dimensions [1 -1 -2 0 0 0 0];

internalField uniform 102928;

boundaryField
{
Periodic-Center
{
type cyclic;
}
Periodic-Combustor
{
type cyclic;
}
Periodic-Holes
{
type cyclic;
}
Periodic-Plenum-2
{
type cyclic;
}
Periodic-Plenum-1
{
type cyclic;
}
SmallTubes-2
{
type zeroGradient;
}
LargeTubes-2
{
type zeroGradient;
}
SmallTubes-1
{
type zeroGradient;
}
LargeTubes-1
{
type zeroGradient;
}
Wall-6
{
type zeroGradient;
}
WallSet-5
{
type zeroGradient;
}
WallSet-4
{
type zeroGradient;
}
WallSet-2
{
type zeroGradient;
}
Wall-3
{
type zeroGradient;
}
Wall-1
{
type zeroGradient;
}
BC-PressOut-center
{
type fixedValue;
value uniform 101325;
}
BC-PressOut-1
{
type fixedValue;
value uniform 101325;
}
BC-PressInlet-2
{
type totalPressure;
p0 uniform 104531;
value uniform 104531;
}
BC-PressInlet-1
{
type totalPressure;
p0 uniform 104531;
value uniform 104531;
}


T:

dimensions [0 0 0 1 0 0 0];

internalField uniform 300;

boundaryField
{
Periodic-Center
{
type cyclic;
}
Periodic-Combustor
{
type cyclic;
}
Periodic-Holes
{
type cyclic;
}
Periodic-Plenum-2
{
type cyclic;
}
Periodic-Plenum-1
{
type cyclic;
}
SmallTubes-2
{
type zeroGradient;
}
LargeTubes-2
{
type zeroGradient;
}
SmallTubes-1
{
type zeroGradient;
}
LargeTubes-1
{
type zeroGradient;
}
Wall-6
{
type zeroGradient;
}
WallSet-5
{
type zeroGradient;
}
WallSet-4
{
type zeroGradient;
}
WallSet-2
{
type zeroGradient;
}
Wall-3
{
type zeroGradient;
}
Wall-1
{
type zeroGradient;
}
BC-PressOut-center
{
type inletOutlet;
inletValue uniform 300;
}
BC-PressOut-1
{
type inletOutlet;
inletValue uniform 300;
}
BC-PressInlet-2
{
type fixedValue;
value uniform 300;
}
BC-PressInlet-1
{
type fixedValue;
value uniform 300;
}


U: (note I have also tried pressureInletOutletVelocity for the outlet)

dimensions [0 1 -1 0 0 0 0];

internalField uniform (1 0.1 0.1);

boundaryField
{
Periodic-Center
{
type cyclic;
}
Periodic-Combustor
{
type cyclic;
}
Periodic-Holes
{
type cyclic;
}
Periodic-Plenum-2
{
type cyclic;
}
Periodic-Plenum-1
{
type cyclic;
}
SmallTubes-2
{
type fixedValue;
value uniform (0 0 0);
}
LargeTubes-2
{
type fixedValue;
value uniform (0 0 0);
}
SmallTubes-1
{
type fixedValue;
value uniform (0 0 0);
}
LargeTubes-1
{
type fixedValue;
value uniform (0 0 0);
}
Wall-6
{
type fixedValue;
value uniform (0 0 0);
}
WallSet-5
{
type fixedValue;
value uniform (0 0 0);
}
WallSet-4
{
type fixedValue;
value uniform (0 0 0);
}
WallSet-2
{
type fixedValue;
value uniform (0 0 0);
}
Wall-3
{
type fixedValue;
value uniform (0 0 0);
}
Wall-1
{
type fixedValue;
value uniform (0 0 0);
}
BC-PressOut-center
{
type inletOutlet;
inletValue uniform (0 0 0);
}
BC-PressOut-1
{
type inletOutlet;
inletValue uniform (0 0 0);
}
BC-PressInlet-2
{
type pressureInletVelocity;
phi phi;
rho rho;
value uniform (0 0 0);
}
BC-PressInlet-1
{
type pressureInletVelocity;
phi phi;
rho rho;
value uniform (0 0 0);
}
daniel_mills is offline   Reply With Quote

Old   September 21, 2006, 12:35
Default Even though this should be a l
  #5
New Member
 
Daniel Mills
Join Date: Mar 2009
Posts: 13
Rep Power: 8
daniel_mills is on a distinguished road
Even though this should be a low mach number(<0.3) would it still make sense to experiment with the pressureTransmissive outlet BC since it seems to be a growing oscillating pressure wave in a cylinder that seems to be causing the problems???
daniel_mills is offline   Reply With Quote

Old   September 22, 2006, 06:28
Default Hi Daniel, Your set-up seem
  #6
Member
 
Pierre Le Fur
Join Date: Mar 2009
Location: UK
Posts: 60
Rep Power: 8
pierre is on a distinguished road
Hi Daniel,

Your set-up seems fine. Apart from that "low wave instabiltiy" what happens to the other fields, do they converge towards reasonable values, do they oscillate consequently too?
You can always try to take the immoral and cowardly step of using upwind for all your variables. Maybe you might also try to tighten your pressure solver tolerance.

Take it easy

Pierre
pierre is offline   Reply With Quote

Old   September 22, 2006, 06:33
Default probably try one of the transi
  #7
Senior Member
 
Markus Hartinger
Join Date: Mar 2009
Posts: 102
Rep Power: 8
hartinger is on a distinguished road
probably try one of the transient codes like rhoSonicFoam and rhopSonicFoam. Using different codes helps spotting errors in the setup.

The total pressure boundary condition should be alright.

markus
hartinger is offline   Reply With Quote

Old   September 22, 2006, 08:02
Default Thank you very much for your r
  #8
New Member
 
Daniel Mills
Join Date: Mar 2009
Posts: 13
Rep Power: 8
daniel_mills is on a distinguished road
Thank you very much for your replies,

We get the same thing when upwinding all values and I have tried playing with the tolerances of pressure, it still develops a unstable pressure wave.

The problem with pressure is usually preluded by a sharp drop in the minimum Ux. A drop from around -33 to around -60. After a couple steps velocity is back to normal, but pressure develops a growing oscillating wave. Rho of course ocsillates with pressure. Temperature and velocity look pretty good for a few steps until variance in pressure begins driving them.

We have played with rhoTurbFoam a little but haven't spent much time with the transient codes yet.
daniel_mills is offline   Reply With Quote

Old   September 22, 2006, 08:14
Default As Markus suggested maybe rhop
  #9
Member
 
Pierre Le Fur
Join Date: Mar 2009
Location: UK
Posts: 60
Rep Power: 8
pierre is on a distinguished road
As Markus suggested maybe rhopSonicFoam might help, as it uses a slightly different way of biulding fluxes. Quite a stable code I hear.

Pierre
pierre is offline   Reply With Quote

Old   September 26, 2006, 15:59
Default Does anyone have anything else
  #10
New Member
 
Daniel Mills
Join Date: Mar 2009
Posts: 13
Rep Power: 8
daniel_mills is on a distinguished road
Does anyone have anything else we can try on this? We get the low wave pressure mode on both rhoTurbFoam and rhoSimpleFoam. It always develops in the channel(cylinder). It always develops after the swirling flow field begins to setup. We have tried more generic cases and the problem persists. The swirl develops then pressure oscillates and becomes unstable.

We have began trying rhopSonicFoam, but have not gotten very far.

Any other suggestions would be a great help.

Thanks
daniel_mills is offline   Reply With Quote

Old   December 5, 2010, 07:59
Default
  #11
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
Quote:
Originally Posted by daniel_mills View Post
Does anyone have anything else we can try on this? We get the low wave pressure mode on both rhoTurbFoam and rhoSimpleFoam. It always develops in the channel(cylinder). It always develops after the swirling flow field begins to setup. We have tried more generic cases and the problem persists. The swirl develops then pressure oscillates and becomes unstable.

We have began trying rhopSonicFoam, but have not gotten very far.

Any other suggestions would be a great help.

Thanks
Hi Daniel,

Did you solve your issue?
If not, I will post my issue here. If affirmatively, I will try your solution.

Regards,

Guilherme
aerothermal is offline   Reply With Quote

Old   December 5, 2010, 18:05
Default
  #12
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Hi, the last comment before yours is from 2006. It is probably more convenient if you open a new thread, and maybe provide a sample case that reproduces the problem.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 5, 2010, 21:52
Default
  #13
Senior Member
 
aerothermal's Avatar
 
Guilherme da Silva
Join Date: Aug 2010
Location: Sao Paulo - Brazil
Posts: 105
Rep Power: 6
aerothermal is on a distinguished road
Hi Alberto,

The last post is from 2006 but the user joined in 2009!
Certainly I will open a new thread. Thanks.


Regards,

Guilherme
aerothermal is offline   Reply With Quote

Old   December 6, 2010, 00:03
Default
  #14
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Oh, I guess this is due to the forum migration.
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 27, 2010, 04:42
Default solver for steady compressible flow in OpenFOAM 1.7.1
  #15
New Member
 
rock.senthilkumar's Avatar
 
senthilkumar.R
Join Date: Sep 2010
Location: Ranchi, India
Posts: 20
Rep Power: 6
rock.senthilkumar is on a distinguished road
Hai all,
I am new to OpenFoam.With my experience in Fluent ( simulated supersonic flow at Mach number 2.2 over Gemini Reentry capsule) thought to try OF. Simulation condition of my Fluent work is steady, Density based, M=2.2, inviscid both inviscid and turbulent flow. So far , I converted my fluent mesh file (.msh) as OpenFOAM mesh file. For steady , compressible flow rhoSimpleFoam seems to be a equivalent solver, but in OpenFOAM 1.7.1 (which is the one I installed in my machine) only rhoPorousSimpleFoam solver is available. Kindly explain what does this porous in rhoPorousSimpleFoam means for, and suggest me with correct solver.. Thanks in advance.

Quote:
Originally Posted by alberto View Post
Oh, I guess this is due to the forum migration.
__________________
Senthil Kumar. R
Department of space Engineering and Rocketry,
Birla Institute of Technology,Mesra.
rock.senthilkumar@gmail.com
rock.senthilkumar is offline   Reply With Quote

Old   December 27, 2010, 04:50
Default
  #16
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
rhoSimpleFoam is part of OpenFOAM 1.7.1
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 27, 2010, 12:23
Post
  #17
New Member
 
rock.senthilkumar's Avatar
 
senthilkumar.R
Join Date: Sep 2010
Location: Ranchi, India
Posts: 20
Rep Power: 6
rock.senthilkumar is on a distinguished road
Dear Alberto,
I would like to thank you for your reply . And I feel very Sorry for my mistake., can you please suggest me any other solver other than rhoSimpleFoam for my case..
__________________
Senthil Kumar. R
Department of space Engineering and Rocketry,
Birla Institute of Technology,Mesra.
rock.senthilkumar@gmail.com
rock.senthilkumar is offline   Reply With Quote

Old   December 27, 2010, 14:04
Default
  #18
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
rhoSimpleFoam is the only compressible steady solver available.

There is rhoCentralFoam, which is suitable for viscid/inviscid flows with high Mach number, but it is unsteady. Similarly, sonicFoam is fine for transonic/supersonic turbulent unsteady flows.

Best,
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto is offline   Reply With Quote

Old   December 27, 2010, 14:30
Default
  #19
New Member
 
rock.senthilkumar's Avatar
 
senthilkumar.R
Join Date: Sep 2010
Location: Ranchi, India
Posts: 20
Rep Power: 6
rock.senthilkumar is on a distinguished road
Dear Alberto,
Thanks a lot for your reply.Now I decided the rhoSimpleFoam solver for my work. Sorry for bothering you again, Kindly send any test case for rhoSimpleFoam to my mail id rock.senthilkumar@gmail.com ., so that I can do any case study also.


Quote:
Originally Posted by alberto View Post
rhoSimpleFoam is the only compressible steady solver available.

There is rhoCentralFoam, which is suitable for viscid/inviscid flows with high Mach number, but it is unsteady. Similarly, sonicFoam is fine for transonic/supersonic turbulent unsteady flows.

Best,
__________________
Senthil Kumar. R
Department of space Engineering and Rocketry,
Birla Institute of Technology,Mesra.
rock.senthilkumar@gmail.com
rock.senthilkumar is offline   Reply With Quote

Old   December 27, 2010, 14:34
Default
  #20
Senior Member
 
Alberto Passalacqua
Join Date: Mar 2009
Location: Ames, Iowa, United States
Posts: 1,894
Rep Power: 26
alberto will become famous soon enoughalberto will become famous soon enough
Take a look at the tutorials :-)
__________________
Alberto Passalacqua

GeekoCFD - A free distribution based on openSUSE 64 bit with CFD tools, including OpenFOAM. Available as live DVD/USB, hard drive image and virtual image.
OpenQBMM - An open-source implementation of quadrature-based moment methods
alberto 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
BC for rhoSimpleFoam uli_u OpenFOAM Running, Solving & CFD 77 April 4, 2013 11:28
RhoSimpleFoam maritozzo OpenFOAM Running, Solving & CFD 1 April 30, 2010 18:18
RhoSimpleFoam jphandrigan OpenFOAM Running, Solving & CFD 18 March 29, 2009 11:05
RhoSimpleFoam negative pressure gzink OpenFOAM Running, Solving & CFD 10 June 4, 2007 05:35
RhoSimpleFoam luca OpenFOAM Running, Solving & CFD 0 August 22, 2005 12:26


All times are GMT -4. The time now is 23:35.