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

Pressure driven cd nozzle flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   March 3, 2015, 20:52
Default Pressure driven cd nozzle flow
  #1
New Member
 
SRIKANTH C S
Join Date: Feb 2014
Posts: 2
Rep Power: 0
srikanthcs93 is on a distinguished road
hello,
i am trying to simulate a pressure driven flow through a convergent divergent nozzle using rhoCentralFoam
conditions given to me are:
nozzle inlet-Po-1.028 bar
ambient inflow-Po-1.007 bar
total temperature-300k
outflow-p-1 bar.
pressure-
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object p;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform 1.01325;

boundaryField
{

inlet
{
type totalPressure;
p0 uniform 1.028;
U U;
phi phi;
rho rho;
psi none;
gamma 1.4;
}
ambientinlet
{
type totalPressure;
p0 uniform 1.007;
U U;
phi phi;
rho rho;
psi none;
gamma 1.4;
}


outlet
{
type waveTransmissive;
field p;
phi phi;
rho rho;
psi thermosi;
gamma 1.4;
fieldInf 1;
lInf 50;
value uniform 1;
}
bottom
{
type symmetryPlane;
}

obstacle
{
type zeroGradient;
}
top
{
type zeroGradient;
}
defaultFaces
{
type empty;
}
}
Velocity-
FoamFile
{
version 2.0;
format ascii;
class volVectorField;
object U;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

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

internalField uniform (0 0 0);

boundaryField
{
inlet
{
type zeroGradient;
}
ambientinlet
{
type zeroGradient;
}

outlet
{
type zeroGradient;

}

bottom
{
type symmetryPlane;
}
obstacle
{
type fixedValue;
value uniform (0 0 0);
}
top
{
type zeroGradient;
}

defaultFaces
{
type empty;
}
}
Temperature-
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object T;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 1 0 0 0];

internalField uniform 300;

boundaryField
{
inlet
{
type totalTemperature;
gamma 1.4;
T0 uniform 300;
value uniform 300;
}
ambientinlet
{
type zeroGradient;
}
outlet
{
type zeroGradient;
}


obstacle
{
type zeroGradient;
}
top
{
type zeroGradient;
}
bottom
{
type symmetryPlane;
}
defaultFaces
{
type empty;
}
}
inlet-nozzle inlet
ambientinlet-ambient inflow
obstacle-nozzle profile
bottom-bottom of the whole domain
top-top boundary
outlet-outlet for the whole domain.

i have attached the geometry, grid and Mach plot for the above described case.I am not able to understand the strange flow pattern in the nozzle region( if i increase the nozzle pressure to 2 bar or above , this problem doesn't exist) . I think there is some problem with the boundary conditions but i am not able to figure it out.Kindly, help me solve this issue.
thank you
srikanth
Attached Images
File Type: jpg nozzlepic.jpg (40.9 KB, 26 views)
File Type: jpg result.jpg (41.5 KB, 29 views)
File Type: jpg grid.jpg (59.4 KB, 22 views)
srikanthcs93 is offline   Reply With Quote

Old   March 6, 2015, 10:07
Default
  #2
New Member
 
Join Date: Nov 2014
Posts: 8
Rep Power: 2
mkiewat is on a distinguished road
To me, it looks like you are generating pressure waves at the sharp corner where the fluid exits into the big rectangular section. Those pressure waves travel downstream (you can see them slightly in the blue region of your Mach-number field). For low pressure differences they also manage to travel upstream into the nozzle where they get reflected from the inlet and interact on the way back with incoming waves. For Mach>1 this can't happen, of course. Does anyone else have a thought?
mkiewat is offline   Reply With Quote

Old   March 6, 2015, 10:28
Default
  #3
New Member
 
SRIKANTH C S
Join Date: Feb 2014
Posts: 2
Rep Power: 0
srikanthcs93 is on a distinguished road
hey thanks for the reply.So, what do you think i should do??
srikanthcs93 is offline   Reply With Quote

Old   March 6, 2015, 11:05
Default
  #4
New Member
 
Join Date: Nov 2014
Posts: 8
Rep Power: 2
mkiewat is on a distinguished road
Since there are no non-reflecting inlet BCs (that I know of), i would extend your inlet into a big box. In that box you can apply your pressure BC. Within that box, you can either coarsen the mesh towards the inlet boundary so that the short wavelength pressure waves are filtered out or use a small porous medium right after the inlet boundary which also damps the pressure waves and should prevent reflections.
mkiewat is offline   Reply With Quote

Old   April 17, 2015, 15:40
Default
  #5
New Member
 
Jason Pearl
Join Date: Jul 2013
Location: Burlington
Posts: 10
Rep Power: 4
jaason is on a distinguished road
Hi Srikanth,
Ive been working on nozzle simulation with similar condition for a good while now (i.e. totalTemp totalPress inlet with waveTrans BC) with Pressure Ratios around 25-250.

what is the scale on the Mach image you posted?
It almost looks like mach waves from surface roughness but with the pressure ratio you have it should be safely subsonic (i.e. no mach waves)?

First thing that jumps out at me: in the images you posted it looks like there is a fairly large jump in your mesh's cell size in the axial direction near the throat. Sharp changes in cell size can definitely cause local oscillations in simulations.
Maybe try smoothing out the mesh a bit in key regions (throat and nozzle lip)?

Also numerical scheme can have a pretty significant impact I typically use TVD vanLeer with good results. I've also heard NVD work well with rhoCentralFoam.

depending on how the sim is initialized rhoCentralFoam can take a while to reach steady state with a lot of pressure waves bouncing around especially in the converging section. Idk if your looking at steady-state or transient results.

the LINF value can cause oscillations too for the waveTransmissive boundary condition (but thats usually in the quiescent medium around the plume)


Just a couple thoughts apologies if this is old news to you. I just recalled banging my head against a wall on some similar problems not too long ago

cheers,
Jason

Last edited by wyldckat; April 19, 2015 at 11:21. Reason: removed bold formatting from the whole text, to make it easier to read
jaason is offline   Reply With Quote

Reply

Tags
cd nozzle, compressible flow, rhocentralfoam

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
Pressure driven flow issues at the inlet of a pipe CRI_CFD OpenFOAM Running, Solving & CFD 0 January 30, 2015 13:26
Appropriate pressure boundary condition in incompressible flow lonelywing OpenFOAM Running, Solving & CFD 9 October 22, 2014 22:06
Compressible Pressure Driven Flow mateiu2003k OpenFOAM Running, Solving & CFD 0 August 18, 2014 15:23
Boudaries for bouynat driven flow with additional mass flux at inlet Charon CFX 2 April 27, 2013 08:02
Non-steady flow simplified for use in Vissim steamerandy Main CFD Forum 0 October 31, 2011 22:08


All times are GMT -4. The time now is 15:50.