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/)
-   -   Pressure BC for compressible flow (http://www.cfd-online.com/Forums/openfoam-solving/115676-pressure-bc-compressible-flow.html)

VSass April 4, 2013 13:57

Pressure BC for compressible flow
 
Hey lads,

i need an outletInlet bc for pressure in my compressible case,for my farfield. I used outletInlet but it doesn't work. I need something like inletOutletTotalTemperature, which i use for temperature. Anything in mind? I already used totalPressure but it works like fixedValue,i need an outletInlet.

Thanks

immortality April 4, 2013 16:17

use waveTransmissive or now pressureTransmissive i think.there is examples in tutorials.

VSass April 5, 2013 06:09

Well, here are my case files.

p

GEOM
{
type zeroGradient;
}
FARFIELD
{
type waveTransmissive;
value uniform 1e+05;
gamma 1.4;
phi phi;
rho rho;
psi psi;
lInf 1;
fieldInf 1e+05;
}

T
GEOM
{
type zeroGradient;
}
FARFIELD
{
type inletOutletTotalTemperature;
U U;
phi phi;
psi psi;
gamma 1.4;
T0 uniform 306.534;
}

U
GEOM
{
type fixedValue;
value uniform (0 0 0);
}
FARFIELD
{
type pressureInletOutletVelocity;
value uniform (100 0 0);
}

I'm a little stuck here,so thanks for your advise.

immortality April 5, 2013 13:17

does this settings of BC's work?you could set T also in waveTransmissive form.whats your doubt about?

VSass April 5, 2013 13:29

No,they don't work. I want to find the correct combination of those in order for my farfield not to be reflective. I could use something like inletOutletTotalPressure but it doesn't exist. I need something like pressure Farfield in Fluent, which i've seen you are familiar within an other post.

immortality April 5, 2013 15:12

in my opinion you should make FarField BC divided into two parts.one for inlet part and one for outlet part.on inlet part you should specify p and T(U be in any kind of zeroGradient BC's) or U and T(p be of zeroGradient kind)
I don't know what do your case and geometry like.do you have an airfoil or something like that?

VSass April 5, 2013 15:57

I have a sphere geometry in a sphere farfield. What you say sounds great but i will need some guidance in making and applying it.

(Thanks a lot for your interest!)

immortality April 5, 2013 16:11

oh i remembered you wanted to simulate vortex shedding in a sphere thats in a flow.can't you change farField patch to a cylindrical form that has an inlet and an outlet?

VSass April 5, 2013 20:31

Yes,that's me.No, 'cause i've already completed the incompressible simulation and i want the compressible results to have a complete comparison.So,any ideas for the combination of p/T/U at farfield?

immortality April 5, 2013 22:16

set T as waveTransmissive as i told you before.if it didn't work set it simply zeroGradien.if this also didn'p work you should set farfield as a cylinder to have certained inflow and outflow patches.do these 3 ones and let me know the results.

VSass April 6, 2013 07:51

Ok, but can you explain to me why zeroGradient at farfield? I thought we need something like inlet/outlet or wave transmissive like you've said.

immortality April 6, 2013 08:36

zeroGradient have to be set for variables that we have to set a value for them for starting numerical calculations and not required by fluid dynamics itself.
inletOutlet is a kind of zeroGradient.when flow is going into domain it has the value we specified ourselves as external value(becomes like fixedValue) and when the flow flows outward! solver read the values of variable in domain and put it on boundary(and becomes zeroGradient).

VSass April 10, 2013 10:06

A brief report:
the boundary conditions were just fine.The reason why i couldn't see the desired vortices was because rhoCentralFoam is inviscid. I came to this conclusion due to the fact that i get the same and desired distributions of p,T,U with different ( but relative when it comes to their nature) boundary conditions, but i don't see any vortices.

So,next step was to change solver. I now use rhoPimpleFoam with laminar simulation, and i can see clearly the desired vortices. The problem know is that the solution crashes after some time, saying something like : Max Number of Iterations Exceeded, which i think is a problem with temperature.

Also, i think that the solution is highly dependable from the maxDeltaT and that CFL condition alone is not enough.

So,you recommend the same bcs for reaching convergence?

dancfd May 19, 2014 23:03

Hello Vasileios,

Could you please expand upon why changing boundary conditions and obtaining the same results suggests that rhoCentralFoam is inviscid? I have been using it to model airfoil flow, and I have found that it does develop a boundary layer and a wake with significant vortices.

Maybe something else is wrong with your simulation. I have had different results with rhoPimpleFoam, rhoCentralFoam, and sonicFoam; not sure why, but it seems as though they are suited to different applications.

Daniel

VSass May 26, 2014 13:39

Daniel,

I supposed that rhoCentralFoam is inviscid because, provided that Reynolds is sufficient and the boundary conditions of the farfield do not create numerical reflections that wouldn't allow the flow to separate and the vortices to detach, I came to the hypothesis that this solver solves the Euler formulation of the equations.

Kind regards


All times are GMT -4. The time now is 05:19.