CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (http://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   Boundary Conditions for Flow Problem (http://www.cfd-online.com/Forums/openfoam-pre-processing/103611-boundary-conditions-flow-problem.html)

 treima June 21, 2012 09:30

Boundary Conditions for Flow Problem

Hello,

I´ve some questions about how to implement boundary conditions.

I have a domain, where something flows through, in my case I´m using rhoCentralFoam.
At the inlet I´ve a fixed velocity, a fixed temperature and a fixed pressure. At the outlet I want to set a fixed pressure and give no defaults to velocity and temperature. These should be calculated from the neighbour cells in the timestep before.
I hope, you know what I mean ;)

How can I do this in OpenFoam? Is there a possiblity with the standard bc or groovyBC?

regards

treima

 gschaider June 21, 2012 09:39

Quote:
 Originally Posted by treima (Post 367649) Hello, I´ve some questions about how to implement boundary conditions. I have a domain, where something flows through, in my case I´m using rhoCentralFoam. At the inlet I´ve a fixed velocity, a fixed temperature and a fixed pressure. At the outlet I want to set a fixed pressure and give no defaults to velocity and temperature. These should be calculated from the neighbour cells in the timestep before. I hope, you know what I mean ;) How can I do this in OpenFoam? Is there a possiblity with the standard bc or groovyBC?
I say "groovyBC" to all of these questions, but in your case fixedValue and zeroGradient is sufficient. Although you might want to set the pressure to zeroGradient at the inlet instead of fixedValue which you're proposing

 treima June 21, 2012 09:52

Thanks.

I´ve tried fixedValue and zeroGradient. If I set these outlet conditions,

p - fixedValue

the case gives a floating exeption and problemes with the courant-number.

If I set

the case works, but doesn´t match to my ideas.

The best think would be, if it´s possible to set a "new" boundary condition for every timestep. But if this isn´t possible i´ve to setup a new case with other physical relations. I´m just wondering that this case haven´t discussed before ;)

regards

treima

 gschaider June 21, 2012 10:07

Quote:
 Originally Posted by treima (Post 367657) Thanks. I´ve tried fixedValue and zeroGradient. If I set these outlet conditions, U - zeroGradient p - fixedValue T - zeroGradient the case gives a floating exeption and problemes with the courant-number. If I set U - zeroGradient p - zeroGradient T - zeroGradient the case works, but doesn´t match to my ideas. The best think would be, if it´s possible to set a "new" boundary condition for every timestep. But if this isn´t possible i´ve to setup a new case with other physical relations. I´m just wondering that this case haven´t discussed before ;) regards treima
What is the inlet condition for the pressure?

 treima June 22, 2012 07:20

My inlet conditions are

p - fixedValue, value uniform 1,
T - fixedValue, value uniform 1,
U - fixedValue, value uniform (3 0 0).

And my outlet conditions just should be

p - fixedValue, value uniform 1,

T and U should be calculated from the domain in the timestep before.

 gschaider June 22, 2012 15:11

Quote:
 Originally Posted by treima (Post 367843) My inlet conditions are p - fixedValue, value uniform 1, T - fixedValue, value uniform 1, U - fixedValue, value uniform (3 0 0). And my outlet conditions just should be p - fixedValue, value uniform 1, T and U should be calculated from the domain in the timestep before.
Usually you fix the pressure only on the outlet and on the inlet have a zeroGradient. Your boundary condition says "I want a velocity, but no pressure drop". It is very hard for a self-respecting fluid (fluid with a viscosity) to fulfill that and probably while trying to do so your solver blows up

 treima June 25, 2012 02:34

1 Attachment(s)

I´ve tried to fix the pressure at the outlet and set zeroGradient at the Inlet, but I still can´t calculate a solution because of a "floating execption"...

Perhaps this is caused by my geomety, which you can see below. My idea was to set at

inlet: p - fixedValue, T - fixedValue, U - fixedValue
outlet: p - fixedValue
Gamma_free and Gamma_fixed: slip condition (u*n=0).

I was searching for good choices for the remaing conditions. I want to use these conditions, because they are just the first step in a bigger calculation. The aim is to do a very simple shape-optimization with adjoint equations for this case. On Gamma_free should be a given pressure-distribution.

 gschaider June 25, 2012 05:34

Quote:
 Originally Posted by treima (Post 368106) Thank you for your advice. I´ve tried to fix the pressure at the outlet and set zeroGradient at the Inlet, but I still can´t calculate a solution because of a "floating execption"...
Can be a lot of things. A stack-trace would be helpful

 treima July 2, 2012 05:21

I´ve solved this problem.
If you take a very low temperature, you have a mach-number > 1, so you have to set just inlet-conditions and no condition at the outlet. Now I´m taking a appropriate proportion between velocity and temperature, so that

Ma = (|U|^2)/T < 1

for all timesteps and every cell. Now it works very well.

Now, in my next step, I want to implement the adjoint equation. I have calculated the adjoint equations and boundary conditions. In the subsonic case, for example, I have just one boundary condition, a function dependent of all adjoint variables. A small example is, with a the adjoint variables,

a1 + 2 a2 + 3 a3 + 4 a4 = 0.

Is it possible to implement this in OpenFoam? I´ve a underdetermined equation system as a boundary condtion...

 All times are GMT -4. The time now is 10:38.