[letzel]

Dear Foamers,

my set-up is a cooling tower. The lowest some meters of the air within this tower act as a porous medium. This porous volume has a cylinder geometry.

Let's say the characteristic vertical coordinates (height above ground) are

• z1: bottom of tower, equal to bottom of porous region
• z2: top of porous region
• z3: top of tower

with 0 < z1 < z2 << z3.

The porous volume acts as a flow conditioner/straightener insofar as u=v=0 within this volume, only w /= 0, i.e. only vertical motion is possible.

Is it possible to realize the following strategy with OpenFOAM, and if so, how?

1. Combine the two solvers porousSimpleFoam and buoyantBoussinesqSimpleFoam into a new solver that includes porosity as well as buoyancy.
2. To drive the flow only by means of buoyancy, prescribe temperature at height z2.
3. To model the effect of the flow conditioner/straightener, force u=v=0 at z1 and z2.
4. My target is to measure the volume flow of air that leaves the tower at height z3, as well as pressure differences between the height levels z1, z2, z3.

Is it possible/advisable to create internal patches at z1, z2 and z3 to solve tasks 2, 3 and 4, and if so, how? Or are there different solutions?

Best regards,
Marcus

[wyldckat]

Greetings Marcus,

In OpenFOAM, what you're looking for is the creation of a cell zone, not internal patches .

As of OpenFOAM 2.2, there are several tutorials that exemplify how to use the fvOption named "explicitPorositySource", as indicated in the release notes for OpenFOAM 2.2.0: http://www.openfoam.org/version2.2.0/fvOptions.php

You can find the tutorials that use this here:

find $FOAM_TUTORIALS -name "fvOptions" | xargs grep explicitPorositySource

Best regards,
Bruno

PS: I erased the post you had at http://www.cfd-online.com/Forums/ope...nal-faces.html, since it was identical to this one and wasn't fully related to that other thread.

[letzel]

Dear Bruno,

thanks a lot for pointing me into this direction. Cell zones will certainly help to model the porosity effect. This even allows to model the effect of the flow conditioner/straightener by setting the horizontal resistance to a value some orders of magnitude larger than the vertical resistance. Great!

So, the decelerating part of my problem should be fine. However, I do not see how this helps me to tackle the ascelerating part of my problem, namely to create buoyancy inside the tower. I would like to do so by prescribing a warmer temperature inside (fixed in time). Is it possible to achieve this by tweaking OpenFOAM using a cyclic patch, i.e. to place a thin pair of cyclic patches at the top of the porosity cell zone and prescribe warm temperature there? Or is there any other way to create buoyancy inside?

Has anybody ever combined the two solvers porousSimpleFoam and buoyantBoussinesqSimpleFoam into one new solver? I only need the Forchheimer part of the porosity model.

Cheers,
Marcus

P.S.: Thank you for cleaning up my post in the other thread, I agree it is more appropriate to treat my questions within the present thread.

[jherb]

Using OpenFOAM 2.2.2 I can specify porousity with fvOptions and use the solver bouyantPimpleFoam so I guess you should be able to do the same with buoyantBoussinesqSimpleFoam

[wyldckat]

Just a quick note: It should also be possible to use a second fvOption for turning the same cellZone into a heat source.

[letzel]

Thank you Joachim and Bruno for your suggestions which pointed me into the right direction.

For the accelerating part of the problem I am now using another fvOption to emulate the effect of warm water injection:

warmWasserEinlass
{
    type            scalarExplicitSetValue;
    active          true;
    selectionMode   cellSet;
    cellSet         warmWasserEinlassEbeneZellen;

    scalarExplicitSetValueCoeffs
    {
        volumeMode      absolute;
        injectionRate
        {
            T              323;
        }
    }
}

For the decelerating part, I confirm that the fvOption named "explicitPorositySource" can be used using the solver buoyantBoussinesqSimpleFoam. This is a very convenient new feature of OpenFOAM 2.2.

I set the DarcyForchheimerCoeffs d to (0 0 0) and f to say (1000 1000 10). The decelerating effect in the vertical direction is fine, i.e. the third component of f, here 10, is out of question.

However, the flow straightening effect (my target is: u=v=0 within the cellZone) is insufficient because the flow should be strictly vertical within the entire cellZone. Even if I increase the first two components of f, here 1000, to even larger values, there will always be a balance of forces and in effect the flow will not be 100% vertical.

So, I am wondering whether there are better ways to achieve a truely vertical flow in OpenFOAM, i.e. to force u=v=0 but leave w unmodified.

Question: is it possible to use fvOption vectorExplicitSetValue but specify only two of the three vector components? Or does swak4Foam offer such functionality?

Best regards,
Marcus

[wyldckat]

Hi Marcus,

I'm not familiar enough with swak4Foam to know if there are any "fvOptions" features in it. But the "README" file inside the swak4Foam folder should indicate if it does and what it is.

As for the flow being fully vertical: I don't have time to test this myself, but the suggestion I have is as follows:

1. Have a look into the folder "$FOAM_SRC/fvOptions" and check the ".H" files therein. They have descriptions on what they do and what they're for. You can see the full path for the relevant folders by running:
   

   echo "$FOAM_SRC/fvOptions/constraints"
   echo "$FOAM_SRC/fvOptions/sources"

2. If none of them do what you need, then you can copy-paste-change one of them to do what you need it to do. Possibly, the porosity one is the best candidate.
3. Copying directly inside the "fvOptions" library isn't a good idea, since it can affect much of OpenFOAM's build structure. Therefore, I suggest that you follow the same lines as this project: https://github.com/wyldckat/forceDirCoeffs/tree/of22x - it's a good example of how to create a new function object, derived from OpenFOAM's own function object "$FOAM_SRC/postProcessing/functionObjects/forces". The steps for doing the same for a new "fvOption" is essentially the same.
4. If you don't have experience yet on how to create your own application/library in OpenFOAM, have a look at this tutorial: http://openfoamwiki.net/index.php/Ho...ure_to_icoFoam

Best regards,
Bruno