[Puglin]

Hi all,

I'm endeavouring to simulate the flow through a duct (with simpleFoam). The duct has a fan pulling air through it, which I'm trying to simulate with a cyclic-type fan. At this stage I'm content with doing so in a 2D context. I used Gmesh to build the duct cross section and extrude it (adding a planar surface to serve as my fan patch).

My first mistake was using a setup for the boundary and 0 files I found in an old tutorial that ceased to be relevant when version 2.0 changed the way you set up cyclic patches; when I went to run the simulation it asked if I wanted to run foamUpgradeCyclics, to automatically convert my files to the new form. I did that, and it altered my boundary file and all the files in 0, saving backups of the old ones. So far so good.

However, when I went to run the simulation, I got a fatal error:

Reading field p



--> FOAM FATAL ERROR:

request for surfaceScalarField phi from objectRegistry region0 failed
available objects of type surfaceScalarField are
0()

From function objectRegistry::lookupObject<Type>(const word&) const
in file /home/opencfd/OpenFOAM/OpenFOAM-2.3.0/src/OpenFOAM/lnInclude/objectRegistryTemplates.C at line 198.

FOAM aborting

I endeavoured to access p to see what was wrong, but when I tried to open it with gedit, gedit was unable to detect the character encoding. I have no idea what foamUpgradeCyclics did to this file (all the other ones it edited open just fine); is this normal?

Is there some way I can edit the (thankfully backed up) old p file to reflect the new nature of the cyclic system? This is how the old (obsolete) p looks:

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

internalField uniform 0;

boundaryField
{
inlet
{
type freestreamPressure;
}

exit
{
type freestreamPressure;
}

Fan
{
type fan;
patchType cyclic;
f List<scalar> 2 (10.0 -1.0);
value uniform 0;
}

top
{
type freestreamPressure;
}

bottom
{
type freestreamPressure;
}

ForeDuct
{
type zeroGradient;
}

RearDuct
{
type zeroGradient;
}

front
{
type empty;
}

back
{
type empty;
}
}

// ************************************************** *********************** //

I guess the question becomes, how on earth do fans work in 2.x?

[Puglin]

Nobody has any ideas?

Surely someone must've had cause to implement some kind of pressure gradient in the latest version of openFOAM. Is there any documentation I can consult...? Any more information I can provide...?

[Wai Phyo Kyaw]

Dear Puglin,

I am a beginner for OF, but I think I made a little modification to fan tutorial. In
0/p, 0/u, 0/k and 0/epsilon, and in the system/fvSchemes too. It worked for me. but I am afraid I have no idea it is right or wrong. Anyway I attached the modified zips. hOpe it will work for you too.

[thg]

Dear Puglin,

you find the use of the fan b.c for 2.3 f.i. in the tutorial

./incompressible/pimpleFoam/TJunctionFan

where one have in 0/p

cyclicFaces_master
{
type fan;
patchType cyclic;
jump uniform 0;
value uniform 0;
jumpTable polynomial
1((100 0));
}

Like everin in OpenFOAm if you want to understand the stuff, you have to dig deeper...

fan b.c.

./finiteVolume/fields/fvPatchFields/derived/fan


in fanFvPatchFields.C

you find the evaluation of the polynomial/list.
The code state that the old format works, but I have not checked this.

if you want to know, how the polynomial is defined you have to ckeck

$FOAM_SRC/OpenFOAM/primitives/functions/DataEntryolynomial/

in "polynomial.C" f.i.

Foam::scalar Foam:olynomial::value(const scalar x) const
{
scalar y = 0.0;
forAll(coeffs_, i)
{
y += coeffs_[i].first()*pow(x, coeffs_[i].second());
}

return y;
}