[alfa_8C]

...problem solved!

since alphaEff = alphat (turbulent alpha) + alpha (laminar alpha),

and alphat as well as alpha is defined as volsclarfield in and thus present, the groovyBC expression can be modified as follows:

SURFACE_SOURCE
{
type groovyBC;
value uniform 283;
valueExpression "283";
gradientExpression "gradT";
fractionExpression "0";
variables "heatFlux=0.00000001;Cp0=1005;rho0=1.18;gradT=heat Flux/((alphat + alpha) * Cp0 * rho0);";
timelines (
);
}

thanx for the hint regarding the connection of alphaEff to turbulence models - it led me to the solution!
Tony

[yashar.afarin]

Hi bernhard,

I am using pisofoam and I want to model a three dimentional free turbulent planar jet with large eddy simulation. in inlet I want to use turbulentinlet for velocity fluctuations generation also I want to specify an equation for mean velocity with groovyBC but for each of them I must use their specific type.
can I use both of them at the same time? what I must specify as "type"?

I would appreciate any help
sincerely yours

[gschaider]

Originally Posted by yashar.afarin

Hi bernhard,

I am using pisofoam and I want to model a three dimentional free turbulent planar jet with large eddy simulation. in inlet I want to use turbulentinlet for velocity fluctuations generation also I want to specify an equation for mean velocity with groovyBC but for each of them I must use their specific type.
can I use both of them at the same time? what I must specify as "type"?

I would appreciate any help
sincerely yours

I'm afraid this is not possible with vanilla groovyBC. You can write a boundary condition that uses the groovyBC engine and link it to your solver (just write a class groovyTurbulentInlet that inherits from turbulentInlet, sets the fields according to expressions then calls the superclass for the actual evaluation). Easy .... if you have done that kind of thing before

[yashar.afarin]

>>just write a class groovyTurbulentInlet that inherits from turbulentInlet, sets the fields according to expressions then calls the superclass for the actual evaluation.

Hi Bernhard,

thanks for your response. unfortunately, I have not done that yet so I would appreciate it if you could give me more details.

sincerely yours,
Yashar

[yashar.afarin]

Originally Posted by gschaider

>>just write a class groovyTurbulentInlet that inherits from turbulentInlet, sets the fields according to expressions then calls the superclass for the actual evaluation.

Hi Bernhard,

thanks for your response. unfortunately, I have not done that yet so I would appreciate it if you could give me more details.

sincerely yours,
Yashar

[gschaider]

Originally Posted by yashar.afarin

>>just write a class groovyTurbulentInlet that inherits from turbulentInlet, sets the fields according to expressions then calls the superclass for the actual evaluation.

Hi Bernhard,

thanks for your response. unfortunately, I have not done that yet so I would appreciate it if you could give me more details.

sincerely yours,
Yashar

Sorry. I currently don't have time for more than the sketchy answer above.

If your average velocity doesn't chnage over time you might want to try funkySetBoundaryField from the swak-suite

Bernhard

[yashar.afarin]

Originally Posted by gschaider

Sorry. I currently don't have time for more than the sketchy answer above.

If your average velocity doesn't chnage over time you might want to try funkySetBoundaryField from the swak-suite

Bernhard

Hi Bernhard

thank you for your reply.
I am trying to write a new boundary condition with those applications.
my velocity is constant over time. do you think that funkySetBoundaryField can be used in turbulent flow?

Regards,
Yashar

[gschaider]

Originally Posted by yashar.afarin

Hi Bernhard

thank you for your reply.
I am trying to write a new boundary condition with those applications.
my velocity is constant over time. do you think that funkySetBoundaryField can be used in turbulent flow?

Yes it can. funkySetBoundaryField just sets entries of the dictionary of a boundary condition to calculated, non-uniform values. It doesn't care what the physics are.

Have a look at the example that comes with swak

Bernhard

[abhi25_itbhu]

Hey,

I am a new user of OpenFoam 1.7.1. I am interested in wave simulation using OpenFoam.
I came through this groovyBC utility recently. As illustrated on the "contrib groovyBC" wiki page, I was able to download the libraries for the groovyBC case....

I dowloaded the full "groovyBC" folder in the following directory:

..../OpenFOAM-1.7.1/applications/solvers/groovy/groovyBC

Then I ran the "wmake libso" command; which I think worked fine as it didn't produce any error message.

Now, I tried to run demo cases in the Demos folder but I couldn't.
For example, for the case pulsedPitzDaily, I was able to create a mesh using blockMesh, but in the next step when I ran the simulation using oodles (application: oodles in ControlDict file) command, I found the following error:

oodles: command not found

I think I am doing sth wrong at this step.
Please help me out....I appreciate your help in advance.

Regards,

Abhishek

[gschaider]

Originally Posted by abhi25_itbhu

Hey,

I am a new user of OpenFoam 1.7.1. I am interested in wave simulation using OpenFoam.
I came through this groovyBC utility recently. As illustrated on the "contrib groovyBC" wiki page, I was able to download the libraries for the groovyBC case....

I dowloaded the full "groovyBC" folder in the following directory:

..../OpenFOAM-1.7.1/applications/solvers/groovy/groovyBC

Then I ran the "wmake libso" command; which I think worked fine as it didn't produce any error message.

Now, I tried to run demo cases in the Demos folder but I couldn't.
For example, for the case pulsedPitzDaily, I was able to create a mesh using blockMesh, but in the next step when I ran the simulation using oodles (application: oodles in ControlDict file) command, I found the following error:

oodles: command not found

I think I am doing sth wrong at this step.
Please help me out....I appreciate your help in advance.

Regards,

Abhishek

oodles is now pisoFoam

[chantre]

Hi,

I am trying to use the groovy BC to create an Inlet, where a uniform velocity-field should change randomly for every time-step within a certain range. Since the function randNormal() gives a random skalar field, I get a non-uniform velocity distribution.
Is it possible to use rand() or randNormal() to get a single random skalar?

INLET
{
type groovyBC;
variables "uMin=0.9*vector(13,0,0);deltaU=0.2*vector(13,0,0) ;";
valueExpression "uMin+randNormal()*deltaU";
value uniform (13 0 0);
}

Thanks in advance for your help
/Andreas

[gschaider]

Originally Posted by chantre

Hi,

I am trying to use the groovy BC to create an Inlet, where a uniform velocity-field should change randomly for every time-step within a certain range. Since the function randNormal() gives a random skalar field, I get a non-uniform velocity distribution.
Is it possible to use rand() or randNormal() to get a single random skalar?

INLET
{
type groovyBC;
variables "uMin=0.9*vector(13,0,0);deltaU=0.2*vector(13,0,0) ;";
valueExpression "uMin+randNormal()*deltaU";
value uniform (13 0 0);
}

Thanks in advance for your help
/Andreas

My first impulse would have been min(rand()), max(rand()) and average(rand()) but that would give approxiamtey 0, 1 and 0.5.

The only way I can think of would be to (I know this means some extra computation) take the value from only one cell and use it for all. Something like (havn't tried it and I'm not quite sure whether id() is in the regular groovyBC-distro or only in the swak-variant):

variables "singleRandom=max(id()==0?rand():-1);";

[chiven]

Hi, Bernhard, happy new year. Thank you for the contribution. Is the GroovyBC able to be used in OpenFOAM Version 1.7.1?

Thanks a lot,
Chiven

[gschaider]

Originally Posted by chiven

Hi, Bernhard, happy new year. Thank you for the contribution. Is the GroovyBC able to be used in OpenFOAM Version 1.7.1?

Thanks a lot,
Chiven

You mean "plain" groovyBC? Yep. The 1.6-version works to my knowledge with the current OF-version (personally I use the version that comes with swak4Foam which should be as stable)

Bernhard

[akidess]

I'm trying to write a boundary condition in groovyBC that requires the tangential gradient of the associated field. Is it possible to calculate a gradient on a patch face (not an snGrad)?

[gschaider]

Originally Posted by akidess

I'm trying to write a boundary condition in groovyBC that requires the tangential gradient of the associated field. Is it possible to calculate a gradient on a patch face (not an snGrad)?

Sorry no. The fvPatchField only voluntarily gives away the snGrad.

The only way I could think of would be to calculate the gradient for the whole field (expensive!) beforehand and then getting the patch value for that field. Calculation of that gradient-Field could be done with the expressionField-functionObject from swak4Foam but as this is only done at the end of a time-step it will probably lag behind. So if this is an issue for you you'll probably have to modify the solver

Bernhard

[akidess]

Thanks Bernhard. I actually noticed that after posting and went on to look if I could calculate a gradient of fvPatchField in the code, but that's far from trivial. fvc::grad works on GeometricFields / volMeshes, but since patches aren't directly related to either I'd have to come up with a whole new machinery to do this. The easy way out is (just as you said) to calculate the gradient for the entire field, and that seems to be a common solution from what I found on the forums.

[usergk]

Hi

I am new to OpenFoam, and was trying to implement the groovyBC in the XiFoam/pitzDaily case, for OF 1.7.1.
I installed and compiled the groovy BC, and used the following in the 0/T file (for wall heat transfer):

upperWall
{
type groovyBC;
variables "htot=100.0;Tinf=298.15;rho=2700.0;cp=900.0;k=DT*r ho*cp;";
valueExpression "Tinf";
fractionExpression "1.0/(1.0 + k/(mag(delta())*htot))";
}
lowerWall
{
type groovyBC;
variables "htot=100.0;Tinf=298.15;rho=2700.0;cp=900.0;k=DT*r ho*cp;";
valueExpression "Tinf";
fractionExpression "1.0/(1.0 + k/(mag(delta())*htot))";
}

However, I got the following error:

attempt to use janafThermo<equationOfState> out of temperature range 200 -> 5000; T = 0

Any ideas why this could be happening?

gk

[akidess]

How did you initialize the internal field?

[usergk]

Hi

Thanks for your reply.

Here is the 0/T file:

dimensions [ 0 0 0 1 0 0 0 ];

internalField uniform 293;

boundaryField
{
inlet
{
type fixedValue;
value uniform 293;
}
outlet
{
type inletOutlet;
inletValue uniform 293;
value uniform 293;
}
upperWall
{
type groovyBC;
variables "htot=100.0;Tinf=298.15;rho=2700.0;cp=900.0;k=DT*r ho*cp;";
valueExpression "Tinf";
fractionExpression "1.0/(1.0 + k/(mag(delta())*htot))";
}
lowerWall
{
type groovyBC;
variables "htot=100.0;Tinf=298.15;rho=2700.0;cp=900.0;k=DT*r ho*cp;";
valueExpression "Tinf";
fractionExpression "1.0/(1.0 + k/(mag(delta())*htot))";
}
frontAndBack
{
type groovyBC;
variables "htot=100.0;Tinf=298.15;rho=2700.0;cp=900.0;k=DT*r ho*cp;";
valueExpression "Tinf";
fractionExpression "1.0/(1.0 + k/(mag(delta())*htot))";
}
}

Please note that I have also changed frontAndBack boundary type from 'cyclic' to 'wall' so that I could give the groovyBC; the upperWall and lowerWall are also of boundary type 'wall'.

When I change the BC at the walls to fixedValue (isothermal BC) simulations seem to run fine.

Thanks,
gk