[bryant_k]

Hello everyone
I want to use funkySetFields function to set the initial nonuniform field in multiregion case.The solver that I am useing is chtMultiregionFoam and the case is modified according to the tutorials name multiRegionHeater.I know how to use funkySetFields in a case which have a singal region.
With the command:

 funkySetFields -time 0

I can have a initial fields I need successfully.
But in a multiregion case I can not make it work.I know that the foamToTecplot have the function for multiregion.So I try the command according to that:

funkySetFields -region heater -time 0

or

funkySetFields  -time 0 -region heater

but it is wrong.

Can you tell me how can I use this funciton in multiregion case?

Thank you very much!

regards!

bryant_K

[gschaider]

Originally Posted by bryant_k

Hello everyone
I want to use funkySetFields function to set the initial nonuniform field in multiregion case.The solver that I am useing is chtMultiregionFoam and the case is modified according to the tutorials name multiRegionHeater.I know how to use funkySetFields in a case which have a singal region.
With the command:

 funkySetFields -time 0

I can have a initial fields I need successfully.
But in a multiregion case I can not make it work.I know that the foamToTecplot have the function for multiregion.So I try the command according to that:

funkySetFields -region heater -time 0

or

funkySetFields  -time 0 -region heater

but it is wrong.

Can you tell me how can I use this funciton in multiregion case?

Thank you very much!

regards!

bryant_K

Define "wrong".

I've used it in the past with -region and it worked. But I think that was in "command line"-mode. You're using a dictionary, right? Try specifying an entry "region heater;" there. I must check the source but it is possible that in dictionary mode the -region-option is ignored

[bryant_k]

Thank you for your reply.
I have put the file name funkySetFieldsDict into folder both "system" and "system/heater". Then I run the command

funkySetFields -region heater -time 0

it occured error:

can not open 
file:../../multiRegionHeater/system/heater/funkySetFieldsDict.heater at line 0.....

But when I run the command

funkySetFields -time 0

,it can run fluently without error.
But it just changed the file in folder "0" rather "0/heater".

Then I add entry in the file funkySetFieldsDict:

expressions
(
    Q1
     {
        field Q;
        expression "...";
        condition "..."
        region heater'
       }
)

It can run without any error,but it also changed the field in folder "0" only.

Can you tell how to add the entry and how can I get fields I want?
Thank you very much!

bryant_k

[gschaider]

Originally Posted by bryant_k

Thank you for your reply.
I have put the file name funkySetFieldsDict into folder both "system" and "system/heater". Then I run the command

funkySetFields -region heater -time 0

it occured error:

can not open 
file:../../multiRegionHeater/system/heater/funkySetFieldsDict.heater at line 0.....

I checked. It works like this. Look at the error message: the location of the dictionary is in a subdirectory of system, not system itself

Originally Posted by bryant_k

But when I run the command

funkySetFields -time 0

,it can run fluently without error.
But it just changed the file in folder "0" rather "0/heater".

Then I add entry in the file funkySetFieldsDict:

expressions
(
    Q1
     {
        field Q;
        expression "...";
        condition "..."
        region heater'
       }
)

It can run without any error,but it also changed the field in folder "0" only.

Can you tell how to add the entry and how can I get fields I want?
Thank you very much!

[STutexas]

Hi

Thank you for your post and your documentation. I am trying to use funkySetFields for setting heterogeneous values of fields in different cell zones. I have already created 2 separate cell zones and I use the following commands in my funkySetFieldsDict file:

setDT
{
field DT;
keepPatches true;
expression "2e-09";
zone PoreWater;
}

setTb
{
field Tb;
keepPatches true;
expression "2";
zone PoreWater;
}

My problem is that funkeSetFields changes the values of DT, Tb fields in the whole domain and not just in the zone PoreWater. Please let me know what am I doing wrongly.

Thank you.

Saurabh

[wyldckat]

Originally Posted by STutexas

My problem is that funkeSetFields changes the values of DT, Tb fields in the whole domain and not just in the zone PoreWater. Please let me know what am I doing wrongly.

Quick answer: Insufficient details. Please provide more details, namely:

1. What's the exact command you are using?
2. Where are the "funkySetFieldsDict" files placed in your case? Namely inside which folder (directory)?

[STutexas]

Hi

Thank you for your reply. I am using the command funkySetFields -time 0. My funkySetFields file is in system directory. I believe that I am using the command right but the value in the entire domain is changed not just in the defined cell.

Thank you.

Saurabh

[wyldckat]

Quick answer: Then if you want the correct region to be affected, then you need to:

1. Place a "funkySetFieldsDict" inside the folder "system/PoreWater".
2. Run like this:
   

   funkySetFields -time 0 -region PoreWater

This was explained in the posts above

[STutexas]

Hi Bruno

Thank you for your suggestion . But I am not running split mesh during preprocessing. I have regions divided (using toposet) into separate cells with names like pore water, bound water, hydrocarbon etc. I use createBaffles to divide the mesh into separate regions. I set Boundary conditions on the 2 generated boundaries. Now I want to set different (hetrogeneous) properties in these different cells. There is only one system folder .

Please let me know if running splitmesh is necessary for me to properly define these different phases. I am not doing that for now .

Thanks again for your feedback. It has been very helpful.

P.S. I have attached is a simplified .msh that I use. Please unzip and open it with gmsh if you would like a better visualization of my problem. Thanks again.


Saurabh

[wyldckat]

Quick answer: Sorry, I read the other post too fast

You should use something like this:

  setTb
  {
    field p_rgh;
    keepPatches true;
    expression "3";
    condition  "zone(porosity)";
  }

Source: http://openfoamwiki.net/index.php/Co...funkySetFields - chapter "Expression syntax" and section "Initialise a pressure field gradient due to gravity".


edit: And you forgot to attach. Either way, I tested with the tutorial case "multiphase/interFoam/ras/angledDuct"

[STutexas]

Hi Bruno

Thank you for all the help and your advice. I have used set fields for simulation of my case. Thanks again for the help.

I have another question pertaining to the same problem. I am using groovyBC in my simulations. This is what my code looks like.

boundaryField
{
PoreWall
{
type groovyBCDirection;
value uniform (0 0 0);
valueExpression "vector (0, 0, Minf)";
gradientExpression "vector(0,0,0)";
fractionExpression "symmTensor(1/(1+D/(rho2*mag(delta()))),0,0,1/(1+D/(rho2*mag(delta()))),0,1/(1+D/(rho1*mag(delta()))))";
evaluateDuringConstruction 0;
variables
4
(
"D=3e-09;"
"rho2=10e-06;"
"rho1=10e-06;"
"Minf=4.2e-07;"
)
;

}

}

but I would like to change the values of rho2, rho1 and Minf based on the set type in the mesh. For example:

if (set_of_face) == set1
Minf = 4.2;
else
Minf = 2.2;

Is it possible to set type non uniform values in the groovyBCset. I really appreciate all the help that you have given and all the help.

Saurabh

[gschaider]

Originally Posted by STutexas

Hi Bruno

Thank you for all the help and your advice. I have used set fields for simulation of my case. Thanks again for the help.

I have another question pertaining to the same problem. I am using groovyBC in my simulations. This is what my code looks like.

boundaryField
{
PoreWall
{
type groovyBCDirection;
value uniform (0 0 0);
valueExpression "vector (0, 0, Minf)";
gradientExpression "vector(0,0,0)";
fractionExpression "symmTensor(1/(1+D/(rho2*mag(delta()))),0,0,1/(1+D/(rho2*mag(delta()))),0,1/(1+D/(rho1*mag(delta()))))";
evaluateDuringConstruction 0;
variables
4
(
"D=3e-09;"
"rho2=10e-06;"
"rho1=10e-06;"
"Minf=4.2e-07;"
)
;

}

}

but I would like to change the values of rho2, rho1 and Minf based on the set type in the mesh. For example:

if (set_of_face) == set1
Minf = 4.2;
else
Minf = 2.2;

Is it possible to set type non uniform values in the groovyBCset. I really appreciate all the help that you have given and all the help.

Saurabh

You can always use the condition-operator in expressions "cond ? 4.2 : 2.2" for such a thing with cond being your conditon. I just don't understand what you mean with "set type in the mesh"

[Mohammad Jam]

Originally Posted by bryant_k

Thank you for your reply.
I have put the file name funkySetFieldsDict into folder both "system" and "system/heater". Then I run the command

funkySetFields -region heater -time 0

it occured error:

can not open 
file:../../multiRegionHeater/system/heater/funkySetFieldsDict.heater at line 0.....

But when I run the command

funkySetFields -time 0

,it can run fluently without error.
But it just changed the file in folder "0" rather "0/heater".

Then I add entry in the file funkySetFieldsDict:

expressions
(
    Q1
     {
        field Q;
        expression "...";
        condition "..."
        region heater'
       }
)

It can run without any error,but it also changed the field in folder "0" only.

Can you tell how to add the entry and how can I get fields I want?
Thank you very much!

bryant_k

Hi Dears

u should probably change funkySetFieldsDict name with funkySetFieldsDict.heater after u put funkySetFieldsDict in heater folder in system folder
(ADD dot heater)= .heater

then run funkySetFields -time 0 -region heater

[Muyiwa]

Hello Foamers

Please show me how to use funkySetFields to create an undulating initial field for alpha.water in the damBreak tutorial. I want to use undulating surface instead of the boxToCell used in the setFields of the tutorial.

[ht2017]

Originally Posted by Muyiwa

Hello Foamers

Please show me how to use funkySetFields to create an undulating initial field for alpha.water in the damBreak tutorial. I want to use undulating surface instead of the boxToCell used in the setFields of the tutorial.

do you have success with funkySetFields? If you did it. could you share with me how to do it?

[harsha_kulkarni]

Originally Posted by Muyiwa

Hello Foamers

Please show me how to use funkySetFields to create an undulating initial field for alpha.water in the damBreak tutorial. I want to use undulating surface instead of the boxToCell used in the setFields of the tutorial.

Have you succeed in your work..
I want to set dam tilted at an angle of 50 degree