how can use Cp and Cv in Swak variables?
 

in below function if I want to use Cp/Cv instead of constant gamma that Cp and Cv can be calculated by the solver how I could do it?

That depends on the OF-version and the solver you're using. Sometimes these fields are already found in memory and are found under different names: cv, Cv or thermo:cv (for the last one you'll need to use the alias-feature which is discussed elsewhere and documented - so don't ask)

Otherwise there are functions that get these fields in the swakThermophysicalFunctions-plugin

Hi Bernhard
thanks for guidance.
I managed to do that in Swak postProcessing functions with the help of dear Bruno through your advice.
now I want to use Cp and Cv in groovyBC variables but it dowsn't know Cp and Cv opposite to postProcessing functions.
this is the error I get:
I put these functions in controlDict and works well for outputs:
but for groovyBC gives that error above.
in variables of groovyBC I wrote these terms in both patches for all variables(fields):

The problem is probably that the expressionField is created AFTER it is needed by groovyBC. This situation is ugly to work around.

Anyway. Before you proceed try removing Cp/Cv temporarily from the groovyBC/functions and use the listRegisteredObjects-functionObject to see if a fitting field is there. Maybe under a different name

Greetings to all!

@Bernhard: Ehsan forgot to update this thread. I had a look into this and answered him via email.
The problem about "Cv" and "Cp" is that these fields are apparently also managed by some other class and they were unregistered at the end/beginning of the following time iteration. By renaming the field names to "CRRv" and "CRRp" in the function objects, it seemed to work just fine.

I'll take the opportunity to consolidate the information I've been sending him over email. The following information was initially based on the example case "Examples/Lagrangian/hotStream" from swak4Foam:

• The following function objects are the latest ones that seem to work as intended:
  
  Code:

  ---

  loadThermo {
    type loadPsiThermoModel;
    correctModel false;
    //        correctModel true;
    allowReload false;
    failIfModelTypeExists false;
    outputControl timeStep;
    outputInterval 1;
}

cvField {
    type expressionField;
    autowrite false;
    outputControl timeStep;
    outputInterval 1;
    expression "thermo_Cv()";
    fieldName CRRv;
}

cpField {
    type expressionField;
    autowrite false;
    outputControl timeStep;
    outputInterval 1;
    expression "thermo_Cp()";
    fieldName CRRp;
}

  ---

• Don't forget to add "libswakThermoTurbFunctionPlugin.so" to the "libs" list, e.g.:
  
  Code:

  ---

  libs (
  "libOpenFOAM.so"
  "libgroovyBC.so"
  "libsimpleSwakFunctionObjects.so"
  "libswakFunctionObjects.so"
  "libfieldFunctionObjects.so"
  "libswakThermoTurbFunctionPlugin.so"
);

  ---

• The "autowrite" option is whether the field should be saved at each time snapshot.
• I think that if "correctModel" is set to "true", it will call "thermo.correct()" at the beginning of each time iteration. As for "allowReload", it's possibly for keeping track of the changes in "constant/thermo*".

Best regards,
Bruno

Hi
whats the problem with reconstructPar about CRRv?

There are a few possibilities:

• Insufficient disk space.
• The file "CRRv" might be damaged for some reason.
• You might have NaN values or similar inside the "CRRv" file.

The bullet-proof way to confirm what the problem is, is to visually inspect the file and line that the error message is telling you:
Both gedit and kate allow you to jump directly to the line in question.
Or you can do it directly from the command line:
To see the lines before and after as well:

Hi Bruno
but there is not CRRv,maybe its because of using ctrl+c.
ehsan@Ehsan-com:~/Desktop/WR_4$ sed '4647!d' processor2/0.002216/CRRv
sed: can't read processor2/0.002216/CRRv: No such file or directory

I'm honestly having a hard time to find words to answer to this...

Let me see if I understand this correctly: instead of checking if the file actually existed or not and what contents it had, as the error message clearly stated that something was wrong with this file, you instead went here to the forum to ask something that only you could see on your computer... which is somewhat common... for beginners!!!
You've been working with OpenFOAM for so long now, that these kinds of questions should no longer occur!


Either way, why on Earth are you still using Ctrl+C? I sent you the other day via email the function object that helps to stop the solver, by simply creating a file named "stop". I'll remind you how it works:

1. Add the following code to "system/controlDict", inside the functions entry, add this code:
   
   Code:

   ---

   CtrlCReplacement
{
  type abort;
  functionObjectLibs ( "libjobControl.so" );
  action noWriteNow; //nextWrite writeNow
  fileName "stop";
}

   ---

   • For other readers, the "system/controlDict" would look something like this:
     
     Code:

     ---

     FoamFile
{
    version 2.0;
    format ascii;
    class dictionary;
    location "system";
    object controlDict;
}

application icoFoam;

startFrom startTime;

startTime 0;

stopAt endTime;

endTime 0.5;

deltaT 0.005;

writeControl timeStep;

writeInterval 20;

purgeWrite 0;

writeFormat ascii;

writePrecision 6;

writeCompression off;

timeFormat general;

timePrecision 6;

runTimeModifiable true;

functions
{
  CtrlCReplacement
  {
    type abort;
    functionObjectLibs ( "libjobControl.so" );
    action noWriteNow; //nextWrite writeNow
    fileName "stop";
  }
}

     ---

2. Now, next time you want to use Ctrl+C, you should instead run the following command on another terminal tab/window, inside the same folder of the case you are running:
   
   Code:

   ---

   touch stop

   ---

   The function object "abort", as soon as it sees this new file "stop", will stop the solver at the end of the current time iteration.
   This way you will no longer have broken results. In addition, you can also change the action to one of the other two options.

Hi Bruno
sorry,I had to leave and hadn't enough time to use touch stop and also was confused with various jobs should be done.CRRv file was there in fact,I saw that at the moment but was empty or incomplete because it couldn't be unzip and also CRRp didn't exist there.now I deleted four time folders and used previous time folder by reconstructPar -latestTime and worked fine.
I'm glad and it seems it made an opportunity for others to use the command you provided with my troubles and mentioned here.
thanks a lot.

Thanks for the clarification

heat transfer simulation at walls
 

Hello I don't want to steal this thread but I think my Problem is quite similar to the problem of immortality. I hope this is okay.

I want to simulate a reactor. The upper part is heated from the outside and in the lower part where the flame is burning there should be like it is normal the heat transfer to the outside. I use of swak4Foam groovyBC to implement this heat transfer. If I try to run the simulation my error looks like this.

So the problem is the definition of cp, but I thought as I implemented it in the T boundary condition with groovyBC that it is already defined?
I use OpenFoam 2.2.2 and the Version of swak4Foam which wyldcat posted (swak4Foam-master). I think this is the Version 0.2.4 but I am not sure.

Thanks a lot for your time and help.
Best regards Martin

I think the problem is that nowadays Cp is available as thermo:cp (or thermo:Cp or something else. But I'm pretty sure about the thermo: ). The problem with the : in the name is that it is already used by the parser. So you'll have to define an alias with it
(I'm doing this from memory. Please check the docu). To get a list of the actually present fields you can use the listRegisteredObjects-functionObject

Thanks a lot for your answer but now I have more questions.

How and where I can use the listRegisteredObjects-functionObject? I tried it in the terminal directly in the swak4Foam folder, but it want not work?

Where I have to implement the aliases into the controlDict?

Sorry for these question which maybe sounds to you trivial but I just started to use OpenFoam and therefore I am already not really familiar with some parts of it.

Again thanks a lot for your time and help.

Best regards Martin

Usually
is your friend: it will find you some usage-examples

Either look it up in the reference guide or use the grep-trick again. Or have a look at the README (where it is described like every other new feature)

You've got to understand my problem: I give you the name of the thing that helps you (listRegisteredObjects) and then expect you to do a minimum of research yourself. The reason is that every time I describe something in detail (especially if I described it several times before on the MessageBoard - You are aware that it has a search function) another paragraph of the documentation does NOT get written (I only have limited time for non-customer-support). The alternative would be that I stop answering redundant questions altogether and with the time saved in half a year there would be a complete reference guide for swak. That half year would be hard for some.

Thanks a lot for your help. You're right I am sorry for my questions in the future I will do more research before I ask something.

Thank you very much!

Best regards Martin

Dear Bernhard,

I have similar issue with the variable defined in meltingandsolidification source in OF 3.0 and ahead.

details are given in post #1

but " aliases { sMS1:alpha1 myfl; }" is not recognised with OF3.X and the corresponding version of Swak4Foam

Also I have tried to list the variables using following commands

----but no success

But I am pretty sure about the name of the variable as I can operate with the variable in coded functions (banana trick works in coded functions but not with type writeRegisteredObject; )

please help, some how the variable "sMS1:alpha1" access with swakExpressions seem very necessary to me.

Thanks and regards.

You've used the aliases dictionary wrong: your name is on the left. The Field you want to access on the right. That's the way dictionaries usually work

(looking down I saw that the confusion comes from one of my answers. But I put the disclaimer below the answer for a reason. I'll edit the answer)

Thanks a lot for Bernhard! your quick and precise reply was very helpful, it means a lot to me...