[immortality]

i want to use value of pressure at a point to set a boundary condition.more clear i need to set a p0,T0 boundary condition when shock is reached at the end of the channel.what command shouldp i use at fractionExpression?

[gschaider]

Originally Posted by immortality

i want to use value of pressure at a point to set a boundary condition.more clear i need to set a p0,T0 boundary condition when shock is reached at the end of the channel.what command shouldp i use at fractionExpression?

You've got to use a "remote" variable (that can be calculated on sampled sets or patches. Your post does not make clear what you mean with "point"). The usage is described in my presentation from the 6th workshop (see the swak-page) and there are several examples in the swak4Foam-distribution

[startingWithCFD]

Hello, I have more or less the same problem.
I would like to set the pressure on a patch equal to a fraction of the pressure in a specific point inside the domain.
So far I was not able to finish the job just by looking at the fillingTheDam example.
Below is what I have done so far.

file 0/p:

myPatch
{
  type            groovyBC;
  value           uniform 10000;
  valueExpression "pinside/2.";
  storedVariables 
  (
    {
      name pinside;
      initialValue "10000";
    }
  );
  variables 
  (
    "pupstream=p;"
  );
}

file system/controlDict:

functions
(
  defineInsidePoint
  {
    type createSampledSet;
    outputControl timeStep;
    outputInterval 1;
    setName insidePoint;
    set
    {
      type cloud;
      axis x;
      points
      (
        (1. 0. 0.)
      );
    }
  }

...

);

Could you please let me know how I can connect these two?

[gschaider]

Originally Posted by startingWithCFD

Hello, I have more or less the same problem.
I would like to set the pressure on a patch equal to a fraction of the pressure in a specific point inside the domain.
So far I was not able to finish the job just by looking at the fillingTheDam example.
Below is what I have done so far.

file 0/p:

myPatch
{
  type            groovyBC;
  value           uniform 10000;
  valueExpression "pinside/2.";
  storedVariables 
  (
    {
      name pinside;
      initialValue "10000";
    }
  );
  variables 
  (
    "pupstream=p;"
  );
}

file system/controlDict:

functions
(
  defineInsidePoint
  {
    type createSampledSet;
    outputControl timeStep;
    outputInterval 1;
    setName insidePoint;
    set
    {
      type cloud;
      axis x;
      points
      (
        (1. 0. 0.)
      );
    }
  }

...

);

Could you please let me know how I can connect these two?

A variable like

pInside{set'insidePoint}=average(p);

would get p at the set insidePoint and put it into pInside (just the way it is shown in that example. The storedVariable-business there is just so that the inlet doesn't switch back once it has been switched. Depends on your application whether you need such a thing)

[startingWithCFD]

First of all thanks a lot for your answer, it was very helpful.
I have changed the pressure file as follows:

myPatch
{
  type            groovyBC;
  value           uniform 10000;
  variables 
  (
    "pinside{set'insidePoint}=average(p);"
  );
  valueExpression "pinside/2.";
}

It seems to work :-) I was originally confused about {set'insidePoint} going on the left hand side, but it now seems more clear.
If I understand correctly, the average function indicates an averaging of the pressure values of the cells around the point only, right?

[gschaider]

Originally Posted by startingWithCFD

First of all thanks a lot for your answer, it was very helpful.
I have changed the pressure file as follows:

myPatch
{
  type            groovyBC;
  value           uniform 10000;
  variables 
  (
    "pinside{set'insidePoint}=average(p);"
  );
  valueExpression "pinside/2.";
}

It seems to work :-) I was originally confused about {set'insidePoint} going on the left hand side, but it now seems more clear.

I know. The original synax of "pinside@set'insidePoint" might have been clearer. But @ is a valid character in OF-names so that might have caused problems with fields/patches/sets with that kind of name

Originally Posted by startingWithCFD

If I understand correctly, the average function indicates an averaging of the pressure values of the cells around the point only, right?

No. It's just a precaution. These "external variables" only allow one value. So if your set has more than one point it will do an arithmetic average of those and use that. In your case: the general expression for the average value of one value is left as an exercise to the reader

[hrushi.397]

Hi Bernhard,

Sorry, I am a bit late on this thread, but I have the same problem. I want to find out the value of alpha variable for a velocity boundary condition in openfoam and I need the value of alpha variable on the neighbouring face center. I know from documentation that I can find out the face center of the neighbouring cell using fn(), but can I use this information to find out value of alpha on that cell face for a velocity boundary condition?

Regards,

Hrushikesh