CFD Online Discussion Forums

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   OpenFOAM Pre-Processing (https://www.cfd-online.com/Forums/openfoam-pre-processing/)
-   -   using groovyBC toPoints? (https://www.cfd-online.com/Forums/openfoam-pre-processing/99477-using-groovybc-topoints.html)

fisch April 4, 2012 06:23

using groovyBC toPoints?
 
Hello,

i read that i can use the groovyBC in meshmotion simulations, too.
I try inside the pointDisplacement file the following:

bottom
{
type groovyBC;
value uniform (0 0 0);
valueExpression "vector(0,toPoint(0.05*(sin(pi*time()))),0)";
}

but i get the following error:
--> FOAM FATAL ERROR:
Parser Error at "1.10-16" :"syntax error, unexpected TOKEN_toPoint"
"vector(0,toPoint(0.05*(sin(pi*time()))),0)"
" ^^^^^^^ "

From function parsingValue
in file lnInclude/CommonValueExpressionDriverI.H at line 724.

FOAM exiting


Is it necessary to include there something or did i a mistake???

thanks in advance,
rupert

gschaider April 4, 2012 07:36

Quote:

Originally Posted by fisch (Post 353081)
Hello,

i read that i can use the groovyBC in meshmotion simulations, too.
I try inside the pointDisplacement file the following:

bottom
{
type groovyBC;
value uniform (0 0 0);
valueExpression "vector(0,toPoint(0.05*(sin(pi*time()))),0)";
}

but i get the following error:
--> FOAM FATAL ERROR:
Parser Error at "1.10-16" :"syntax error, unexpected TOKEN_toPoint"
"vector(0,toPoint(0.05*(sin(pi*time()))),0)"
" ^^^^^^^ "

From function parsingValue
in file lnInclude/CommonValueExpressionDriverI.H at line 724.

FOAM exiting


Is it necessary to include there something or did i a mistake???

thanks in advance,
rupert

OK. Two problems here:

a) to construct a pointVectorField it must be "vector(toPoint(0),toPoint(0.05*(sin(pi*time()))), toPoint(0))"
b) it seems that the construction of a pointVectorField is in the grammar for Fields (== funkySetFields) but not in Patches (==groovyBC)

If a bug-report shows up on the OF-extend-Mantis I will take care of point b. Point a you'll have to take care of yourself ;)

fisch April 4, 2012 08:17

Hi,

point a i already tried, but it seems that he's not able to get the function toPoint.

I tried to post it in the bugtracker; did i do it the right way?

thanks a lot,
rupert

fisch April 10, 2012 04:34

If anybody is interested, the problem is solved. See:

https://sourceforge.net/apps/mantisb...iew.php?id=130

fisch April 10, 2012 05:14

Hi,

now it's running without error messages but the result is not the desired one.
The code only moves the points on the mesh boundary and not the mesh (using the specified meshMotion solver) himself.
What I tried to get is a result like using the BC oscillatingDisplacement...

can you help me?

gschaider April 10, 2012 05:44

Quote:

Originally Posted by fisch (Post 353925)
Hi,

now it's running without error messages but the result is not the desired one.
The code only moves the points on the mesh boundary and not the mesh (using the specified meshMotion solver) himself.
What I tried to get is a result like using the BC oscillatingDisplacement...

can you help me?

Have you set up the cellDisplacement-field to be consistent to be consistent with the point displacement? (have a look at the movingCone-example in the swak ... as far as I remember it is done just by using toFace( ... ) )

fisch April 10, 2012 07:13

Hi,

you were right; My mistake..

regarding the compiler flag: __linux__ solved the problem with icc

Tobi March 5, 2015 11:57

Hi all,

just one question... it the output of the face to point interpolation always there or could we suppress it?


Thanks in advance,

gautami January 6, 2016 18:50

P { margin-bottom: 0.08in; } Hello Everybody,


I am trying to simulate a numerical wave tank using interDyMFoam solver on OpenFOAM version 2.2.0 (SuSE Linux 12.2). The idea is to generate waves by a piston wave maker, using groovy boundary condition at the inlet of the wave tank.


The dynamic mesh option is specified as:
  1. In the file “dynamicMeshDict” in “constant folder”
solver displacementLaplacian;
displacementLaplacianCoeffs
{
diffusivity uniform;
}


The groovyBC at the inlet is implemented as:


  1. In the file “pointDisplacement” under the folder “0”
    inlet
    {
    type groovyBC;
    value uniform (0 0 0);
    valueExpression "vector(toPoint(cos(-time())),toPoint(0),toPoint(0))";

    }
  2. In the file “cellDisplacement” under the folder “0”

inlet
{
type groovyBC;
value uniform (0 0 0);
valueExpression "toFace(pointDisplacement)";
}


4. In the file “U” under the folder “0”
inlet
{

type groovyBC;
value uniform (1 0 0);
valueExpression "toFace(pointDisplacement)";

}
The solver for the cellDisplacement in the “fvSolution” file is GAMG.


When I run the case using interDyMFOAM, I do not get any syntax errors, but the run blows up for the very first time step.


In the log file it shows:


Interface Courant Number mean: 0 max: 0
Courant Number mean: 0.00934266978331 max: 0.165086855307
deltaT = 0.00111111111111
Time = 0.00111111

swak4Foam: Allocating new repository for sampledGlobalVariables
GAMG: Solving for cellDisplacementx, Initial residual = 1, Final residual = 9.36444116038e-06, No Iterations 8
GAMG: Solving for cellDisplacementz, Initial residual = 0, Final residual = 0, No Iterations 0
Execution time for mesh.update() = 0.08 s
time step continuity errors : sum local = 4.46786639335e-10, global = -2.72113359451e-11, cumulative = -0.000200000046943
GAMGPCG: Solving for pcorr, Initial residual = 1, Final residual = 4.75866102817e-06, No Iterations 7
time step continuity errors : sum local = 0.245271051403, global = 0.243261713162, cumulative = 0.243061713115


When solving for alpha:


MULES: Solving for alpha1
Phase-1 volume fraction = -5.36408246329e+291 Min(alpha1) = -4.12021901801e+295 Max(alpha1) = 2.42152309773
#0 Foam::error::printStack(Foam::Ostream&) in "/opt/OpenFOAM-2.2.0/platforms/linux64GccDPOpt/lib/libOpenFOAM.


The alpha values go out of bounds.





I would like to mention here that if I run the same simulation with the following options, the code runs smoothly and the results seem to be good:


dynamic mesh option:


solver velocityComponentLaplacian;

velocityComponentLaplacianCoeffs
{
component x;
diffusivity inverseDistance (inlet);
}


And the groovyBC at the inlet is specified using:


PointMotionUx
cellMotionUx


Kindly can somebody please guide me, how to resolve this issue. The reason I am trying to implement the groovyBC using pointDisplacement to pointMotion is, I would like to add a floating box in the middle of the wave tank with “sixDoFRigidBodyDisplacement” and provide it a “linearSpring” restraint. I am assuming that this can be done only in pointDisplacement. Please do let me know if I am wrong and any ideas and suggestions would be highly invaluable.Thank you.


Most&More,
Gautami Erukulla.

gautami January 7, 2016 14:32

Dear All,

It was an oversight at my end.
If anyone is interested the "U" file in "0" folder should be declared as:
In the file “U” under the folder “0”
inlet
{

type movingWallVelocity;
value uniform (0 0 0);


}

Now it works fine.Thank you.

Most&More
Gautami Erukulla.


All times are GMT -4. The time now is 19:05.