[amin144]

Hi dear FOAMers
especially Bernhard Gschaider ( usual replier to timeVarying B.C.)

I've read almost all posts about timeVaryingUniform
But I have problem using it
I use OF 1.5-dev and I want to work by viscoelasticFluidFoam solvers
what should I do ? what's the problem ? should I compile anything?

Thanks very much

Error:

Reading field p

Reading field U

Reading/calculating face flux field phi


Starting time loop

Time = 0.005

Courant Number mean: 0 max: 0 velocity magnitude: 0
PBiCG: Solving for Ux, Initial residual = 1, Final residual = 7.46317e-06, No Iterations 5
PBiCG: Solving for Uy, Initial residual = 0, Final residual = 0, No Iterations 0



gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type timeVaryingUniform)
on patch inlet of field p in file "/home/amin/OpenFOAM/amin-1.5-dev/run/cavity/0/p"
You are probably trying to solve for a field with a generic boundary condition.

From function genericFvPatchField<Type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 692.

FOAM exiting


0/p:

boundaryField
{
inlet
{

type timeVaryingUniform;
timeDataFileName "inlet.dat";
value uniform 1e5 ;
}
outlet
{
type fixedValue;
value uniform 0;
}

wallup
{
type zeroGradient;
}
walllow
{
type zeroGradient;
}

frontAndBack
{
type empty;
}
}

inlet.dat:

(
0 1
.01 5
.02 10
.03 20
.07 100
)

[amin144]

I attached case file for simplicity

[amin144]

AnyBody answer me this simple question?

[wyldckat]

Hi Amin,

Originally Posted by amin144

I use OF 1.5-dev and I want to work by viscoelasticFluidFoam solvers
what should I do ? what's the problem ? should I compile anything?

I'm not even certain you know what you're asking!

The viscoelasticFluidFoam solver is available in the OpenFOAM variant 1.6-ext, not 1.5-dev. There you will also find tutorials on how to use this solver.
edit: wait, I'm wrong. I completely forgot that they were already present in 1.5-dev Sorry about that. But still, I can't fully understand the question...

Good luck!
Bruno

[amin144]

Originally Posted by amin144

I attached case file for simplicity

I could do my job by using GroovyBC and this thread:
time varying vector boundary condition using patch normal

I attached my case in order to using of others.
I should mention that I used myIcoFoam solver which it's different to icoFoam is adding the line " -lgroovyBC " to "option" file and compile new solver.

After all I'll be happy if someOne say my fault in using timeVaryingUniform

[amin144]

Hi dear Bruno
Thanks again
I swear GOD I'm not a confused man ( the way you think )
I know what I'm saying

The viscoelastic solver exist in 1.5 dev like 1.6 ext
My problem is using the boundary condition "timeVaryingUniform" not using solver
I appreciat if you can upload me a case using this kind of boundary condition

[bigphil]

Originally Posted by amin144

gradientInternalCoeffs cannot be called for a genericFvPatchField (actual type timeVaryingUniform)
on patch inlet of field p in file "/home/amin/OpenFOAM/amin-1.5-dev/run/cavity/0/p"
You are probably trying to solve for a field with a generic boundary condition.

From function genericFvPatchField<Type>::gradientInternalCoeffs( ) const
in file fields/fvPatchFields/basic/generic/genericFvPatchField.C at line 692.

FOAM exiting

Hi Amin,

this errors essentially means that the solver can't find the timeVaryingUniform boundary condition.

In OpenFOAM-1.6-ext, there doesn't seem to be a boundary condition called "timeVaryingUniform".

If you check in the directory $FOAM_SRC/finiteVolume/fields/fvPatchFields/derived, you can see the time varying boundary conditions, they are:
timeVaryingFlowRateInletVelocity
timeVaryingMappedTotalPressure
timeVaryingUniformTotalPressure
timeVaryingMappedFixedValue
timeVaryingUniformFixedValue
timeVaryingMappedPressureDirectedInletVelocity
timeVaryingUniformInletOutlet

Maybe you mean to use one of these?

Best regards,
Philip

[amin144]

Hi dear philip
Thanks for your quick reply

I have used timeVaryingUniformFixedValue but it doesn't work

maybe ma data file is not correct or maybe I should add any library to solver and recompile it
I'm confused

[wyldckat]

Hi Amin,

You're lucky I had a 1.5-dev build in my machine. I've taken a look at the first case you provided and the modified version is attached.

Changes:

• I had to fix "wallup" as "Wallup" in the files at the "0" folder.
• Saw the list of possible BCs by running this command (1.5-dev is really old... the "bananas" trick didn't work ):
  

  tree $FOAM_SRC/finiteVolume/fields/fvPatchFields

• Switched to "timeVaryingUniformFixedValue" in the file "0/p".
• icoFoam started complaining about missing info. To be in compliance with the complaints, I ended up with:

  inlet
  {
       type timeVaryingUniformFixedValue;
       outOfBounds clamp;
       fileName "inlet.dat";
       value uniform 1e5 ;
  }

• Also had to modify "inlet.dat" to something more... compliant:
  

  (
   (0.0 1.0)
   (0.01 5 )
   (0.02 10)
   (0.03 20)
   (0.07  100)
  );

Have fun trying to make this work, because with me, icoFoam just blasted the Courant number out of the ballpark...

Best regards,
Bruno

[amin144]

oh!
What a nice and great favor from you
Thanks dear Bruno

I wish I can help others in future in this forum
Atthaching cases is a good job because someone else who have problem like me can solve his/her problem very very quickly

[wyldckat]

Originally Posted by amin144

Atthaching cases is a good job because someone else who have problem like me can solve his/her problem very very quickly

Or they'll simply go deeper into trouble... of not knowing what they're doing

[amin144]

But there isn't any known and clear reference to understanding deeply
maybe trial and error is a way for learning OF
It would be nice and great work if there be a extended and expanded user guide which is summarize of threads in forum

[wyldckat]

Originally Posted by amin144

It would be nice and great work if there be a extended and expanded user guide which is summarize of threads in forum

Yes it would be great work... and a lot of work... and a lot of time! And very... veeeery tedious

Nonetheless, there are at least 2 places where you or anyone else can do this kind of information collection and cataloguing:

• The personal Blog made available to each member here at cfd-online.com/Forums, namely at http://www.cfd-online.com/Forums/blogs/
• Then there is the unofficial openfoamwiki.net.

And as you can see from my signature link, my focus here at the forum has been of cataloguing the installation methods and some other details...