[lr103476]

Hi,

I've got some problems converting movingFlapFvMesh to OpenFOAM version 1.3. Before putting my compiler errors in this forum, I will ask you the following question:

Are there any fundamentally different changes in the way the mesh moves? If any, how is the easiest way to convert movingFlapFvMesh to the new version.

Regards,
Frank

[hjasak]

There has been a bunch of name changes but without substantial algorithmic changes (e.g. various motion solvers are now run-time selectable + you can choose your diffusion model at run-time as well). On top of that, there is a new virtual base class for dynamicFvMeshes, called (obviously) dynamicFvMesh. If you wish to use the dynamic mesh top-level solvers which rely on the virtual base class.

Anyway, I'm not sure why you want to rewrite the moving flap example: should it not be enough to take the dynamicMotionSolverFvMesh and play around with the boundary conditions? If you use the oscillating fixed value boundary conditions you're 99% there; if you want a full 6-DOF solver kind of thing (this would include phase lags and independent frequency in each direction), only a small extension of the boundary condition is required.

In any case, the bulk of your job is already done in the dynamicMotionSolverFvMesh.

Hrv

Hrv

[lr103476]

Allright. In version 1.2 I used the movingFlapFvMesh class to provide for the motion. Last week I moved to version 1.3, which involved some rewriting of my user apps. So for the motion I automatically took the old movingFlapFvMesh stuff.

I think you're right, modifying the boundary condition of the wing to make it oscillate should do the trick. Could you give a hint of where to start, which class do I have to copy (to my userapps) and modify for my needs.

Regards, Frank

[lr103476]

allright, I setup the case using oscillatingFixedValue BC's, but nothing is moving though.

Right now I use for the wing wall the following settings for motionU:

wing_wall
{
type oscillatingFixedValue;
refValue uniform (1 0 0);
amplitude 1.0;
frequency 10.0;
}

And for U, I use:
wing_wall
{
type fixedValue;
value uniform (0 0 0);
}

What am I doing wrong?

Regards, Frank

[hjasak]

Easy: have a look at your flux file and you will see you've got a flux through the wall.

This is because you have specified the velocity to be zero in the absolute reference frame and the wall is moving: the real velocity is not zero.

Use the movingWallVelocity boundary condition on U and all will be well. This corrects the normal component of your velocity b.c. to allow you to specify the b.c. with respect to the moving reference frame of your wall.

Clever or what? :-)

Hrv

[lr103476]

OK, I understand. But still no motion occurs. The point is that I used the movingFlapFvMesh in previous simulations, but I am not familiar with this oscillatingFixedValue BC.

Now I have in the 0/motionU:
wing_wall
{
type oscillatingFixedValue;
refValue uniform (1 0 0);
amplitude 1.0;
frequency 10.0;
}

And for 0/U, I use:
wing_wall
{
type movingWallVelocity;
value uniform (0 0 0);
}

I use the standard icoDyMFoam solver. Still no motion occurs as can be seen from the output below. Nothing has to be solved for motionUx,y,z.

================================================
================================================

Mean and max Courant Numbers = 0.0230254 1.04542
deltaT = 0.007945
Time = 0.02055

Correct mesh motion diffusion field.
ICCG: Solving for motionUx, Initial residual = 0, Final residual = 0, No Iterations 0
ICCG: Solving for motionUy, Initial residual = 0, Final residual = 0, No Iterations 0
ICCG: Solving for motionUz, Initial residual = 0, Final residual = 0, No Iterations 0
ICCG: Solving for pcorr, Initial residual = 1, Final residual = 9.80538e-07, No Iterations 340
time step continuity errors : sum local = 4.59652e-14, global = -3.76461e-16, cumulative = -6.50917e-11
BICCG: Solving for Ux, Initial residual = 0.918317, Final residual = 1.91578e-06, No Iterations 2
BICCG: Solving for Uy, Initial residual = 0.0853413, Final residual = 1.68193e-06, No Iterations 2
ICCG: Solving for p, Initial residual = 0.00112938, Final residual = 9.66379e-07, No Iterations 237
time step continuity errors : sum local = 5.45017e-08, global = 2.95663e-10, cumulative = 2.30571e-10
ICCG: Solving for p, Initial residual = 0.00151305, Final residual = 9.19579e-07, No Iterations 203
time step continuity errors : sum local = 4.49651e-08, global = 8.32157e-11, cumulative = 3.13787e-10
ExecutionTime = 22.12 s ClockTime = 22 s

================================================
================================================

What do I wrong? Do I have to define the amplitude /frequency in the dynamicMeshDict, or so?


Regards, Frank

[hjasak]

Sounds like a boundary condition problem to me. Do you my any chance have a 2-D geometry with a symmetry plane front and back? Also, have a look at the motionU files in the time directories and see if the b.c. value changes.

I have changed the way oscillaing b.c. works for me so I cannot answer the detailed setup question. The fixed value is calculated by multiplying with the current scale as:

currentScale() const
{
return Foam::cos
(
2*mathematicalConstant::pi*frequency_*
this->db().time().value()
);
}

and

patchField = refValue_ + amplitude_*currentScale();

That all looks fine to me. In short, your b.c. looks OK, but you need to find out what else in the setup is stopping you from getting the motion.

Hrv

[lr103476]

I still have a 2D geometry with two empty planes front and back. Also, the bc value does not change in the time directories.

Since I use the oscillatingFixedValue out-of-the-box I assume that the implementation is correct. I also copied some of the solver settings of the movingCone case, but still no motion.

Do I have to define "amplitude" and "frequency" in the 0/motionU or in a separate oscillatingDict file or something like that.

Is there anyone else working with this oscillatingFixedValue BC?

Regards, Frank

[hjasak]

OK, I have prepared a little example for you. Have a look at the movie:

http://powerlab.fsb.hr/ped/kturbo/Op...MeshMotion.mpg

The b.c. specification I am using is:

movingWall
{
type oscillatingFixedValue;
refValue uniform (0 0 0);
amplitude uniform (0 0.2 0);
frequency 2;
value uniform (0 0 0);
}

As you see, it works fine.

Hrv

[hjasak]

Forgot to say: if you want the case, please E-mail me. Also, there may be a mionr difference on how you specify the amplitude (mine is a vector, yours might be a scalar), but that's easily fixed. You can put a print statement into the scaling furction to see if it is being called and if it's calculated correctly.

Hrv

[lr103476]

I cant get your case moving. It appears that you wrote an extra class, called solverLib, which is called in dynamicMeshDict.

I just replaced this line in dynamicMeshDict as shown below:

//solverLib "libtetDecompositionMotionSolver.so";
dynamicFvMeshLib "libtetDecompositionMotionSolvers.so";
dynamicFvMesh dynamicMotionSolverFvMesh;

twoDMotion yes;

solver laplaceTetDecomposition;

diffusion constant 1.0;

frozenDiffusion off;

distancePatches
(
movingWall
);

Furhter I initialised the U and p fields, such that I could use icoDyMFoam. Again no motion occurs. The motionU field is not updated in the new time directories.

Any ideas?

Regards, Frank

[hjasak]

Send me an E-mail and I'll give you access to my development source - I think that's the easiest way forward.

Hrv

[philippose]

Hello everybody,
A Good day to you all !

I use openFOAM 1.3, and have the need to do a moving mesh CFD analysis. I have been looking up the OpenFOAM forum, and noticed that there were many references to:

icoFoamAutoMotion

I dont seem to have this solver, and nor do I have the tutorial associated with it. I found "sonicFoamAutoMotion", but no "icoFoamAutoMotion".

Is there some way I can obtain this module?

Awaiting a reply!

Have a nice day!

Regards,

Philippose

[jens_klostermann]

Hi Phillipose,

as far as I know exists the icoFoamAutoMotion solver just until OF 1.2 .

Since OF 1.3 the solver for moving meshes is now called icoDyMFoam, see further information

http://www.opencfd.co.uk/openfoam/doc/ReleaseNotes-1.3

Regards Jens

[philippose]

Hello Jens,
Thank you very much for the information. I was wondering whether icoDyMFoam could be the same, because in the forums, I keep seeing Moving meshes referred to as "Dynamic meshes" too.

Shall try to use icoDyMFoam.

Have a nice day!

Regards,
Philippose

[lr103476]

Dear prof. Hrvoje,

Using your development code I am still not able to get your example (oscillatingCavityMesh) working. I assume that you probably also use some user libs.

Could you try to get your example working with the 'out-of-the-box' openFOAM 1.3? Is guess it should work.

Regards, Frank

[lr103476]

How do I access the currentScale() function and the amplitude/frequency values from my solver source files?

Info << "var =" << oscillatingFixedValueFvPatchField::currentScale() << nl << endl;

Something like this?

Regards, Frank

[hjasak]

Try:

1. Save the file in your home directory

run
tar xzf oscillatingCavityMesh.tgz
cd oscillatingCavityMesh
blockMesh $FOAM_RUN oscillatingCavityMesh
moveMesh $FOAM_RUN oscillatingCavityMesh
paraFoam $FOAM_RUN oscillatingCavityMesh

The animation is on the link above.

The file is attached. I am using my development version but I cannot recall any reason why this would not work. If you want my development sources, please let me know.

oscillatingCavityMesh.tgz

Hrv

[hjasak]

Doh. Go to

void oscillatingFixedValueFvPatchField<type>::updateCoe ffs() and do:

Info <<>currentScale() << endl;

Clear?

Hrv

[hjasak]

That lot should say

this - > currentScale()

all together. Looks like the forum software is playing games with me.