[Daniel_Khazaei]

Originally Posted by sloti

Hi everyone,

I had a look at Philips FSI solver and am especially excited about the possibility to run it in parallel, as icoFsiFoam is apparently not running in parallel yet.

However, I managed to run the HronTurekFsi case in parallel but I can't reconstruct the data.. the results of the processors are all stored under the fluid/processor*/"time" folder where also the solid results are located within another folder (fluid/processor*/"time"/solid). When I run reconstructPar that folder is ignored and only the fluid data is reconstructed.

Probably I just make a stupid fault.. Any help would be appreciated!

Regards, Anna

Update: problem solved. not sure whether this is the most elegant way, but I wrote a batch sorting things out!

Hi Anna

were you able to run the FSI case in parallel without any problem? (completely I mean, end of simulation time)
I have a problem you can see in this post : click

@ Dr. Cardiff

can FSI solver handle multiple FSI interfaces that are separate?

[bigphil]

Originally Posted by Daniel_Khazaei

can FSI solver handle multiple FSI interfaces that are separate?

Hi Daniel,

the solver currently setup to use only one FSI interface; however, it should be straight-forward to extend it to an arbitrary number if you don't mind a bit of coding.
Alternatively, you could merge your patch to make sure you have only one FSI interface (it doesn't matter is the FSI interface is discontinuous).

Philip

[davidsblom]

Hi,

I've modified the settings of the test case to run the FSI2 case. However, after some simulation time the solver stops, and when I look into the mesh there is a large overlap at the tip of the flap.I have attached a couple of screenshots in order to visualize the problem.

https://dl.dropboxusercontent.com/u/...pshot3.png.zip

Any idea what is happening here? Is the interpolation between the solid and fluid mesh which is not correct? Or the problems lies somewhere else? Hints anyone?

Thanks alot!

Best regards,
David

[VincentChai]

Hi Philip,

I am trying to plot the displacement of the plate (at the plate back center point)
in paraView by create selection and "plot selection over time", however, the following error appear:

ERROR: In /home/vin-82/OpenFOAM/OpenFOAM-1.6-ext/ThirdParty/rpmBuild/BUILD/ParaView-3.12.0/VTK/Charts/vtkContext2D.cxx, line 177
vtkContext2D (0x9ce0930): Attempted to paint a line with <2 points.

and there is no data appear on the plot.
May i know how to solve this problem?
Thanks

[bigphil]

Originally Posted by VincentChai

Hi Philip,

I am trying to plot the displacement of the plate (at the plate back center point)
in paraView by create selection and "plot selection over time", however, the following error appear:

ERROR: In /home/vin-82/OpenFOAM/OpenFOAM-1.6-ext/ThirdParty/rpmBuild/BUILD/ParaView-3.12.0/VTK/Charts/vtkContext2D.cxx, line 177
vtkContext2D (0x9ce0930): Attempted to paint a line with <2 points.

and there is no data appear on the plot.
May i know how to solve this problem?
Thanks

Hi Vincent,

I have noticed problems using the ParaView filter "Plot selection over time" when there are a large number of time-steps.

So I would suggest you try a test case with about 10 time-steps and see if that works, then try large numbers of time-steps.

Best regards,
Philip

[Daniel_Khazaei]

@ Dr. Cardiff

I want to use dynamicRefineFvMesh as a dynamicFvMesh in dynamicMeshDict on FSI solver. I have changed what I think is necessary for dynamicRefineFvMesh.

But I am still getting this error:

Time = 1e-06, iteration: 3
Current fsi under-relaxation factor (Aitken): 0.999595
Maximal accumulated displacement of interface points: 0.0251937


--> FOAM FATAL ERROR: 
Problem with mesh motion solver selection

    From function pimpleFsiElasticNonLinULSolidFoam
    in file moveFluidMesh.H at line 140.

FOAM aborting

Aborted (core dumped)

is it possible to use dynamicRefineFvMesh with FSI solver?


regards

[bigphil]

@Bruno
Nice work!

@Daniel
Sorry, I am not familiar with dynamicRefineFvMesh.

Philip

[Daniel_Khazaei]

Originally Posted by bigphil

@Bruno
Nice work!

@Daniel
Sorry, I am not familiar with dynamicRefineFvMesh.

Philip

Hi Dr. Cardiff

sorry for lots of questions

Does FSI solver support topological changes in the fluid region?
I want to use dynamicTopoFvMesh for my test case, I have problems with PatchToPatchInterpolation.

this problem occurs after mesh refinement.


regards

[VincentChai]

Hi Philip,

Good morning!
I have found a file "gpDeflection" in the tutorial, is this file for plotting the deflection of the plate? Thanks.



Regards,
Vincent

[cutty4sark]

I've been following this post for some time and having been playing around with trying to merge the CHT solver with the FSI solver. The problem I keep coming back to is how the different solvers handle the solid and fluid. In the FSI solver, there are separate directories for the different regions with separate meshes whereas the CHT solver seems to lump everything together into one mesh with different regions. Am I wrong in thinking that there will need to be some major reworking of how the CHT handles the fluid and solid since it does not match the FSI solver? Any pointers would certainly be appreciated and I will happily share results if there ever are any! Also, if I need to clarify anything, please let me know.

[Daniel_Khazaei]

Hi Dr. Cardiff

I am working on simulation of flexible pipe with FSI solver.
I have changed the fluid solver to use pimple algorithm.

I have a question about FSI outer corrector:

In my simulation, in each time step I get only 3 outer iteration for every time step. The solver also produces FSI under relaxation factor higher than 1 (e.g. 1.00078)

furthermore, FSI residual suddenly drop in iteration 3, it acts like:

iteration #1: fsi residual = 1

iteration #2: fsi residual = 0.997888

iteration #3: fsi residual = 5.4322e-5

Any suggestion would be appreciated, tell me if you need more information about case setup.


regards

[ahmmedshakil]

Hi Cardif,
I'm having problem with the analytical solution of the hot Cylinder case that is provided with the elasticThermalSolidFoam. When I run the case it gives error like this:
Create time

Create mesh for time = 0

Writing analytical solution for a plain strain cylinder with concentric hole,
where
inner radius = 0.5
outer radius = 0.7
inner temperature = 100
outer temperature = 0
inner pressure = 0
outer pressure = 0
E = 200e9
u = 0.3
alpha = 1e-5

Writing analytical termpature field

Writing analytical sigmaR field

Writing analytical sigmaTheta field

Writing analytical sigmaZ field
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3
in "/home/adminuser/OpenFOAM/adminuser-2.1.0/platforms/linux64GccDPOpt/bin/analyticalHotCylinder"
#4 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#5
in "/home/adminuser/OpenFOAM/adminuser-2.1.0/platforms/linux64GccDPOpt/bin/analyticalHotCylinder"
Basically it creates the problem when calculating the sigmaZ. Will you please suggest me how to get rid of this??

Originally Posted by bigphil

Hi Sangeeta,

The solidMechanics solvers and library use a number of features (such as GGI) that are only found in the OpenFOAM Extend (not the standard OpenCFD OpenFOAM). Therefore, I would recommend you install OpenFOAM-1.6-ext if you want to use solidMechanics (Note: OpenFOAM-1.6.x is released by OpenCFD and OpenFOAM-1.6-ext is realised by the Extend Project).

It would probably be possible to compile the solvers in standard OpenFOAM but you would have to exclude quite a bit of the functionality. So it is much easier to install OpenFOAM-1.6-ext.

Philip

[ahmmedshakil]

I solved the problem. It was coming from the atan(y/x) function. I am using OpenFoam 2.1.0 and for two argument passing through arc tan function -->the correct function is: atan2(y,x).

Originally Posted by ahmmedshakil

Hi Cardif,
I'm having problem with the analytical solution of the hot Cylinder case that is provided with the elasticThermalSolidFoam. When I run the case it gives error like this:
Create time

Create mesh for time = 0

Writing analytical solution for a plain strain cylinder with concentric hole,
where
inner radius = 0.5
outer radius = 0.7
inner temperature = 100
outer temperature = 0
inner pressure = 0
outer pressure = 0
E = 200e9
u = 0.3
alpha = 1e-5

Writing analytical termpature field

Writing analytical sigmaR field

Writing analytical sigmaTheta field

Writing analytical sigmaZ field
#0 Foam::error:rintStack(Foam::Ostream&) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#1 Foam::sigFpe::sigHandler(int) in "/opt/openfoam210/platforms/linux64GccDPOpt/lib/libOpenFOAM.so"
#2 in "/lib/x86_64-linux-gnu/libc.so.6"
#3
in "/home/adminuser/OpenFOAM/adminuser-2.1.0/platforms/linux64GccDPOpt/bin/analyticalHotCylinder"
#4 __libc_start_main in "/lib/x86_64-linux-gnu/libc.so.6"
#5
in "/home/adminuser/OpenFOAM/adminuser-2.1.0/platforms/linux64GccDPOpt/bin/analyticalHotCylinder"
Basically it creates the problem when calculating the sigmaZ. Will you please suggest me how to get rid of this??

[Daniel_Khazaei]

Hello Dr. Cardiff

I have tested my case with fixedRelaxationFactor method with value of 0.2 and the solution will converge and FSI residual reduces smoothly and after 43 outer iterations it will reach to FSI convergence tolerance.

Is there anything special that I am missing with Aitken method?

I have found this old topic with the same problem that I have:

http://www.cfd-online.com/Forums/ope...ation-fsi.html


regards

[bigphil]

@Daniel
As regards topological changes, changes may be required but I do not have any experience with this.

As regards "Aitken" vs. "Fixed" relaxation, there is quite a bit of literature on this for FSI if you search google. For instance, the implemented Aitken procedure is presented here by Z. Tukovic.

@Vincent
The "gpDeflection" file is a gnuplot script; but it was used when the solver specifically wrote out the beam tip displacement to a file. It was removed to make the code more generic, it would have to be coded in to the solver.

@ahmmedshakil
Thanks for the fix!

Philip

[Daniel_Khazaei]

Originally Posted by bigphil

@Daniel
As regards topological changes, changes may be required but I do not have any experience with this.

As regards "Aitken" vs. "Fixed" relaxation, there is quite a bit of literature on this for FSI if you search google. For instance, the implemented Aitken procedure is presented here by Z. Tukovic.

Philip

Nice to have you back

thanks for the answer.

well I have read 4 papers so far on coupling algorithm, Fixedrelaxation, Aitken and IQN-ILS. But I can not understand why fsi under relaxation factor goes higher than 1.

This is the case I am working on it for now: (you can see the geometry in attachment)

as for the fluid region:

fluid/0/motionU:

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    FSI
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    OUTLET
    {
         type            zeroGradient;
    }
    INLET
    {
        type            zeroGradient;
    }
}

fluid/0/p

dimensions      [0 2 -2 0 0 0 0];

internalField   uniform 0;

boundaryField
{
    FSI
    {
        type            zeroGradient;
    }
    OUTLET
    {
        type            fixedValue;
        value           uniform 0;
    }
    INLET
    {
        type            fixedValue;
        value           uniform 50;
    }
}

fluid/0/U

dimensions      [0 1 -1 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    FSI
    {
        type            fixedValue;
        value           uniform (0 0 0);
    }
    OUTLET
    {
        type            zeroGradient;
    }
    INLET
    {
        type            pressureInletVelocity;
        value        uniform (0 0 0);
    }
}

for the solid region (DU):

dimensions      [0 1 0 0 0 0 0];

internalField   uniform (0 0 0);

boundaryField
{
    FSI
    {
        type solidTraction;
        nonLinear updatedLagrangian;
        traction uniform ( 0 0 0 );
        pressure uniform 0;
        value uniform (0 0 0);
    }

    O_WALL
    {
        type solidTraction;
        nonLinear updatedLagrangian;
        traction uniform ( 0 0 0 );
        pressure uniform 0;
        value uniform (0 0 0);
    }

    INLET
    {
       type            zeroGradent;
    }

    OUTLET
    {
       type            zeroGradent;
    }
}

for coupling properties:

solidPatch FSI;
solidZone FSIZone;


fluidPatch FSI;
fluidZone FSIZone;

//movingRegion region0;

fsiRelaxationFactor 0.01;

interfaceDeformationLimit 0.01;

outerCorrTolerance 1e-4;

couplingScheme Aitken;

fsi yes;

for dynamicMesh settings:

dynamicFvMesh   dynamicMotionSolverFvMesh;

twoDMotion      no;

//solver          velocityLaplacian;

solver          laplaceFaceDecomposition;

diffusivity quadratic inverseDistance 1(FSI);

frozenDiffusion yes;

distancePatches 
(
    FSI
);

what movingWallVelocity actually does? when I use it in my case I get floating point exception error. (instead I am using fixedValue)

Is there anything obviously wrong with my setup? Actually I dont know what kind of boundary condition should I use for patch which is shown by arrow in the attachment.


sorry for long question!

regards

[ahmmedshakil]

Hi,
I'm solving similar problem as arc welding in thin plate. I'm using elasticThermalSolidFoam solver. In my cases, I have to impose the boundary condition for U as follows (given in diagram also),
(a) At X=0 and X= L ------------> sigmaxx = 0, sigmaxy =0,
(b) At Y=0 -------------> du/dy =0, v=0,
(c) At Y =H ---------------> sigmayx =0, sigmayy=0.
As I am new to solid mechanics solver in OpenFoam, I'm wondering which boundary condition should I use.... either it
(1) fixedDisplacement boundary with value (0 0 0) OR
(2) fixedDisplacementZeroShare with value (0 0 0) OR anything else
Anyone have idea which boundary condition I can use??

| Y sigmayx=0, sigmayy=0
|---------------------------------------------------------|
| |
sigmaxx=0 | | sigmaxx=0
sigmaxy=0 | | sigmaxy=0
| |
| |
|---------------------------------------------------------|-------------->X
du/dy =0, v=0

The problem is similar to the case 4.4 mentioned by the paper: "I. Demirdžić, D. Martinović Finite volume method for thermo-elasto-plastic stress analysis, Computer Methods in Applied Mechanics and Engineering, vol 109, 331-349".

[ahmmedshakil]

Sorry, the image will be as attached (above the diagram a bit disfigured)..

Originally Posted by ahmmedshakil

Hi,
I'm solving similar problem as arc welding in thin plate. I'm using elasticThermalSolidFoam solver. In my cases, I have to impose the boundary condition for U as follows (given in diagram also),
(a) At X=0 and X= L ------------> sigmaxx = 0, sigmaxy =0,
(b) At Y=0 -------------> du/dy =0, v=0,
(c) At Y =H ---------------> sigmayx =0, sigmayy=0.
As I am new to solid mechanics solver in OpenFoam, I'm wondering which boundary condition should I use.... either it
(1) fixedDisplacement boundary with value (0 0 0) OR
(2) fixedDisplacementZeroShare with value (0 0 0) OR anything else
Anyone have idea which boundary condition I can use??

| Y sigmayx=0, sigmayy=0
|---------------------------------------------------------|
| |
sigmaxx=0 | | sigmaxx=0
sigmaxy=0 | | sigmaxy=0
| |
| |
|---------------------------------------------------------|-------------->X
du/dy =0, v=0

The problem is similar to the case 4.4 mentioned by the paper: "I. Demirdžić, D. Martinović Finite volume method for thermo-elasto-plastic stress analysis, Computer Methods in Applied Mechanics and Engineering, vol 109, 331-349".

[bigphil]

Hi ahmmedshakil,

For your boundary conditions, the left, top and right are traction boundaries so use solidTraction with zero pressure and traction.

For the bottom boundary, it is effectively a symmetryPlane (zero normal displacement, zero normal gradient of shear displacements). directionMixed can be also be used but is only necessary when the normal displacement is non-zero.

Philip

[bigphil]

Hi Daniel,

Originally Posted by Daniel_Khazaei

well I have read 4 papers so far on coupling algorithm, Fixedrelaxation, Aitken and IQN-ILS. But I can not understand why fsi under relaxation factor goes higher than 1.

If you search for "Aitken acceleration" on google, you will finds lots of explanations, but essentially the acceleration factor does not have to be limited to be less than 1 or even positive.
As regards application of the Aitken's method to under-relaxation in FSI procedure, sometimes people may limit it but I am not sure of the reasoning (maybe they feel uncomfortable with relaxation factor >1 and/or <0)

Originally Posted by Daniel_Khazaei

what movingWallVelocity actually does? when I use it in my case I get floating point exception error. (instead I am using fixedValue)

You should be able to find descriptions of movingWallVelocity on the forum or at least in the code.
As far as I know, it is a boundary condition for the fluid velocity field for a wall that is moving.
This should not be used as a solid boundary condition.

Originally Posted by Daniel_Khazaei

Is there anything obviously wrong with my setup? Actually I dont know what kind of boundary condition should I use for patch which is shown by arrow in the attachment.

I don't think you have set the correct boundary condition types for FSI in U and DU.
As regards what boundary condition to use for the patch shown, this depends on what physical condition you want to enforce. Typically you don't use zeroGradient as a solid boundary as it does not really correspond to a physical condition (it's kind of like zero strain).

Philip