CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   turbDyMFoam and refineMesh utility (http://www.cfd-online.com/Forums/openfoam/85496-turbdymfoam-refinemesh-utility.html)

fusij February 27, 2011 22:57

turbDyMFoam and refineMesh utility
 
Hello all,

I have been developing a case using the turbDyMFoam solver. I use blockMesh to create my mesh and have been using the refineMesh utility to decrease grid spacing around an object. When I run the solver after having pre-processed the case I get the following terminal output:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create dynamic mesh for time = 0

Selecting dynamicFvMesh mixerGgiFvMesh
void mixerGgiFvMesh::addZonesAndModifiers() : Zones and modifiers already present. Skipping.
Mixer mesh:
origin: (0 0 0)
axis : (0 0 1)
rpm : 16
Reading field p

Reading field U

Reading/calculating face flux field phi

Segmentation fault


When I run the case without using the refineMesh utility it works just fine. Also, when I view the mesh before I run it after I have used the refineMesh utility, it looks just the way I want. So the utility is working for me.

Maybe there is some conflict because of the sets that get created? Has someone encountered a similar problem or can point to a possible solution to this problem?

Thank you.

fusij February 28, 2011 11:49

Now I am able to proceed little bit further or until the next timestep. Then this comes up:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create dynamic mesh for time = 0

Selecting dynamicFvMesh mixerGgiFvMesh
void mixerGgiFvMesh::addZonesAndModifiers() : Zones and modifiers already present. Skipping.
Mixer mesh:
origin: (0 0 0)
axis : (0 0 1)
rpm : 16
Reading field p

Reading field U

Reading/calculating face flux field phi

Initializing the GGI interpolator between master/shadow patches: insideSlider/outsideSlider
Evaluation of GGI weighting factors:
Largest slave weighting factor correction : 9.000149e-05 average: 5.829659e-05
Largest master weighting factor correction: 3.066436e-13 average: 1.706539e-15

Selecting incompressible transport model Newtonian
Selecting RAS turbulence model kEpsilon
kEpsilonCoeffs
{
Cmu 0.09;
C1 1.44;
C2 1.92;
alphaEps 0.76923;
}

Reading field rAU if present


Starting time loop

Courant Number mean: 0.4258401 max: 2.4 velocity magnitude: 3
deltaT = 0.001041667
Time = 0.001041667

Segmentation fault


I know now that the segmentation fault arises because OF is trying to go into a list or similar with an index that is out of the list's domain. Since I do not have the debug option on with my OF compilation, I am not able to see where exactly this happens.
Can someone help me on this one or does someone now what the solver is doing when this happens (What is happening after the timestep calculation)?

linnemann February 28, 2011 12:40

Hi

This is a common mistake.

using mixerGgiFvMesh the cellZone MUST be named "movingCells"

This name is hard-coded into the code so thats why.

Open your constant/polyMesh/cellZones file and change the name.

I bet this is the error.

fusij February 28, 2011 12:54

Thank you very much, this works like a charm it seems. At least the compilation is running now. You are a genius!

aqua November 18, 2011 11:23

Hi, could you please tell me in which version of OpenFoam i can find the solver turbDymFoam? I have been looking forward to that for a long time...thank you so much!
Quote:

Originally Posted by fusij (Post 297222)
Hello all,

I have been developing a case using the turbDyMFoam solver. I use blockMesh to create my mesh and have been using the refineMesh utility to decrease grid spacing around an object. When I run the solver after having pre-processed the case I get the following terminal output:

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create dynamic mesh for time = 0

Selecting dynamicFvMesh mixerGgiFvMesh
void mixerGgiFvMesh::addZonesAndModifiers() : Zones and modifiers already present. Skipping.
Mixer mesh:
origin: (0 0 0)
axis : (0 0 1)
rpm : 16
Reading field p

Reading field U

Reading/calculating face flux field phi

Segmentation fault


When I run the case without using the refineMesh utility it works just fine. Also, when I view the mesh before I run it after I have used the refineMesh utility, it looks just the way I want. So the utility is working for me.

Maybe there is some conflict because of the sets that get created? Has someone encountered a similar problem or can point to a possible solution to this problem?

Thank you.


bluebase December 12, 2011 09:22

Hi aqua,

in the latest version turbDymFoam is called pimpleDymFoam.

The two solvers turbDymFoam and icoDymFoam were merged. By selecting a turbulence modell or laminar flow you now can choose between the two old solvers.

aqua December 12, 2011 10:39

Hi, Thank you so much for your reply!

Cheers!
Quote:

Originally Posted by bluebase (Post 335539)
Hi aqua,

in the latest version turbDymFoam is called pimpleDymFoam.

The two solvers turbDymFoam and icoDymFoam were merged. By selecting a turbulence modell or laminar flow you now can choose between the two old solvers.



All times are GMT -4. The time now is 08:42.