CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Questions to Dynamic Mesh solver and diffusivity (http://www.cfd-online.com/Forums/openfoam-solving/59234-questions-dynamic-mesh-solver-diffusivity.html)

florian_krause January 10, 2008 06:16

Hi OF-Folks, working on a s
 
Hi OF-Folks,

working on a simulation of a sinking (rigid) particle in a water cylinder with a modified icoDyMFoam(OF-1.4.1) I run in trouble with the mesh quality.

I tried several diffusivity algorithms:

directional: bad results after a relative short time
quadratic: good results for mesh quality, even if the particle goes through half of the cylinder
exponential: bad and confusing mesh moving after a short time

It was more or less trial and error because I dont really know what the different diffusivity algorithms do and stand for. And I dont know what the values after the keyword stand for, like:

exponential 2000

Does anyone know and has experience with the different diffusivity options and the influence of the values???Is there a documentation of this?

For solvers I use:

dynamicFvMesh dynamicMotionSolverFvMesh
motionSolverLibs libfvMotionSolvers.so
solver velocityComponentLaplacian

I know from several "moving mesh" threads from the forum that there exits other solvers in OF, but does anyone know in which case it is better to use which solver?

I know, alot of question to a often discussed topic. But I really appreciate any help and hints! http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Thanks & Kindest Regards,
Flo

lr103476 January 10, 2008 17:02

Hi Florian, Generally quad
 
Hi Florian,

Generally quadratic inverseDistance diffusivity gives pretty good (if not the best) results for plunging bodies. For that kind of simulations I use the fvMotionSolver, velocityLaplacian. When you are encountering large rotations, the laplacian is not the right equation to use, a good alternative would be the displacementSBRStress motion solver. For really large rotation, subsets of meshes or user defined diffusivity could provide solutions......This is what I am dealing with now :-S

The following paper describes some theory about the laplacian motion solver:
http://powerlab.fsb.hr/ped/kturbo/Op...Manuscript.pdf


Regards, Frank

lr103476 January 10, 2008 17:15

How large is you body translat
 
How large is you body translation / rotation ???

Frank

florian_krause January 10, 2008 17:41

Hi Frank, by now I have no
 
Hi Frank,

by now I have no (or very less) rotation of my particle, but I think large deformation.

The paper from Jasak and Tukovic is definitly what I was searching for - its a good discription of the background of the solver and the diffusivity terms http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

I will send you a two pictures - one of the deformed mesh and one of the undeformed mesh - to your eMail adress ok?!

Regards,
Florian

florian_krause January 10, 2008 18:11

ok.. I try to post them here
 
ok.. I try to post them here

I use quadratic diffusivity in this case, and at this time I only have some nonorthogonal faces

http://www.cfd-online.com/OpenFOAM_D...ges/1/6371.jpg

http://www.cfd-online.com/OpenFOAM_D...ges/1/6372.jpg

Regards,
Florian

florian_krause January 10, 2008 18:52

In fact the screeshot of the d
 
In fact the screeshot of the deformed mesh is not really representative and only gives an idea of the mesh deformation... My 3D Mesh only consists of hexa cells, but making a cut in paraView the visualization of the cut cells is very strange - something like R-Trias...

But this is another, not soo important issue ;)

Regards,
Florian

lr103476 January 11, 2008 04:04

If the sphere is moving down a
 
If the sphere is moving down all the way, you really need some cell layering.

Visualization of moving 3D meshes is really a pain, I use ensight to visualize complete cells instead of a cutting plane.....

Frank

florian_krause January 11, 2008 05:33

Frank, I agree with you reg
 
Frank,

I agree with you regarding the use of additional/removal layer because my cell layers faces are parallel.

But what happens when I have a unstructured Tet mesh? The structued Hex Mesh was only possible because I have only one sphere and buliding the more or less good hex mesh around the cylinder was not the easiest thing.

For the add/rem cell layer I think I need something like:


dynamicFvMeshLibs ("libtopoChangerFvMesh.so");

dynamicFvMesh topoChangerFvMesh;

solver velocityLaplacian ;

How can I define the max and min layer thickness in the dynamicMeshDict?

Regards,
Florian

lr103476 January 11, 2008 05:44

I haven't use cell layering be
 
I haven't use cell layering before, so I don't know ....Try to look inside the code to find out how you define the dictionary....it's quit easy.

Frank

florian_krause January 11, 2008 05:54

I found a topo Change movingCo
 
I found a topo Change movingCone example from the OF 1.4.1 dev source, I will check on it what is necassary for add/rem cell layers http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Regards,
Florian

msrinath80 January 11, 2008 07:10

Florian, for the sphere are yo
 
Florian, for the sphere are you also solving for the conservation of angular momentum?

florian_krause January 11, 2008 21:35

Hi pUI, when I simulate the
 
Hi pUI,

when I simulate the sinking process, I start with a (0 0 0) velcoity vector for the sphere. For the next iteration I calculate the new velocity for n+1 iteration with the resulting gravity force, the pressure/viscous force and the velocity from iteration n.

Further, I calculate the moments on the sphere BUT I dont use the results for the moments to update the the velocity and dont take into account the possible influence of the moments on the rotation of the sphere.

So, I dont think that I solve the conservation of angular momentum, but its a good hint for the future... ;)

Is this what you mean?

Regards,
Florian

msrinath80 January 11, 2008 22:33

yup, thanks
 
yup, thanks


All times are GMT -4. The time now is 19:53.