CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Paraview & paraFoam (http://www.cfd-online.com/Forums/openfoam-paraview/)
-   -   PolyMesh Question (http://www.cfd-online.com/Forums/openfoam-paraview/61268-polymesh-question.html)

tj22 June 19, 2006 10:13

In regards to a simulation tha
 
In regards to a simulation that has a mesh that changes with time. If the only instance of polyMech occurs in the constant folder then that mesh is used for the whole simulation. And if there is an instance of polyMesh within each time then the mesh is reloaded each time step.

My question is if there is a polyMesh in constant and one in time step 1, do I use the mesh from constant or from timestep 1 for my other timesteps?

Or is it impossible for this to happen?

Thanks.

lucchini June 19, 2006 10:26

Hi Terry, I hope this can b
 
Hi Terry,

I hope this can be helpful....

======================================
CASE 1

startTime 0;
no mesh in 0/polyMesh
the solver will create the mesh from constant/polyMesh
======================================
CASE 2

startTime 1;
no mesh in 1/polyMesh
the solver will create the mesh from constant/polyMesh
======================================
CASE 3

startTime 1;
mesh defined in 1/polyMesh
the solver will create the mesh from 1/polyMesh
=====================================

Regards.
Tommaso

tj22 June 19, 2006 11:06

I need to clarify my question.
 
I need to clarify my question. I am not running the simulations I am using the visualizing the results in paraview using a reader I am writing, so I know the following:

There will be a polymesh in constant.
There can be a polymesh in the time steps.

My question is if there is a polymesh dir in constant and say time step 1 and none in the others. For say, time step 3 do I use the polymesh instances from timestep 1 or constant?

Or is it not possible to have polymeshes at random time steps ie if there is a polymesh directory in timestep 1, there will also be one in 2,3,4..etc?

Thanks.

eugene June 19, 2006 11:49

For this purpose, just think o
 
For this purpose, just think of constant as time = -1

The mesh from the most recent timestep will generally be used (unless specified otherwise).

It is possible to have polyMeshes in any combination of timesteps and/or constant. The above still holds.

tj22 June 19, 2006 15:33

In which file is that specifie
 
In which file is that specified?

mattijs June 20, 2006 02:32

The current time is specified
 
The current time is specified normally by system/controlDict (for OF applications) or by the time slider (in the ParaFoam reader).

From there it searches backwards for the first time directory containing polyMesh/points (those are the new points, i.e. geometry) and same for polyMesh/faces (and from this it reads the topology - owner,neighbour,faces,points,boundary). They can be different!

tj22 June 20, 2006 07:14

So the points can reside separ
 
So the points can reside separately at one time say "constant" and the other attributes (faces, owner, neighbor, boundary, cellzones, pointzones, and facezones) will reside together at another time say timestep 1?

mattijs June 21, 2006 03:21

No, but the other way round ca
 
No, but the other way round can: the geometry ('points') is 'newer' than the topology.

Basically if the mesh is moving we only write out the 'points' file but if the mesh topology is changing we write out all the files (including points)

tj22 June 21, 2006 08:15

OK. Thanks.
 
OK. Thanks.


All times are GMT -4. The time now is 05:52.