|
[Sponsors] |
June 19, 2006, 10:13 |
PolyMesh Question
|
#1 |
Member
Terry Jordan
Join Date: Mar 2009
Posts: 95
Rep Power: 17 |
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. |
|
June 19, 2006, 10:26 |
Hi Terry,
I hope this can b
|
#2 |
Member
Tommaso Lucchini
Join Date: Mar 2009
Posts: 87
Rep Power: 17 |
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 |
|
June 19, 2006, 11:06 |
I need to clarify my question.
|
#3 |
Member
Terry Jordan
Join Date: Mar 2009
Posts: 95
Rep Power: 17 |
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. |
|
June 19, 2006, 11:49 |
For this purpose, just think o
|
#4 |
Senior Member
Eugene de Villiers
Join Date: Mar 2009
Posts: 725
Rep Power: 21 |
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. |
|
June 19, 2006, 15:33 |
In which file is that specifie
|
#5 |
Member
Terry Jordan
Join Date: Mar 2009
Posts: 95
Rep Power: 17 |
In which file is that specified?
|
|
June 20, 2006, 02:32 |
The current time is specified
|
#6 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
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! |
|
June 20, 2006, 07:14 |
So the points can reside separ
|
#7 |
Member
Terry Jordan
Join Date: Mar 2009
Posts: 95
Rep Power: 17 |
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?
|
|
June 21, 2006, 03:21 |
No, but the other way round ca
|
#8 |
Senior Member
Mattijs Janssens
Join Date: Mar 2009
Posts: 1,419
Rep Power: 26 |
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) |
|
June 21, 2006, 08:15 |
OK. Thanks.
|
#9 |
Member
Terry Jordan
Join Date: Mar 2009
Posts: 95
Rep Power: 17 |
OK. Thanks.
|
|
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
small question about the functionalities of topological changes in OpenFoam | ngj | OpenFOAM Running, Solving & CFD | 2 | February 28, 2013 10:02 |
Question Re Engineering Data Source | imnull | ANSYS | 0 | March 5, 2012 13:51 |
internal field question - PitzDaily Case | atareen64 | OpenFOAM Running, Solving & CFD | 2 | January 26, 2011 15:26 |
In the header file of 'polyMesh' | sblee1977 | OpenFOAM | 1 | November 24, 2010 18:57 |
Poisson Solver question | Suresh | Main CFD Forum | 3 | August 12, 2005 04:37 |