View Issue Details
| ID | Project | Category | View Status | Date Submitted | Last Update |
|---|---|---|---|---|---|
| 0001259 | OpenFOAM | Bug | public | 2014-04-04 14:02 | 2014-04-15 16:57 |
| Reporter | Assigned To | will | |||
| Priority | high | Severity | major | Reproducibility | always |
| Status | resolved | Resolution | fixed | ||
| Platform | Linux | OS | Debian | OS Version | 7 |
| Summary | 0001259: solver DPMFoam no dispersion model selectable | ||||
| Description | By setting up a case in the new particle-solver DPMFoam it is not possible to choose any dispersionModel (e.g. stochasticDispersionRAS) known from particle-solvers (e.g. icoUncoupledKinematicParcelFoam). The solver knows only the None-type dispersionModel. | ||||
| Steps To Reproduce | 1. Set up the tutorial-case /tutorials/lagrangian/DPMFoam/Goldschmidt 2. set the option "dispersionModel" to "stochasticDispersionRAS" the dict "submodels" of the files /constant/kinematicCloudProperties 3. in the file /constant/turbulenceProperties.air set the type to "RAS" and add the dict RAS { RASModel kEpsilon;//continuousGasKEpsilon; turbulence on; printCoeffs on; } 4. run the blockMesh-command and start the case with DPMFoam 5. The solver produces the output: "--> FOAM FATAL ERROR: Unknown dispersion model type stochasticDispersionRAS Valid dispersion model types are: 1(none) From function DispersionModel<CloudType>::New(const dictionary&, CloudType&) in file /OpenFOAM/OpenFOAM-2.3.x/src/lagrangian/intermediate/lnInclude/DispersionModelNew.C at line 54. FOAM exiting" | ||||
| Additional Information | Unfortunately the path for the dispersionModels has changed in OpenFOAM-2.3.x compared to OpenFOAM-2.2.x from src/lagrangian/intermediate/submodels/Kinematic/DispersionModel to src/lagrangian/turbulence/submodels/Kinematic/DispersionModel. In the former path just the None-type model exists, whereas in the latter path the known models are located. To solve that problem this path should be added to the Make/options in the DPMFoam solver. | ||||
| Tags | No tags attached. | ||||
|
|
Additionally I posted a similar problem on http://www.cfd-online.com/Forums/openfoam-solving/132594-how-use-mppicfoam-turbulence-effects-particle-motion.html The answer I got was mainly: 1) In "$FOAM_SRC/lagrangian/turbulence/submodels/Kinematic/DispersionModel/" are only templates. 2) It is in "$FOAM_SRC/lagrangian/turbulence/parcels/derived" that the dispersion models are created... or at least I think they are created there. 3) The turbulence models used by the solvers in question are actually created in the library "$FOAM_SOLVERS/lagrangian/DPMFoam/DPMTurbulenceModels". This is because these models are relying on the "Turbulence" template library. 4) Problem is that so is the library "$FOAM_SRC/lagrangian/turbulence" and that is why there is an object conflict when we load this library into memory for these solvers. --> From what I can figure out, the only way to have dispersion models in these solvers, is to somehow recreate these dispersion models directly in the "DPMTurbulenceModels" library. |
|
|
DPMFoam and MPPICFoam use the new turbulence structure (src/Turbulence) which takes the volume fraction of the phase into account. The dispersion models depend upon the old turbulence structure (src/turbulence), which is why thy are not available in these solvers. As a temporary fix to your problem, I've updated the dispersion models and put them into a new library, which is linked only by DPMFoam and MPPICFoam. The dispersion models should now be available in these solvers. The commit is 1115c18a8140c83894bcbf9d739dee0b7ac4feb5. |
