View Issue Details
| ID | Project | Category | View Status | Date Submitted | Last Update |
|---|---|---|---|---|---|
| 0004252 | OpenFOAM | Bug | public | 2025-07-08 17:28 | 2025-07-11 16:58 |
| Reporter | otaolafr | Assigned To | will | ||
| Priority | normal | Severity | crash | Reproducibility | always |
| Status | closed | Resolution | no change required | ||
| Platform | linux | OS | ubutnu | OS Version | 24.02 |
| Product Version | 13 | ||||
| Summary | 0004252: crash with unexpected error when using mass transfer and population balance together | ||||
| Description | Hello, I am trying to migrate from my simulation in V12 to the newest V13. I am doing a multiphaseEuler simulation, a bubbleColumn with two phases: liquid containing H2O gas containing O2 and N2 and having mass transfer and population balance for the gas bubbles. with the migration to V13, i moved the massTransfer to fvModels, separated heatTransfer to a file and momentumTransfer to another. the simulation without population balance runs correctly but when I add it to the simulation I am getting this error: ``` populationBalance bubbles: Iteration 1 --> FOAM FATAL IO ERROR: Cannot find fieldSource entry for phaseChange file: unknown From function const Foam::GeometricFieldSources<Type, GeoMesh, PrimitiveField>::Source& Foam::GeometricFieldSources<Type, GeoMesh, PrimitiveField>::operator[](const Foam::word&) const [with Type = double; GeoMesh = Foam::volMesh; PrimitiveField = Foam::Field; Source = Foam::fvFieldSource<double>] in file /home/ubuntu/OpenFOAM/OpenFOAM-13/src/OpenFOAM/lnInclude/GeometricFieldSources.C at line 251. ``` I am adding the different dictionaries from the case (eventhought i based myself on the tutorials) | ||||
| Additional Information | without the population balance the case does not crash. | ||||
| Tags | No tags attached. | ||||
|
|
|
|
|
so the issue is coming from not having a source in the f files. I solved by adding a dummy source: ``` sources { phaseChange { type uniformFixedValue; uniformValue 0; } } ``` I might be wrong, but the source term for this files are only important for dissolving or evaporating, but when we want to transfer only species from one another of the phases it is not necessary. |
|
|
This is by design. The error message isn't terribly helpful at present because it seems to lose which file it refers to as it gets copied from the fDefault field to the numbered f fields. But the principle is correct. You have enabled mass transfer from the liquid to the gas (or vice versa). The gas has an f field, but the liquid doesn't. So, something needs to tell the code what value of f is to be created or destroyed in the gas. It can't work it out automatically, so if the user doesn't specify it is considered an error. In your case, setting zero isn't a good idea. Your mass transfer will be growing or shrinking the bubbles, or it might be nucleating new ones entirely. This source condition specifies which. So, you probably want either `interfacialGrowthSizeGroup` or `nucleationSizeGroup`. There are examples in the tutorials. |
| Date Modified | Username | Field | Change |
|---|---|---|---|
| 2025-07-08 17:28 | otaolafr | New Issue | |
| 2025-07-08 17:28 | otaolafr | File Added: example.tar.xz | |
| 2025-07-11 12:07 | otaolafr | Note Added: 0013601 | |
| 2025-07-11 16:54 | will | Assigned To | => will |
| 2025-07-11 16:54 | will | Status | new => closed |
| 2025-07-11 16:54 | will | Resolution | open => no change required |
| 2025-07-11 16:54 | will | Note Added: 0013614 | |
| 2025-07-11 16:58 | will | Relationship added | has duplicate 0004256 |
| 2025-07-11 16:58 | will | Note Edited: 0013614 |
