|
[Sponsors] |
Phasechangemodel -liquidEvapFuchsKnudsenCoeffs |
|
LinkBack | Thread Tools | Search this Thread | Display Modes |
May 2, 2024, 03:32 |
Phasechangemodel -liquidEvapFuchsKnudsenCoeffs
|
#1 |
New Member
harshavardhan
Join Date: Nov 2017
Posts: 24
Rep Power: 9 |
Hello everyone,
I am running an spray injection simulation in openfoam v2312. The solver I am using is sprayfoam. For the Lagrangian phase change model I want to implement liquidevapfuchsknudsencoeff. But unfortunately I could find the co-efficient available for this model. below is the error it throws when I run my simulation. --> FOAM FATAL IO ERROR: (openfoam-2312) [4] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "stream/subModels" [4] [4] [4] file: stream/subModels at line 0. [4] [4] From [0] [0] [0] --> FOAM FATAL IO ERROR: (openfoam-2312) [0] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "constant/sprayCloudProperties/subModels" [0] [0] [0] file: constant/sprayCloudProperties/subModels at line 56 to 180. [0] [0] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType:ption) const [0] in file db/dictionary/dictionary.C at line 457. const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType:ption) const [4] in file db/dictionary/dictionary.C at line 457. [4] FOAM parallel run exiting [4] [2] [2] [2] --> FOAM FATAL IO ERROR: (openfoam-2312) [2] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "stream/subModels" [2] [2] [2] [0] FOAM parallel run exiting [0] file: stream/subModels at line 0. [2] [2] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType:ption) const [2] in file db/dictionary/dictionary.C at line 457. [2] FOAM parallel run exiting [2] [5] [7] [7] [7] --> FOAM FATAL IO ERROR: (openfoam-[5] [5] --> FOAM FATAL IO ERROR: (openfoam-2312) [5] 2312) [7] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "stream/subModels" [7] [7] [7] [3] [3] file: stream/subModels at line 0. [7] [6] [6] [6] --> FOAM FATAL IO ERROR: Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "stream/subModels" [5] [5] [5] file: stream/subModels at line 0. [5] [5] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType:ption) const[3] --> FOAM FATAL IO ERROR: (openfoam-2312) [3] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "stream/subModels" [3] [3] [3] file: [7] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType:ption) const [7] in file db/dictionary/dictionary.C at line 457. [7] FOAM parallel run exiting [7] (openfoam-2312) [6] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "stream/subModels" [6] [6] [6] file: stream/subModels at line 0.stream/subModels at line 0. [3] [3] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType:ption) const [3] in file db/dictionary/dictionary.C at line 457. [5] in file db/dictionary/dictionary.C at line 457. [5] FOAM parallel run exiting [5] [6] [6] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType:ption) const [6] in file db/dictionary/dictionary.C at line 457. [6] FOAM parallel run exiting [6] [3] FOAM parallel run exiting [3] [1] [1] [1] --> FOAM FATAL IO ERROR: (openfoam-2312) [1] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "stream/subModels" [1] [1] [1] file: stream/subModels at line 0. [1] [1] From const Foam::dictionary& Foam::dictionary::subDict(const Foam::word&, Foam::keyType:ption) const [1] in file db/dictionary/dictionary.C at line 457. [1] FOAM parallel run exiting [1] |
|
May 3, 2024, 03:04 |
|
#2 |
Senior Member
|
Hi,
There are several ways to find out what is necessary to be filled in. The error here: Code:
[4] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "stream/subModels" [4] [4] [4] file: stream/subModels at line 0. [4] [4] From [0] [0] [0] --> FOAM FATAL IO ERROR: (openfoam-2312) [0] Entry 'liquidEvapFuchsKnudsenCoeffs' not found in dictionary "constant/sprayCloudProperties/subModels" [0] [0] [0] file: constant/sprayCloudProperties/subModels at line 56 to 180. Then what it expects to be found there can be gathered from the source code. If you read there, some entries are there that lookup something from the coeffDict, in this case it looks for: Code:
gamma_(this->coeffDict().getScalar("gamma")), alpha_(this->coeffDict().getScalar("alpham")), solution_(this->coeffDict().lookup("solution")), Code:
const word activityCoefficienType ( this->coeffDict().getWord("activityCoefficient") ); if (activityCoefficienType == "Hoff") { method_ = pHoff; } else if (activityCoefficienType == "UNIFAC") { method_ = pUNIFAC; } else { FatalErrorInFunction << "activityCoefficient must be either 'Hoff' or 'UNIFAC'" << nl << exit(FatalError); } Code:
liquidEvapFuchsKnudsenCoeffs { activityCoefficient Hoff; // or UNIFAC gamma 2.5; alpham 0.5; solution (liquid solid); } Code:
if (solution_.size() > 2) { FatalErrorInFunction << "Solution is not well defined. It should be (liquid solid)" << nl << exit(FatalError); } Hope this helps, Tom |
|
May 8, 2024, 22:42 |
|
#3 |
New Member
harshavardhan
Join Date: Nov 2017
Posts: 24
Rep Power: 9 |
HI Tom,
Thank you for your reply. I fixed the issues, and I am able to run the simulation now. I downloaded an tutorial problem and added the missing the lines and files to make it run without any issues. thanks once again. |
|
Tags |
openfoam 1.5-dev, openfoam solver |
|
|
Similar Threads | ||||
Thread | Thread Starter | Forum | Replies | Last Post |
Custom Lagrangian Phase Change Model | craven.brent | OpenFOAM Programming & Development | 4 | December 25, 2022 20:22 |
Add new PhaseChangeModel in OpenFOAM 2.2.0 | ray | OpenFOAM Programming & Development | 0 | June 1, 2013 06:22 |