CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Running, Solving & CFD

Phasechangemodel -liquidEvapFuchsKnudsenCoeffs

Register Blogs Community New Posts Updated Threads Search

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   May 2, 2024, 03:32
Default Phasechangemodel -liquidEvapFuchsKnudsenCoeffs
  #1
New Member
 
harshavardhan
Join Date: Nov 2017
Posts: 24
Rep Power: 8
harsha002 is on a distinguished road
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]
harsha002 is offline   Reply With Quote

Old   May 3, 2024, 03:04
Default
  #2
Senior Member
 
Tom Fahner
Join Date: Mar 2009
Location: Breda, Netherlands
Posts: 646
Rep Power: 32
tomf will become famous soon enoughtomf will become famous soon enough
Send a message via MSN to tomf Send a message via Skype™ to tomf
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.
basically tells you that OpenFOAM expects something in the subModels part of your file constant/sprayProperties and that this should be between lines 56 and 180 of that file, which I am guessing are the lines with { and } for the subModels subDict in that file.

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")),
and further down:

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);
        }
I have no idea what these entries would mean, or what the values should be for the model, I will leave that up to you. My expectation would be that you need something like this in the subModels part in constant/cloudProperties:

Code:
    liquidEvapFuchsKnudsenCoeffs
    {
        activityCoefficient Hoff; // or UNIFAC
        gamma 2.5; 
        alpham 0.5;
        solution (liquid solid);
    }
The solution entry is based on this part of the code:

Code:
    if (solution_.size() > 2)
    {
        FatalErrorInFunction
            << "Solution is not well defined. It should be (liquid solid)"
            << nl <<  exit(FatalError);
    }
Again, I have no clue what this model does or defines exactly, just reading code and translating into instructions. So please do not just copy these values blindly, I just expect that this is the required format.

Hope this helps,
Tom
tomf is offline   Reply With Quote

Old   May 8, 2024, 22:42
Default
  #3
New Member
 
harshavardhan
Join Date: Nov 2017
Posts: 24
Rep Power: 8
harsha002 is on a distinguished road
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.
harsha002 is offline   Reply With Quote

Reply

Tags
openfoam 1.5-dev, openfoam solver


Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


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


All times are GMT -4. The time now is 04:23.