CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Running, Solving & CFD (http://www.cfd-online.com/Forums/openfoam-solving/)
-   -   Foam warnings - related to swak4Foam (http://www.cfd-online.com/Forums/openfoam-solving/126820-foam-warnings-related-swak4foam.html)

Salam-H November 26, 2013 15:59

Foam warnings - related to swak4Foam
 
5 Attachment(s)
Hi ever one. I am trying to run a case where all the files can be found in the following link
:https://www.hpc.ntnu.no/display/hpc/...Postprocessing
I followed every single steps as described. However, when I try to run blockMesh I get warnings , I have attached all the warning I get , the first document is the warning I get from running the blockMesh, the second is from setFields and the third is from decompose. After decomposing , I tried to run it in parallel but then I get errors which I have attached to this quote. I have also attached controlDict file where I have the libs and functions added to it.

Why I want to run this case? I have to model a case which is very similar to this one. I know how to model it and how to run it successfully but with out adding any thing to the controlDict file.. the only reason I want to model the case is to find out how alpha1 (Volume of Fluid ) decreases with time.

Attachment 27015

Attachment 27016

Attachment 27017

Attachment 27018

Attachment 27019

The link, has a graph in it, I have attached the graph to this quote as well. This is want I need to produce , but I cannot without your help. So please someone help me I really need to solve the problem and learn it. I do really appreciate your help a lot.

Best regards,

Salam

Salam-H November 26, 2013 16:05

1 Attachment(s)
Quote:

Originally Posted by Salam-H (Post 463629)
Hi ever one. I am trying to run a case where all the files can be found in the following link
:https://www.hpc.ntnu.no/display/hpc/...Postprocessing
I followed every single steps as described. However, when I try to run blockMesh I get warnings , I have attached all the warning I get , the first document is the warning I get from running the blockMesh, the second is from setFields and the third is from decompose. After decomposing , I tried to run it in parallel but then I get errors which I have attached to this quote. I have also attached controlDict file where I have the libs and functions added to it.

Why I want to run this case? I have to model a case which is very similar to this one. I know how to model it and how to run it successfully but with out adding any thing to the controlDict file.. the only reason I want to model the case is to find out how alpha1 (Volume of Fluid ) decreases with time.

Attachment 27015

Attachment 27016

Attachment 27017

Attachment 27018

Attachment 27019

The link, has a graph in it, I have attached the graph to this quote as well. This is want I need to produce , but I cannot without your help. So please someone help me I really need to solve the problem and learn it. I do really appreciate your help a lot.

Best regards,

Salam

The graph that I need to produce is :

Salam-H November 29, 2013 08:26

Swak4Foam
 
2 Attachment(s)
Hi people. I hope I get some help here.

I have added the following lines to my controlDict file, Please can you have a look at the attachments :
Code:

libs (
          "libOpenFOAM.so"
          "libsimpleSwakFunctionObjects.so"
          "libswakFunctionObjects.so"
      );

functions
{
    #include "sampledSets"
    #include "sampledSurf"
}

And when I run blockMesh I get the following warning :

Code:

Create time 
 

 --> FOAM Warning : 
    From function dlOpen(const fileName&, const bool) 
    in file POSIX.C at line 1179 
    dlopen error : libsimpleSwakFunctionObjects.so: cannot open shared object file: No such file or directory 
 --> FOAM Warning : 
    From function dlLibraryTable::open(const fileName&, const bool) 
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 99 
    could not load "libsimpleSwakFunctionObjects.so" 
 --> FOAM Warning : 
    From function dlOpen(const fileName&, const bool) 
    in file POSIX.C at line 1179 
    dlopen error : libswakFunctionObjects.so: cannot open shared object file: No such file or directory 
 --> FOAM Warning : 
    From function dlLibraryTable::open(const fileName&, const bool) 
    in file db/dynamicLibrary/dlLibraryTable/dlLibraryTable.C at line 99 
    could not load "libswakFunctionObjects.so" 
 Creating block mesh from 
    "/home/salam/OpenFOAM/salam-2.2.x/run/tutorials/multiphase/interFoam/laminar/beerBottle/constant/polyMesh/blockMeshDict"
 Creating curved edges 
 Creating topology blocks 
 Creating topology patches 
 

 Creating block mesh topology 
 --> FOAM Warning : 
    From function polyMesh::polyMesh(... construct from shapes...) 
    in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 901 
    Found 2 undefined faces in mesh; adding to default patch. 
 

 Check topology 
 

    Basic statistics 
        Number of internal faces : 0 
        Number of boundary faces : 6 
        Number of defined boundary faces : 6 
        Number of undefined boundary faces : 0 
    Checking patch -> block consistency
 

 Creating block offsets 
 Creating merge list . 
 

 Creating polyMesh from blockMesh 
 Creating patches 
 Creating cells 
 Creating points with scale 1 
 

 Writing polyMesh 
 ---------------- 
 Mesh Information 
 ---------------- 
  boundingBox: (-0.04 -0.005 0) (0.04 0.005 0.16) 
  nPoints: 90522 
  nCells: 44800 
  nFaces: 179660 
  nInternalFaces: 89140 
 ---------------- 
 Patches 
 ---------------- 
  patch 0 (start: 89140 size: 140) name: inletOutlet 
  patch 1 (start: 89280 size: 780) name: walls 
  patch 2 (start: 90060 size: 89600) name: defaultFaces 
 

 End 
 

 salam@salam:~/OpenFOAM/salam-2.2.x/run/tutorials/multiphase/interFoam/laminar/beerBottle$

Thanks for your help in advance.

wyldckat November 29, 2013 18:14

Hi Salam,

In reference to you posts on this thread: http://www.cfd-online.com/Forums/ope...trol-dict.html - we can gather a full picture of the problem.

The main issue is whether swak4Foam is properly installed or not. From what I can see, you're using OpenFOAM 2.2.2. Here are the steps I suggest that you follow:
  1. If I'm guessing correctly, you probably have installed the Deb package of OpenFOAM 2.2.2 for Ubuntu. This means that you might be missing some essential build tools, so I suggest that you make sure they are installed, by running:
    Code:

    sudo apt-get install build-essential flex bison zlib1g-dev libreadline-dev libncurses-dev
  2. Next, let's get into a good work folder and download (git clone and checkout) the version of swak4Foam that I know for certain that will build with success:
    Code:

    mkdir -p $FOAM_RUN
    cd $FOAM_RUN
    cd ..
    git clone https://github.com/wyldckat/swak4foam.git
    cd swak4foam
    git checkout OF22X

  3. Now build swak4Foam, by running:
    Code:

    ./Allwmake > make.log 2>&1
    It will take a while to build everything. All of the usual output will be written into the file "make.log".
  4. Now run the same command again:
    Code:

    ./Allwmake > make.log 2>&1
    This will make a summary of whether all of the libraries and utilities were built properly. Once it's done, check the contents written into the file "make.log", which should look something like this:
    Code:

    No 'swakConfiguration'. Python etc won't work
    Checking swak4Foam-version and generating file
    abort: no repository found in '/home/ofuser/OpenFOAM/ofuser-2.2.2/swak4foam' (.hg not found)!
    Swak version is 0.2.4
    Bison is version 2.5
    Flex is version 2.5.35 (Minor version: 35)
    OpenFOAM-version: Major 2 Minor 2 Patch 2 (-1 == x)
    No change to swak4FoamParsers/foamVersion4swak.H
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswak4FoamParsers.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libgroovyBC.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakFunctionObjects.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libsimpleFunctionObjects.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libsimpleLagrangianFunctionObjects.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libsimpleSearchableSurfaces.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libsimpleSwakFunctionObjects.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakTopoSources.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakSourceFields.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libgroovyStandardBCs.so' is up to date.
    SWAK_PYTHON_INCLUDE not defined .... no Python-Integration
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakMeshQualityFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakLocalCalculationsFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakRandomFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakFvcSchemesFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakThermoTurbFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakTransportTurbFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakSurfacesAndSetsFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakLagrangianCloudSourcesFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakVelocityFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakChemistryModelFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakRadiationModelFunctionPlugin.so' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/replayTransientBC' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/calcNonUniformOffsetsForMapped' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/funkyDoCalc' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/funkySetFields' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/funkySetBoundaryField' is up to date.


    If you want to use swakCoded-function object or compile software based on swak set the environment variable SWAK4FOAM_SRC to /home/ofuser/OpenFOAM/ofuser-2.2.2/swak4foam/Libraries (most people will be fine without setting that variable)

  5. If the content of the "make.log" file is substantially different from the one above, please search and replace any sensitive information, zip the file and attach it to your next post.


Now comes the part regarding the aforementioned case, available at the end of this page: https://www.hpc.ntnu.no/display/hpc/...Postprocessing
I ran the following commands to download and unpack the package:
Code:

cd $FOAM_RUN
wget "https://www.hpc.ntnu.no/download/attachments/4587593/beerBottle.tar.gz?version=1&modificationDate=1344854891000&api=v2" -O beerBottle.tar.gz
tar -xzf beerBottle.tar.gz

To run the case, I did these commands:
Code:

cd beerBottle
./Allrun

There seems to be several outdated definitions:
  • Edit the file "fillLevel.plot" and change these lines:
    Code:

    plot 'volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid', \
        'swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'

    To this:
    Code:

    plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid', \
        'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'

  • Get a fresh copy of the fvSchemes file from the original tutorial:
    Code:

    cp $FOAM_TUTORIALS/multiphase/interFoam/laminar/damBreak/system/fvSchemes system/fvSchemes
Now, to run the case again, do it like this:
Code:

./Allclean
./Allrun

And I think that solves all of the reported problems!

Best regards,
Bruno

Salam-H November 29, 2013 18:20

Quote:

Originally Posted by wyldckat (Post 464095)
Hi Salam,

In reference to you posts on this thread: http://www.cfd-online.com/Forums/ope...trol-dict.html - we can gather a full picture of the problem.

The main issue is whether swak4Foam is properly installed or not. From what I can see, you're using OpenFOAM 2.2.2. Here are the steps I suggest that you follow:
  1. If I'm guessing correctly, you probably have installed the Deb package of OpenFOAM 2.2.2 for Ubuntu. This means that you might be missing some essential build tools, so I suggest that you make sure they are installed, by running:
    Code:

    sudo apt-get install build-essential flex bison zlib1g-dev libreadline-dev libncurses-dev
  2. Next, let's get into a good work folder and download (git clone and checkout) the version of swak4Foam that I know for certain that will build with success:
    Code:

    mkdir -p $FOAM_RUN
    cd $FOAM_RUN
    cd ..
    git clone https://github.com/wyldckat/swak4foam.git
    cd swak4foam
    git checkout OF22X

  3. Now build swak4Foam, by running:
    Code:

    ./Allwmake > make.log 2>&1
    It will take a while to build everything. All of the usual output will be written into the file "make.log".
  4. Now run the same command again:
    Code:

    ./Allwmake > make.log 2>&1
    This will make a summary of whether all of the libraries and utilities were built properly. Once it's done, check the contents written into the file "make.log", which should look something like this:
    Code:

    No 'swakConfiguration'. Python etc won't work
    Checking swak4Foam-version and generating file
    abort: no repository found in '/home/ofuser/OpenFOAM/ofuser-2.2.2/swak4foam' (.hg not found)!
    Swak version is 0.2.4
    Bison is version 2.5
    Flex is version 2.5.35 (Minor version: 35)
    OpenFOAM-version: Major 2 Minor 2 Patch 2 (-1 == x)
    No change to swak4FoamParsers/foamVersion4swak.H
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswak4FoamParsers.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libgroovyBC.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakFunctionObjects.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libsimpleFunctionObjects.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libsimpleLagrangianFunctionObjects.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libsimpleSearchableSurfaces.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libsimpleSwakFunctionObjects.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakTopoSources.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakSourceFields.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libgroovyStandardBCs.so' is up to date.
    SWAK_PYTHON_INCLUDE not defined .... no Python-Integration
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakMeshQualityFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakLocalCalculationsFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakRandomFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakFvcSchemesFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakThermoTurbFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakTransportTurbFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakSurfacesAndSetsFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakLagrangianCloudSourcesFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakVelocityFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakChemistryModelFunctionPlugin.so' is up to date.
    '/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/lib/libswakRadiationModelFunctionPlugin.so' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/replayTransientBC' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/calcNonUniformOffsetsForMapped' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/funkyDoCalc' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/funkySetFields' is up to date.
    make[1]: `/home/ofuser/OpenFOAM/ofuser-2.2.2/platforms/linux64GccDPOpt/bin/funkySetBoundaryField' is up to date.


    If you want to use swakCoded-function object or compile software based on swak set the environment variable SWAK4FOAM_SRC to /home/ofuser/OpenFOAM/ofuser-2.2.2/swak4foam/Libraries (most people will be fine without setting that variable)

  5. If the content of the "make.log" file is substantially different from the one above, please search and replace any sensitive information, zip the file and attach it to your next post.


Now comes the part regarding the aforementioned case, available at the end of this page: https://www.hpc.ntnu.no/display/hpc/...Postprocessing
I ran the following commands to download and unpack the package:
Code:

cd $FOAM_RUN
wget "https://www.hpc.ntnu.no/download/attachments/4587593/beerBottle.tar.gz?version=1&modificationDate=1344854891000&api=v2" -O beerBottle.tar.gz
tar -xzf beerBottle.tar.gz

To run the case, I did these commands:
Code:

cd beerBottle
./Allrun

There seems to be several outdated definitions:
  • Edit the file "fillLevel.plot" and change these lines:
    Code:

    plot 'volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid', \
        'swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'

    To this:
    Code:

    plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid', \
        'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'

  • Get a fresh copy of the fvSchemes file from the original tutorial:
    Code:

    cp $FOAM_TUTORIALS/multiphase/interFoam/laminar/damBreak/system/fvSchemes system/fvSchemes
Now, to run the case again, do it like this:
Code:

./Allclean
./Allrun

And I think that solves all of the reported problems!

Best regards,
Bruno

Dear Bruno,

Thank you very much for all of the help and effort, I have no words strong enough to express how thankful I am for your help. I will follow the steps, and hopefully it works. Thank you again.

Salam-H November 29, 2013 19:19

Quote:

Originally Posted by Salam-H (Post 464096)
Dear Bruno,

Thank you very much for all of the help and effort, I have no words strong enough to express how thankful I am for your help. I will follow the steps, and hopefully it works. Thank you again.

I can't believe it !! wow , it is running now, can't wait to see the graphs . I feel like I am on the moon. Thank you so much, if there is any thing that I could do for you in return please let me know.

Do you think that I can find someone as good as yourself to teach me how to learn OpenFOAM ? Of course not for free.

Best regards

Salam

wyldckat November 30, 2013 06:21

Hi Salam,

Check the links at http://openfoamwiki.net/index.php/Main_Page - section "3.1 Training".

Best regards,
Bruno

Salam-H November 30, 2013 06:30

1 Attachment(s)
Quote:

Originally Posted by wyldckat (Post 464127)
Hi Salam,

Check the links at http://openfoamwiki.net/index.php/Main_Page - section "3.1 Training".

Best regards,
Bruno

Hi Bruno,

Thanks for the reply, I will check the website . About the above case, I could run it successfully , but when I tried to do the graph I got the following message and never got the graph. Can I ask for some help with this please?

Code:

salam@salam:~$ cd OpenFOAM/salam-2.2.2/run/beerBottle/
salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$ plot  'volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title  'Volume of liquid', \
>      'swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'
plot: volumeIntegrate_totalLiquid/0/alpha1: No such file or directory
plot: ignoring this file
plot: axes: No such file or directory
plot: ignoring this file
plot: x1y1: No such file or directory
plot: ignoring this file
plot: with: No such file or directory
plot: ignoring this file
plot: lines: No such file or directory
plot: ignoring this file
plot: title: No such file or directory
plot: ignoring this file
plot: Volume of liquid,: No such file or directory
plot: ignoring this file
plot: swakExpression_volFlow/0/volFlow: No such file or directory
plot: ignoring this file
plot: axes: No such file or directory
plot: ignoring this file
plot: x1y2: No such file or directory
plot: ignoring this file
plot: with: No such file or directory
plot: ignoring this file
plot: lines: No such file or directory
plot: ignoring this file
plot: title: No such file or directory
plot: ignoring this file
plot: Flow rate: No such file or directory
plot: ignoring this file
salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$

Best regards,

Salam

wyldckat November 30, 2013 06:34

Quote:

Originally Posted by wyldckat (Post 464095)
There seems to be several outdated definitions:
  • Edit the file "fillLevel.plot" and change these lines:
    Code:

    plot 'volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid', \
        'swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'

    To this:
    Code:

    plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid', \
        'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'


If you notice, when I wrote the instructions above, I added before the path to each file the path "postProcessing/".

In addition, if you run the script "fillLevel.plot":
Code:

./fillLevel.plot
It will runs the plot commands.

Salam-H November 30, 2013 06:49

Quote:

Originally Posted by wyldckat (Post 464129)
If you notice, when I wrote the instructions above, I added before the path to each file the path "postProcessing/".

In addition, if you run the script "fillLevel.plot":
Code:

./fillLevel.plot
It will runs the plot commands.

Hi again,

I did the change to the line, and I got a fresh copy of fvScheme manually. When I run allclean it goes through, but when I run allrun I get this :

Code:

salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$ ./Allclean
Cleaning /home/salam/OpenFOAM/salam-2.2.2/run/beerBottle case
Clearing ./constant/polyMesh
salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$ ./Allrun
./Allrun: ./meshgen.m: /usr/bin/octave: bad interpreter: No such file or directory

plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1  with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines  title 'Flow rate'
                                                                                      ^
"./fillLevel.plot", line 15: warning: Skipping data file with no valid points

plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1  with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines  title 'Flow rate'
                                                                                                                                                                                              ^
"./fillLevel.plot", line 15: warning: Skipping data file with no valid points

plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1  with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines  title 'Flow rate'
                                                                                                                                                                                                        ^
"./fillLevel.plot", line 15: x range is invalid

salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$ ./Allclean
Cleaning /home/salam/OpenFOAM/salam-2.2.2/run/beerBottle case
Clearing ./constant/polyMesh
salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$ ./Allrun
./Allrun: ./meshgen.m: /usr/bin/octave: bad interpreter: No such file or directory

plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1  with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines  title 'Flow rate'
                                                                                      ^
"./fillLevel.plot", line 16: warning: Skipping data file with no valid points

plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1  with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines  title 'Flow rate'
                                                                                                                                                                                              ^
"./fillLevel.plot", line 16: warning: Skipping data file with no valid points

plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1  with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines  title 'Flow rate'
                                                                                                                                                                                                        ^
"./fillLevel.plot", line 16: x range is invalid

salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$

Thank you.

Salam

wyldckat November 30, 2013 06:53

Hi Salam,

Please follow the instructions from the second link on my signature, for posting code and terminal output. And, please, also edit your previous posts as well, to wrap the outputs into the "[CODE]" markers.

As for the error at the beginning of Allrun, that's because Octave is not installed. If you are using Ubuntu, run:
Code:

sudo apt-get install octave
Best regards,
Bruno

Salam-H November 30, 2013 07:21

Quote:

Originally Posted by wyldckat (Post 464132)
Hi Salam,

Please follow the instructions from the second link on my signature, for posting code and terminal output. And, please, also edit your previous posts as well, to wrap the outputs into the "[CODE]" markers.

As for the error at the beginning of Allrun, that's because Octave is not installed. If you are using Ubuntu, run:
Code:

sudo apt-get install octave
Best regards,
Bruno

Hi Bruno,

Thank you for the reply, I will do as you said. I have installed octave, but I still get the following warning:

Code:

salam@salam:~$ cd OpenFOAM/salam-2.2.2/run/beerBottle/
salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$ ./Allclean
Cleaning /home/salam/OpenFOAM/salam-2.2.2/run/beerBottle case
Clearing ./constant/polyMesh
salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$ ./Allrun


plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'
                                                                                      ^
"./fillLevel.plot", line 16: warning: Skipping data file with no valid points

plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'
                                                                                                                                                                                            ^
"./fillLevel.plot", line 16: warning: Skipping data file with no valid points

plot 'postProcessing/volumeIntegrate_totalLiquid/0/alpha1' axes x1y1 with lines title 'Volume of liquid',      'postProcessing/swakExpression_volFlow/0/volFlow' axes x1y2 with lines title 'Flow rate'
                                                                                                                                                                                                      ^
"./fillLevel.plot", line 16: x range is invalid

salam@salam:~/OpenFOAM/salam-2.2.2/run/beerBottle$ ./fillLevel.plot

I have booked a traing course in London.

Regards,

Salam

wyldckat November 30, 2013 08:04

Hi Salam,

Check the contents of the files located in the folder "output". They should give a clear idea of what happened.

Best regards,
Bruno

Salam-H December 1, 2013 13:52

Hi Bruno,

Thanks a lot for your valuebale comments.

I did run my case. At the final step , where I to run ./Allrun , I get the following error message, do you have any ideas on how to solve this please?

Code:

salam@salam:~/OpenFOAM/salam-2.2.2/run/mycase$ paraFoam
created temporary 'mycase.OpenFOAM'
salam@salam:~/OpenFOAM/salam-2.2.2/run/mycase$ ./Allclean
Cleaning /home/salam/OpenFOAM/salam-2.2.2/run/mycase case
Clearing ./constant/polyMesh
salam@salam:~/OpenFOAM/salam-2.2.2/run/mycase$ ./Allrun
"./fillLevel.plot", line 15: warning: Skipping unreadable file "postProcessing/volumeIntegrate_totalLiquid/0/alpha1"
"./fillLevel.plot", line 15: warning: Skipping unreadable file "postProcessing/swakExpression_volFlow/0/volFlow"
"./fillLevel.plot", line 15: No data in plot

Best regards,

Salam

wyldckat December 1, 2013 14:06

Hi Salam,

Once again, you need to check the contents of the files located in the folder "output", because they can give a better idea as to what went wrong.

You should also check the contents of the folder "postProcessing", since the Allrun script is indicating that the aforementioned files were not accessible.

Best regards,
Bruno

Salam-H December 1, 2013 14:52

Hi Bruno,

I am terribly sorry for bothering, but your help means a lot to me. I did check the output folder, and I found error messages there . One of the errors is due to polyMesh , I don't know why there should be any errors. The error is :

Code:

/*---------------------------------------------------------------------------*\
| =========                |                                                |
| \\      /  F ield        | OpenFOAM: The Open Source CFD Toolbox          |
|  \\    /  O peration    | Version:  2.2.2                                |
|  \\  /    A nd          | Web:      www.OpenFOAM.org                      |
|    \\/    M anipulation  |                                                |
\*---------------------------------------------------------------------------*/
Build  : 2.2.2-9240f8b967db
Exec  : setFields
Date  : Dec 01 2013
Time  : 19:43:53
Host  : "salam"
PID    : 4720
Case  : /home/salam/OpenFOAM/salam-2.2.2/run/mycase
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Disallowing user-supplied system call operations

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
Create time

Create mesh for time = 0



--> FOAM FATAL ERROR:
Cannot find file "points" in directory "polyMesh" in times 0 down to constant

    From function Time::findInstance(const fileName&, const word&, const IOobject::readOption, const word&)
    in file db/Time/findInstance.C at line 203.

FOAM exiting

I have more error files , but I believe if this error gets fixed the rest will be fixed along with it.

Best regards,

Salam

wyldckat December 1, 2013 14:57

Hi Salam,

You need to check the output files by the order they are created, according to the script file Allrun.
The very first output file is the one to check, namely "output/1-blockMesh.log". If it shows you an error message, then that's the one that needs to be fixed first.

Best regards,
Bruno

Salam-H December 1, 2013 15:17

Quote:

Originally Posted by wyldckat (Post 464275)
Hi Salam,

You need to check the output files by the order they are created, according to the script file Allrun.
The very first output file is the one to check, namely "output/1-blockMesh.log". If it shows you an error message, then that's the one that needs to be fixed first.

Best regards,
Bruno

Hi Bruno,

Thank you so much for your help. I would never be able to solve this without your help. I think the problem is fixed now, and I get the graphs . Thank you again.

Best regards,

Salam

Salam-H December 2, 2013 19:48

Hi Bruno,

I hope you are doing well. I am sorry for taking your time again. I did run my case, and in the output folder, I always get the following warning in the interFoam.log file, but the simulation still goes through:
can you help me to fix it please? .

Code:

    'outputInterval' not found in totalLiquid
Assuming: 1
--> FOAM Warning :
    From function simpleFunctionObject::simpleFunctionObject
    in file simpleFunctionObject/simpleFunctionObject.C at line 108
    'outputControlMode' not found in volFlow
Assuming: timestep
--> FOAM Warning :
    From function simpleFunctionObject::simpleFunctionObject
    in file simpleFunctionObject/simpleFunctionObject.C at line 116
    'outputInterval' not found in volFlow
Assuming: 1
swak4Foam: Setting default mesh
surfaces cuttingPlane: Reading surface description:
    neckCut
    freeSurface

Courant Number mean: 0 max: 0
Interface Courant Number mean: 0 max: 0
deltaT = 0.00119048
Time = 0.00119048

The graph that I get for Alpha1 (Volume of fluid) against Time (from controlDict ) , End time. Is the EndTime represents the actual real life time? If it is not a real life time, then how can I find the real life time? If it is a real life time then:

Why when I go for finer mesh , the volume of fluid (Alpha1) runs slower , I mean lesser fluid leaves the domain with finer mesh (even though I don't change the EndTime), can you please kindly explain this to me?

I would be grateful for your help. I know you have already helped me more than enough , I really appreciate it.

Best regards,

Salam

gschaider December 3, 2013 06:37

Quote:

Originally Posted by Salam-H (Post 464496)
Hi Bruno,

I hope you are doing well. I am sorry for taking your time again. I did run my case, and in the output folder, I always get the following warning in the interFoam.log file, but the simulation still goes through:
can you help me to fix it please? .

Code:

    'outputInterval' not found in totalLiquid
Assuming: 1
--> FOAM Warning :
    From function simpleFunctionObject::simpleFunctionObject
    in file simpleFunctionObject/simpleFunctionObject.C at line 108
    'outputControlMode' not found in volFlow
Assuming: timestep
--> FOAM Warning :
    From function simpleFunctionObject::simpleFunctionObject
    in file simpleFunctionObject/simpleFunctionObject.C at line 116
    'outputInterval' not found in volFlow
Assuming: 1
swak4Foam: Setting default mesh
surfaces cuttingPlane: Reading surface description:
    neckCut
    freeSurface

Courant Number mean: 0 max: 0
Interface Courant Number mean: 0 max: 0
deltaT = 0.00119048
Time = 0.00119048


I think the warnings are pretty clear: you have not set outputInterval. But instead of failing swak makes an assumption for you. Either set the described parameters to the values that swak reports (then everything will behave the way it did before. Just without warnings) or set them to different values (for instance to report less frequently)


All times are GMT -4. The time now is 14:43.