CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM Pre-Processing

Problem with fluentDataToFoam (from OF 1.6 ex) in OF 2.1.1

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree8Likes

Reply
 
LinkBack Thread Tools Display Modes
Old   March 10, 2013, 08:35
Default Problem with fluentDataToFoam (from OF 1.6 ex) in OF 2.1.1
  #1
DDB
New Member
 
DDB
Join Date: Jan 2013
Posts: 12
Rep Power: 5
DDB is on a distinguished road
Hi all,

I followed the instructions in this thread to overcome the compilation problems
can not complie fluentDataToFoam in OF2.1.1

I have already generated the OF mesh using fluent3DMeshToFoam. However, when I run fluentDataToFoam I get the error:

Code:
--> FOAM FATAL IO ERROR: 
cannot find file

file: /home/.../constant/polyMesh/zoneToPatchName at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 73.

FOAM exiting
There is no file called zoneToPatchName in my polyMesh folder. Is this due to a change in fluent3DMeshToFoam since v1.6 or is it a problem with fluentDataToFoam?

Any help gratefully received!
DDB is offline   Reply With Quote

Old   March 10, 2013, 08:39
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,556
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi DDB,

Can you create a simple test case and share it so that I (or anyone else) can try to replicate the same error!?

Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   March 10, 2013, 10:02
Default
  #3
DDB
New Member
 
DDB
Join Date: Jan 2013
Posts: 12
Rep Power: 5
DDB is on a distinguished road
I'd love to, but I don't have access to fluent anymore :-(

I did some cases at uni a few years ago & now I want to work on them in OF, but I am not at uni now and I certainly cannot afford the fluent fees!
DDB is offline   Reply With Quote

Old   March 10, 2013, 11:42
Default
  #4
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,556
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi DDB,

Very well, then lets reverse engineer this thing.

First I'm going to use the tutorial "incompressible/icoFoam/cavity" as basis for creating the simple Fluent dataset:
  1. Run the tutorial:
    Code:
    blockMesh
    icoFoam
  2. Then extract the components for U:
    Code:
    foamCalc components U
Now to convert the mesh and data to Fluent format:
  1. Create the file "system/foamDataToFluentDict" with the following contents:
    Code:
    /*--------------------------------*- C++ -*----------------------------------*\
    | =========                 |                                                 |
    | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
    |  \\    /   O peration     | Version:  2.1.x                                 |
    |   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
    |    \\/     M anipulation  |                                                 |
    \*---------------------------------------------------------------------------*/
    FoamFile
    {
        version     2.0;
        format      ascii;
        class       dictionary;
        location    "system";
        object      foamDataToFluentDict;
    }
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
    
    p 1;
    
    Ux 111;
    Uy 112;
    Uz 113;
    I know the codes, because I looked at the fluentDataToFoam source code, more specifically inside the file "fluentDataToFoam.L".
  2. Converted the OpenFOAM mesh and data to Fluent format:
    Code:
    foamMeshToFluent
    foamDataToFluent


Now for converting stuff back from Fluent to OpenFOAM:
  1. Convert the mesh by running:
    Code:
    fluentMeshToFoam fluentInterface/cavity.msh
    This is only because this is the simple cavity. fluent3DMeshToFoam should be used for more complicated cases.
  2. Then look into the file "fluentInterface/cavity.msh" and find the codes for each patch. At the end of the file you should find this:
    Code:
    (39 (1 fluid fluid-1)())
    (39 (2 interior interior-1)())
    (39 (10 wall movingWall)())
    (39 (11 wall fixedWalls)())
    (39 (12 pressure-outlet frontAndBack)())
    This is what we'll use as reference for the "zoneToPatchName" file.
  3. Create the file "constant/polyMesh/zoneToPatchName" with the following contents:
    Code:
    /*--------------------------------*- C++ -*----------------------------------*\
    | =========                 |                                                 |
    | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
    |  \\    /   O peration     | Version:  2.1.x                                 |
    |   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
    |    \\/     M anipulation  |                                                 |
    \*---------------------------------------------------------------------------*/
    FoamFile
    {
        version     2.0;
        format      ascii;
        class       wordList;
        location    "constant/polyMesh";
        object      zoneToPatchName;
    }
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
    
    /*
    (39 (1 fluid fluid-1)())
    (39 (2 interior interior-1)())
    (39 (10 wall movingWall)())
    (39 (11 wall fixedWalls)())
    (39 (12 pressure-outlet frontAndBack)())
    */
    
    13
    (
      dummy    //foam 0 - no fluent correspondence
      unknown  //foam 1 - fluent 1
      interior //foam 2 - fluent 2
      dummy    //foam 3 - fluent 3
      dummy    //foam 4 - fluent 4
      dummy    //foam 5 - fluent 5
      dummy    //foam 6 - fluent 6
      dummy    //foam 7 - fluent 7
      dummy    //foam 8 - fluent 8
      dummy    //foam 9 - fluent 9
      movingWall    //foam 10 - fluent 10
      fixedWalls    //foam 11 - fluent 11
      frontAndBack  //foam 12 - fluent 12
    );
    Notice the details:
    • The commented block that has the files from the "cavity.msh" file are only there for reference for creating the array of names.
    • "unknown" is the default name given for the internal field, as defined in fluentDataToFoam's source code.
    • Keep in mind that the full array of names has to be given, with dummy names for the patches that don't have a name assigned on OpenFOAM's side of things.
    • Said array starts at 0 (zero), which is why there is the extract line at the top of the array.
  4. Then you can run the converter for the desired time instance:
    1. Edit the file "system/controlDict" and adjust the "startTime" entry accordingly. For example, I want to convert the time instance "0.1":
      Code:
      startTime       0.1;
    2. The convert:
      Code:
      fluentDataToFoam fluentInterface/cavity0.1.dat


A few notes of caution:
  • This conversion method does not take into account all of the possible boundary conditions! For example, the original boundary condition for "U" had the following "boundaryField":
    Code:
    boundaryField
    {
        movingWall
        {
            type            fixedValue;
            value           uniform (1 0 0);
        }
        fixedWalls
        {
            type            fixedValue;
            value           uniform (0 0 0);
        }
        frontAndBack
        {
            type            empty;
        }
    }
    The converted form resulted in:
    Code:
    boundaryField
    {
        movingWall
        {
            type            calculated;
            value           uniform (1 0 0);
        }
        fixedWalls
        {
            type            calculated;
            value           uniform (0 0 0);
        }
        frontAndBack
        {
            type            empty;
        }
    }
    This means that you have to edit the field files after conversion and correct appropriately.
  • Convertible fields can be found the source code file "fluentDataToFoam.L", in the "main" function. If you feel lost in the file, search for "momentum".
Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   March 10, 2013, 14:42
Default
  #5
DDB
New Member
 
DDB
Join Date: Jan 2013
Posts: 12
Rep Power: 5
DDB is on a distinguished road
Bruno, you are an OF guru! Thank you so much!

I had no issues at all with the cavity problem, following the steps as you outlined, however I ran into some issues with my old fluent files.

The msh file is easier to find info for the zoneToPatchName than the cas file, but searching for "(39 (" found the stuff ok.

(For my reference when I come back to this, change the number in the zoneToPatchName to correspond to the number of patches! 13 is not unique!)

I have changed the startTime in system/controlDict, but the data only writes to the 0 folder (whereas following your example there was no issue in writing to whatever folder I chose).

I haven't had a chance to look at the boundary conditions yet, but your help so far has been amazing, thank you :-)
DDB is offline   Reply With Quote

Old   March 21, 2013, 06:20
Question
  #6
Senior Member
 
Join Date: Nov 2012
Posts: 168
Rep Power: 5
hz283 is on a distinguished road
Hello Bruno,

Your procedures listed are veru useful. I did the fluentDataToFoam but the following error:

Create time

Machine config: 600012484888
Grid size: nCells = 5984008 nFaces = 12248025 nPoints = 1156110
00Grid size: nCells = 1 nFaces = 25 nPoints = 1


--> FOAM FATAL IO ERROR:
wrong token type - expected int, found on line 1 the punctuation token '('

file: IStringStream.sourceFile at line 1.

From function operator>>(Istream&, int&)
in file primitives/ints/int/intIO.C at line 68.


FOAM exiting

Does it mean the format of the dat files are not correct?


Quote:
Originally Posted by wyldckat View Post
Hi DDB,

Very well, then lets reverse engineer this thing.

First I'm going to use the tutorial "incompressible/icoFoam/cavity" as basis for creating the simple Fluent dataset:
  1. Run the tutorial:
    Code:
    blockMesh
    icoFoam
  2. Then extract the components for U:
    Code:
    foamCalc components U
Now to convert the mesh and data to Fluent format:
  1. Create the file "system/foamDataToFluentDict" with the following contents:
    Code:
    /*--------------------------------*- C++ -*----------------------------------*\
    | =========                 |                                                 |
    | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
    |  \\    /   O peration     | Version:  2.1.x                                 |
    |   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
    |    \\/     M anipulation  |                                                 |
    \*---------------------------------------------------------------------------*/
    FoamFile
    {
        version     2.0;
        format      ascii;
        class       dictionary;
        location    "system";
        object      foamDataToFluentDict;
    }
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
    
    p 1;
    
    Ux 111;
    Uy 112;
    Uz 113;
    I know the codes, because I looked at the fluentDataToFoam source code, more specifically inside the file "fluentDataToFoam.L".
  2. Converted the OpenFOAM mesh and data to Fluent format:
    Code:
    foamMeshToFluent
    foamDataToFluent


Now for converting stuff back from Fluent to OpenFOAM:
  1. Convert the mesh by running:
    Code:
    fluentMeshToFoam fluentInterface/cavity.msh
    This is only because this is the simple cavity. fluent3DMeshToFoam should be used for more complicated cases.
  2. Then look into the file "fluentInterface/cavity.msh" and find the codes for each patch. At the end of the file you should find this:
    Code:
    (39 (1 fluid fluid-1)())
    (39 (2 interior interior-1)())
    (39 (10 wall movingWall)())
    (39 (11 wall fixedWalls)())
    (39 (12 pressure-outlet frontAndBack)())
    This is what we'll use as reference for the "zoneToPatchName" file.
  3. Create the file "constant/polyMesh/zoneToPatchName" with the following contents:
    Code:
    /*--------------------------------*- C++ -*----------------------------------*\
    | =========                 |                                                 |
    | \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
    |  \\    /   O peration     | Version:  2.1.x                                 |
    |   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
    |    \\/     M anipulation  |                                                 |
    \*---------------------------------------------------------------------------*/
    FoamFile
    {
        version     2.0;
        format      ascii;
        class       wordList;
        location    "constant/polyMesh";
        object      zoneToPatchName;
    }
    // * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
    
    /*
    (39 (1 fluid fluid-1)())
    (39 (2 interior interior-1)())
    (39 (10 wall movingWall)())
    (39 (11 wall fixedWalls)())
    (39 (12 pressure-outlet frontAndBack)())
    */
    
    13
    (
      dummy    //foam 0 - no fluent correspondence
      unknown  //foam 1 - fluent 1
      interior //foam 2 - fluent 2
      dummy    //foam 3 - fluent 3
      dummy    //foam 4 - fluent 4
      dummy    //foam 5 - fluent 5
      dummy    //foam 6 - fluent 6
      dummy    //foam 7 - fluent 7
      dummy    //foam 8 - fluent 8
      dummy    //foam 9 - fluent 9
      movingWall    //foam 10 - fluent 10
      fixedWalls    //foam 11 - fluent 11
      frontAndBack  //foam 12 - fluent 12
    );
    Notice the details:
    • The commented block that has the files from the "cavity.msh" file are only there for reference for creating the array of names.
    • "unknown" is the default name given for the internal field, as defined in fluentDataToFoam's source code.
    • Keep in mind that the full array of names has to be given, with dummy names for the patches that don't have a name assigned on OpenFOAM's side of things.
    • Said array starts at 0 (zero), which is why there is the extract line at the top of the array.
  4. Then you can run the converter for the desired time instance:
    1. Edit the file "system/controlDict" and adjust the "startTime" entry accordingly. For example, I want to convert the time instance "0.1":
      Code:
      startTime       0.1;
    2. The convert:
      Code:
      fluentDataToFoam fluentInterface/cavity0.1.dat


A few notes of caution:
  • This conversion method does not take into account all of the possible boundary conditions! For example, the original boundary condition for "U" had the following "boundaryField":
    Code:
    boundaryField
    {
        movingWall
        {
            type            fixedValue;
            value           uniform (1 0 0);
        }
        fixedWalls
        {
            type            fixedValue;
            value           uniform (0 0 0);
        }
        frontAndBack
        {
            type            empty;
        }
    }
    The converted form resulted in:
    Code:
    boundaryField
    {
        movingWall
        {
            type            calculated;
            value           uniform (1 0 0);
        }
        fixedWalls
        {
            type            calculated;
            value           uniform (0 0 0);
        }
        frontAndBack
        {
            type            empty;
        }
    }
    This means that you have to edit the field files after conversion and correct appropriately.
  • Convertible fields can be found the source code file "fluentDataToFoam.L", in the "main" function. If you feel lost in the file, search for "momentum".
Best regards,
Bruno
hz283 is offline   Reply With Quote

Old   March 24, 2013, 13:13
Default
  #7
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,556
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi hz283,

Follow my example with the tutorial case and then compare the file formats.
I say this because I can't figure out what's wrong just from your error message So you'll have to compare the files yourself!

Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   March 24, 2013, 14:15
Default
  #8
Senior Member
 
Join Date: Nov 2012
Posts: 168
Rep Power: 5
hz283 is on a distinguished road
Hi Bruno,

Thank you so much for your continuous help.

best H

Quote:
Originally Posted by wyldckat View Post
Hi hz283,

Follow my example with the tutorial case and then compare the file formats.
I say this because I can't figure out what's wrong just from your error message So you'll have to compare the files yourself!

Best regards,
Bruno
hz283 is offline   Reply With Quote

Old   October 6, 2013, 11:09
Default
  #9
Senior Member
 
Alhasan's Avatar
 
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 196
Rep Power: 6
Alhasan is on a distinguished road
Hi Bruno,
From all this i just have one question for you I'm not that familiar with openFOAM so that being said
in the foamDatatoFluentDict

how do you know what value corresponds to what like u have entered
p 1;

Ux 111;
Uy 112;
Uz 113;

i want to know the values for objects such as k, alpha, p_mean, u_mean and all such objects and their corresponding number where is the dictionary with the list of values and i dunno where is "fluentDataToFoam.L" been searching all inside open foam

Best Regards,
Hasan K.J.
Alhasan is offline   Reply With Quote

Old   October 6, 2013, 11:16
Default
  #10
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,556
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Hasan,

Good question! I was going to say that I didn't know, but then I did a quick search and found this: https://github.com/OpenFOAM/OpenFOAM...nitNumbers.txt

Best regards,
Bruno
Alhasan likes this.
__________________
wyldckat is offline   Reply With Quote

Old   October 6, 2013, 11:35
Default
  #11
Senior Member
 
Alhasan's Avatar
 
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 196
Rep Power: 6
Alhasan is on a distinguished road
Hi Bruno,

Thanks for the reply, clearly i have to improve my searching skills coz i have been searching for quite some time now u saved me a lot of time.
So in the link u sent me it comes like
XF_RF_DATA_NULL=0,
XF_RF_DATA_NULL_M1=0,
XF_RF_DATA_NULL_M2=0,
XF_RF_DATA_NULL_MEAN=0,
XF_RF_DATA_NULL_RMS=0,
XF_RF_DATA_PRESSURE=1,

so the nomenclature we put doesnot matter only the number maters or we need to put the nomenclature that will be there on the "0" file ?

Thanks a lot for your time

Regards,
Hasan K.J
Alhasan is offline   Reply With Quote

Old   October 14, 2013, 15:30
Question Thanks for sharing... :) :) :)
  #12
Senior Member
 
Alhasan's Avatar
 
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 196
Rep Power: 6
Alhasan is on a distinguished road
Quote:
Originally Posted by wyldckat View Post
Hi Hasan,

Good question! I was going to say that I didn't know, but then I did a quick search and found this: https://github.com/OpenFOAM/OpenFOAM...nitNumbers.txt

Best regards,
Bruno
Hi Bruno,

That helped me a lot i have been playing with it for the past few days and i am not still able to figure which of the those numbers go for
pMean, PMean2Prime, UMean and UMean2Prime.

atleast for pMean and PMean2Prime i can guess XF_RF_DATA_PRESSURE_MEAN=400,
XF_RF_DATA_PRESSURE_RMS=401,

but for UMean and UMean2Prime (openFOAM has only one file) could it be
XF_RF_DATA_X_VELOCITY_MEAN=402,
XF_RF_DATA_X_VELOCITY_RMS=403,
XF_RF_DATA_Y_VELOCITY_MEAN=404,
XF_RF_DATA_Y_VELOCITY_RMS=405,
XF_RF_DATA_Z_VELOCITY_MEAN=406,
XF_RF_DATA_Z_VELOCITY_RMS=407,

i tired but no luck,
any wise suggestions

Kind Regards,
Hasan K.J
Alhasan is offline   Reply With Quote

Old   October 14, 2013, 16:33
Default
  #13
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,556
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Hasan,

I don't have access to Fluent, therefore I have absolutely no idea
Given that Fluent uses such a coded way of distinguishing fields, my guess is that there are no such fields in Fluent.

My suggestion if that you run a simple example case in Fluent and try to generate those fields. Then save the case in ASCII format and then try to figure out where those fields are defined in the file and which code is used by Fluent.

Good luck! Best regards,
Bruno
Alhasan likes this.
__________________
wyldckat is offline   Reply With Quote

Old   October 14, 2013, 16:49
Default
  #14
Senior Member
 
Alhasan's Avatar
 
Hasan K.J.
Join Date: Dec 2011
Location: Bristol, United Kingdom
Posts: 196
Rep Power: 6
Alhasan is on a distinguished road
Hey Bruno,

Perfect i did that when i had some trouble importing data to CFDPost, but i dunno why it dint strike me now

Thanks a lot for the suggestion
Kind Regards,
Hasan K.J
Alhasan is offline   Reply With Quote

Old   February 3, 2014, 10:16
Default
  #15
New Member
 
Saeed Salehi
Join Date: Aug 2010
Posts: 17
Rep Power: 8
salehi144 is on a distinguished road
Dear Bruno,

First Thanks for your helps.
I did follow your example step by step and it works fine. But when i try to do my own case i get this

------------------------------------------------------------------------------------------------------
Machine config: 600012444888
Grid size: nCells = 1594250 nFaces = 4842786 nPoints = 1654892
\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\\00Grid size: nCells = 1 nFaces = 2 nPoints = 1
E�s���俟h

--> FOAM FATAL IO ERROR:
Attempt to get back from bad stream

file: IStringStream.sourceFile at line 0.

From function void Istream::getBack(token&)
in file db/IOstreams/IOstreams/Istream.C at line 56.

FOAM exiting
------------------------------------------------------------------------------------------------------

What do you think the problem is. Just so you know i am using Ansys Fluent 14.5. Does "fluentDataToFoam" support newer version of fluent files?

Thanks,
Cheers.
salehi144 is offline   Reply With Quote

Old   February 4, 2014, 15:35
Default
  #16
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,556
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Saeed,

Quote:
Originally Posted by salehi144 View Post
What do you think the problem is. Just so you know i am using Ansys Fluent 14.5. Does "fluentDataToFoam" support newer version of fluent files?
I've never used Fluent, so I have no idea.
But I believe that the problem is related to the export option you're using, namely that you cannot use the binary export mode, you must use the ASCII (text) mode.

Best regards,
Bruno
salehi144 likes this.
__________________
wyldckat is offline   Reply With Quote

Old   February 10, 2014, 08:30
Default
  #17
New Member
 
Saeed Salehi
Join Date: Aug 2010
Posts: 17
Rep Power: 8
salehi144 is on a distinguished road
Dear Bruno,

Thanks for your guidance. I'm gonna give it a try.

Best Regards,
salehi144 is offline   Reply With Quote

Old   March 26, 2015, 05:44
Default
  #18
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 9
isabel is on a distinguished road
Dear everybody,

I type fluentDataToFoam name.dat and I also have the following error:

--> FOAM FATAL IO ERROR:
wrong token type - expected int, found on line 1 the punctuation token '('

file: IStringStream.sourceFile at line 1.

From function operator>>(Istream&, int&)
in file primitives/ints/int/intIO.C at line 68



Has anyone solved it?
isabel is offline   Reply With Quote

Old   March 28, 2015, 16:50
Default
  #19
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 9,556
Blog Entries: 39
Rep Power: 97
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Greetings Isabel,

After re-reading most of the posts above, I have to ask you this: is your Fluent data file in ASCII or in binary format?
Because fluentDataToFoam can only handle ASCII format.

Best regards,
Bruno
__________________
wyldckat is offline   Reply With Quote

Old   April 9, 2015, 07:54
Default
  #20
Senior Member
 
isabel
Join Date: Apr 2009
Location: Spain
Posts: 171
Rep Power: 9
isabel is on a distinguished road
Dear Bruno,

Thank you very much. I have disabled the option "write binary files" when I write the Fluent data and now I can execute fluentMeshToFoam and fluentDataToFoam.
Nevertheless, when I open the results in ParaView these are different from the original Fluent ones. I am working with a 3D simulation. Does anybody know what happens?
isabel is offline   Reply With Quote

Reply

Thread Tools
Display Modes

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 On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
UDF compiling problem Wouter Fluent UDF and Scheme Programming 6 June 6, 2012 04:43
Problem Importing Geometry ProE to CFX fatb0y CFX 3 January 14, 2012 20:42
Solve single but higher order equation by OF 1.6 suffering Problem alundilong OpenFOAM Programming & Development 0 December 23, 2010 14:53
natural convection problem for a CHT problem Se-Hee CFX 2 June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem) ParodDav CFX 5 April 29, 2007 19:13


All times are GMT -4. The time now is 07:57.