[blockMesh] #codeStream loop inside a blockMeshDict

francois · April 11, 2015, 12:08

Hi all,

I would like to use #codeStream to define the points of splines in a blockMeshDict.

Here is the code snippet I use:

Code:

 spline 0 1 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$L/(nbPoints-1);
       scalar yi = $Ri - ($Re-$Ri) * (6*pow(xi/$L,5) - 15*pow(xi/$L,4) + 10*pow(xi/$L,3));
        os  << point(xi, -yi, 0) << endl;
        // Info  << point(xi, -yi, 0) << endl;
     }
   #};
  };
   )

The full blockMeshDict file is attached in this post.

I've got this error message:

Code:

--> FOAM FATAL IO ERROR: 
Expected a '(' while reading VectorSpace<Form, Cmpt, nCmpt>, found on line 79 the punctuation token ';'

file: /home/beaubert/OpenFOAM/beaubert-2.3.0/run/convergentMarie/convergentCase/constant/polyMesh/blockMeshDict.edges at line 79.

    From function Istream::readBegin(const char*)
    in file db/IOstreams/IOstreams/Istream.C at line 94.

FOAM exiting

The mesh is fine if I directly put the points coordinates (retrieved with Info) into the blockMeshDict.

Any idea ?
Thanks a lot for your help

Happy foaming

François

hk318i · April 15, 2015, 07:18

Just remove the red semicolon

Quote:

Originally Posted by francois

Hi all,

I would like to use #codeStream to define the points of splines in a blockMeshDict.

Here is the code snippet I use:

Code:

 spline 0 1 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$L/(nbPoints-1);
       scalar yi = $Ri - ($Re-$Ri) * (6*pow(xi/$L,5) - 15*pow(xi/$L,4) + 10*pow(xi/$L,3));
        os  << point(xi, -yi, 0) << endl;
        // Info  << point(xi, -yi, 0) << endl;
     }
   #};
  };
   )

The full blockMeshDict file is attached in this post.

I've got this error message:

Code:

--> FOAM FATAL IO ERROR: 
Expected a '(' while reading VectorSpace<Form, Cmpt, nCmpt>, found on line 79 the punctuation token ';'

file: /home/beaubert/OpenFOAM/beaubert-2.3.0/run/convergentMarie/convergentCase/constant/polyMesh/blockMeshDict.edges at line 79.

    From function Istream::readBegin(const char*)
    in file db/IOstreams/IOstreams/Istream.C at line 94.

FOAM exiting

The mesh is fine if I directly put the points coordinates (retrieved with Info) into the blockMeshDict.

Any idea ?
Thanks a lot for your help

Happy foaming

François

francois · April 17, 2015, 08:36

Thank you very much hk318i !

Note for myself: always read twice before posting, especially if it's in front of my nose

Here is a working example if someone wants to try this #codeStream feature:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;

// Geometry parameters

D 44.45; // Pipe diameter
Lc 263.36625; // Length of the contraction
Re #calc "$D/2.0"; // Exit radius
Ri 67.230625; // Inlet radius
H #calc "0.1*$D"; // Depth
Lp 200; // Length of the pipe
Ld #calc "$Lc+$Lp";

// Mesh parameters

Nx 20;
Ny 20;
Nz 1;

Gx 0.5;
Gy 1;
Gz 1;

// Vertices of the geometry

vertices
(

 (0  #calc "-$Ri" 0)   // Point 0
 ($Lc #calc "-$Re" 0)  // Point 1
 ($Lc $Re 0)           // Point 2
 (0  $Ri 0)            // Point 3

 (0  #calc "-$Ri" $H)  // Point 4
 ($Lc #calc "-$Re" $H) // Point 5
 ($Lc $Re $H)          // Point 6
 (0  $Ri $H)           // Point 7

 ($Ld #calc "-$Re" 0)   // Point 8
 ($Ld $Re 0)            // Point 9
 ($Ld #calc "-$Re" $H)  // Point 10
 ($Ld $Re $H)           // Point 11

);

// Blocks definition

blocks
(
 hex (0 1 2 3 4 5 6 7) ($Nx $Ny $Nz) simpleGrading ($Gx $Gy $Gz)
 hex (1 8 9 2 5 10 11 6) ($Nx $Ny $Nz) simpleGrading ($Gx $Gy $Gz)
);

edges
(

 BSpline 0 1 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, -yi, 0) << endl;
       Info  << point(xi, -yi, 0) << endl;
     }
   #};
  }
   )

 BSpline 4 5 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, -yi, $H) << endl;
       Info  << point(xi, -yi, $H) << endl;
     }
   #};
  }
   )

 BSpline 3 2 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, yi, 0) << endl;
       Info  << point(xi, yi, 0) << endl;
     }
   #};
  }
   )

 BSpline 7 6 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re-$Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, yi, $H) << endl;
       Info  << point(xi, yi, $H) << endl;
     }
   #};
  }
   )
);

// Boundaries

boundary
(
 inlet
 {
   type patch;
   faces
     (
      (0 4 7 3)
      );
 }
 outlet
 {
   type patch;
   faces
     (
      (8 10 11 9)
      );
 }
 upperWallUpstream
 {
   type wall;
   faces
     (
      (3 2 6 7)
      );
 }
 lowerWallUpstream
 {
   type wall;
   faces
     (
      (0 1 5 4)
      );
 }
 upperWallDownstream
 {
   type wall;
   faces
     (
      (2 9 11 6)
      );
 }
 lowerWallDownstream
 {
   type wall;
   faces
     (
      (1 8 10 5)
      );
 }
 frontAndBack
 {
   type empty;
   faces
     (
      (0 1 2 3)
      (4 5 6 7)
      (1 8 9 2)
      (5 10 11 6)
      );
 }
 );

mergePatchPairs
(
);

And the result is attached below

hk318i · April 17, 2015, 09:44

Don't worry, it happens with every foamer

I have only one comment about your code, which could be useful for someone else in the future. Instead of repeating the code for each edge, you can use the codeStream directly inside edges.

Code:

edges (#codeStream { 
   code
   #{
        Calculate all the points....;
       Then
          os << "edgetype1 A B" << pointsList ;
          os << "edgetype2 A B" << pointsList ;
 
   #}
}
);

or you can define new function in separate file myfun.H and include it the you call the function in codeStream.

Code:

#codeStream
{
     codeInclude
    #{
        #include "pointField.H"
        #include "myfun.H"
    #};
            codeOptions
            #{
                -I$(FOAM_CASE)/constant/polyMesh        <-- location of myfun.H
            #};
            codeLibs
            #{

            #};
     code
    #{
          type y = myfunName(inputs);
   os <<  ........ ;
     #}

myfun.H

Code:

using namespace Foam;
type myfunName(type inputs)
{

   forAll(y, i)
   {
       y[i] = function;
   }

   return y;

}

Hopefully these tips will be useful for someone coming directly from google search.

Best wishes,
Hassan

Quote:

Originally Posted by francois

Thank you very much hk318i !

Note for myself: always read twice before posting, especially if it's in front of my nose

Here is a working example if someone wants to try this #codeStream feature:

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;

// Geometry parameters

D 44.45; // Pipe diameter
Lc 263.36625; // Length of the contraction
Re #calc "$D/2.0"; // Exit radius
Ri 67.230625; // Inlet radius
H #calc "0.1*$D"; // Depth
Lp 200; // Length of the pipe
Ld #calc "$Lc+$Lp";

// Mesh parameters

Nx 20;
Ny 20;
Nz 1;

Gx 0.5;
Gy 1;
Gz 1;

// Vertices of the geometry

vertices
(

 (0  #calc "-$Ri" 0)   // Point 0
 ($Lc #calc "-$Re" 0)  // Point 1
 ($Lc $Re 0)           // Point 2
 (0  $Ri 0)            // Point 3

 (0  #calc "-$Ri" $H)  // Point 4
 ($Lc #calc "-$Re" $H) // Point 5
 ($Lc $Re $H)          // Point 6
 (0  $Ri $H)           // Point 7

 ($Ld #calc "-$Re" 0)   // Point 8
 ($Ld $Re 0)            // Point 9
 ($Ld #calc "-$Re" $H)  // Point 10
 ($Ld $Re $H)           // Point 11

);

// Blocks definition

blocks
(
 hex (0 1 2 3 4 5 6 7) ($Nx $Ny $Nz) simpleGrading ($Gx $Gy $Gz)
 hex (1 8 9 2 5 10 11 6) ($Nx $Ny $Nz) simpleGrading ($Gx $Gy $Gz)
);

edges
(

 BSpline 0 1 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, -yi, 0) << endl;
       Info  << point(xi, -yi, 0) << endl;
     }
   #};
  }
   )

 BSpline 4 5 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, -yi, $H) << endl;
       Info  << point(xi, -yi, $H) << endl;
     }
   #};
  }
   )

 BSpline 3 2 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re - $Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, yi, 0) << endl;
       Info  << point(xi, yi, 0) << endl;
     }
   #};
  }
   )

 BSpline 7 6 ( #codeStream
 {
   codeInclude
   #{
      #include "pointField.H"
   #};

   code
   #{
     label nbPoints = 20;
     for (label i = 0; i < nbPoints; i++)
     {
       scalar xi = 0 + i*$Lc/(nbPoints-1);
       scalar yi = $Ri + ($Re-$Ri) * (6*pow(xi/$Lc,5) - 15*pow(xi/$Lc,4) + 10*pow(xi/$Lc,3) );
       os  << point(xi, yi, $H) << endl;
       Info  << point(xi, yi, $H) << endl;
     }
   #};
  }
   )
);

// Boundaries

boundary
(
 inlet
 {
   type patch;
   faces
     (
      (0 4 7 3)
      );
 }
 outlet
 {
   type patch;
   faces
     (
      (8 10 11 9)
      );
 }
 upperWallUpstream
 {
   type wall;
   faces
     (
      (3 2 6 7)
      );
 }
 lowerWallUpstream
 {
   type wall;
   faces
     (
      (0 1 5 4)
      );
 }
 upperWallDownstream
 {
   type wall;
   faces
     (
      (2 9 11 6)
      );
 }
 lowerWallDownstream
 {
   type wall;
   faces
     (
      (1 8 10 5)
      );
 }
 frontAndBack
 {
   type empty;
   faces
     (
      (0 1 2 3)
      (4 5 6 7)
      (1 8 9 2)
      (5 10 11 6)
      );
 }
 );

mergePatchPairs
(
);

And the result is attached below

francois · April 17, 2015, 10:03

Thanks Hassan for your kind and very relevant suggestions.

I was thinking myself of refactoring the code which was submitted here only as proof of concept for myself or other newcomers to #codeStream.

Anyway, those are indeed very nice additions to put into the code, thanks !
I may put all this stuff on the wiki when I'll find the time.

You're a good example that illustrates why I like so much the OpenFOAM community.
Happy foaming

hk318i · April 29, 2015, 13:25

Hello!
I hit one of the codeStream limitations today. I would like to share it with everyone here.

Code:

string "
         int N = 100;
         scalar cw = $cw*$ftTom; // chord
         scalar..."
    is too long (max. 8000 characters)

Although I used the method which I mentioned above, I had to write a very very long codeStream. Fortunately, I found a solution for this problem which is dividing the code stream to many .H files and includes directly inside the code not as a header file.

Code:

    code
    #{
#include "myLongCode.H"
     #};

BUT, there is a drawback for this method, you cannot use the macro substitutions ($parameter). I desperately tried "#inputMode merge" but it doesn't work.
So to read any variable from the blockMeshDict in this case, you have to lookup it.

Code:

scalar a = readScalar(dict.lookup("a"));

Next time, I have to FOAM responsibly

arieljeds · October 1, 2015, 07:07

On using codestream... I understand the syntax to duplicate points but I want to then see the points so I can construct the blocks... Maybe this is a stupid question but I'm very very new to CFD and meshing so I don't understand how, once I've duplicated the points, I "know" where each one is and how the block structure should be using the new points... can anyone advise on the best practice for this?

hk318i · October 1, 2015, 09:09

Quote:

Originally Posted by arieljeds

On using codestream... I understand the syntax to duplicate points but I want to then see the points so I can construct the blocks... Maybe this is a stupid question but I'm very very new to CFD and meshing so I don't understand how, once I've duplicated the points, I "know" where each one is and how the block structure should be using the new points... can anyone advise on the best practice for this?

You can use

Code:

paraFoam -block

It shows the points so you could create the blocks which is really helpful.
I am not sure if that what you are looking for or not. Maybe you mean if you have list called points and you want use points[5] in blocks.
In this case, based on my experience, you cannot do that directly because the variables are limited to codeStream scope.

BUT there is a way around this problem which is including the blocks section inside the same codeStream as points. Then use os stream to print blocks as well. Or you can write a script (using python or octave or m4 .) to create blockMesh file.

arieljeds · October 1, 2015, 09:18

Hi there,

Thanks for that. Actually I wasn't sure if that would work without running blockMesh first...

Ok just tried and how is it possible to do this without first building the blocks? Or do I just put:

Code:

blocks
(
);

And leave the blocks blank?

hk318i · October 1, 2015, 09:26

It works without executing blockMesh, just make sure that boundary is empty as well. It will show you the points and edges

arieljeds · October 1, 2015, 09:28

perfect! Thanks for that... very difficult to find something so simple online!

arieljeds · October 1, 2015, 09:55

Sorry, last question.. say I'm trying to duplicate both the z points (as done in the cylinder tutorial) and the y points. I tried to just include a second loop as follows:

Code:

label sy = points.size();
points.setSize(2*sy);
for (label i = 0; i < sy; i++)
{
     const point& pt = points[i];
     points[i+sy] = point(pt.x(), -pt.y(), pt.z());
}

os << points;

But this (perhaps obviously) didn't work... Can you offer any guidance on the correct syntax to use?

luks1910 · March 8, 2021, 19:27

I realize this is an old thread but thought I would try and revive it to ask a related question. I am using openfoam8 and #codeStream in blockMeshDict. The vertices are computing okay, but there are issues with the edges. It seems that the quoted response provided by hk318i to output the edge dictionary does not work anymore in openfoam8. Here is the loop in my code where i output each line:

Code:

//std::string v1,  v2;
int v1,  v2;
for (int i=0; i<np;  i++)
{
// vertices of  interest
if ((i+1)%4==0)  {
 //v1 =  std::to_string(i);
//v2 =  std::to_string(i-3);
v1 =  i;
v2 =  i-3;
} else  {
//v1 =  std::to_string(i);
//v2 =  std::to_string(i+1);
v1 =  i;
v2 =  i+1;
}
//  output
Info << "arc " << v1 << " " << v2 << " "  << points[i] <<  endl;
os << "arc " << v1 << " " << v2 << " "  << points[i] <<  endl;
//Info << "arc "+v1+" "+v2+" " << points[i] <<  endl;
//os << "arc "+v1+" "+v2+" " << points[i] <<  endl;
}

The Info output looks like what I would type into the blockMeshDict file, but I get the following error:

Code:

 -->  FOAM FATAL IO  ERROR:
incorrect first token, expected <int> or '(', found on line 0 the  word 'arc'

Unfortunately there are no #codeStream examples where edges are output in the tutorials, only vertices. I have tried out the vertices as a string (shown in commented line), without spaces and anything I could think of pretty much but no luck. Any suggestions?

Thanks!
Luca

Quote:

Originally Posted by hk318i

Don't worry, it happens with every foamer

I have only one comment about your code, which could be useful for someone else in the future. Instead of repeating the code for each edge, you can use the codeStream directly inside edges.

Code:

edges (#codeStream { 
   code
   #{
        Calculate all the points....;
       Then
          os << "edgetype1 A B" << pointsList ;
          os << "edgetype2 A B" << pointsList ;
 
   #}
}
);

or you can define new function in separate file myfun.H and include it the you call the function in codeStream.

Code:

#codeStream
{
     codeInclude
    #{
        #include "pointField.H"
        #include "myfun.H"
    #};
            codeOptions
            #{
                -I$(FOAM_CASE)/constant/polyMesh        <-- location of myfun.H
            #};
            codeLibs
            #{

            #};
     code
    #{
          type y = myfunName(inputs);
   os <<  ........ ;
     #}

myfun.H

Code:

using namespace Foam;
type myfunName(type inputs)
{

   forAll(y, i)
   {
       y[i] = function;
   }

   return y;

}

Hopefully these tips will be useful for someone coming directly from google search.

Best wishes,
Hassan

Tobermory · March 12, 2021, 05:14

It would helpful if you added in a full listing of the blockMeshDict that the code tried to create. From the error message, it looks like you have the wrong syntax for the arc command - check out section 5.3.1.2 in https://cfd.direct/openfoam/user-guide/v6-blockmesh/ and compare against what you have in your file.

Good luck!

luks1910 · March 12, 2021, 12:42

Here is the full blockMeshDict file, as well as a geometryInput file from the constant directory which is required for it to run. I am trying to recreate a previously generated blockMeshDict file with codeStream, so it can eventually be expanded. There is a commented out edges() dictionary in the file as well with hardcoded values, the blockMeshDict file fine runs with this edges dictionary. The boundaries are eliminated for use with paraFoam -block. Thanks for taking the time to look at this!

Tobermory · March 12, 2021, 13:55

Could you also just include the Info output? I.e. from this, we can see the parsing of the previous lines and the line that it crashes on ... would be quicker than debugging your code.

Tobermory · March 12, 2021, 13:59

One quick thing to consider - your codestream creates lists of vertices and then edges ... these need to be bracketed, and I don't see those brackets in your code. e.g.

Code:

vertices
(
    <list of vertices here>
);
   
  
edges
(
    <list of edges here>
);

that might be screwing with the parser ... Eg, should you not have

Code:

vertices (#codeStream
{

etc.

luks1910 · March 12, 2021, 14:31

Yes that makes sense, I apologize for the missing info. Here is the last line of my output including Info output for edges in the blockMeshDict I sent:

Code:

 arc01(0.041 0 0)
arc12(0 0.041 0)
arc23(-0.041 0 0)
arc30(0 -0.041 0)
arc45(0.045 0 0)
arc56(0 0.045 0)
arc67(-0.045 0 0)
arc74(0 -0.045 0)
arc89(0.041 0 3.96)
arc910(0 0.041 3.96)
arc1011(-0.041 0 3.96)
arc118(0 -0.041 3.96)
arc1213(0.045 0 3.96)
arc1314(0 0.045 3.96)
arc1415(-0.045 0 3.96)
arc1512(0 -0.045 3.96)
arc1617(0.1426 0 5.333)
arc1718(0 0.1426 5.333)
arc1819(-0.1426 0 5.333)
arc1916(0 -0.1426 5.333)
arc2021(0.041 0 5.333)
arc2122(0 0.041 5.333)
arc2223(-0.041 0 5.333)
arc2320(0 -0.041 5.333)
arc2425(0.045 0 5.333)
arc2526(0 0.045 5.333)
arc2627(-0.045 0 5.333)
arc2724(0 -0.045 5.333)
arc2829(0.1426 0 5.333)
arc2930(0 0.1426 5.333)
arc3031(-0.1426 0 5.333)
arc3128(0 -0.1426 5.333)
arc3233(0.03134 -0.0085 5.422)
arc3334(0 0.02284 5.422)
arc3435(-0.03134 -0.0085 5.422)
arc3532(0 -0.041 5.422)
arc3637(0.0365 -0.0085 5.422)
arc3738(0 0.028 5.422)
arc3839(-0.0365 -0.0085 5.422)
arc3936(0 -0.045 5.422)
arc4041(0.13294 -0.0085 5.422)
arc4142(0 0.12444 5.422)
arc4243(-0.13294 -0.0085 5.422)
arc4340(0 -0.1426 5.422)
Creating block edges                                                                         



 --> FOAM FATAL IO ERROR:
wrong token type - expected word, found on line 0 the doubleScalar 0.041


file: /home/limponenti/OpenFOAM/limponenti-8/run/emptyHCE/system/blockMeshDict/edges at line 0.


From function Foam::Istream& Foam::operator>>(Foam::Istream&, Foam::word&)
in file primitives/strings/word/wordIO.C at line 74.


FOAM exiting

Note that I have tried adding as spaces into the initial string as well which is why this error message is a little different from the original post. Regarding your second comment, I believe the brackets (vs parenthesis) are due to the codeStream command. It is the same in the example for vertices found in: $FOAM_TUTORIALS/basic/potentialFoam/cylinder/system/blockMeshDict .

Tobermory · March 13, 2021, 11:23

Quote:

Originally Posted by luks1910

Regarding your second comment, I believe the brackets (vs parenthesis) are due to the codeStream command. It is the same in the example for vertices found in: $FOAM_TUTORIALS/basic/potentialFoam/cylinder/system/blockMeshDict .

Ah - I think I see the problem now. Try run the above tutorial and add in a print command to see what it is that the codestream is delivering:

Code:

vertices #codeStream
{
...
    code
    #{
        pointField points(19);
        points[0]  = point(0.5, 0, -0.5);
        points[1]  = point(1, 0, -0.5);
...
        os  << points;
        Info << points;
    #};
};

This prints a list of points (since it is writing out the entire points array rather than value by value):

Code:

38
(
(0.5 0 -0.5)
(1 0 -0.5)
...
(-0.707107 2 0.5)
)

That's why it did not need to add the brackets that I highlighted in my earlier post. When you are writing out your edge data, you are not writing a list (i.e. an array of values), but instead are writing out each arc line by line, so you need to tell the parser that a list of edge definitions is coming ... that's why you need the brackets that I highlighted earlier. Chack back to hk318i's pervious posts and you'll see that he has them in.

luks1910 · March 13, 2021, 12:29

Yes thank you! With the brackets added, and also outputting the vertices as integers with spaces in between, everything works. Here is the final edges call with codeStream output for each point:

Code:

edges (#codeStream
{
    codeInclude
    #{ 
        #include "pointField.H"
    #};

    code
    #{
        // calculate required points, in this case midpoint of arcs
        // ...
    
        // get vertices and output edge
        int v1, v2;
        for (int i=0; i<np; i++)
        {
            // vertices of interest
            if ((i+1)%4==0) {
                v1 = i;
                v2 = i-3;
            } else {
                v1 = i;
                v2 = i+1;
            }

            // output
            Info << "arc " << v1 << " " << v2 << " " << points[i] << endl;
            os << "arc " << v1 << " " << v2 << " " << points[i] << endl;
        }
    #};
}
);

April 17, 2015, 10:03		#5
francois Senior Member Francois Beaubert Join Date: Mar 2009 Location: Lille, France Posts: 147 Rep Power: 17	Thanks Hassan for your kind and very relevant suggestions. I was thinking myself of refactoring the code which was submitted here only as proof of concept for myself or other newcomers to #codeStream. Anyway, those are indeed very nice additions to put into the code, thanks ! I may put all this stuff on the wiki when I'll find the time. You're a good example that illustrates why I like so much the OpenFOAM community. Happy foaming hk318i likes this.

April 29, 2015, 13:25		#6
hk318i Senior Member Hassan Kassem Join Date: May 2010 Location: Germany Posts: 242 Rep Power: 17	Hello! I hit one of the codeStream limitations today. I would like to share it with everyone here. Code: string " int N = 100; scalar cw = $cw*$ftTom; // chord scalar..." is too long (max. 8000 characters) Although I used the method which I mentioned above, I had to write a very very long codeStream. Fortunately, I found a solution for this problem which is dividing the code stream to many .H files and includes directly inside the code not as a header file. Code: code #{ #include "myLongCode.H" #}; BUT, there is a drawback for this method, you cannot use the macro substitutions ($parameter). I desperately tried "#inputMode merge" but it doesn't work. So to read any variable from the blockMeshDict in this case, you have to lookup it. Code: scalar a = readScalar(dict.lookup("a")); Next time, I have to FOAM responsibly

October 1, 2015, 09:18		#9
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Hi there, Thanks for that. Actually I wasn't sure if that would work without running blockMesh first... Ok just tried and how is it possible to do this without first building the blocks? Or do I just put: Code: blocks ( ); And leave the blocks blank?

October 1, 2015, 09:55		#12
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	Sorry, last question.. say I'm trying to duplicate both the z points (as done in the cylinder tutorial) and the y points. I tried to just include a second loop as follows: Code: label sy = points.size(); points.setSize(2*sy); for (label i = 0; i < sy; i++) { const point& pt = points[i]; points[i+sy] = point(pt.x(), -pt.y(), pt.z()); } os << points; But this (perhaps obviously) didn't work... Can you offer any guidance on the correct syntax to use?

March 12, 2021, 13:59		#17
Tobermory Senior Member Join Date: Apr 2020 Location: UK Posts: 670 Rep Power: 14	One quick thing to consider - your codestream creates lists of vertices and then edges ... these need to be bracketed, and I don't see those brackets in your code. e.g. Code: vertices ( <list of vertices here> ); edges ( <list of edges here> ); that might be screwing with the parser ... Eg, should you not have Code: vertices (#codeStream { etc.

October 1, 2015, 07:07		#7
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	On using codestream... I understand the syntax to duplicate points but I want to then see the points so I can construct the blocks... Maybe this is a stupid question but I'm very very new to CFD and meshing so I don't understand how, once I've duplicated the points, I "know" where each one is and how the block structure should be using the new points... can anyone advise on the best practice for this?

October 1, 2015, 09:26		#10
hk318i Senior Member Hassan Kassem Join Date: May 2010 Location: Germany Posts: 242 Rep Power: 17	It works without executing blockMesh, just make sure that boundary is empty as well. It will show you the points and edges

October 1, 2015, 09:28		#11
arieljeds Senior Member ArielJ Join Date: Aug 2015 Posts: 127 Rep Power: 10	perfect! Thanks for that... very difficult to find something so simple online!

March 12, 2021, 05:14		#14
Tobermory Senior Member Join Date: Apr 2020 Location: UK Posts: 670 Rep Power: 14	It would helpful if you added in a full listing of the blockMeshDict that the code tried to create. From the error message, it looks like you have the wrong syntax for the arc command - check out section 5.3.1.2 in https://cfd.direct/openfoam/user-guide/v6-blockmesh/ and compare against what you have in your file. Good luck!

March 12, 2021, 13:55		#16
Tobermory Senior Member Join Date: Apr 2020 Location: UK Posts: 670 Rep Power: 14	Could you also just include the Info output? I.e. from this, we can see the parsing of the previous lines and the line that it crashes on ... would be quicker than debugging your code.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
[Other] Contribution a new utility: refine wall layer mesh based on yPlus field	lakeat	OpenFOAM Community Contributions	58	December 23, 2021 02:36
[Other] refineWallLayer Error	Yuby	OpenFOAM Meshing & Mesh Conversion	2	November 11, 2021 11:04
Star-CCM+ Macro - Loop over just wall boundary conditions	jbatchel	STAR-CCM+	5	March 2, 2018 13:42
Pressure distribution on a wall	darazsbence	CFX	17	October 6, 2015 10:38
How to determine a point is inside a tetrahedral?	G.P. Xia	Main CFD Forum	16	January 12, 2000 11:15