[ninoleum]

Okay, Bruno you were right: I was living in the illusion that the blocks topology could take advantage from the edges curvature (spline in my case) so I tried to define with just one block the helical sweep of each block face whose normal is in tangential direction (local x axis). Instead topology is built, as far as I understand, by only connecting the edges in the block's vertexes list with straight lines.
So I solved the negative volume error by defining 27 blocks instead of 9, sweeping on the helical path by only 120° and not 360° (sigh).

Hassan, I did not get any error from the #codestream routines during blockmeshing. What errors did it show to you?

Thank you both for your help

Cheers

Gianluca

[hk318i]

Hello Gianluc,

I am investigating the reasons of this error (log attached). It is strange error but it seems to be related to OpenFOAM version. I am not sure yet. I tried your code using two versions of OpenFOAM-2.3.x. The newer version (18th Jun 2015) is not working, however the older version (26th Feb) is fine.
I will update both and recompile both to pinpoint the problem. Another possibility, maybe, it is related to gcc version. I will check that as well.

Best wishes,
Hassan

[hk318i]

I updated OpenFOAM-2.3.x, to check if this error due to any new commits. It seems not, because your blockMesh worked even with the updated OpenFOAM-2.3.x. Therefore I tried a third updated version of OpenFOAM-2.3.x on different system and I get the same error.
Now, I think (maybe), it is something related to GCC version because it worked with GCC-4.9.2 (Ubuntu 15.04) but it did not work with GCC-4.8.4 (Ubuntu 14.04LTS) nor GCC-4.7.3 (CentOS 6.5).

Could you please check your GCC version?

Bw,
Hassan

[ninoleum]

Hi Hassan,
here is the output of "gcc -v": gcc version 4.9.2 (Debian 4.9.2-10).

The error you are getting seems to be strange to me because in my humble experience, normally the use of uninitialized array leads to a gcc warning, unless gcc is instructed to treat warnings as errors.

Regards

Gianluca

[luks1910]

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:

//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:

 -->  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

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.

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.

#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

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]

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]

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]

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]

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.

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

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

vertices (#codeStream
{

etc.

[luks1910]

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:

 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]

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:

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):

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]

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:

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;
        }
    #};
}
);