CFD Online Discussion Forums - [blockMesh] Writing a blockMeshDict file with variables

CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)

- OpenFOAM Meshing & Mesh Conversion (https://www.cfd-online.com/Forums/openfoam-meshing/)

- - [blockMesh] Writing a blockMeshDict file with variables (https://www.cfd-online.com/Forums/openfoam-meshing/164502-writing-blockmeshdict-file-variables.html)

Writing a blockMeshDict file with variables

Hi there,
I'm trying to write a blockmesh file using variables for the vertices and the number of cells but I'm not quite sure how to do this. At the moment, I'm trying this:

Code:

convertToMeters 1;



x   20.0;        // Length of tank

y1  -3.0;        // Width of tank/2

y2   3.0;        // Width of tank/2

zf  -0.4;        // Water depth 

za   0.2;            // Distance above free surface

L    3.6942;    // Wavelength 

n    5;                // Number of cells per wavelength 



xn   ($x/$L)*$n;        // Calculating the number of cells

//yn    

//zn 



vertices        

(

    ( 0   $y1  $zf )         // 0                

    ( $x  $y1  $zf )     // 1

    ( $x  $y2  $zf )         // 2

    ( 0   $y2  $zf )         // 3

   

    ( 0   $y1  $za )         // 4 

    ( $x  $y1  $za )         // 5

    ( $x  $y2  $za )         // 6

    ( 0   $y2  $za )         // 7    

);



blocks 

         

(

  hex (0 1 2 3 4 5 6 7) ($xn 10 10) simpleGrading (1 1 1) //(1 10 0.1)

);



edges           

(

);



boundary         

( 

   inlet

   {

       type patch;

       faces

           (

                ( 0 3 7 4 )

           );

   }

   

   outlet

   {

       type patch; 

       faces

           (

          ( 1 2 6 5 )

           );

   }

   

   atmosphere

   {

       type patch;

       faces

           (

          ( 4 5 6 7 )

           );

   }

   

   front

   {

       type symmetryPlane;

       faces

          (

                 ( 3 2 6 7 )

        );

   }

Perhaps unsurprisingly, I'm running into problems with the line where I am attempting to calculate xn. Does anyone know the syntax how I can do this? Or if it's possible at all to do a simple calculation in the blockMeshDict?

Thanks in advance for any advice

Hi,

Code:

$ cd $FOAM_TUTORIALS

$ grep -r '#calc' *

incompressible/simpleFoam/pipeCyclic/system/blockMeshDict:radHalfAngle    #calc "degToRad($halfAngle)";

incompressible/simpleFoam/pipeCyclic/system/blockMeshDict:y               #calc "$radius*sin($radHalfAngle)";

incompressible/simpleFoam/pipeCyclic/system/blockMeshDict:minY            #calc "-1.0*$y";

incompressible/simpleFoam/pipeCyclic/system/blockMeshDict:z               #calc "$radius*cos($radHalfAngle)";

incompressible/simpleFoam/pipeCyclic/system/blockMeshDict:minZ            #calc "-1.0*$z";

multiphase/interDyMFoam/ras/floatingObject/constant/dynamicMeshDict:    mass            #calc "$rho*$Lx*$Ly*$Lz";

$ less incompressible/simpleFoam/pipeCyclic/system/blockMeshDict

...

//- Half angle of wedge in degrees

halfAngle 45.0;



//- Radius of pipe [m]

radius 0.5;





radHalfAngle    #calc "degToRad($halfAngle)";

y               #calc "$radius*sin($radHalfAngle)";

minY            #calc "-1.0*$y";

z               #calc "$radius*cos($radHalfAngle)";

minZ            #calc "-1.0*$z";

...

@alexeym - Thanks a lot. That's what I was looking for

Ok one more question on this.. Because the calculation I am making is going to be for the number of cells, I need to convert it to an integer. I'm having trouble finding an example of how to do this.

Any ideas?

Thanks again!

Well, if you take a look into src/OpenFOAM/db/dictionary/functionEntries/calcEntry/calcEntry.H, there is a note:

Code:

Note

    Internally this is just a wrapper around codeStream functionality - the

    #calc string gets used to construct a dictionary for codeStream.

So you can use usual C++ functions, for example, std::floor or std::ceil.

Hi Alexey, thanks again for getting back to me so quickly. Ok so as I'm understanding it, the use of calc would be:

Code:

x     20.0; 

n = 5; 

L = 3.69;



xn  #calc "($x/$L)*n";

xn1 #calc "std::floor(float $xn)"; 



...



blocks 

{

    hex ( 0 1 2 3 4 5 6 7 ) (xn1 10 10) simpleGrading (1 1 1)

}



...

Is this correct?

Just

Code:

std::floor($xn)

If we take an example from tutorials (incompressible/simpleFoam/pipeCyclic) and add the lines:

Code:

test            #calc "std::floor($halfAngle/4)";

#calc "Info<< $test << endl";

output of blockMesh would be

Code:

... codeStream object compilation output ...

11

Creating curved edges

Creating topology blocks

...

So in your expressions you forget $ before n and used unnecessary float in function call.

Hi Alexey,

I should've written back quicker... I messed around with it a bit and found my way to that syntax and have it working now.

thanks a lot again for your help!

Ariel

Hello,

I was trying to implement something similar, but i have problems with negative variables.
It seems i can decleare them but as soon i use them in the calc expression the blockMesh gives me an error.

So in

Code:

x1 -30;

//x1 30;

x2 50;



dx #calc "$x1";

//dx 10;

If x1 is declared as positive, everything is ok.
If x1 is declared as negative and dx =10 , everything is ok.
if x1 is declared as negative and dx as ´ #calc "$x1";´ i get an error.

Does anybody knows the reason and a work around?

Note that the real operation that i would like to do is something like

Code:

nx #calc "std::floor( ($x2-$x1)*$n )";

Thank you in advance.

Hi,

You need to have a space between the variables and the operator for it to recognize it as subtraction.

Instead of: $x2-$x1

So it should be: $x2 - $x1

Not sure if this is documented, but this was what I found out when I was playing around with this feature.

Hope this helps.

Cheers,
Antimony

Correct,

This worked.

Thank you

Using Regular C++ syntax to write Blockmesh file

hello everyone,
if i wanted to use regular C++ or objective C syntax to organize my code could I do that?
for example

Code:



class cPlane

{ // whatever you need

};



class cSphere

{

int MyVariable;

// whatever else you need

};



class cObject

{ cPlane MyPlane;

   cSphere MySphere;



//  whetever else you need

};



int main()

{

   cObject MyObjects[99];



// whatever  you need



}

i mostly write in python. So please don't fill me in on how there are better languages for writing text files than C++. I am WELL AWARE LOL! But i like learning languages by writing in them. So this is a good way for me to improve.

i want to get practice writing in C++11 so that I can more easily ready the source code.
I am working on a pretty complex blockmesh right now and would like to use oop in my code to try to help organize the shapes.

Has anyone done this? Would I use #codestream for this. I am working my way through the manual. But found the codestream section a bit confusing...

Figured out how to do this. #include. The of manual says it all

Sent from my SM-G930V using CFD Online Forum mobile app

Error while using calc

Hi everyone!

I'm having lots of trouble with this functionality...Can someone help me please?

I started with a very basic expression:

xA 30;
xU 20;
acaso #calc "xA + xU";

and it gives the following error:

Creating block mesh from
"/home/laj/OpenFOAM/laj-6/run/interFoam/expo/expoBCTest/system/blockMeshDict"
Using #calcEntry at line 33 in file "/home/laj/OpenFOAM/laj-6/run/interFoam/expo/expoBCTest/system/blockMeshDict"
Using #codeStream with "/home/laj/OpenFOAM/laj-6/run/interFoam/expo/expoBCTest/dynamicCode/platforms/linux64GccDPInt32Opt/lib/libcodeStream_a9cfc2467f9de95ca529e46e98786f31497c cff1.so"
Creating new library in "dynamicCode/_a9cfc2467f9de95ca529e46e98786f31497ccff1/platforms/linux64GccDPInt32Opt/lib/libcodeStream_a9cfc2467f9de95ca529e46e98786f31497c cff1.so"
Invoking "wmake -s libso /home/laj/OpenFOAM/laj-6/run/interFoam/expo/expoBCTest/dynamicCode/_a9cfc2467f9de95ca529e46e98786f31497ccff1"
wmake libso /home/laj/OpenFOAM/laj-6/run/interFoam/expo/expoBCTest/dynamicCode/_a9cfc2467f9de95ca529e46e98786f31497ccff1
/opt/openfoam6/wmake/wmake: riga 410: make: command not found
/opt/openfoam6/wmake/wmake: riga 413: make: command not found
wmake error: file 'Make/linux64GccDPInt32Opt/sourceFiles' could not be created in /home/laj/OpenFOAM/laj-6/run/interFoam/expo/expoBCTest/dynamicCode/_a9cfc2467f9de95ca529e46e98786f31497ccff1

--> FOAM FATAL IO ERROR:
Failed wmake "dynamicCode/_a9cfc2467f9de95ca529e46e98786f31497ccff1/platforms/linux64GccDPInt32Opt/lib/libcodeStream_a9cfc2467f9de95ca529e46e98786f31497c cff1.so"

file: /home/laj/OpenFOAM/laj-6/run/interFoam/expo/expoBCTest/system/blockMeshDict from line 17 to line 32.

From function static void (* Foam::functionEntries::codeStream::getFunction(con st Foam::dictionary&, const Foam::dictionary&))(Foam::Ostream&, const Foam::dictionary&)
in file db/dictionary/functionEntries/codeStream/codeStream.C at line 218.

FOAM exiting

Any clue?

Thank you very much!

Quote:

Originally Posted by Jack_Landis (Post 714978)

you need a dollar sign before all your variables when you call them, so:

Code:

xA 30;

xU 20;

acaso #calc "$xA + $xU";

Hello!

I tried but it gave me the same error...Anyother ideas?

Make sure 2 add spaces aroundathematical characters such as -+×÷/.

Creating a parametric array of geometries

Hi everyone,

I am relatively new to OpenFOAM. I want to create an array of rectangular grooves in my geometry that are defined by some parameters (width, height, and spacing). From what I learned in this thread, I am able to use a while loop to create the required vertices for the grooves. However, I am having some issues when intend to create the blocks using hex inside a while loop. Below is my code;

Code:

convertToMeters 0.001;



plate_length 96;

domain_height 30;

a 1; //defines the spacing between each two grooves

b 7; // defines the width of the grooves

c 2; // defines the height of the grooves



vertices 

(

    (0 0 0)

    ($plate_length 0 0)

    ($plate_length $domain_height 0)

    (0 $domain_height 0)

    (0 0 1)

    ($plate_length 0 1)

    ($plate_length $domain_height 1)

    (0 $domain_height 1)

    

    #codeStream

    {

        codeInclude

        #{

          #include "pointField.H"

        #};



        code

        #{

        

        label trenchNo =1;

        



        while (trenchNo <= $plate_length/($a+$b))

          //the total number of the grooves is equal to $plate_length/($a+$b)

        {

          os << point ((trenchNo-1)*($a+$b)+$a, 0, 0) << endl;

          os << point (trenchNo*($a+$b), 0, 0) << endl;

          os << point (trenchNo*($a+$b), -$c, 0) << endl;

          os << point ((trenchNo-1)*($a+$b)+$a, -$c, 0) << endl;

          os << point ((trenchNo-1)*($a+$b)+$a, 0, 1) << endl;

          os << point (trenchNo*($a+$b), 0, 1) << endl;

          os << point (trenchNo*($a+$b), -$c, 1) << endl;

          os << point ((trenchNo-1)*($a+$b)+$a, -$c, 1) << endl;



          ++trenchNo;

        }

        #};

    }



);





blocks

(

    hex (0 1 2 3 4 5 6 7) (100 100 1) simpleGrading (1 1 1)

    #codeStream

    {

        codeInclude

        #{

          #include "pointField.H"



        #};



        code

        #{

        

        label trenchNo = 1;

        

          

        while (trenchNo <= $plate_length/($a+$b)) //Here I want to create the block of each groove

        {



          label vertexNo {(trenchNo-1)*8 + 8};

          

         hex (vertexNo, vertexNo+1, vertexNo+2, vertexNo+3, vertexNo+4, vertexNo+5,  vertexNo+6, vertexNo+7) (10 10 1) simpleGrading (1 1 1) 





          ++trenchNo;



        }

        #};

    }



);

Once I execute the blockMesh, I receive the following error messages;

Code:

error: invalid initialization of reference of type ‘Foam::IOstream&’ from expression of type ‘Foam::label {aka int}’

In file included from /opt/openfoam6/src/OpenFOAM/lnInclude/Ostream.H:39:0,

                 from /opt/openfoam6/src/OpenFOAM/lnInclude/UILListIO.C:27,

                 from /opt/openfoam6/src/OpenFOAM/lnInclude/UILList.C:91,

                 from /opt/openfoam6/src/OpenFOAM/lnInclude/UILList.H:383,

                 from /opt/openfoam6/src/OpenFOAM/lnInclude/ILList.H:39,

                 from /opt/openfoam6/src/OpenFOAM/lnInclude/IDLList.H:35,

                 from /opt/openfoam6/src/OpenFOAM/lnInclude/entry.H:45,

                 from /opt/openfoam6/src/OpenFOAM/lnInclude/dictionary.H:53,

                 from codeStreamTemplate.C:29:

/opt/openfoam6/src/OpenFOAM/lnInclude/IOstream.H:565:18: note: in passing argument 1 of ‘Foam::IOstream& Foam::hex(Foam::IOstream&)’

 inline IOstream& hex(IOstream& io)

                  ^~~

/home/pooyanni/OpenFOAM/pooyanni-6/run/a1b1c1/system/blockMeshDict.#codeStream:101:107: error: expected ‘)’ before numeric constant

/opt/openfoam6/wmake/rules/General/transform:25: recipe for target 'Make/linux64GccDPInt32Opt/codeStreamTemplate.o' failed

make: *** [Make/linux64GccDPInt32Opt/codeStreamTemplate.o] Error 1





--> FOAM FATAL IO ERROR: 

Failed wmake "dynamicCode/_7bf46a550e1a99fa827dba743e26405dd82708a9/platforms/linux64GccDPInt32Opt/lib/libcodeStream_7bf46a550e1a99fa827dba743e26405dd82708a9.so"





file: /home/pooyanni/OpenFOAM/pooyanni-6/run/a1b1c1/system/blockMeshDict from line 17 to line 73.



    From function static void (* Foam::functionEntries::codeStream::getFunction(const Foam::dictionary&, const Foam::dictionary&))(Foam::Ostream&, const Foam::dictionary&)

    in file db/dictionary/functionEntries/codeStream/codeStream.C at line 218.



FOAM exiting

I would appreciate if anyone has any idea how I can create the blocks for my mesh in a while loop.:)