[bhperfect]

This one's a two-parter:

First, the implementation. In the definitions section in blockMeshDict, I want to define and discretize the domain. So I define

>back -600;
>front 250;

Cool. Now, I'd like to define the number of grid cells along this dimension. Previously I had been doing

>nx 40;

But now I'm playing around with changing the domain size. I would like to be able to say something like,

>nx floor((front-back)/8);

How can I accomplish this? OpenFOAM gets angry at me whenever I try to insert a math expression.

Now, for the second part:

I can't find any information about how these FoamFile definitions are stored. Do they stay local to whatever application calls the file that it's in, or could I, for example, define all of my parameters that might change in my executable file? Going with the same example as above, is there a way to define 'front' and 'back' in my executable so that I only have to edit one file every time I do a run?

[alexeym]

Hi,

You know, you can search forums:

http://www.cfd-online.com/Forums/ope...constants.html

http://www.cfd-online.com/Forums/ope...variables.html

http://www.cfd-online.com/Forums/ope...kmeshdict.html

Also you can use grep:

$ cd $FOAM_TUTORIALS
$ grep -r '#calc' *
incompressible/simpleFoam/pipeCyclic/constant/polyMesh/blockMeshDict:radHalfAngle    #calc "degToRad($halfAngle)";
incompressible/simpleFoam/pipeCyclic/constant/polyMesh/blockMeshDict:y               #calc "$radius*sin($radHalfAngle)";
incompressible/simpleFoam/pipeCyclic/constant/polyMesh/blockMeshDict:minY            #calc "-1.0*$y";
incompressible/simpleFoam/pipeCyclic/constant/polyMesh/blockMeshDict:z               #calc "$radius*cos($radHalfAngle)";
incompressible/simpleFoam/pipeCyclic/constant/polyMesh/blockMeshDict:minZ            #calc "-1.0*$z";
multiphase/interDyMFoam/ras/floatingObject/constant/dynamicMeshDict:    mass            #calc "$rho*$Lx*$Ly*$Lz";

And finally, you can generate blockMeshDict using whatever language you know. Since #calc is just convenience wrapper around C++.

[bhperfect]

FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 1;
back -600;
front 250;
side -215;
z1 -40;
//40m depth permits waves up to 80m long to propagate as deep water waves
z2 3.87;
z3 5.87;
z4 50;
hsize 8;
vsize 6;

nx #calc "std::ceil(($front-$back)/$hsize)";
#calc "Info<< $nx << endl"
ny #calc "std::ceil(-$side/$hsize)";

when run, this yields

/*---------------------------------------------------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.0                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
Build  : 2.3.0-f5222ca19ce6
Exec   : blockMesh
Date   : Jan 21 2016
Time   : 14:30:39
Host   : "fourier"
PID    : 17214
Case   : /home/bperfect/OpenFOAM/bperfect-2.3.0/run/small
nProcs : 1
sigFpe : Enabling floating point exception trapping (FOAM_SIGFPE).
fileModificationChecking : Monitoring run-time modified files using timeStampMaster
allowSystemOperations : Allowing user-supplied system call operations

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

Creating block mesh from
    "/home/bperfect/OpenFOAM/bperfect-2.3.0/run/small/constant/polyMesh/blockMeshDict"
Using #calcEntry at line 29 in file "/home/bperfect/OpenFOAM/bperfect-2.3.0/run/small/constant/polyMesh/blockMeshDict"
Using #codeStream with "/home/bperfect/OpenFOAM/bperfect-2.3.0/run/small/dynamicCode/platforms/linux64GccDPOpt/lib/libcodeStream_d8e5566d16e6b658bc2352d18ed09d52db601d72.so"
Invoking "wmake -s libso /home/bperfect/OpenFOAM/bperfect-2.3.0/run/small/dynamicCode/_d8e5566d16e6b658bc2352d18ed09d52db601d72"
: In function ‘void Foam::codeStream_d8e5566d16e6b658bc2352d18ed09d52db601d72(Foam::Ostream&, const Foam::dictionary&)’:
:1:22: error: lvalue required as decrement operand
:1:24: error: expected ‘)’ before numeric constant
:1:32: error: expected ‘)’ before ‘;’ token
make: *** [Make/linux64GccDPOpt/codeStreamTemplate.o] Error 1


--> FOAM FATAL IO ERROR: 
Failed wmake "dynamicCode/_d8e5566d16e6b658bc2352d18ed09d52db601d72/platforms/linux64GccDPOpt/lib/libcodeStream_d8e5566d16e6b658bc2352d18ed09d52db601d72.so"


file: /home/bperfect/OpenFOAM/bperfect-2.3.0/run/small/constant/polyMesh/blockMeshDict from line 17 to line 26.

    From function functionEntries::codeStream::execute(..)
    in file db/dictionary/functionEntries/codeStream/codeStream.C at line 177.

FOAM exiting

So, it looks like I was able to make it understand my #calc calls, but now everything else defined in the dictionary is failing. Do you know how I might fix this?

[alexeym]

Hi,

Though strictly speaking it is just shitty Gcc diagnostics, but try to control your expansions. Here is clang output:

  [CC] codeStreamTemplate.C
:1:22: error: expression is not assignable
os << (std::ceil((250--600)/8));
                  ~~~^
1 error generated.
make: *** [Make/darwin64ClangDPInt64Opt/codeStreamTemplate.o] Error 1

As you can see, your $front-$back was expanded into 250--600, which is not quite valid C++ expression. Use brackets. Or spaces ($front - $back). -$side is also expanded into --215.