[agustinvo]

Hi all,


I am trying to run the airfoil case of Sebastiano Stipa using OpenFOAM v10, however when I run blockMesh I get an error related with the macro expansion:

Creating block mesh from 
    "system/blockMeshDict" 


--> FOAM FATAL IO ERROR:  
Illegal dictionary entry or environment variable name ":aerofoil.xUpper" 
Valid dictionary entries are 1(type)

As far as I know, there is a bug related to this (link), where they complain about the wrong indications at the User Guide. Nevertheless, I'm trying different configurations but I always get the same error.


I have run blockMesh successfully with OpenFOAM v7 so I suppose that something has changed on the Macro expansion declaration but it is not clear the new formulation.


Has someone found a solution or walkaround to this problem?


Regards
Agustín

[KasperWayne]

Take a look at the documentation for OF10 and you can see the difference :-)
https://doc.cfd.direct/openfoam/user...17-1320004.2.9

[agustinvo]

Well, that is actually the bug I linked in the first post. It is said that there are mistakes on the macro definition.


If you check in the OF v7 documentation the same section, you will see that the sole difference is the 'slash' introduction in OF v10, and after that the 'dot' formulation is always applied.


If the contents of the Macro Expansion are mostly, why can't I run it properly? If there are changes, they are not correctly indicated in the documentation.

[kakila]

I can confirm this. I have a set of parametrized files and they are not working anymore in OF10.
It seems that there is an undocumented change in the macro expansion.
Anybody knows what is this change?

Also the "/" (dot) in the documentation is also a bug. It is a dot or a slash? In OF10 it seems it is a slash https://bugs.openfoam.org/view.php?id=3877.


Update:
Form that bug: the dot notation is deprecated (not working in OF10).
Looking at the source code:https://cpp.openfoam.org/v10/diction...ce.html#l00897
I found that for the slash notation (what you need to use in OF10) the references to other levels also change (undocumented). so root level for slash notation is "!" not ":".
I cannot find whether the relative scopes (use of "..") are valid for the slash notation, it is not transparent from the source code.

[tniemi]

The new slash syntax is documented in this commit message: https://github.com/OpenFOAM/OpenFOAM...3519b0d187e485

The documentation for OF10 is not yet fully updated and a bit confusing.

The reason for this change was to add flexibility and eg. support easily referring to entries which contain a dot (typical for multiphase simulations).

It is still possible revert to using the old syntax, either globally by editing etc/controlDict or locally case by case.

[agustinvo]

Thank you! I have been busy with other bussiness but I have checked your comment and it works!

[moh raafat]

Originally Posted by agustinvo

Thank you! I have been busy with other bussiness but I have checked your comment and it works!

I have the same issue, and tried to modify the syntax but in vain, can you provide exactly the required modification to the file.

Thanks in advance

[tniemi]

I have not run the case, but I just checked and basically to run blockMesh, do the following changes:

$: -> $!
domain. -> domain/
aerofoil. -> aerofoil/

So for example
$:aerofoil.xUpper -> $!aerofoil/xUpper

and a bit longer snippet:

geometry
{
aerofoil
{
type triSurfaceMesh;
file "NACA0012.obj";
}
cylinder
{
type searchableCylinder;
point1 ($!aerofoil/xUpper -1e3 0);
point2 ($!aerofoil/xUpper 1e3 0);
radius $!domain/zMax;
}
}

vertices
(
project ($aerofoil/xLower -0.1 $domain/zMin) (cylinder)
($aerofoil/xTrail -0.1 $domain/zMin)
($domain/xMax -0.1 $domain/zMin)

[moh raafat]

thanks a lot, it works for blockeMesh, noting that the there other syntax errors for version s OF9 and OF10 included in the mentioned tutorials due to syntax changes, such as functions part in controlDict file, I will try generate the entire tutorial and make updates.