[krikre]

Hello!

I'm sharing an alternative to the makeAxialMesh utility. It should be easier to use and understand and should work on OF-3, OF-4 and OF-5.

https://github.com/krebeljk/wedgePlease

The Y axis is assumed as the axis of rotation for the initial 2D mesh in the XY-plane. There is no dictionary needed. Just run

wedgePlease -angle 5

It's based on the flattenMesh utility which comes with OpenFOAM. It was developed on OpenFOAM-3.0.1 but it should work on OF-4 and OF-5 because the flattenMesh.C looks the same in the current OpenFOAM-dev repository.

Two examples are provided:

• blockMesh
• fluentMeshToFoam

The examples were modified from the makeAxialMesh (a thanks the authors!).

The handling of the collapsed faces is done in the provided Allmesh scripts (same as with the makeAxialMesh). There is also a simple call to the createPatch utility in the provided examples to remove the patch named axis which is left with no faces after the conversion.

Because this is a simlpe makeAxialMesh, expect the same problems and solutions as with makeAxialMesh.

Press like if it helps!

Let me know if you find any mistakes or if you have improvement suggestions!

[mkhm]

I have the following error when I run the command ./Allmesh in caseBM:

Create time

Create mesh for time = 0

// using new solver syntax:
p
{
    solver          PCG;
    preconditioner  DIC;
    tolerance       1e-06;
    relTol          0;
}

// using new solver syntax:
U
{
    solver          PBiCG;
    preconditioner  DILU;
    tolerance       1e-05;
    relTol          0;
}

Read dictionary changeDictionaryDict.toWedge with replacements for dictionaries 1(dictionaryReplacement)
Reading polyMesh/boundary file to extract patch names
Loaded dictionary boundary with entries 
4
(
axis
wedge_pos
wedge_neg
walls
)

Replacing entries in dictionary dictionaryReplacement
Loading dictionary dictionaryReplacement


--> FOAM FATAL IO ERROR: 
cannot find file

file: /home/Axisym/wedgePlease-master/caseBM/constant/polyMesh/dictionaryReplacement at line 0.

    From function regIOobject::readStream()
    in file db/regIOobject/regIOobjectRead.C at line 72.

FOAM exiting

Could you help with that ? I ran the wedgePlease successfully.

[krikre]

I updated the repository. Clone it and see if it works.


Seems the changeDictionaryDict utility was removed at least in OF6 if not earlier. I replaced it with the foamDictionary utility. Also did some cleanup.

[mkhm]

Originally Posted by krikre

I updated the repository. Clone it and see if it works.


Seems the changeDictionaryDict utility was removed at least in OF6 if not earlier. I replaced it with the foamDictionary utility. Also did some cleanup.

I download it but still I have an error (another one). I attach the log file below. Thanks for your help.

[krikre]

I think you forgot the attachment.

[mkhm]

Originally Posted by krikre

I think you forgot the attachment.

Sorry, just add it.

[krikre]

Two patches named 'wedge_pos' and 'wedge_neg' need to have the type wedge. The problem is that the switch to type wedge is failing in OF4 for some reason. I'd say the OF4 foamDictionary isnt finding the entry0. I can't get my hands on an OF4 installation right now so I can't solve this for you.



I think you could solve this one by switching to OF7. If you can't do that you can do the step that is failing by manually editing the constant/polyMesh/boundary file. You could also find a way to script this in OF4.


I'll get back at you if test this in OF4.

[krikre]

Ok, you can clone again and git-checkout the of4 branch.


OF4 doesn't use the dictionaryReplacement keyword in dict for the changeDictionary utility. I removed that and it ran fine.

[mkhm]

Originally Posted by krikre

Ok, you can clone again and git-checkout the of4 branch.


OF4 doesn't use the dictionaryReplacement keyword in dict for the changeDictionary utility. I removed that and it ran fine.

Are you sure that you upedated github with the new version ? I still have the same errors:

--> FOAM Warning : 
    From function entry::getKeyword(keyType&, Istream&)
    in file db/dictionary/entry/entryIO.C at line 80
    Reading constant/polyMesh/boundary
    found on line 18 the label 4
    expected either } or EOF


--> FOAM FATAL IO ERROR: 
keyword entry0 is undefined in dictionary "" or is not a dictionary
Valid keywords are 1(FoamFile)

file:  from line 10 to line 14.

    From function void setScoped(Foam::dictionary&, const Foam::word&, bool, Foam::entry*)
    in file foamDictionary.C at line 224.

FOAM exiting

--> FOAM Warning : 
    From function entry::getKeyword(keyType&, Istream&)
    in file db/dictionary/entry/entryIO.C at line 80
    Reading constant/polyMesh/boundary
    found on line 18 the label 4
    expected either } or EOF


--> FOAM FATAL IO ERROR: 
keyword entry0 is undefined in dictionary "" or is not a dictionary
Valid keywords are 1(FoamFile)

file:  from line 10 to line 14.

    From function void setScoped(Foam::dictionary&, const Foam::word&, bool, Foam::entry*)
    in file foamDictionary.C at line 224.

FOAM exiting

[krikre]

You need to go to the of4 branch.


https://github.com/krebeljk/wedgePlease/tree/of4


I only changed the blockMesh case. In case you want to run the fluent mesh case you just make the same change to the system/changeDictionaryDict.toWedge. Remove that
dictionaryReplacement dictionary.

[mkhm]

Originally Posted by krikre

You need to go to the of4 branch.


https://github.com/krebeljk/wedgePlease/tree/of4


I only changed the blockMesh case. In case you want to run the fluent mesh case you just make the same change to the system/changeDictionaryDict.toWedge. Remove that
dictionaryReplacement dictionary.

Thanks. Now, it works properly.

[mkhm]

Dear Kristjan,

The mesh was created successfully. However, I've a question for the case where the axis of symmetry is not the y axis but the x axis. Does that require to change the source code or is there any trick to do it with you your original code ?

Thanks for your reply

[mkhm]

I modified the source code as follows:

forAll(points, pointI)
        {
            if (points[pointI].component(vector::Z) < midPoint.component(vector::Z))
            {
                points[pointI].replace(vector::Z, -sinus*points[pointI].component(vector::Y));//first use old x as radius
                points[pointI].replace(vector::Y, cosinus*points[pointI].component(vector::Y));//then change x
            }
            else
            {
                points[pointI].replace(vector::Z, sinus*points[pointI].component(vector::Y));
                points[pointI].replace(vector::Y, cosinus*points[pointI].component(vector::Y));
            }
        }

Basically, replace X by Y. The utility makes the mesh as what I expected.