[babakflame]

Dear Foamers

My problem seems easy, however I can not solve it (till now at least).

I want to grid a space between to converging plates.

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  1.5                                   |
|   \\  /    A nd           | Web:      http://www.OpenFOAM.org               |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.01;

vertices        
(
/*  (-0.5 -0.5 -0.01)
    (0.5 -0.5 -0.01)
    (0.5 0.5 -0.01)
    (-0.5 0.5 -0.01)
    (-0.5 -0.5 0.01)
    (0.5 -0.5 0.01)
    (0.5 0.5 0.01)
    (-0.5 0.5 0.01)
*/
    (0      5  0.1)//0
    (0      0  0.1)//1
    (0.25 0  0.1)//2
    (1    5  0.1)//3
    (0    5 -0.1)//4
    (0    0 -0.1)//5
    (0.25 0 -0.1)//6
    (0.25 5 -0.1)//7
  

);

blocks          
(
    hex (0 1 2 3 4 5 6 7) (300 30 1) simpleGrading (1 1 1)
);

edges           
(
);
boundary
(
    INLET
    {
        type patch;
        faces
        (
            (0 3 7 4)
        );
    }
    front
    {
        type empty;
        faces
        (
            (0 1 2 3)
        );
    }
    back
    {
        type empty;
        faces
        (
            (4 5 6 7)
        );
    }
    OUTLET
    {
        type patch;
        faces
        (
            (1 2 6 5)
        );
    }
    Electrode
    {
        type wall;
        faces
        (
            (0 4 5 1)
            
        );
    }
     WALL
    {
        type wall;
        faces
        (
            (3 7 6 2)
        );
    }
);

mergePatchPairs
(
);

// ************************************************************************* //

how can I get rid of this skewed lines in this grid?
I just want straight lines that create a structured grid.

[avila.vc]

Hi,

Maybe I'm reaching here, but have you sliced a plan of your mesh for this printscreen? If so, could you show the original mesh?

Also, could you post a printscreen of the whole paraview window? so we can take a look at the configurations

edit:
obs: point 3 isnt supposed to be 0.25 5 0.1?

(0 5 0.1)//0
(0 0 0.1)//1
(0.25 0 0.1)//2
(1 5 0.1)//3
(0 5 -0.1)//4
(0 0 -0.1)//5
(0.25 0 -0.1)//6
(0.25 5 -0.1)//7

[babakflame]

Hi,

Thanks for your reply.
Yeah, this is a slice.

I have attached a screen shot of paraview.

My wondering is the presence of skewed lines? how this happnes?

[avila.vc]

When you slice you get triangles. It is just a viewing issue.

"People usually tend to use the filters Slice and Clip to diagnose the interior mesh of a case. Although it's an idea in the right direction (wanting to look inside the mesh), it will not give you the best results for assessing if the mesh is OK or not. This is because these filters require that the polyhedral cells in the mesh be decomposed to tetrahedral cells and the resulting surfaces will all be composed by triangles."

https://openfoamwiki.net/index.php/FAQ/Postprocessing

[babakflame]

thanks for your nice reply.

I hope that its the issue. I am going to read this page.

Regards

[babakflame]

I tried to use "Extract cells by region", However it was not clear for the settings required to see a slice of the grid with this filter.

This is a picture of my paraview screen shot, can you help me with hints?
I can send my case as well.

I uploaded it.
Regards

[avila.vc]

How I do it, step-by-step:

1-select "Use VTKPolyhedron"
2-extract the cells by region
3-select "Extract only intersected" and "Extract intersected"
4-Apply.

Any problems, send a printscreen of paraview, specially the properties bar options on the left

Obs: There was no image attached on your last post

[babakflame]

Originally Posted by avila.vc

How I do it, step-by-step:

1-select "Use VTKPolyhedron"
2-extract the cells by region
3-select "Extract only intersected" and "Extract intersected"
4-Apply.

Any problems, send a printscreen of paraview, specially the properties bar options on the left

Obs: There was no image attached on your last post

Hi
where is the location of "Use VTKPolyhedron"
My paraview version is 3.12.
Does it related to version?
I can not see it.

[avila.vc]

Hi Bobi, if you managed to use extract cells it was probably already selected.

Anyway, it is right above mesh parts (on your "initialSimulation" mesh), like the pictures at the link I gave you show.

Try now
3-select "Extract only intersected" and "Extract intersected" (the last boxes on the left menu on your last printscreen)
4-Apply

It should work.

[babakflame]

Hi Vinicius

I found it. However, still can not visualize the grid in a way to show a slice of it. It gives me nothing. As the last picture I uploaded in previous post.
I want to have a picture showing that my grid is a rectangular-type structured grid.

I learned from your link that what I receive is an illusion due to slice filter that we should use "Extract cells by region" filter. However, this new filter gives me nothing.

[avila.vc]

Hi. I think I got it. You must have your initialsimulation selected when extracting cells. Then it will be deselected automatcally when the extracted cells are generated. Post prints of your steps if you still dont manage to do it.

Select wireframe to visualize also.
Are you managing to visualize the original mesh, with inlet, outlet etc?

Take a better look até that link too.. Maybe there is something that we are not noticing with your case

[avila.vc]

I tested what I said here with a tutorial. It worked Just fine. (same paraview version). You are accessing paraview with paraFoam command right?

Sorry I could not help more. If you get me your printscreens with the steps you are following I might have some other idea.

Best luck.

[babakflame]

Just one thing:

Is the mesh representation by "Extract Cells by Region" filter is 3D or 2D?

From the provided link, it seems that it is 3D; however, for showing that my grid is rectangular-typed, I need a 2D pic (or slice) anyway.

A 3D visualization does not help.


Regards

[avila.vc]

Hi

with step 3-select "Extract only intersected" and "Extract intersected", you get a slice of the mesh with one cell size thickness

[Tobi]

Hi all, hi bobi,

I was in vacation; so I am sorry for delay (:
If you make slice or clip you should deselect the "split polyhedrals", its left in the options of the slice or clip.

I did not read all posts due to the fact that there are so many messages I have to replay.

Cheers

[babakflame]

Thanks Bro.

You are always helpful.

Regards

[Tobi]

So was it your solution? Or you had it already?

[Tobi]

Just to complete this topic.

You also can visual your cells in several ways.
For example you can use threshold for the coordsX and set the threshold to the limit you need.

Further more you can use a slice and select "Crinkle slice"
The method I mentioned above is called "Triangulate the slice" you should de-select this option.

And at last, "decompose polyhedrals". You find this option in the properties tree for your loaded case.