Dear OpenDX lovers, The new
 

Dear OpenDX lovers,

The new version of OpenDX has been out for a while and I have updated the OpenFOAM reader module to version 4.4.0. All works fine.

The only issue to report is that on Suse 10.1 I had to add -lssp to the link line in several places during the dx build. For more info or if you encounter problems, feel free to give me a shout.

Hrv

Hrv, can you send me some of y
 

Hrv, can you send me some of your .net files for glyphs and contours (preferably with the capability to use the sequencer for different time steps).

Thanks!

You can find my dx networks in
 

You can find my dx networks in a pack in:

http://powerlab.fsb.hr/ped/kturbo/OpenFOAM/misc/

Enjoy,

Hrv

Many thanks Hrv. Much apprecia
 

Many thanks Hrv. Much appreciated!

Hi Hrv, Can you post the dx
 

Hi Hrv,

Can you post the dxFoam sources that have been modified to work with OpenFOAM version 1.3. I'm having a hard time using paraFoam to visualize the grid when I merge patches whilst creating non-conformal meshes. I gather that dx displays the mesh exactly. Right?

Thanks http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Yes, correct: this is why I ke
 

Yes, correct: this is why I keep it alive. Attached, enjoy,

Hrv

http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif dxFoamExec_HJ_21Feb2007.tgz

Hi Hrv, Thanks for the sour
 

Hi Hrv,

Thanks for the source. I set DXROOT to /usr/local/dx and DXARCH to linux. Follow that with a 'wmake dxFoamExec' and it seems to work; except that I am stuck with this error message midway during compiling:

foamChangeTime.C: In function 'Error m_foamChangeTime(object**, object**)':
foamChangeTime.C:238: error: 'lagrangianSubDir' is not a member of 'Foam::Cloud<foam::passiveparticle>'
make: *** [Make/linuxAMD64Gcc4DPOpt/foamChangeTime.o] Error 1

Any hints?

Hi pUl|, I had the same probl
 

Hi pUl|,
I had the same problem, and Hrv's suggestion was:

For the moment, just put "lagrangian" instead of lagrangianSubDir.

, though I still could not compile it, so here is a small work around:

In order to complete the compilation I had to comment the lines involving the sprayObjects object (lines 234-254 in foamChangeTime.C). At least for the moment I'm not postprocessing particle tracks so it is OK.

I have a simple net example, that might help you in using the excelent reader dxFoamExec: http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif simple.net .

I hope this will be helpfull,
Dragos

Thanks Dragos! After commentin
 

Thanks Dragos! After commenting out those lines I was able to rebuild dxFoamExec. I then pulled out the dxFoam script from OpenFOAM 1.1 and put it back in 1.3. Now I can view the non-conformal mesh the way it was intended! Oh, and I had to rebuild OpenDX with the --with-shared option when running the configure script.

One question however remains: If indeed the two patches in the mesh are merged using polyhedral cells, why does checkMesh report non-orthogonality and skewness when there should be none?

Excerpt from checkMesh:

Mesh non-orthogonality Max: 40.6013 average: 4.5195
Non-orthogonality check OK.

Face pyramids OK.

Max skewness = 8.83042 percent. Face skewness OK.

Minumum edge length = 0.000714286. Maximum edge length = 0.01.

All angles in faces are convex or less than 10 degrees concave.

Face flatness (1 = flat, 0 = butterfly) : average = 1 min = 1
All faces are flat in that the ratio between projected and actual area is > 0.8

Geometry check done.

Number of cells by type:
hexahedra: 865
prisms: 0
wedges: 0
pyramids: 0
tet wedges: 0
tetrahedra: 0
polyhedra: 35
Number of regions: 1 (OK).
Mesh OK.

A visual picture of the mesh from OpenDX is available here:

http://www.ualberta.ca/~madhavan/image.png

Oh, and one more thing How do
 

Oh, and one more thing How do I use your simple.net. Just running dxFoamExec leaves me at some kind of OpenDX shell prompt. Any hints on how to proceed?

The simplest way to use simple
 

The simplest way to use simple.net is to place it in ~/OpenFOAM/OpenFOAM-1.3/.OpenFOAM-1.3/apps/dxFoam/networks and then run

dxFoam simple

I hope you'll like it!

Dragos

Hi pUl|, How did you construc
 

Hi pUl|,
How did you constructed that mesh? It seems that you successfully converted a "hanging nodes" mesh.

Dragos

I will post the blockMeshDict
 

I will post the blockMeshDict in a few minutes.

Here it is: Actually I foun
 

Here it is:

Actually I found it on this forum some time back http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

/*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.0 |
| \ / A nd | Web: http://www.openfoam.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/

FoamFile
{
version 2.0;
format ascii;

root "";
case "";
instance "";
local "";

class dictionary;
object blockMeshDict;
}

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


convertToMeters 0.1;

vertices
(
// Back plane
(0 0 0)
(0.5 0 0)
(0.5 0 0)
(1 0 0)
(0 1 0)
(0.5 1 0)
(0.5 1 0)
(1 1 0)

// Front plane
(0 0 0.1)
(0.5 0 0.1)
(0.5 0 0.1)
(1 0 0.1)
(0 1 0.1)
(0.5 1 0.1)
(0.5 1 0.1)
(1 1 0.1)
);

blocks
(
hex (0 1 5 4 8 9 13 12) (20 35 1) simpleGrading (1 1 1)
hex (2 3 7 6 10 11 15 14) (10 20 1) simpleGrading (1 1 1)
);

edges
(
);

patches
(
wall bottom
(
(0 1 9 8)
(2 3 11 10)
)
wall top
(
(4 12 13 5)
(6 14 15 7)
)
wall left
(
(0 8 12 4)
)
wall right
(
(3 7 15 11)
)

patch leftMerge
(
(1 5 13 9)
)
patch rightMerge
(
(2 10 14 6)
)

);

mergePatchPairs
(
( leftMerge rightMerge )
);


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

Heya, Basically, checkMesh
 

Heya,

Basically, checkMesh reports the non-orthogonality and skewness on the mesh because the faces are skew and non-orthogonal. Look at the mesh connected with merge patch pairs and tell me if:

- is the line connecting two cell centres across the merged patches normal to the face? It is not, which represents mesh non-orthogonality

- does the line connecting two cell centres across the merged patches go through the centre of the face? It does not, which represents skewness.

Remember, the cells lert and right are now truly polygons (in 2-D) and not some cooked up hexes like in some other codes I won't mention.

Hope that's clear,

Hrv

Thanks for that really enlight
 

Thanks for that really enlightening explanation Hrv. It all makes sense now. Really appreciate your help http://www.cfd-online.com/OpenFOAM_D...part/happy.gif

Oh, and one more thing. The ca
 

Oh, and one more thing. The case seems to run fine even without any non-orthogonal correctors. Why is that?

Could someone explain to me in
 

Could someone explain to me in 2 or 3 lines how openDX should be started / used.

I compiled the last dxFoamExec and I use the networks from prof. Jasak's site. Furthermore I start opendx by just typing: dxFoam in the run dir.

1) First I get three warnings from postFoam.net (unrecognized comments (ignored)).

2) I am able to load cases and visualise stuff, but at every button I click the editor for postFoam.net is opened. Why should I want that??

3) How can I change views and/or zoom in/out or pan inside the windows (which shows the mesh/solution) I cant find a manual, unless you pay for it.

Mostly I use Tecplot, but I am just curious about OpenDX.

Regards, Frank

I can answer some of your quer
 

I can answer some of your queries:

For instance:

How can I change views and/or zoom in/out or pan inside the windows (which shows the mesh/solution) I cant find a manual, unless you pay for it.

In the Image Window, Search for Options -> View Control. Basically everything you need should be in the Options Menu.

And look here (/usr/local/dx/html) for complete documentation.

Hi Frank, I also started with
 

Hi Frank,
I also started with Tecplot, but after that I was forced to use OpenDX (licensing reasons). At start I was confused and I thought it is very hard to use compared to Tecplot, but no longer.
You can find a very comprehensive documentation, incuding a search engine at: OpenDX official documentation. It also includes the manuals in pdf format if you want to print them.
Anyway, if you are a begginer, you may try the simple.net that I placed above. It surely does not have the complexity of postFoam.net but it is much easy-er to be digested by a begginer.

Basically what you have to do is:
1.

cp simple.net ~/OpenFOAM/OpenFOAM-1.3/.OpenFOAM-1.3/apps/dxFoam/networks

2.

cd to_the_root_of_your_case

3.

dxFoam simple

It will load the first case found in that directory. If you have more, you will be able to change the case name from a drop down list, later on.

This is a short introduction, and in no way complete, but I hope it will help you.

Dragos