[ali]

Dear Hrv,

Thanks very much for your time. I didn't say there is something wrong with the code, I just wanted to know what I had done wrong in setting up the boundaries or patches etc. Now, I see my problem was that I expected the code to converge much sooner (the same oder of the basic case 0.5 sec).

So, the thing I learned here is that in cases that we have patch merging and stuff, it may result in run times much higher than the base case. Ok, now I got it, thank you again for teaching me this.

Best Regards.

[arno]

Is blockMesh limited to 4 GB of memory?

I ran into the same trouble, blockMesh simply crashes or is crashed by the OS, when I try to generate a mesh with 6 million cells. blockMesh works up to 3.7 Mcells, which translates into about 4 GB of memory required during the run. Beyond that, everything runs and then suddenly, there is just a message:

Killed

and no mesh nor error messages are generated.

The platform is LinuxAMD64Opt, i.e. 64-bit, so the memory limitation should not be in effect. However, is blockMesh maybe compiled as a 32-bit application nevertheless?


ArNO
2

PS: Could the list administrator check my account, since I get every message twice. This is probably due to my presence on this mailing list since the year 0 or 1. When I resubscribed in order to be able to send messages through this new web interface instead of e-mail, I get everything doubled since then.

[mattijs]

There is no limit in blockMesh.

Do an ldd on the blockMesh executable. Check which libraries it uses. Are they all 64 bit? Check with the 'file; command.

[arno]

Yes, they are all 64-bit.

However, there _is_ a limitation nevertheless: the amount of RAM + virtual memory on the machine, that runs blockMesh ;).

When it was running, I only looked a the amount of RAM it needed, not how much swap it also consumes. It turned out the machine in question has only 2 GB of swap + 4 GB of RAM and this was not enough to create a mesh with more than 3,7 million cells. The operating system shoots down processes trying to go past its max. virtual memory space, that's where the "Killed" came from.

The solution was to find another machine with more memory. Then it worked just as it should have and I got a mesh created.

BTW, this is actually a bit problematic, since meshing the problem takes much more memory than actually running it. This is because the run can be broken up to several CPU-nodes distributing also the memory requirements, while blockMesh is a single threaded application, that needs all the memory in one machine.

ArNO
2

[musahossein]

Gentlemen:

I am running the following block mesh file. It is a variation of the dambreak problem without the obstacle. However I get an error stating that 2 faces are missing.

Any suggestions will be appreciated.

The blockmesh output is:
*---------------------------------------------------------------------------*\
| ========= | |
| \ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \ / O peration | Version: 1.5 |
| \ / A nd | Web: http://www.OpenFOAM.org |
| \/ M anipulation | |
\*---------------------------------------------------------------------------*/
Exec : blockMesh
Date : Sep 24 2008
Time : 10:39:15
Host : linux-ip9p
PID : 3868
Case : /home/musa/OpenFOAM/musa-1.5/run/tutorials/interFoam/damBreaktest
nProcs : 1

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


Reading block mesh description dictionary

Creating block mesh

Creating blockCorners

Creating curved edges

Creating blocks

Creating patches

Creating block mesh topology

Default patch type set to empty
--> FOAM Warning :
From function polyMesh::polyMesh(... construct from shapes...)
in file meshes/polyMesh/polyMeshFromShapeMesh.C at line 576
Found 2 undefined faces in mesh; adding to default patch.

Check block mesh topology

Basic statistics
Number of internal faces : 0
Number of boundary faces : 6
Number of defined boundary faces : 6
Number of undefined boundary faces : 0

Checking patch -> block consistency

Creating block offsets

Creating merge list .

Creating points

Creating cells

Creating patches

Creating mesh from block mesh

Default patch type set to empty

Writing polyMesh

end

The input file is:

/*--------------------------------*- 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 0 0)
(14 0 0)
(14 0 0.1)
(0 0 0.1)
(0 10 0)
(14 10 0)
(14 10 0.1)
(0 10 0.1)
);

blocks
(
hex (0 1 5 4 3 2 6 7) (140 100 1) simpleGrading (1 1 1)
);

edges
(
);

patches
(
wall leftWall
(
(0 3 7 4)
)
wall rightWall
(
(1 2 6 5)
)

wall lowerwall
(
(0 1 2 3)
)

patch atmosphere
(
(4 5 6 7)
)
);

mergePatchPairs
(
);

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

[alexm]

is seems that you have forgotten to define the patches of the type "empty" for the front and back side of a 2 dimensional mesh.

Furthermore the numbering of the vertices is a little confusing. How OpenFOAM handles this, is described in the user manual:
http://www.opencfd.co.uk/openfoam/doc/blockMesh.html

OpenFOAM is very strict with numbers and directions of the entities.

Hope that helps.

Good night, Axel

[musahossein]

Axel:

Got it. Many thanks for your help.

Musa

I want to make simple model but I have some error in that


Creating block mesh topology
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary&)
in file createTopology.C at line 412
negative volume block : 0, probably defined inside-out


can someone help me?

thanks in advnace...

Emo

and my blockMeshDict file looks like

convertToMeters 1;

vertices
(
(0 -0.05 0)
(0 0 0.05)
(0 0.05 0)
(0 0 -0.05)
(1 -0.05 0)
(1 0 0.05)
(1 0.05 0)
(1 0 -0.05)
);

blocks
(
hex (0 1 2 3 4 5 6 7) (10 10 10) simpleGrading (1 1 1)

);

edges
(
arc 0 1 (0 -0.03536 0.03536)
arc 1 2 (0 0.03536 0.03536)
arc 2 3 (0 0.03536 -0.03536)
arc 3 0 (0 -0.03536 -0.03536)
arc 4 5 (1 -0.03536 0.03536)
arc 5 6 (1 0.03536 0.03536)
arc 6 7 (1 0.03536 -0.03536)
arc 7 4 (1 -0.03536 -0.03536)
);
patches

(
wall fixedWalls
(
(0 4 5 1)
(1 5 6 2)
(2 6 7 3)
(3 7 4 0)
)

patch inlet

(
(0 1 2 3)
)

patch outlet

(
(4 5 6 7)
)
);

mergePatchPairs
(
);

thanks again

Emo

can anybody help me?
I m quite new in OpenFoam

thanks

Emo

[mattijs]

Your point ordering is probably wrong. Have a look at the cavity tutorial and table 5.1 in the user guide.

thanks Mattijs

I have looked several times and rearrange it but it does not work...

Anyone can see the mistake...
I have to finish it till afternoon...
please help me

EMO

convertToMeters 1;

vertices
(
(-0.5 -0.05 0)
(-0.5 0 0.05)
(-0.5 0.05 0)
(-0.5 0 -0.05)
(0.5 -0.05 0)
(0.5 0 0.05)
(0.5 0.05 0)
(0.5 0 -0.05)
);

blocks
(
hex (0 1 2 3 4 5 6 7) (100 10 10) simpleGrading (1 1 1)

);

edges
(
arc 0 1 (-0.5 -0.03536 0.03536)
arc 1 2 (-0.5 0.03536 0.03536)
arc 2 3 (-0.5 0.03536 -0.03536)
arc 3 0 (-0.5 -0.03536 -0.03536)
arc 4 5 (0.5 -0.03536 0.03536)
arc 5 6 (0.5 0.03536 0.03536)
arc 6 7 (0.5 0.03536 -0.03536)
arc 7 4 (0.5 -0.03536 -0.03536)
);
patches

(
wall fixedWalls
(
(2 6 5 1)
(1 5 4 0)
(0 4 7 3)
(3 7 6 2)
)

patch inlet

(
(0 1 2 3)
)

patch outlet

(
(4 5 6 7)
)
);

mergePatchPairs
(
);
I have changed it like this but I had same warning like

Creating block mesh topology
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 0
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 1
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 2
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 3
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 4
--> FOAM Warning :
From function cellModel::mag(const labelList&, const pointField&)
in file meshes/meshShapes/cellModel/cellModel.C at line 134
zero or negative pyramid volume: -0.000833333 for face 5
--> FOAM Warning :
From function blockMesh::createTopology(IOdictionary&)
in file createTopology.C at line 412
negative volume block : 0, probably defined inside-out

please someone help me fixed this problem

thanks Emo

[gschaider]

Hi Emo!

I don't know for sure (I only checked the blockMesh with pyFoamDisplayBlockmesh, it looks topological OK there), but the problem might be that you're trying to build a tube with a single block, which distorts the cells on the "corners" quite heavily.
Try commenting out the arcs and rerun blockMesh. If it doesn't complain then that is surly the problem. Another way of finding the problem might be looking at the mesh in paraFoam (blockMesh issued only warnings, so it should habe produced a polyMesh.

But the best guess would be to make a 5-blocks mesh like it is described in
http://www.cfd-online.com/OpenFOAM_D...es/1/3249.html
The mesh quality is superior to anything you could achieve with your approach

Bernhard

thank you very much Bernhard...
I have change the fixed walls and it is OK now but after running parafoam I saw that only two blocks are meshed. the solver after a while stopping
what do you think I should do it with 4 blocks?

Thank you again

Emo

[cedric_duprat]

Hi Emilian,

Usually to mesh a pipe, we use 5 blocks.
You can find some example (and blockMeshDict) in the turbomachinery SIG : http://openfoamwiki.net/index.php/Si...nical_diffuser
I hope it will help,

Cedric

Thanks Cedic

[nandiganavishal]

[nandiganavishal]

The shape is the same.. but the dimensions are

2 Vertical blocks 1m * 1m and the horizontal block is 5m * 0.03 m