Hello!

I want to creata a mesh that is described by a area (lets say in x-y plane) and then extruded in the z direction because it is uniform in with hight.

I have created the 2D mesh in gmsh (.msh ending) and I'm presently trying to transfer it to OpenFOAM. I dont know whether I should extrude it first with the Openfoam command or if I have to convert it first with gmshToFoam command and then try to extrude it.

Either way I get Error messages.

Does anyone have an idea of how to create a mesh in this manner?

Thanks
/Erik

[mattijs]

You probably want to do the extrusion in gmsh itself. The gmshToFoam converter only converts 3D meshes.

Thanks for the hint!

When I try to extrude my 2D mesh in gmsh I want to form prism and hexahedral cells, but it wont extrude the mesh, only the "geometrical configuration".

/Erik

Do you know if I can convert my 2D mesh to OpenFOAM- format and then extrude it as an alternative method?

/Erik

[mattijs]

Use extrudeMesh on an existing mesh with the -sourcePatch -sourceRoot -sourceCase arguments. Check the surface file it writes. Is a very simple format you can easily write a converter to from another meshing program. Then use extrudeMesh with the -surface option to extrude from that surface file.

Would be nice if you could post your steps & solution over here.

Thank you

Ok I will do that once I get it to work.

Im trying to extrude icoFoam/cavity, but since the command extrudeMesh only expects 4 arguments I can only write:

target root
target case
number of layers
overall thickness

And with the execution of only this arguments it complaints about the missing root, case and patch ofcourse.

A second question concerning this is how the sourcePatch should be defined in the case above with openfoam. Should it perhaps be named:
"empty FrontAndBack"

[mattijs]

Is this a question? The error message I get is

--> FOAM FATAL ERROR : Need to specify either -sourceRoot/Case/Patch or -surface option to specify the source of the patch to extrude

and if I type 'extrudeMesh' without any arguments to see all possibilities I see it has -sourceRoot, -sourceCase and -sourcePatch arguments which is exactly all the data it requires (root+case gives a mesh, patch gives the faces to extrude). The source root/case does not have to be the same as the destination root/case.

I managed to get past that problem.

The way I got it go work was by having the source and destination root/cases diferent from eachother.

I tried first to handle the problem in FoamX but got an error message as soon as I entered the -sourceCase.
It said something like rootAndCase file can not be split up to root directory and case file.

But now Im past that.

Thank You!

Hello!

Ive managed to get the format in which OpenFOAM describes an meshed surface as explained to me above. Now im trying to extrude a 2D mesh surface of my own choosing with this format.

I use the etrude command with arguments:
-layers
-thickness
-surface to be extruded(with .sMesh ending)

When using this arguments I get the following error message:

Exec : extrudeMesh /home/erik/OpenFOAM/erik-1.3/run/tutorials/icoFoam cavity 3 5.0 -surface surface.sMesh
Date : Apr 04 2006
Time : 10:14:29
Host : compadre
PID : 8496
Root :
Case :
Nprocs : 1
Target: "/home/erik/OpenFOAM/erik-1.3/run/tutorials/icoFoam" "cavity"
Extruding layers:
number of layers 3
overall thickness 5

Create time

Extruding surfaceMesh read from file "surface.sMesh"

Read patch from file "surface.sMesh":
points : 82
faces : 108



--> FOAM FATAL ERROR : Error in face ordering: mixed used and unused faces at the end of face list.
Number of used faces: 842 and face 874 is owned by cell 88

From function void polyMesh::initMesh(cellList& c) const
in file meshes/polyMesh/polyMeshCalcFaceCells.C at line 266.

FOAM aborting

Foam::error::printStack(Foam:stream&)
Foam::error::abort()
Foam::polyMesh::initMesh(Foam::List<foam::cell>&)
Foam::polyMesh::polyMesh(Foam::IOobject const&, Foam::Field<foam::vector<double> > const&, Foam::List<foam::face> const&, Foam::List<foam::cell> const&)
extrudeMesh [0x805ce57]
Foam::polyMesh::readUpdate()
__libc_start_main
__gxx_personality_v0


Could anybody please tell me what to do to correct this error.

Thanks
/Erik

Sorry for my frequent messaging.

I had a mesh (surface.sMesh) consisting of elements with both 2 and 4 nods.

Since 2 nods cant make up an element I tried to delete these. I got rid of the error message but the figure in paraview looks vary messed up and nothing in resemblance with the mesh I made in gmsh.

question:
Was the 2 nod elements necessary, or what should I do to extrude my 2D mesh correctly?

/Erik

[mattijs]

You've tried the extruding from a patch I assume ? (-sourceXXX options).

Can you use the .sMesh file this writes as a -surface argument correctly? (i.e. does extrudeMesh work)

My guess is that the sMesh file has to have the vertices numbered compactly so starting from 0 and no gaps. Maybe gmsh has options for what to export?

I chose to extrude the movingWall patch in the cavity case with the source- arguments entered.

Then I got a file caled movingWall.sMesh which looks like this:

42
(
(0 0.1 0)
(0.005 0.1 0)
(0.01 0.1 0)
....and so on...
)


20
(
4(0 21 22 1)
4(1 22 23 2)
4(2 23 24 3)
....and so on...
)

This should be nodes (42) and elements (20) probably in correct order but without indexnumbers.

I altered my 2D mesh to have this format (thru spread sheet program) and removing 2 nod elements. After that I extruded it using the surface- argument (.sMesh ending). This gave a totaly messed up picture in parafoam.

I will now look into what you said about certain orderig of nodes and elements

And yes, the movingWall looked ok when I extruded it using surface argument

Thank you Mattijs for all your help trying to convert the 2D mesh from gmsh.

I have now found a way to extrude both the geometry and my mesh simultaneous im gmsh. So now Im on the road again.

I still dont know what I did wrong when trying to extrude the 2D mesh from gmsh (when alterd in same format as in openfoam)

But Im leaving that subject now.

Thanks
/Erik

[mattijs]

Shame that you did not find a way to do the extrusion in OF. Could you post your gmsh solution?

=)

It was an easy solution. The function extrude had two extra (alternative) argument i.e. -Layers and -Recombine-

If only Surface is difined below then only the geometry will be extruded. The Recombine argument recombines the cells in the direction of the extrudsion, so that thay have the same cross section area at their topp as their bottom i.e. rods not pyramids.

my entre of the command extrude:

Extrude {0,0,50} {
Surface{19}; Layers{ {1}, {1}, {1} }; Recombine;
}
---------------------------------------
entry explanation:


Extrude { expression-list } { extrude-list layers }
Extrudes both the geometry and the mesh using a translation (see section 3.1.5 Extrusions). The layers option determines how the mesh is extruded and has the following syntax:

layers:
Layers { { expression-list }, <{>
{ expression-list } } | Recombine; ...

The first expression-list defines how many elements should be created in each extruded layer. The (optional) second expression-list assigns a region number to each layer, which, if non-zero, overrides the elementary entity number of the extruded entity. This is useful when there is more than one layer, as the elements in each layer can then be identified in a unique way. If the region number is set to zero, or if the expression-list is omitted, the elements are associated with the automatically created elementary geometrical entity (line, surface or volume) created during the extrusion. The last expression-list gives the normalized height of each layer (the list should contain a sequence of n numbers 0 < h1 < h2 < ... < hn <= 1). See 7.3 `t3.geo', for an example.

For line extrusions, the Recombine option will recombine triangles into quadrangles when possible. For surface extrusions, the Recombine option will recombine tetrahedra into prisms, hexahedra or pyramids.

---------------------------------------
This was maybe a bit to thorough.

/Erik

Hi,

I am tring play with tutorial (cavity). When I started paraFoam I get this error:

--> FOAM FATAL ERROR : Cannot find file "points" in directory "constant/polyMesh"

Could you help me?

Best regards,
Margarita

[dmoroian]

You have to run blockMesh first! This will generate the actual mesh, including the "points" file.

Dragos

[louisgag]

I successfully imported a "virtual 2D" mesh using gmshToFoam into OpenFOAM 1.5. The trick I had to perform was to use the Layers and Recombine options of the extrude function in Gmsh (see Gmsh documentation). I was also able to choose between extruded rectangle or triangle meshes; both successfully ran into OF icoFoam and Paraview.

[kawikablyth]

Hey thanks to "newbee" up there for the insight on the gmsh extrude command. Big help with my 2D case.