CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM (http://www.cfd-online.com/Forums/openfoam/)
-   -   *.msh conversion + axissymetric problem (http://www.cfd-online.com/Forums/openfoam/78132-msh-conversion-axissymetric-problem.html)

bruxellois4 July 13, 2010 18:19

*.msh conversion + axissymetric problem
 
Hi everybody!!

I've converted a mesh (*.msh), it is an axissymetric problem (a barrel of a gun) but now after conversion i'm not sure that's a an axissymetric problem yet!!

The wedge explanation on the user guide is not clear!!

you can see my boundary file here http://www.4shared.com/file/nSG5aXjl/boundary.html

How can I define a 2D an axissymetric problem, i have to define my symmetry axis (revolution axis) as a wedge? If yes how can i do it?

Is there a tutorial case with an 2D axissymetric problem?

Best regards!!

wyldckat July 13, 2010 18:50

Greetings Abdel,

I've been remembering about your posts about this, but never found the time again to try to answer them. Additionally, I have literally no experience in axisymetric cases, so that was another reason for not replying sooner :(.

But since you opened a another thread, I remembered to search in the usual places:
  1. In openfoamwiki.net: http://openfoamwiki.net/index.php/Ma...s/AxiSymmetric
  2. To search for text in files (I google'd it ;)), simply go to the tutorials folder in a terminal and run this command line:
    Code:

    find . | xargs grep 'wedge' -sl
    You can also try inside the applications folder of OpenFOAM, because sometimes there are pearls of wisdom in them!
  3. Just two hours ago, this thread was updated about 3D axissymetry: http://www.cfd-online.com/Forums/ope...c-problem.html
  4. Using the advanced search mode in this forum, searching for "axisymmetric" (note only one 's') and in OpenFOAM forums only, it gave me 15 threads that talk about it!
Good luck! Best regards,
Bruno

bruxellois4 July 13, 2010 19:37

Thanks Bruno for your response hope that can help me!!

marcbest July 14, 2010 03:30

hi bruxellois4,

think you can not copy the fluent axissymetry-mesh directly to openfoam as a wedge mesh. either you create a new mesh with blockMesh or (i've never tried this) you create a mesh in gabit with the following rules (page 18)

http://projekter.aau.dk/projekter/fi...784/Report.pdf

i hope this helps

PS: in this report has some other interesting information

phsieh2005 July 14, 2010 07:41

Hi,

Someone developed an utility called makeAxialMesh for OpenFOAM. It will convert a 2D mesh to an axi-symmetric mesh. Search makeAxialMesh on OpenFOAM wiki. You can download the code + some documentation on how to use it. It is quite straight forward.

Pei

marcbest July 14, 2010 08:55

hi phsieh,

the link you are talking about is:
http://openfoamwiki.net/index.php/Contrib_MakeAxialMesh :)

this converts a 2D block mesh file (with parallel faces) into an wedge-mesh, but i don't think it can convert a fluent axissymetry-mesh to open-foam wedge. for the axissymetry-mesh the type "cyclic" must be taken. am i wrong with this?

bruxellois4 July 14, 2010 12:20

3 Attachment(s)
I don't think that MakeAxialMesh works with openFOam 1.7.

I have to simulate a barrel of a gun, as you can see in screen shots (attachments), i have one cell thick in y i direction, but in my boundary file i don't see how to define a wedge, SO has an idea, help plzz
13
(
tube5
{
type wall;
nFaces 30;
startFace 60334;
}
tube4
{
type wall;
nFaces 3;
startFace 60364;
}
FREIN3
{
type wall;
nFaces 70;
startFace 60367;
}
FREIN2
{
type wall;
nFaces 15;
startFace 60437;
}
FREIN1
{
type wall;
nFaces 30;
startFace 60452;
}
Frein
{
type wall;
nFaces 20;
startFace 60482;
}
Pressure_inlet
{
type patch;
nFaces 30;
startFace 60502;
}
Tube3
{
type wall;
nFaces 21;
startFace 60532;
}
Tube2
{
type wall;
nFaces 10;
startFace 60553;
}
Tube1
{
type wall;
nFaces 139;
startFace 60563;
}
Axe
{
type symmetryPlane;
nFaces 215;
startFace 60702;
}
Pressure_outlet
{
type patch;
nFaces 209;
startFace 60917;
}
frontAndBackPlanes
{
type empty;
nFaces 60730;
startFace 61126;
}
)

phsieh2005 July 14, 2010 16:58

hi,

did you checkout the latest version from svn? It works for me on OpenFOAM-1.7.x.

Pei

phsieh2005 July 14, 2010 17:01

Hi, bruxellois4,

I assume that your frontAndBackPlanes are the wedge BC.

So,

frontAndBackPlanes
{
type wedge;
nFaces 60730;
startFace 61126;
}

Pei

bruxellois4 July 14, 2010 17:08

Hi Pei,

i 've changed the frontAndBackPlanes to wedge type but that i didn't see any change under paraview i steel having the same graphics.

Do you have any idea how to install MakeAxialMesh under OF 1.7!

Thanks

Abdel

phsieh2005 July 14, 2010 19:25

Hi, bruxellois4

In your 0/ folder, all variables, say p and U, you should also have frontAndBackPlanes set to wedge, for example,

frontAndBackPlanes
{
type wedge;
}
--------------
I don't understand what you mean by you still have the same graphics under paraview.

To install makeAxialMesh under OF-1.7.x, just download the latest version from svn (mentioned on the wiki page).

Then, cd do the MakeAxialMesh folder, type
./Allwmake

Good Luck!

Pei

bruxellois4 July 14, 2010 19:32

[QUOTE=phsieh2005;267323]Hi, bruxellois4

In your 0/ folder, all variables, say p and U, you should also have frontAndBackPlanes
--------------
I don't understand what you mean by you still have the same graphics under paraview.
[/QUOTErmar

Yes it's done but ididn' remark any change in graphics (paraview) withe empty patch or wedge, it 's the same

regards Pei

bruxellois4 July 14, 2010 19:42

For makeAxialMess i've puted the folder under mesh/manipulation (makeAxialMes folder contain a folder (make) and a makeAxialMes.C file) i tried ./Alwemake but tha doesnt work.

1: wmake not found

Abdel

phsieh2005 July 14, 2010 21:33

Hi, Abdel,

When you check out the MakeAxialMesh files, you cd to MakeAxialMesh folder. You should have the following files/directories:

TestCases (a folder)
makeAxialMesh (a folder)
Allwmake
README

type ./Allwmake in this folder. DO NOT cd to makeAxialMesh folder.

Pei

phsieh2005 July 14, 2010 21:35

[QUOTE=bruxellois4;267324]
Quote:

Originally Posted by phsieh2005 (Post 267323)
Hi, bruxellois4

In your 0/ folder, all variables, say p and U, you should also have frontAndBackPlanes
--------------
I don't understand what you mean by you still have the same graphics under paraview.
[/QUOTErmar

Yes it's done but ididn' remark any change in graphics (paraview) withe empty patch or wedge, it 's the same

regards Pei

If you do not mind, pack up the case. I can take a quick look at it.

Send it to phsieh2005@yahoo.com

Pei

bruxellois4 July 14, 2010 23:37

[QUOTE=phsieh2005;267337]
Quote:

Originally Posted by bruxellois4 (Post 267324)

If you do not mind, pack up the case. I can take a quick look at it.

Send it to phsieh2005@yahoo.com

Pei

Yes of course

thank you Pei!

mvoss November 26, 2010 06:55

hi,

I am running OF 1.7.x. under suse, installed MakeAxialMesh without any problems.
Iím facing some trouble whilst coming from msh. to a running axialmesh case using the makeAxialMesh tool.

What i did so far:
- created a quasi 2D Mesh in ICEM (1 cell height, frontandback in one patch, all patches are walls for now) --> exported to Fluent.V6
- used fluentMeshToFoam successfully
-checkMesh ran without pointing out any mistakes
- makeAxialMesh ran upto some fancy failure in
"Attempt to cast type polyMesh to type fvMesh" AFTER successfully "copying patches ...."
- the Output is pointing @ typeInfo.H (which is checking the types objects???)

So. Anybody ever faced smth. similar?

neewbie

mvoss November 26, 2010 07:03

me again,

i solved the problem by just simply deleting every .lib entry in my controlDict.

neewbie


All times are GMT -4. The time now is 16:49.