CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > OpenFOAM

How to use an ICEM wedge geometry?

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   May 22, 2012, 07:05
Default How to use an ICEM wedge geometry?
  #1
Member
 
Fabian E.
Join Date: Nov 2009
Posts: 36
Rep Power: 7
galap is on a distinguished road
Dear community,

I'm trying to get a simple wedge geometry running in OpenFOAM, which I created in ICEM. The wedge is a 10 deg slice with axis points (2 0 0) and (7 0 0). I ensured that the patch areas aren't aligned to coordinate planes. Front and back side are aligned to the yz plane. Symmetrie plane is aligned to yx plane (so both wedge patches are rotated by 5 deg). I attached an ICEM screenshot.
After importing in OpenFOAM by fluent3DMesh.. the boundary file looks like:

WEDGE1
{
type wedge;
nFaces 81;
startFace 819;
}
WEDGE2
{
type wedge;
nFaces 81;
startFace 900;
}
FRONT
{
type wall;
nFaces 36;
startFace 981;
}
BACK
{
type wall;
nFaces 36;
startFace 1017;
}
WALL
{
type wall;
nFaces 36;
startFace 1053;
}

Now, the probleme comes in when I checkMesh the case. The error is the, popular?, ***Number of edges not aligned with or perpendicular to non-empty directions: 5
<<Writing 10 points on non-aligned edges to set nonAlignedEdges



I absolutely have no clue what is the problem and how to fix this. I'm very grateful for your help. I'm looking forward to.
Attached Images
File Type: png wedge.png (68.0 KB, 52 views)
galap is offline   Reply With Quote

Old   May 22, 2012, 08:28
Default
  #2
Senior Member
 
linnemann's Avatar
 
Niels Nielsen
Join Date: Mar 2009
Location: NJ - Denmark
Posts: 451
Rep Power: 15
linnemann will become famous soon enough
Hi

Page 18 of this report shows how to make a wedge geometry.

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

Keep in mind that a wedge case in OF does not handle flow normal to the wedge patch so you wont see swirl.

If you want to use your mesh directly and see swirl use cyclic with rotational offset BC's for the wedge patches.
__________________
Linnemann

PS. I do not do personal support, so please post in the forums.
linnemann is offline   Reply With Quote

Old   May 22, 2012, 09:07
Default
  #3
Member
 
Fabian E.
Join Date: Nov 2009
Posts: 36
Rep Power: 7
galap is on a distinguished road
Thanks, I'm going to check these things.
galap is offline   Reply With Quote

Old   May 22, 2012, 09:11
Default
  #4
Senior Member
 
Tobi's Avatar
 
Tobias Holzmann
Join Date: Oct 2010
Location: Leoben (Austria)
Posts: 1,100
Blog Entries: 6
Rep Power: 19
Tobi will become famous soon enough
Send a message via ICQ to Tobi Send a message via Skype™ to Tobi
Quote:
Originally Posted by galap View Post
Dear community,

I'm trying to get a simple wedge geometry running in OpenFOAM, which I created in ICEM. The wedge is a 10 deg slice with axis points (2 0 0) and (7 0 0). I ensured that the patch areas aren't aligned to coordinate planes. Front and back side are aligned to the yz plane. Symmetrie plane is aligned to yx plane (so both wedge patches are rotated by 5 deg). I attached an ICEM screenshot.
After importing in OpenFOAM by fluent3DMesh.. the boundary file looks like:

WEDGE1
{
type wedge;
nFaces 81;
startFace 819;
}
WEDGE2
{
type wedge;
nFaces 81;
startFace 900;
}
FRONT
{
type wall;
nFaces 36;
startFace 981;
}
BACK
{
type wall;
nFaces 36;
startFace 1017;
}
WALL
{
type wall;
nFaces 36;
startFace 1053;
}

Now, the probleme comes in when I checkMesh the case. The error is the, popular?, ***Number of edges not aligned with or perpendicular to non-empty directions: 5
<<Writing 10 points on non-aligned edges to set nonAlignedEdges



I absolutely have no clue what is the problem and how to fix this. I'm very grateful for your help. I'm looking forward to.

Hi if you wanna use wedge you should have ONE CELL in the rotation direction.

Tobi
Tobi is offline   Reply With Quote

Old   May 22, 2012, 09:28
Default
  #5
Member
 
Fabian E.
Join Date: Nov 2009
Posts: 36
Rep Power: 7
galap is on a distinguished road
Yes indeed, the problem was the cell thickness. Ok, I don't want only one cell, so I'll try the cyclic boundaries..
galap is offline   Reply With Quote

Old   July 3, 2013, 13:55
Default
  #6
Member
 
Vasileios Sassanis
Join Date: Nov 2012
Posts: 76
Rep Power: 4
VSass is on a distinguished road
Quote:
Originally Posted by linnemann View Post
Hi

Page 18 of this report shows how to make a wedge geometry.

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

Keep in mind that a wedge case in OF does not handle flow normal to the wedge patch so you wont see swirl.

If you want to use your mesh directly and see swirl use cyclic with rotational offset BC's for the wedge patches.
Why is this happening? Is it because of the mesh been generated in Fluent or a feature of OF code?
VSass is offline   Reply With Quote

Old   November 25, 2014, 14:40
Default
  #7
New Member
 
minoominaii
Join Date: Nov 2014
Posts: 7
Rep Power: 2
bgane67 is on a distinguished road
i want to design a nuzzle with cylinder to observe droplet's pinch off
i converted 2D to 3D with extrudeMeshDict
but after running setFields i recieved this error:
wedge front plane aligns with a coordinate plane.
The wedge plane should make a small angle (~2.5deg) with the coordinate plane
and the the pair of wedge planes should be symmetric about the coordinate plane.
Normal of face 0 is (0 0 -1) , implied coordinate plane direction is (0 0 -1)

From function wedgePolyPatch::initTransforms()
in file meshes/polyMesh/polyPatches/constraint/wedge/wedgePolyPatch.C at line 78.

my BlockMesh is:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object blockMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

convertToMeters 0.001;


vertices
(
//back
(0 0 0)
(1 0 0)
(5 0 0)

(0 0.5 0)
(1 0.5 0)
(5 0.5 0)

(1 2 0)
(5 2 0)

//front
(0 0 0.1)
(1 0 0.1)
(5 0 0.1)

(0 0.5 0.1)
(1 0.5 0.1)
(5 0.5 0.1)

(1 2 0.1)
(5 2 0.1)

);

blocks
(
hex (0 1 4 3 8 9 12 11) (10 5 1) simpleGrading (1 1 1)
hex (1 2 5 4 9 10 13 12) (50 5 1) simpleGrading (1 1 1)
hex (4 5 7 6 12 13 15 14) (50 15 1) simpleGrading (1 1 1)

);

edges
(
);

boundary
(
inlet
{
type patch;
faces
(
(0 3 11 8)
);
}
outlet
{
type patch;
faces
(
(2 5 13 10)
(5 7 15 13)
(6 7 15 14)
);
}

fixedWall
{
type wall;
faces
(
(3 4 12 11)
(4 6 14 12)
);
}
axis
{
type patch;
faces
(
(0 1 9 8)
(1 2 10 9)
);
}

front
{
type patch;
faces
(
(0 1 4 3)
(1 2 5 4)
(4 5 7 6)
);
}
back
{
type patch;
faces
(
(8 9 12 11)
(9 10 13 12)
(12 13 15 14)
);
}
);

mergePatchPairs
(
);

// ************************************************** *********************** //
and my extrudemeshdict is:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object extrudeMeshDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

// What to extrude:
// patch : from patch of another case ('sourceCase')
// mesh : as above but with original case included
// surface : from externally read surface

constructFrom patch;
sourceCase "."; //the address of 2D geometry
sourcePatches (front);

// If construct from patch: patch to use for back (can be same as sourcePatch)
exposedPatchName back;

// Flip surface normals before usage. Valid only for extrude from surface or
// patch.
flipNormals true;

//- wedge extrusion in theta direction
extrudeModel wedge;
/*
6
(
linearDirection
linearNormal
linearRadial
radial
sigmaRadial
wedge
)
*/

nLayers 1;

expansionRatio 1.0;

wedgeCoeffs
{
axisPt (0 0 0); // point of axis
axis (1 0 0); // vector of axis
angle 5; // angle between front and back face
}

// Do front and back need to be merged? Usually only makes sense for 360
// degree wedges.
mergeFaces false;

// Merge small edges. Fraction of bounding box.
mergeTol 0.001;//1;


// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //
after creating mesh, i modified front and back patch boundary type from
patch to wedge in constant/polyMesh/bondary file



and my alpha.water is:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.3.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class volScalarField;
object alpha.water;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

dimensions [0 0 0 0 0 0 0];

internalField uniform 0;

boundaryField
{
inlet
{
type zeroGradient;
}

outlet
{
type zeroGradient;
}

fixedWall
{
type zeroGradient;
}

axis
{
type zeroGradient;
}

front
{
type wedge;
}
back
{
type wedge;
}
}

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




and my setFeildsDict is:



/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.2.0 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
location "system";
object setFieldsDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

defaultFieldValues
(
volScalarFieldValue alpha.water 0
);

regions
(
sphereToCell
{
centre (0 0 0);
radius 0.0005;
fieldValues
(
volScalarFieldValue alpha.water 1
);
}
);


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






thanks for your attention[/QUOTE]
bgane67 is offline   Reply With Quote

Old   January 18, 2015, 11:10
Default
  #8
New Member
 
Peng Liang
Join Date: Mar 2014
Posts: 24
Rep Power: 3
tjliang is on a distinguished road
Quote:
Originally Posted by Tobi View Post
Hi if you wanna use wedge you should have ONE CELL in the rotation direction.

Tobi
Hello Tobi, I have made almost the same geometry , when i export it from icem to fluent mesh , i just can't get the axis bounary in the mesh file. The axis is automatically neglected in the .msh file. Do you think i should change the axis boundary from edge to a very very narrow face(with only one cell broad). Axis is very important in openfoam especially when a wedge boundary appears.Thank you in advance.

Peng
tjliang is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Why Icem can't craeate Unstructured 2d Mesh on Circular Geometry Jvb ANSYS Meshing & Geometry 6 January 2, 2012 12:41
[ICEM] Icem Geometry creation strategy for hollow cube tony00 ANSYS Meshing & Geometry 1 March 16, 2011 12:05
Replace the geometry for an existing mesh in ICEM CFD Suzzn ANSYS Meshing & Geometry 2 September 7, 2009 17:59
Design Modeler to ICEM..... Joe CFX 0 January 24, 2008 04:39
workbench geometry in ICEM Ross CFX 6 November 2, 2006 07:51


All times are GMT -4. The time now is 05:44.