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

Setting side/wedge boundary condition

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

Reply
 
LinkBack Thread Tools Display Modes
Old   August 1, 2012, 22:12
Default Setting side/wedge boundary condition
  #1
New Member
 
Thomas S
Join Date: Aug 2012
Posts: 11
Rep Power: 4
Thoma is on a distinguished road
Hello,

I am trying to set a proper boundary condition for sidewalls. To illustrate my problem, I have attached a screenshot.

The problem is to set boundary conditions on the green parts in the picture. I'd like to apply identical conditions for both sides. So for instance, flow stream leaving one side should enter the volume on the other side.
I think some kind of 'wedge' boundary condition is most convenient but I haven't managed it so far.

Is it possible to do it with wedge conditions? Or are there any more convenient?

I am using Salome for meshing.

Thanks for your help.

Thoma
Attached Images
File Type: jpg boundary condition.jpg (60.7 KB, 123 views)
Thoma is offline   Reply With Quote

Old   August 21, 2012, 23:49
Default
  #2
New Member
 
Thomas S
Join Date: Aug 2012
Posts: 11
Rep Power: 4
Thoma is on a distinguished road
Ok. I managed it by using cyclicAMI which is available since OpenFoam v2.1.0

http://www.openfoam.org/version2.1.0/

Here you don't need exact matching points on both sides. Nevertheless a similar meshing is required. To mesh it with Salome see here:

http://www.salome-platform.org/forum/forum_10/272693881

Finally my boundary file looks like this:

/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 2.1.1 |
| \\ / A nd | Web: www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class polyBoundaryMesh;
location "constant/polyMesh";
object boundary;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

6
(
inlet
{
type patch;
nFaces 350;
startFace 125878;
}
outlet
{
type patch;
nFaces 342;
startFace 126228;
}
side1
{
type cyclicAMI;
neighbourPatch side2;
transform translational;
separationVector (-0.04 0 0);
nFaces 1478;
startFace 126570;
}
side2
{
type cyclicAMI;
neighbourPatch side1;
transform translational;
separationVector (0.04 0 0);
nFaces 1478;
startFace 128048;
}
wall
{
type wall;
nFaces 4431;
startFace 129526;
}
vane
{
type wall;
nFaces 981;
startFace 133957;
}
)

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

I hope this helps anyone who struggles with a similar problem I had.

regards,

Thomas
Thoma is offline   Reply With Quote

Old   February 20, 2013, 17:00
Default
  #3
New Member
 
Peter Skrifvars
Join Date: Oct 2009
Posts: 3
Rep Power: 7
Skrifvars is on a distinguished road
Hi Thoma,
You mentioned
'Nevertheless a similar meshing is required.'

Does this mean that you had to reorder the coupled faces in some manner that I don't
find in Salome or OF applications ?

Did you create this cyclicAMI with createPatch or just by editing the boundary file ?

BR
Peter
Skrifvars is offline   Reply With Quote

Old   February 20, 2013, 17:32
Default
  #4
New Member
 
Thomas S
Join Date: Aug 2012
Posts: 11
Rep Power: 4
Thoma is on a distinguished road
Hi Peter.

you have to copy the mesh information from one side to the other. Follow the link I have posted above. There it is sxplained.

I didn't use createPatch. Just edited the boundary file.

Regards, Thomas
Thoma is offline   Reply With Quote

Old   July 15, 2014, 18:06
Default transform type
  #5
New Member
 
ZD
Join Date: Jul 2014
Posts: 11
Rep Power: 2
zhixuan is on a distinguished road
hi all,
I tried the processes above on my simulation using OF2.3. However, there is some problems.

My case is a quarter of a cylinder. So the two section planes should be defined as cyclic BC. At beginning, I thought I should set the transform type to be "rotational" according this link.

However, this setup causes a rotation of the entire flow field.

Now, I think I should use the type of "translational". I set the separationVector to be the Z axis (0 0 1). But it reports errors as follows:

Quote:
Create time

Create mesh for time = 0

Reading field p

--> FOAM Warning :
From function polyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 461
Patch bottom specifies a group wall which is also a patch name. This might give problems later on.
--> FOAM Warning :
From function polyBoundaryMesh::groupPatchIDs() const
in file meshes/polyMesh/polyBoundaryMesh/polyBoundaryMesh.C at line 461
Patch wall specifies a group wall which is also a patch name. This might give problems later on.
AMI: Creating addressing and weights between 3320 source faces and 3320 target faces
--> FOAM Warning :
From function AMIMethod<SourcePatch, TargetPatch>::checkPatches()
in file lnInclude/AMIMethod.C at line 57
Source and target patch bounding boxes are not similar
source box span : (0.07875 4.82189e-18 0.5105)
target box span : (3.61641e-18 0.07875 0.5105)
source box : (0 0 0) (0.07875 4.82189e-18 0.5105)
target box : (-2.41094e-18 0 -1) (1.20547e-18 0.07875 -0.4895)
inflated target box : (-0.0258269 -0.0258269 -1.02583) (0.0258269 0.104577 -0.463673)

So I'm wondering if there is anyone can kindly provide any hints regarding this issue.

Thank you
Attached Images
File Type: png rotational1.png (25.8 KB, 19 views)
File Type: jpg rotational2.jpg (29.4 KB, 17 views)
zhixuan 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
Setting the inlet boundary condition with inclination saisanthoshm88 CFX 1 October 4, 2011 06:41
Cells with t below lower limit Purushothama CD-adapco 2 May 31, 2010 21:58
vorticity boundary condition bearcharge Main CFD Forum 0 May 14, 2010 11:32
boundary condition velocity inlet dont have gauge pressure setting value? coolyihao FLOW-3D 0 March 17, 2009 11:17
Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Other Meshers: ICEM, Star, Ansys, Pointwise, GridPro, Ansa, ... 2 July 15, 2005 04:15


All times are GMT -4. The time now is 12:57.