CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > SU2

Mesh Generating Using Spring Analogy

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

Reply
 
LinkBack Thread Tools Display Modes
Old   January 3, 2014, 10:56
Default Mesh Generating Using Spring Analogy
  #1
New Member
 
Yosheph Yang
Join Date: Nov 2012
Location: Ankara, Turkey
Posts: 24
Rep Power: 4
andromeda91 is on a distinguished road
Dear All,

I am planning to perform analysis around flapped airfoil. I have prepared mesh for unflapped airfoil. By any chance, is it possible for me to deform the airfoil geometry (mesh as well) using spring analogy method in SU2?
By doing that, I don't need to generate new mesh for the flapped airfoil.


Regards,

Yosheph Yang
andromeda91 is offline   Reply With Quote

Old   January 3, 2014, 12:33
Post
  #2
Member
 
Jianming Liu
Join Date: Mar 2009
Location: China
Posts: 66
Rep Power: 8
liujmljm is on a distinguished road
Quote:
Originally Posted by andromeda91 View Post
Dear All,

I am planning to perform analysis around flapped airfoil. I have prepared mesh for unflapped airfoil. By any chance, is it possible for me to deform the airfoil geometry (mesh as well) using spring analogy method in SU2?
By doing that, I don't need to generate new mesh for the flapped airfoil.


Regards,

Yosheph Yang
In SU2, u can use FEA moving mesh method, which is more stable than spring analogy method
liujmljm is offline   Reply With Quote

Old   January 5, 2014, 15:52
Default
  #3
New Member
 
Yosheph Yang
Join Date: Nov 2012
Location: Ankara, Turkey
Posts: 24
Rep Power: 4
andromeda91 is on a distinguished road
I tried to find the FEA moving mesh method that you mentioned. However, I couldn't find it.
Can you describe to me how I am supposed to do it?



Quote:
Originally Posted by liujmljm View Post
In SU2, u can use FEA moving mesh method, which is more stable than spring analogy method
andromeda91 is offline   Reply With Quote

Old   January 7, 2014, 08:19
Smile
  #4
Member
 
Jianming Liu
Join Date: Mar 2009
Location: China
Posts: 66
Rep Power: 8
liujmljm is on a distinguished road
Quote:
Originally Posted by andromeda91 View Post
I tried to find the FEA moving mesh method that you mentioned. However, I couldn't find it.
Can you describe to me how I am supposed to do it?
please look at the templete cfg file carefully or the source code, u will find that. good luck
liujmljm is offline   Reply With Quote

Old   January 11, 2014, 22:47
Default
  #5
Super Moderator
 
Francisco Palacios
Join Date: Jan 2013
Location: Stanford, CA
Posts: 301
Rep Power: 5
fpalacios is on a distinguished road
Yes, SU2_MDC is the right solver for grid deformation. It uses a FEA method (we have removed the spring analogy method - this method didn't work with high stretching grids - ).

There are different deformation implemented in the code. It could be useful for you to take a look at a pitching airfoil optimization problem (Anyone has realized optimization for unsteady flows?).

Best Regards,
Francisco
fpalacios is offline   Reply With Quote

Old   January 20, 2014, 09:27
Default
  #6
New Member
 
Yosheph Yang
Join Date: Nov 2012
Location: Ankara, Turkey
Posts: 24
Rep Power: 4
andromeda91 is on a distinguished road
Quote:
Originally Posted by fpalacios View Post
Yes, SU2_MDC is the right solver for grid deformation. It uses a FEA method (we have removed the spring analogy method - this method didn't work with high stretching grids - ).

There are different deformation implemented in the code. It could be useful for you to take a look at a pitching airfoil optimization problem (Anyone has realized optimization for unsteady flows?).

Best Regards,
Francisco
Dear Francisco,

I have tried to look at the configuration file that you mentioned. I don't know how to modify the configuration file in here. I want to remesh the airfoil into flapped airfoil whose flap is deflected around 0.7c with around 10 degree without performing any optimization at all. If you don't mind, how should I perform this using SU2_MDC module?

Regards,

Yosheph
andromeda91 is offline   Reply With Quote

Old   February 12, 2014, 21:55
Default
  #7
Super Moderator
 
Thomas D. Economon
Join Date: Jan 2013
Location: Stanford, CA
Posts: 260
Rep Power: 5
economon is on a distinguished road
Hi Yosheph,

If you can modify the locations of the surface nodes for the particular airfoil (just your flap for instance), you can input their new locations in a file to SU2_MDC and choose the option DV_KIND= SURFACE_FILE. MDC will then deform the volume mesh around the new airfoil geometry. You will also need to give the filename in the options:

% Surface deformation input filename (SURFACE_FILE DV only)
MOTION_FILENAME= mesh_motion.dat

Please see the routine CSurfaceMovement::SetSurface_Deformation(CGeometry *geometry, CConfig *config) in the file grid_movement_structure.cpp for more details on the format for the file with the new airfoil coordinates.

Cheers,
Tom
economon is offline   Reply With Quote

Old   February 26, 2014, 16:36
Default
  #8
Member
 
Tommy Chen
Join Date: Mar 2011
Location: University of Michigan
Posts: 93
Rep Power: 6
Tommy Chen is on a distinguished road
Quote:
Originally Posted by economon View Post
Hi Yosheph,

If you can modify the locations of the surface nodes for the particular airfoil (just your flap for instance), you can input their new locations in a file to SU2_MDC and choose the option DV_KIND= SURFACE_FILE. MDC will then deform the volume mesh around the new airfoil geometry. You will also need to give the filename in the options:

% Surface deformation input filename (SURFACE_FILE DV only)
MOTION_FILENAME= mesh_motion.dat

Please see the routine CSurfaceMovement::SetSurface_Deformation(CGeometry *geometry, CConfig *config) in the file grid_movement_structure.cpp for more details on the format for the file with the new airfoil coordinates.

Cheers,
Tom
Hi Tom

Actually SU2_MDC would create an initial mesh_motion file, if MOTION_FILENAME has been set and mesh_motion.dat does not exist. The related code is as:
################################################## ############
/*--- A surface file does not exist, so write a new one for the
markers that are specified as part of the motion. ---*/
if (Surface_File.fail()) {

if (rank == MASTER_NODE)
cout << "No surface file found. Writing a new file: " << filename << "." << endl;

Surface_File.open(filename.c_str(), ios:ut);
Surface_File.precision(15);
unsigned long iMarker, jPoint, GlobalIndex, iVertex; double *Coords;
for (iMarker = 0; iMarker < config->GetnMarker_All(); iMarker++) {
if (config->GetMarker_All_DV(iMarker) == YES) {
for(iVertex = 0; iVertex < geometry->nVertex[iMarker]; iVertex++) {
jPoint = geometry->vertex[iMarker][iVertex]->GetNode();
GlobalIndex = geometry->node[jPoint]->GetGlobalIndex();
Coords = geometry->node[jPoint]->GetCoord();
Surface_File << GlobalIndex << "\t" << Coords[0] << "\t" << Coords[1];
if (nDim == 2) Surface_File << endl;
else Surface_File << "\t" << Coords[2] << endl;
}
}
}
################################################## ############

However , after I test it with 3D ONERA M6 wing case in parallel mode, I found out that only the surface mesh points which owned by the master_node have been outputed. I think this is a bug somehow, I want to fix it , but do not know how.
Tommy Chen 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
SnappyHexMesh for internal Flow vishwa OpenFOAM Native Meshers: snappyHexMesh and Others 23 August 6, 2014 03:50
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 06:20
[ICEM] Generating Mesh for STL Car in Windtunnel Simulation tommymoose ANSYS Meshing & Geometry 48 April 15, 2013 04:24
ParaView and Qt 4.3.5 on Mac OS X 10.6 Adrian OpenFOAM 3 August 8, 2010 03:16
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10


All times are GMT -4. The time now is 19:14.