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

Morph mesh given displacement of boundary points

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

Like Tree1Likes
  • 1 Post By ngj

Reply
 
LinkBack Thread Tools Display Modes
Old   November 5, 2011, 02:12
Default Morph mesh given displacement of boundary points
  #1
Super Moderator
 
praveen's Avatar
 
Praveen. C
Join Date: Mar 2009
Location: Bangalore
Posts: 244
Blog Entries: 6
Rep Power: 9
praveen is on a distinguished road
Hello

Is there anything in openfoam which allows me to morph the interior mesh, given the displacement of the boundary mesh nodes ?

praveen
praveen is offline   Reply With Quote

Old   November 5, 2011, 04:04
Default
  #2
Super Moderator
 
Bruno Santos
Join Date: Mar 2009
Location: Lisbon, Portugal
Posts: 8,301
Blog Entries: 34
Rep Power: 84
wyldckat is just really nicewyldckat is just really nicewyldckat is just really nicewyldckat is just really nice
Hi Praveen,

Does this tutorial suit your requirements: "tutorials/mesh/moveDynamicMesh/simpleHarmonicMotion"

Best regards,
Bruno
wyldckat is offline   Reply With Quote

Old   November 5, 2011, 07:05
Default
  #3
Super Moderator
 
praveen's Avatar
 
Praveen. C
Join Date: Mar 2009
Location: Bangalore
Posts: 244
Blog Entries: 6
Rep Power: 9
praveen is on a distinguished road
Thanks. That seems relevant to me. I will check it out. Is it possible to specify the displacement of each individual boundary mesh point ?
praveen is offline   Reply With Quote

Old   November 5, 2011, 08:33
Default
  #4
ngj
Senior Member
 
Niels Gjoel Jacobsen
Join Date: Mar 2009
Location: Deltares, Delft, The Netherlands
Posts: 1,603
Rep Power: 25
ngj will become famous soon enoughngj will become famous soon enough
Hi Praveen,

Yes, it is possible to specify the displacement on the point level. This type of boundary condition can be put into two categories:

1. You know the motion by an algebraic equation, hence you loop over every boundary point and specify the displacement (Note: Some solvers use the boundary velocity, thus differentiate your algebraric equation with respect to time and evaluate it). Furthermore, if you are using tet-decomposition (available in 1.6-ext), you specify both the motion on the points and in the centers of the boundary faces. On the boundary, they are ordered as [<points> <face centers>].

2. You move the mesh based on results from the state of your simulation. Typically you can compute the motion in the face centers, and then you perform an interpolation to the points on the boundary. Again, be aware when you are using displacement or velocity solvers for the mesh motion.

With respect to the interpolation methods you can either look through the forum, or so-forth you have 1.6-ext installed, you can see an example of the implementation in the file "freeSurface.C" located somewhere in the "applications/solvers" directory.

A final comment: If the boundary you are moving also has a very fine boundary layer resolution, then my experience is that laplaceFaceDecomposition (1.6-ext) is the most robust combined with a very stiff mesh diffusivity next to that boundary. The diffusivity is the \gamma term in the following Laplace equation for the velocity of the mesh motion:

\nabla \gamma\boldsymbol\cdot\nabla\mathbf{u}_m=\boldsymbol{0}

The diffusivity is specified in the dynamicMeshDict in <rootCase>/constant.

Good luck and kind regards,

Niels
fumiya likes this.
ngj 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
2D foam mesh and internal points virginie_e OpenFOAM Meshing Format & General Technical 3 February 28, 2014 01:05
How to set boundary layer of a moving body in GAMBIT to a mesh zone for dynamic mesh tomyangbath FLUENT 16 January 18, 2012 05:47
FSI - Specified Mesh Displacement Vinzent CFX 2 September 17, 2010 07:09
Import problem ARC Open Source Meshers: Gmsh, Netgen, CGNS, ... 0 February 27, 2010 11:56
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 01:16.