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

Folding mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   December 18, 2007, 05:41
Default Folding mesh
  #1
Anders T Svendsen
Guest
 
Posts: n/a
I have a problem with deforming mesh. When translating a structure (located centrally in a structured mesh) in a circular motion, folds starts appearing in the mesh. For each such circular motion the folds are getting larger and larger, and seems to result in the creation of negative volume elements in the longer runs.

Is there any way to ensure that the mesh carries no history of previous deformations, that is, once the structure in the mesh has returned to it's original position, the mesh should return to it's original form as well.

Any help is muchly appreciated.

Anders T. Svendsen, Aalborg University, Denmark
  Reply With Quote

Old   December 18, 2007, 06:03
Default Re: Folding mesh
  #2
Anders T Svendsen
Guest
 
Posts: n/a
I forgot to mention that I am using CFX 10.0 and that I use fortran routines to govern the mesh deformation, by moving the structure and setting the mesh stiffness in the domain.
  Reply With Quote

Old   December 18, 2007, 17:19
Default Re: Folding mesh
  #3
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

Large mesh motion is difficult to do in CFX as it is difficult not to fold the mesh while doing it. Really the only option you have is to start being tricky with the mesh stiffness. Maybe if you locally increase the mesh stiffness near the moving body it can help? You can also do things like making the mesh stiffness higher for small elements or some combination of small elements and proximity to the moving body.

Glenn Horrocks
  Reply With Quote

Old   December 18, 2007, 18:42
Default Re: Folding mesh
  #4
jakjak
Guest
 
Posts: n/a
Anders,

As Glenn has suggested, you can increase the stiffness of the mesh in the domain. What you want to make sure the motion of the mesh is properly diffused away from the moving body. A few things you can try are:
  1. Mesh stiffness - you can try setting the mesh stiffness as a function of wall distance and volume of finite volume. [1]
  2. Transient timestep - as mesh motion is only available in transient simulation, by reducing the timestep, you effectively reduce the motion of the mesh. This allows the mesh displacement to converge easier and faster.
  3. Mesh displacement equation - either increase the coefficient loops and/or lower (tighter) convergence criteria for the mesh displacement equation (Under Solver Control -> Equation Class -> Mesh Displacement). This should the same net effect as reducing timestep.

You can try one of the above or combination of them and see which one works better for you.

Good Luck!

jakjak

Ref: [1] ANSYS CFX-Solver, Release 10.0: Modelling, pp. 18-19

  Reply With Quote

Old   December 19, 2007, 06:12
Default Re: Folding mesh
  #5
Anders T Svendsen
Guest
 
Posts: n/a
Thank you both for the feedback.

I am currently meddling with the mesh stiffness (1[m^(2+n) s^-1]/(wall distance)^n for n=1,2,3..) which reduces the problem, but doesn't quite resolve it.

I will try to reduce my timesteps and see if I can optimize the solver criterias as jakjak suggests.

Thanks again,

- Anders
  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
Converting Starccm+ mesh Ladnam OpenFOAM 0 September 14, 2011 06:30
engrid -> save as .stl with boundarie codes Zymon enGrid 31 August 29, 2011 13:40
Meshing aifoil in ICEM student123a ANSYS Meshing & Geometry 13 December 8, 2010 11:40
2d irregular grid Remy Main CFD Forum 1 December 22, 2008 05:49
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 12:55


All times are GMT -4. The time now is 13:51.