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

Moving (structured) mesh

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

Reply
 
LinkBack Thread Tools Display Modes
Old   February 1, 2007, 05:39
Default Moving (structured) mesh
  #1
Jesper
Guest
 
Posts: n/a
Hey CFX-users

I have a question regarding moving mesh in CFX. The mesh is a structured mesh made in ICEM. The problem to be solved is a bridge profil moving under wind load.

Problems encounterd in CFX:

1) when moving the profile lateral the maximal distance it can be moved is 35cm before the mesh starts to curle around the profile edges and creates negativ volumes= solver error. (BC 2 x inlet and 2 x outlet to make diffrent angles of attack possible - and symmetry walls on the sides)

2) Changing the top/bottom to symmetry making "unspecified mesh motion" possible results in the mesh starts to curle near the outer boundaries again creating neg. volumes = solver error. And here the option of changing the angle of attack is lost.

General problem: The inlet/outlet can only be set to stationary (mesh motion). And changing the mesh stiffness from a constanc C to i.e C/wall distance or C/element volume do not make any changes.

Any ideas how to solve this problem without encounting these errors/difficulties? Is translation of the entire problem possible?

The spacing in ICEM is 0.0001 - does CFX concider this as a distance of 0? - because CFX says that C/Wall distance is equal to dividing by zero.

Thanks in advance

Jesper
  Reply With Quote

Old   February 1, 2007, 09:04
Default Re: Moving (structured) mesh
  #2
jon
Guest
 
Posts: n/a
Bigger domain?

An irrelevant point but why do you need two inlets? could you not just use an inlet with a different XYZ component? effectively changing the angle of attack?
  Reply With Quote

Old   February 1, 2007, 10:00
Default Re: Moving (structured) mesh
  #3
Robin
Guest
 
Posts: n/a
Hi Jesper,

Try running with double precision turned on. You're grid spacing is very small relative to the size of the structure and the motion involved (Do you really need a mesh size of .0001 for this?). You might also need to reduce your timestep if the mesh motion is too great within a timestep.

Inlets and outlets can have mesh motion set to "unspecified", but the option does not appear in the gui. You can edit the CCL in the command editor to make this change.

If you're domain is very small it might help to move the far field conditions further away.

Regards, Robin
  Reply With Quote

Old   February 1, 2007, 10:50
Default Re: Moving (structured) mesh
  #4
Jesper
Guest
 
Posts: n/a
Tanks a lot an will try that

The domain is 20 X corde length of the profile an should be more than enough. Can not just use one inlet with an angle of attack while this will not create the rigth simulation.

This spacing is normal for such simulations, and nessesary to keep the y-plus value small enough.

If any one else has other ideas you are more than welcome to post them.

tanks again

Jesper
  Reply With Quote

Old   February 1, 2007, 17:14
Default Re: Moving (structured) mesh
  #5
Glenn Horrocks
Guest
 
Posts: n/a
Hi,

In addition to Robin's comments, you can weight the mesh motion so certain parts of the mesh are "stiffer" than others and sometimes that can help. Often a good approach is to make the stiffness a function of element size or distance from a wall. This is discussed in the documentation.

Often this does not help but it is worth a try.

Glenn Horrocks
  Reply With Quote

Old   February 2, 2007, 04:43
Default Re: Moving (structured) mesh
  #6
Mads
Guest
 
Posts: n/a
This is intended to Robin. I have the similar situation about the mesh. Do you have a guide or walktrough have to edit the CCL in the command editor so i can set Inlets to "Unspecified". The command editor is not familiar to me.

Regards Mads V
  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
2D Mesh Generation Tutorial for GMSH aeroslacker Open Source Meshers: Gmsh, Netgen, CGNS, ... 12 January 19, 2012 04:52
salome, openfoam and moving mesh prhlava OpenFOAM Running, Solving & CFD 8 November 9, 2009 09:59
Structured mesh refinement Andrea Panizza FLUENT 1 November 9, 2003 04:48
Gambit problems Althea FLUENT 21 February 6, 2001 08:05


All times are GMT -4. The time now is 11:02.