# Moving (structured) mesh

 User Name Remember Me Password
 Register Blogs Members List Search Today's Posts Mark Forums Read

 LinkBack Thread Tools Search this Thread Display Modes
 February 1, 2007, 04:39 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

 February 1, 2007, 08:04 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?

 February 1, 2007, 09:00 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

 February 1, 2007, 09:50 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

 February 1, 2007, 16:14 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

 February 2, 2007, 03:43 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

 Thread Tools Search this Thread Search this Thread: Advanced Search Display Modes Linear Mode

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Althea FLUENT 22 January 4, 2017 03:19 [snappyHexMesh] SnappyHexMesh for internal Flow vishwa OpenFOAM Meshing & Mesh Conversion 24 June 27, 2016 08:54 aeroslacker OpenFOAM Meshing & Mesh Conversion 12 January 19, 2012 03:52 prhlava OpenFOAM Running, Solving & CFD 8 November 9, 2009 08:59 Andrea Panizza FLUENT 1 November 9, 2003 03:48

All times are GMT -4. The time now is 01:37.

 Contact Us - CFD Online - Privacy Statement - Top