# Deformation Issues...

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

April 12, 2011, 11:24
Deformation Issues...
#1
New Member

Join Date: Oct 2010
Posts: 29
Rep Power: 9
I was trying to run a simulation with mesh deformation in a HEXA grid. In order to have a simple "bellow-like" deformation motion, I divided the domain in several sub-domain connected by "sliding" GGI interfaces. Unfortunatly I didn't get the "bellow-like" motion but some strange mesh distortion occurs at some boundaries.

To study the possible causes of the problem I made a simplified 2D model similar to the sub-domain that shown mesh distortion:

2D Wedge with low angle (~20°) with inclined walls closing in the vertical direction (see attached figure).
With the settings shown in the figure for the mesh deformation I was hoping to obtain a uniform distribution of the nodes in the lateral walls similar to a bellow-like motion. Unfortunately distortion occurs at the high angle corners (shown in the right part of the figure). I tried different parameters for the mesh stiffness (exponent or values...) with little change in the result (a slightly better behaviour is obtained if the exponent is decreased from 10, default value, to 1).

Anyone knows how can I solve such a problem? (possibly wothout having to impose each node displacement with User Fortran Routines

Thanks
Attached Images
 Wedge_Deformation.png (72.1 KB, 43 views)

 April 12, 2011, 13:40 #2 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 14 Under Expert Parameters try 'meshdisp diffusion scheme = 3'. If that doesn't help then it would be best to define the motion of each node using a subdomain, but you don't need User Fortran for that. Create a weighting function that varies linearly from 0 on the stationary boundary to 1 on the moving boundary, then multiply that by the imposed displacement. For a Cartesian aligned rectangle the weighting function is trivial, for a wedge it still not too difficult.

 April 14, 2011, 08:29 #3 New Member   Join Date: Oct 2010 Posts: 29 Rep Power: 9 Thanks very much, I've tried the expert parameter and the weighting function too, both give quite good results, even if some problem still arises. With this improvement probably I can just run a simulation for long enough till mesh start to degenerate, stop the calculation, and restart with a fresh-new mesh until the motion ends. By the way, what's the difference between the mesh diffusion scheme 2 and 3? Why there's such a difference in element distortion? Thank you again

 April 14, 2011, 08:48 #4 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 14 That parameter changes the numerics of the diffusion scheme. According to the documentation it changes the interior and boundary nodes to positive definite values. Basically I think that means you avoid wiggles in the solution. Positive definite values can give unphysical solutions, but in this case there is no real physics tied to the diffusion equation that is being solved so it doesn't matter if it's "physical". The boundary displacements are explicitly defined (they're not part of the solution), so it's not applicable here.

 April 26, 2011, 06:32 #5 New Member   Join Date: Jan 2011 Posts: 24 Rep Power: 8 hi, i am quite new to sliding mesh technique. i have done simulation using MFR. can u giv a gist of how to perform sliding mesh in CFX.. i have read about SM method in articles still i dont understand properly... and also in cfx while defining interfaces, we have an option for pitch change. does that have anything connected to sliding mesh??? please help me...

 April 26, 2011, 13:24 #6 Senior Member   Join Date: Apr 2009 Posts: 532 Rep Power: 14 In CFX you usually don't want to use a "sliding mesh" for an MFR case. CFX has a transient rotor-stator interface to deal with relative motion between rotating/stationary components. Some codes don't have that, so they have to physically clock the rotating mesh, hence you get a sliding mesh at the interface.

 Thread Tools 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 On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Silmaril CFX 7 October 19, 2010 10:00 titio OpenFOAM Running, Solving & CFD 1 March 22, 2009 09:45 Alexv CFX 6 October 6, 2008 12:01 Jon P CFX 0 November 27, 2007 19:20 Virag Mishra CFX 0 October 9, 2007 00:37

All times are GMT -4. The time now is 19:06.