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

Deformation Issues...

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

Reply
 
LinkBack Thread Tools Display Modes
Old   April 12, 2011, 11:24
Default Deformation Issues...
  #1
New Member
 
Join Date: Oct 2010
Posts: 29
Rep Power: 6
Silmaril is on a distinguished road
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
File Type: png Wedge_Deformation.png (72.1 KB, 39 views)
Silmaril is offline   Reply With Quote

Old   April 12, 2011, 13:40
Default
  #2
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   April 14, 2011, 08:29
Default
  #3
New Member
 
Join Date: Oct 2010
Posts: 29
Rep Power: 6
Silmaril is on a distinguished road
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
Silmaril is offline   Reply With Quote

Old   April 14, 2011, 08:48
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy is offline   Reply With Quote

Old   April 26, 2011, 06:32
Default
  #5
New Member
 
Join Date: Jan 2011
Posts: 24
Rep Power: 6
vidhya is on a distinguished road
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...
vidhya is offline   Reply With Quote

Old   April 26, 2011, 13:24
Default
  #6
Senior Member
 
Join Date: Apr 2009
Posts: 511
Rep Power: 12
stumpy is on a distinguished road
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.
stumpy 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
CFX Mesh Deformation problem Silmaril CFX 7 October 19, 2010 10:00
Calculation of the deformation rate titio OpenFOAM Running, Solving & CFD 1 March 22, 2009 09:45
Predefined Mesh Deformation Alexv CFX 6 October 6, 2008 12:01
Mesh Deformation issues Jon P CFX 0 November 27, 2007 19:20
Mesh Deformation Problem Virag Mishra CFX 0 October 9, 2007 00:37


All times are GMT -4. The time now is 23:57.