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

FSI with time interval remeshing ?

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 31, 2009, 20:43
Default FSI with time interval remeshing ?
  #1
New Member
 
Join Date: May 2009
Posts: 21
Rep Power: 8
realanony87 is on a distinguished road
Hello,
I am doing a transient FSI simulation of a wing with Ansys Simulation in Workbench and CFX. and due to large deflections (the same order as the length), the mesh quality gets poorer with each time interval.
Is there a way that I can Remesh the region around the wing instead of relying on the mesh interpolator, every X time intervals ? It seems to have been done in the literature with in-house codes but Is there a relatively easy way to do it in the Ansys Suite ?
Thanks
realanony87 is offline   Reply With Quote

Old   June 1, 2009, 04:53
Default
  #2
New Member
 
Join Date: Jun 2009
Posts: 21
Rep Power: 8
mortazavi is on a distinguished road
hi realanony87
sorry I don't know the answer,but :
would you please help me with the error"the connection between cfx and external solver has died unexpectedly" in FSI modeling in CFX????
what does this error means & how can i solve this problem?
mortazavi is offline   Reply With Quote

Old   June 1, 2009, 08:33
Default
  #3
New Member
 
Join Date: May 2009
Posts: 21
Rep Power: 8
realanony87 is on a distinguished road
It is probably due to an error from the Structural solver. Check the .out file from Ansys ( not the CFX out file) to see what went wrong. I cannot help you because it could happen due to many reasons.
realanony87 is offline   Reply With Quote

Old   June 2, 2009, 19:59
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 513
Rep Power: 12
stumpy is on a distinguished road
Remeshing + FSI is not currently possible with ANSYS + CFX. But there's a lots of ways to maintain mesh quality for large deflections. Using a mesh stiffness of "Increase Near Boundaries" with an exponent of say 2 would be a starting point. Then you need to look at where the mesh is folding - and change the mesh motion boundary conditions, or add subdomain mesh motion, or insert sliding interfaces etc to imporve things. Sorry i can't be more specific; the best approach is always case dependent.
stumpy is offline   Reply With Quote

Old   September 14, 2010, 05:32
Default different mesh stiffnesses of subdomains
  #5
New Member
 
Join Date: Jul 2010
Posts: 22
Rep Power: 7
Vinzent is on a distinguished road
Hello,

to play with mesh stiffness is very usefuel in case of large deflections. How is it possible, to define different mesh stiffnesses of subdomains? I just know this for a whole domain. So I have to control these complicated with if statements. Is there an easier way?

Vinzent
Vinzent is offline   Reply With Quote

Old   September 14, 2010, 09:04
Default
  #6
Senior Member
 
Join Date: Apr 2009
Posts: 513
Rep Power: 12
stumpy is on a distinguished road
To get a different mesh stiffness in a subdomain you will need if() statements, but the inside()@ function should make this fairly easy, e.g.
if(inside()@subdomain1, meshstiffness1, meshstiffness2)
stumpy is offline   Reply With Quote

Old   September 14, 2010, 10:11
Default
  #7
New Member
 
Join Date: Jul 2010
Posts: 22
Rep Power: 7
Vinzent is on a distinguished road
stumpy, thank you very much!
this is, what i was searching for.

vinzent
Vinzent is offline   Reply With Quote

Old   September 17, 2010, 07:29
Default
  #8
New Member
 
Join Date: Jul 2010
Posts: 22
Rep Power: 7
Vinzent is on a distinguished road
Hello Stumpy,

when I try to define mesh stiffness with "inside" like your example following error occurs:

##############################################
Error processing expression 'Mesh Stiffness'. Error at position 4. The condition expression in 'if' statement is not logical valued.
Error processing expression: Mesh Stiffness = MS

##############################################


Is there something missing?


Vinzent
Vinzent is offline   Reply With Quote

Old   September 17, 2010, 12:04
Default
  #9
Senior Member
 
Join Date: Apr 2009
Posts: 513
Rep Power: 12
stumpy is on a distinguished road
The inside() function returns 0 or 1 - I was assuming this was enough for CFX to evaluate if it's true of false, but perhaps not. Try if(inside()@subdomain1 > 0.5, ....
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
air bubble is disappear increasing time using vof xujjun CFX 9 June 9, 2009 07:59
why did my time interval set for output nouse? ShFlow FLOW-3D 2 January 11, 2009 21:25
IcoFoam parallel woes msrinath80 OpenFOAM Running, Solving & CFD 9 July 22, 2007 02:58
Repeating same time steps (FSI). cjtune CD-adapco 0 February 20, 2003 00:05
unsteady calcs in FLUENT Sanjay Padhiar Main CFD Forum 1 March 31, 1999 12:32


All times are GMT -4. The time now is 23:42.