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

FSI-Oscillating Flexible Fin

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

Like Tree1Likes
  • 1 Post By stumpy

Reply
 
LinkBack Thread Tools Display Modes
Old   August 25, 2011, 00:58
Question FSI-Oscillating Flexible Fin
  #1
New Member
 
Join Date: Aug 2011
Posts: 4
Rep Power: 7
Mid Grove is on a distinguished road
Dear all

Iím researching a propulsion mechanism in fluid using an oscillating fin. Iím trying to simulate a 2 - way FSI simulation (2D) of an oscillating flexible fin. The objective is to achieve the thrust force generated by oscillating the fin.

This approach is similar to Tutorial No. 23 Oscillating Plate.

The flexible fin system consists of some materials as shown in the attached image. And the fin has been modeled as solid body in DM. The fluid domain is rectangular cuboid.
The setup conditions of Mechanical ADPL and CFX were as follows.

< Mechanical ADPL >
Analysis Settings
-Step End Time: 6s,
-Auto Time Stepping: On
-Define by: Sub Steps
-Initial Sub Step: 1
-Minimum Sub Step: 1
-Maximum Sub Step: 10

Remote Displacement
Scope
-Coordinate System: Global Coordinate System
(The z-axis is the same as the rotational axis)
Definition
-Rotation Z: 4.e0*atan(1.e0))/6*sin(2*(4.e0*atan(1.e0))/3*time

<CFX>
Total Time: 6s, Time step: 0.001s
Coupling Data Transfer Control
-Under Relaxn. Fac.: 0.3
-Convergence Target: 1e-5

I received the error message that the fatal error occurred when requesting Total Mesh Displacement for FF when simulation time = 0.256s. FF is FSI interface. And also the image of mesh deformation right before the error message had occurred (simulation time = 0.255s) was attached.

I estimate that this error was caused by less-accuracy mesh of structure. I next created finer mesh of structure and simulated. However, the same error message as the above occurred. Therefore, I stopped the simulation right before the error message had occurred. By the simulation results, the gap between the interface of structure (Mechanical ADPL) and that of fluid (CFX) was occurred. This is first question: Why does the gap between those interfaces occurred?

I created some mesh of structure and fluid using ANSYS Meshing for improving the accuracy of the mesh and simulated using those meshes. The tendency for the mesh deformation for each time step decreased by fining of the mesh was observed from those results.
Next question: How is the mesh set to improve both the value of mesh deformation for each time step and the mesh accuracy?

Any help will be very much appreciated. Thanks in advance.


Mid Grove
Attached Images
File Type: jpg Structual.jpg (94.2 KB, 104 views)
File Type: jpg Mesh Deformation.jpg (94.3 KB, 103 views)
File Type: jpg Fluid mesh.jpg (93.0 KB, 94 views)
Mid Grove is offline   Reply With Quote

Old   September 15, 2011, 04:48
Default
  #2
New Member
 
Join Date: Jul 2010
Posts: 22
Rep Power: 8
Vinzent is on a distinguished road
hi,
try different meshstiffnesses. the gap region (connection) should be softer than the surrounding.
vinzent
Vinzent is offline   Reply With Quote

Old   September 15, 2011, 21:23
Default
  #3
Senior Member
 
Bruno
Join Date: Mar 2009
Location: Brazil
Posts: 273
Rep Power: 13
brunoc is on a distinguished road
Use a fixed timestep for the structural side of your simulation. The timescale for the fluid simulation is probably smaller anyway. Then play with the mesh stiffness on CFX. Use the option where stiffness if bigger near walls or boundary conditions.
brunoc is offline   Reply With Quote

Old   September 16, 2011, 16:48
Default
  #4
Senior Member
 
Join Date: Apr 2009
Posts: 530
Rep Power: 13
stumpy is on a distinguished road
As bruno said get rid of the auto timestepping in ANSYS and just use 1 substep. Your under relaxation factor of 0.3 is also very small. This means CFX only gets 30% of the change in displacement from ANSYS each coupling iteration, so you'll need a lot of coupling iterations to get the meshes to match up.
stumpy is offline   Reply With Quote

Old   September 21, 2011, 04:24
Default
  #5
New Member
 
ST
Join Date: Sep 2010
Posts: 9
Rep Power: 7
bbhv is on a distinguished road
have you checked your scaling?
especially when you import the geometry from another software.
i experienced it once, the design modeller scaled the model automatically.
so, make sure they are the same in the structural and fluid models.
bbhv is offline   Reply With Quote

Old   February 13, 2012, 23:42
Default
  #6
New Member
 
Join Date: Aug 2011
Posts: 4
Rep Power: 7
Mid Grove is on a distinguished road
Thanks all.
I tried simulations in some different conditions. In the results, it succeeded by setting up as follows.
< Mechanical ADPL>
Analysis Setting
-Step End Time: 6s
-Auto Time Stepping: Off
-Define by: Substeps
-Number of substeps; 1
<CFX>
Total Time: 6s, Time step: 0.01s
Mesh stiffness: 1000[m^5 s^-1] / (max (0.1[mm], wall distance)^3
Under relaxation factor: 0.30 (minimum iteration: 3, maximum iteration: 30)
Convergence Target: 0.01
And crushing of a mesh was prevented by making a sliding interface in the fluid around a fin. But, Computational time is too long and is troubled.
Please teach me how to decrease computational time? Computational time has taken no less than 12 days.

Last edited by Mid Grove; February 14, 2012 at 03:46.
Mid Grove is offline   Reply With Quote

Old   February 14, 2012, 12:17
Default
  #7
Senior Member
 
Join Date: Apr 2009
Posts: 530
Rep Power: 13
stumpy is on a distinguished road
Use an under relaxation of 0.75 or higher, so fewer coupling iterations are needed. If this is unstable, then use an under relaxation factor of 1 then add a 'mass flux pressure coefficient' on the FSI boundary on the Source tab. If you have access to the ANSYS Customer Portal then you can see how this works by searching for "FSI" in the knowledge resource section (it's the first hit).
mvoss likes this.
stumpy is offline   Reply With Quote

Old   September 24, 2012, 23:59
Default
  #8
New Member
 
Join Date: Aug 2011
Posts: 4
Rep Power: 7
Mid Grove is on a distinguished road
Thanks stumpy.
I'm sorry I have much slower response.
Using the mass flux coefficient, calculation is finished in two days.
Mid Grove is offline   Reply With Quote

Reply

Tags
fsi, interface, mesh deformation, oscillation

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
The problem of inner iteration when calling the subroutine guoxj CFX 18 October 23, 2010 20:37
Fin inside supersonic flow Liol Calvert FLUENT 8 March 22, 2010 10:31
BCs in an FSI simulation of a flexble pipe vivekcfd OpenFOAM 10 January 8, 2010 05:14
FSI oscillating plate spatialtime CFX 4 April 29, 2009 15:04
how to extend FSI 2D codes to 3D, need advises abouziar Main CFD Forum 1 May 30, 2008 04:08


All times are GMT -4. The time now is 03:40.