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

FSI of a hydrofoil- MESH deforamtion issue

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

Reply
 
LinkBack Thread Tools Display Modes
Old   November 30, 2017, 11:06
Default FSI of a hydrofoil- MESH deforamtion issue
  #1
Member
 
Join Date: Jun 2009
Location: CANADA
Posts: 63
Rep Power: 11
mortazavi is on a distinguished road
Hi,
i am silumating fsi of a 3D hydrofoil at high Re numbers.
The simulation is unsteady, however i only look at the staedy-state final results.
the simulation converges to 2e-4 but the issue is that the final solution is on a low-quality mesh because of the deformation of hydrofoil.
The picture is attached to post.
Any idea to avoid low-quality final mesh???thanks
Attached Images
File Type: jpg Untitled.jpg (191.0 KB, 18 views)
mortazavi is offline   Reply With Quote

Old   November 30, 2017, 16:16
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,003
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
First thing to try is to adjust the mesh smoothing parameters in the moving mesh options.

Then check the mesh smoothing equations are accurately resolved - try tightening the mesh smoothing convergence tolerance.

If that does not work you might need to consider dynamic remeshing.
ghorrocks is online now   Reply With Quote

Old   December 1, 2017, 09:44
Default
  #3
Member
 
Join Date: Jun 2009
Location: CANADA
Posts: 63
Rep Power: 11
mortazavi is on a distinguished road
Dear ghorrocks, thanks for your helpful comment.
for the first and second comments i have found enough documents.
could you please intoduce me a good reference or tutorial for dynamic remeshing? cfx help is not helping me.

Quote:
Originally Posted by ghorrocks View Post
First thing to try is to adjust the mesh smoothing parameters in the moving mesh options.

Then check the mesh smoothing equations are accurately resolved - try tightening the mesh smoothing convergence tolerance.

If that does not work you might need to consider dynamic remeshing.
mortazavi is offline   Reply With Quote

Old   December 1, 2017, 18:56
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,003
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
There are examples on dynamic remeshing in ICEM on the ANSYS customer webpage.
ghorrocks is online now   Reply With Quote

Old   December 7, 2017, 13:16
Default
  #5
Member
 
Join Date: Jun 2009
Location: CANADA
Posts: 63
Rep Power: 11
mortazavi is on a distinguished road
Hi ghorrocks,
Is dynamic remeshing supported with fsi in workbench?

Quote:
Originally Posted by ghorrocks View Post
There are examples on dynamic remeshing in ICEM on the ANSYS customer webpage.
mortazavi is offline   Reply With Quote

Old   December 7, 2017, 22:38
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,003
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
I am not sure, you will have to check. But I suspect you can do it.
ghorrocks is online now   Reply With Quote

Old   December 13, 2017, 12:15
Default
  #7
Member
 
Join Date: Jun 2009
Location: CANADA
Posts: 63
Rep Power: 11
mortazavi is on a distinguished road
hi ghorrocks,
remeshing is not applicable for fsi with cfx.
Another question; do you think if with using domain interface i can get rid of low quality mesh under the hydrofoil as depicted in this picture?
i mean a very fine mesh near the hydrofoil for the boundary layer elements and wake region, and coarser mesh far. in this case i can use stiffness increase near small volumes without any issues.
thanks

Quote:
Originally Posted by ghorrocks View Post
I am not sure, you will have to check. But I suspect you can do it.
Attached Images
File Type: jpg Untitled.jpg (194.5 KB, 5 views)
mortazavi is offline   Reply With Quote

Old   December 13, 2017, 16:35
Default
  #8
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,003
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Yes, using GGIs can help.

Some other comments:
* The mesh smoother should not do what you show when it is adjusted properly. Are you sure the mesh smoothing convergence tolerance is tight enough?
* Your mesh is also not ideal as you have high aspect ratio elements in the bulk flow. If you improved your mesh such that the high aspect ratio elements were only in the foil boundary layer that would improve things and probably help the mesh smoother as well.
ghorrocks is online now   Reply With Quote

Old   December 22, 2017, 10:28
Default
  #9
Member
 
Join Date: Jun 2009
Location: CANADA
Posts: 63
Rep Power: 11
mortazavi is on a distinguished road
Hi ghhorocks,
As you can see in the attached photo, my main issue now is in the wake region. so according to my supervisor's reccomendation, what i have to do is to define a CEL for the stiffness (increase near small vol). For now the exponent is a constant value. the foil moves up while the small volume elements in the wake region are stiff enough to stay in their initial position and don't move. So I have to decrese the exponent for X> X(TE).
for example exponent=0.2 but for X>X(TE) exponent=0.01.
Any idea please?
If you agree can you guide me to write this CEL?
thanks
Attached Images
File Type: jpg 2.jpg (192.4 KB, 4 views)
File Type: jpg 3.jpg (198.0 KB, 4 views)
mortazavi is offline   Reply With Quote

Old   December 22, 2017, 17:14
Default
  #10
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,003
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
What version of CFX are you using? Recent versions of CFX have much more options here than older versions.

I would have thought that simply increasing the mesh stiffness diffusion value in proximity of the foil would be best. This is a GUI option in recent versions of CFX.

And by the way: rapid changes in stiffness like you suggest are a bad idea because the mesh at the interface gets highly distorted. You need to gently ramp between values to avoid this.
ghorrocks is online now   Reply With Quote

Old   December 23, 2017, 23:18
Default
  #11
Member
 
Join Date: Jun 2009
Location: CANADA
Posts: 63
Rep Power: 11
mortazavi is on a distinguished road
ghorrocks Thanks,

I am using version 16. Could you please explain more about GUI option in your previous post?
by the way, as in the attached file, according to your recommendation i have created multiple zone in the foil and wake region to be able to define different stiffness for different domains. is that acceptable you think?
regards,
Attached Images
File Type: png CFX.png (79.3 KB, 4 views)
mortazavi is offline   Reply With Quote

Old   December 25, 2017, 03:04
Default
  #12
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 15,003
Rep Power: 115
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Yes, your regions should help. But still you will have to be careful about the transitions.

I am on holidays and away from my workstation so cannot look up the new options in current CFX versions for you.
ghorrocks is online now   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
Two-way FSI dynamic mesh issue khhan0543 FLUENT 0 January 31, 2017 00:31
Gambit problems Althea FLUENT 22 January 4, 2017 03:19
No layers in a small gap bobburnquist OpenFOAM Native Meshers: snappyHexMesh and Others 6 August 26, 2015 09:38
Issue with arbitrary Lagrangian-Eulerian method and mesh optimization mikolchon Main CFD Forum 0 August 16, 2014 15:50
fluent add additional zones for the mesh file SSL FLUENT 2 January 26, 2008 11:55


All times are GMT -4. The time now is 07:19.