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

Mesh Folding ... different experience!

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

Like Tree4Likes
  • 1 Post By p.galimutti
  • 1 Post By ghorrocks
  • 1 Post By ghorrocks
  • 1 Post By p.galimutti

Reply
 
LinkBack Thread Tools Display Modes
Old   May 25, 2012, 16:11
Default Mesh Folding ... different experience!
  #1
New Member
 
Pouya
Join Date: Feb 2012
Posts: 17
Rep Power: 5
Pouya is on a distinguished road
hello dear CFD-online users!


I want to study on interaction of marine risers and water flows surround them (FSI problem)! So I decided to use Ansys MFX capability, but now Iíve faced with some problems: mesh folding!


Iíve studied advices have been written on the forum, but somehow they are not very useful in my case. There are 3 main advices:


1)Increasing mesh quality: I think my mesh quality is ok!
2)Increasing mesh stiffness: I changed mesh stiffness near small volume (model component = 1000), but results didnít change!
3)Decreasing time steps: Iíve uploaded two of my out files here. It seems by decreasing time steps results don't change!


Let me know your idea please! Ö and another question: Does Ďunder relaxation factorí impress mesh folding? I set this factor to 0.5! Is it appropriate or not?


Thanks in advance Ö Pouya!
Attached Files
File Type: txt 1.txt (36.3 KB, 34 views)
File Type: txt 2.txt (35.7 KB, 17 views)

Last edited by Pouya; May 26, 2012 at 04:13.
Pouya is offline   Reply With Quote

Old   May 26, 2012, 05:42
Default
  #2
Member
 
Peter Galimutti
Join Date: May 2012
Posts: 37
Rep Power: 5
p.galimutti is on a distinguished road
You might have to change your mesh deformation to 'unspecified' for the regions that are connected to multifield region (wall). If you give 'stationary' option to the moving walls, the mesh will definitely fold.

Also, a model exponent of '1000' is of no use as the stiffness values range from 1e-15 - 1e15. So it doesn't matter how much exponent value you give. But first try the default 10 and then go for 20.

In the expert controls change 'mesh displacement diffusion' to value of 3.

depending on your elements monitor the orthogonal angle, which should be close to 90 for hex and close to 60 for tetra.

HTH
Pouya likes this.
p.galimutti is offline   Reply With Quote

Old   May 26, 2012, 06:01
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,935
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
Please post an image of what you are modelling and a description of the sorts of motion you expect to undergo.
Pouya likes this.
ghorrocks is offline   Reply With Quote

Old   May 27, 2012, 03:01
Default
  #4
New Member
 
Pouya
Join Date: Feb 2012
Posts: 17
Rep Power: 5
Pouya is on a distinguished road
Hi & Thanks for your responses!


I’m studying a vertical riser vortex induced vibrations (VIV) under sheared current. The riser was made of a 9.63m brass pipe with an outer diameter of 0.02m and a wall thickness of 0.45mm. It was pinned at its two ends and the tension imposed on the two ends was 817N. Dear Mr. Galimutti this is why I think surface and bottom of domain (which are connected to multi-field region) wouldn’t be affected by mesh deformation. I changed 'mesh displacement diffusion' to value of 3, but there was not a big change in results.


Dear Mr. Horrocks let me say about VIV phenomenon. When water flows around a cylindrical body like the riser, it separates around the surface of riser. It frequently does so in an alternating series of vortices called the von Karman vortex street. This is known as vortex shedding. The effect of these vortices is to exert alternating forces on either side of the riser. If the periodicity of these forces coincides with the natural frequency of the riser string, a powerful resonance can be set up.


I hopefully wait for your ideas.
Thank you!
Attached Images
File Type: jpg Domain.jpg (37.7 KB, 55 views)
File Type: jpg Surface Mesh.jpg (70.1 KB, 51 views)
File Type: jpg Vortex Shedding Behind a Circular Cylinder.jpg (35.6 KB, 34 views)
Pouya is offline   Reply With Quote

Old   May 27, 2012, 07:07
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,935
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I am well aware of von Karman vortex streets.

What motions does the cylinder possess? It sounds like there are no rotational modes. What about translational? X and Y (assumign flow in the X direction)? or just Y?
Pouya likes this.
ghorrocks is offline   Reply With Quote

Old   May 27, 2012, 07:46
Default
  #6
New Member
 
Pouya
Join Date: Feb 2012
Posts: 17
Rep Power: 5
Pouya is on a distinguished road
X is in the flow direction and Y is the cross flow direction. Z direction coincides with riser axis. Cylinder has no motion at first. Its transitional degrees of freedom are constrained at 2 ends in X and Y directions (and Z direction at lower end of riser) and the tension of 817N is imposed on upper end of riser in Z direction. Rotational degrees of freedom are available at constraints. After vortex shedding riser would start to vibrating in both X and Y directions.

Last edited by Pouya; May 27, 2012 at 08:10.
Pouya is offline   Reply With Quote

Old   May 27, 2012, 18:11
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,935
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
I see. How big are the motions relative to the cylinder diameter? Also, you say rotation is not constrained - does that mean the cylinder can rotate about its axis or some other axis?
ghorrocks is offline   Reply With Quote

Old   May 28, 2012, 03:41
Default
  #8
New Member
 
Pouya
Join Date: Feb 2012
Posts: 17
Rep Power: 5
Pouya is on a distinguished road
Thank you for your reply! Yesterday, after your post, I tried my solid model without any rotational degrees of freedom. Unfortunately results were the same.
I post the RMS A/D ( normalized instantaneous vibration amplitude) pattern of cross-flow response along the riser in the case of sheared current of U2=0.42 m/s and U2=0.84 m/s (These figures have been extracted from a paper written by Huang, Ching Chen & Rong Chen!!!). I ‘ve no more information about flow direction motions of riser.
Thanks for your promising responses!
Attached Images
File Type: jpg CF Response U2=0.42.jpg (35.5 KB, 21 views)
File Type: jpg CF Response U2=0.84.jpg (34.4 KB, 17 views)
File Type: jpg U2=0.42 After 8s.jpg (88.3 KB, 24 views)
File Type: jpg U2=0.84 After 8s.jpg (94.7 KB, 16 views)
File Type: jpg Velocity Profile.jpg (7.4 KB, 12 views)

Last edited by Pouya; May 29, 2012 at 02:06.
Pouya is offline   Reply With Quote

Old   May 28, 2012, 06:13
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,935
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
The charts do not define the variables so I do not know what they are referring to.

But it is starting to look like this case is best done by a region around the cylinder which is quite stiff, so the motion can be absorbed by the larger mesh elements further out. You can do this with things like a mesh motion stiffness parameter which is a function of distance from the wall.
ghorrocks is offline   Reply With Quote

Old   May 29, 2012, 07:21
Default
  #10
New Member
 
Pouya
Join Date: Feb 2012
Posts: 17
Rep Power: 5
Pouya is on a distinguished road
Thank you Mr. Horrocks for your patience!
As you said I changed my stiffness. I used this function: [1/wall distance], but mesh folding occurred again!
I changed my solid model and increased number of elements but results didn't change!
These are pictures of Interface region after mesh folding!

& another mesh stiffness function: [1/wall distance^2]. I tried it and I faced this problem: DIVIDE-BY-ZERO
Attached Images
File Type: jpg Interface Region 1.jpg (28.4 KB, 38 views)
File Type: jpg Interface Region 2.jpg (28.4 KB, 34 views)
Attached Files
File Type: txt Fluid_001.txt (37.2 KB, 15 views)
Pouya is offline   Reply With Quote

Old   May 29, 2012, 07:30
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,935
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
What do those images show? I have no idea what that is.

Have you tried a smaller time step?
ghorrocks is offline   Reply With Quote

Old   May 29, 2012, 16:40
Default
  #12
Member
 
Peter Galimutti
Join Date: May 2012
Posts: 37
Rep Power: 5
p.galimutti is on a distinguished road
What was your minimum orthogonal quality? You can see the 'min orthogonal quality' values in the monitors. Minimum orthogonal quality decrease with iterations or time (if it's transient) and once it falls below 5 or 6 you'll likely have mesh folding.
Pouya likes this.
p.galimutti is offline   Reply With Quote

Old   May 31, 2012, 07:56
Default
  #13
New Member
 
Pouya
Join Date: Feb 2012
Posts: 17
Rep Power: 5
Pouya is on a distinguished road
Thank you for your help! I tried your ideas, but I still face the same problem! I decreased time steps ... I found out smaller time steps would result in larger "negative SECTOR volume" and "negative ELEMENT volume"! I even tried larger time steps!!! Time steps larger than 0.025 sec would result in "Floating point exception: Overflow" error!
I tried coarse elements and decreased mesh density near solid boundary. According to mesh statistics (out file) minimum Orthogonality Angle in my case is 60.6 [deg].
I'm really confused!

Last edited by Pouya; June 1, 2012 at 01:40.
Pouya is offline   Reply With Quote

Old   May 31, 2012, 14:04
Default
  #14
Member
 
Peter Galimutti
Join Date: May 2012
Posts: 37
Rep Power: 5
p.galimutti is on a distinguished road
Minimum orthogonal quality of 60 is good. what kind of wall boundary condition you used at the top surface, is it given multi-field too? i guess, due to tension the solid deforms in Y and hence shall the fluid. from what you said you only gave multi-field to surface and bottom walls. I believe the top one is causing problems. When you see negative volume elements you should be able to see the locations. See where in you model negative elements are developing?
p.galimutti is offline   Reply With Quote

Old   May 31, 2012, 16:13
Default Problem in solving ansys FSI tutorial
  #15
New Member
 
Yogesh Sukal
Join Date: May 2012
Posts: 1
Rep Power: 0
yogi is on a distinguished road
hello everyone,
I am solving ansys tutorial to learn FSI, but in upto structural setup i solved it correctly but when i started with ansys cfx, pick face command is showing inactive which i want to create named selections.
any body please help me sort out this problem.
yogi is offline   Reply With Quote

Old   June 5, 2012, 03:00
Default
  #16
New Member
 
Pouya
Join Date: Feb 2012
Posts: 17
Rep Power: 5
Pouya is on a distinguished road
Hi everyone!
In the past few days I did something: I increased time steps to a value of 0.018 sec & changed turbulence model to SAS SST. My model used to crash after the first stagger iteration but now it works for the second stagger iteration and then it crashes. So I can check mesh quality after first stagger iteration! You were right Mr. Galimutti. It sees not very good!

+--------------------------------------------------------------------+
| Mesh Statistics |
+--------------------------------------------------------------------+
| Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio |
+----------------------+---------------+--------------+--------------+
| | Minimum [deg] | Maximum | Maximum |
+----------------------+---------------+--------------+--------------+
| Default Domain | 69.0 OK | 10 ok | 97 OK |
+----------------------+---------------+--------------+--------------+
| | %! %ok %OK | %! %ok %OK | %! %ok %OK |
+----------------------+---------------+--------------+--------------+
| Default Domain | 0 0 100 | 0 1 99 | 0 0 100 |
+----------------------+---------------+--------------+--------------+

after first stagger iteration:

+--------------------------------------------------------------------+
| Mesh Statistics |
+--------------------------------------------------------------------+
| Domain Name | Orthog. Angle | Exp. Factor | Aspect Ratio |
+----------------------+---------------+--------------+--------------+
| | Minimum [deg] | Maximum | Maximum |
+----------------------+---------------+--------------+--------------+
| Default Domain | 29.8 ok | 10 ok | 540 ok |
+----------------------+---------------+--------------+--------------+
| | %! %ok %OK | %! %ok %OK | %! %ok %OK |
+----------------------+---------------+--------------+--------------+
| Default Domain | 0 1 99 | 0 1 99 | 0 1 99 |
+----------------------+---------------+--------------+--------------+

I guess I have to change my mesh. I will write about the results.

Thanks!
Pouya is offline   Reply With Quote

Old   June 5, 2012, 09:54
Default one possible FSI folding mesh solution
  #17
Member
 
Nick Cleveland
Join Date: Mar 2012
Posts: 34
Rep Power: 5
NCle is on a distinguished road
Hi Pouya,

I recently had the same folding mesh "error 3840" problem. It was caused by the numerical instability of the fluid and solid "bouncing" back and forth with increasing amplitude until divergence and the wild mesh distortions you see.

What fixed it for me was the knowledge resource video "2022119 - Stabilizing strongly coupled 2-way FSI simulations between FLUENT or CFX and Mechanical" Hope it works for you. You have to use trial and error to find just the right amount of damping so that it converges but also gets an accurate solution, I believe.

My model is much smaller and liquid much more viscous than yours, but it could still work.
NCle is offline   Reply With Quote

Reply

Tags
mesh folding, mfx

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
Mesh motion with Translation & Rotation Doginal CFX 2 January 12, 2014 07:21
Icemcfd 11: Loss of mesh from surface mesh option? Joe CFX 2 March 26, 2007 18:10
Gambit problems Althea FLUENT 21 February 6, 2001 08:05
Mesh for 3 dim Geometry Phil FLUENT 9 July 12, 2000 04:39
unstructured vs. structured grids Frank Muldoon Main CFD Forum 1 January 5, 1999 11:09


All times are GMT -4. The time now is 04:57.