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

Convergence but incorrect results in Free Surface flow

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

Reply
 
LinkBack Thread Tools Display Modes
Old   October 17, 2011, 10:43
Default Convergence but incorrect results in Free Surface flow
  #1
New Member
 
Join Date: Oct 2011
Location: Netherlands
Posts: 6
Rep Power: 6
fmjb is on a distinguished road
Dear all,

I'm new to the CFD-online forum, so if this new thread does not meet the requirements, please let me know, I am happy to adjust this ask for your help.

Currently i'm working on the resistance analysis of the the free surface flow around a wigley hull in ANSYS workbench 2.0 framework V13.0.0

A geometry containing both water and air domain is imported. This is a cube of 4*L long, 2*L wide water depth of 1*L and a heigth of 1/2*L. Here L is the boat length, which is for this case 2.5 meter.

the mesh is made with meshing 13.0.
Mesh Method: patch conforming Method, thetrahedrons.
Face sizing is added at the hull. where the element size is set to .02 meter. elsewhere, min sizi is .100 meter and max face size = max size = 0.250 meter. Inflation is applied to the hull. The first layer height is .001 meter, max layers is 5
This leads to a mesh with 764406 elements

The boundary conditions are accordingly to the free surface flow tutorial (flow over a bump), including the mesh adaption, The physical timestep is adjusted to 0.05s, and the maximum number of iterations to 1000. The advection scheme is set to upwind. I use the k-epsilon turbulence model with scalable wall function, and the intensity is set to medium.

after about 470 iterations convergence is reached.

The total force in x-direction is -5.2 Newton, which is equal to a total resistance coefficient of 0.0073. According to the paper The summary of cooperative experiments in wigley parabolic model in Japan by Kajitani et al (1983), the resistance coefficient should be around 0.0046.

Now I am wondering how a physical realistic result can be obtained. I don't know how i can diagnose the problem, so any help in this direction is highly appreciated.

If more details are required, please let me know.

Regards,

Friso
fmjb is offline   Reply With Quote

Old   October 17, 2011, 17:19
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,401
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Your question is a FAQ:

http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   October 18, 2011, 03:32
Default Mesh Refinement Error
  #3
New Member
 
Join Date: Oct 2011
Location: Netherlands
Posts: 6
Rep Power: 6
fmjb is on a distinguished road
Dear Gorrocks,

Thanks for your reply. As I understand, the aproach to this problem is based on trial-and-error (sensitivity analysis)? there are no ways to diagnose possible causes to this result?

I started with coarsening the mesh I use

the mesh is made with meshing 13.0.
Mesh Method: patch conforming Method, thetrahedrons.
Face sizing is added at the hull. where the element size is set to .02 meter. elsewhere, min sizi is .100 meter and max face size = max size = 0.400 meter. Inflation is applied to the hull. The first layer height is .001 meter, max layers is 5
This leads to a mesh with 697860 elements

When the mesh is refined (after about 80 iterations), The following error is returned:

-----------------------------------------------------------
Refiner 13.0 [2010.10.01-23.02]
Adaption step 1 of 2.
10374 prismatic stacks have been identified in the original mesh.
Maximum height = 5
Minimum height = 1

Marking elements for coarsening and refinement:
~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~~
Number of elements initially marked for refinement: 656842
Number of elements removed because:
They already meet the minimum length criteria: 0
They are in regions not marked for refinement: 0
They are already in the deepest refinement level: 0
There are not enough nodes available to refine them: -565904
----------
Number of elements actually marked for refinement: 90938
----------
Target number of nodes at end of step: 446428
Assertion failed: success && noOfSides == 4, file d:\builds\v130\cfx\src\refiner\src\elements\TriCol umn.ixx, line 669
This application has requested the Runtime to terminate it in an unusual way.
Please contact the application's support team for more information.
+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX mesh refiner exited with return code 3. |
+--------------------------------------------------------------------+

-----------------------------------------------------------------

Searching for this error on google did not give very helpfull hits. Does anyone have a clue about the cause of this error (and if it might be the cause to the inaccurate results?)

Regards,

Friso
fmjb is offline   Reply With Quote

Old   October 18, 2011, 06:22
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,401
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
As I understand, the aproach to this problem is based on trial-and-error (sensitivity analysis)? there are no ways to diagnose possible causes to this result?
Sensitivity analysis is trial and error? I do not think you understand it. You systematically vary each tunable parameter until you find settings where you prove your solution is accurate. No trial and error in that at all.

Some general comments:
* upwind advection is too diffusive. You will never get accurate results with that.
* You have not stated your Re number but for many boat flows you need a turbulence transition model with the SST turbulence model. k-e is probably over-predicting drag.
* I would not use auto mesh refinement for a model like this. I would manually mesh a series of high quality meshes for the mesh sensitivity study. Mesh quality will be important.
* Does the hull rise due to the motion? Have you correctly positioned the hull for that?
ghorrocks is offline   Reply With Quote

Old   October 21, 2011, 10:30
Default
  #5
New Member
 
Join Date: Oct 2011
Location: Netherlands
Posts: 6
Rep Power: 6
fmjb is on a distinguished road
Thank you for your advice.

I changed the upwind advection to high resolution, and changed to the SST turbulence model.
The meshrefinement is removed. To get a good resolution in vertical (Z)direction I did the following:
  • Split the domain in two bodies using CAD at the desing water line (Z=0)
  • add share topology in the DesignModeler
  • inflate into both bodies from the splitplane
  • Add a domain interface as boundary condition with automatic mesh connection
In combination with the inflation at the surface of the hull, this gives the mesh as shown in following figure
20111021SSTwaterlineproblem.jpg
The purple grid is the mesh in the YZ-plane. To put things in perspective a large scale image is added.

The problem becomes clear from this figure as well. The red line is the intersection of the water surface and the surface of the hull. Discontinuities appear at the plane Z=0. It appears that the solutions is different in both domains.

It is likely that this is caused by a wrong alligned mesh or wrong connection between the two domains. In the following figure the mesh at the lower plane of the upper domain is shown in blue, and the mesh at the upper plane of the lower domain is shown in red.
20111021SSTmeshmismatch.jpg

Could the misalignment in the mesh be the problem?
Could the discontinuity be caused by something else than a misalignment in the mesh
How can I solve this?

Regards,

Friso
fmjb is offline   Reply With Quote

Old   October 22, 2011, 06:01
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,401
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
A GGI interface can handle a mismatch between different sides of the interface.

If you are running this model at Re where turbulence transition is significant then you will need the turbulence transition model.
ghorrocks is offline   Reply With Quote

Old   October 25, 2011, 03:55
Default Domain Interface setting
  #7
New Member
 
Join Date: Oct 2011
Location: Netherlands
Posts: 6
Rep Power: 6
fmjb is on a distinguished road
I applied the GGI interface, and somehow the problem appears to persist. 20111025SST_WVF.jpg
in the figure you can see the water volume fraction in the YZ-plane. It shows a sharp gradient in the volume fraction at Z=0.

Is this caused by rendering, or is this the real solution?
what additional setting could solve this? Would setting intersection control yield an improvement? What is the preferred method, Bitmap or Direct?

Regards,

Friso
fmjb is offline   Reply With Quote

Old   October 25, 2011, 04:24
Default move interface
  #8
New Member
 
Join Date: Oct 2011
Location: Netherlands
Posts: 6
Rep Power: 6
fmjb is on a distinguished road
Should I move the interface between the two domains away from the free surface?

Will the GGI interface work in a region that does not intersect the free surface?

Regards,

Friso
fmjb is offline   Reply With Quote

Old   October 25, 2011, 05:56
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,401
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
The sharp gradient you are seeing is just an artifact of the post processing interpolation inside an element.

And Friso raises a critical point - you should not put a GGI interface on the free surface. You want the free surface to be as accurately resolved as possible and that means moving GGIs away from it.

Why do you have a GGI anyway? You should be able to mesh this as a single block.
ghorrocks is offline   Reply With Quote

Old   October 26, 2011, 03:51
Default vertical resolution Free Surface
  #10
New Member
 
Join Date: Oct 2011
Location: Netherlands
Posts: 6
Rep Power: 6
fmjb is on a distinguished road
Dear Ghorrocks,

The choice to mesh this as two blocks stems from using the mesher of Ansys workbench. To increase the vertical resolution I decided to apply inflation in the region of the free surface. As far I'm concerned a face is required to appy inflation. Therefore I splitted the domain in two parts, creating the possibility to apply inflation, but also introducing the need of an interface between the two domains.

Currently I'm moving the interface to a plane just below the hull. Im happy to hear if it is possible to apply a high vertical resolution at the free surface with another method.

Suggestions for creating the mesh, especially around the free surface are welcome. I'm not particularly happy with the mesh as it is right now (see also the images in my post of October 21, 2011 16:30.

Regards,

Friso
fmjb is offline   Reply With Quote

Old   October 26, 2011, 07:18
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 12,401
Rep Power: 97
ghorrocks is a jewel in the roughghorrocks is a jewel in the roughghorrocks is a jewel in the rough
Quote:
As far I'm concerned a face is required to appy inflation.
Yes, but you can make it a continuous mesh by joining the two blocks into a part. Then it comes into CFX-Pre as a single block and you have no need for a GGI.

Putting a GGI at the interface is a really bad idea.
ghorrocks is offline   Reply With Quote

Reply

Tags
free surface flow, hull, mesh, turbulence, wigley

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
Free surface flow settubg boundary conditions and plotting velocity profiles prashanthreddyh FLUENT 2 October 21, 2015 09:58
Free surface flow over a bump qtian OpenFOAM Running, Solving & CFD 17 August 10, 2010 10:15
free surface flow same as FSI??? Ken CFX 1 February 18, 2008 20:43
CFX 4.4 New free surface option Viatcheslav Anissimov CFX 0 April 3, 2002 06:27
free convection heat transfer from a heated horizontal surface through a liquid to a thin cooled fin Kaushik FLUENT 1 May 8, 2000 06:47


All times are GMT -4. The time now is 16:23.