CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Convergence but incorrect results in Free Surface flow (http://www.cfd-online.com/Forums/cfx/93488-convergence-but-incorrect-results-free-surface-flow.html)

fmjb October 17, 2011 10:43

Convergence but incorrect results in Free Surface flow
 
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

ghorrocks October 17, 2011 17:19

Your question is a FAQ:

http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

fmjb October 18, 2011 03:32

Mesh Refinement Error
 
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

ghorrocks October 18, 2011 06:22

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?

fmjb October 21, 2011 10:30

2 Attachment(s)
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
Attachment 9644
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.
Attachment 9645

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

ghorrocks October 22, 2011 06:01

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.

fmjb October 25, 2011 03:55

Domain Interface setting
 
1 Attachment(s)
I applied the GGI interface, and somehow the problem appears to persist. Attachment 9712
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 October 25, 2011 04:24

move interface
 
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

ghorrocks October 25, 2011 05:56

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.

fmjb October 26, 2011 03:51

vertical resolution Free Surface
 
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

ghorrocks October 26, 2011 07:18

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.


All times are GMT -4. The time now is 22:59.