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

Error solving free surface flow on Wigley hull

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   September 7, 2015, 20:49
Exclamation Error solving free surface flow on Wigley hull
  #1
New Member
 
Daniel Coelho
Join Date: Mar 2012
Posts: 9
Rep Power: 12
dancoelhoptr is on a distinguished road
I was hoping for your help. I'm doing a multiphasic simulation with free surface of a Wigley hull. I started doing mesh convergence (comparing with experimental results) and when I do a finer mesh (maintaining the same mesh quality) the solver generates the "floating point error overflow", or it just converges from 1e-3 to 1e-8 in only one iteration which makes the results extremely strange.

I'm generating the mesh on ICEM CFD with hexaedral elems., SST turbulence model (in BC the turbulence intensity is 5%) and steady state. Here are the boundary conditions used:

-Inlet: Velocity inlet with Volume Fraction calculated with a step function;
-Outlet: Static pressure (hydrostatic pressure varying with coordinate z height);
-Top surface: Opening pressure with Entrainment option and pressure equals to 0 Pa. Pressure option: Opening Pressure. Turbulence: Zero Gradient.
-Symmetry

Initial conditions: Hydrostatic pressure varying with coordinate z height, Volume Fraction with step funcion and Velocity in coordinate x.

On Solver Control, I'm using High Resolution for both Advection Scheme and Turbulence Numerics. Volume Fraction Coupling: Coupled. And I tryed to change Timescale Control, to see if I could make the model convergence, but without success.

Here is the BC picture:
http://imagizer.imageshack.us/a/img913/3354/YieJiS.png

And the result for waterheight on the hull for the last mesh (you can see that the waterheight profile oscillates too much from 0.4 to 0.8 and I tried to get this better with a mesh convergence):
http://imagizer.imageshack.us/a/img537/3369/IPcDLt.png

And below the CCL file with the CFX-Pre options:

fig1.PNG

RESULT.png

CCL-file.txt
dancoelhoptr is offline   Reply With Quote

Old   September 7, 2015, 21:46
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Are you using double precision numerics? You will probably need it for the fine mesh cases.

Also: Are you running this steady state? Free surface models often need transient simulations to resolve the free surface perturbations as they have very little damping. Steady state cannot handle these very well with fine meshes.
ghorrocks is offline   Reply With Quote

Old   September 7, 2015, 22:25
Default
  #3
New Member
 
Daniel Coelho
Join Date: Mar 2012
Posts: 9
Rep Power: 12
dancoelhoptr is on a distinguished road
Thank you for your reply, I'll try to use that!
dancoelhoptr is offline   Reply With Quote

Old   September 14, 2015, 18:23
Default
  #4
New Member
 
Daniel Coelho
Join Date: Mar 2012
Posts: 9
Rep Power: 12
dancoelhoptr is on a distinguished road
Using double precision did work, but not for all meshes so, I raised the distance between the free surface and the top surface of the domain and changed the opening BC to free slip, and I don't have anymore convergece problems.
But, the waterheight profile remains almost the same even with a finer mesh.

Here is the waterheight profile:
figggg.PNG

I want something like this (someone knows the ANSYS wigley domain size or BC?):
ansys.jpg
dancoelhoptr is offline   Reply With Quote

Old   September 14, 2015, 18:28
Default
  #5
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Those charts look pretty similar to me. What is not correct about it?

But now this sounds like a question on general accuracy: http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F
ghorrocks is offline   Reply With Quote

Old   September 14, 2015, 18:34
Default
  #6
New Member
 
Daniel Coelho
Join Date: Mar 2012
Posts: 9
Rep Power: 12
dancoelhoptr is on a distinguished road
I've seen that FAQ dozens of times already. From what I've seen, everything is correct and I already tryed a lot of suggestions from other posts and the results remain the same.
dancoelhoptr is offline   Reply With Quote

Old   September 14, 2015, 20:30
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
When you are close but a bit off the expected answer there is no substitute but a careful analysis of all the key parameters. Have you looked at:
* domain depth, width, height
* free surface modelling parameters (smoothing etc)


And how much are you off by?
ghorrocks is offline   Reply With Quote

Old   September 14, 2015, 23:03
Default
  #8
New Member
 
Daniel Coelho
Join Date: Mar 2012
Posts: 9
Rep Power: 12
dancoelhoptr is on a distinguished road
What could you suggest for free surface parameters? I cannot find enough information on ANSYS HELP.
dancoelhoptr is offline   Reply With Quote

Old   September 14, 2015, 23:32
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,170
Rep Power: 134
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
All of them

I find the free surface model can be tuned for specific cases quite a bit, and some changes to the defaults can give significant improvements. But my method of finding the necessary changes is crude: Set up a quick benchmark case of your model and give every free surface option a try and adjust all tuneable parameters. Most will not do anything (so just leave them at defaults), some will wreck it, but a few will be a step forwards. If you have a good benchmark simulation and script all these permutations up you can run them quickly and sort out the ones worth investigating.
ghorrocks is offline   Reply With Quote

Old   September 21, 2015, 11:31
Default
  #10
New Member
 
Daniel Coelho
Join Date: Mar 2012
Posts: 9
Rep Power: 12
dancoelhoptr is on a distinguished road
I solved my problem. Now I am using Fluent with the following BC: pressure-inlet, pressure-outlet (in Fluent you can select pressure for both inlet and outlet BC in a VOF case because you set on the inlet a velocity for the fluid). For the external boundaries I am using wall BC.

The mesh must have numerical beach. The "numerical beach" is basically a very coarse mesh, with big jumps in cell size, near the external boundaries. It helps avoid wave reflection at the boundaries of your domain and therefore convergence issues. And now I get a smooth wave profile for the Wigley hull
dancoelhoptr is offline   Reply With Quote

Reply

Tags
cfx, floating point error, free surface, overflow, wigley hull

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
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
Problem with capturing water-spreading for free surface flow devesh.baghel OpenFOAM 2 December 10, 2009 01:21
Free - Surface Flow: Split Fluid Forces acting on a Boat Hull eee CFX 2 August 28, 2009 08:36
free surface flow same as FSI??? Ken CFX 1 February 18, 2008 19:43
CFX 4.4 New free surface option Viatcheslav Anissimov CFX 0 April 3, 2002 06:27


All times are GMT -4. The time now is 18:45.