# Error solving free surface flow on Wigley hull

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

 September 7, 2015, 21:49 Error solving free surface flow on Wigley hull #1 New Member   Daniel Coelho Join Date: Mar 2012 Posts: 9 Rep Power: 13 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

 September 7, 2015, 22:46 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,323 Rep Power: 138 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.

 September 7, 2015, 23:25 #3 New Member   Daniel Coelho Join Date: Mar 2012 Posts: 9 Rep Power: 13 Thank you for your reply, I'll try to use that!

 September 14, 2015, 19:23 #4 New Member   Daniel Coelho Join Date: Mar 2012 Posts: 9 Rep Power: 13 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

 September 14, 2015, 19:28 #5 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,323 Rep Power: 138 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

 September 14, 2015, 19:34 #6 New Member   Daniel Coelho Join Date: Mar 2012 Posts: 9 Rep Power: 13 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.

 September 14, 2015, 21:30 #7 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,323 Rep Power: 138 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?

 September 15, 2015, 00:03 #8 New Member   Daniel Coelho Join Date: Mar 2012 Posts: 9 Rep Power: 13 What could you suggest for free surface parameters? I cannot find enough information on ANSYS HELP.

 September 15, 2015, 00:32 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,323 Rep Power: 138 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.

 September 21, 2015, 12:31 #10 New Member   Daniel Coelho Join Date: Mar 2012 Posts: 9 Rep Power: 13 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

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

 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 OffTrackbacks are Off Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post prashanthreddyh FLUENT 2 October 21, 2015 10:58 devesh.baghel OpenFOAM 2 December 10, 2009 02:21 eee CFX 2 August 28, 2009 09:36 Ken CFX 1 February 18, 2008 20:43 Viatcheslav Anissimov CFX 0 April 3, 2002 07:27

All times are GMT -4. The time now is 06:52.