CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Free Surface Question (http://www.cfd-online.com/Forums/cfx/23044-free-surface-question.html)

Joe September 11, 2006 10:27

Free Surface Question
 
Hi,

I am running a free surface simulation of a hull (Steady state) and I observe the drag coefficient as means of convergence.

1. My rediduals are higly oscilatory and in the manual i saw that it might be the lenght ratio so from 180 i minimize it to 82. There are still some oscilation for maybe 300 iterations, stopping and then again the same. Does my edge to length ratio is high or OK?

2. I observe the drag coefficient and instead of converging towards about 0.02, it converges towards 0 where i dont know why.

Can anyone help me in the above questions? Thanks in advance. Joe

Joe September 11, 2006 11:00

Re: Free Surface Question
 
Post a cross section of your mesh including the boundayr layer.

And name yourself Joe2 or something ... its called forum ettiquette.

Charles September 11, 2006 12:46

Re: Free Surface Question
 
Which version of CFX are you using? For this kind of flow there is a big difference between even CFX10 & CFX11


JoeSa September 11, 2006 13:45

Re: Free Surface Question
 
Hi again,

I am using CFX 5.7, unfortunately I dont have 10 or 11. I am using this version in the university.

Here are some picts of my mesh:

This is at inlet http://img235.imageshack.us/img235/9915/inletqt8.png

At symmetry plane http://img218.imageshack.us/img218/1492/symper2.png

Top http://img235.imageshack.us/img235/2202/toplc8.png

Cross-section at mid-hull http://img218.imageshack.us/img218/8...sectionwq4.png

Any advice to try is welcomed. Thanks in advance, JoeSa

Charles September 11, 2006 14:00

Re: Free Surface Question
 
Your mesh looks OK, maybe just a little coarse at midship. Get the university to obtain and install CFX11. There are crucial differences in the way it deals with free surface calculations.

Joe September 11, 2006 15:34

Re: Free Surface Question
 
Doing a free surface flow with CFX 5.7 is going to be difficult convergence wise. Start simple e.g. 2D and work up from there ...

These are three obvious issues that could cause convergence problems: -The flow isnt really steady state. This can be tested with a trasient trial run. Look for dramatically improved convergence. -You only seem to be selectively resolving the boundary layer. Read the help section "Modelling flow near the wall" and adjust your grid accordingly. -There appear to be extreme cell size gradients in your mesh e.g. in your last pic at the bottom right corner of the hull. Use the hexa smoothing algorithms in Edit mesh to improve your mesh quality. And open the .def file inside CFX post to calculate and visualise the local mesh quality variations.


JoeSa September 12, 2006 06:23

Re: Free Surface Question
 
Thanks for your answers.

The mesh calculator gives the following for my mesh..

Element volume ratio 1(min) - 1.77353(max) Connectivity number 1(min) - 8(max) Edge Length ratio 1.069(min)- 92.80(max) Min face angle 33.123(min) - 90(max) MAx face angle 90(min) - 146.912(max)

Do these values seem OK? According to the manual they are within the limit of CFX.

Also my Y+ is between 50 and 90.

Regards. JoeSa

Joe September 12, 2006 08:04

Re: Free Surface Question
 
The mesh values look fine assuming the high edge length ratio is not at an important part of the flow, or is from the first layer of the boundary layer.

Im not familiar with hull boundary layer best practice so I wont comment on your y+ values. Google for 'marine 'best practice" cfd'

As regards the poor convergence I would suggest trouble shooting with a 2D model located on the longitudinal centreplane of the hull. Use that to develop a properly converging command file and then apply it to the 3D geometry.

JoeSa September 12, 2006 09:16

Re: Free Surface Question
 
Thanks Joe I ll try that and post any problem or success i have.

I would like to set the timestep be controled by the Courant number. Say I want Courant to be 0.9 then

dt=0.9*(minimum cell length) / (maximum velocity)

but I cant see any variable names within CFX to use, or do i have to create my own?

For the maximum velocity is it the inlet velocity or the max domain velocity? The min element length is it incorporated within CFX or have to calculate from my grid?

Thanks, JoeSa

Joe September 12, 2006 14:07

Re: Free Surface Question
 
Easy ...

Simulation type > Transient > Time steps > Adaptive > Time step adaption > RMS/MAX Courant number


All times are GMT -4. The time now is 02:40.