CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Y plus (http://www.cfd-online.com/Forums/cfx/23122-y-plus.html)

anna September 29, 2006 09:37

Y plus
 
Dear all,

Through a tube with inner diameter 0.1m, is flowing water with a constant flow rate. Inside of tube is placed a magnetic coil with outer diameter 0.08 m. The Y plus next to the coil surface is about 3.7 and next to the tube inner wall is 13. Can I assume that the results from a simulation performed according to SST model will be correct? Thanks for your opinion. Anna

Joe September 29, 2006 10:34

Re: Y plus
 
No. Read "modelling flow near the wall" in the manual.

TB October 1, 2006 20:20

Re: Y plus
 
Converged solution is NOT equal to correct solution.

You should verified and validate your solution. See Roache's book for details.

Roache, P.J., "Verification and validation in computational science and engineering", Hermosa Publishers, New Mexico, USA, 1998.

ben akih October 4, 2006 05:50

Re: Y plus
 
according to the manual reasonable results are only to be expected with y+ values of less than or equal to 1. and the cell expansion ratio should be at least less than 2. you have the option to refine your mesh and use sst or try k-e with wall function. as TB said converged does not imply physically correct. regards ben

Robin October 4, 2006 10:36

Re: Y plus
 
Hi Anna,

The SST model can use both linear and logarithmic wall functions. At very small Y+ (~1), the wall function is linear and you can essentially integrate right through the boundary layer (assuming you have enough nodes in the boundary layer and not just one element that is close to the wall). At Y+ larger than ~11, it uses a wall function. In between, it blends between the two.

Wall functions are OK if the boundary layer is in equilibrium (this is an essential assumption to the logarithmic profile). If that is the case, your set up is fine. Where this becomes problematic is when there are adverse pressure gradients and separation.

Even if your set up is OK, there is no guarantee that the solution is correct. There are many other factors that can affect accuracy, such as your boundary conditions, how well your CAD model and subsequent mesh reflect the real geometry, fluid property selection and other models. The only way to know for sure is to validate against known data.

Scary, but it's true. That said, what you observe in your simulation is probably approximately correct and can still reveal potential problems.

Regards, Robin


All times are GMT -4. The time now is 22:32.