Flat Plate Boundary Layer Height
 

Hi guys,

My first time posting in this forum. I have a question regarding my simulation of a flow over flat plate.
I have flow over flat plate with the following parameters:
1. Reference Length 230m
2. Reference Velocity 10
http://s18.postimg.org/e7tkxzc0l/Capture_2.jpg

I have tried my best to explain the boundary conditions in the diagram but the word explanation is as follow:

The flat plate portion is split into two portion, early part and later part and represented by the coloured portion of the bottom surface. The flat plate portion has wall function boundary condition. With the remaining bottom surface having boundary condition of SLIP.

The inlet and outlet are set as far field, with inlet being 240m away from the leading edge of flat plate, while the outlet is 230m away from the trailing edge of flat plate. The flat plate is 10m wide with the boundary condition of side wall closest to the flat plate being mirror, and the side wall 40m away from the flat plate set as far field.

The simulation is solved using K-Omega SST Menter.

The problem that I have now is that the boundary layer does not start at 0 at the leading edge. Does anyone has any idea what causes this issue? and how I can fix it?
Let me know if there is something that is unclear.
Thanks.

Additional info
 

The boundary layer is in the hundreds of micrometer, and the boundary layer starts around 1m away from the leading edge.

Hi
You are using a low Re turbulen e model while applying wall function.
You need to use a bery dense boundary layer mesh to resolve it properly. As kennedy mentioned, a one micrometer thickness is a good choice. Wall function uses some correlations to mimic the near wall gradients and usually work with low mesh densities near wall.

Dear Hamid,

Thank you for the reply. Thank you for the suggestion, that sounds like a solution to my problem. However, setting first wall thickness as one micrometer would require a huge number of cells? Currently I am already at 2 million cells.

How do you think the two far field boundary conditions at the outlet and inlet have affected the solution?

Thank you once again for the reply.

Hi;
Far field boundaries makes sense.
Regarding the mesh please note that near wall mesh starts from 1 micron and the width of other layers will increase by a expansion ratio (something between 1.2 to 1.5) and the number of layers can be as much as 10 to 15. The rest of meshes can be coarse and therefore managed to lower the number of overall meshes. Moreover, streamwise mesh size can be larger since the gradients are mainly in radial direction.

Hi Hamid,

Thanks again for giving me tips and feedback.

I understand that as the gradient is mainly in the conventional Z direction, mesh in x (streamwise direction) can be coarse. However, shouldn't the mesh be kept cuboid (equal length in 3 directions) to ensure better mesh quality?

Also, I would like to seek your opinion in terms of the number of viscous layer mesh. Currently I have layer number as many as 100, as the trailing edge, boundary layer is as high as 2.8m and the viscous layer mesh would need to cover up to that height. What is your opinion on this?

Many thanks to your feedback.

Kennedy

Regarding the quality of the mesh it is not a problem at all. you always need to compromise between mesh quality and CPU time.
Regarding the number of bl meshes, you should first find an approximation of bl height, and then find the proper thickness of first cell which is mainly dependent on Re number. (you can find some correlations for guessing of first cell thickness in the literature.) after that you will be able to select an expansion factor to increase the thicknesses of other layers which I mentioned before.
My experiences in internal flows with moderate to high Re numbers tells that usually 10 to 15 layers will be adequate. But your case may need a different configuration.

Regards

Hi Hamid,

Thank you very much for your help!

Kennedy