I had problems in the process of verifying myself-developed 3D NS code to match Blasius. My U/Ue profile is developing much fast in the BL, then the U/Ue curve goes flat and it seems U hits Ue far outside the eta scale. The Re is 10e5 per meter in my calculation and the flat plate is 1. meter long. I set my upper bc as the same of inflow bc (U=Ue,P=Pinf, etc.), and the first y+ of my grid above the flat plate is around 3.0. In BL my grid has 20-30 points which should be enough. Could anyone experienced with Blasius verification give me some advice? Much thanks in advance.

(1). There are several areas you can explore. (2). The boundary layer development from a flat plate with sharp leading edge requires the highly stretch mesh in both x and y direction from the leading edge. (3). In this area, you can change the mesh stretching and plot the skin friction distribution. When this is done, try to increase the mesh points until the solution is mesh independent. (4). Then there are two areas which can affect the results. One is the numerical method, and the other is the turbulence model. (5). Normally, a first order method tends to give more diffusive solution. But you can increase the mesh points to reduce the effect. (6). Then the turbulence model is the most troublesome area. There, you can plot the eddy viscosity distribution from the wall to the domain outer boundary. In this way, you can see how the eddy viscosity changes across the boundary layer edge. (7). When I was working on low Re two-equation k-epsilon model in early 70's, I remembered that I needed 100 points to obtain nearly mesh independent solution in a fully developed channel flow. So, 20-30 points is probably not adequate. But then it also depends on the turbulence model you use. (using wall function could reduce the mesh points needed. But then, you still have to show that it is producing mesh independent solution.) (8). You will be surprised that even this seemingly simple problem is actually hard to get it right. So, dont' expect it to match the test results.

I would like to give something in more details.

For such problem, if the Re number is less than 5x10e5, the flow is still laminar and you can compare with the Blasius profile. Usually, 50 grid points are needed within the boundary layer at the location of x=1.0. The first y1 may be taken as less than 1/50 of the boundary thickness, that is to say, y1 < SQRT(x)*0.1/SQRT(RE), where x is the distance from the leading edge. For turbulence computation (Re > 5.0e10e5), 80-120 grid points are needed in the boundary layer, and at least 3 points must be used in the sublayer region ( y+ < 20). The first y+ must be less than 15-20, and may be taken as 5-10. Check the outside boundary in your computation region, and confirm whether yout is large enough, i.e., yout > 5.0/SQRT(Re). Another problem may be the boundary conditions on the outside and the exit. If yout were not large enough and the outside boundary were set to be U=Ue, or the exit condition were set to be du/dx=0, the boundary layer would develop faster.

To verify the grid-independence, a good way is to double the grid number and then compare the velocity and Reynolds stresses profiles.

Z. Lei

thanx for sharing.

I am grateful for your prompt and detailed advice.