[Shomaz ul Haq]

Dear all,

Hello. Hope everyone is well. I want to ask how can one find y^+ or Yplus value in CFD-Post for convective flow in internal laminar pipe? I mean what method is more meaningful? I have used formula as follows

[y^+=(ρΔyu_τ)/μ

where Δy is the first cell height (I took it as the variable geometric variable y)
u_τ=√(τ_w/ρ) is the friction velocity or shear velocity
τ_w is the wall shear stress

I have computed y^+ at wall using a polyline. The thing is I am getting two values that are symmetric about axis or line y^+=0 and vary from -46.43 to 0 to around 40. It starts at 46.43/-46.43 at entrance and stabilizes to to 28.31/-28.31 after a short length till end of pipe. Also, I read in "ANSYS Documentation->CFX->Modeling Guide->Chapter 4: Turbulence and Near-Wall Modeling->4.2. Modeling Flow Near the Wall->4.2.6 Solver Yplus and Yplus" that there is exists a variable Yplus in CFD but I couldn't find it in CFD-Post that is why I made my own variable. How can I find that variable's value? I calculated areaAve(Yplus)@Wall but that gives me a negative and extremely small value of -1.69206e-006. Lastly can "ANSYS Documentation->CFX->Modeling Guide->Chapter 4: Turbulence and Near-Wall Modeling->4.2. Modeling Flow Near the Wall->4.2.7. Guidelines for Mesh Generation" be applied for convective flow in internal laminar pipe? I read somewhere r/38 (where r is the pipe radius) can be applied for calculating Δy in laminar flow. Would be grateful for any help in this regard. Thanks.

[evcelica]

Y+ is a variable in turbulent flow, not laminar. It will not show up in the variables if you ran a laminar simulation.

[Shomaz ul Haq]

Thanks Erik. But even for laminar flow there is a boundary layer, right? I mean I calculated the value. Resolution of the boundary layer plays a significant role in the accuracy of the calculated τ_w and heat transfer coefficient (htc). This is particularly true in laminar flows where the grid adjacent to the wall must follow. According to "ANSYS Documentation->Fluent->User's Guide->Chapter 5: Reading and Manipulating Meshes->5.2. Mesh Requirements and Considerations->5.2.2. Mesh Quality->5.2.2.1. Mesh Element Distribution

y_p*√(U_∞/(μ*x))<=1

where y_p is the distance to the wall from the adjacent cell centroid
u_∞ is the free-stream velocity
x is distance along the wall from the starting point of the boundary layer

Above equation is based upon the Blasius solution for laminar flow over a flat plate at zero incidence.

Everything comes down to calculating τ_w that can be for both laminar as well as the turbulent flow depending upon the case under consideration. For laminar flow it is defined by the normal velocity gradient at the wall. I personally think it carries more physical meaning in laminar flows than turbulent ones. I know boundary layer has three areas in turbulent i.e. laminar layer or viscous sub layer, buffer or equilibrium layer, and logarithm (ln) layer with dimensionless mean stream-wise or near wall velocity (u^+) linear in sub layer and logarithmic for ln layer. There must be a certain dimensionless or normalized grid independent distance of first cell node from the wall and depends only on flow nature (in first instants the velocity) (e.g. in my high compressible flows (Mach number (M)~0.7) a first cell layer thickness of 0.3 mm is required). For y^+<1 first cell is deep in laminar layer accompanied by assumption that the turbulent stresses are insignificant. For y^+<5 first cell is in laminar layer and u^+ for first cell is calculated linearly. For y^+~30 first cell is in equilibrium layer assuming that turbulent energy generation balances turbulent energy destruction and that transport terms are negligible. If y^+>30 first cell is in ln layer and u^+ for first cell is calculated logarithmically.

I read that there are certain methods/recommendations for calculating Δy.
1. Based on boundary conditions (how?)
2. Based on maximum displacement of boundary layer from Blasius solution, deciding an initial ds (should be small enough e.g. of order 10^-4), and calculating number of points needed in order to cover this (e.g. with a geometric distribution).
3. Based on order of magnitude analysis that gives y^+=1 by approximating 1/1000 of the overall boundary layer thickness and maybe selecting half that height to be conservative (El. K. suggested 10^-4).
4. Based on power law grid distribution giving equal increments of velocity across each cell for a constant viscosity laminar flow or Hagen-Poiseuille flow with a parabolic velocity profile (e.g. if u_wall=0 and u_max=1 m/s, and you use 10 cells across the channel width, then each cell would be at the position that correlates to velocity profile increments of 0.1 m/s).
5. Based on analytical solution for fully developed flow flow in a pipe i.e. Δn/r<=0.1 (where Δn is the distance between the first and second grid points off the wall) predicting τ_w within 10% of the theoretical values for fully developed flows and placement of grid lines closer than these guidelines (e.g. in developing flows) improves accuracy of prediction.
5. Based on formula Δy=r/38 for Reynolds (Re) number<=2000 (what is the authenticity of this?)

I have explored the following reasons for not calculating/optimizing y^+ in laminar flow.
1. Flow grid resolution criteria is based on refinement and that gradients in all cells are adequately resolved which is a function of the discretization scheme and how well the gradients need to be resolved at the cell location (e.g. a fully developed flow in a pipe may require only 1 cell to be fully resolved with a higher order numerical scheme or tens of cells for a low order scheme).
2. Flow is strongly influenced by the boundary layer, but the boundary layer is much thicker than in turbulent flow so a coarser mesh can sometimes resolve it depending on Re number. Inflation layers are still useful above extremely low Re numbers, i.e. Stokes flow.

Moreover, calculating y^+ can be a grid independence criterion. Maybe I should not calculate it but if so what method is more accurate and how can I apply it.The node of the first cell-layer away from the wall must have a certain distance. This distance is normalized (dimensionless). The needed distance is INDEPENDEND from the mesh, and belongs only to the nature of the flow (in first instants the velocity). You HAVE TO create a first layer of a certain thickniss. E.G. in my high compresible flows (mach about 0.7) I need a cell-layer thickness of 0.3 mm (!!!)

Hope to hear soon. Thanks.

[ghorrocks]

I have never seen anybody do anything with y+ for a laminar flow. While it can report a measure of boundary layer resolution I know of no useful correlation using y+ in laminar flow.

The normal approach is to use a mesh refinement study to define the mesh density in the boundary layer region. If you want to us y+ then this is new work to me - so it is up to you to determine if it is relevant and how to use it.

[Shomaz ul Haq]

Thanks Glenn. You're right. I've heard that it doesn't matter what Δy (first cell thickness or spacing 1) is for laminar flow but won't I still need it especially in the radial direction in a pipe for grid refinement. What method/standard should I use from the six points I mentioned? Thanks.

[ghorrocks]

I would not use any of the methods you suggest. I would do a mesh size sensitivity study and determine it that way.