Meshing for turbulence modeling

The turbulent boundary layer that forms over a flow surface is characterized by the sharp velocity gradient along the direction normal to the wall as shown in the following picture. Boundary layer meshes, which are high aspect ratio grids with very fine spacing along the wall normal direction, are typically used inside boundary layers in order to capture the sharp velocity gradient while maintaining a reasonable overall grid count and computational efficiency.

Velocity profile near the wall	Equally spaced mesh	Boundary layer mesh

The appropriate mesh size next to walls is determined by the non-dimension distance value y^+.

y^+ is computed using the following equation:

y^+ = \frac{\Delta{y}\sqrt{\rho{\tau}_{\omega}}}{\mu}

where:

• For body-fitted fluid meshing, \Delta{y}=\Delta{y}{p} is the distance between the centroid (point P) of the wall-adjacent control volume and the wall. You can approximate \Delta{y}{p} from the distance of the first node and the wall, \Delta{y}{e}, as follows:\frac{\Delta{y}{e}}{4} \leq \Delta{y}{p} \leq \frac{\Delta{y}{e}}{3}In the following graphics, the centroid is represented by the point P.For immersed boundary meshing, \Delta{y} = \Delta{y}{e,avg} is the average value of the normal wall distances between the boundary element's N nodes and the closest immersed wall boundary.\Delta{y}{e,avg} = \frac{\sum_{i=1}^N{\Delta{y}_{i}}}{N}

• \rho is the density of the fluid.

• \mu is the dynamic viscosity of the fluid.

• \tau_{\omega} is the wall shear stress. To approximate the wall shear stress for streamlined geometries, use the drag coefficient to compute the total shear force over the surface and divide that value by the total area. This approximation is unsuitable for a bluff body such as a cylinder in crossflow. Because most of the drag of a bluff body is form drag instead of skin friction, you would grossly overestimate the shear stress. For some internal flows such as pipe flows, the wall shear stress is approximated using the Darcy or Fanning friction factor and the Moody diagram.

The software can display y^+ results at element nodes. To request y^+ results, select Y+ in the 3D Flow group on the Results page in the Solution dialog box.

Velocity in the turbulent boundary layer

The turbulent boundary layer is divided into the inner layer (4) and the outer layer (5). The inner layer in turn is divided into:

• The viscous sublayer (1) where y^+ is less than 5. In the viscous sublayer, the mean velocity represented by the red curve, is given by the following equation represented by the blue curve:U^+ = y^+U^+ is the dimensionless velocity computed as:U^+ = U\sqrt{\frac{\rho}{\tau_{\omega}}}

• The buffer layer (2) where y^+ is between 5 and 30.

• The log-law region (3) where y^+ is between 30 and 200. In the log-law region, the mean velocity is given by the log-law equation represented by the green curve:U^+ = \frac{\ln{y^+}}{k} + C^+where k and C^+ are experimental constants.

When creating the mesh for turbulence modeling, the first node inside the boundary layer should always be in the inner layer. Further care must be made on where the first node needs to be inside the inner layer depending on the turbulence model used, and whether or not wall functions are used. For more information, see Meshing consideration and wall functions.

Requirements for LES modeling

For LES turbulence model, the maximum cell size is usually much smaller than what you use for the other turbulence models. The maximum cell size depends on the Reynolds number: the higher the Reynolds number the smaller the maximum cell size. This size should be small enough to resolve eddies in the inertial subrange. For a general flow configuration, this size is not available a priori. After one LES simulation, you need to analyze the results and calculate the energy spectra to verify whether the grid size is small enough.

For wall resolved flow surfaces, in addition to the previous requirements, you should also refine your mesh in streamwise and spanwise directions such that the streamwise x^+ and spanwise z^+ values are around 5 to 7.

How do I

Create a primitive

Learn more

Thermal meshing

Fluid meshing

Immersed boundary meshing

Duct network meshing

Primitives for Simcenter 3D Space Systems Thermal

Meshing for flow surfaces

Understanding the turbulence models

Flow Blockage

Flow Surface

Printed Circuit Board

Look up more details

Meshing for Simcenter 3D Thermal/Flow, Electronic Systems Cooling, Space Systems Thermal

Special considerations for thermal meshing

Working with multi-layer shell elements

Geometry creation for body-fitted fluid meshing

Geometry preparation for immersed boundary method

Defining the mesh size for fluid modeling

Node to geometry matching in large dimension models

Meshing consideration and wall functions

Thermal and flow element quality

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Simcenter 3D Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal boundary conditions

Thermal/Flow, Electronic Systems Cooling, and Space Systems Thermal

Meshing for turbulence modeling, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });