Meshing for flow surfaces

You must mesh the surfaces you select in Flow Surface simulation objects with 2D elements with thermal material properties. The primary convecting surface has the material and surface properties of the flow surface elements. These elements convect from both sides if the two sides are in contact with or immersed in the fluid elements. If a single side is in contact with the fluid flow domain, then only this side will convect.

If you apply a Flow Surface simulation object to free faces of the fluid flow domain, without a thermal mesh on them, the flow solver uses only the roughness surface properties to perform the CFD analysis.

Flow surfaces and body-fitted fluid meshing

The free faces of the 3D flow elements that contact one or both sides of the flow surfaces must be coplanar with the flow surfaces.

For two adjacent bodies that contain 3D fluid and non-fluid elements, the mating surface that separates them can be selected in a Flow Surface simulation object. You do not need to mesh the faces of a 3D fluid volume with 2D elements to define them as a flow surface.

The faces you select in a Flow Surface simulation object using only the Rotating/Translating Surface in Shear and no surface properties do not need to be meshed.

Flow surfaces and immersed boundary meshing

Surfaces that you select in a Flow Surface simulation object must be meshed separately from the immersed boundary mesh.

When using immersed boundary method, in a flow only solution, the flow solver uses the resolution of the flow surface mesh to resolve the fluid domain boundary. In a coupled thermal-flow solution, this mesh is also used by the thermal solver to exchange convection information with the flow solver.

Meshing when modeling turbulent flow

When modeling turbulent flow, the fluid element size next to a convecting Flow Surface depends on the selected turbulence model and whether or not wall functions are used. The first node inside the fluid flow domain should always be in the inner layer of the boundary layer. When wall functions are used, the first node should have y+ value that satisfies: 15 ≤ y+ ≤ 30. When wall functions are not used, the first node should have y+ value that satisfies: y+ ≈ 1.

Nodal alignment

The nodes on the Flow Surface elements do not need to align with the fluid flow nodes. You can use a finer or coarser mesh for the fluid flow domain than for the thermal conduction model. However, if possible, ensure that the elements of the flow surface are coplanar with internal faces in the fluid flow mesh. Alignment between the periphery of the surface elements and the internal boundaries of the fluid elements results in accurate modeling of convecting surfaces.

How do I

Create a flow surface

Learn more

Understanding flow surfaces

Modeling flow surface obstructions

Modeling semi-permeable surfaces

Convection Properties

Inputs to expressions

Fluid meshing

Immersed boundary meshing

Two-way fluid-structure interaction

Look up more details

Auto-generated expressions

Meshing for turbulence modeling

Geometry creation for body-fitted fluid meshing

Geometry preparation for immersed boundary method

Quick links

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

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

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Meshing for flow surfaces, 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 } });