Fluid Domain mesh quality

The Fluid Domain mesh is defined in the Simulation file and created automatically by the flow solver during the analysis. You can view the mesh only after you generate it as part of the solver input file. When you generate the solver input file, the software generates 3D fluid elements and the results sets that allow you to check element quality. You post process these results to check the element aspect ratio, element size, element skew, and fluid mesh.

Solution 1
Element Aspect Ratio— Elemental
Element Size— Elemental
Element Skew— Elemental
Fluid Mesh— Elemental
Scalar

Element Aspect Ratio

The element aspect ratio helps locate malformed elements that may cause convergence and accuracy problems. The element aspect ratio, AR, is:

AR = L/S

where L is the longest edge of the element (1) and S is the shortest altitude (2).

The aspect ratio range is from 1.0 to infinity. For an optimal mesh, the element aspect ratio results should be as close as possible to 1.0.

Example:

The following graphics show a 2D example of an optimal element (1) and a malformed element with high aspect ratio (2).

Element Size

The element size represents the element volume for 3D elements. This results set helps you to locate the elements that are too small or too large.

Element Skew

The element skew helps locate malformed elements that may cause convergence and accuracy problems. The skewness, S3D, for 3D tetrahedral elements is:

S3D = (Voptimal —Velem)/Voptimal

where Voptimal is the optimal volume of the element and Velem is the actual volume of the element.

The element skew ranges from 0.0 to 1.0 and applies only to tetrahedral elements. For an optimal mesh, the skew factor should be as close as possible to 0.0.

Note:

A result value of —1 appears for other elements, such as wedge and pyramid elements, for which the skew result is not calculated.

Example:

The following graphic shows a 2D example of an optimal element for skewness (1) and a malformed skewed element (2).

Fluid Mesh

The fluid mesh results set represents the types of elements that are generated by the fluid domain mesher: a value of 0 is used for tetrahedral elements, a value of 1 for pyramid elements, and a value of 2 for wedge elements.

You can improve the quality of your mesh by adjusting the following parameters in the Fluid Domain Mesh Parameters group on the 3D Flow page in the Solution dialog box:

• You can control the shape of your 2D surface seed elements and 3D elements using one of the following properties: the reverse aspect ratio, skew, or maximum angle.

• You can refine the mesh by a refinement factor using the Element Shape Threshold Refinement option. The refinement factor can range from 0 to 1. The mesh, MSnew, is refined using the following equation:MSnew = RF x MSwhere RF is the specified refinement factor and MS is the initial mesh size.

• You can control the rate of transition of the mesh size from finer regions to coarser regions, using the Element Growth Through Volume option. The rate of transition values range from 0 to 1.Example: In the following example, mesh (1) has an element growth through volume value of 0. The mesh jumps from a fine to coarse mesh with no transition. Mesh (2) has a value of 1. The mesh doubles in size with each element as it transitions from the fine to coarse regions.

• You can control the level of geometric approximation of the surface when generating the mesh, using the Surface Curvature Based Variation option. The curvature refinement values range from 0.01 to 0.4. A smaller value means that you will have a more refined mesh along the curve.Example: In the following example, mesh (1) has a value of 0.4 and mesh (2) has a value of 0.03. The geometric approximation of the surface is better approximated with mesh (2).

You can set the fluid domain customer defaults to specify the fluid domain mesh parameters in the Fluid Domain Mesh Parameters group on the 3D Flow page in the Solution dialog box.

Tip:

To find a customer default, choose File→Utilities→Customer Defaults, and click Find Default .

How do I

Create a Fluid Domain mesh

Check Fluid Domain mesh quality

Learn more

Creating geometry for Fluid Domain meshing

Defining a boundary layer mesh using a Fluid Domain

Modeling obstructions in the Fluid Domain

Inputs to expressions

Look up more details

Auto-generated expressions

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

Fluid Domain mesh quality, 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 } });