Fill out the form to download

Required field
Required field
Not a valid email address
Required field

Standard Mesher

The Standard mesher operation type uses a finite volume mesher. This tool generates a three-dimensional unstructured mesh using tetrahedral or hexahedral elements.

Shown below are the default settings that the mesh will contain:

mesh settings for a standard mesher in simscale
Figure 1: Mesh settings panel showing all setup options for the default mesher.

Sizing and Fineness

The sizing defines how coarse or fine the discretization of the input geometry will be. The sizing control can be set to automatic, where local properties are adjusted automatically based on geometrical estimations. Manual sizing can also be applied where a maximum edge length can be defined.

For the automatic sizing, only a global mesh fineness needs to be set and all additional parameters will be set automatically according to the geometry features and the chosen fineness. Its value basically defines the characteristic element size for each solid, ranging from 1 – very coarse to 10 – very fine.

A fine mesh will result in a better resolution of small geometric features, but will also increase computation time and memory demand of the simulation. The standard setting of 5 (moderate) will usually provide a good compromise between accuracy and resource consumption and is recommended for a first trial.
For mesh independence or convergence studies the sizing can be refined.

Physics-Based Meshing

This feature, when enabled, builds the mesh taking into account the information entered as a part of the simulation setup. This important information ranges from the material properties, boundary conditions, additional source terms (e.g., momentum and power sources), etc. Essentially, the physics involved in the fluid simulation is given priority while sizing the mesh elements.

The following adaptations are primarily observed when Physics-based meshing is toggled on:

  • Mesh refinement at the inlet and outlet of the domain
  • Additional operations on the boundary layers at the walls

Hex Element Core

This defaults to ‘on’ for CFD and ‘off’ for FEA.
It is recommended to leave the default settings alone.

Number of Processors

This defines the machine size that the mesh will be created on. Most meshes will be successful on a 16 core machine and this is a great starting point.

Advanced Settings

Set to zero by default, these would have no effect unless modified.
There are two options that can help when working with highly detailed geometry.

Small Feature Suppression

This can be used to ignore small surfaces during the meshing process.
It essentially merges surfaces together to avoid unnecessary levels of refinement around small features.

Gap Refinement Factor

This feature enables users to better capture small gaps in the model. For example, the air between the fins of a heat-sink or even the solid heat-sink fins themselves.

The feature does not guarantee a specific number of cells across the gap thickness since it is dependent on the algorithm’s constraints to accommodate the right amount of cells by an approximate gap thickness to desired cell size ratio. For example, if a value of 1.5 is entered, it is guaranteed that 1.5 cells will be accommodated across the gap thickness, and this will naturally change when the gap thickness gradually increases.

For example, consider the following image of a meshed “gap” which has a slight taper for illustration purposes. Note how setting a Gap Refinement Factor for 2 accommodates the cells at a small gap thickness.

Tet mesh on tapered fin with 2 cells
Figure 2: Meshed “Gap” Fin accomodating 2 cells across its thickness

For the same meshed solid, notice how the number of cells across the gap change (Figure 3) as the thickness increases further for the same Gap Refinement Factor of 2. So as explained earlier, the factor does not guarantee a specific number of cells across the gap and is dependent on constraints on the mesher that need to be taken into account for a consistent mesh.

tet mesh with varing cells for the tapering fin
Figure 3: Meshed “Gap” Fin showing more cells accommodating the varying thickness as the tapering increases

Increasing the value from 0 onwards can often provide a far better mesh to capture the movement of a fluid, with a greater emphasis on quality improvement between 0 to 1. Through a solid, this is also sometimes necessary in order to capture a thermal gradient.

Mesh Refinements

Mesh refinements can be used to refine the mesh locally and only where it is needed. This enables the generation of very efficient meshes with respect to result accuracy versus computational resource demand.

A mesh refinement can be added via the refinements node in the meshing tree.
Current mesh refinement types allowed are:

  • Region Refinement
  • Local Element Size
  • Inflate Boundary Layer

Local settings will always override the global setup for the assigned entities.
If multiple refinements of the same type are defined on the same entities, this may lead to conflicts and should thus be avoided.

Region Refinement

A region refinement is used to refine the volume mesh for one or more user-specified volume regions. The refinement needs to be assigned to geometry primitives or topological entities and a uniform mesh would be applied to the entire volume.

Local Element Size

This is applied to surfaces and gives the surface a uniform mesh based on the input.

Inflate Boundary Layer

This adds a volume mesh with cells aligned to the surface to all assigned surfaces. Only faces of the geometry domain can be assigned for refinement. The following four parameters are required inputs:

Default Boundary Layer Settings
Figure 4: Multiple options can be changed within the boundary layer settings – it is recommended to utilize the defaults
  • Number of Layers: Specifies the total number of layers to be added
  • Overall Relative Thickness: Specifies the overall thickness of all layers to be added. This is relative to the element nearest to the wall. It is not recommended to lower this below 0.25
  • Layer Gradation Control: There are two options here, Specify Growth Rate and Specify First Layer Size
    • Growth Rate: This controls the relative sizing between adjacent elements. 1.5 means 50% difference between layers
    • First Layer Size: This fixes the height of the first element next to the wall and is a global control

Cell Zones

A cell zone is a collection of cells grouped together. It is basically a part (volume) of the CAD model that needs to be present before the model is imported to the Workbench. Cell zones are required to assign specific properties to a subset of cells, like defining it as a rotating region (MRF-Multiple Reference Frame or AMI-Arbitrary Mesh Interface), a momentum source, a power source, porous media, or as a passive scalar source. This feature only appears when the Physics-based meshing feature is toggled off.

Figure 5: Cell zones feature appears in the simulation tree only when Physics-based meshing is disabled.

When Physics-based meshing is toggled on users don’t have to worry about creating a separate cell zone as it will automatically be taken care of. This saves a lot of time which would otherwise be spent creating cell zones one by one in case there are plenty of them.


A list of meshing tutorials can be found in the tutorial section. Visit today!

Last updated: October 23rd, 2020

What's Next

part of: Meshing in SimScale

Data Privacy