Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field
  • Set up your own cloud-native simulation in minutes.

  • 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 a standard mesh.

    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 minimum and a maximum edge length can be defined.

    Automatic Sizing

    For the automatic sizing, only a global mesh fineness needs to be defined and all additional parameters will be set automatically according to the geometry features and the chosen fineness. Its value 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 the 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.

    Manual Sizing

    Manual sizing gives you the freedom to define the maximum edge length and the minimum edge length of the cells. The intermediate cell size is adjusted accordingly.

    Mesh Order for Structural Simulations

    For Structural simulations (solid mechanics) the mechanical and thermal order of the mesh, i.e., first or second order, can be defined under the Element technology item in the simulation tree.

    Automatic Boundary Layers

    This feature, when enabled, builds layered mesh cells next to only those surfaces of the CAD model which are assigned a wall boundary condition. The settings and their functions are the same as described for inflate boundary layer feature below.

    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. When activated the interior of the mesh gets covered with hexahedral elements. The transition from hexahedral to triangulated surface mesh is done using pyramidal and tetrahedral elements.

    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.

    Learn with the video!

    Here’s a short video on the Basics of Meshing in SimScale. It explains different parameters from the mesh settings panel.

    Advanced Settings

    When set to zero, advanced settings do not affect the meshing process. Two options can prove helpful 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 to avoid unnecessary levels of refinement around small features.

    You get to define a minimum edge length below which small features like tiny edges or sliver faces should not be resolved during meshing. Setting it to ‘0’ would mean a request to resolve every detail leading to a large mesh size.

    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 gap refinement factor is better defined as the ratio between the gap thickness and the mesh edge length in the gap:

    • For values > 1, the value (integer) is also the number of elements across the gap.
    • For values < 1, the gap refinement factor is basically the inverse of the aspect ratio of the elements in the gap (see picture below).
    gap refinement factor schematic
    Figure 2: Schematic representation of the Gap refinement factor

    The default value of 0.05 is there to guarantee that the elements across a thin gap are not too flat causing quality to decrease substantially.

    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 expected that 1-2 cells will be accommodated across the minimum gap thickness, and this will naturally change when the gap thickness gradually increases.

    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 in the small gap thickness.

    Tet mesh on tapered fin with 2 cells
    Figure 3: Meshed “Gap” Fin accommodating 2 cells across its thickness

    For the same meshed solid, notice how the number of cells across the gap change (Figure 4) 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 4: Meshed “Gap” Fin showing more cells accommodating the varying thickness as the tapering increases

    Global Gradation Rate

    The Global gradation rate is the ratio between the size of two adjacent cells in the computational domain. This setting controls how quickly the cells transition from small to large.

    The global gradation rate can receive any value between 1 and 3. By default, it has a value of 1.22, which is a good compromise between cell size transition and mesh size. Defining a gradation rate of 1 causes the resulting mesh to be uniform, with the smallest cell size everywhere. For larger gradation rates, the transition from small to large cells accelerates.

    Setting a value of 1 is not recommended, since the resulting meshes may be very large. Similarly, setting large values for the gradation rate is also not desired, as the cell size transition will be abrupt.

    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 concerning 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
    • Sweep Meshing Refinement (currently only for FEA analysis types)

    Important

    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, the algorithm opts for the finer setting irrespective of the order in which the refinement levels were assigned. Multi-refinement, however, should be avoided for clarity purposes.

    mesh refinements simscale
    Figure 5: To apply mesh refinements go to Mesh > Refinements in the simulation and select one of the available options

    Region Refinement

    A region refinement is used to refine the volume mesh for one or more user-specified volume regions. The refinement can be assigned to volumes, topological entity sets of volumes, or geometry primitives. For the Standard mesher, there are two types of refinement modes available: Inside and Distance.

    • Inside: Refines all volume mesh cells inside the selected volumes up to the specified cell maximum edge length.
    mesh region refinement settings using inside refinement mode
    Figure 6: Region refinement settings using the Inside refinement mode
    • Distance: Refines mesh cells according to the distance to the surface of the assigned volume(s). The Distance mode can accommodate different refinement levels at multiple distances. The smallest value for Maximum edge length must be assigned to the smallest Distance. In other words, the value for edge length must increase as the distance from the surface of the volume increases. (The order in which entries are made in the table does not matter)
    mesh region refinement settings using distance refinement mode
    Figure 7: Region refinement settings using the Distance refinement mode. The finest cell size corresponds to the smallest distance in the refinement table.

    For both the above methods, a maximum edge length can be defined. The meshing algorithm is developed such that finer features on your CAD model will get appropriate mesh sizing.

    Local Element Size

    This is applied to surfaces of the CAD model and gives the surface a relatively uniform mesh based on the input of maximum edge length for the mesh elements.

    The algorithm will apply a finer size where mesh quality restrictions or geometrical details require so.

    Inflate Boundary Layer

    This adds a volume mesh with prismatic cells aligned to the surface of the assigned faces. Only faces of the geometry domain can be assigned for refinement. This feature is generally used to refine the boundary layer to capture it better. The following four parameters are required as inputs:

    Default Boundary Layer Settings
    Figure 8: 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 combined, relative to the surface mesh element adjacent to the boundary layers. It is not recommended to set this value below 0.25.
    overall boundary layer thickness
    Figure 9: The Overall relative thickness represents the length of all boundary layers (blue arrow) divided by the size of the first cell adjacent to the boundary layers (yellow arrow)
    • Layer Gradation Control:
      • Specify growth rate: Specify the growth rate that controls the relative sizing between elements of adjacent layers. 1.5 means a 50% difference between layers.
      • Specify first layer thickness: Specify first layer size that fixes the absolute height of the first element next to the wall.

    Sweep Meshing Refinement

    This refinement, currently available only for solid mechanics analysis types, meshes a given volume with layers of prisms, sweeping from a start to an end face of the same volume. Please note that this refinement only works for bodies that can be entirely swept.

    sweep mesh user interface set up
    Figure 10: Each volume assigned to a sweep meshing refinement can have a single Start and a single End face.

    The following settings are required in the setup:

    • Sweep sizing type: The user can define the Number of elements or the Element thickness along sweep. These parameters control the number of prism layers between the Start and End faces. For example, in the figure above, a total of 30 prism layers were created in the z-direction.
    • Surface element type: With this setting, the user defines the type of cells to be generated on the start and end faces. In Triangular mode, the mesh cells will be prisms with a triangular base. In Quad dominant mode, the mesh will consist mainly of hexahedrons and possibly some triangular-based cells.
    • Specify start/end mesh size: If toggled on, this option allows the user to control the maximum edge length of the cells on the start and end faces.
    • Start and End faces: The user needs to define one Start and one End face that belong to the same volume. Note that several volumes can have their start and end faces assigned to the same refinement, as long as each volume has a single start and end face
    assigning multiple sweep refinements at the same time
    Figure 11: A pair of start and end faces for multiple bodies can be defined. The T-junction volume from assembly 1 is not sweepable, therefore trying to assign a sweep refinement to it would result in a mesh error. All volumes in assembly 2 can be swept without problems

    The result of the mesh settings shown above is the following:

    sweep mesh results
    Figure 12: It is possible to use the sweep method for some volumes of your CAD model while meshing other volumes with the traditional meshing refinements.

    Cell Zones

    A cell zone is a collection of cells grouped. It is 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 a passive scalar source. This feature only appears when the Physics-based meshing feature is toggled off.

    creating cell zones with the standard meshing tool
    Figure 13: The 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 that would otherwise be spent creating cell zones one by one in case there are plenty of them.

    Tutorials

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

    Last updated: October 28th, 2022

    What's Next

    part of: Meshing in SimScale

    Contents