Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field


Subsonic Analysis

The Subsonic analysis type offers a robust meshing strategy producing hexahedral cells suitable for the underlying solver thereby reducing mesh generation times by huge margins. Because the mesh is high quality, it requires fewer cells to achieve the same level of accuracy. It offers faster convergence at the cost of a reduced feature set. Some highlights of the mesher are:

  • Body fitted Cartesian meshing
  • Cells suitable for finite volume discretization
  • Highly parallelized meshing algorithm (i.e. very fast)

Subsonic is a Finite Volume based CFD solver with segregated pressure-velocity coupling using a proprietary variant of the SIMPLE\(^1\) algorithm. It provides the possibility to simulate both incompressible and compressible, laminar or turbulent flow with or without heat transfer in a single framework.

subsonic cartesian mesh
Figure 1: CFD simulation over a centrifugal compressor with non-orthogonality and velocity contours displayed on a highly Cartesian Subsonic mesh.

Within SimScale, one can effortlessly set up a Subsonic simulation which involves the following steps:

Creating a Subsonic Analysis

To create a Subsonic analysis, first, select the desired geometry and click on ‘Create Simulation’:

create simulation
Figure 2: Steps to create a simulation in SimScale

Next, a window with a list of several analysis types supported in SimScale will be displayed:

subsonic analysis
Figure 3: Select Subsonic analysis type from the tree above and click on ‘Create Simulation’ at the bottom.

Choose Subsonic analysis type and click on ‘Create Simulation’. This will lead to the SimScale Workbench with the following simulation tree and the respective settings:

simulation tree subsonic cartesian
Figure 4: Simulation tree for Subsonic analysis in SimScale Workbench

Global Settings

To access the global settings, click on ‘Subsonic’ in the simulation tree. At present, the user can set a steady-state analysis and the following parameters are available to define the fluid simulation:


The Geometry section allows you to view and select the CAD model required for the simulation. In general, having a clean CAD model always helps to avoid any meshing or simulation related errors. However, the mesher is pretty robust and if the CAD is genuinely dirty then a message of mesh failure and further instructions on CAD cleaning or mesh refinement should appear.

Find more details on CAD preparation and upload here.


Under Materials, the appropriate fluid for the simulation can be chosen from the materials library. The user has the option to change certain fluid properties. For compressible simulations, since the temperature is involved the user needs to specify the corresponding thermophysical properties for the fluid in consideration.

For more information, please visit the relevant documentation page for materials.

Boundary Conditions

Boundary conditions help to add a closure to the problem at hand by defining how a system interacts with the environment. In an incompressible simulation, the computational domain will be solved for two fields: pressure \((P)\), velocity \((U)\), while for a compressible simulation the temperature \((T)\) field is also involved. Additional turbulent transport quantities may be included based on the turbulence model selected.

The user gets to choose from velocity, pressure, and wall boundary conditions to be assigned.


In case no boundary conditions are assigned to a face, by default it will receive a no-slip wall boundary condition with wall function for turbulence resolution along with a zero-gradient condition for temperature.

Simulation Control

The Simulation control settings define the general controls over the simulation. For a Subsonic analysis the following series of variables can be set:

  • Number of iterations: It is the amount of iterations in a stready-state simulation beyond which the simulation terminates, i.e., no more iterations will be performed.
  • Write control & Write interval: It defines how often the result output will be written. The interval value represents the number of iterations between two writes of results.
  • Maximum runtime: Here, the maximum time limit can be set in real time after which the simulation will be terminated automatically irrespective of the value set under Number of iterations.
  • Convergence criteria: The simulation is assumed to be converged and will stop if the relative residuals for all the equations fall below this criteria. Relative residual is the ratio of current iteration residual to the inital residual.

For a complete overview of these parameters and their meaning, check out this page.

Mesh Settings

Meshing is the process of discretizing the simulation domain into a large set of finite volumes adhering to the CAD geometry.

For this analysis type, the mesh generated is a Cartesian mesh which means that each cell represents a cube with edges parallel to the XYZ Cartesian axes making the mesh highly orthogonal.

The meshing algorithm follows a top-down approach which works by creating a binary tree structure. The bounding box (an imaginary box encompassing the dimensions of the flow domain) is refined anisotropically by cutting cells in the first layer in the x-direction, second layer in the y-direction, and third layer in the z-direction.

Most features on an input tessellated surface smaller than the local cell size are ignored. More importantly, the algorithm does not generate boundary layers. Pyramidal cells are also used to capture the features and walls by projecting the mesh to the object’s surface.

For the mesh in Subsonic analysis, the settings can be set to automatic or manual. The parameters under each mode are described below:


The user gets to define a fineness level for the mesh cells varying from Coarse (1) to Fine (10).


The user gets to define the following parameters:

  • Minimum cell size: This parameter specifies the minimum size for all cells of the resulting mesh. We recommend starting with a value of 0.05 times the smallest dimension (smallest of x, y, z) of the geometry bounding box. Reduce it further until the mesh quality is satisfactory.
  • Maximum cell size: This parameter specifies the maximum size for all cells of the resulting mesh. We recommend starting with a value of 0.1 times the smallest dimension (smallest of x, y, z) of the geometry bounding box. Reduce it further until the mesh quality is satisfactory.
  • Cell size on surfaces: This parameter specifies the size for all cells on and close to the surfaces. We recommend starting with a value of 0.075 times the smallest dimension (smallest of x, y, z) of the geometry bounding box. Reduce it further until the mesh quality is satisfactory.
  • Specify growth rate: This parameter specifies the cell size ratio between the adjacent cells. It needs to be a whole number greater than 1 such that the cell size increases towards the interior of the mesh domain. For eg. a value of 2 would mean that the inner cell is twice as big as its adjacent cell closer to the surface.


The meshing log and the mesh are only visible once the simulation is finished. However, the time per iteration and the time to convergence are a lot lower compared to other solvers.

Your core hours will be consumed only after a successful simulation run.

Result Control

The Result Control section allows users to define additional simulation result outputs. It controls how the results will be written meaning the write frequency, location, statistics of the output data, etc. The following control items are supported:

  • Forces and moments: Calculates the forces and moments on a specific surface or set of surfaces. This is useful, for example, when one wants to find pressure and viscous forces on turbine blades in a hydrodynamic analysis.
  • Surface data: Calculates average or an integral sum of the simulation results on a specified surface area.

Did you know?

An advantage of using Subsonic analysis involving rotating flows is that power about the axis of rotation is directly output.

Advanced Concepts

Under Advanced concepts, you will find additional setup option for rotating zones. Rotating zones can be used to model rotating systems such as turbines, fans, ventilators, and similar systems. Currently, for the steady-state analysis type, the MRF (Multiple Reference Frame) type is supported.

We recommend you to visit this dedicated page on how to set up rotating zones for more details.

Once all the settings are defined, click on ‘Simulation Runs’ to begin the simulation.

Last updated: September 21st, 2021

Data Privacy