InsightCAE Documentation

CFD simulations are said to be expensive and complicated. We are working to change that using our Software InsightCAE. The developed software specifically supports the automation of simulations with open source software to save licence costs and to enable specified workflows. InsightCAE also includes other tools that are useful in the development of automatic workflows (e.g. OpenFOAM Case Builder) or for parametric geometry creation and editing (the script-based CAD program ISCAD). In this example, the same simple external aerodynamics problem for a Volkswagen Touran as in the previous example is solved: the result will be the drag forces on some object exposed to a wind speed. This tutorial can be found as an online video The object could be any geometry for external flows like a vehicle or a building or something else. We have chosen the object below (downloaded from here: The object can either be a triangulated mesh (STL) or a STEP file. These formats can be exported from almost every CAD software. The preview in paraview looks like: Touran Geometry Bounding Box

First, start the workbench and create a new analysis of type "Numerical Wind Tunnel". This analysis conducts a simulation of the flow around an object positioned on the ground. The flow is incompressible and isothermal. The object is automatically centered and can optionally be reoriented.

The workbench parameter form is shown below:

InsightCAE Workbench Numerical Wind Tunnel

The available parameters are listed in the tree widget on the left. Once a parameter is selected, its description and the edit controls are shown in the area right of the parameter tree. On the right side, there is 3D window with a graphical preview of the analysis features. On the very right, all graphical elements are listed and can be hidden or shown by clicking in the associated checkbox.

The parameters highlighted by yellow background need to be revised for each case. The parameters in gray can usually be left at their default values. The others are preset such that:

  • the medium is air,
  • a reasonably universal turbulence model is selected,
  • the most up-to-date OpenFOAM version is selected,
  • the domain size is reasonable,
  • the mesh is rather coarse.

    For the current analysis, we need to set the following parameters:

  • geometry/objectfile: select the proper geometry file ("elephant_with_Howdah.stl")

  • geometry/upwarddir: enter a vector, which is pointing upward in the coordinate system of the object
  • geometry/forwarddir: enter a vector, which is pointing forward in the coordinate system of the object
  • operation/v: set the inflow speed

It is most important to find parameters for a decent mesh in the following. Commonly, this requires some iterations: the usual practice is to start with the analysis and to review the mesh as soon as it is created. To start the ParaView viewer in the analysis directory, click on the "ParaView" button on the right. If the mesh is too coarse or too large or the geometric details not sufficiently resolved, then the process is cancelled ("Kill" button), the created files are removed ("Clean" button), the parameters adapted and the next iteration may start.

The most important parameters for mesh quality are

  • mesh/nax: the number of cells in the template mesh along the diagonal of the objects boundary box
  • mesh/lmsurf: the minimum refinement level on the object's surface
  • mesh/lxsurf: the maximum refinement level on the object's surface

If more elaborate control of the mesh resolution is required, local refinement zones may be added to the array mesh/refinementZones. Also, for objects with longitudinal symmetry, only half of the model can be analyzed with a symmetry BC at the center plane. Set the switch mesh/longitudinalSymmetry for this.

If all parameters are set. I start the simulation by clicking on the "Run" button in the upper right corner. The GUI switches to the tab "Run" and the progress is displayed in the log window and, as soon as the solver has started, the residuals, forces and so on are also displayed graphically:

InsightCAE Workbench Numerical Wind Tunnel: Run

Then the flow solver starts. While the flow solver is running, the most important parameters that CFD specialists are usually interested in are displayed online in various diagrams. These include residuals and continuity errors, both of which should be as small as possible, and the forces and moments that will eventually become stationary and should no longer change. The simulation runs for 1000 iterations. If one determines beforehand that forces and moments have become stationary, one can force by clicking on the button "Write+Stop" that output is written immediately and the solver stops afterwards and starts the evaluation. By clicking on the button "Write now", a signal file is created in the case directory, which is recognized by the OpenFOAM solver and leads to immediate output of the current time step. This is useful, if Paraview is running with the current case loaded and an update is demanded.

Analogously, by hitting the button "Write+Stop", immediate output is triggered but the solver is gracefully stopped immediately. This is useful, if you recognize that the solver has converged and you do not want to wait any longer.

Once the solver has finished, the evaluation is run. A number of figures and renderings are created and displayed in the "Output" tab:

InsightCAE Workbench Numerical Wind Tunnel: Output

The displayed so-called result elements, can be compiled into a PDF-Report by selecting "Results > Create report..." in the menu. You can either create a TEX file or a PDF file. In the same directory as the report, a directory "report_data_[input filename]" is created. In this directory, all figures from the report (except the rendering images) are contained in script-readable ASCII format.

InsightCAE Workbench Numerical Wind Tunnel: Output

If the generated renderings do not suffice, you can also perform further evaluations with Paraview afterwards. The generated OpenFOAM case with all results is left in the working directory of the simulation. A click on "Paraview" on the right side starts Paraview.