<< Click to Display Table of Contents >>

Navigation:  Menu > PROJECT > Additional > Export > CFD, FEA >


Previous pageReturn to chapter overviewNext page

Geometry settings

In addition to the STL settings, the user can select which files should be exported.

Export all files: Configuration file (*.spro) and STL files and gas property files (compressible fluids only) are exported .

Export configuration file only: STL files are not exported. This option can be useful for saving export time if the user wants to generate a new configuration file with different settings (e.g. mesh parameters, rotational speed, boundary condition values, fluid data etc.). In this case, all geometrical export requirements (like solid trimming) are disabled in the CFturbo Export window.

Export STL files only: The configuration file is not exported. This option is useful, e.g. if STL files for some (but not all) components have to be exported again due to an unsatisfactory triangulation. In this case, the original configuration file, which refers to all components, should not be overwritten.

Mesh settings

Mesh settings are specified globally for all selected CFturbo components to be exported.

The following global mesh parameters are available:

Min. cell size

Max. cell size

Cell size on surfaces

If the user wants to set specific parameters for predefined regions, the option “Use local cell size on surfaces” must be activated.
If not, the global value “Cell size on surfaces” is used for all regions. Specific mesh parameters can be set for the following regions:

Rotational symmetric components







Blade sides

Blades suction and pressure sides

Blades LE / TE / Tip

Blades edges leading, trailing and tip

Secondary flow path hub

Hub material domain surfaces

Secondary flow path shroud

Shroud material domain surfaces





For RSI-Connection surfaces, the “Hub” parameters are used for meshing:

Secondary flow path mesh parameters are useful if a fine meshing is necessary in gap zones between solid bodies and casing.
Enabling the option "Refine casing", local cell sizes set for hub and shroud are also used for the casing surfaces.











Volute splitter (double volutes)





For RSI-Connection surfaces, the “Spiral” parameters are used for meshing:

In case the volute extension is exported, “Diffuser” mesh parameters are used for the extension walls.
“Inlet” and “Outlet” mesh parameters are used for the extension inlet and outlet:

Refinement zones

In some cases mesh refinement zones are more effective than applying local mesh sizes. This might be true e.g. for secondary flow path simulations where very small gaps have to be meshed. The images below show a typical case:

Mesh resulting from setting local mesh parameters on hub and shroud as well as casing surfaces

Mesh resulting from setting local mesh parameters on hub and shroud as well as casing surfaces


Mesh resulting from using refinement zones in isolated regions

Mesh resulting from using refinement zones in isolated regions

The use of refinement zones allows for high quality refinement in regions with small gaps, avoiding high numbers of cells. Refinement zones can be applied within the whole geometry and can be set by defining the refinement cell size and cylindrical refinement area:

Solver settings

The following parameters are available:

Solver selection (Simerics-MP or Simerics-MP+)

Selection of simulation type: Steady or transient

Number of iterations

Result saving frequency (only for transient simulations)


For transient simulations, two special parameters are available. These parameters differ from the Simerics original ones, but are more comfortable for turbomachinery:

Number of revolutions: number of impeller rotations to be simulated. The original Simerics parameter “Simulation Time (Duration)” is calculated using this new parameter and the rotational speed of the impeller. Default value is 3 revolutions.

Rotation angle per step: number of degrees the mesh is rotated by per step. The original Simerics parameter “Number of time steps” is calculated using this new parameter and the number of revolutions to be simulated. Default value is 3 degrees.


A global value for converge criterion can be set. This value is used for all active modules. In case the default Simerics value (0.001 for steady simulations and 0.1 for transient simulations) is used, values are not written in the SPRO-file allowing Simerics to change the values automatically if the user switches interactively in the Simerics-GUI between steady and transient simulation.

Numeric scheme and Relaxation values

Cavitation (activated by default for pumps). Not available for compressible flow (compressors, gas turbines, fans)

Reversible pump turbine: enabling this option, adapted boundary conditions are used to simulate the pump as a turbine.

Turbomachinery expressions are useful to check the simulation convergence.
IMPORTANT: Plotting of user defined expressions is not supported for Simerics versions lower than 4.2.8 and can cause problems in these versions.

Real gas

If the fluid to be used in the simulation is compressible, data for density, enthalpy, dynamic viscosity and thermal conductivity can be exported. Precondition for that is that the gas model is not perfect but any real gas model. In that case the necessary entries will be done in the spro-file. The data will be derived from the selected gas and its gas model within a pressure and temperature range. Please note, that the size of this range will influence the computational time necessary to calculate all data.

Not supported characters

The character "_" is not allowed for component names for the time being.