<simulation>

For thermal simulations, the <simulation> category contains additional parameters describing thermal method, thermal wall model, initialization of temperature field, setup of gravity, surface mesh and the fluid material.

<simulation>- <general>

The <general> category contains the parameters for specifying thermal model used in the simulation. Currently, ultraFluidX supports the following options for thermal model:

<thermal_method>

With the thermal method option, you can either disable the thermal solver or enable thermal solver using either a Boussinesq model or passive scalar transport.

<thermal_method> (off / passive_scalar_transport / Boussinesq / isobaric_ideal_gas)

Default: off

off: No thermal simulation will be performed.

passive_scalar_transport: Unidirectional coupling from velocity to temperature field: this method does not consider buoyancy forces.

Boussinesq: Bidirectional coupling between temperature and velocity field on basis of buoyancy forces due to heating. This method allows you to describe natural convection.

isobaric_ideal_gas: Effects of the variations of density, viscosity and fluid conductivity with temperature are inherently considered. Density is updated by an ideal gas model while viscosity and fluid conductivity are updated by the Sutherland law for air. The isobaric ideal gas model should be used if the difference between minimum and maximum temperature in the simulation is significant. The isobaric_ideal_gas model is based on the assumption of weak compressibility – significant gradients in background pressure cannot be captured. The absolute thermodynamic pressure of the system has to be close to or fluctuate around the atmospheric pressure of 1 bar.

<gravity>

Specifies the gravity as a vector via the child parameters.

<x_dir>

<y_dir>

<z-dir>

If <thermal_method> is set to Boussinesq or isobaric_ideal_gas, the default value for the gravity vector is (0, 0, -9.816).

If <thermal_method> is set to off or passive_scalar_transport the gravity vector is not considered.

<thermal_coupling>

Specifies if the thermal simulation is coupled with an external thermal solver. Currently only coupling between ultraFluidX and TAITherm is supported. Default is false. If set to true, the coupling is executed after every number of iterations specified in <num_coarsest_coupling_iterations>, starting from <coupling_start_iteration>.

<num_coarsest_coupling_iterations>

Specifies the number of coarsest iterations after which the coupling is executed.

<coupling_start_iteration>

Specifies the coarsest iteration after which the first coupling is executed. After that, coupling is executed after every number of iterations specified in <num_coarsest_coupling_iterations>.

<thermal_coupling_temporal_type>

Specifies the type of heat transfer coefficient <coupling_htc> and near-wall temperature <coupling_temperature> that are sent to the external thermal solver. The following types of data are available:

instantaneous: instantaneous values at coupling time are used.
window-averaged: window-averaged values at coupling time are used. The window interval should be specified in <avg_window_size_thermal>. Otherwise, it is set to <num_coarest_coupling_iterations>.
time-averaged: time-averaged values at the coupling time are used.

<thermal_coupling_data_file>

Specifies the location of the EnSight file with which the part temperature is imported to ultraFluidX.

Note: ultraFluidX-TAITherm coupling is part-to-part coupling. This means data exchange happens between a single part in ultraFluidX and a corresponding part in TAITherm. A part in ultraFluidX is coupled only if:

its boundary condition is temperature
and the name of the corresponding part in TAITherm is identical.

<simulation>- <material>

For thermal simulations, the <material>category contains the following parameters:

<temperature>: Temperature [in K] at which material properties are estimated. This temperature is used to initialize flow field unless you specify a file or fallback temperature in the <initialization> section. Temperature value is also used as inlet/outlet/wall temperature if you do not specify a temperature when using temperature boundary condition.
<thermal_conductivity>: Thermal conductivity of the fluid material. Default value is set to 0.025 W/m-K.
<thermal_expansion>: Thermal expansion coefficient. Default is 0.00341 1/K.
<density>: Density of the material at specified temperature in .
<dynamic_viscosity>: Specifies dynamic viscosity of the material at specified temperature.
<specific_heat_capacity>: Allows you to specify the specific heat capacity of the fluid material. The default value is set to 1006.0 J/kg-K.
<specific_heat_ratio>: Allows you to set the specific heat ratio of the material. The default value is set to 1.4.
<specific_gas_constant>: Allows you to set the specific gas constant of the material. The default value is set to 287.058 J/kg-K.

<simulation> <thermal_wall_modeling>

This section enables the thermal wall model in a thermal simulation. If <thermal_method> is set to either Boussinesq, passive_scalar_transport or isobaric_ideal_gas, <thermal_wall_model> is activated by default.

<thermal_wall_modeling>: <wall_model> (TLW, off); default: TLW; TLW refers to thermal law of the wall, a function that describes the near wall temperature slope.; <coupling> adaptive_two-way; The thermal adaptive_two-way wall model imposes the appropriate near wall slope of the temperature as well as the right wall eddy diffusivity based on different information collected in the wall vicinity and the chosen thermal law of the wall.