Setup

Physics

For the gas domain, you can choose from the following flow and energy scenarios:

Forced Convection—the fluid movement results only from external sources (for example a fan).
You solve for flow and/or energy within a turbulent or laminar flow regime. The density of the fluid phase is assumed to be constant throughout the domain.
Natural Convection—as Forced Convection, but includes gravity effects and radiation.
This scenario allows you to model buoyancy due to small density differences that are caused by temperature gradients.
Custom—as Natural Convection, but you can choose to use the ideal gas model which allows you to model flows with large variations of density due to temperature and pressure variations.

For a liquid domain, such as a cooling loop, the default scenario is Forced Convection.

The Setup > Physics node allows you to set the following properties that are common to all fluid domains and flow scenarios:

Physics—Common Properties

Ambient Conditions

Specifies the physical conditions of the environment.

Temperature

Specifies the temperature of the environment. This temperature is used as default value for every fixed temperature setting, for example, for a fixed temperature boundary condition on a wall.

Note	If you want to change a specific fixed temperature setting to another temperature value, delete the $DefaultAmbientTemperature entry and enter the required value.

Solution Physics

Specifies the physical effects that you want to consider in the simulation.

Solve for

Defines the equations that you want to solve.

Flow: When activated, solves the Navier-Stokes equations for continuity and momentum (see Fluid Flow).
Selecting this option allows you to evaluate the flow field in the fluid domains.
Energy: When activated, solves the energy equation (see Fluid Flow).
Selecting this option enables you to analyze the temperature distribution within the fluid and solid domains.

Pressure

Specifies the reference pressure for the gas domain and liquid domain, respectively.

The reference pressure is simply a device that is used to reduce the numerical roundoff error in the numerical calculations involving pressure. This reduction in numerical error is necessary since the differences in pressure are important, and these differences can be small relative to the absolute value of the pressure (for example, in fully incompressible, or very low-Mach number flows). By subtracting a suitable constant reference pressure, a working pressure is obtained that is less prone to roundoff errors.

For constant density flows, the actual value of the reference pressure has no relevance to the calculations. However, when using the ideal gas model, the reference pressure is used as in Eqn. (671).

Set the reference pressure to some ambient value such that the working pressures are small. The default value is 101325.0 Pa.

Flow Regime

Defines the flow pattern within the gas and liquid domain, respectively.

Turbulent: Solves for a flow that is in a state of continuous instability and exhibits irregular, small-scale, high-frequency fluctuations.
Turbulent flow is modeled using a K-Epsilon approach to provide closure to the Reynolds-Averaged Navier-Stokes (RANS) equations. For more detailed information on the turbulence model that is used, see Realizable Two-Layer K-Epsilon Model.
Laminar: Solves for a well-ordered flow that is free of macroscopic, non-repeating fluctuations.
Numerical instabilities can arise from simulating laminar flows at a Reynolds number (the ratio of viscous to inertial forces) that is too large. These instabilities can impede convergence. Therefore, a laminar flow simulation is only appropriate if you already know that the Reynolds number of the problem is sufficiently low.

Materials

Specifies the materials that are present within the electronic device.

Solid Sim Materials

Specifies the materials of the different solid components.

Default Solid

Specifies the default material that is used for a new solid QuickPart. To reduce the time to set up the solid components, select the material that characterizes most components.

Note	Usually, most materials that are present within an electronics device are isotropic. For this reason, Solid Sim Materials with anisotropic thermal conductivity are not supported as Default Solid.

Default Gas

Specifies the material of the gas domain.

Default Liquid

Specifies the material of the liquid domain.

The following properties are available for the gas domain. The availability of the properties depends on the flow scenario that you choose in the Solve drop-down menu within the Solution Physics box:


Solution Physics—Gases				Natural Convection	Custom
Gas Model	Defines the equation of state for the density of the gaseous phase. The following options are available: Constant Density: The density of the gaseous phase is assumed to be invariant throughout the domain. Ideal Gas: Uses the ideal gas law to express density as a function of temperature and pressure.
Gravity Effects	Allows you to account for the effect of gravitational acceleration in the gaseous phase due to density variations. For more information, see Modeling Gravity. When activated, the following options are available: X, Y, or Z: Sets the direction in which gravity acts to the respective axis of the Laboratory coordinate system. Custom: Set the components of the gravity vector to the specified X, Y, and Z values.
Radiation	Allows you to include radiative heat transfer between diffuse surfaces independently of wavelength. The medium that fills the space between the surfaces is non-participating. That is, it does not absorb, emit, or scatter radiation. For more information, see Modeling Surface-to-Surface Radiation and The Gray Thermal Radiation Model. When activated, the following properties are available: Radiation Temperature Specifies the temperature that is effectively radiated from the environment. The thermal environment is modeled as a black body with unit emissivity. Default Surface Emissivity Specifies the default surface emissivity that is set on every new QuickPartSurface. Set the emissivity that applies to most of the surfaces.

Units

The Setup > Units node allows you to set the preferred units for the various fundamental and derived dimensions (like temperature or mass flow rate):


Units Properties
Dimension	Specifies the physical dimension of the unit.
Preferred Units	Specifies the preferred unit for the dimension. For each dimensional combination in use in the simulation, the Electronics Cooling Toolset marks exactly one unit to be the preferred unit for that dimension. For example the preferred unit for quantities with the dimension of length might be m and the preferred unit for quantities with dimensions of length per time might be m/s. The preferred units are the ones that are used by default for any new physical quantity. You can change the preferred unit for an individual dimensional combination. Although the preferred unit is used by default, you can override it on specific settings. For example, you might have the preferred unit for dimensions of velocity to be m/s, but for a specific velocity boundary condition you could change the units to km/h.


Units Actions
(Add a new unit)	Adds a user-defined unit. The following properties characterize a user-defined unit: Description Specifies the full name of the unit. Conversion Specifies the conversion factor that converts the quantity from this unit to SI units. Offset Specifies the offset factor used to convert the quantity from this unit to SI units (for example for Celsius and Fahrenheit temperatures).
(Edit Unit)	Allows you to edit the properties of a user-defined unit.
(Delete Unit)	Deletes a user-defined unit.

Solver

The Setup > Solver node allows you to set the following stopping criteria and numerical parameters for the solver:


Solver Settings
Stopping Criteria	Defines how long the solution runs. The stopping decision is based on the number of steps that the solver executes, including any steps that are executed in a previous session. If you clear the solution, the counter resets to zero. Maximum Steps Specifies the maximum number of steps to take before the criterion is satisfied. The default is 1000 steps.
Segregated Flow	Controls the solution update and thus the convergence of the solvers that compute the intermediate velocity field and the update of the pressure field. Velocity Under-Relaxation Factor, Pressure Under-Relaxation Factor At each iteration, these properties govern the extent to which the newly computed solution supplants the old solution. For the theoretical background, see Finite Volume Discretization. The default values of 0.7 for velocity and 0.3 for pressure are conservative, that is they lead to a converged solution in most cases. For further guidelines, see Setting Under-Relaxation Factors for Steady State Computations.
Segregated Energy	Controls the solution update of the solver that computes the temperature field in the fluid and solid domains. Fluid Under-Relaxation Factor, Solid Under-Relaxation Factor In order to promote convergence, these properties under-relax changes of the solution during the iterative process, see Finite Volume Discretization. The default values are 0.99 for fluid energy and 0.9999 for solid energy. These values are progressive parameters that produce a fast solution convergence for a wide range of physical situations. Sometimes it is necessary to decrease the fluid energy relaxation to 0.9 and the solid energy relaxation to 0.99 to achieve a stable solution.

Libraries

The Setup > Libraries node allows you to edit the QuickParts that are stored in a previously created QuickPart library.

Using the QuickPart Library Editor, you can perform the following actions:

Overwriting the definition of a library QuickPart
Deleting a QuickPart from a library

See Creating and Editing QuickPart Libraries.

Environment

The Setup > Environment node allows you to set up the environment for the import of ODB++ files.


Environment Settings
ODB++ Import Software	Enables the import of ODB++ files that contain printed circuit board (PCB) design information. Install Location Specifies the absolute path to extracted saflt directory.