Heat Transfer Boundary Conditions

Use the Boundary Conditions quick edit dialog to assign all boundary conditions. There several ways to open the quick edit dialog:

• Left click on the surface, and click the Edit icon on the context toolbar.

• Right click on the surface, and click Edit.
• Click Edit in the Boundary Conditions context panel.

Surface Boundary Conditions

Surface-based heat transfer boundary conditions represent either a known physical state, such as temperature, or an amount of heat entering or leaving the device, such as a heat flux. Temperature is the only condition that can be applied to openings and wall surfaces. You should apply the others only to wall surfaces.

Temperature

A temperature boundary condition should be specified at all inlets when running heat transfer.

To assign a Temperature condition:

1. Set the Type to Temperature, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Optionally, set the Spatial Variation to Linear Variation.
4. Enter the value in the Temperature field.
5. Select either Static or Total
6. Click Apply.

Example assigning Temperature Boundary Condition

A static temperature condition is recommended for most heat transfer analyses. Use total temperature as an inlet temperature for compressible heat transfer analyses.

Heat Flux

Heat flux is a surface condition that imposes a given amount of heat directly to the applied surface. It is a heat value divided by area.

To assign a Heat Flux condition:

1. Set the Type to Heat Flux, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Specify the value in the Heat Flux field.
4. Click Apply.

For example, if the heat input is 10 W, and the area is 5 sq. inches, apply 2 W/sq. inch ( = 10W/5 sq. inches).

Heat flux should only be applied to outer wall surfaces.

Total Heat Flux

Total Heat flux is a surface condition that imposes heat directly to the applied surface.

To assign a Total Heat Flux condition:

1. Set the Type to Total Heat Flux, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Specify the value in the Total Heat Flux field.
4. Click Apply.

Apply the total heat flux condition directly without dividing by the surface area. This is very useful because the value does not have to be recalculated if the area of the applied surface is changed.

Total heat flux should only be applied to outer wall surfaces.

Note: For axisymmetric models, apply the actual total heat flux to edges. Do not apply a per-radian value of total heat flux. Total heat flux boundary conditions applied to Axisymmetric models in CFdesign 2010 are automatically converted to the total value from the per-radian value applied in CFdesign 2010.

Film Coefficient

Also known as a convection condition, this is often used to simulate a cooling effect for heat transfer analyses. Assign film coefficients to external surfaces to simulate the effect of the environment that is external to the device. The film coefficient boundary condition can only be applied to external surfaces.

To assign a Film Coefficient condition:

1. Set the Type to Film Coefficient.
2. Set the Time dependence (Steady State or Transient).
3. Specify the Coefficient Units.
4. Specify the value in the Film Coefficient field.
5. Specify the Temperature Units.
6. Specify the value of the surrounding temperature in the Ref Temperature field.
7. Click Apply.

In many simulations, a Film Coefficient boundary condition simulates natural convection from exterior surfaces to regions that are outside of the physical model (but not included). Several engineering resources recommend a film coefficient value between 5 and 25 W/m²K as a good approximation for natural convection. The choice of value is influenced by the physical size of the physical (not-modeled) air volume as well as by the strength of any exterior air circulation.

In most cases, a value of 5 W/m²K is a good approximation for use with Autodesk Simulation CFD, but the following conditions may warrant a higher value:

• External regions that are physically small can lead to increased levels of heat transfer close to the exterior walls.
• External regions that are very large due to the larger thermal reservoir of ambient air that can cause more heat to be absorbed.
• If a strong ventilation system is known to exist outside of the simulation model, use a higher value to account for the elevated levels of heat transfer that will occur.

Example assigning a Film Coefficient Boundary Condition

Note: External walls that do not have any applied heat transfer conditions (temperature, film coefficient, radiation, heat flux, etc.) are considered perfectly insulated.

Radiation

The Radiation boundary condition simulates the radiative heat transfer between the selected surfaces and a source external to the model. It is a “radiation film coefficient” in that it exposes a surface to a given heat load using a source temperature and a surface condition.

To assign a Radiation condition:

1. Set the Type to Radiation.
2. Set the Time dependence (Steady State or Transient).
3. Specify the surface emissivity in the Emissivity field.
4. Set the Temperature Units (of the background temperature).
5. Specify the background temperature in the Ref Temperature field.
6. Click Apply.

Note: Assign the radiation boundary condition to external surfaces only.

Current

Current is used to define a Joule heating analysis. Joule heating is the generation of heat by passing an electric current through a metal. Also known as resistance heating, this feature allows the simulation of stove-top burner elements as well as electrical resistance heaters.

To assign a Current condition:

1. Set the Type to Current, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Enter the current in the Current field
4. Click Apply.

Note: Current is a total current, not a current density.

Voltage

Voltage is used to define a Joule heating analysis. Joule heating is the generation of heat by passing an electric current through a metal. Also known as resistance heating, this feature allows the simulation of stove-top burner elements as well as electrical resistance heaters.

To assign a Voltage condition:

1. Set the Type to Voltage, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Enter the current in the Voltage field. (A typical value is 0.)
4. Click Apply.

Note: Alternatively, a voltage difference can be applied to the solid to represent a potential difference. In this mode, do not specify a Current condition.

Transparent

The radiation model allows for the computation of radiative heat transfer through transparent media. The level of transmissivity is defined as a material property on the Materials Task dialog. To simulate transparent media that is completely immersed in the working fluid, only the material transmissivity needs to be specified. To simulate transparency through surfaces on an exterior solid, the Transparent boundary condition is also required.

This boundary condition is used to indicate that an exterior surface of a solid part is transparent (such as a window), allowing radiative energy to pass through it . Exterior wall surfaces that do not have this condition are considered opaque, and will not allow radiative energy to pass, regardless of the value of transmissivity assigned to the material.

More about external transparency.

To assign a Transparent condition:

1. Set the Type to Transparent, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Specify the Background Temperature. This is the temperature of the environment outside of the analysis domain.
4. Click Apply.

Note: Radiation must be enabled (on the Solve dialog) for the Transparent boundary condition to work.

Note: The Background Temperature can be varied with time by clicking the Transient bullet, and specifying the time function.

Volumetric Boundary Conditions

Volumetric conditions in Autodesk Simulation CFD are used to generate heat. They are used in many heat transfer analyses. For 3D models, volume conditions are available when the selection type is Volume. For 2D models, Surface must be the selection type.

Heat Generation

Heat Generation condition is a volumetric heat load assigned to a volume. The specified value must be divided by the volume of the part.

This is most often used to simulate the presence of heat-dissipating components in electronics assemblies.

To assign a Heat Generation condition:

1. Select one or more volumes.
2. Set the Type to Heat Generation, and select the Unit type.
3. Set the Time dependence (Steady State or Transient).
4. Set the Temperature Dependence.
5. Specify the value in the Heat Generation field.
6. Click Apply.

Note: For axisymmetric models, divide by the total heat generation by the 3D volume: (pi * r² * L)

Total Heat Generation

The Total Heat Generation condition is a heat load that is not divided by part volume. This is the recommended condition for most heat-load applications as the value does not have to be adjusted if the part volume changes.

To assign a Total Heat Generation condition:

1. Select one or more volumes.
2. Set the Type to Total Heat Generation, and select the Unit type.
3. Set the Time dependence (Steady State or Transient).
4. Set the Temperature Dependence.
5. Specify the value in the Total Heat Generation field.
6. Click Apply.

Example assigning a Volumetric Heat Generation Boundary Condition

Note: For axisymmetric models, apply the actual total heat generation. Do not apply a per-radian value. Total heat generation boundary conditions applied to Axisymmetric models in CFdesign 2010 are automatically converted to the total value from the per-radian value applied in CFdesign 2010.

Temperature Dependent Heat Generation

A temperature-dependent heat generation simulates an industrial process that operates within a narrow temperature band. Physically this is a thermostat which shuts off the heating device when a target temperature is reached. This option is available for both volumetric and total heat generation boundary conditions. The location of the sensing temperature can be either the part centroid or another location.

To assign a temperature dependent heat generation:

1. Change the Temperature Dependent setting to Enabled.
2. Open the Sensing Location pop-out menu.
3. To choose the part centroid as the sensing location, simply click the Part Centroid button.
4. To select a different location, click the Select Surface button, and click on a surface. The centroid of that surface will be the sensing location.

Note: Heat Generation cannot vary with temperature and time simultaneously.