Surface Boundary Conditions

Velocity is commonly used as an inlet boundary condition. It can be specified as normal to the selected surface or in Cartesian coordinates. A velocity can be applied to an outlet, if the direction is defined as out of the model.

To assign a Velocity condition that is normal (perpendicular) to the selected surface:

1. Set the Type to Velocity, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Set the Method to Normal.
4. Enter the value in the Velocity Magnitude field.
5. Optionally, click Reverse Normal to change the flow direction.
6. Optionally, define a fully developed profile by checking Fully Developed. (See note below.)
7. Click Apply.

Example assigning Velocity Boundary Condition

Fully Developed flow

To apply velocity components

To simulate a moving ground plane

This condition applies a rotating velocity to a wall, and is used for simulating a rotating object surrounded by a fluid. An example is the rotating disk in a computer hard drive. This condition does not induce flow caused by rotation (as in a pump impeller), and is not a turbo-machinery condition. (Use a rotating region for such applications.)

To assign a Rotational Velocity condition:

1. Set the Type to Rotational Velocity, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Enter the velocity in the Rotation Speed field.
4. To set the rotational axis, first set the Point on Axis. Click the pop-out, and select a surface. The centroid of the selected surface will be a point on the axis.
5. To set the Axis Direction, click the pop-out. Choose the Global X, Y, or Z axes to choose a Cartesian direction as an axis direction.
6. To graphically set the direction, click the Pick on button, and select a surface. The axis will be normal to the selected surface.
7. Click Apply.

A Volume Flow Rate is applied to a planar openings. It is most often used as inlet condition, and is particularly useful if the density is constant throughout the analysis. A volume flow rate can be applied to an outlet, if the flow direction is out of the model.

To assign a Volume Flow Rate condition:

1. Set the Type to Volume Flow Rate, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Enter the value in the Volume Flow Rate field
4. Optionally, click Reverse Normal to change the flow direction.
5. Optionally, define a fully developed profile by checking Fully Developed. (See note below.)
6. Click Apply.

Fully Developed flow

A Mass Flow Rate is applied to a planar inlets or outlets. It is most often used as an inlet condition. A mass flow rate can be applied to an outlet, if the flow direction is out of the model.

To assign a Mass Flow Rate condition:

1. Set the Type to Mass Flow Rate, and set the Unit type.
2. Set the Time dependence (Steady State or Transient).
3. Enter the value in the Mass Flow Rate field
4. Optionally, click Reverse Normal to change the flow direction.
5. Click Apply.

When applying to multiple surfaces at the same time, the flow direction must be the same.

The Pressure boundary condition is typically used as an outlet condition. The recommended (and most convenient) outlet condition is a static, gage pressure with a value of 0. When applied, no other conditions are needed at an outlet.

A non-zero pressure condition can be applied as an inlet condition. If the pressure drop through a device is known, specify the pressure drop at the inlet (as a static gage pressure), and a value of 0 static gage at the outlet.

To assign a Pressure condition:

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

Example assigning Pressure Boundary Condition

Gage is a relative pressure, and is the default. Absolute pressure is the sum of the gage and the Material Environment pressures.

Total pressure is the sum of the static pressure and the dynamic pressure, and is often useful for compressible analyses. For certain analyses, such as some turbomachinery applications, the total pressure is physically constant and the static pressure and velocity vary. For these analyses, applying a non-zero total pressure boundary condition is a recommended strategy.

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. Enter the value in the Temperature field.
4. Select either Static or Total
5. 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.

The slip condition causes the fluid to flow along a wall instead of stopping at the wall, which typically occurs along a wall. Fluid is prevented from flowing through the wall, however.

Slip walls are useful for defining symmetry planes. The symmetry surface does not have to be parallel to a coordinate axis.

To assign a Slip condition:

1. Set the Type to Slip/Symmetry.
2. Click Apply.

There is no value associated with the Slip condition.

Example assigning a Slip/Symmetry boundary condition

The slip condition can be used with a very low fluid viscosity to simulate Euler (inviscid) flow.

This is a “natural” condition meaning that boundary is open, but no other constraints are applied.

Unknown is used mostly at the outlets of compressible flow analyses. For supersonic flow, neither the outlet pressure nor the velocity are known. Either condition could result in shock or expansion waves at the outlet.

To assign an Unknown condition:

1. Set the Type to Unknown.
2. Click the Apply button.

There is no value associated with the Unknown condition.

Theoretical explanation

The Unknown boundary condition is a mixed Neumann-Dirichlet-type (specified value) boundary condition applied to the pressure variable. It is implemented into the solution in a two-part process:

1. During the matrix solution of the pressure equation, nodes assigned an Unknown boundary condition are treated as fixed or specified (Dirichlet).
2. After the matrix solution, the values on these nodes are re-calculated as the average of the neighboring values, effectively enforcing a zero gradient (Neumann) condition on the pressure equation.

Example assigning an Unknown boundary condition

This is a unitless quantity ranging between 0 and 1 that represents the concentration of the scalar quantity for tracking concentrations.

To assign a Scalar condition:

1. Set the Type to Scalar.
2. Set the Time dependence (Steady State or Transient).
3. Specify the value (between 0 and 1) in the Scalar field.
4. Click Apply.

This is a unitless quantity ranging between 0 and 1 that represents relative humidity (1 corresponds to a humidity level of 100%).

To assign a Humidity condition:

1. Set the Type to Humidity.
2. Set the Time dependence (Steady State or Transient).
3. Specify the value (between 0 and 1) in the Humidity field.
4. Click Apply.

This is a unitless quantity ranging between 0 and 1 that represents the steam quality (1 corresponds to a quality of 100%--pure steam).

To assign a SteamQuality condition:

1. Set the Type to Steam Quality.
2. Set the Time dependence (Steady State or Transient).
3. Specify the value (between 0 and 1) in the Steam Quality field.
4. Click Apply.

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 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.

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 Wm²/K 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 Wm²/K 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

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.

External fan is another way to move flow in or out of a device. An external fan is defined as a head-capacity curve, resulting in an inlet flow rate that varies with the pressure drop of the device. This is a convenient way to determine the operating point of a fan for a particular flow path.

To assign an External Fan condition:

1. Set the Type to External Fan, and set the Unit type.
2. Enter the rotation speed of the fan in the Rotational Speed field.
3. If needed, change the rotational direction by clicking Reverse Direction. The direction is drawn with an arrow.
4. Specify the fan curve by clicking the Fan Characteristic Edit button.
   • Click Insert to add rows between defined rows.
   • Click the Plot button to view the plot.
   • The Import button imports a comma separated variable (CSV) file, and the Save button saves the curve information to a CSV file.
   • To enter a fan that pulls flow (at an outlet), enter all flow rate and pressure values as negative.
5. Enter a slip factor (between 0 and 1) in the Slip Factor field.
6. Click Apply.

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.

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.

Periodic boundary conditions (cyclic symmetry) enable the simulation of a single passage of an axial or centrifugal turbomachine or of a non-rotating device with repeating features (passages).

Periodic boundaries are always applied in pairs; the two members of a periodic pair have identical flow distributions, and must be geometrically similar.

Periodic pairs are used at the inlet and outlets of repeating devices:

To assign a Periodic condition to Pair 1:

1. Select the first surface of pair 1.
2. Set the Pair ID to 1 and the Side ID to 1.
3. Click Apply.
4. Select the second surface of Pair 1.
5. Set the Pair ID to 1 and Side ID to 2.
6. Click Apply.

Repeat for the remaining pairs.

Periodic boundary conditions are a convenient way to include the effect of multiple repeating features in a simplified model. Because of the repeating geometry, the flow upstream and downstream of a device will be the same for each passage.

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.