Product help with community knowledge

### Page statistics

3510 views2 edit(s)61474 characters(s) Page last modified 06:44, 24 Oct 2012 by len.whitehead

# Surface Boundary Conditions

Surface boundary conditions typically represent a quantity or flux that enters or leaves the model (flow, temperature, or heat, for example). For 3D models, surface conditions are available when the selection type is Surface. For 2D models, Edge must be the selection type.

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.

Velocity

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.

Fully Developed flow

Unless the objective of an internal flow simulation is to study entrance effects, most pipe and duct flows are assumed to be fully developed. The fully developed flow profile is generally more physically realistic than a uniform (slug) profile. Its use eliminates the need to add an entrance length upstream of the model inlet.

The Fully Developed profile is an option for the Velocity (Normal direction) and Volume Flow Rate boundary conditions. It is available for the following planar surface types: quadrilateral (4 edges), circular (1 edge or 2 edges), or triangular (3 edges).

To assign a fully developed flow profile, check Fully Developed on the Boundary Conditions quick edit dialog.

To apply velocity components

1. Change the Method to Component.
2. Check the components to specify.
3. Enter the velocity value for each component in the corresponding Magnitude field.
4. Click Apply.

To simulate a moving ground plane

To correctly model many land-based aerodynamic applications such as the ground-effects on a car, the velocity difference between the object and the ground must be simulated. If the relative motion with the ground is neglected, the aerodynamic interaction between the object and the ground will not be properly computed.

1. Select the ground surface, and select Velocity as the boundary condition type.
2. Specify the desired units.
3. Set the Method to Component.
4. Check the desired component of velocity that corresponds to the direction of the flow, and specify the value. (The direction is typically the same as the inlet air velocity, which is the opposite to the direction of travel of the object. Because the object does not move in the analysis, the flow and ground move relative to it.)

When the analysis is run, the velocity applied to the ground surface simulates the relative air flow between the object and the ground.

Rotational Velocity

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.

Volume Flow Rate

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.
NoteWhen applying to multiple surfaces at the same time, the flow direction must be the same.
NoteStandard flow rate can be applied as a boundary condition if the properties of the fluid are also at standard conditions. If the fluid properties different from standard, you should convert your standard flow rate condition to an actual flow rate condition. Do this by multiplying the standard flow rate by the ratio of the standard fluid density to the actual fluid density.

Fully Developed flow

Unless the objective of an internal flow simulation is to study entrance effects, most pipe and duct flows are assumed to be fully developed. The fully developed flow profile is generally more physically realistic than a uniform (slug) profile. Its use eliminates the need to add an entrance length upstream of the model inlet.

The Fully Developed profile is an option for the Velocity (Normal direction) and Volume Flow Rate boundary conditions. It is available for the following planar surface types: quadrilateral (4 edges), circular (1 edge or 2 edges), or triangular (3 edges).

To assign a fully developed flow profile, check Fully Developed on the Boundary Conditions quick edit dialog.

Mass Flow Rate

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.

Pressure

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.

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.

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

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

Slip/Symmetry

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.

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

NoteFor axisymmetric analyses, the symmetry condition along the axis is automatically set, and does not need to be applied manually.

Unknown

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.

Scalar

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.

Humidity

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.

Steam Quality

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

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.

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

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.
NoteAssign the radiation boundary condition to external surfaces only.

External Fan

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.
NoteThe slip factor is the ratio of the true rotational speed of the flow to the rotational speed of the fan blades. Due to inefficiencies in the fan, slip can result in a slower flow tangential flow velocity than expected. Autodesk Simulation CFD determines the flow tangential velocity component by multiplying the slip factor by the user-supplied fan rotational speed. The default slip factor is 1.0. This means that the rotational speed of the flow is the same as the rotational speed of the fan.

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

Periodic

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.

NoteMesh Enhancement is automatically disabled when Periodic boundary conditions are applied. This is done to improve solution stability. To enable Mesh Enhancement, open the Mesh quick edit dialog, and click the Enhancement button, and check the Enable mesh enhancement box.

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.

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.
NoteRadiation must be enabled (on the Solve dialog) for the Transparent boundary condition to work.
NoteThe Background Temperature can be varied with time by clicking the Transient bullet, and specifying the time function.