Chapter 9: Assigning Boundary Conditions

Previous: Exercise 2 | Next: Exercise 3

In the previous chapter, we discussed assigning, creating, and managing materials within the design study. In this chapter, we focus on how the design interacts with its surroundings. By assigning boundary conditions such as flow rate, pressure, and temperature to openings and other specific locations, we effectively "connect" the design with the physical world. Additionally, boundary conditions allow us to specify internal heat loading, such as heat dissipation often found in electronics thermal management simulations.

Boundary conditions define the inputs of the simulation model. Some conditions, like velocity and volumetric flow rate, define how a fluid enters or leaves the model. Other conditions, like film coefficient and heat flux, define the interchange of energy between the model and its surroundings.

Boundary conditions connect the simulation model with its surroundings. Without them, the simulation is not defined, and in most cases cannot proceed. Most boundary conditions can be defined as either steady-state or transient. Steady-state boundary conditions persist throughout the simulation. Transient boundary conditions vary with time, and are often used to simulate an event or a cyclical phenomena.

Note: Flow and heat enter and leave the model at specified locations. External surfaces that have no boundary conditions are considered adiabatic walls (no flow and no heat transfer).

Using Boundary Conditions

To assign a Boundary Condition

To begin, enable the Boundary Condition task from either the Setup (tab) > Setup Tasks (panel) (A) or from the Design Study bar (B):

To work close to the model:

  1. Left click on the model entity (surface or part).
  2. Click the Edit button on the context toolbar.
  3. Specify settings in the Boundary Conditions quick edit dialog.

Alternatively, right click on the model entity or branch on the Design Study bar, and click Edit...

To work away from the model:

  1. Left click on the model entity (surface or part) to select it.
  2. Click Edit in the Boundary Conditions context panel.
  3. Specify settings in the Boundary Conditions quick edit dialog.

To assign the boundary condition in the quick edit dialog:

  1. Set the Type of condition.
  2. Set the Units (if applicable).
  3. Set the Time Variation (Steady State or Transient).
  4. Apply condition-specific settings such as Normal or Component for Velocity or Static or Gage for Pressure. Change the flow direction for velocity, volume flow rate, or mass flow rate.
  5. Specify the value.
  6. Click Apply.

To define and then apply a boundary condition

An alternative workflow is to create a boundary condition before applying it to the model.

  1. Click Edit on the Boundary Conditions context panel. Alternatively, right click on the Boundary Conditions branch of the Design Study bar, and click New BC....
  2. Define the boundary condition in the Boundary Conditions quick edit dialog, and click Apply.
  3. Drag the unassigned setting from the Design Study bar onto the model entity:

Note: To assign a setting that is currently assigned to another object, drag it from the Design Study bar onto the model entity.

To Remove a Boundary Condition

To remove a boundary condition from a specific entity (several ways):

To remove a single boundary condition from multiple entities:

  1. Expand the Boundary Condition branch in the Design Study Bar.
  2. Right click on the condition to remove.
  3. Click Remove.

To delete all boundary conditions:

  1. Right click on the Boundary Condition branch of the Design Study bar.
  2. Click Remove All.

Flow Boundary Conditions

Flow boundary conditions answer these questions:

Flow can be driven in several ways:

Flow boundary conditions are applied to exterior surfaces, and typically include:

Inlet

Outlet

Flow rate

Pstatic = 0

P static = 0

Flow rate

Pstatic > 0

Pstatic = 0

External fan (push)

Pstatic = 0

Pstatic = 0

External fan (pull)

Pstatic = 0 (internal fan)

Pstatic = 0

The most commonly used flow boundary conditions...

Velocity

  • Velocity is typically used as an inlet boundary condition.
  • Specify either normal to the selected surface or in Cartesian components.
  • A velocity can be applied to an outlet, if the direction is defined as out of the model.
  • To define a fully developed flow profile to a velocity condition, check Fully Developed.

Volume Flow Rate

  • Apply to planar inlets (and sometimes outlets).
  • This is most useful if the density is constant.
  • To define a fully developed flow profile to a volume flow rate condition, check Fully Developed.

Mass Flow Rate

  • Mostly applied to inlets (planar only).
  • A mass flow rate can be applied to an outlet, if the flow direction is out of the model.

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.
  • No other conditions are needed at an outlet.
  • 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.

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.

There are more flow boundary conditions available in Autodesk Simulation CFD. The conditions listed above are the most commonly used. Click here to view descriptions of all flow boundary conditions in Autodesk Simulation CFD...

Heat Transfer Boundary Conditions

Heat can come from a known temperature, a heat load (such as an electronic chip), radiation, or resistance to electrical current. Heat boundary conditions answer these questions:

Note: A temperature must be specified in the model for Autodesk Simulation CFD to solve for heat transfer. This can be a temperature or a film coefficient boundary condition.

The most commonly used heat transfer boundary conditions...

Temperature

  • A temperature boundary condition should be specified at all inlets when running heat transfer.
  • A static temperature condition is recommended for most heat transfer analyses.
  • Use total temperature as an inlet temperature for compressible heat transfer analyses.

Total Heat Flux

  • Total Heat flux is a surface condition that imposes heat directly to the applied surface.
  • Apply the total heat flux condition directly. (Do not divide 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.

Film Coefficient

  • Also known as a convection condition, this is often used to simulate a cooling effect.
  • Assign film coefficients to external surfaces to simulate the effect of the environment that is external to the device.
  • Should only be applied to external surfaces.

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.

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.

There are more heat transfer boundary conditions available in Autodesk Simulation CFD. The conditions listed above are the most commonly used. Click here to view descriptions of all heat transfer boundary conditions in Autodesk Simulation CFD...

Previous: Exercise 2 | Next: Exercise 3

Back to Training Title Page

Parent topic: Self-Paced Fundamentals Training