Creating a Simulation-Ready HVAC Layout

Simulating the performance of an HVAC layout can be expedited with the setup process presented here. The process consists of several steps addressing the analysis scope, component characterization, mesh considerations, and solver settings.

An HVAC layout can be designed to achieve an assortment of project specific goals using Simulation CFD.  Contaminant mitigation of lab spaces or hospitals, human comfort in atriums, and energy consumption in factories are only a few examples of design goals influenced by the air and temperature distribution of an HVAC layout. 

Before assessing performance results, the HVAC layout must first be simulated.  An approach to setup HVAC layout simulations will be presented in this section.

HVAC layouts share the following primary concerns which need to be considered in the characterization strategy to prepare your model for Autodesk Simulation CFD.

1. Define Analysis scope

Determine the simulation objectives and the required components.

Simulating the flow and thermal performance of an entire building's HVAC system can be difficult due to the meshing requirements and time to reach a solution.  Often, individual zones are isolated to eliminate unnecessary complexity while understanding their performance as a piece of the whole system.  

An entire building’s HVAC layout is shown above with multiple zones and units.  Simulating all of the details and complexities for the entire building would not be practical.

The ground floor cafeteria zone will be isolated for simulation.

2. Characterize components

Production CAD models are usually not suitable to use directly in simulation.  A process for preparing geometry for simulation can be found in the CAD Chapter, where new simulation-specific geometry is created by referencing existing entities.  Once the geometry is prepared for simulation, materials and boundary conditions characterize their operation and influence on the system. 

Air Space

The cafeteria air space (red outlines) is created in CAD by referencing existing entities.

The cafeteria air space (red outlines) is created in CAD by referencing existing entities.

What it is: Domain where flow and thermal performance will be evaluated.

How it is simulated: Explicitly modeled or automatically created from void (empty space between walls, windows, ceiling, and floor).  See the Component Characterization section.

The air space is created by referencing wall, window, floor, and ceiling entities that exist.  Typically a simple extrusion from floor to ceiling is created by projecting wall edges.  More complicated spaces may require additional features to create a volume representing the air space.


Walls, windows, doors, and other exterior elements

What it is: Contain the air space and influence system performance by absorbing and transferring energy.

How it is simulated: Represented as boundary conditions or simple geometry. See the Walls and Windows page in the component characterization section.

These elements are typically not modeled explicitly as they are represented by boundary conditions that account for their influence on the system.    

Boundary conditions view of an air volume with film coefficients defined on two (2) of the exterior windows (surfaces with green stripes) to represent their respective U-factors.  Exterior faces without boundary conditions will be considered adiabatic.

Supply / Return

What it is: Provide or remove air and thermal energy from the space.

How it is simulated: Boundary conditions on surfaces are used, ducting is not typically modeled. See the Diffuser characterization page.

Supplies and returns provide or remove air and thermal energy from the space.  Boundary conditions are used to define the openings and transfer of thermal energy.

Review the video below for details on representing supply and return ducting.

Simulation model consisting of an air volume (1), a single solid volume representation of the ducting (2), and returns (3).

The internal flow characteristics of ducting are typically unnecessary in the simulation of a room’s air space.  The internal ducting complexities can be omitted by modeling a single volume, from the external surfaces of the ducting, that is then suppressed in simulation.

The system’s flow rate and supply temperature are applied to the model surfaces that represent the supplies and the returns.  Please review Boundary Conditions section for further details on properly constraining an AEC simulation.

Indented supply faces of ducting model improves the simulation results.

Indented supply faces of ducting model improves the simulation results. 

TIP: Indenting simulation inlet faces (supply faces of ducting model) improves the solution at inlets, see the diffuser characterization page for further details.  Outlets should be extended as well to allow flow to develop prior to exiting the system.


A detailed generator model (left) is idealized for simulation (right).

A detailed generator model (left) is idealized for simulation (right).

What it is: Machinery, computers, or any other pieces of equipment that add heat and/or influence air movement.

How it is simulated: Devices or simple shapes with heat generation or temperature boundary conditions are typically used to represent equipment.

Machinery, electronics, or any other pieces of equipment that add heat and/or influence air movement may need to be considered in a simulation.  Equipment comes in many forms and is typically represented by solid volumes with material properties and boundary conditions used to define their influence on the space. 

TIP: Including the complexities of equipment should only occur after simple simulations, done without the equipment, have been completed successfully.  This not only helps quantify the impact of the equipment but also expedites the initial setup and solution of a simulation.

Some pieces of equipment can be characterized with material devices such as air handlers and heat exchangers shown in the component characterization module.  Others require a custom representation as shown in the generator image on this page.  Review the component characterization process section for guidance on approaching custom characterization.

Temperature boundary conditions are applied to all external surfaces of the idealized generator (left).  The boundary conditions allow the piece of equipment to interact with its surroundings; temperatures are shown on the generator and surrounding air on the right.


What it is: Add heat, act as flow obstructions, and are considered for thermal comfort predictions.

How it is simulated: Are only modeled when thermal comfort predictions are necessary; otherwise, their heat generation is applied to the air space volume.

Most HVAC layouts are designed to accommodate occupants by handling their heat load without high velocity air movement.  Occupants’ influence on a space can typically be accounted for by assigning their heat generation as a boundary condition to the air space volume (or resistance volume) without explicitly modeling people in CAD.  Review the occupant characterization page for strategies to account for occupants. 

However, occupants should be explicitly modeled when their thermal comfort is to be solved for.  Review the section on interpreting CFD results for further details.

An occupant sitting at his desk (left) is modeled for thermal comfort result (right)

An occupant sitting at his desk (left) is modeled for thermal comfort result (right)

3. Mesh Considerations

Flow openings and volume growth should be refined.

Understanding and implementing concepts from the meshing module will guide mesh generation for most AEC situations.  However, HVAC layout simulations typically require additional refinements due to their large air domains in conjunction with relatively small details of supplies and returns.  The two most common refinements in HVAC layout simulations are:

  1. Volume growth rate adjustment
  2. Uniform refinement of openings

Volume growth rate is an advanced meshing control that defines the rate at which mesh elements grow in a volume.  The default value is 1.35 (35% growth) and is commonly adjusted to 1.15 - 1.25 for larger domains.  The impact of adjusting this setting is depicted here.

Volume growth rate in the Advanced Meshing Controls of the Advanced Mesh Size dialog is adjusted to 1.25.  Note the checkbox must be selected to invoke the adjustment.

Using a uniform mesh ensures opening surfaces have an adequate resolution. The Use Uniform button of the mesh dialog forces the mesher to maintain the mesh element size of selected entities (recall that mesh element sizes can shrink or grow).  This is most useful for openings of HVAC layout simulations (also applicable to devices).  

Top: Default mesh with five (5) nodes along the height (red arrow).  The element sizes grow away from the edge and degenerate to less elements in the center of the face.

Bottom: Uniform mesh refined to have nine (9) elements along the height.  Note the element sizes remain the same size along the surface.

4. Solver settings

The large domain size, heat loads, supplies, and returns of HVAC layout analyses typically result in a mixed convection simulation.

For best practices on adjusting solver settings for forced and mixed convection scenarios, please refer to the Solver Settings page.