User Guide: Thermal Comfort in a Theater Room

This user guide contains a thermal comfort project, which analyses the duct positioning inside a theater, in order to have an effective ventilation system.
Reference case:
Thermal Comfort in a Theater Room through Ventilation

Relevant pages:

• Simulating Thermal Comfort In a Ventilated Office Space | SimScale Tutorial
• HVAC Simulation of an Office – Testing Thermal Comfort

Geometry

Geometry Preparation

Prepare the geometry for the simulation:

• If the CAD model contains small features, fillets or round faces, which are unlikely to have an impact on the result, it is recommended to remove those details before importing the model into SimScale.
• The solid volumes should be non-overlapping and should all be touching each other.

Flow Volume Extraction

This CAD model does not contain the fluid volume by default. However, the fluid region can be extracted as a single part, using the flow volume extraction operation within the SimScale workbench. As this is a model with no openings, the closed inner region feature is applied.
You can find a detailed tutorial on flow volume extraction here.

Simulation Setup

Create a Simulation

• To create a new simulation click on the ‘+’ option next to the ‘Simulations’ tab.
• Choose the ‘Convective heat transfer’ (This analysis type is used when temperature changes in the fluid lead to density variations and movement of the fluid due to gravity).

• Choose the ‘k-omega SST‘ turbulence model (This turbulence model switches in between the k-omega and k-epsilon models automatically. Therefore it takes advantage of both models).
• Apply the ‘Steady-state‘ option (In most thermal comfort analysis projects, the area of interest is the final state).

Model

Click on ‘Model’ in the simulation tree to define the gravity force acting on the domain. In this case, gravity is defined in the negative y-direction:

Materials

Assign the standard ‘Air‘ material to the fluid domain. Here is a short video on how to assign ‘Materials‘ to different parts of the model. You can customize the material properties as you want.

Initial Conditions

Default values for initial condition parameters are usually enough. If these parameters estimated correctly, the solution will converge faster.

Boundary Conditions

Flow inlet and outlet boundary conditions can be defined in the two following ways:

• Inlet controlled (defining velocity, flow rate or pressure, on domain inlet).
• Outlet controlled (defining suction velocity, flow rate or pressure on domain outlet).

Walls can be defined with specific temperature and heat transfer parameters.
While surface heat sources can be defined by ‘fixed temperature‘ or ‘turbulent heat source’, adiabatic conditions can be defined by ‘zero gradient’ Temperature.
By leaving surfaces unassigned, the default ‘No-slip‘ wall condition is applied to them.
Assign the following boundary conditions:

• Duct inlets: Volumetric flow rate of 0.11 m^3/s

• Duct outlet: Pressure outlet with a fixed value of 101325 Pa.

• Building and seating surfaces: 303 K fixed temperature, ‘No-slip’ wall condition.

Boundaries can be selected in the following way:

1. Hide the duct walls (right-click, Hide selection).
2. Select the rest of the geometry (right-click, select all).
3. Assign the wall conditions to the rest of the walls.

Duct walls: ‘No-slip’ wall condition, ‘Zero gradient’ temperature.

Numerics

The default settings are usually suitable. Experienced users can use the manual settings for better convergence.

Simulation

The Simulation Control settings define the general controls over the simulation. Apply the following controls:

• Start time: 0 s
• End time: 2000 s
• Delta t: 1 s (Since this is a steady-state analysis, time variables define iteration number. 2000 iterations would be enough for thermal comfort analysis.)
• Write interval: 2000 timestep (in a steady-state analysis, only the final state of the system is important.)
• The number of processors: 32 (Increase the number of processors according to the complexity of the model.)
• Maximum runtime: 120000 s

Meshing

Use the ‘Hex-Dominant (only-CFD)’ mesh. This is the most automated approach and is usually the best starting point. In mesh mode select:

• Meshing Mode: Internal
• Fineness: Moderate
• Mesh with 32 processors as a starting point. Increase the mesh ‘Fineness’ and ‘Number of processors’ according to the complexity of the model.

Simulation Run & Results

After the meshing, create a new ‘Simulation Run‘.
For thermal comfort studies, usual parameters of interest are the PMV (Predicted Mean Vote) and PPD (Predicted Percentage of Dissatisfied). The inputs for those parameters can be found in this page, and the calculated values should be within the following ranges:

• PMV valid range: -3 (cold) to +3 (hot)
• PPD valid range : 5% – 100%

PMV (Predicted Mean Vote) Parameter

And in order to comply with the standards, the PMV values should be within these ranges:

• PMV comfort range:
  • ASHRAE 55 recommended limit: [-0.5, 0.5]
  • ISO 7730:
    • Hard limit: [-2, +2]
    • New buildings: [-0.5, +0.5]
    • Existing buildings: [-0.7, +0.7]

Here you can see the results for the PMV parameter:

PPD (Predicted Percentage of Dissatisfied) Parameter

According to the PPD ASHARE-55, the recommended comfort range is: [0%, 20%], and the results for this parameter are the following:

Both the PMV and PPD results show no compliance with the standards for the thermal comfort of this theater, so new measures regarding the ducting should be taken into account in order to improve them.
For a general overview of SimScale online post-processing capabilities, the following documentation can be used: here.
This video shows how the velocity fields can be shown by cutting planes.

Last updated: March 30th, 2020