Advanced Tutorial: Thermal Comfort in a Theater Room

This tutorial contains a thermal comfort project, which analyzes the duct positioning inside a theater, in order to have an effective ventilation system.

Overview

This tutorial teaches how to:

• set up and run a thermal comfort simulation
• assign boundary conditions, material, and other properties to the simulation
• mesh with the SimScale standard mesher

We are following the typical SimScale workflow:

1. Preparing the CAD model for the simulation
2. Setting up the simulation
3. Creating the mesh
4. Run the simulation and analyze the results

1. Prepare the CAD Model and Select the Analysis Type

First of all, click the button below. It will copy the tutorial project containing the geometry into your own Workbench.

The following image demonstrates what should be visible after importing the tutorial project:

If you want to perform the flow volume extraction on your own, you can use the second geometry available:

If you want to extract the flow region

In this case, the model has no opening, so a closed inner region will be created. If you are using another geometry that has openings, refer to this article, that describes all the flow volume extraction methods.

Before you create a closed inner region, you have to hide the walls so you can click on the internal face that is needed. You can do that by selecting the face on the Workbench, then right-clicking on it, and finally by choosing the ‘Hide face‘ option as you can see below:

Please repeat this procedure once more, so that you can see the chairs in the room.

Now we can go back to creating the flow volume. Click on the ‘+‘ next to the CAD model, choose the ‘Add geometry operation‘ , and then select the ‘Closed inner region‘ .

Now you can see the settings panel, make sure the ‘Assignment‘ option is toggled on, choose the floor of the theater by clicking on it after hiding the walls (as you can see below), and finally click on the ‘Start‘ button to proceed.

After the operation is completed, the flow region will appear as in Figure 2.

If you want to extract the flow region

In this case, the model has no opening, so a closed inner region will be created. If you are using another geometry that has openings, refer to this article, that describes all the flow volume extraction methods.

Before you create a closed inner region, you have to hide the walls so you can click on the internal face that is needed. You can do that by selecting the face on the Workbench, then right-clicking on it, and finally by choosing the ‘Hide face‘ option as you can see below:

Please repeat this procedure once more, so that you can see the chairs in the room.

Now we can go back to creating the flow volume. Therefore click on the ‘+‘ next to the CAD mode, choose the ‘Add geometry operation‘ , and then select the ‘Closed inner region‘ .

Now you can see the settings panel, make sure the ‘Assignment‘ option is toggled on, choose the floor of the theater by clicking on it after hiding the walls (as you can see below), and finally click on the ‘Start‘ button to proceed.

After the operation is completed, the flow region will appear as in Figure 2.

And after you extract the flow volume, you can proceed by assigning the following topological entity sets:

• duct outlet
• duct inlet
• seats
• seating floor

For example, in order to set the topological entity set for the duct outlet:

• Click on the outlet of the theater, as you can see below.
• Select the ‘+‘ icon and name it as ‘duct outlet’.

Repeat this for the rest of the sets.

1.1 Create the Simulation

To create a new simulation click on the ‘+’ option next to the ‘Simulations’ tab. Choose ‘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) and hit the ‘Create Simulation‘ button.

Now a new simulation tree will pop up, and you will see the following global settings:

• 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).

The radiation is toggled off for this project. However, all bodies with a temperature greater than absolute zero emit radiation, and in contrast to conduction or convection, this phenomenon requires no medium, so it could also be added, and it becomes more important when the simulation has high temperatures. Learn more about simulating radiation with SimScale here.

2. Assigning the Material and Boundary Conditions

Now we are ready to set up the physics of the simulation. This section includes determining the conditions of the case, from the gravitational load inside the room, to the surfaces’ temperature and flow rate, in order to perform a realistic analysis.

2.1 Assign the 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:

2.2 Define a Material

Click on the ‘+’ icon next to the Materials to start with this assignment:

Assign the standard ‘Air‘ material to the fluid domain by picking it in the material library:

Select ‘Air’ and hit ‘Apply’. Note that you can also just select any material and customize the properties to define whatever material you want to.

Once you have created the new material, you can see the materials data in a new panel:

As there is only one volume, the SimScale platform automatically assigns the material to the flow volume. All you need to do here is hit the ‘Check’ button at the top of the panel.

2.3 Initial Conditions

Default values for initial condition parameters are usually enough. Note that those should not affect the end result of your simulation. However, if these parameters are estimated correctly, the solution will converge faster and the overall convergence stability will improve.

2.4 Boundary Conditions

For the boundary condition set up, a velocity inlet wand a pressure outlet will be assigned on the air entrances and exit. The seats will have a fixed temperature value corresponding to the human organization.

In order to assign a boundary condition, click on the ‘+‘ icon next to the Boundary conditions. Then choose the desired type on the menu that appears:

a. Velocity Inlet

As mentioned before, the two duct inlet faces will receive a flow rate input. Add a new velocity inlet condition and follow the steps below:

• Change the Velocity type to ‘Flow rate‘.
• Change the Flow rate type to ‘Volumetric flow’.
• Volumetric flow rate: \(V\) = 0.3 (m^3 \over\ s).
• Temperature: \(T\) = 15.85 \(°C\).

In order to assign a boundary condition on a topological entity set, make sure the ‘Assignment‘ option is toggled on, then proceed to select the desired topological entity set from the tree at the right of the page.

b. Pressure outlet

For the duct outlet face, use a pressure outlet condition with a fixed gauge pressure value: \(P\) = 0 \(Pa\).

c. ‘No-slip’ walls

For the seats use a no-slip wall condition fixed temperature value: \(T\) = 29.85 \(°C\)

2.5 Set the Numerics & Simulation Control

The default settings for Numerics and Simulation Control are usually suitable. Experienced users can use the manual settings for better convergence. For this thermal comfort tutorial, only change the maximum runtime to 30000 sec, as the simulation will take longer than the default time (1000 sec).

3. Mesh

Click on ‘Mesh‘ to access the global mesh settings, shown in the following picture. Choose the ‘Standard‘ algorithm, and set the ‘Fineness‘ to Level 9 and the ‘Growth rate‘ of the automatic boundary layer to 1.3. Then set the ‘Number of processors’ to 64:

If you are interested to see how to use the standard meshing tool, take a look at this tutorial.

3.1 Adding Refinements

In order to make the mesh more detailed in critical areas, click on the ‘+‘ next to the Refinements, and then choose the ‘Local Element size‘.

Set this refinement by following the next steps:

1. Apply a value of 0.02 \(m\) as a ‘Maximum edge length‘.
2. Make sure the ‘Assignment‘ option is toggled on.
3. Select the ‘seats‘ and ‘seating floor‘ from the Topological Entity Sets list.

4. Start the Simulation

Create a new run by clicking on the ‘+‘ icon next to the ‘Simulation Runs‘:

The mesh will be generated first, and then, while the simulation results are being calculated, you can already have a look at the intermediate results in the post-processor.

As a Community user you cannot perform this step. Instead, you can click the button below to import the results into your own Workbench:

5. Post-Processing

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 on 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%

5.1 PMV (Predicted Mean Vote) Parameter

PMV is an index that aims to predict the mean value of votes of a group of occupants on a seven-point thermal sensation scale. Thermal equilibrium is obtained when an occupant’s internal heat production is the same as its heat loss. The heat balance of an individual can be influenced by levels of physical activity, clothing insulation, as well as the parameters of the thermal environment. For example, thermal sensation is generally perceived as better when occupants of a space have control over indoor temperature (i.e., natural ventilation through opening or closing windows), as it helps to alleviate high occupant thermal expectations on a mechanical ventilation system.
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]

Ideally, the value should be neutral (zero).
Here you can see the results for the PMV parameter:

5.2 PPD (Predicted Percentage of Dissatisfied) Parameter

PPD essentially gives the percentage of people predicted to experience local discomfort. The main factors causing local discomfort are unwanted cooling or heating of an occupant’s body. Common contributing factors are draft, abnormally high vertical temperature differences between the ankles and head, or floor temperature.
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. To learn more about these parameters, visit this blog post: What Is PMV? What Is PPD? The Basics of Thermal Comfort. For a general overview of SimScale’s online post-processing capabilities, the following documentation can be used: New Integrated Post-Processor.
This video shows how the velocity fields can be shown by cutting planes.

Have a look at our post-processing guide to learn how to use the post-processor.

Congratulations! You finished the tutorial!

Last updated: January 8th, 2021