Fill out the form to download

Required field
Required field
Not a valid email address
Required field
Required field
  • Set up your own cloud-native simulation in minutes.

  • Documentation

    Advanced Tutorial: Thermal Comfort in a Theater Room

    This tutorial analyzes the duct positioning inside of a theater room, aiming to study the effectiveness of the ventilation system and the resulting thermal comfort.

    temperature result from theater simulation tutorial simscale
    Figure 1: Visualization of the temperature across a cutting plane


    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. Prepare the CAD model for the simulation
    2. Set up the simulation
    3. Create the mesh
    4. Run the simulation and analyze the results

    1. Prepare the CAD Model and Select the Analysis Type

    Attention (if you have a Community or an Academic account)!

    Performing the calculation of this tutorial will consume around 200 core hours.

    This might be a big hit for Community and Academic plans. However, if you want to explore the possibilities of SimScale, you can follow all the instructions regarding the setup. During this tutorial, you will have the option to import the results for the mesh and the calculations in your Workbench with one click. By doing so, you can continue analyzing the results by yourself.

    Note (if you are not using the tutorial CAD model)

    Prepare the geometry for the simulation (only if you are not using the tutorial’s CAD model):

    • 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.

    Imported model

    The imported model represents the flow volume, and the saved selections have already been created so you don’t have to spend time selecting the faces manually. If you want to learn more regarding flow volume extractions, have a look here.

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

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

    cad model for theater thermal comfort study
    Figure 2: This CAD model of a theater room will be used for a thermal comfort study.

    If you want to perform the flow volume extraction on your own, you can use the ‘Theater – without flow volume extraction’ geometry, and use the CAD mode tool:

    model without the flow volume extraction and topological entities
    Figure 3: The model of the theater room without a flow volume extraction. The button to enter CAD mode is highlighted in blue

    The icon highlighted in Figure 3 will take you to the CAD mode, where you can perform the flow volume extraction. For more details and instructions, please refer to this article. Additionally, you can have a look at the CAD mode operations performed for the ‘Theater’ geometry and repeat the same.

    After you extract the flow volume, you can proceed by assigning the following saved selections (notice that in the ‘Theater’ geometry the sets are already created):

    • duct outlet
    • duct inlet
    • seats
    • seating floor

    For example, to set the saved selection 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’.
    saved selection creation duct outlet theater room, study of thermal comfort
    Figure 4: Creating a saved selection for the duct outlet

    Repeat this for the rest of the sets.

    topological entity set names
    Figure 5: Saved selections that will later be used for boundary conditions and mesh refinements

    1.1 Create the Simulation

    To create a new simulation click on the ‘+’ option next to the ‘Simulations’ tab. Choose ‘Convective Heat Transfer’, which is used when temperature changes in the fluid lead to density variations and movement of the fluid due to gravity. Finally, hit the ‘Create Simulation‘ button.

    analysis type convective heat transfer
    Figure 6: Choosing the convective heat transfer analysis

    At this point, a new simulation tree will appear. By clicking on the first entry in the simulation tree, you will see the following global settings:

    turbulence model for the convective heat transfer analysis is k-omega SST, for thermal comfort analysis
    Figure 7: Setting the time dependency to steady-state and the turbulence model to k-omega SST at the simulation properties
    • Choose the ‘k-omega SST‘ turbulence model. This turbulence model blends between the k-omega and k-epsilon models automatically, therefore, it takes advantage of both models.

    The radiation button 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 rates.

    2.1 Define Gravity

    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:

    gravity model in the simscale workbench
    Figure 8: Adding the properties for gravity according to the part’s coordinate system

    2.2 Define a Material

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

    simulation tree at the beginning of the simulation setup of tutorial
    Figure 9: Adding the material of the flow region

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

    material library air assignment
    Figure 10: Choosing air 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:

    air properties for the fluid
    Figure 11: The properties of air that will be used for the flow region

    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 result of your simulation. However, if these parameters are estimated reasonably, the solution will converge faster and the overall convergence stability will improve.

    2.4 Boundary Conditions

    Options for defining boundary conditions for flow simulations

    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 ‘adiabatic’ temperature.
    By leaving surfaces unassigned, the default ‘No-slip‘ wall condition is applied to them.

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

    overview of boundary conditions for theater thermal comfort simulation
    Figure 12: Boundary conditions overview

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

    add boundary condition
    Figure 13: Adding a new boundary condition

    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 \(°C\).

    To assign a boundary condition on a saved selection, proceed to select the desired saved selection from the tree at the right of the page.

    velocity inlet for entrance of ducts
    Figure 14: Velocity inlet with a volumetric flow input for the entrance of the ducts

    b. Pressure outlet

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

    pressure outlet assignment for the ducts of theater room, thermal comfort study
    Figure 15: Pressure outlet with a fixed value input for the outlet of the ducts

    c. ‘No-slip’ walls

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

    no slip wall assignment with foxed value for seats of theater room
    Figure 16: No-slip wall conditions for the building walls and the seatings of the theater

    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 seconds, as the simulation will take longer than the default maximum runtime.

    maximum runtime value for the simulation
    Figure 17: Simulation control panel with the assigned maximum runtime input


    The maximum runtime of your simulation is specified in real clock time. When the simulation run surpasses this limit, it will be cancelled.

    3. Result Control

    Result control items allow us to request the solver to compute special quantities from the simulation, that are not delivered by default. In this case, we will request the Thermal Comfort Parameters fields, as we are interested in these quantities for the evaluation of the results.

    For this, create a new Field calculation under Result control, of type ‘Thermal Comfort Parameters’, as shown in the image:

    thermal comfort parameters result control field calculation
    Figure 18: Requesting Thermal Comfort Parameters as a result field

    In the setup panel that opens, we can leave the default values and click the blue check-mark button to accept and close.

    4. Mesh

    Click on ‘Mesh‘ to access the global mesh settings, shown in the following picture. Choose the ‘Standard‘ algorithm, and set:

    • Fineness to ‘9’
    • Under Advanced settings, set Small feature suppression to ‘0.001’
    settings for the standard meshing
    Figure 19: Mesh panel for the Standard mesher with automatic sizing

    If you are interested to see all configuration options from the standard meshing tool, please take a look at this tutorial.

    5. Start the Simulation

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

    how to start a new thermal comfort simulation run after the setup
    Figure 20: Simulation setup tree before starting the simulation

    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 Workbench:

    6. Post-Processing

    For thermal comfort studies, the 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%

    6.1 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, the thermal sensation is generally perceived as better when occupants have control over indoor temperature (i.e., natural ventilation through an opening or closing windows), as it helps to alleviate high occupant thermal expectations on a mechanical ventilation system.

    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, from a thermal comfort perspective, the PMV value should be neutral (zero). To analyze the PMV levels around the occupants, let’s start by hiding the ducts and outer walls from the computational domain. The intention is to have a clear view of the inside:

    hiding faces of the computational domain in the post processor
    Figure 21: By selecting the external faces of the domain and hiding them, you get a clearer view of the internal faces
    1. With face selection enabled, select the faces to be removed from the view
    2. Once the faces are selected, right-click on the viewer
    3. Choose the ‘Hide selection’ option

    At this point, the interior of the theater will be visible:

    post processor view after hiding faces
    Figure 22: View of the theater after hiding faces that were blocking the view

    A good way to analyze the PMV contours around the seats is with a Cutting plane filter. The following image shows an example:

    predicted mean vote parameter distribution theater, thermal comfort, convective heat transfer post processing
    Figure 23: Cutting planes are highly customizable, allowing different positioning, orientation, coloring, and vectors, amongst other options.
    1. To create a brand new cutting plane, click on ‘Cutting Plane’ in the filters ribbon
    2. Since the seats go up at an angle, you can expand the Orientation tab and adjust the normal directions to ‘-0.27’ in X, ‘1’ in Y, and ‘0’ in Z
    3. Likewise, the Position tab can be changed to place the cutting plane in the region of interest
    4. Finally, adjust the Coloring to ‘Predicted Mean Vote’.

    Now the PMV value around the seats is visible, with some regions extrapolating the 0.5 PMV threshold, as well as two small regions with PMV less than -0.5.

    6.2 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%]. By using the same cutting plane that was created previously, adjust the Coloring to ‘Predicted Percentage of Dissatisfied’:

    ppd parameter distribution theater thermal comfort convective heat transfer post processing
    Figure 24: The distribution of the PPD parameter through the room.

    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 to improve them. To learn more about these parameters, visit this blog post: What Is PMV? What Is PPD? The Basics of Thermal Comfort.

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

    Congratulations! You finished the tutorial!


    If you have questions or suggestions, please reach out either via the forum or contact us directly.

    Last updated: October 25th, 2023