Documentation

User Guide: Thermal Comfort

Geometry Preparation

Geometry

Make the geometry ‘CFD ready’:

  • If the CAD has so many small fillets or round faces which can be insignificant for the analysis, then It is recommended to clean the CAD in this case – Remove fillets, Merge small faces
  • Small features which don’t contribute to the flow need to be removed.
  • The solid volumes should be non-overlapping and should all be touching each other.

This is a thermal comfort project, which analyses the duct positioning inside a theatre space, in order to have an effective ventilation system. For thermal comfort studies, it is important to see Effective Draft Temperature (EDT) and Air diffusion performance index (ADPI).  While the EDT provides a quantifiable indication of comfort, ADPI quantifies the overall comfort of space when in cooling.

Theater model ready for CFD analysis with thermal comfort

Reference Case

Import CAD geometry. The supported formats are STEP, IGES, STL, SolidWorks, Autodesk Inventor, Rhino, Parasolid and ACIS.

Create the air volume

Extract the fluid region by using geometry operations. A detailed tutorial is shown here.

Flow Volume Extraction within the platform

Add a Simulation

  • 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.)
  • k-omega SST (This turbulence switches in between k-omega and k-epsilon models automatically, therefore it takes the advantage of both models.)
  • Steady-state (In thermal comfort analysis, often the area of interest is the final state)

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: Very Coarse
  • mesh with 32 processors as a starting point. Increase mesh Fineness and Number of processors according to the complexity of the model.

Coarse mesh as a good starting point for the theater analysis

Once the mesh is complete, check its quality with these two steps:

 

  • Open the Meshing log and scroll down to the last few lines – use event log, reach support if there is an error

This is demonstrating that we have a good quality mesh

  • Here no errors were detected. Please contact SimScale support for assistance on solving this issue.

Simulation

Note that if setup tasks are not mentioned below then default values should be sufficient.

Model

Define Gravity based on its direction on your CAD model. Here we have this assigned in the negative y-direction:

Assigning gravity

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. Materials in the product library can also be customized as necessary.

 

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 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.

 

Leaving all other surfaces unassigned will mean that the default no-slip wall condition is applied.

 

Assign the following boundary conditions:

  • Duct inlets: Volumetric flow rate of 0.11 m^3/s
  • Duct outlet: Pressure outlet
  • Building and seating surfaces: 303 K fixed temperature, No-slip velocity condition

Boundaries can be selected in the following way:

Hide the duct walls (right-click, Hide selection), select the rest of the geometry (right-click, select all) and assign the wall conditions to the rest of the walls.

Numerics

The default settings are usually suitable. Experienced users can use 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
  • Create a new Simulation Run
  • There is usually a warning that certain surfaces will be set to wall boundary condition – this means that the unassigned faces will be set to walls and is totally normal.

Results

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:

EDT shown in cut planes to help understand and improve thermal comfort

For thermal comfort studies, it is important to see Effective Draft Temperature (EDT) and Air diffusion performance index (ADPI). The inputs for EDT and ADPI calculation can be found under this link. The images below give the EDT (slice across the section and as threshold) values in the domain. These were created in Paraview.

This is an ISO volume that is displaying Using and ISO volume to show EDT (Effective Draft Temperature)

 

 

Contents

Cookie Policy

SimScale uses cookies to improve your user experience. By using this website you consent to our cookie policy. Don't worry, we are not storing any personal information.

Accept Data Privacy