Clean Room Ventilation - CFD Simulation CFD Software Tutorial

This tutorial guides you through the process of simulating a clean room ventilation system using SimFlow CFD software. To follow this tutorial, you may download SimFlow free version.

Clean Room
Clean rooms are specialized environments designed to maintain extremely low levels of contaminants such as dust, microorganisms, airborne particles, or water vapor. By precisely controlling air quality, temperature, and humidity, these rooms provide the sterile and stable conditions required for sensitive research, manufacturing, and testing processes. To achieve this level of cleanliness, clean rooms rely on advanced ventilation and filtration systems that continuously supply purified air and remove impurities.

In this tutorial, you will learn how to:

By the end of this tutorial, you will have a solid understanding of how to simulate and assess the performance of a clean room ventilation system, including the calculation of air residence time and analysis of flow behavior.

Open SimFlow and create a new case named clean room

Firstly, we need to download and import the following geometries:

Download GeometriesEquipmentFiltersFloorInletOutlet

If the imported geometry is in STL format, be aware that STL files do not include unit information. Therefore, you must manually specify the correct unit after import. If you’re unsure of the original unit used during export, you can estimate it by checking the Geometry size displayed in the interface.

In this case, since the fan geometry is correctly defined in meters, no rescaling is required.

After importing the geometry, it will appear in the 3D window. The geometry components include:

The walls of the cleanroom are not included, as they will be defined by the base mesh in later steps.

To create the mesh, we need to specify the meshing options for the given geometries.

For the equipment inside the room, we will refine the mesh.

For the filters, we will also refine the mesh. Since the filters are modeled as a porous medium, we need to create a dedicated cell zone for them. This will allow us to apply the porous media model and accurately represent the flow resistance introduced by the filter.

In this simulation, we want to model a suspended floor on which equipment is placed, with open space below for air to be discharged. Since a floor is permeable but includes filters and ventilation grilles resist airflow, we will again use a porous medium. In this case, the floor thickness is very small, so we can model it as a 2D surface. The porosity will be defined later using the Porous Baffle boundary condition.

To model the floor by the surface inside the domain (immersed boundary), make sure to enable the Create Baffle option. A baffle is a thin internal surface that separates regions without adding physical thickness. It is commonly used for internal walls, fans, or porous surfaces. By duplicating the original surface, the baffle creates two coincident faces, allowing different boundary conditions to be applied on each side (immersed boundary approach).

For the inlet and outlet, apply mesh refinement near its surface to level 1, ensuring accurate resolution of airflow entering and leaving the cleanroom.

Repeat the same setup for the outlet.

To define the cleanroom boundaries, we will use the Box base mesh type. It matches the rectangular shape of the room.

The material point indicates which side of the geometry the mesh will be retained on. Since we are simulating airflow inside the clean room, the material point must be placed within the base mesh and outside the equipment.

In this step, we will initiate the meshing process.

In the meshing panel, you can indicate how many CPUs you would like to use for this process. Note that if you are using the free version of SimFlow, you may only use serial meshing and cannot create meshes larger than 200,000 nodes.

To meet this limit, we need to reduce the cell count by decreasing the number of cells between refinement levels.

If you would like to test full version Request 30-day Trial

After the meshing process is complete, the mesh will appear on the screen.
To preview the mesh resolution and internal boundaries of the cleanroom, we can hide the external boundary faces while keeping the edges and remaining internal boundaries visible.

In the mesh setup, we enabled baffle creation for the floor, which splits the mesh along the surface Now, we will create a Cyclic Interface to connect both sides of the internal boundary, allowing airflow through the floor.

Review the boundary list and assign appropriate types to each boundary. Wall type prevents fluid from crossing, while Patch type allows fluid to pass through, making it suitable for inlets and outlets.

Cleanroom simulations can be performed as transient analyses, capturing the full flow history. However, such calculations are typically very time-consuming. In this tutorial, we will show an alternative approach to measure air residence time using a steady-state simulation with a passive scalar model.
For this purpose, we will use the SIMPLE (simpleFoam) solver.

We are going to use the standard \(k{-}\omega \; SST\) model to resolve turbulence.

As a fluid material, we will use air.

Selecting material from the Material Database will fill all inputs in the Transport Properties panel. We are still able to overwrite these values at any time.

In a steady-state cleanroom simulation, the flow field is assumed to be constant over time, making direct tracking of fluid impossible. To estimate residence time, the duration that fluid particles spend within the domain, a passive scalar model can be used as an indirect indicator.

A passive scalar is a variable that is transported by the flow but does not influence it (for example, dye concentration or fluid age). In this approach, the scalar is defined to increase linearly along the flow path, effectively representing how long the fluid has remained in the domain.

Method approach:

This approach transforms the steady-state solution into a virtual time-tracking system by using a passive scalar that accumulates continuously throughout the flow field. It provides an efficient alternative to transient simulations, enabling estimation of fluid residence time without the computational cost of time-dependent calculations.

Now, we will create a passive scalar representing Residence Time and assign it a negligible diffusivity.

In the Cell Zone panel, we will define the source term for the Residence Time field. In each cell, the fluid residence time will increase at a constant rate of 1 per second.
Additionally, we will add an implicit source to limit the maximum value of the residence time to 1e8 s. Beyond this threshold, the residence time will no longer increase, effectively acting as an upper limit.

Now, we will apply porosity to the previously created cell zone to model the HEPA filters located after the inlet.

We will now specify the model’s boundary conditions.
To model the permeable floor, we will apply Porous Baffle boundary conditions to the floor interface.

To model the ventilation inlet, we will set the constant velocity using Velocity Inlet preset.

We will also update the turbulent mixing length at the inlet.

During the calculation, we can track fluid parameters or observe intermediate results using section planes or probe plots. Note that runtime post-processing must be defined before starting the calculations and cannot be modified afterward.

Firstly, we will define volume monitor to track maximum and average residence time in the clean room.

Now, we will create two slices to preview the field map across the domain.

Create the second slice.

Now, we need to specify the variables to be sampled.

Finally, we can start our computation.

To speed up the calculation process, take advantage of parallel computing and increase the number of CPUs based on your PC’s capability. The free version allows you to use only one processor (serial mode). To get the full version, you can use the contact form to Request 30-day Trial

Estimated computation time for serial mode: 10 minutes

When the calculation is finished, we should see a similar residual plot. All the residual values have reached \(10^{-4}\) and the solver has automatically stopped the calculation. The residuals are the measure of how results change between iteration. Reaching a very low value indicates that we have found a steady-state solution and results do not change regardless of further computations.

During the simulation, the Slices tab appears next to the Residuals. Under this tab, you can preview live results on the defined section planes.

Now, we can monitor the average and maximum residence time within the entire cleanroom domain during the iterations. As the calculations converge, the maximum residence time stabilizes at approximately 55 s.

Once the computations have been completed, we can preview the stagnation region in the clean room using ParaView.

Load the results into the program.

To identify regions where the air residence time exceeds a critical value, we will use the Clip filter. This filter allows us to threshold the part of the volume where a selected field variable falls outside a specified range. In this case, we will set the threshold to 45 seconds to highlight areas with higher residence time.

The area can be identified as shown in the image below.

To identify the flow pattern in the region where higher residence time persists, we will visualize simplified streamlines. For this purpose, we will create a slice crossing the area of interest and display it using Surface LIC.

Surface LIC is a visualization technique that maps the flow direction and pattern directly onto a surface using texture shading. It helps reveal the flow structure without generating separate streamline objects.

The results are shown in the image below. Areas with higher residence time are caused by flow recirculation and vortices near the inlet.

This concludes the tutorial, covering all the aspects we intended to showcase. For a finely tuned presentation of the results, you may take advantage of the more advanced features.

In ParaView, you can display streamlines, contour plots, vector fields, line or time plots, calculating volume or surface integrals and create animations.

To familiarize yourself with the ParaView capabilities, it’s worth checking out our video tutorial, Paraview CFD Tutorial - Advanced Postprocessing in ParaView, in which we demonstrate some of the most commonly used post-processing techniques.

Paraview CFD Tutorial - Advanced Postprocessing in ParaView