# Session 1: Air-conditioning simulation of an office space

**URL:** <https://www.simscale.com/forum/t/session-1-air-conditioning-simulation-of-an-office-space/87678>\
**Category:** Air Conditioning and Ventilation Workshop\
**Created:** [February 13, 2020, 12:14am UTC](https://www.simscale.com/forum/t/session-1-air-conditioning-simulation-of-an-office-space/87678 "2020-02-13T00:14:21Z")\
**Posts on this page:** 2\
**Page:** 1

<div class="post-metadata">

**Author:** ![Ricardopg](https://www.simscale.com/forum/user_avatar/www.simscale.com/ricardopg/32/26909_2.png) [@Ricardopg](https://www.simscale.com/forum/u/Ricardopg)\
**Post date:** [February 13, 2020, 12:14am UTC](https://www.simscale.com/forum/t/session-1-air-conditioning-simulation-of-an-office-space/87678/1 "2020-02-13T00:14:22Z")

</div>

## Air Conditioning and Ventilation Webinar

[Air Conditioning and Ventilation Workshop (Session 1) ― CFD for Data Center Cooling](https://www.youtube.com/watch?v=iT1CTS5YMrQ)

### Air-conditioning simulation of an office space

Import the project by clicking the link below.

**Project Link:** [SimScale Login](https://www.simscale.com/workbench?publiclink=e7a054af-0fa6-41a8-97e2-61c9f486677f)

**Once the project is imported, the workbench is automatically opened. Then follow the steps below for setting up a convective heat transfer simulation**.

## Step-by-Step

The first step is to create a simulation. Click on the geometry named **office** and then on **Create Simulation**.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/c/6cc436bdfb1f27d20af78d391a8f539fb5e2a90b.png)

For the analysis type, select **Convective heat transfer**. Then click on the **Create Simulation** button.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/b/8b88f99b2ca3bffecd4148d02d3bcf859dc44f1c.png)

The simulation tree can be seen in the panel to the left-hand side of your screen. Red entries in the tree have to be filled out in order to run simulations.  
In the simulation tree, select the newly created **Convective heat transfer** simulation and adjust the configuration as shown:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/c/8/c8c7d12fdd3f7e5ace8fd00101b691a74bb0de14.png)

The Boussinesq approximation can be disabled or enabled by the **Compressible** on/off switch. Note that when **Compressible** is **ON** , the Boussinesq approximation is not used.

### Meshing

Navigate to **Mesh** in the simulation tree. Select the **Algorithm** type to be **Hex-dominant (only CFD)** and also change **Fineness** to **Moderate**. A boundary layer refinement will be set up in the next step, so please disable **Automatic boundary layers**.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/4/a481128768a781b080016d0d02f8e6cd2ad57a87.png)

To create a mesh refinement, click on the **+** icon next to **Refinements** and select the desired type of refinement.  
Layer addition is important to capture the flow phenomenon near the boundaries. Hence layers should be added to all the surfaces except the inlet and outlet. This can be done by selecting all surfaces and then unselecting the inlet and outlet boundaries, as shown in the following 2 images.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/9/d9747aed8a833f0bd4c419a147319916c1402f9f.png)

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/8/084cd062646bc97a935fb5033e8170c61493eaa3.png)

Make sure to check if 445 faces have been assigned. In case of doubt, notice that unselected faces are grey and assigned faces are blue.

Now, in the simulation tree, head back to **Mesh** and click on the **Generate** button. You don’t have to worry with the number of processors that will be employed for this task, as SimScale automatically chooses the most appropriate number depending on the job size.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/9/09ed4a9e5d6c3e99dde942a54b42b43b319f51b5.png)

This mesh operation takes around 50 minutes to finish. It is possible to continue working on the set up while the mesh is being generated.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/d/bd76c36ea7eed0a3dc7dbbde96de261886bc6a44.png)

In the simulation tree, click on **Model** and enter **-9.81** in the **z** direction:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/e/d/ed96d64a880faeffb417344d9510897f383e31d6.png)

Now please select **Materials**. Choose **Air** and hit **Apply**.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/4/c/4c7798ed3539db7deedbb3437af82ab70617e1ce.png)

Air is automatically assigned to the flow region **1**. Therefore, please click on the blue mark to save.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/6/66fe509dd811d0d167003dfbc41dff7b8638812a.png)

Let’s now create **Topological Entity Sets** which will help us to set boundary conditions later on. To create a new topological entity set:

- Select the face or faces that will constitute the new set;
- Click on the **+** icon next to **Topological Entity Sets** in the right-hand side of your screen;
- Name the topological entity set appropriately.

Creating a topological entity set for the **Inlet** :

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/4/1/41b4a134892cddcc7370f8a22a67cf113e0d75aa.png)

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/6/c/6c0d7f6d618c30e489c76dee5986f19c607edead.png)

Similarly for the **Outlet** :

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/e/8e2001bee1cc913021a611c77555693623b234cf.png)

To create a **Walls** entity set, right click in the viewer and **Select all** faces, then unselect inlet and outlet:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/a/da598770f849c9829e91f1fc979e0d828b85dd4d.png)

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/f/c/fc690de9435c4db805778a666fc7febca6264384.png)

Under **Initial conditions** from the tree, select **(U) Velocity** and enter a **Uy** value of **-0.1** m/s . Then **Save** these settings

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/f/9/f99713093e4a2a14caeb5872f2d903f5c95d4d7c.png)

Heading over to **Boundary conditions** now, we will set up boundary conditions for the previously created topological entity sets. To create a new boundary condition, click on the **+** icon and select the appropriate type.

The **Inlet** boundary condition will be a **Velocity inlet** of **-0.75** m/s in the **y** direction, with **10** Celsius temperature. Assign it to the **Inlet** entity set:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/f/d/fd1b4bf72471f27d3e597fcac9efc875d57dd5e8.png)

The **Outlet** is going to be a **Pressure outlet** condition:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/4/8/48710aa26d4668fa46ff449b49a2e0b5d053c3a5.png)

Finally, for the **Walls** entity set, select a **Wall** boundary condition with a fixed value of **20** Celsius assigned for the temperature.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/5/4/54436285f30c8a317f72867ff69941ef14e1e34f.png)

Under **Numerics** , change the **Relaxation type** to **Manual** :

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/4/a/4a774d3fff4667c3d08c839de8bbe0c90635bd4a.png)

In **Simulation control**. Please change **Maximum runtime** to **20000** seconds.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/0/d09455f69b067cc32947bd2fd86e9a69a4b3e1d4.png)

In order to allow us to better assess convergence, let’s set up an **Area average**  **Result control** on the outlet surface:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/e/8ec28b9735f3079e59170c9dcefd5e39a5f00a33.png)

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/3/a34ccb1d1b2ca777e06b3895ba31a156bcdcb540.png)

That’s it, now head over to **Simulation Runs** and hit **Start**.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/8/a/8a7b0e5b48e0b50fbabd8006efc8a93daaa5d40a.png)

### Post-processing

This simulation takes about 75 minutes to finish running. When it’s over, click on **Solution Fields** to go to the post-processing environment.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/4/2/42f204b60a5f2bb49c40eba414083f78f739503d.png)

Multiple filters can be found in a panel towards the left-hand side of the screen. Click on **Particle Traces** to generate streamlines. In **SETTINGS** , change **Compute vector** to **Velocity [node]** and **Map scalar** to **Temperature [node]**. Also change the streamlines’ **Radius** to 0.0025:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/9/c/9c7b96be980756e5db6c565de05df4094cbb6244.png)

Now, in **SEEDS** , adjust the number of cells in **u** and **v** to **10** and **5** , respectively. **Spacing** between the lines was set to 0.03. The surfaces representation was changed to **Transparent surfaces** to give it a nice effect. By clicking on **PICK** and then selecting a face of interest (usually inlet or outlet), the streamlines will be generated.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/a/3/a3dbde43ad8a387dc1aab7964e91c9c94a53c374.png)

Now please delete the stream lines by right clicking on **Particle Trace 1** and selecting **Delete**. We will proceed to creating some cutting planes on our geometry.  
To add a cutting plane, click on the **+** icon next to **Cutting Planes**. The first one will be normal to the **Z** direction. Adjust the sliding bar next to **Point** to level it with the inlet:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/c/0/c057a2a24e1e98b6bdf934420cc3c5cc2dd1ed9d.png)

Now scroll down the cutting plane settings and locate **Clip model**. It is enabled by default. Please disable it. Now the slice is still visible but it’s not clipping our model anymore:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/3/0/300136124213c8b9ae4bce24d59f355f54f8a026.png)

Now add another cutting plane and follow the same steps, but this time place it on the outlet level:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/0/0/00830d296cc8f1e6b954abb1974487e1cfcab706.png)

Make yet another cutting plane, this time normal to the **X** direction and place it so that it shows the outlet:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/b/5/b5d8b03ab9bb8e4cf137d5ca79bbf5bb779b3337.png)

Now please go back to **Cutting Plane 1** and select **Velocity [node]** to the **Vector** field. Velocity vectors will be plotted on the slice. Bigger vectors indicate higher velocities.

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/c/e/cef3b475a9bfcce48fb0be1059cfca4a0377f0ea.png)

Repeat the process for the other 2 cutting planes:

 ![image](https://www.simscale.com/forum/uploads/default/original/3X/d/f/df1b9a9a1db301193bf05bd419213e05d7ee8392.png)

---

<div class="post-metadata">

**Author:** ![jousefm](https://www.simscale.com/forum/user_avatar/www.simscale.com/jousefm/32/34908_2.png) [@jousefm](https://www.simscale.com/forum/u/jousefm)\
**Post date:** [March 20, 2020, 7:01pm UTC](https://www.simscale.com/forum/t/session-1-air-conditioning-simulation-of-an-office-space/87678/2 "2020-03-20T19:01:45Z")

</div>

Listed on March 20, 2020, 7:01pm UTC


