# ACU-T: 4201 Condensation & Evaporation - Air Box

## Prerequisites

This tutorial provides instructions for running a transient simulation of an enclosed air-box using the humidity model. Prior to starting this tutorial, you should have already run through the introductory tutorial, ACU-T: 1000 Basic Flow Set Up, and have a basic understanding of HyperMesh CFD and AcuSolve. To run this simulation, you will need access to a licensed version of HyperMesh CFD and AcuSolve.

Before you begin, copy the file(s) used in this tutorial to your working directory.

## Problem Description

The problem to be addressed in this tutorial is shown schematically in Figure 1. As an example, an enclosed air-box problem is attached here to show the capability of the humidity modelling (condensation and evaporation) using AcuSolve. The main goal is to demonstrate and quantify accumulation and loss of water vapor on the bottom wall surface due to temperature change in an air domain at 70% relative humidity.
In this particular domain, we assume that air is at a certain level of humidity. Condensation, evaporation, relative humidity, and temperature are all associated with dew point temperature. When the surface temperature drops below the dew point temperature, that is when condensation should start accumulating, and then accumulate up to a point where it reaches 100%. And again on the surface as the temperature rises and attains dew point again, it starts evaporating. This whole definition of both condensation and evaporation is explained in the below attached figure.

From the above plot, we can see that the Air volume initial temperature is set to 297.15 K. The Bottom Wall temperature drops to 285.13 K over 1 sec, maintains 285.13 K for 1 sec, and then rises back to 297.15 K over 1 sec. The dew point temperature of the air at 70% RH is 291.14 K and is reached at 0.5 and 2.5 sec. On the whole we can see that both condensation and evaporation occurs when the dew point temperature is reached, as explained above.

## Start HyperMesh CFD and Open the HyperMesh Database

1. Start HyperMesh CFD from the Windows Start menu by clicking Start > Altair <version> > HyperMesh CFD.
2. From the Home tools, Files tool group, click the Open Model tool.
The Open File dialog opens.
3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T4201_Air_Box.hm and click Open.
4. Click File > Save As.
5. Create a new directory named Air_Box and navigate into this directory.
This will be the working directory and all the files related to the simulation will be stored in this location.
6. Enter Air_Box as the file name for the database, or choose any name of your preference.
7. Click Save to create the database.

## Validate the Geometry

The Validate tool scans through the entire model, performs checks on the surfaces and solids, and flags any defects in the geometry, such as free edges, closed shells, intersections, duplicates, and slivers.

To focus on the physics part of the simulation, this tutorial input file contains geometry which has already been validated. Observe that a blue check mark appears on the top-left corner of the Validate icon on the Geometry ribbon. This indicates that the geometry is valid, and you can go to the flow set up.

## Set Up Flow

### Set Up the Simulation Parameters and Solver Settings

1. From the Flow ribbon, click the Physics tool.
The Setup dialog opens.
2. Under the Physics models setting:
1. Select the Multiphase flow radio button.
2. Set the Multifluid type to Humidity transport.
3. Set the Time step size to 0.1 s and the Final time to 10 s.
4. Set the Turbulence model to Spalart-Allmaras.
5. Set the Gravity to (0,-9.81,0).
6. Set the Pressure scale to Gauge and click . In the microdialog, set the Absolute pressure offset to 101325 Pa then press Esc.
3. Click the Solver controls setting.
4. Set the Minimum stagger iterations to 2 and the Maximum to 4.
5. Close the dialog and save the model.

### Define Flow Boundary Conditions

1. From the Flow ribbon, click the No Slip tool.
2. Select the bottom surface (the surface with the minimum y-coordinate).
3. In the microdialog, click on Temperature tab and set the Thermal boundary condition to Temperature.
4. Set the Temperature to 1, expand the multiplier function drop-down, and select Create new.
5. In the multiplier dialog, set the Type to Piecewise Linear.
6. Set the Variable to Time Step.
7. Click twice to add two rows.
8. Enter the values as shown in the figure below then close the dialog.
9. In the Boundaries legend, double-click on Wall and rename it to Bottom.
10. On the guide bar, click to execute the command and exit the tool.
11. Click the Slip tool.
12. Select the surface with the maximum z-coordinate.
13. In the Boundaries legend, double-click on Slip and rename it to z_pos.
14. On the guide bar, click to execute the command and remain in the tool.
15. Select the surface with the minimum z-coordinate.
16. In the Boundaries legend, double-click on Slip and rename it to z_neg.
17. Click on the guide bar.
18. Save the model.

## Compute the Solution

The input HyperMesh database contains the mesh, hence you do not need to generate the mesh again.

### Define the Nodal Initial Conditions

1. From the Solution ribbon, click the Part tool.
2. Select the box solid.
3. In the dialog, click , select Relative Humidity from the list of variables then click on the white space in the dialog.
4. Set the value to 70.
5. Click on the guide bar.

### Run AcuSolve

1. From the Solution ribbon, click the Run tool.
2. Set the Parallel processing option to Intel MPI.
3. Optional: Set the number of processors to 4 or 8 based on availability.
4. Expand Default initial conditions and enter the values as shown below.
5. Leave the remaining options as default and click Run to launch AcuSolve.
Tip: While AcuSolve is running, right-click on the AcuSolve job in the Run Status dialog and select View Log File to monitor the solution process.
6. Click the Plot tool.
7. In the Plot Utility dialog, double-click on Residual Ratio to plot the residuals.
8. Click to add a new plot.
9. Set the X-Axis to Time.
10. To set the Y-Axis variable, click and then double click on temperature under Surface Output from the list of variables.
11. In the list of surface outputs, select Bottom - Output.
12. Click Create.
13. Similarly, view the plots for Relative Humidity and Dewpoint Temperature.

## Post-Process the Results with HM-CFD Post

In this step, you will create contour plots for temperature, relative humidity, and dew point temperature.

1. Once the solution is completed, navigate to the Post ribbon.
2. From the menu bar, click File > Open > Results.
3. Select the AcuSolve log file in your problem directory to load the results for post-processing.
The solid and all the surfaces are loaded in the Post Browser.
4. In the Post Browser, click on the icon beside Flow Boundaries to turn off the display of all the surfaces.
5. Drag the slider on the Animation toolbar to the 10th frame.
6. Click the Slice Planes tool.
7. Select the x-y plane in the modeling window.
8. In the slice plane microdialog, click to create the slice plane.
9. In the display properties microdialog, set the display to temperature.
10. Click then activate the Legend toggle.
11. Click and set the Colormap Name to Rainbow Uniform.
12. On the guide bar, click to create the temperature contour plot.
13. Hide the temperature contour, then repeat the steps 6-12 to create a similar contour plot for relative humidity.
14. Hide the relative humidity contour, then repeat the steps 6-12 to create a similar contour plot for dew point temperature.

## Summary

In this tutorial, you learned how to set up and solve a multiphase humid air condensation and evaporation simulation using HyperMesh CFD and AcuSolve. You started by importing the HyperMesh CFD input database and then defined the flow setup. Once the solution was computed, you created a plot of residual ratios using the plot utility in HyperMesh CFD. Finally, you created a contour plot of temperature distribution, relative humidity, and dew point temperature using HyperMesh CFD Post.