ACU-T: 4201 Condensation & Evaporation - Air Box


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 HyperWorks UI Introduction, and have a basic understanding of AcuSolve. To run this simulation, you will need access to a licensed version of HyperMesh and AcuSolve.

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

Since the HyperMesh database (.hm file) contains meshed geometry, this tutorial does not include steps related to geometry import and mesh generation.

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.

Figure 1.
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.

Figure 2.

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.

Open the HyperMesh Model Database

  1. Start HyperMesh and load the AcuSolve user profile.
    Refer to the HM introductory tutorial, ACU-T: 1000 HyperWorks UI Introduction, to learn how to select AcuSolve from User Profiles.
  2. Click the Open Model icon located on the standard toolbar.
    The Open Model dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file and click Open.
  4. Click File > Save As.
    The Save Model As dialog opens.
  5. Create a new directory named Air_Box_Humidity 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.

Set the General Simulation Parameters

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. In the Entity Editor, enter Air Box as the Title.
  3. Set the Analysis type to Transient.
  4. Set Abs. pressure offset to 101325.
  5. Change the Temperature equation to Advective Diffusive.
  6. Set the Turbulence Model to Spalart Allmaras.
  7. Switch the Humid Air Model to On.
    The will automatically change the multiphase equation to Advective Diffusive.
  8. Set the Global Gravity parameters as shown below.

    Figure 3.
  9. In the Solver Browser, click 02.SOLVER_SETTINGS under 01.Global.
  10. In the Entity Editor, set Max time steps to 100.
  11. Set the Initial time increment to 0.1 and change other parameters as shown in the figure below.

    Figure 4.

Set Up Nodal Initial Conditions

In this step, you will define the Nodal Initial Condition (NICs) for the problem for both Temperature and Relative Humidity.
  1. In the Solver Browser, click 03.NODAL_INTIAL_CONDITION under 01.Global.
  2. Change the Default value of Temperature to 297.15 K.
  3. Change the Default value of Eddy viscosity to 0.0001 m2/sec.
  4. Change the Default value of Relative Humidity to 70.

    Figure 5.

Set Up Material Model Parameters and Body Force

In this step, you will define the material properties for the problem and assign body force to the fluid volume.

Set Material Model Parameters

  1. In the Solver Browser, expand 02.Materials > FLUID then click Air_HM.
  2. In the Entity Editor, set the Material Type to FLUID if not already set.
  3. Set the Density type to Boussinesq.
  4. Enter the values for Density as shown in the figure below and leave the remaining material parameters unchanged.

    Figure 6.
  5. In the Solver Browser, expand MULTIPHASE under Materials then click HumidAir_HM.
  6. Verify that the Material type is set to MULTIPHASE and the Filed Interaction Type is set to Advective Diffusive.

    Figure 7.

Set Up Body Force

  1. In the Solver Browser, expand 03.Body_Force > BODY_FORCE then click Gravity_HM.
  2. Set Gravity in the Z direction to -9.81.

    Figure 8.

Create a Multiplier Function

  1. In the Solver Browser, right-click on 05.Multiplier_Function and select Create.
    A new function named MULTIPLIER_FUNCTION.1 is created.
  2. Rename the function as Temp_MF.
  3. In the Entity Editor, chance the Multiplier Function Type to Piecewise Linear.
  4. Right-click on the Curves field and select Create.
  5. In the embedded Entity Editor, change the name to curve_Temp_MF.

    Figure 9.
  6. Again, right-click on the Curves field and select Plot Curves.
    A Curve editor window opens.
  7. Enter the data as shown in the figure below then click Update in the bottom-left of the window.

    Figure 10.
  8. Click Close to close the window.

Set Up Boundary Conditions

  1. Go to the Model Browser and expand the list of Components.
  2. Click Fluid. In the Entity Editor,
    1. Set the Type to MULTIPHASE.
    2. Set the Material to HumidAir_HM.
    3. Under Element Output, set Active Element Output to On and verify that the other parameters are as shown below.

    Figure 11.
  3. Click front. In the Entity Editor, change the Type to SLIP.

    Figure 12.
  4. Similarly, click back and change the Type to SLIP.
  5. Click left. In the Entity Editor,
    1. Change the Type to WALL.
    2. Change the Temperature BC type to Flux.

    Figure 13.
  6. Similarly, click right and top, change their types to WALL, and set the Temperature BC type to Flux.
  7. Click bottom. In the Entity Editor,
    1. Change the Type to WALL.
    2. Set Show advanced features to On.
    3. Change the Temperature BC type to Value.
    4. Set the Temperature value to 1.
    5. Set the Temperature multiplier function to Temp_MF.
    6. Under Surface Output, ensure that Activate Surface Output is On.
      Note: Turning this options on allows you to calculate the surface integral output of a particular surface using post-processing programs like AcuProbe and AcuTrans.

    Figure 14.
  8. Save the model.

Set Up Nodal Output Variables

  1. In the Solver Browser, expand 17.Output then click NODAL_OUTPUT.
  2. In the Entity Editor, set the Time step frequency to 5.
  3. Check the box for Output initial condition.

    Figure 15.

Compute the Solution

In this step, you will launch AcuSolve directly from HyperMesh and compute the solution.

  1. Turn on the visibility of all mesh components.
    For the analysis to run, the mesh for all active components must be visible.
  2. Click on the ACU toolbar.
    The Solver job Launcher dialog opens.
  3. Optional: For a faster solution time, set the number of processors to a higher number (4 or 8) based on availability.
  4. Verify that the Output time steps is set to All.
  5. Leave the remaining options as default and click Launch to start the solution process.

    Figure 16.

Monitor the Solution with HyperGraph

HyperGraph can be used to monitor various variables over solution time.
  1. Click the client selector in the bottom-left corner of the graphics area then select HyperGraph 2D.

    Figure 17.
  2. Once the HyperGraph interface loads, click in the panel area and select the result file from the current working directory.
    In this example, the file to be selected is Air_Box.1.Log.
  3. Make sure that the X Type is set to Time.
  4. Set the Y Type to Temperature (surface) and the Y Request to bottom.
  5. Select temperature under Y Component.

    Figure 18.
  6. Click Apply.

    Figure 19.
  7. Similarly, plot other variables like Relative_humidity and Dewpoint_temperature on the same surface group – bottom.

    Figure 20.

    Figure 21.

Post-Process the Results with HyperView

Open HyperView and Load the Model and Results

  1. In the HyperMesh main menu area, click Applications > HyperView.
    Once the HyperView window is loaded, the Load model and results panel should be open by default. If you do not see the panel, click File > Open > Model.
  2. In the Load model and results panel, click next to Load model.
  3. In the Load Model File dialog, navigate to your working directory and select the AcuSolve .Log file for the solution run that you want to post-process. In this example, the file to be selected is Air_Box.1.Log.
  4. Click Open.
  5. In the panel area, click Reader Options.
  6. In the dialog, set the Reader to AcuSolve Result Reader and Extended nodal output to No.

    Figure 22.
  7. Click Apply then close the dialog.
  8. Click Apply in the panel area to load the model and results.
    The model is colored by geometry after loading.

Create Contours on a Cut Plane

In this step, you will create temperature, relative humidity, and dew point temperature contours on a cut plane.
  1. Since this is a transient case, you need to plot the results at the last timestep. To do this, click the Time drop-down menu in the Results Browser and select the last option in the list.

    Figure 23.

    Here we have the last time as 10 sec.

  2. To create a new cut plane, right-click in the Results Browser and select Create > Section Cut > Planar from the context menu.
    A new entity, Section 1, is created under the Section Cuts heading.
  3. Right-click on Section 1 and select Edit from the context menu.
  4. In the Section cut panel, change Define plane to the Z Axis.
  5. Under Display options, activate the Cross section option.
  6. Verify that the Clip elements option is active.
  7. Click Apply.
  8. Move the Define plane slider bar (located under the Z Axis button) to choose a desired position for the section cut plane.

    Figure 24.

    Figure 25.
  9. Orient the display to the xy-plane by clicking on the Standard Views toolbar.
  10. Click on the Results toolbar to open the Contour panel.
  11. In the panel area, set the Result type to Temperature (s).
  12. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
  13. Click Apply.
  14. Under the Display tab, turn off the Discrete color option.

    Figure 26.

    Figure 27.
  15. Change the Result type to Relative_humidity (s) to view the relative humidity contour of the XY plane.

    Figure 28.
  16. Change the Result type to Dew_Point_Temperature (s) to view the dew point temperature contour of the XY plane.

    Figure 29.
  17. Save the plots as an image file.
    1. On the Image Capture toolbar, toggle the Save Image File/Clipboard icon (/) so that it shows .
    2. Click the Capture Graphics Area icon .
    3. Provide a name for the image in the dialog then click Save.
      Note: If you wish to use the images in a presentation, you can copy them to the clipboard by toggling the Save Image to File/Clipboard icon to instead of . Then, paste the image in your presentation.


In this tutorial, you worked through a basic workflow to set up and solve a transient multiphase flow problem using HyperMesh and AcuSolve. You also learned how to use the humidity model to quantify accumulation and loss of water vapor on the bottom wall surface due to temperature change. Once the solution was computed, you monitored the solution in HyperGraph and post-processed the results in HyperView, where you created contour plots.