ACU-T: 4200 Humidity – Pipe Junction


Prior to starting this tutorial, you should have already run through the introductory HyperWorks tutorial, ACU-T: 1000 HyperWorks UI Introduction. 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, a pipe junction problem is attached here to show the capability of the Humidity modelling in AcuSolve. In this problem, there are two inlets with different flow, thermal, and humidity conditions. As the flow proceeds downstream of the pipe, two pipes merge into a single pipe to create a single outlet and a distinct profile of temperature and humidity is attained. The geometry is symmetric about the XZ midplane of the pipe, as shown in the figure.

Figure 1.

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 PipeJunction_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 Humidity 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

Set the Analysis Parameters

  1. Go to the Solver Browser, expand 01.Global, then click PROBLEM_DESCRIPTION.
  2. Optional: In the Entity Editor, change the Title to Humidity Modeling.
  3. Set Abs. pressure offset to 101325 N/m2.
  4. Change the Temperature equation to Advective Diffusive.
  5. Set the Turbulence model to Spalart Allmaras.
  6. Switch Humid Air Model to On.
    This will automatically change the Multiphase equation to Advective Diffusive.

    Figure 2.
  7. In the Solver Browser, click 02.SOLVER_SETTINGS under 01.Global.
  8. Set Initial time increment to 1 sec.
  9. Set the Relaxation factor to 0.

    Figure 3.

Set Up Body Force Parameters

In this step, you will define the body force.
  1. In the Solver Browser, expand the 03.Body_Force tree then select BODY_FORCE > Gravity_HM.
  2. Set Gravity in the Y direction to -9.81 m/sec2 and change the Z direction to 0.

    Figure 4.

Set Up Boundary Conditions and Nodal Initial Conditions

Set the Boundary Conditions

By default, all components are assigned to the wall boundary condition. In this step, you will change them to the appropriate boundary conditions and assign material properties to the fluid volumes.
  1. In the Solver Browser, expand 12.Surfaces > WALL.
  2. Click Hot_Inlet. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Set the Inflow type to Average velocity.
    3. Set the Average velocity to 1 m/s.
    4. Set the Temperature to 333.15 K.
    5. Set Incoming Humidity type to Dew Point Temperature and set the value to 278.15 K.

    Figure 5.
  3. Click Cold_Inlet. In the Entity Editor,
    1. Change the Type to INFLOW.
    2. Set the Inflow type to Average velocity.
    3. Set the Average velocity to 3 m/s.
    4. Set the Temperature to 283.15 K.
    5. Set Incoming Humidity type to Relative Humidity and set the value to 20.

    Figure 6.
  4. Click Outlet. In the Entity Editor, change the type to OUTFLOW.

    Figure 7.
  5. Click plusY. In the Entity Editor, change the type to SLIP.

    Figure 8.
  6. Similarly click minusY and change the Type to SLIP.
  7. Click Walls. In the Entity Editor, verify that the Type is set to WALL.

    Figure 9.
  8. Click Fluid. In the Entity Editor,
    1. Change the Type to MULTIPHASE.
    2. Select HumidAir_HM as the Material.
    3. Set Body force to Gravity_HM.

    Figure 10.
  9. Save the model.

Set the Nodal Initial Conditions

  1. Go to the Solver Browser, expand the 01.Global tree then select 03.NODAL_INTIAL_CONDITION > NODAL_INTIAL_CONDITION.
  2. Under the Velocity tab, set X Velocity to 1 m/sec.
  3. Change the Default value of Temperature to 333.15 K.
  4. Change the Default value of Eddy viscosity to 0 m2/sec.
  5. Change the Default value of Relative Humidity to 20.

    Figure 11.

Compute the Solution

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

Run AcuSolve

  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. Leave the remaining options as default and click Launch to start the solution process.

    Figure 12.

Post-Process the Results with HyperView

Once the solution has converged, close the AcuProbe and AcuTail windows. Go to the HyperMesh window and close the AcuSolve Control tab.

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 PipeJunction.1.Log.
  4. Click Open.
  5. Click Apply in the panel area to load the model and results.
    The model is colored by geometry after loading.

Create Contour Plots

In this step, you will create contour plots of temperature, relative humidity, mass fraction humidity and velocity magnitude.
  1. In the Results Browser, expand the list of Components.
  2. Click the Isolate shown icon and then click on the minusY component to turn off the display of all components except the minusY component.

    Figure 13.
  3. Orient the display to the xz-plane by clicking on the Standard Views toolbar.
  4. Click on the Results toolbar to open the Contour panel.
  5. Select Temperature (s) as the Result type.
  6. Click the Components entity selector. In the Extended Entity Selection dialog, select Displayed.
  7. Click Apply.
  8. In the panel area, under the Display tab, turn off the Discrete color option.

    Figure 14.
  9. Click the Legend tab then click Edit Legend. In the dialog, change the Numeric format to Fixed then click OK.
  10. Verify that the contour looks like the figure below.

    Figure 15.
  11. Change the Result type to Relative_humidity (v) then click Apply to view the relative humidity contour on the minus-Y plane.

    Figure 16.
  12. Change the Result type to Mass_fraction-1-Humidity_HM.HumidAir(s) then click Apply.
    Use the range 0.001306 to 0.0406.

    Figure 17.
  13. Change the Result type to Velocity (v) then click Apply.
    Use the range 0 to 3.753.

    Figure 18.


In this tutorial, you worked through a basic workflow to set-up a CFD model, carried out a CFD simulation, and then post-processed the results using HyperWorks products, namely AcuSolve, HyperMesh and HyperView. You started by importing the model in HyperMesh. Then, you defined the simulation parameters and launched AcuSolve directly from within HyperMesh. Upon completion of the solution by AcuSolve, you used HyperView to post-process the results and create contour plots.