ACU-T: 4200 Humidity – Pipe Junction

Prerequisites

This tutorial provides the instructions for setting up and running a basic transient humidity transport simulation using a pipe junction 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, 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.

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.


    Figure 2.
    The Open File dialog opens.
  3. Browse to the directory where you saved the model file. Select the HyperMesh file ACU-T4200_Humidity.hm and click Open.
  4. Click File > Save As.
  5. Create a new directory named 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.

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.


Figure 3.

Set Up Flow

Set Up the Simulation Parameters and Solver Settings

  1. From the Flow ribbon, click the Physics tool.


    Figure 4.
    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 1 s and the Final time to 50 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.


    Figure 5.
  3. Click the Solver controls setting.
  4. Set both the Minimum and Maximum stagger iterations to 2.


    Figure 6.
  5. Close the dialog and save the model.

Define Flow Boundary Conditions

  1. From the Flow ribbon, Profiled tool group, click the Profiled Inlet tool.


    Figure 7.
  2. Select the surface highlighted in the figure below.
  3. In the microdialog:
    1. Set the Average velocity to 1 m/sec.
    2. Set the Temperature to 333.15 K.
    3. Set the Humidity input type to Dewpoint Temperature.
    4. Set the Dewpoint temperature to 278.15 K.


    Figure 8.
  4. In the Boundaries legend, double-click on Inlet, change the name to Hot_inlet, then press Enter.
  5. On the guide bar, click to execute the command and remain in the tool.
  6. Select the surface highlighted in the figure below.
  7. In the microdialog:
    1. Set the Average velocity to 3 m/sec.
    2. Set the Temperature to 283.15 K.
    3. Set the Humidity input type to Relative Humidity.
    4. Set the Relative humidity to 20.


    Figure 9.
  8. In the Boundaries legend, double-click on Inlet, change the name to Cold_inlet, then press Enter.
  9. On the guide bar, click to execute the command and exit the tool.
  10. Click the Outlet tool.


    Figure 10.
  11. Select the surface highlighted in the figure below then click on the guide bar.


    Figure 11.
  12. Click the Slip tool.


    Figure 12.
  13. Select the surface highlighted in the figure below (the surface with the minimum y-coordinate).


    Figure 13.
  14. In the Boundaries legend, double-click on Slip, change the name to y_neg, then press Enter.
  15. Click on the guide bar.
  16. Select the surface highlighted in the figure below (the surface with the maximum y-coordinate).


    Figure 14.
  17. In the Boundaries legend, double-click on Slip, change the name to y_pos, then press Enter.
  18. Click on the guide bar.
  19. 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.


    Figure 15.
  2. Select the pipe solid.
  3. In the dialog, click , select Relative Humidity and Temperature from the list of variables, then click on the white space in the dialog.
  4. Set the initial values of Relative Humidity and Temperature to 20 and 333.15 K, respectively


    Figure 16.
  5. Click on the guide bar.

Run AcuSolve

  1. From the Solution ribbon, click the Run tool.


    Figure 17.
  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.
  5. Set the Temperature to 333.15 K and the remaining fields as shown in the figure below.
  6. Click Run to launch AcuSolve.


    Figure 18.
    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.

Post-Process the Results with HM-CFD Post

In this step, you will create contour plots for temperature, relative humidity, mass fraction humidity, and velocity.

  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.


    Figure 19.
  5. Click the Slice Planes tool.


    Figure 20.
  6. Select the x-z plane in the modeling window.


    Figure 21.
  7. In the slice plane microdialog, click to create the slice plane.
  8. In the display properties microdialog, set the display to temperature.
  9. Click then activate the Legend toggle.
  10. Click and set the Colormap Name to Rainbow Uniform.


    Figure 22.
  11. On the guide bar, click to create the temperature contour plot.


    Figure 23.
  12. Hide the temperature contour and repeat the steps 5-11 to create a similar contour plot for relative humidity.


    Figure 24.
  13. Hide the relative humidity contour and repeat the steps 5-11 to create a similar contour plot for mass fraction humidity.


    Figure 25.
  14. Hide the mass fraction humidity contour and repeat the steps 5-11 to create a similar contour plot for velocity.


    Figure 26.

Summary

In this tutorial, you learned how to set up and solve a humidity transport 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 contour plot of temperature distribution, relative humidity, humidity mass fraction, and velocity using HyperMesh CFD Post.