Chapter 6: Flow in a Process Injection Mixing Pipe

This tutorial includes:

 

6.1. Tutorial Features

In this tutorial you will learn about:

  • Applying a profile boundary using data stored in a file.

  • Visualizing the velocity on a boundary in CFX-Pre.

  • Using the CFX Expression Language (CEL) to describe temperature-dependent fluid properties in CFX-Pre.

  • Using the k-epsilon turbulence model.

  • Using streamlines in CFD-Post to track flow through the domain.

Component

Feature

Details

CFX-Pre

User Mode

General mode

Analysis Type

Steady State

Fluid Type

General Fluid

Domain Type

Single Domain

Turbulence Model

k-Epsilon

Heat Transfer

Thermal Energy

Boundary Conditions

Boundary Profile Visualization

Inlet (Profile)

Inlet (Subsonic)

Outlet (Subsonic)

Wall: No-Slip

Wall: Adiabatic

CEL (CFX Expression Language)

 

Timestep

Physical Time Scale

CFD-Post

Plots

Default Locators

Outline Plot (Wireframe)

Slice Plane

Streamline

Other

Changing the Color Range

Expression Details View

Legend

Viewing the Mesh

 

6.2. Overview of the Problem to Solve

The goal of this tutorial is to understand the general approach taken when working with an existing mesh. In this tutorial, you will go through the three main steps when solving a problem, which are defining a simulation using General mode in CFX-Pre, obtaining a solution using CFX-Solver Manager and viewing the results in CFD-Post.

The injection mixing pipe, common in the process industry, is composed of two pipes: one with a larger diameter than the other. Analyzing and optimizing the mixing process is often critical for many chemical processes. CFD is useful not only in identifying problem areas (where mixing is poor), but also in testing new designs before they are implemented.

The geometry for this example consists of a circular pipe of diameter 1.0 m with a 90° bend, and a smaller pipe of diameter 0.3 m which joins with the main pipe at an oblique angle. Water at 315.0 K enters in the 0.3 m diameter pipe at a rate of 5.0 m/s while water at 285.0 K enters in the 1.0 m diameter pipe at a rate of 0.5 m/s.

Figure 6.1: Injection Mixing Pipe

Injection Mixing Pipe

In this tutorial, you will establish a general workflow for analyzing the flow of the water fluid into and out of an injection pipe. First, a simulation will be created and an existing mesh will be imported in CFX-Pre. A viscosity expression will also be created, and will be used to modify the water properties later on in this tutorial to increase the solution accuracy. Finally, initial values will be set and a solution will be found using CFX-Solver Manager. The results will then be viewed in CFD-Post. Streamlines originating from the main inlet will be generated to show the flow of the water into and out of the injection pipe.

If this is the first tutorial you are working with, it is important to review the following topics before beginning:

 

6.3. Preparing the Working Directory

  1. Create a working directory.

    Ansys CFX uses a working directory as the default location for loading and saving files for a particular session or project.

  2. Download the inject_mixer.zip file here .

  3. Unzip inject_mixer.zip to your working directory.

    Ensure that the following tutorial input files are in your working directory:

    • InjectMixerMesh.gtm

    • InjectMixer_velocity_profile.csv

  4. Set the working directory and start CFX-Pre.

    For details, see Setting the Working Directory and Starting Ansys CFX in Stand-alone Mode.

 

6.4. Defining the Case Using CFX-Pre

The tutorial follows this general workflow for setting up the case in CFX-Pre:

  1. In CFX-Pre, select File > New Case.

  2. Ensure that General is selected and click OK.

  3. Select File > Save Case As.

  4. Under File name, type InjectMixer.

  5. Click Save.

 

6.4.1. Importing a Mesh

The following steps will demonstrate how to import a mesh.

  1. Right-click Mesh and select Import Mesh > CFX Mesh.

    The Import Mesh dialog box appears.

  2. Configure the following setting(s):

    Setting

    Value

    File name

    InjectMixerMesh.gtm

  3. Click Open.

  4. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Y up) from the shortcut menu.

 

6.4.2. Setting Temperature-Dependent Material Properties

Viscosity varies with temperature, which implies that the water will behave differently when coming through the 1.0 m and the 0.3 m diameter pipes. In the following steps, you will create an expression for viscosity as a function of temperature. This expression will then be used to modify the properties of the library material: Water to increase the accuracy of the solution. By setting temperature-dependent material properties, Viscosity will be made to vary linearly with temperature between the following conditions:

  • =1.8E-03 N s m-2 at T=275.0 K

  • =5.45E-04 N s m-2 at T=325.0 K

The variable T (Temperature) is a CFX System Variable recognized by CFX-Pre, denoting static temperature. All variables, expressions, locators, functions, and constants can be viewed by double-clicking the appropriate entry (such as Additional Variables or Expressions) in the tree view.

All expressions must have consistent units. You should be careful if using temperature in an expression with units other than [K].

The Expressions tab lets you define, modify, evaluate, plot, copy, delete and browse through expressions used within CFX-Pre.

  1. From the main menu, select Insert > Expressions, Functions and Variables > Expression.

  2. In the New Expression dialog box, type Tupper.

  3. Click OK.

    The details view for the Tupper equation is displayed.

  4. Under Definition, type 325 [K].

  5. Click Apply to create the expression.

    The expression is added to the list of existing expressions.

  6. Ensure that no expression is highlighted, then right-click in the Expressions workspace and select Insert > Expression.

  7. In the New Expression dialog box, type Tlower.

  8. Click OK.

  9. Under Definition, type 275 [K].

  10. Click Apply to create the expression.

    The expression is added to the list of existing expressions.

  11. Create expressions for Visupper, Vislower and VisT using the following values.

    Name

    Definition

    Visupper

    5.45E-04 [N s m^-2]

    Vislower

    1.8E-03 [N s m^-2]

    VisT

    Vislower+(Visupper-Vislower)*(T-Tlower)/(Tupper-Tlower)

 

6.4.3. Plotting an Expression

  1. Right-click VisT in the Expressions tree view, and then select Edit.

    The Expressions details view for VisT appears.

    Tip:  Alternatively, double-clicking the expression also opens the Expressions details view.

  2. Click the Plot tab and configure the following setting(s):

    Tab

    Setting

    Value

    Plot

    Number of Points

    10

    T

    (Selected)

    Start of Range

    275 [K]

    End of Range

    325 [K]

  3. Click Plot Expression.

    A plot showing the variation of the expression VisT with the variable T is displayed.

 

6.4.4. Evaluating an Expression

  1. Click the Evaluate tab.

  2. In T, type 300 [K].

    This is between the start and end range defined in the last module.

  3. Click Evaluate Expression.

    A value of around 0.0011[kg m^-1 s^-1] for VisT at the given value of T appears in the Value field.

 

6.4.5. Modify Material Properties

As mentioned earlier in this tutorial, the default material properties of Water will be modified using the Viscosity expression to increase the accuracy of the solution.

  1. Click the Outline tab.

  2. Double-click Water under Materials to display the Basic Settings tab.

  3. Click the Material Properties tab.

  4. Expand Transport Properties.

  5. Select Dynamic Viscosity.

  6. Under Dynamic Viscosity, click in Dynamic Viscosity.

  7. Click Enter Expression  .

  8. Enter the expression VisT into the data box.

  9. Click OK.

 

6.4.6. Creating the Domain

The domain will be set to use the thermal energy heat transfer model, and the (k-epsilon) turbulence model.

Both Basic Settings and Fluid Models are changed in this module. The Initialization tab is for setting domain-specific initial conditions, which are not used in this tutorial. Instead, global initialization is used to set the starting conditions.

  1. Select Insert > Domain from the main menu or click Domain  .

  2. In the Insert Domain dialog box, type InjectMixer.

  3. Click OK.

  4. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Location and Type

    > Location

     

    B1.P3

    Fluid and Particle Definitions

    Fluid 1

    Fluid and Particle Definitions

    > Fluid 1

    > Material

     

     

    Water

    Domain Models

    > Pressure

    > Reference Pressure

     

     

    0 [atm]

  5. Click Fluid Models.

  6. Configure the following setting(s):

    Setting

    Value

    Heat Transfer

    > Option

     

    Thermal Energy

    Turbulence

    > Option

     

    k-Epsilon

  7. Click OK.

 

6.4.7. Creating the Side Inlet Boundary

The side inlet boundary must be defined.

  1. Select Insert > Boundary from the main menu or click Boundary  .

  2. Set Name to side inlet.

    Note:  A boundary named after a region will use that region as its location by default.

  3. Click OK.

  4. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Inlet

    Location

    side inlet

    Boundary Details

    Mass and Momentum

    > Option

     

    Normal Speed

    Mass and Momentum

    > Normal Speed

     

    5 [m s^-1]

    Heat Transfer

    > Option

     

    Static Temperature

    Heat Transfer

    > Static Temperature

     

    315 [K]

  5. Click OK.

 

6.4.8. Creating the Main Inlet Boundary

The main inlet boundary for the large pipe must be defined. This inlet is defined using a velocity profile. Profile data must be initialized before the boundary can be created.

You will create a plot showing the velocity profile data, marked by higher velocities near the center of the inlet, and lower velocities near the inlet walls.

  1. Select Tools > Initialize Profile Data.

    The Initialize Profile Data dialog box appears.

  2. Beside Profile Data File, click Browse  .

    The Select Profile Data File dialog box appears.

  3. From your working directory, select InjectMixer_velocity_profile.csv.

  4. Click Open.

  5. Click OK.

    The profile data is read into memory.

    Note:  After profile data has been initialized from a file, the profile data file should not be deleted or otherwise removed from its directory. By default, the full file path to the profile data file is stored in CFX-Pre, and the profile data file is read directly by CFX-Solver each time the solver is started or restarted.

  6. Select Insert > Boundary from the main menu or click Boundary  .

  7. Set name Name to main inlet.

  8. Click OK.

  9. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Inlet

    Location

    main inlet

    Profile Boundary Conditions

    > Use Profile Data

     

    (Selected)

    Profile Boundary Setup

    > Profile Name

     

    main inlet

  10. Click Generate Values.

    This causes the profile values of U, V, W to be applied at the nodes on the main inlet boundary, and U, V, W entries to be made in Boundary Details. In order to later reset the velocity values at the main inlet to match those that were originally read from the boundary condition profile file, revisit Basic Settings for this boundary and click Generate Values.

  11. Configure the following setting(s):

    Tab

    Setting

    Value

    Boundary Details

    Flow Regime

    > Option

     

    Subsonic

    Mass And Momentum

    > Option

     

    Cart. Vel. Components

    Turbulence

    > Option

     

    Medium (Intensity = 5%)

    Heat Transfer

    > Option

     

    Static Temperature

    Heat Transfer

    > Static Temperature

     

    285 [K]

    Plot Options

    Boundary Contour

    (Selected)

    Boundary Contour

    > Profile Variable

     

    W

  12. Click OK.

  13. Zoom into the main inlet to view the inlet velocity contour.

 

6.4.9. Creating the Main Outlet Boundary

In this module you create the outlet boundary. All other surfaces that have not been explicitly assigned a boundary will remain in the InjectMixer Default object, which is shown in the tree view. This boundary uses a No-Slip Adiabatic Wall by default.

  1. Select Insert > Boundary from the main menu or click Boundary  .

  2. Set Name to outlet.

  3. Click OK.

  4. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Boundary Type

    Outlet

    Location

    outlet

    Boundary Details

    Flow Regime

    > Option

     

    Subsonic

    Mass and Momentum

    > Option

     

    Average Static Pressure

    Relative Pressure

    0 [Pa]

  5. Click OK.

 

6.4.10. Setting Initial Values

For this tutorial, the initial values will be set automatically. An automatic guess is sufficient for this particular problem.

  1. Click Global Initialization   and review, but do not change, the current settings.

  2. Click Close.

 

6.4.11. Setting Solver Control

  1. Click Solver Control  .

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Advection Scheme

    > Option

     

    High Resolution

    Convergence Control

    > Max. Iterations

     

    50

    Convergence Control

    > Fluid Timescale Control

    > Timescale Control

     

     

    Physical Timescale

    Convergence Control

    > Fluid Timescale Control

    > Physical Timescale

     

     

    2 [s] [ a ]

    Convergence Criteria

    > Residual Type

     

    RMS

    Convergence Criteria

    > Residual Target

     

    1.E-4 [ b ]

    1. The physical timescale that will be set up is derived from the pipe diameter (1 m) and the rate at which the water flows in the pipe (0.5 m/s).

    2. An RMS value of at least 1.E-5 is usually required for adequate convergence, but the default value is sufficient for demonstration purposes.

  3. Click OK.

 

6.4.12. Writing the CFX-Solver Input (.def) File

Once the problem has been defined you move from General mode into CFX-Solver.

  1. Click Define Run  .

  2. Configure the following setting(s):

    Setting

    Value

    File name

    InjectMixer.def

  3. Click Save.

    The CFX-Solver input file (InjectMixer.def) is created. CFX-Solver Manager automatically starts and, on the Define Run dialog box, Solver Input File is set.

  4. When you are finished, select File > Quit in CFX-Pre.

  5. Click Save & Quit if prompted, to save InjectMixer.cfx

 

6.5. Obtaining the Solution Using CFX-Solver Manager

You will now generate a solution for the CFD simulation that you just prepared.

 

6.5.1. Starting the Run

At this point, CFX-Solver Manager is running, and the Define Run dialog box is displayed, with the CFX-Solver input file set.

  1. Click Start Run.

  2. When the run ends, ensure that the check box next to Post-Process Results is cleared and click OK to close the dialog box.

 

6.5.2. Moving from CFX-Solver Manager to CFD-Post

  1. Select Tools > Post-Process Results or click Post-Process Results  .

  2. If using CFX-Solver Manager in stand-alone mode, optionally select Shut down CFX-Solver Manager.

  3. Click OK.

 

6.6. Viewing the Results Using CFD-Post

When CFD-Post starts, the viewer and Outline workspace display by default.

The tutorial follows this general workflow for viewing results in CFD-Post:

 

6.6.1. Modifying the Outline of the Geometry

Throughout this and the following examples, use your mouse and the Viewing Tools toolbar to manipulate the geometry as required at any time.

  1. In the tree view, double-click Wireframe.

  2. Set the Edge Angle to 15 [degree].

  3. Click Apply.

 

6.6.2. Creating and Modifying Streamlines Originating from the Main Inlet

When you complete this module you will see streamlines (mainly blue and green) starting at the main inlet of the geometry and proceeding to the outlet. Above where the side pipe meets the main pipe, there is an area where the flow re-circulates rather than flowing roughly tangent to the direction of the pipe walls.

  1. Select Insert > Streamline from the main menu or click Streamline  .

  2. Under Name, type MainStream.

  3. Click OK.

  4. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Type

    3D Streamline

    Definition

    > Start From

     

    main inlet

  5. Click Apply.

  6. Right-click a blank area in the viewer, select Predefined Camera from the shortcut menu, then select Isometric View (Y up).

    The pipe is displayed with the main inlet in the bottom right of the viewer.

 

6.6.3. Modifying Streamline Color Ranges

You can change the appearance of the streamlines using the Range setting on the Color tab.

  1. Under User Locations and Plots, modify the streamline object MainStream by applying the following settings

    Tab

    Setting

    Value

    Color

    Range

    Local

  2. Click Apply.

    The color map is fitted to the range of velocities found along the streamlines. The streamlines therefore collectively contain every color in the color map.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Color

    Range

    User Specified

    Min

    0.2 [m s^-1]

    Max

    2.2 [m s^-1]

    Note:  Portions of streamlines that have values outside the range shown in the legend are colored according to the color at the nearest end of the legend. When using tubes or symbols (which contain faces), more accurate colors are obtained with lighting turned off.

  4. Click Apply.

    The streamlines are colored using the specified range of velocity values.

 

6.6.4. Coloring Streamlines with a Constant Color

  1. Configure the following setting(s):

    Tab

    Setting

    Value

    Color

    Mode

    Constant

    Color

    (Green)

    Color can be set to green by selecting it from the color pallet, or by repeatedly clicking on the color box until it cycles through to the default green color.

  2. Click Apply.

 

6.6.5. Creating Streamlines Originating from the Side Inlet

The following steps illustrate using this feature to add a streamline object that originates at the side inlet.

  1. Right-click MainStream and select Duplicate from the shortcut menu.

  2. In the Name window, type SideStream.

  3. Click OK.

  4. Double-click the newly created streamline, SideStream.

  5. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Definition

    > Start From

     

    side inlet

    Color

    Mode

    Constant

    Color

    (Red)

  6. Click Apply.

    Red streamlines appear, starting from the side inlet.

  7. For better view, select Isometric View (Y up).

 

6.6.6. Examining Turbulence Kinetic Energy

Away from walls, turbulence kinetic energy has an influence on the level of mixing. A plane will be created to view the Turbulence Kinetic Energy variable within the domain.

Note:  This module has multiple changes compiled into single steps in preparation for other tutorials that provide fewer specific instructions.

  1. Turn off the visibility of both the MainStream and the SideStream objects.

  2. Create a plane named Plane 1 that is normal to X and passing through the X = 0 Point. To do so, specific instructions follow.

    1. From the main menu, select Insert > Location > Plane and click OK.

    2. In the details view, set Definition > Method to YZ Plane and X to 0 [m].

    3. Click Apply.

  3. Color the plane using the variable Turbulence Kinetic Energy, to show regions of high turbulence. To do so, apply the settings below.

    Tab

    Setting

    Value

    Color

    Mode

    Variable

    Variable

    Turbulence Kinetic Energy

  4. Click Apply.

  5. Experiment with other variables to color this plane (for example, Temperature to show the temperature mixing of the two streams).

    Commonly used variables are in the drop-down menu. A full list of available variables can be viewed by clicking   next to the Variable data box.

 

6.6.7. Quitting CFD-Post

  1. When you are finished, select File > Quit to exit CFD-Post.

  2. If prompted by a dialog box, save the state at your discretion.