Chapter 4: Flow in a Static Mixer (Refined Mesh)

This tutorial includes:

Important:  This tutorial requires files StaticMixer.def and StaticMixer_001.res, which are produced by following tutorial Simulating Flow in a Static Mixer Using CFX in Stand-alone Mode.

 

4.1. Tutorial Features

In this tutorial you will learn about:

  • Using the General mode of CFX-Pre (this mode is used for more complex cases).

  • Rerunning a problem with a refined mesh.

  • Importing a CCL (CFX Command Language) file to copy the definition of a different simulation into the current simulation.

  • Viewing the mesh with a Sphere Volume locator and a Surface Plot.

  • Using the Report Viewer to analyze mesh quality.

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

Inlet (Subsonic)

Outlet (Subsonic)

Wall: No-Slip

Wall: Adiabatic

Timestep

Physical Time Scale

CFD-Post

Plots

Slice Plane

Sphere Volume

Other

Viewing the Mesh

 

4.2. Overview of the Problem to Solve

In this tutorial, you use a refined mesh to obtain a better solution to the Static Mixer problem created in Simulating Flow in a Static Mixer Using CFX in Stand-alone Mode. You establish a general workflow for analyzing the flow of fluid into and out of a mixer. This tutorial uses a specific problem to teach the general approach taken when working with an existing mesh.

You start a new simulation in CFX-Pre and import the refined mesh. This tutorial introduces General mode (the mode used for most tutorials) in CFX-Pre. The physics for this tutorial are the same as for Simulating Flow in a Static Mixer Using CFX in Stand-alone Mode; therefore, you can import the physics settings used in that tutorial to save time.

 

4.3. 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 static_mixer_refined_mesh.zip file here .

  3. Unzip static_mixer_refined_mesh.zip to your working directory.

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

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

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

 

4.4. 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. Select General in the New Case dialog box and click OK.

  3. Select File > Save Case As.

  4. Under File name, type StaticMixerRef and click Save.

 

4.4.1. Importing a Mesh

At least one mesh must be imported before physics are applied.

  1. Select File > Import > Mesh.

    The Import Mesh dialog box appears.

  2. Configure the following setting(s):

    Setting

    Value

    Files of type

    CFX Mesh (*gtm *cfx)

    File name

    StaticMixerRefMesh.gtm [a]

    1. This mesh is more refined than the one used in the other "Static Mixer" tutorials (StaticMixerMesh.gtm).

  3. Click Open.

    The Mesh tree shows the regions in the StaticMixerRefMesh.gtm assembly in a tree structure. The first tree branch displays the 3D regions and the level below each 3D region shows the 2D regions associated with it. The check box next to each item in the Mesh tree indicates the visibility status of the object in the viewer; you can click these to toggle visibility.

    Note:  An assembly is a group of mesh regions that are topologically connected. Each assembly can contain only one mesh, but multiple assemblies are permitted.

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

 

4.4.2. Importing Settings from Tutorial 1

Because the physics and region names for this simulation are very similar to that for Tutorial 1, you can save time by importing the settings used there. You will be importing CCL from Tutorial 1 that contains settings that reference mesh regions. For example, the outlet boundary condition references the mesh region named out. In this tutorial, the name of the mesh regions are the same as in Tutorial 1, so you can import the CCL without error.

  1. Select File > Import > CCL.

    The Import CCL dialog box appears.

  2. Under Import Method, select Replace.

    Replace is useful if you have defined physics and want to update or replace them with newly imported physics.

  3. Under Files of type, select CFX-Solver input files (*def *res).

  4. Select StaticMixer.def.

  5. Click Open.

  6. View the Outline tab.

    The tree view displays a summary of the current simulation in a tree structure. Some items may be recognized from Tutorial 1; for example the boundary condition objects in1, in2, and out.

Note:

  • If you import CCL that references nonexistent mesh regions, you will get errors.

  • A number of file types can be used as sources to import CCL, including:

    • Simulation files (*.cfx)

    • Results files (*.res)

    • CFX-Solver input files (*.def)

  • The physics for a simulation can be saved to a CCL file at any time by selecting File > Export > CCL.

 

4.4.3. Viewing Domain Settings

It is useful to review the options available in General mode.

Various domain settings can be set. These include:

  • Basic Settings

    Specifies the location of the domain, coordinate frame settings and the fluids/solids that are present in the domain. You also reference pressure, buoyancy and whether the domain is stationary or rotating. Mesh motion can also be set.

  • Fluid Models

    Sets models that apply to the fluid(s) in the domain, such as heat transfer, turbulence, combustion, and radiation models. An option absent in Tutorial 1 is Turbulent Wall Functions, which is set to Scalable. Wall functions model the flow in the near-wall region. For the k-epsilon turbulence model, you should always use scalable wall functions.

  • Initialization

    Sets the initial conditions for the current domain only. This is generally used when multiple domains exist to enable setting different initial conditions in each domain, but can also be used to initialize single-domain simulations. Global initialization allows the specification of initial conditions for all domains that do not have domain-specific initialization.

  1. In the Outline tree view, under Simulation > Flow Analysis 1, double-click Default Domain.

    The domain Default Domain is opened for editing.

  2. Click the Basic Settings tab and review, but do not change, the current settings.

  3. Click Fluid Models and review, but do not change, the current settings.

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

  5. Click Close.

 

4.4.4. Viewing the Boundary Condition Setting

For the k-epsilon turbulence model, you must specify the turbulent nature of the flow entering through the inlet boundary. For this simulation, the default setting of Medium (Intensity = 5%) is used. This is a sensible setting if you do not know the turbulence properties of the incoming flow.

  1. Under Default Domain, double-click in1.

  2. Click the Boundary Details tab and review the settings for Flow Regime, Mass and Momentum, Turbulence and Heat Transfer.

  3. Click Close.

 

4.4.5. Defining Solver Parameters

Solver Control parameters control aspects of the numerical-solution generation process.

In Tutorial 1 you set some solver control parameters, such as Advection Scheme and Timescale Control, while other parameters were set automatically by CFX-Pre.

In this tutorial, High Resolution is used for the advection scheme. This is more accurate than the Upwind Scheme used in Tutorial 1. You usually require a smaller time step when using this model. You can also expect the solution to take a higher number of iterations to converge when using this model.

  1. Select Insert > Solver > Solver Control from the menu bar or click Solver Control  .

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Basic Settings

    Advection Scheme

    > Option

     

    High Resolution

    Convergence Control

    > Max. Iterations [a]

     

    150

    Convergence Control

    > Fluid Timescale Control

    > Timescale Control

     

     

    Physical Timescale

    Convergence Control

    > Fluid Timescale Control

    > Physical Timescale

     

     

    0.5 [s]

    1. If your solution does not meet the convergence criteria after this number of time steps, the CFX-Solver will stop.

  3. Click Apply.

  4. Click the Dynamic Model Control tab.

    Tip:  To select Dynamic Model Control you might need to click the navigation icons next to the tabs to move ‘forward’ or ‘backward’ through the various tabs.

  5. Ensure that Global Dynamic Model Control is selected.

  6. Click OK.

 

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

Once all boundaries are created you move from CFX-Pre into CFX-Solver.

The simulation file, StaticMixerRef.cfx, contains the simulation definition in a format that can be loaded by CFX-Pre, enabling you to complete (if applicable), restore, and modify the simulation definition. The simulation file differs from the CFX-Solver input file in two important ways:

  • The simulation file can be saved at any time while defining the simulation.

  • The CFX-Solver input file is an encapsulated set of meshes and CCL defining a solver run, and is a subset of the data in the simulation file.

  1. Click Define Run  .

    The Write Solver Input File dialog box is displayed.

  2. If required, set the path to your working directory.

  3. Configure the following setting(s):

    Setting

    Value

    File name

    StaticMixerRef.def

  4. Click Save.

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

  5. If you are notified in CFX-Pre that the file already exists, click Overwrite.

  6. Quit CFX-Pre, saving the simulation (.cfx) file.

 

4.5. Obtaining the Solution Using CFX-Solver Manager

Two windows are displayed when CFX-Solver Manager runs. There is an adjustable split between the windows that is oriented either horizontally or vertically, depending on the aspect ratio of the entire CFX-Solver Manager window (also adjustable).

The tutorial follows this general workflow for generating the solution in CFX-Solver Manager:

 

4.5.1. Starting the Run with an Initial Values File

In CFX-Solver Manager, the Define Run dialog box is visible and Solver Input File has automatically been set to the CFX-Solver input file from CFX-Pre: StaticMixerRef.def.

Configure the settings so that the results from Tutorial 1 (contained in StaticMixer_001.res) will be used to initialize the solution:

  1. Under the Initial Values tab, select Initial Values Specification.

  2. Set Initial Values Specification > Initial Values > Initial Values 1 > Initial Values 1 Settings > File Name to StaticMixer_001.res.

    If you did not complete the first tutorial, you can use StaticMixer_001.res from your working directory.

  3. Set Use Mesh From to Solver Input File.

  4. Clear Initial Values Specification > Continue History From.

    This will cause the CFX-Solver to use the results in the StaticMixer_001.res file as a basic initial guess for the solution, and will cause the iteration count to start from 1 instead of from the last iteration number in the initial values file.

  5. Click Start Run.

    Note:  Convergence information is plotted once the second outer loop iteration is complete.

 

4.5.2. Confirming Results

When the run is finished, specific information appears in the text window of CFX-Solver Manager.

To confirm that results interpolation was successful, look in the text window in CFX-Solver Manager. The following text appears before the convergence history begins:

+----------------------------------------------------------+
| Initial Conditions Supplied by Fields in the Input Files |
+----------------------------------------------------------+

This lists the variables that were interpolated from the results file.

After the final iteration, a message similar to the following content appears in a message window:

StaticMixerRef_001 has completed normally.
Run concluded at: Fri Nov 27 11:57:57 2009

This indicates that CFX-Solver has successfully calculated the solution for the problem to the specified accuracy or has run out of coefficient loops.

  1. In the Solver Run Finished Normally window, ensure that the check box next to Post-Process Results is cleared to prevent CFD-Post from launching at this time.

  2. Click OK.

  3. Review the CFX-Solver Manager's Out File tab for details on the run results.

 

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

Once CFX-Solver has finished, you can use CFD-Post to review the finished results.

  1. On the CFX-Solver Manager, select Tools > Post-Process Results or click Post-Process Results   in the toolbar.

  2. In the Start CFD-Post dialog box, next to Results File, ensure that StaticMixerRef_001.res is set. If it is not, click Browse   and select StaticMixerRef_001.res (located in the working directory).

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

    This forces stand-alone CFX-Solver to close. This option is not required in Workbench.

  4. Click OK.

    After a short pause, CFD-Post starts.

 

4.6. Viewing the Results Using CFD-Post

In the following sections, you will explore the differences between the mesh and the results from this tutorial and Tutorial 1.

 

4.6.1. Creating a Slice Plane

More information exists for use by CFD-Post in this tutorial than in Tutorial 1 because the slice plane is more detailed.

Once a new slice plane is created it can be compared with Tutorial 1. There are three noticeable differences between the two slice planes.

  • Around the edges of the mixer geometry there are several layers of narrow rectangles. This is the region where the mesh contains prismatic elements (which are created as inflation layers). The bulk of the geometry contains tetrahedral elements.

  • There are more lines on the plane than there were in Tutorial 1. This is because the slice plane intersects with more mesh elements.

  • The curves of the mixer are smoother than in Tutorial 1 because the finer mesh better represents the true geometry.

  1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).

  2. From the menu bar, select Insert > Location > Plane or under Location, click Plane.

  3. In the Insert Plane dialog box, type Slice and click OK.

    The Geometry, Color, Render and View tabs enable you to switch between settings.

  4. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Domains

    Default Domain

    Definition

    > Method

     

    XY Plane

    Definition

    > Z

     

    1 [m]

    Plane Type

    Slice

    Render

    Show Faces

    (Cleared)

    Show Mesh Lines

    (Selected)

  5. Click Apply.

  6. Right-click a blank area in the viewer and select Predefined Camera > View From +Z.

  7. If necessary, click Zoom Box   and zoom in on the geometry to view it in greater detail.

  8. Compare the on-screen image with the equivalent picture from Simulating Flow in a Static Mixer Using CFX in Stand-alone Mode (in the section Rendering Slice Planes).

 

4.6.2. Coloring the Slice Plane

Here, you will color the plane by temperature.

  1. Configure the following setting(s):

    Tab

    Setting

    Value

    Color

    Mode [a]

    Variable

    Variable

    Temperature

    Range

    Global

    Render

    Show Faces

    (Selected)

    Show Mesh Lines

    (Cleared)

    1. A mode setting of Constant would enable you to color the plane with a fixed color.

  2. Click Apply.

 

4.6.3. Loading Results from Tutorial 1 for Comparison

In CFD-Post, you may load multiple results files into the same instance for comparison.

  1. To load the results file from Tutorial 1, select File > Load Results or click Load Results  .

  2. (Do not click Open until instructed to do so.) In the Load Results File dialog box, select StaticMixer_001.res from your working directory.

  3. On the right side of the dialog box, there are three frames:

    • Case options

    • Additional actions

    • CFX run history and multi-configuration options.

    Under Case options, select Keep current cases loaded and ensure that Open in new view is selected.

  4. Under Additional actions, ensure that the Clear user state before loading check box is cleared.

  5. Under CFX run history and multi-configuration options, ensure that Load only the last results is selected.

  6. Click Open to load the results.

    In the tree view, there is now a second group of domains, meshes and boundary conditions with the heading StaticMixer_001.

    In the 3D Viewer, there are two viewports named View 1 and View 2; the former shows StaticMixer_001 and the latter shows StaticMixerRef_001.

  7. Double-click the Wireframe object under User Locations and Plots.

  8. In the Definition tab, set Edge Angle to 5 [degree].

  9. Click Apply.

  10. Click Synchronize camera in displayed views   so that all viewports maintain the same camera position.

  11. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).

    Both meshes are now displayed in a line along the Y axis. Notice that one mesh is of a higher resolution than the other.

  12. Set Edge Angle to 30 [degree].

  13. Click Apply.

 

4.6.4. Comparing Slice Planes Using Multiple Views

The visibility status of each object is maintained separately for each viewport. This allows some planes to be shown while others are hidden. However, you can also use the Synchronize visibility in displayed views   to synchronize the visibility of objects that you add.

  1. Under User Locations and Plots, select the check box beside Slice.

  2. Right-click in the viewer and select Predefined Camera > View From -Z.

    Note the difference in temperature distribution.

  3. In the viewer toolbar, click Synchronize visibility in displayed views   to deselect the option.

  4. Click in View 1 in the 3D Viewer, then clear the visibility check box for Slice in the Outline tree view.

  5. Click in View 2. Note that the visibility check box for Slice has been re-selected as it describes the state of the plane for View 2. Clear the visibility check box for Slice in this view.

  6. To return to a single viewport, select the option with a single rectangle.

  7. Ensure that the visibility check box for Slice is cleared.

  8. Right-click StaticMixer_001 in the tree view and select Unload.

 

4.6.5. Viewing the Surface Mesh on the Outlet

In this part of the tutorial, you will view the mesh on the outlet. You will see five layers of inflated elements against the wall. You will also see the triangular faces of the tetrahedral elements closer to the center of the outlet.

  1. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).

  2. In the tree view, ensure that the visibility check box for StaticMixerRef_001 > Default Domain > out is selected, then double-click out to open it for editing.

    Because the boundary location geometry was defined in CFX-Pre, the details view does not display a Geometry tab as it did for the planes.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Render

    Show Faces

    (Cleared)

    Show Mesh Lines

    (Selected)

    Color Mode

    User Specified

    Line Color

    (Select any light color)

  4. Click Apply.

  5. Click Zoom Box  .

  6. Zoom in on the geometry to view out in greater detail.

  7. Click Rotate  on the Viewing Tools toolbar.

  8. Rotate the image as required to clearly see the mesh.

 

4.6.6. Looking at the Inflated Elements in Three Dimensions

To show more clearly what effect inflation has on the shape of the elements, you will use volume objects to show two individual elements. The first element that will be shown is a normal tetrahedral element; the second is a prismatic element from an inflation layer of the mesh.

Leave the surface mesh on the outlet visible to help see how surface and volume meshes are related.

  1. From the menu bar, select Insert > Location > Volume or, under Location click Volume.

  2. In the Insert Volume dialog box, type Tet Volume and click OK.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Definition

    > Method

     

    Sphere

    Definition

    > Point [a]

     

    0.08, 0, -2

    Definition

    > Radius

     

    0.14 [m]

    Definition

    > Mode

     

    Below Intersection

    Inclusive [b]

    (Cleared)

    Color

    Color

    Red

    Render

    Show Faces

    > Transparency

     

    0.3

    Show Mesh Lines

    (Selected)

    Show Mesh Lines

    > Line Width

     

    1

    Show Mesh Lines

    > Color Mode

     

    User Specified

    Show Mesh Lines

    > Line Color

     

    Grey

    1. The z slider’s minimum value corresponds to the minimum z value of the entire geometry, which, in this case, occurs at the outlet.

    2. Only elements that are entirely contained within the sphere volume will be included.

  4. Click Apply to create the volume object.

  5. Right-click Tet Volume and choose Duplicate.

  6. In the Duplicate Tet Volume dialog box, type Prism Volume and click OK.

  7. Double-click Prism Volume.

  8. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Definition

    > Point

     

    -0.22, 0.4, -1.85

    Definition

    > Radius

     

    0.206 [m]

    Color

    Color

    Orange

  9. Click Apply.

 

4.6.7. Viewing the Surface Mesh on the Mixer Body

  1. Double-click the Default Domain Default object.

  2. Configure the following setting(s):

    Tab

    Setting

    Value

    Render

    Show Faces

    (Selected)

    Show Mesh Lines

    (Selected)

    Line Width

    2

  3. Click Apply.

 

4.6.8. Viewing the Layers of Inflated Elements on a Plane

You will see the layers of inflated elements on the wall of the main body of the mixer. Within the body of the mixer, there will be many lines that are drawn wherever the face of a mesh element intersects the slice plane.

  1. From the menu bar, select Insert > Location > Plane or under Location, click Plane.

  2. In the Insert Plane dialog box, type Slice 2 and click OK.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Definition

    > Method

     

    YZ Plane

    Definition

    > X

     

    0 [m]

    Render

    Show Faces

    (Cleared)

    Show Mesh Lines

    (Selected)

  4. Click Apply.

  5. Turn off the visibility of all objects except Slice 2.

  6. To see the plane clearly, right-click in the viewer and select Predefined Camera > View From -X.

 

4.6.9. Viewing the Mesh Statistics

You can use the Report Viewer to check the quality of your mesh. For example, you can load a .def file into CFD-Post and check the mesh quality before running the .def file in the solver.

  1. Click the Report Viewer tab (located below the viewer window).

    A report appears. Look at the table shown in the "Mesh Report" section.

  2. Double-click Report > Mesh Report in the Outline tree view.

  3. In the Mesh Report details view, select Statistics > Maximum Face Angle.

  4. Click Refresh Preview.

    Note that a new table, showing the maximum face angle for all elements in the mesh, has been added to the "Mesh Report" section of the report. The maximum face angle is reported as 148.95°.

As a result of generating this mesh statistic for the report, a new variable, Maximum Face Angle, has been created and stored at every node. This variable will be used in the next section.

 

4.6.10. Viewing the Mesh Elements with Largest Face Angle

In this section, you will visualize the mesh elements that have a Maximum Face Angle value greater than 140°.

  1. Click the 3D Viewer tab (located below the viewer window).

  2. Right-click a blank area in the viewer and select Predefined Camera > Isometric View (Z up).

  3. In the Outline tree view, select the visibility check box of Wireframe.

  4. From the menu bar, select Insert > Location > Volume or under Location, click Volume.

  5. In the Insert Volume dialog box, type Max Face Angle Volume and click OK.

  6. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Definition

    > Method

     

    Isovolume

    Definition

    > Variable

     

    Maximum Face Angle [a]

    Definition

    > Mode

     

    Above Value

    Definition

    > Value

     

    140 [degree]

    Inclusive [b]

    (Selected)

    1. Select Maximum Face Angle from the larger list of variables available by clicking   to the right of the Variable box.

    2. This includes any elements that have at least one node with a variable value greater than or equal to the given value.

  7. Click Apply.

    The volume object appears in the viewer.

 

4.6.11. Viewing the Mesh Elements with Largest Face Angle Using a Point

Next, you will create a point object to show a node that has the maximum value of Maximum Face Angle. The point object will be represented by a 3D yellow crosshair symbol. In order to avoid obscuring the point object with the volume object, you may want to turn off the visibility of the latter.

  1. From the menu bar, select Insert > Location > Point or under Location, click Point.

  2. Click OK to use the default name.

  3. Configure the following setting(s):

    Tab

    Setting

    Value

    Geometry

    Definition

    > Method

     

    Variable Maximum

    Definition

    > Location

     

    Default Domain

    Definition

    > Variable

     

    Maximum Face Angle

    Symbol

    Symbol Size

    2

  4. Click Apply.

 

4.6.12. 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.