Chapter 3: Steam Stator

This tutorial includes:

This tutorial teaches you how to:

  • Import hub, shroud, and blade geometry from individual curve files.

  • Change the method of constructing the hub and shroud curve types.

  • Make colored surfaces to show variations in mesh measures (such as Minimum Face Angle).

  • Add a blade blend made using the rolling ball process with a constant radius (BladeModeler or BladeBuilder license required).

As you work through this tutorial, you will create a mesh for a blade passage of a steam stator. A typical blade passage is shown by the black outline in the figure below.

The stator contains 60 blades distributed about the Z axis. A clearance gap exists between the blades and the shroud, with a width of 2% of the total span. Within the blade passage, the maximum diameter of the shroud is approximately 97.5 cm.

If this is the first tutorial you are working with, it is important to review Introduction to the Ansys TurboGrid Tutorials before beginning.

 

3.1. Preparing the Working Directory

  1. Create a working directory.

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

  2. Download the stator.zip file here .

  3. Unzip stator.zip to your working directory.

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

    • BladeGen.inf

    • shroud.curve

    • hub.curve

    • profile.curve

  4. Set the working directory and start TurboGrid.

    For details, see Setting the Working Directory and Starting Ansys TurboGrid.

 

3.2. Defining the Geometry

In the first tutorial, you loaded a BladeGen.inf file in order to specify the machine data (# of blade sets, rotation axis, and units) and curve files. In this tutorial, you will enter such data manually using the Load Profile Points Or CAD command.

 

3.2.1. Loading the Curves

Load the curve files for the steam stator as follows:

  1. Click File > Load Profile Points Or CAD.

    The geometry browser (the main object editor of the Geometry workspace) appears. TurboGrid fills in the names of the curve files based on the files that are present in the working directory; The first .crv or .curve file found that has a name containing “hub”, ”shroud”, or “blade”/”profile” is selected as the hub, shroud, or blade file, respectively.

  2. Ensure that, under Point Data Definition > TurboGrid Curve Files, Hub is set to ./hub.curve, Shroud is set to ./shroud.curve, and Blades is set to ./profile.curve.

  3. Set Point Data Definition > Coordinates and Units > Coordinates to Cartesian and Length Units to cm.

    These units are used to interpret the data in the curve files.

  4. Set Geometry Setup > Rotation > Method to Principal Axis and Axis to Z.

  5. Set Geometry Setup > # of Bladesets to 60.

  6. Click Apply to save the settings.

  7. Return to the Mesh tab to view the geometry.

The progress bar at the bottom right of the screen shows the geometry generation progress. After the geometry has been generated, you can see the hub, shroud, and blade for one passage. Along the blade, you can see the leading and trailing edge curves (green and red lines, respectively). Near the blade, you can see the inlet and outlet markers (white octahedrons).

Figure 3.1: Incorrect Hub and Shroud Representations

Incorrect Hub and Shroud Representations

As shown in Figure 3.1: Incorrect Hub and Shroud Representations, the hub and shroud are greatly distorted. This is the result of using spline curves to construct the hub and shroud based on relatively few data points. This problem will be corrected in the next section.

 

3.2.2. Setting the Curve Type

Set the method of constructing the hub and shroud as follows:

  1. Open Geometry > Hub.

  2. Set Geometric Representation > Curve Type to Piece-wise linear.

  3. Click Apply.

  4. Set Shroud in the same way.

 

3.2.3. Defining the Shroud Tip

To complete the geometry, create a small gap between the blade and the shroud. The blade should be shortened to 98% of its original span because the gap width is 2% of the total span, as specified in the problem description.

  1. Open Geometry > Blade Set > Shroud Tip.

  2. Set Tip Option to Constant Span.

  3. Set Span to 0.98.

  4. Click Apply.

This completes the geometry definition.

 

3.3. Creating the Topology and Mesh

  1. Click Hide all geometry objects   to turn off the visibility of the geometry.

  2. Right-click Topology Set and turn off Suspend Object Updates.

    After some time, you will see a warning message about the inlet domain being turned off.

  3. Dismiss the warning message.

    The topology and 3D mesh are generated.

  4. Turn on the visibility of Layers > Hub to show the topology on the hub.

  5. Turn on the visibility of Layers > Shroud Tip to show the topology on the shroud tip.

Note:  It might be useful to keep the same topology when studying a range of blade geometries, or the same blade on different computers. To keep the same topology, use the Manual (Advanced) setting for the topology. This setting is available after clicking Edit > Options and selecting Enable Advanced Features.

 

3.4. Reviewing the Mesh Data Settings

TurboGrid automatically computes a default mesh and sets the base mesh dimensions.

Each unique mesh dimension has an edge refinement factor that is multiplied by the base mesh dimension and global size factor to determine the final mesh size. The overall mesh size is controlled using the Method setting in the Mesh Data object editor on the Mesh Size tab. Setting the Method to Target Passage Mesh Size enables you to specify a Node Count. Using this method specifies an approximate mesh size (in nodes) and lets TurboGrid compute the mesh dimensions automatically. Setting the Method to Global Size Factor enables you to specify a Size Factor. Increasing this factor will increase the overall mesh size, and decreasing it will decrease the overall mesh size. The change is nonlinear.

The Boundary Layer Refinement Control settings affect the mesh in the O-Grid region around the blade:

  • Note that, when Boundary Layer Refinement Control > Method is set to Proportional to Mesh Size, the number of elements across the boundary layer is calculated as Base Count * Global Size Factor * (Factor Base + Factor Ratio * Global Size Factor). The default values of Factor Base and Factor Ratio are 3 and 0 respectively.

  • The Target Maximum Expansion Rate setting affects the expansion rates that are used just outside the blade profile.

  • The Near Wall Element Size Specification settings control the method by which the near-wall node spacing is specified on the Passage, Hub Tip, and Shroud Tip tabs. The near-wall node spacing is the distance between a wall (for example, hub, shroud, or blade) and the first layer of nodes from the wall. The Method setting has these options:

    • Y Plus — The y+ method sets the near-wall spacing to a target value, y+, in relation to a set Reynolds number.

    • Absolute — The Absolute method enables you to set the near-wall spacing directly on the Passage, Hub Tip, and Shroud Tip tabs.

  • The Inlet Domain and Outlet Domain check boxes enable you to generate the inlet and outlet domains as part of the mesh. Settings that affect these grid regions are found on the Inlet/Outlet tab.

Selecting the Lock mesh size check box forces the total number of nodes and elements to remain constant.

On the Shroud Tip tab, you can use the Blade Tip > Override Target Maximum Expansion Rate setting to override the Target Maximum Expansion Rate value set on the Mesh Size tab, to govern the expansion rate of elements that cross the tip mesh.

 

3.5. Reviewing the Mesh Quality on the Hub and Shroud Layers

If the topology were grossly skewed or distorted on the hub or shroud layer, the Layers object would be shown with red text in the object selector. Since the Layers object is shown in black text, the mesh contains no regions with high skew on the hub or shroud.

By default, TurboGrid automatically generates the recommended number of layers before the mesh is generated. This default behavior can be disabled by editing the Layers object so that Insertion Mode is not set to Automatic - Adaptive.

A turbo surface of constant "K" (a nodal coordinate) appears. This surface is listed in the object selector as 3D Mesh > Show Mesh. You can change the location and coloring of this surface to explore the mesh.

 

3.6. Analyzing the Mesh

Check the 3D mesh statistics:

  1. Open Mesh Analysis.

    The mesh statistics are acceptable based on the current quality criteria.

  2. Close the Mesh Statistics dialog box.

 

3.6.1. Examining the Mesh Qualitatively

The predefined surfaces found under the 3D Mesh object in the object selector are useful for showing variations in the mesh statistics.

In the following section, you will color 3D Mesh > Show Mesh by Minimum Face Angle. You will then create a legend for that object.

 

3.6.1.1. Editing a Turbo Surface

Turbo Surfaces can be created by selecting Insert > User Defined > Turbo Surface. In this case, you will simply edit the predefined turbo surface.

  1. Open 3D Mesh > Show Mesh.

  2. Leave Variable, and Value unchanged.

  3. Click the Color tab and set Mode to Variable.

  4. Set Variable to Minimum Face Angle.

  5. Set Range to Local.

    This will cause the range of colors in the color map to be distributed over the range of values found on the turbo surface, rather that over the global range or a user-defined range.

  6. Click the Render tab.

  7. Ensure that Draw Faces is selected.

  8. Click Apply to apply the changes to the turbo surface.

 

3.6.1.2. Creating a Legend

To illustrate the scale of the Minimum Face Angle variable, create a legend for the turbo surface:

  1. Click Insert > User Defined > Legend.

  2. Click OK to accept the default name.

  3. Set Plot to TURBO SURFACE:Show Mesh.

  4. Set Title Mode to Variable and Location.

  5. Click Apply to create the legend.

 

3.7. Adding a Blade Blend

In this section of the tutorial, you will add a blade blend (fillet) using the blade blend object. A blade blend object specifies hub and/or shroud blends (fillets) made by the rolling ball process with a constant radius.

Note:  The blade blend object makes use of the CAD From Profile Points input mode, which, in general, requires either a BladeModeler license or a BladeBuilder license. This tutorial happens to use BladeEditor as a CAD generator, so requires a BladeModeler license. The CAD From Profile Points input mode is available only in stand-alone mode; it is not supported in Ansys Workbench.

Add a blade blend object as follows:

  1. In the Mesh workspace, right-click Blade 1 and select Insert > Blade CAD Feature > Blade Blend.

    The Blade CAD Features object editor opens with the Blade Blends tab displayed.

  2. In the object editor, select Hub Blend and set Hub Blend > Rolling Ball Radius to 2.5 [mm].

  3. Click Apply.

    (Do not click Apply And Generate CAD because you will review settings in the geometry browser before generating CAD.)

  4. In the Geometry workspace, in the geometry browser:

    1. On the Input Selection tab, set Input Mode to CAD From Profile Points.

      The CAD Properties tab appears.

    2. On the CAD Properties tab, ensure that Blend Style is set to Approximate Blend (Low Fidelity Geometry Only) and that CAD Generation Tool > Tool is set to BladeEditor.

      Note that the default tool is specified by a user preference.

    3. Click Apply And Generate CAD.

      TurboGrid drives Ansys BladeModeler in the background to generate CAD geometry.

  5. The geometry is now entirely represented by CAD that was generated, using Ansys BladeModeler, based on the profile point definition (provided by curve files) and the blade blend specification (provided by the blade blend object).

    If there is any change to the curve files or blade blend object, be sure to regenerate the geometry. You can regenerate the geometry from the Apply and Generate CAD button or from File > Update Geometry. In particular, even after loading a state file, you might need to regenerate the geometry if the profile point definition or blade blend specification has changed since the last time the CAD geometry was generated.

The blade blend is shown in Figure 3.2: Blade Blend Shown.

Figure 3.2: Blade Blend Shown

Blade Blend Shown

Note:  A known issue with using the blade blend object can result in failure of CAD generation. If CAD generation fails, try making a very small change to the blend radius.

Other troubleshooting alternatives:

  • Specify the Layers object with Insertion Mode set to Automatic - Adaptive.

  • Specify the Layers object with Insertion Mode set to Manual - Uniform.

  • Specify the Topology Set object with Mesh Generation Mode set to ATM3D.

 

3.8. Saving the Mesh

Save the mesh:

  1. Click File > Save Mesh As.

  2. Ensure that Files of type is set to Ansys CFX Mesh Files.

  3. Set Export Units to cm.

  4. Set File name to steam_stator.gtm.

  5. Ensure that your working directory is set correctly.

  6. Click Save.

 

3.9. Saving the State (Optional)

If you want to revisit this mesh at a later date, save the state:

  1. Click File > Save State As.

  2. Enter an appropriate state filename.

  3. Click Save.