Chapter 4: Radial Compressor

This tutorial includes:

This tutorial teaches you how to:

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

The blade row contains 9 main blades and 9 splitter blades that revolve about the negative Z axis. The blades have cut-off trailing edges. A clearance gap exists between the blades and the shroud, with a width of 5% of the total span. Within the blade passage, the maximum diameter of the shroud is approximately 125 mm.

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

 

4.1. Preparing the Working Directory

  1. Create a working directory.

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

  2. Download the radcomp.zip file here .

  3. Unzip radcomp.zip to your working directory.

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

    • BladeGen.inf

    • profile.crv

    • hub.crv

    • shroud.crv

  4. Set the working directory and start Ansys TurboGrid.

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

 

4.2. Defining the Geometry

In the Rotor 37 tutorial, you loaded a BladeGen.inf file in order to specify the machine data (# of blade sets, rotation axis, and units) and the hub, shroud, and blade curve files. In the Steam Stator tutorial, you entered the same data using the Load Profile Points Or CAD command. In this tutorial, you will define the machine data and curve files individually, by editing the corresponding geometry objects.

 

4.2.1. Defining the Machine Data

Set up the Machine Data object, which contains basic information about the geometry:

  1. In the Mesh workspace, open Geometry > Machine Data.

  2. Set # of Bladesets to 9.

  3. Set Base Units to mm.

  4. Click Apply to save the settings.

 

4.2.2. Defining the Hub

  1. Open Geometry > Hub.

  2. Set Length Units to mm.

  3. Ensure that File Name is set to ./hub.crv from your working directory.

  4. Click Apply.

 

4.2.3. Defining the Shroud

  1. Open Geometry > Shroud.

  2. Set Length Units to mm.

  3. Ensure that File Name is set to ./shroud.crv from your working directory.

  4. Click Apply.

    Note:  If you had loaded the BladeGen.inf file, the Curve Type settings for the Hub and Shroud objects would have been set to Piece-wise linear instead of the default: Bspline. Either setting will work for this geometry.

At this point, the entire hub and shroud surfaces are shown. After a blade is defined (in the next step), the hub and shroud will be trimmed to show only one passage.

Figure 4.1: Hub and Shroud of Radial Compressor

Hub and Shroud of Radial Compressor

 

4.2.4. Defining the Blade

  1. In the Mesh workspace, open Geometry > Blade Set > Blade 1.

  2. Ensure that File Name is set to ./profile.crv.

  3. Set Length Units to mm.

  4. Set Geometric Representation > Method to Specify.

  5. Set Geometric Representation > Lofting to Spanwise.

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

  7. Set Geometric Representation > Surface Type to Ruled.

  8. Under Trailing Edge Definition, select Cut-off or square.

  9. Click Apply.

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).

 

4.2.5. Defining the Splitter Blade

  1. Right-click Geometry > Blade Set and select Insert > Blade.

  2. Click OK to accept the default name.

  3. Set Blade Number to 2.

  4. Click Apply.

 

4.2.6. Defining the Shroud Tip

To complete the geometry, create a small gap between the blade and the shroud. The blade should be shortened to 95% of its original span because the gap width is 5% 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 0.95.

  4. Click Apply.

 

4.3. Creating the Topology and Mesh

In this tutorial, you will manually choose a set of ATM topology templates, called a topology family.

  1. Click the Topology Viewer tab.

  2. Open Topology Set.

  3. Browse through ATM Topology > Method.

    ATM Topology > Method provides a list of topology families from which you can manually choose. When you mouse over or cursor through the list, the Topology Viewer shows a picture of the highlighted topology family and a description of the type of blade that the family best fits.

  4. Set ATM Topology > Method to Single Splitter.

  5. Click Apply to set the topology.

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

    The topology and 3D mesh are generated.

 

4.4. Mesh Data Settings

The Mesh Data object indicates that there is a problem with mesh quality.

  1. Click the 3D Viewer tab.

  2. Expand the Mesh Data object in the object selector.

  3. Open one of the Boundary Layer Control objects under Mesh Data.

Note that the near wall expansion rate is outside the established limit within the boundary layer region. The affected mesh regions are colored red in the viewer.

Add more elements to the boundary layer region as follows:

  1. Open the Mesh Data object.

  2. On the Mesh Size tab, ensure that Boundary Layer Refinement Control > Method is set to Proportional to Mesh Size.

  3. Set Boundary Layer Refinement Control > Parameters > Factor Base to 4.0.

  4. Click Apply.

The Mesh Data object no longer indicates that there is a problem with mesh quality.

As an exercise, change the distribution of elements across the cut-off edge as follows:

  1. Set Cutoff Edge Split Factor > Trailing to 0.9.

  2. Click Apply.

Note that, for a blade that has one rounded edge and one cut-off edge, the distribution of elements across the blade tip mesh is governed by the distribution across the cut-off edge.

 

4.5. 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.

 

4.6. 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 radial_compressor.gtm.

  5. Ensure that your working directory is set correctly.

  6. Click Save.

 

4.7. 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.