10. MIXED-FLOW PUMP IMPELLER

This tutorial employs the configuration of a mixed-flow pump impeller to demonstrate the use of hybrid hexahedral/tetrahedral meshing capabilities in conjunction with GAMBIT turbo modeling. Such capabilities are particularly useful for meshing turbo models that involve highly twisted blades.

10.1 Prerequisites

Prior to reading and performing the steps outlined in this tutorial, you should familiarize yourself with the steps, principles, and procedures described in Tutorials 1, 2, 3, 4, and 8.

10.2 Problem Description

Figure 10-1 shows the turbomachinery configuration to be modeled and meshed in this tutorial. The configuration consists of an impeller rotor on which are affixed five identical blades, each of which is spaced equidistant from the others on the rotor hub.

Figure 10-1: Mixed-flow impeller rotor

The overall goal of this tutorial is to create a geometric model of the flow region immediately surrounding one of the impeller blades and to mesh the model using hybrid hexahedral/tetrahedral mesh.

10.3 Strategy

The GAMBIT turbo modeling procedure includes seven basic steps:

Creating or importing edge data that describes the turbo profile
Creating the turbo profile
Creating the turbo volume
Assigning zone types to regions of the turbo volume
Decomposing the turbo volume
Meshing the turbo volume
Viewing the turbo volume

This tutorial illustrates six of the seven steps listed above. The tutorial excludes the turbo decomposition step, because the bulk of the turbo volume is to be meshed using unstructured tetrahedral mesh elements. Turbo volume decomposition is primarily used to facilitate the creation of structured meshes (see Tutorial 9 in this guide).

NOTE: In this tutorial, the turbo-volume viewing operation (Step 7, above) is illustrated in conjunction with the mesh examination step (see "Step 10: Examine the Mesh," below).

10.4 Procedure

1. Copy the file

path/Fluent.Inc/gambit2.x/help/tutfiles/rotor-cyl-mod.tur

(where 2.x is the GAMBIT version number) from the GAMBIT installation area in the directory path to your working directory.

2. Start GAMBIT using the session identifier "Pump_Impeller".

Step 1: Select a Solver

1. Choose the solver from the main menu bar:

Solver —> FLUENT 5/6

The choice of solver affects the types of options available in the Specify Boundary Types form (see below). For some systems, FLUENT 5/6 is the default solver. The currently selected solver is shown at the top of the GAMBIT GUI.

Step 2: Import a Turbo Data File

Turbo data files contain information that GAMBIT uses to define the turbo profile (see "Step 3: Create the Turbo Profile," below). Such information includes: point data that describes the shapes of the profile edges, edge-continuity data, and specification of the rotational axis for the turbo volume.

1. Select the Import Turbo File option from the main menu bar.

File —> Import —> Turbo...

This command sequence opens the Import Turbo File form.

2. Click the Browse... button.

This action opens the Select File form.

a) In the Files list, select rotor-cyl-mod.tur.

b) On the Select File form, click Accept.

3. On the Import Turbo File form, click Accept.

GAMBIT reads the information contained in the data file and constructs the set of edges shown in Figure 10-2. The two straight edges shown in the figure describe the hub and casing for the turbo volume. The five sets of curved edges constitute cross sections of a single turbo blade.

Figure 10-2: Imported impeller geometry

Step 3: Create the Turbo Profile

The turbo profile defines the basic characteristics of the turbo volume, including the shapes of the hub, casing, and periodic (side) surfaces. In GAMBIT, the edges that describe the hub, casing, and blade cross sections are defined by means of their inlet endpoint vertices.

1. Specify the hub, casing, and blade-cross-section edges of the turbo profile.

TOOLS —> TURBO —> CREATE PROFILE

This command sequence opens the Create Turbo Profile form.

In this step, you will specify vertices that define the hub, casing, and blade cross-sections. All instructions listed in this step refer to the vertex labels shown in Figure 10-3.

Figure 10-3: Vertices used to specify the turbo profile

a) Activate the Hub Inlet list box on the Create Turbo Profile form.

b) Select vertex A.

c) Activate the Casing Inlet list box.

d) Select vertex B.

e) Activate the Blade Tips list box.

f) Select (in order) the following vertices: C, D, E, F, and G.

! The order in which the Blade Tips vertices are selected is important to the definition of a turbo profile. Specifically, the Blade Tips vertices must be selected in order from the hub to the casing.

g) Click Apply to accept the vertex selections and create the turbo profile.

GAMBIT creates the turbo profile shown in Figure 10-4.

Figure 10-4: Turbo profile for low-speed centrifugal compressor blade

The turbo profile for this tutorial includes 10 (real) rail edges and five (virtual) medial edges, each of which corresponds to one of the blade cross sections.

Step 4: Modify the Inlet and Outlet Vertex Locations

It is often useful to control the shape of the turbo volume such that its inlet and outlet surfaces represent smooth flow transitions to and from the inlet and outlet ends, respectively, of the turbo blade. In GAMBIT, you can control the shape of the turbo volume by adjusting the positions of the medial-edge endpoint vertices prior to constructing the volume.

1. Open the Slide Virtual Vertex form.

TOOLS —> TURBO —> SLIDE VIRTUAL VERTEX

This command sequence opens the Slide Virtual Vertex form.

a) Select the inlet endpoint vertex of the medial edge for the upper blade cross section (vertex A in Figure 10-4, above).

b) In the U Value field, enter the value 0.021.

As an alternative to entering a value in the U Value field, you can select the vertex in the graphics window and drag it along its host rail edge until the U Value field value is 0.021.

c) Retain the (default) Move with links option.

The Move with links option specifies that GAMBIT is to apply the current Slide Virtual Vertex specifications to all medial-edge inlet endpoint vertices in addition to the selected vertex.

d) Click Apply to accept the new position of the medial-edge inlet endpoint vertices.

e) Select the outlet endpoint vertex of the medial edge for the upper blade cross section (vertex B).

f) In the U Value field, enter the value 0.703.

g) Retain the Move with links option.

h) Click Apply to accept the new position of the medial-edge outlet endpoint vertices.

The modified turbo profile appears as shown in Figure 10-5.

Figure 10-5: Turbo profile with modified inlet and outlet vertex locations

Step 5: Create the Turbo Volume

The turbo volume characteristics are determined by the turbo profile and by specification of the number of blades on the rotor (or angle between blades), the tip clearance, and the number of spanwise sections. This example does not include either a tip clearance or spanwise sectioning.

1. Specify the pitch for the turbo volume.

TOOLS —> TURBO —> CREATE TURBO VOLUME

This command sequence opens the Create Turbo Volume form.

a) In the Pitch text box, enter 5.

b) On the Pitch option button (located to the right of the Pitch text box), select the Blade count option.

c) In the Spanwise Sections text box, enter 1.

d) Click Apply.

GAMBIT creates the turbo volume shown in Figure 10-6.

Figure 10-6: Turbo volume for mixed-flow impeller blade

Step 6: Define the Turbo Zones

This step assigns standard zone types to surfaces of the turbo volume. The zone-type specifications determine which faces are linked for meshing. In addition, GAMBIT automatically associates turbo zone types to boundary zone definitions for some solvers.

1. Specify the faces that constitute the hub, casing, inlet, outlet of the turbo volume, as well as the pressure and suction sides of the turbo blade.

TOOLS —> TURBO —> DEFINE TURBO ZONES

This command sequence opens the Define Turbo Zones form.

(NOTE: Due to slight differences in entity numbering between computer platforms, the entity numbers for the faces shown below might differ from those displayed on the Define Turbo Zones form, above.) a) Activate the Hub list box, and select the bottom (hub) face of the turbo volume (see Figure 10-7).

Figure 10-7: Hub, Casing, Inlet, and Outlet faces

b) Activate the Casing list box, and select the top (casing) face.

c) Activate the Inlet list box, and select the front (inlet) face.

d) Activate the Outlet list box, and select the back (outlet) face.

e) Activate the Pressure list box, and select the inner (pressure) face of the turbo blade (see Figure 10-8).

Figure 10-8: Pressure and Suction faces

f) Activate the Suction list box, and select the outer (suction) face of the turbo blade.

g) Click Apply to assign the turbo zone types.

Step 7: Apply 3-D Boundary Layers

For turbo models, 3-D boundary layers allow you to ensure the creation of high-quality mesh elements in regions adjacent to the turbo blade surfaces. Such boundary layers are particularly useful when the turbo volume is to be meshed using an unstructured meshing scheme.

1. Apply boundary layers to the faces of the turbo blade.

TOOLS —> TURBO —> CREATE/MODIFY BOUNDARY LAYERS

This command sequence opens the Create Boundary Layer form.

a) In the First row text box, enter a value of 1.

b) In the Growth factor text box, enter a value of 1.2.

c) In the Rows text box, specify a value of 5, either by direct input of the value or by sliding the Rows slider bar.

GAMBIT automatically calculates a Depth value of 7.4416, based on the First row, Growth factor, and Rows specifications.

d) Select the Internal continuity option.

e) In the Attachment input field, select the Faces option.

f) Activate the Faces list box, select the pressure and suction faces on the turbo blade.

g) Click Apply.

Figure 10-9 shows the 3-D boundary layers projected onto the hub and casing surfaces of the turbo volume.

Figure 10-9: Turbo volume with 3-D boundary layers

By default, GAMBIT displays the boundary layers in the graphics window unless they are made invisible by direct user action. The boundary layer display can make it difficult to view the model during subsequent steps in the modeling process; therefore, it is advisable to render the boundary layers invisible before continuing the tutorial.

2. Select the SPECIFY DISPLAY ATTRIBUTES command button on the Global Control toolpad.

This action opens the Specify Display Attributes form.

a) Select the B. Layers check box.

b) Select the Visible:Off option.

c) Click Apply.

d) Click Close to close the Specify Display Attributes form.

Step 8: Mesh the Pressure and Suction Faces

To grow hexahedral cells from the blade surfaces, it is necessary to pre-mesh them using a Quad Map scheme.

1. Mesh the pressure and suction surfaces of the turbo blade.

TOOLS —> TURBO —> MESH EDGES/FACES/VOLUMES R

This command sequence opens the Mesh Faces form.

a) Activate the Faces list box, and select the pressure and suction faces on the turbo blade.

GAMBIT automatically selects the Quad and Map Scheme options based on the face characteristics.

b) Retain the automatically selected Scheme options.

c) On the Spacing option button, select the Interval size option.

d) In the Spacing text box, enter a value of 5.

e) Click Apply.

GAMBIT meshes the pressure and suction faces as shown in Figure 10-10.

Figure 10-10: Meshed faces of impeller blade

Step 9: Mesh the Volume

In this step, you will mesh the turbo volume using a hybrid scheme that employs hexahedral elements near the blade surface and tetrahedral elements in the bulk of the volume.

1. Mesh the turbo volume.

TOOLS —> TURBO —> MESH EDGES/FACES/VOLUMES R

This command sequence opens the Mesh Volumes form.

a) Activate the Volumes list box, and select the geometric volume that comprises the turbo volume.

b) On the Scheme:Elements option button, select Tet/Hybrid.

c) On the Scheme:Type option button, select TGrid.

d) On the Spacing option button, select Interval size.

e) In the Spacing text box, enter a value of 6.

f) Click Apply.

GAMBIT meshes the volume as shown in Figure 10-11.

Figure 10-11: Meshed turbo volume for mixed-flow impeller blade

Step 10: Examine the Mesh

1. Select the EXAMINE MESH command button at the bottom right of the Global Control toolpad.

This action opens the Examine Mesh form.

a) Click Update at the bottom of the Examine Mesh form.

GAMBIT does not automatically update the graphics display when you open the Examine Mesh form or modify its specifications, such as Display Type or Quality Type. To update the graphics display, you must click the Update pushbutton located at the bottom of the form. GAMBIT displays the Update pushbutton label in red lettering whenever the display needs to be updated to reflect the current Examine Mesh specifications.

Some Examine Mesh operations automatically update the graphics display. For example, if you select the Display Type:Range option and click one of the histogram bars, GAMBIT automatically updates the display.

The Examine Mesh form allows you to view various mesh characteristics for the 3-D mesh. For example, Figure 10-12, Figure 10-13, and Figure 10-14 display hexahedral, pyramidal, and tetrahedral volume mesh elements, respectively, for which the EquiSize Skew parameter is between 0.2 and 0.3. In this case, the hexahedral elements (Figure 10-12) result from the imposition of the 3-D boundary layer and are confined to the region immediately adjacent to the impeller blade. The pyramidal elements (Figure 10-13) constitute a single transition layer between the hexahedral and tetrahedral (Figure 10-14) elements.

Figure 10-12: Hexahedral mesh elements—EquiSize Skew = 0.2 - 0.3

Figure 10-13: Pyramidal mesh elements—EquiSize Skew = 0.2 - 0.3

Figure 10-14: Tetrahedral mesh elements—EquiSize Skew = 0.2 - 0.3

The Examine Mesh command and options can be used in conjunction with the View Turbo Volume command to view 2-D characteristics of the mesh on the hub and casing surfaces. Such views are particularly useful when examining the mesh on highly twisted blades.

2. Display the casing surface in a cascade turbo view.

TOOLS —> TURBO —> VIEW TURBO VOLUME

This command sequence opens the View Turbo Volume form.

a) Select the Cascade surface:Casing option.

The Cascade surface specifications described above specify a flattened, 2-D display of the casing surface.

b) Click Apply.

Figure 10-15 displays an enlarged view of the casing-surface face mesh elements for which the EquiSize Skew parameter is between 0.1 and 0.6 in the region surrounding the impeller outlet tip. (NOTE: To view the 2-D face elements shown in Figure 10-15, select the Display Type:2D Element option on the Examine Mesh form, and specify the display of both quadrilateral () and triangular () elements.)

Figure 10-15: Casing-surface face mesh elements—EquiSize Skew = 0.1 - 0.6

c) Select the Off option and click Apply to turn off the cascade turbo view before specifying zone types.

Step 11: Specify or Check Zone Types

For some Solver options, including the Fluent 5/6 option used in this tutorial, GAMBIT automatically assigns boundary zone specifications to the turbo volume faces when you define the turbo zones (see Step 6: Define the Turbo Zones). You can check such specifications and/or apply solver-specific boundary specifications (for cases in which they are not automatically applied) by means of the Specify Boundary Types form. It is useful to turn off the mesh display before checking and/or applying the boundary zone specifications.

1. Select the SPECIFY DISPLAY ATTRIBUTES command button on the Global Control toolpad.

This action opens the Specify Display Attributes form.

a) Select the Mesh:Off option.

b) Click Apply.

c) Click Close to close the Specify Display Attributes form.

2. Check the automatically applied boundary zone types.

ZONES —> SPECIFY BOUNDARY TYPES

This command sequence opens the Specify Boundary Types form.

If you select the Show labels option, GAMBIT displays labels in the graphics window for all of the assigned boundary zones. If you select the Show colors option, GAMBIT shades and colors the faces for which boundary zones have been defined.

Step 12: Export the Mesh and Exit GAMBIT

1. Export a mesh file.

a) Open the Export Mesh File form.

File —> Export —> Mesh...

This command sequence opens the Export Mesh File form.

i. Enter the File Name for the file to be exported—for example, the file name "pump_impeller.msh".

ii. Click Accept.

GAMBIT writes the mesh file to your working directory.

2. Save the GAMBIT session and exit GAMBIT.

a) Select Exit from the File menu.

File —> Exit

This action opens the Exit form.

b) Click Yes to save the current session and exit GAMBIT.

10.5 Summary

This tutorial demonstrates the use of the GAMBIT turbo modeling operations as applied to a mixed-flow pump impeller. In this case, 3-D boundary layers were applied to the impeller faces, and the bulk of the turbo volume was meshed using tetrahedral elements. As a result, the meshed turbo volume contained three volume element types: hexahedral (in the region adjacent to the impeller blade), pyramidal (a single transition layer), and tetrahedral (in the bulk of the turbo volume).