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.
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.
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.
The GAMBIT turbo modeling procedure includes seven basic steps:
|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).|
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".
1. Choose the solver from the main menu bar:
Solver > FLUENT 5/6
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...
2. Click the Browse... button.
b) On the Select File form, click Accept.
Figure 10-2: Imported impeller geometry
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
Figure 10-3: Vertices used to specify the turbo profile
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.
g) Click Apply to accept the vertex selections and create the turbo profile.
Figure 10-4: Turbo profile for low-speed centrifugal compressor blade
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
b) In the U Value field, enter the value 0.021.
c) Retain the (default) Move with links option.
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.
Figure 10-5: Turbo profile with modified inlet and outlet vertex locations
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
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.
Figure 10-6: Turbo volume for mixed-flow impeller blade
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
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.
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
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.
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: Turbo volume with 3-D boundary layers
2. Select the SPECIFY DISPLAY ATTRIBUTES command button on the Global Control toolpad.
b) Select the Visible:Off option.
c) Click Apply.
d) Click Close to close the Specify Display Attributes form.
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
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.
Figure 10-10: Meshed faces of impeller blade
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
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.
Figure 10-11: Meshed turbo volume for mixed-flow impeller blade
1. Select the EXAMINE MESH command button at the bottom right of the Global Control toolpad.
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.
Figure 10-12: Hexahedral mesh elementsEquiSize Skew = 0.2 - 0.3
Figure 10-13: Pyramidal mesh elementsEquiSize Skew = 0.2 - 0.3
Figure 10-14: Tetrahedral mesh elementsEquiSize Skew = 0.2 - 0.3
2. Display the casing surface in a cascade turbo view.
TOOLS > TURBO > VIEW TURBO VOLUME
b) Click Apply.
Figure 10-15: Casing-surface face mesh elementsEquiSize Skew = 0.1 - 0.6
c) Select the Off option and click Apply to turn off the cascade turbo view before specifying 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.
b) Click Apply.
c) Click Close to close the Specify Display Attributes form.
ZONES > SPECIFY BOUNDARY TYPES
1. Export a mesh file.
File > Export > Mesh...
ii. Click Accept.
File > Exit
b) Click Yes to save the current session and exit GAMBIT.
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).