PDF
Thermal-Stress Analysis of a Turbine Stator Blade
Introduction
The conditions within gas turbines are extreme. The pressure can be as high as 40  bars, and the temperature far above 1000 K. Any new component must therefore be carefully designed to be able to withstand thermal stress and vibrations due to the rotating machinery and aerodynamic loads exerted by the fluid rushing through the turbine. If a component fails, the high rotational speeds can result in a complete collapse of the whole turbine.
The most extreme conditions are found in the high pressure section, downstream of the combustion chamber where hot combustion gas flows through a cascade of rotors and stators. To prevent melting, relatively “cold” air is taken from bleeding vanes located in the high-pressure compressor casing; this cold air is then led past the combustion chamber into the turbine casing as coolant. Directly behind the combustion chamber, both internal cooling within ducts, and film cooling over the blade side surfaces are applied. Besides, a surface treatment (coating) is often added to the blades to protect them from hot corrosion. Further downstream, where the temperature is somewhat lower, it may suffice with internal cooling. For more details on gas turbines, see Ref. 1.
Since the physics within a gas turbine is very complex, simplified approaches are often used at the initial stages of the development of new components. In this tutorial, the thermal stresses in a stator blade with internal cooling are analyzed (coating and film cooling are not considered in this example).
Note: This model requires the Structural Mechanics Module and the CFD Module or Heat Transfer Module. It also uses the Material Library.
Model Definition
The model geometry is shown in Figure 1. The stator blade profile is a modified version of a design shown in Ref. 2. The geometry includes some generic mounting details as well as a generic internal cooling duct.
Figure 1: A stator blade with mounting details.
Use the Thermal Stress interface from the Structural Mechanics Module to set up the model. The blade and the mounting details are assumed to be made of the directionally solidified (DS) GTD111 nickel-based alloy with high tensile strength (Ref. 1). This material is available in the COMSOL Material Library. In addition to the data covered by the Material Library, the linear elastic model requires a reference temperature that is set to 310 K and a Poisson’s Ratio that is set to 0.33, a number comparable to that for other stainless steels.
Figure 2 shows the cooling duct. The duct geometry is simplified and does not include details such as the ribs typical for cooling ducts (Ref. 3). Instead of simulating the complicated flow in the duct, an average Nusselt number correlation from Ref. 3 is used to calculate a heat transfer coefficient. Assume the cooling fluid to be air at 30 bar and 650 K.
Figure 2: The internal cooling duct.
The heat flux on the stator blade surfaces is calculated using the heat transfer coefficient. The pressure and suction sides are approximated as two flat plates using the local heat transfer coefficient for external forced convection. The combustion gases are approximated as air at 30 bar and 1150 K. The corresponding speed of sound is approximately 650 m/s.
Ref. 4 contains a Mach number plot of stators without film cooling. A typical Mach number is 0.45 on the pressure side (the concave side) and 0.7 on the suction side (the convex side). This corresponds to approximately 300 m/s on the pressure side and 450 m/s on the suction side.
The platform walls adjacent to the stator blades are treated in the same way as the stator itself but with the free stream velocity set to 350 m/s.
The stator blade exchanges heat with the cooling air through the boundaries highlighted in Figure 3. It is assumed that the turbine has a local working temperature of 900 K, and that the heat transfer coefficient to the stator is 25 W/(m2·K).
Figure 3: Boundaries through which heat is exchanged with the cooling air.
The attachment of the stator element to a ring support is simulated via roller and spring foundation boundary conditions on a few boundaries. All other boundaries are free to deform as a result of thermal expansion.
Results and Discussion
Figure 4 shows a temperature surface plot. The internal cooling creates significant temperature gradients within the blade. However, the trailing edge reaches a temperature close to that of the combustion gases, which indicates that the cooling might be insufficient. The side walls also become very hot, and some additional cooling can be beneficial.
Figure 4: Surface temperature plot.
Figure 5 shows a surface plot of the von Mises stress. The maximum stress does not exceed the yield stress of the material, which indicates that no static failure occurs. However, the component may still be at risk for thermal fatigue, so no definite assessment can be made without conducting a more advanced analysis that includes, for example, creep and other transient effects.
Figure 5: Surface plot of the von Mises stress.
Figure 6: Surface plot of the displacement.
Notes About the COMSOL Implementation
The default suggested solver for a thermal stress analysis assumes that the displacement field and the temperature field are two-way coupled. However, in this example there is only a one-way coupling such that the temperature field is independent of the deformations. In this case, a more efficient solver can be set up where the physics are solved in series. To modify the default solver, set Termination technique to Iterations in the Segregated solver node and make sure that Iterations are set to 1. Moreover, set Termination technique to Tolerance in each Segregated step node. With these modifications, the temperature field is first solved to convergence, before the displacements are solved for.
References
1. M.P. Boyce, Gas Turbine Engineering Handbook, 2nd ed., Gulf Professional Publishing, 2001.
2. NASA, “Power Turbine,” Glenn Research Center, www.grc.nasa.gov/WWW/K-12/airplane/powturb.html.
3. J. Bredberg, “Turbulence Modelling for Internal Cooling of Gas-Turbine Blades,” Thesis for the degree of doctor of philosophy, Chalmers University of Technology, 2002.
4. P. Dahlander, “Source Term Model Approaches to Film Cooling Simulations,” Thesis for the degree of doctor of philosophy, Chalmers University of Technology, 2001.
Application Library path: Structural_Mechanics_Module/Thermal-Structure_Interaction/turbine_stator
Modeling Instructions
Note: Instructions below require to select entities corresponding to a particular numbers list. For example:
Select Boundaries 113 and 139 only.
In most cases the easiest way to select them is to click the Paste Selection button and paste the numbers as they are printed in the document (for example paste “113 and 139” for the example above).
From the File menu, choose New.
New
In the New window, click  Model Wizard.
Model Wizard
1
In the Model Wizard window, click  3D.
2
In the Select Physics tree, select Structural Mechanics > Thermal–Structure Interaction > Thermal Stress, Solid.
3
Click Add.
4
Click  Study.
5
In the Select Study tree, select General Studies > Stationary.
6
Click  Done.
Global Definitions
Parameters 1
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
Click  Load from File.
4
Browse to the model’s Application Libraries folder and double-click the file turbine_stator_parameters.txt.
Geometry 1
Import 1 (imp1)
1
In the Geometry toolbar, click  Import.
2
In the Settings window for Import, locate the Source section.
3
Click  Browse.
4
Browse to the model’s Application Libraries folder and double-click the file turbine_stator.mphbin.
5
Click  Import.
To see the interior:
6
Click the  Transparency button in the Graphics toolbar.
The imported geometry should look as shown in the Figure 1.
7
In the Geometry toolbar, click  Build All.
8
Click the  Zoom Extents button in the Graphics toolbar.
Define a number of selections to simplify the model setup.
Geometry 1
Cleanup Log
1
In the Definitions toolbar, click  Box.
2
In the Geometry Cleanup dialog that opens, click Clean up Automatically to automatically clean up the geometry.
Now, go back to defining selections. First define the internal cooling duct boundaries.
Definitions
Cooling Duct
1
In the Model Builder window, under Component 1 (comp1) > Definitions > Selections click Box 1.
2
In the Settings window for Box, type Cooling Duct in the Label text field.
3
Locate the Geometric Entity Level section. From the Level list, choose Boundary.
4
Locate the Box Limits section. In the x minimum text field, type 0.02.
5
Locate the Output Entities section. From the Include entity if list, choose Entity inside box.
6
Locate the Box Limits section. In the x maximum text field, type 0.17.
7
In the z minimum text field, type 1.04.
8
Click the  Transparency button in the Graphics toolbar.
9
Click the  Wireframe Rendering button in the Graphics toolbar.
The selection is shown in Figure 2.
Proceed to select the boundaries through which the heat exchange with the rest of the turbine occurs (Figure 3).
Exchange Boundaries
1
In the Definitions toolbar, click  Explicit.
2
In the Settings window for Explicit, type Exchange Boundaries in the Label text field.
3
Locate the Input Entities section. From the Geometric entity level list, choose Boundary.
4
Click  Paste Selection.
5
In the Paste Selection dialog, type 1-5, 9, 11, 14, 16, 17, 21-31, 36-39, 42-56, 63, 65-70, 113, 114-134 in the Selection text field.
6
Click OK.
Add Material
1
In the Materials toolbar, click  Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Material Library > Nickel Alloys > GTD111 DS > GTD111 DS [solid] > GTD111 DS [solid,longitudinal].
4
Click the Add to Component button in the window toolbar.
5
In the Materials toolbar, click  Add Material to close the Add Material window.
Materials
GTD111 DS [solid,longitudinal] (mat1)
1
In the Settings window for Material, locate the Material Contents section.
2
In the table, enter the following settings:
Property
Variable
Value
Unit
Property group
Poisson’s ratio
nu
0.33
1
Young’s modulus and Poisson’s ratio
3
In the Model Builder window, expand the GTD111 DS [solid,longitudinal] (mat1) node.
Piecewise (E_solid_longitudinal_1)
1
In the Model Builder window, expand the Component 1 (comp1) > Materials > GTD111 DS [solid,longitudinal] (mat1) > Young’s modulus and Poisson’s ratio (Enu) node, then click Piecewise (E_solid_longitudinal_1).
2
In the Settings window for Piecewise, locate the Definition section.
3
From the Extrapolation list, choose Nearest function.
Multiphysics
Thermal Expansion 1 (te1)
1
In the Model Builder window, under Component 1 (comp1) > Multiphysics click Thermal Expansion 1 (te1).
2
In the Settings window for Thermal Expansion, locate the Model Input section.
3
Click  Go to Source for Volume reference temperature.
Global Definitions
Default Model Inputs
1
In the Model Builder window, under Global Definitions click Default Model Inputs.
2
In the Settings window for Default Model Inputs, locate the Browse Model Inputs section.
3
Find the Expression for remaining selection subsection. In the Volume reference temperature text field, type 310[K].
Heat Transfer in Solids (ht)
Initial Values 1
1
In the Model Builder window, under Component 1 (comp1) > Heat Transfer in Solids (ht) click Initial Values 1.
2
In the Settings window for Initial Values, locate the Initial Values section.
3
In the T text field, type T_gas.
Heat Flux 1
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
In the Settings window for Heat Flux, locate the Boundary Selection section.
3
From the Selection list, choose Exchange Boundaries.
4
Locate the Heat Flux section. From the Flux type list, choose Convective heat flux.
5
In the h text field, type 25.
6
In the Text text field, type T_work.
Heat Flux 2
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
In the Settings window for Heat Flux, locate the Boundary Selection section.
3
From the Selection list, choose Cooling Duct.
4
Locate the Heat Flux section. From the Flux type list, choose Convective heat flux.
5
In the h text field, type Nu_cool*mu_cool*Cp_cool/2/Pr_cool/H_cool.
6
In the Text text field, type T_cool.
Heat Flux 3
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
Select Boundary 41 only.
3
In the Settings window for Heat Flux, locate the Heat Flux section.
4
From the Flux type list, choose Convective heat flux.
5
From the Heat transfer coefficient list, choose External forced convection.
6
From the list, choose Plate, local transfer coefficient.
7
In the xpl text field, type 0.1675-x.
8
In the U text field, type U_suction_side.
9
In the pA text field, type p_high.
10
In the Text text field, type T_gas.
Heat Flux 4
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
Select Boundary 40 only.
3
In the Settings window for Heat Flux, locate the Heat Flux section.
4
From the Flux type list, choose Convective heat flux.
5
From the Heat transfer coefficient list, choose External forced convection.
6
From the list, choose Plate, local transfer coefficient.
7
In the xpl text field, type 0.1675-x.
8
In the U text field, type U_pressure_side.
9
In the pA text field, type p_high.
10
In the Text text field, type T_gas.
Heat Flux 5
1
In the Physics toolbar, click  Boundaries and choose Heat Flux.
2
Select Boundaries 10, 15, and 32–35 only.
3
In the Settings window for Heat Flux, locate the Heat Flux section.
4
From the Flux type list, choose Convective heat flux.
5
From the Heat transfer coefficient list, choose External forced convection.
6
From the list, choose Plate, local transfer coefficient.
7
In the xpl text field, type 0.19-x.
8
In the U text field, type U_platform.
9
In the pA text field, type p_high.
10
In the Text text field, type T_gas.
Solid Mechanics (solid)
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
Spring Foundation 1
1
In the Physics toolbar, click  Boundaries and choose Spring Foundation.
2
Select Boundaries 42, 43, 54, 127, and 129 only.
3
In the Settings window for Spring Foundation, locate the Spring section.
4
From the list, choose Diagonal.
5
Specify the kA matrix as
1e9
0
0
0
0
0
0
0
0
Spring Foundation 2
1
In the Physics toolbar, click  Boundaries and choose Spring Foundation.
2
Select Boundaries 27, 29, 51, and 68 only.
3
In the Settings window for Spring Foundation, locate the Spring section.
4
From the list, choose Diagonal.
5
Specify the kA matrix as
0
0
0
0
0
0
0
0
1e9
Spring Foundation 3
1
In the Physics toolbar, click  Boundaries and choose Spring Foundation.
2
Select Boundaries 6 and 12 only.
3
In the Settings window for Spring Foundation, locate the Spring section.
4
From the list, choose Diagonal.
5
Specify the kA matrix as
0
0
0
0
1e9
0
0
0
0
Mesh 1
Size 1
In the Model Builder window, under Component 1 (comp1) right-click Mesh 1 and choose Size.
Size
1
In the Settings window for Size, locate the Element Size section.
2
Click the Custom button.
3
Locate the Element Size Parameters section. In the Maximum element size text field, type 0.025.
4
In the Minimum element size text field, type 0.0025.
5
In the Maximum element growth rate text field, type 2.
6
In the Curvature factor text field, type 0.75.
Size 1
1
In the Model Builder window, click Size 1.
2
In the Settings window for Size, locate the Geometric Entity Selection section.
3
From the Geometric entity level list, choose Boundary.
4
From the Selection list, choose Exchange Boundaries.
Also add boundaries 40 and 41 to the selection.
5
Locate the Element Size section. Click the Custom button.
6
Locate the Element Size Parameters section.
7
Select the Maximum element size checkbox. In the associated text field, type 0.0035.
8
Select the Maximum element growth rate checkbox. In the associated text field, type 1.1.
Free Tetrahedral 1
1
In the Mesh toolbar, click  Free Tetrahedral.
2
In the Settings window for Free Tetrahedral, click  Build All.
Study 1
Heat Transfer in Solids and Solid Mechanics are in this model one-way coupled. This allows the physics to be solved in series, which is more efficient than the suggested default solver.
Solution 1 (sol1)
1
In the Study toolbar, click  Show Default Solver.
2
In the Model Builder window, expand the Solution 1 (sol1) node.
3
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 node, then click Segregated 1.
4
In the Settings window for Segregated, locate the General section.
5
From the Termination technique list, choose Iterations.
6
In the Model Builder window, expand the Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 > Segregated 1 node, then click Temperature.
7
In the Settings window for Segregated Step, click to expand the Method and Termination section.
8
From the Termination technique list, choose Tolerance.
9
In the Tolerance factor text field, type 1.
10
In the Model Builder window, under Study 1 > Solver Configurations > Solution 1 (sol1) > Stationary Solver 1 > Segregated 1 click Solid Mechanics.
11
In the Settings window for Segregated Step, locate the Method and Termination section.
12
From the Termination technique list, choose Tolerance.
13
In the Tolerance factor text field, type 1.
14
In the Study toolbar, click  Compute.
Results
Stress (solid)
The first default plot shows the von Mises stress. Disable the deformation and create a max/min marker to identify the critical point in the stator.
Volume 1
1
In the Model Builder window, expand the Stress (solid) node, then click Volume 1.
2
In the Settings window for Volume, locate the Expression section.
3
From the Unit list, choose MPa.
Deformation
1
In the Model Builder window, expand the Volume 1 node.
2
Right-click Deformation and choose Disable.
Marker 1
1
In the Model Builder window, right-click Volume 1 and choose Marker.
2
In the Settings window for Marker, locate the Display section.
3
From the Display list, choose Max.
4
Locate the Text Format section. In the Precision text field, type 3.
5
Locate the Coloring and Style section. From the Background color list, choose From theme.
6
Select the Show frame checkbox.
Transparency 1
1
Right-click Volume 1 and choose Transparency.
2
In the Settings window for Transparency, locate the Transparency section.
3
Find the Transparency subsection. In the Transparency text field, type 0.2.
4
Find the Fresnel transmittance subsection. In the Fresnel transmittance text field, type 0.5.
5
In the Stress (solid) toolbar, click  Plot.
The second default plot shows the temperature distribution Figure 4.
Temperature (ht)
1
In the Model Builder window, under Results click Temperature (ht).
2
In the Settings window for 3D Plot Group, locate the Plot Settings section.
3
Clear the Plot dataset edges checkbox.
Transparency 1
1
In the Model Builder window, expand the Temperature (ht) node.
2
Right-click Volume 1 and choose Transparency.
3
In the Settings window for Transparency, locate the Transparency section.
4
Find the Transparency subsection. In the Transparency text field, type 0.2.
5
Find the Fresnel transmittance subsection. In the Fresnel transmittance text field, type 0.5.
6
In the Temperature (ht) toolbar, click  Plot.
7
Click the  Zoom Extents button in the Graphics toolbar.
Finally, plot the displacement (Figure 6).
Displacement
1
In the Results toolbar, click  3D Plot Group.
2
In the Settings window for 3D Plot Group, type Displacement in the Label text field.
Surface 1
1
Right-click Displacement and choose Surface.
2
In the Settings window for Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1 (comp1) > Solid Mechanics > Displacement > solid.disp - Displacement magnitude - m.
3
Locate the Expression section. From the Unit list, choose mm.
4
Locate the Coloring and Style section. From the Color table list, choose SpectrumLight.
5
In the Displacement toolbar, click  Plot.
6
Click the  Zoom Extents button in the Graphics toolbar.