You are viewing the documentation for an older COMSOL version. The latest version is available here.
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, 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 rupture of the whole turbine.
The most extreme conditions are found in the high pressure part downstream of the combustion chamber where hot combustion gas flows through a cascade of rotors and stators. To prevent the parts from melting, relatively “cold” air is taken from bleeding vanes located in the high-pressure compressor casing, then led past the combustion chamber into the turbine casing in order to be used as a coolant. Directly behind the combustion chamber, both internal cooling within ducts and film cooling over the blade side surfaces are applied. 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 initial stages of the development of the new components. In this tutorial, the thermal stresses in a stator blade with internal cooling are analyzed.
Note: This application 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 model 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 M-152 alloy which is a 12 Cr alloy with high tensile strength (Ref. 1). M-152 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 300 K and a Poisson’s Ratio that is set to 0.33, a number comparable to that for other stainless steels. Any coating has been neglected.
Figure 2 shows the cooling duct. The duct geometry is simplified and does not include details such as the ribs (Ref. 3) typical for cooling ducts. 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 600 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 1100 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 0.7 on the pressure side (the concave side) and 0.45 on the suction side (the convex side). This corresponds to approximately 450 m/s on the pressure side and 300 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 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 with a value close to the yield stress for the material (Ref. 5) occurs in the internal cooling duct. No definite assessment can however be made without conducting a more advanced analysis that includes details of the flow inside the duct.
Figure 5: Surface plot of the von Mises stress.
Figure 6: Surface plot of the displacement.
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.
5.  http://www.cnalloys.co.uk/stainless-jethete-m152
Application Library path: Heat_Transfer_Module/Thermal_Stress/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 Stress.
3
Click Add.
4
Click Study.
5
In the Select Study tree, select General Studies>Stationary.
6
Click Done.
Global Definitions
1
In the Model Builder window, under Global Definitions click Parameters 1.
2
In the Settings window for Parameters, locate the Parameters section.
3
In the table, enter the following settings:
Name
Expression
Value
Description
Pr_cool
0.72
0.72
Cooling Prandtl number
U_suction_side
450[m/s]
450 m/s
Gas velocity on stator suction side
U_pressure_side
300[m/s]
300 m/s
Gas velocity on stator pressure side
U_platform
350[m/s]
350 m/s
Gas velocity along platform walls
T_gas
1100[K]
1100 K
Gas temperature
p_high
30[bar]
3E6 Pa
High pressure level
mu_cool
3.1e-5[Pa*s]
3.1E-5 Pa·s
Viscosity of the cooling air
Cp_cool
770[J/kg/K]
770 J/(kg·K)
Heat capacity of the cooling air
T_cool
800[K]
800 K
Cooling air temperature
H_cool
0.01[m]
0.01 m
Characteristic length scale of cooling channels
T_work
900[K]
900 K
Working temperature
Nu_cool
400
400
Average Nusselt number in cooling channel
Geometry 1
Import 1 (imp1)
1
In the Home toolbar, click Import.
2
In the Settings window for Import, locate the Import 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 Home toolbar, click Build All.
8
Click the Zoom Extents button in the Graphics toolbar.
Definitions
Define a number of sections to simplify the model setup. First define the internal cooling duct boundaries.
Explicit 1
1
In the Definitions toolbar, click Explicit.
2
In the Settings window for Explicit, type Cooling_Duct 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 box, type 222-225, 236, 261-266, 270-271, 278-279, 283-285, 292-305, 308-311, 313-314, 316, 321 in the Selection text field.
If you are reading an electronic version of this document, you can copy the geometric entity numbers from the text.
6
Click OK.
7
Click the Transparency button in the Graphics toolbar.
8
Click the Wireframe Rendering button in the Graphics toolbar.
The selection is shown in Figure 2.
Proceed to select the boundaries through which heat exchanger with the rest of turbine occur Figure 3.
Explicit 2
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 box, type 3-4, 9, 12, 14, 16, 19-20, 22-24, 28-96, 98-117, 122-135, 138-162, 166-221, 223, 226-231, 239-260, 267-269, 272-277, 280-282, 322-444 in the Selection text field.
6
Click OK.
Add Material
1
In the Home toolbar, click Add Material to open the Add Material window.
2
Go to the Add Material window.
3
In the tree, select Material Library>Iron Alloys>JETHETE M-152 or Moly Ascoloy>JETHETE M-152 or Moly Ascoloy [solid].
4
Click Add to Component in the window toolbar.
5
In the Home toolbar, click Add Material to close the Add Material window.
Materials
JETHETE M-152 or Moly Ascoloy [solid] (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
Solid Mechanics (solid)
1
In the Model Builder window, under Component 1 (comp1) click Solid Mechanics (solid).
2
In the Settings window for Solid Mechanics, click to expand the Discretization section.
3
From the Displacement field list, choose Linear.
Multiphysics
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.
Global Definitions
Common Model Inputs
1
In the Model Builder window, under Global Definitions click Common Model Inputs.
2
In the Settings window for Common Model Inputs, locate the Browse Model Inputs section.
3
Find the Expression for remaining selection subsection. In the Volume reference temperature text field, type 300[K].
Heat Transfer in Solids (ht)
In the Physics toolbar, click Solid Mechanics (solid) and choose 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, type T_gas in the T text field.
3
In the Model Builder window, click Heat Transfer in Solids (ht).
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. Click the Convective heat flux button.
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. Click the Convective heat flux button.
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 Boundaries 137 and 163 only.
3
In the Settings window for Heat Flux, locate the Heat Flux section.
4
Click the Convective heat flux button.
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 Boundaries 136 and 312 only.
3
In the Settings window for Heat Flux, locate the Heat Flux section.
4
Click the Convective heat flux button.
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 15, 21, 118–121, 164, 165, 232, 234, 235, 237, 286, 289–291, 306, 307, 315, 317, and 320 only.
3
In the Settings window for Heat Flux, locate the Heat Flux section.
4
Click the Convective heat flux button.
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).
Roller 1
1
In the Physics toolbar, click Boundaries and choose Roller.
2
Select Boundaries 140, 146, and 213 only.
Spring Foundation 1
1
In the Physics toolbar, click Boundaries and choose Spring Foundation.
2
Select Boundaries 426 and 428 only.
3
In the Settings window for Spring Foundation, locate the Spring section.
4
From the list, choose Diagonal.
5
In the kA table, enter the following settings:
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 82, 90, 192, and 255 only.
3
In the Settings window for Spring Foundation, locate the Spring section.
4
From the list, choose Diagonal.
5
In the kA table, enter the following settings:
0
0
0
0
0
0
0
0
1e10
Spring Foundation 3
1
In the Physics toolbar, click Boundaries and choose Spring Foundation.
2
Select Boundary 17 only.
3
In the Settings window for Spring Foundation, locate the Spring section.
4
From the list, choose Diagonal.
5
In the kA table, enter the following settings:
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.
2
In the Settings window for Size, locate the Element Size section.
3
From the Predefined list, choose Fine.
Size 1
1
In the Model Builder window, under Component 1 (comp1)>Mesh 1 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 Cooling_Duct.
5
Locate the Element Size section. From the Predefined list, choose Fine.
Free Tetrahedral 1
1
In the Model Builder window, right-click Mesh 1 and choose Free Tetrahedral.
2
Click Build All.
Study 1
In the Home toolbar, click Compute.
Results
Stress (solid)
The first default plot show the von Mises stress. Disable the deformation and create a max/min plot to display the critical point in the stator.
Surface 1
In the Model Builder window, expand the Stress (solid) node.
Deformation
1
In the Model Builder window, expand the Surface 1 node.
2
Right-click Deformation and choose Disable.
Max/Min Surface 1
1
In the Stress (solid) toolbar, click More Plots and choose Max/Min Surface.
2
In the Settings window for Max/Min Surface, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1>Solid Mechanics>Stress>solid.mises - von Mises stress - N/m².
3
In the Stress (solid) toolbar, click Plot.
Table
1
Go to the Table window.
2
Click the Zoom Extents button in the Graphics toolbar.
3
Click the Transparency button in the Graphics toolbar.
The second default plot shows the temperature distribution Figure 4.
Results
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 data set edges check box.
4
In the Temperature (ht) toolbar, click Plot.
5
Click the Zoom Extents button in the Graphics toolbar.
Finally, plot the total displacement (Figure 6).
Volume 1
1
In the Home toolbar, click Add Plot Group and choose 3D Plot Group.
2
In the Model Builder window, right-click 3D Plot Group 4 and choose Volume.
3
In the Settings window for Volume, click Replace Expression in the upper-right corner of the Expression section. From the menu, choose Component 1>Solid Mechanics>Displacement>solid.disp - Total displacement - m.
4
Locate the Expression section. From the Unit list, choose mm.
5
In the 3D Plot Group 4 toolbar, click Plot.
6
Click the Zoom Extents button in the Graphics toolbar.