TM BladePro : An ANSYS-Based Turbine Blade Analysis System Avinash V. Sarlashkar Girish A. Modgil Mark L. Redding Impact Technologies, LLC, Rochester, NY 14623, U.S.A Abstract This paper summarizes the architecture and capabilities of BladePro, an ANSYS based turbine blade analysis system with extensive automation for solid model and F.E. model generation, boundary condition application, file handling and job submission tasks for a variety of complex analyses; the program also includes turbomachinery specific post-processing and life assessment modules. BladePro is a cutting-edge example for vertical applications built on the core ANSYS engine using ANSYS APDL and Tcl/Tk. Examples of how the program makes effective use of the ANSYS preprocessor to mesh complex turbine blade geometries and apply boundary conditions are presented using specific examples. A real world application is used to demonstrate the pre-processing capabilities, static and dynamic stress analyses results, generation of Campbell and Interference diagrams and life assessment. The principal advantage of BladePro is its ability to generate accurate results in a short amount of time, thus reducing the design cycle time. Introduction Over the years, ANSYS has evolved into a very powerful FE-based analysis system to suit a variety of engineering applications in specific areas such as structural and thermal engineering, electro-magnetics, acoustics, computational fluid dynamic analyses, etc. ANSYS has rapidly become one of the most widely used simulation and analysis software. Selection of ANSYS as the core engine for development of vertical application such as BladePro is driven by many of its strengths. Some of the important strengths are: a) robustness and ability in generating and meshing complex geometries driven by parametric inputs, b) "low level" information for the solid and FE model entities available to the end user through APDL calls, c) support for a variety of physics environments, d) continuous development of fast and efficient solvers capable of handling large problems, and e) minimal effort involved in porting an ANSYS vertical application to a variety of hardware / operating system combinations. Ever since the evolution of FEA, there has been a continuous and growing need for a powerful design analysis tool in the power generation industry. In general, turbines represent a class of challenging mechanical prime movers where steady and transient stresses (mechanical and thermal), turbine blade vibrations, and the start/stop cycling of the machines present interesting design challenges to produce a highly reliable machine with long design lives. These design lives may be as long as 20-25 years (150,000 to 200,000 hours of operation) for steam turbines, and as short as 3 years (25,000 hours) for certain components in a gas turbine. Of particular interest is the analysis of turbine blades, as these rotating components, if separated from their attachment to the rotor, have the potential for causing a tremendous amount of consequential damage, both in the form of human life and property damage. BladePro attempts to satisfy this need by using the industry-leading FE analysis platform to provide a menu driven, easy-to- use analysis tool. BladePro has been developed with two very broad areas of interest in mind. 1. Basic Design Analysis: Provide the turbine blade designer with a user-friendly interactive interface that allows for rapid model generation and access to a variety of analyses options in a typical design process for turbine blades. Designers can obtain the magnitude and distribution of static stresses the blade would be subjected to under operating conditions and possibly modify the design at the very nascent stages of the design cycle thereby reducing costs and time delays associated with changes late in the design cycle and in some cases after field testing. 2. Advanced Vibration and Lifing Analysis: These advanced analysis options provide the turbine blade designer with turbomachinery-specific analysis tools required for modal and forced response analyses, contact analysis, post-processing tools such as Campbell and Interference diagrams and Goodman diagrams. All these analyses areas represent essential ingredients in the turbine blade design process to either produce reliable designs or to better understand the cause of failures or to predict the remaining life of an existing design. As the developer of BladePro, Impact Technologies has over 50 years of combined experience in analytical and practical life evaluation, design audits and failure analysis of turbomachinery. Leveraging the ANSYS Architecture The ANSYS architecture is very versatile and quite open in terms of access to low-level information in the ANSYS database. The following specific features of the ANSYS architecture allow for the development of a vertically integrated application such as BladePro that can be tightly integrated with ANSYS and at the same time can be run as a stand-alone application with limited capabilities. 1) Command-line interface to ANSYS. This is the most fundamental ANSYS facility that is key to "driving" ANSYS either through input files, macros or other interfaces such as Tcl/Tk or UIDL. 2) Use of parameters in the form of scalars, arrays, and character strings as arguments to all ANSYS commands. Again, this is another fundamental ANSYS feature allowing the generation of "parametric" models. Although at the present time, the ANSYS solid models are not parametric in a true sense, i.e., the input command sequence needs to be run in its entirety if changes are to be made to even a single dimension in a given model, it offers a very viable approach in generating models very quickly, even on inexpensive PCs. For example, once the BladePro input file is in place, a typical BladePro model generation phase that includes generation of solid model, FE model, and boundary conditions takes typically between 1-3 minutes on a 1000 MHz PC running Windows NT or Windows 2000. 3) Macro facility within ANSYS. Macros are an essential part of producing a vertical application that is highly modularized. For example, BladePro currently incorporates over 300 ANSYS macros. Equally important is the facility within ANSYS to encrypt the macros for distribution within a commercial package such as BladePro. 4) Built-in Tcl/Tk interpreter. This is an extremely important facility that allows rapid development of the graphical user interface (GUI) using the industry-standard Tcl/Tk programming language. It is the use of third-party language that makes possible the stand-alone use of BladePro features that do not depend upon ANSYS enabling the freeing up of an ANSYS license for non-ANSYS features. The versatility of Tcl/Tk combined with the power of APDL, makes it possible to create tools that are capable of automatic generation and analysis of highly complex geometries (such as turbine blades) with minimum user inputs. BladePro: General outline Figure 1 shows a snapshot of the ANSYS GUI with the BladePro button inside the ANSYS Toolbar, and the BladePro main toolbar that is launched after clicking on the BladePro button. The user interacts with the BladePro main menu to a) Enter blade geometry, material properties and associated necessary input defining a turbine stage, b) Define and initiate various analysis options, c) Perform a variety of post- processing operations. Figure 1 - BladePro Main Menu Figure 2 shows a sector model for a typical blade design with an integral shroud. Several different components are labeled. Design-specific features of this blade design are an integral cover (shroud), and a slanted axial entry firtree style root (dovetail attachment). Figure 2 - Blade Components This model was generated using BladePro by entering data directly from an engineering drawing through the BladePro GUI. As shown in figure 1, the main menu contains five menu items described below: File Menu: Used for saving and reading in bpr files (the native BladePro input file). Another feature allows the user to merge data of different components from different bpr files into a single file. Model Input: All the geometry associated with the different components is entered under this menu that contains submenus for cover (shroud), tenon, airfoil, platform, tiewire (mid-span shroud), root and disk data. Stage information such as blade count, speed of rotation, blade grouping, material properties and aerodynamic forcing is also entered here. This menu also contains a comprehensive material database that is used to assign material properties to the different components. Generate Model: Through this menu, the user can generate 2D and 3D models, calculate section properties of individual components and display boundary conditions (BC's). During model generation, BladePro will assign BC's such as couplings, displacement constraints, aerodynamic forcing and master DOF's by either using default (internal) settings or through user input. The information is written out to a free-format file that can be easily edited if the BC's need to be customized for a particular application. Analysis: The FE model generated can be submitted for an analysis. BladePro supports the following types: steady stress, modal analysis, harmonic response, dynamic stress, thermal (steady-state and transient) and a 2D attachment analysis. Analysis options, amongst other things, allow the user to control the type of solver, number of processors, large deformation effects and frequencies of interest for modal analyses. Post-Process: Tools include stress and displacement postprocessing, modeshape animation, Interference diagram, Campbell diagram, Goodman diagram, local-strain fatigue, and 2D attachment analysis postprocessing. These are described later in this paper. Help: Brings up a detailed browser-driven context-sensitive help with keyword search capabilities. In addition to the functionality offered by the BladePro main menu, the user always has the option to use the ANSYS command line to perform any of the standard ANSYS operations. Model Input The input format for a few of the significant components with their related features will be discussed here. Airfoil: Figure 3 shows the airfoil input dialog box. Axial and Tangential points input by the user define the airfoil section geometry. Up to 100 points can be defined for each airfoil section with no restriction on the number of airfoil sections. Airfoil sections can be viewed individually and displayed with section property calculations or multiple sections can be stacked and viewed together. The airfoil template also gives the user the option of interactively adding or deleting airfoil input points. Sections can be scaled, rotated, and translated to allow for rapid analysis screening of design modifications. Airfoil geometry profile can be input either as a series of points in which case a spline is fitted through the points (Figure 3) or by a series of arcs. Figure 3 - Airfoil Input Root: Multiple templates exist for various blade roots. Figure 4 illustrates the dialog boxes and graphical display for the axial entry type. Other root types supported are straddle mount, finger root and T-root. Like the airfoil, the graphical display is interactive and gets updated with changes in root attachment geometry. Element size and number control is provided for mesh refinement or the internal default can be used. Figure 4 - Dovetail Input Disk: Geometry can be defined for symmetric and asymmetric disk profiles. BC's and element divisions can be specified for each input point, or default settings can be used. Figure 5 shows a disk profile defined where the points at the disk bore are constrained in all three directions. Figure 5 - Disk Input Cover/Shroud: Integral shrouds and those attached with tenons can be modeled. Figure 6 (left) illustrates an integral shroud being defined in two different planes (axial-tangential and radial-axial planes). The figure on the right shows a sample mesh for a multiple tenon configuration. The detailed fillet modeling allows for accurate stress prediction in this critical region. Blade-to-blade connectivity information is handled automatically and various blade group configurations can be analyzed. The angle on the airfoil tip (if any) is defined by the radial coordinates of the upstream and downstream points entered in the cover data template. Figure 6 - Shroud Configurations Wheel Configuration: The Wheel Configuration Data dialog box (Figure 7) allows definition of blade-to-blade connections at cover and one or more tie-wires. Connections can be defined only when at least a cover (blue) or a tie-wire (red) is present. Edit fields allow the user to select the start and end blade number. User can select the number of blade groups to define and also the number of blades that are in each group. Figure 7 - Wheel Definition Material Database: BladePro contains a comprehensive material database with mechanical and thermal, fatigue and Goodman material property data sets (Figure 8). The database can be customized to contain user-defined materials and the can be populated from third-party sources. Material properties can be plotted as a function of temperature and each component can be associated with a reference temperature at which material properties will be calculated during model generation and analysis. Figure 8 - Material Database Miscellaneous modeling features: 1. The user has direct control over the mesh refinement at both global and component levels. 2. Scaling, rotation and transformations can be applied at both global and component levels. 3. Both English and SI units can be used. Toggling from one to the other automatically reassigns material properties to the correct system. By providing geometry templates for different components of a blade model, BladePro is able to exploit the solid modeling capabilities of ANSYS. The templates that have been developed using Tcl/Tk take the information from the GUI and write it to the bpr file that is subsequently read in by the macro library to parametrically generate blade components. The macro library makes extensive use of ANSYS boolean capabilities to create highly complex blade geometries with the closest degree of precision. Design Aspects in Turbine Blade Design In this paper, results of analysis for a 15" blade design are presented. This blade represents a typical design for a last stage on a medium-sized gas turbine or a more modern steam turbine. The design uses an axial- entry blade dovetail with three hook pairs. The shroud portion is integral with the blade that is preloaded at assembly. Through the BladePro GUI, the designer can simulate a variety of operating conditions by specifying different boundary conditions and wheel configurations. BladePro makes use of the underlying ANSYS engine to: • Perform Static Stress analysis with the option to incorporate spin softening and stress stiffening effects. • Perform Modal analysis of a cyclic sector or full wheel model. • Assign temperature dependant material properties. • Apply aerodynamic and centrifugal loads. • Simulate large deformation effects for long blades. • Perform harmonic response analysis using modal super-position. A design analysis is usually performed to identify potential resonance conditions during startup and operation and also to check whether static and dynamic stress distributions fall within design limits. If possible, a modal test could be performed on the blade row to determine its standing blade frequencies which can then be compared with frequencies calculated in a zero rpm modal analysis in BladePro (Figure 9). The comparison illustrated in Figure 9 is for a blade geometry similar to the 15" blade design used in this paper as an example. The graph is a plot of normalized frequencies vs. nodal diameters (harmonic numbers). The minimum and maximum percentage differences between theoretical and test results were found to be 0.2% and 4.8% respectively. Once a good correlation is established (up to 5% difference in predicted vs. measured frequencies), the BladePro model can be submitted for at-speed frequency and forced (harmonic) response analyses. As described later in this paper, the results of at-speed frequency and forced response analyses are reviewed using the Campbell and Goodman diagrams. Figure 9 - Correlation of zero rpm modal test with BladePro results BladePro Analysis Options The analysis options offered by BladePro include: 1) Static Analysis. The static analysis of a single-blade sector model or of a blade-group sector model can be performed. The former analysis option would be applicable to designs involving either freestanding or integrally shrouded designs common to gas turbine designs. The latter option is applicable to traditional steam turbine design practice. Loading options include centrifugal and aerodynamic forcing. 2) Modal Analysis. Standing and at-speed frequency calculations (modal analysis) for cyclic, as well as, non-cyclic wheel configurations are available. Modal analysis for the cyclic wheel configurations use the well-established solution techniques where several frequencies and mode shapes are calculated for a given set of nodal diameters (inter-blade phase angles). BladePro also supports modal analysis for wheel configurations that are not cyclic. This situation is more common to the conventional steam turbine design practice where blade groups can be of different lengths and/or certain features such as shrouds and tie-wire may be staggered or overlapping. The three Eigen solution methods for symmetric matrices available within ANSYS (Reduced, Block Lanczos, and Subspace) are all supported by BladePro. The experience gained by Impact Technologies personnel over many years in analyzing a large of variety of turbine blade designs has played a major role in implementing the best modeling techniques for conducting modal analysis of turbine blades. 3) Harmonic Response. Harmonic response analyses for cyclic and non-cyclic wheel configurations are also supported within BladePro. The harmonic response calculation uses the mode superposition method, and therefore, a modal analysis prior to a harmonic response analysis is required. The harmonic response analysis allows the user to "freeze" the response of the turbine blade at a specific phase angle within a single cycle of vibration. This allows for a complete visualization of vibratory or dynamic stress distribution throughout the blade during a complete cycle of vibration. 4) Fatigue Analysis. The fatigue analysis tool calculates fatigue life using the strain-life approach which has been found to be appropriate for situations involving significant plastic deformation due to stress concentration. The user can define low and high cycle fatigue loads. The tool uses techniques such as rain-flow counting method for identifying damaging events and one of two methods (Morrow's or Manson & Halford) to incorporate mean stress effects on fatigue life. A linear damage summation technique is used to sum the damage due to different loading cycles. All the necessary boundary conditions for the variety of analysis options discussed above are generated by BladePro during the model generation phase. Therefore, the user has to provide minimal information to initiate any of the analyses discussed above. For example, as a minimum, initiating a static analysis of a blade sector would involve specifying the shaft speed. Of course, there are additional controls that user can set. Some of the analysis options discussed above provide a "restart" capability wherever applicable to reduce solution times. It should be pointed out that for all analyses options, the user interface allows specification of ANSYS solution controls such as the selection of the ANSYS solver, the number of processors to use on multi-processor shared memory architecture machines, etc. BladePro Performance and Solution Times As far as run times are concerned, a static analysis for a typical BladePro model takes up to 5 minutes on a 1000 MHz PC running Windows NT/2000. We prefer the use of the Sparse Solver within ANSYS which experience has shown to be quite robust. The BladePro GUI does provide access to the frontal solver and the PCG solver. The frontal solver is perhaps the most robust solver within the ANSYS family of solvers, but comes with a penalty of high disk storage requirement for models with wavefronts in excess of 2500. BladePro provides access to Eigen value solutions using all three methods: The Reduced method, the Block Lanczos method (LANB) and the Subspace method. We have typically used the Reduced method and the Block Lanczos method. The Reduced method works well for most models where lower modes of vibration involving low disk participation are of interest. However, more complex modes, especially, with substantial disk participation are better calculated with the Block Lanczos method. The reduced method certainly offers the benefit of lower memory requirement (less than 200 MB for typical BladePro models) than the Block Lanczos method. The memory requirements for the Block Lanczos method can be significantly greater (upto 400 MB for typical BladePro models) when using the cyclic symmetry method. Finally, typical modal analysis runs where up to 20 nodal diameters may be calculated for up to 5 mode families can take up to an hour to calculate on a 1000 MHz PC with two processors running Windows NT/2000. We have found the overall performance of the Intel PC/Windows NT combination to be very acceptable for routine BladePro analyses. Turbomachinery-Specific Postprocessing Tools A typical mechanical design review of a turbine blade design for a fixed-speed machine involves design adequacy checks from a stress view point (static and vibratory stresses) as well as from the view point of placement of operating natural frequencies with respect to the multiples of machine running speed. For variable speed machines, vibratory stresses need to be calculated for all possible resonant conditions over the operating speed range of the machine. The generated vibratory stress information can be analyzed using a Goodman diagram approach as discussed later. Campbell Diagram Change in blade natural frequencies with respect to machine speed are plotted on a Campbell diagram (named after Wilfred Campbell, 1884-1924). Figure 10 shows the Campbell diagram for the 15" turbine blade used as an example. The Campbell diagram in this figure shows intersections of different nodal- diameter modes within each mode family (Axial, Tangential and Twist), with the respective per-rev lines. For blade designs where frequency tuning is a requirement, , the points of mode family/per-rev line intersection will have sufficient margin with respect to the operating speed range. Figure 10 - Campbell diagram for the 15" integrally shrouded blade design.