Accounting for the Stiffness of Three-Dimensional Features in a Two-Dimensional Axisymmetric

Accounting for the Stiffness of Three-Dimensional Features in a Two-Dimensional Axisymmetric Rotating Disk Analysis

by

Kurt E. Leach

A Project Submitted to the Graduate

Faculty of Rensselaer Polytechnic Institute

in Partial Fulfillment of the

Requirements for the degree of

MASTER OF ENGINEERING

IN MECHANICAL ENGINEERING

Approved:

_________________________________________

Ernesto Gutierrez-Miravete, Project Adviser

Rensselaer Polytechnic Institute

Hartford, Connecticut

April, 2012

© Copyright 2012

by

Kurt Leach

All Rights Reserved

CONTENTS

Accounting for the Stiffness of Three-Dimensional Features in a Two-Dimensional Axisymmetric Rotating Disk Analysis 1

LIST OF TABLES 5

LIST OF FIGURES 6

TABLE OF SYMBOLS 7

ACKNOWLEDGMENT 8

ABSTRACT 9

1. Introduction 10

2. Methodology 11

2.1 Description of Problem 11

2.2 Test Variables 11

2.3 Analysis Methodology 13

2.3.1 CAD Model Creation 13

2.3.2 FEA Model Creation 15

2.3.3 Boundary Conditions 17

3. Results and Discussion 19

3.1 Model Validation 19

3.1.1 Two-Dimensional Model 19

3.1.2 Three-Dimensional Model 24

3.2 Two Dimensional Interface Load vs. Three Dimensional Interface Load 25

3.2.1 Interface Load Results 25

3.2.2 General Sensitivities 27

3.3 Accounting for Stiffness Difference in Two-Dimensional Axisymmetric Analysis 29

3.3.1 Plane Strain Elements at Tab 30

3.3.2 Axisymmetric Elements at Tab with Zero Out-of-Plane Modulus 33

3.3.3 Plane Stress Elements with Decrease Axial Modulus at Tab to Reduce Bending Stiffness 33

4. References 34

5. Appendix 36

5.1 Appendix A 36

LIST OF TABLES

Table 2.1 – Test Matrix for Parameter Evaluation 12

Table 3.1 – Force Summations for All Cases 21

Table 3.2 – Summary of Contact Results for 25% Material Removed Case 21

Table 3.3 – Summary of Contact Results for 50% Material Removed Case 22

Table 3.4 – Summary of Contact Results for 25% Material Removed Case 23

Table 3.5 – Interface Loads for 25% Material Removed Case 26

Table 3.6 – Interface Loads for 50% Material Removed Case 26

Table 3.7 – Interface Loads for 75% Material Removed Case 26

Table 3.8 – Interface Load as a Function of Mesh Size 27

Table 3.9 – Interface Load as a Function of Planar Element Type 28

Table 3.10 – Interface Load as a Function of Contact Element Type 29

Table 3.11 -- Interface Loads for 25% Material Removed Case with Plane Strain Elements 32

Table 3.12 – Interface Loads for 50% Material Removed Case with Plane Strain Elements 32

Table 3.13 – Interface Loads for 75% Material Removed Case with Plane Strain Elements 32

LIST OF FIGURES

Figure 2.1 – Sketch Showing the Tab and Slot of a Typical Interrupted Interface 13

Figure 2.2 – General Dimensions of Generic Rotating Disk used for this Study 14

Figure 2.3 – Schematic showing Sector Angle and Tab Thickness 15

Figure 2.4 – Finite Element Mesh used for the Two-Dimensional Analysis 16

Figure 2.5 – Finite Element Mesh used for the Three-Dimensional Analysis (shown is the 50% mat’l removed, 16 tab case) 17

Figure 2.6 – Boundary Conditions to be applied to the Models 18

Figure 3.1 – Free body diagram for the 1st Disk (2D Model – 25% material removed case) 20

Figure 3.2 – Free body diagram for the 2nd Disk (2D Model – 25% material removed case) 20

Figure 3.3 – Plot of Nodal Reaction Forces for All Three Cases 23

Figure 3.4 – 2D vs. 3D Radial Deflections for the 25% Material Removed 64 Tab Case 24

Figure 3.5 – 2D vs. 3D Radial Deflections for the 25% Material Removed 4 Tab Case 25

Figure 3.6 – Radial Deflections for Different Mesh Sizes 28

Figure 3.7 – Screenshot of Finite Element Model showing where Plane Strain Elements are used 30

TABLE OF SYMBOLS

TPS = Thickness applied to Plane Stress with Thickness Element (in)

N = Total Number of Tabs

T = Width of One Tab in Circumferential Direction (in)

R = Net section radius (in)

% = Percent Material Removed to create the Tab

Fcentrif = Centrifugal Load (lbf)

m = mass of disk (lbf-s2/in)

r = radial center of mass (in)

ω = Angular Velocity (rad/s)

Fhoop = Radial Constraining Load due to Circumferential Strains (lbf)

σH = Circumferential Stress (psi)

A = Cross-sectional Area of the Fully Circumferential Section (in2)

Finterface = Force transmitted Between 1st Disk and 2nd Disk due to Contact (lbf)

Fconstraint = Reaction force at Radial Constraint (lbf)

ACKNOWLEDGMENT

Type the text of your acknowledgment here.

ABSTRACT

The analysis of gas turbine engine rotating hardware is extremely important in order to estimate the rotor’s durability as well as other design criteria. The geometric nature of gas turbine engines lend themselves to be easily modeled in a two-dimensional axisymmetric structural finite element model. However, most rotors are not completely axisymmetric. Features such as holes, broach slots, tabs and slots can provide inaccuracies in the axisymmetric model. Here, the effect of tabs on the axisymmetric analysis was evaluated. A typical approach to modeling tabs in a two-dimensional axisymmetric model is to use plane stress with thickness element for the tab. The thickness value used is equivalent to the number of tabs multiplied by the thickness of one tab. The number of tabs and percent of material removed by the tab (metal-to-air ratio in the tab region) were evaluated for a generic representative rotor model. The two-dimensional axisymmetric interface loads were then compared to that of a three-dimensional cyclic symmetric model, which is generally considered to be more correct. Using the plane stress with thickness method, the difference in interface load between the axisymmetric model and the three-dimensional cyclic symmetric model was larger for low count tabs and small for high count tabs. The percent difference was shown to be as high as 30%. Then a number of different techniques were used to try to more accurately capture the true stiffness of the slotted interface. The techniques attempted were, using plane strain elements in the tabbed region, using axisymmetric elements with no out-of-plane stiffness, reducing the axial modulus of the tab to match the three-dimensional model and reducing the axial modulus of the full hoop material adjacent to the tab. These techniques were compared for all cases.

1. Introduction

In the gas turbine industry, both aviation and power generation, the performance and durability of the engine’s components are of the utmost importance. In aviation gas turbines, such as commercial turbofan engines, this attention to component durability is magnified since public safety is in the balance. Therefore, it is essential for any aircraft engine producer to ensure that safety and component durability are at held in high regard. Along with that notion, weight and cost are the biggest drivers toward competitiveness. One of the biggest weight and cost contributors to a turbofan engine are the compressor and turbine rotors. The rotors also pose the highest safety in the case that they fail. With today’s modern advances in finite element analysis, a rotor system for either a turbine or compressor can be modeled to understand the state of stress in each rotating component. With today’s capability, it is impractical to create a full three-dimensional model of a rotor system; therefore, axi-symmetry is taken advantage of for modeling these rotors. However, most rotors have non-axisymmetric features such as holes, tabs, slots, splines, etc. These features are necessary to rotor and engine functionality; however it can be challenging to model these features in a two-dimensional axi-symmetric model. This project will examine the ways that some of the error caused by non-axisymmetric features, specifically tabs, can be reduced.

2. Methodology

2.1 Description of Problem

In two-dimensional rotating disk analyses, three-dimensional out-of-plane features need to be accounted for since almost all rotors are not perfectly axisymmetric. A popular way to account for the out-of-plane features is to use plane stress with thickness element and then apply the appropriate thickness amount to account for the mass of the feature. In the case of tabs, the thickness that is applied is shown by Equation 2.1.

TPS=N*T

Equation 2.1

Where: TPS = Thickness applied to Plane Stress with Thickness Element (in)

N = Total Number of Tabs

T = Width of One Tab in Circumferential Direction (in)

Assuming the same material properties are applied to the plane stress with thickness elements as the axisymmetric elements, then the mass will be accurately captured; however, there will be significant differences in stiffness. For the same metal-to-air ratio in the tab, the same thickness value will be applied regardless of the number of features. In other words, the thickness value applied in the model will be the same whether there are 2 large tabs of 100” thickness with or 100 small tabs of 2” thickness. In each of these instances the stiffness will be different and therefore should be treated differently in the two-dimensional axisymmetric model. Understanding the difference between the plane stress with thickness stiffness and the true stiffness (measured with a three-dimensional cyclic symmetric model) will be an aid to help determine what corrective action to take to account of this stiffness difference in the two-dimensional axisymmetric model.

2.2 Test Variables

The first step in finding a way to correct the stiffness in the two-dimensional axi-symmetric analysis is to understand the variables that contribute to the stiffness difference. A three-dimensional model will be run in order to understand what the true stiffness of the slotted flange should be. Then it will be compared to the two-dimensional representation to evaluate the difference in load transferred through the contact. Here, two variables will be evaluated, the number of tabs and the percent material removed by the slots.

Table 2.1 – Test Matrix for Parameter Evaluation

The equation for percent material removed by the slot is shown in Equation 2.2.

%=1-NT2πR

Equation 2.2

Where: N = Number of Tabs

T = Thickness of One Tab (in)

R = Net section radius (in)

% = Percent Material Removed to create the Tab

The sketch in Figure 2.1 shows the tab thickness defined as well as the slot width for a sector cut of a typical high pressure turbine rotating disk.

Figure 2.1 – Sketch Showing the Tab and Slot of a Typical Interrupted Interface

2.3 Analysis Methodology

2.3.1 CAD Model Creation

First, three-dimensional and two-dimensional solid models must be created in a Computer Aided Design (CAD) software. For this project, NX 6 was be used to create the solid models. To make the model creation easier, the CAD model was built using parametric modeling. By creating a parametric model, the tab thickness and the number of tabs can be defined at a variable, and when the variable changes, the updates propagate through the rest of the model. A sketch of the generic model along with some dimensions is shown in Figure 2.2.

Figure 2.2 – General Dimensions of Generic Rotating Disk used for this Study

For the three-dimensional model, the two-dimensional section was swept in order to create a sector. The sector angle was defined as 360˚ divided by number of tabs modeled. Equation 2.2 can be rearranged in order to come up with an appropriate tab thickness for a given the number of tabs and percent of material removed by the tab. Figure 2.3 shows an example of one of the three-dimensional models that was created along with the sector angle and tab thickness definition.

Figure 2.3 – Schematic showing Sector Angle and Tab Thickness

Using this methodology, all the CAD models necessary to complete the test matrix will be built.

2.3.2 FEA Model Creation

After the two-dimensional sheet bodies and the three-dimensional solid bodies are created the models will be imported in to finite element analysis software. For this project ANSYS will be used as the analysis software. The two-dimensional ANSYS models will be built first.

2.3.2.1 Two-Dimensional Model

The two-dimensional models will be analyzed using PLANE42 elements. The axisymmetric option will be used for the axisymmetric regions of the part, and the plane stress with thickness option will be used to model the tab. The thickness value applied to the plane stress with thickness region will be equal to the number of tabs multiplied by the tab thickness. For the contacts, CONTAC12 node-to-node contact elements will be used. An initial contact stiffness of 1E+10 will be used, and the penetrations and relative sliding will be checked in order to ensure the proper contact behavior. CONTAC12 elements have a significant advantage over 2D surface-to-surface in terms of solution time and convergence probability. A mesh size study will be performed in order to make sure that the loads and deflections are converged as a function of mesh size. The two-dimensional mesh size will then be carried over into the three-dimensional model. Figure 2.4 shows the finite element mesh that will be used for the two-dimensional analysis.

Figure 2.4 – Finite Element Mesh used for the Two-Dimensional Analysis

2.3.2.2 Three-Dimensional Model

The three-dimensional models will be analyzed using SOLID45 elements. The axisymmetric portion of the two disks will be sweep meshed such that each of the symmetry boundaries has a matching mesh. This facilitates the application of cyclic symmetric boundary conditions. The cyclic symmetric boundary condition can be achieved by coupling the nodes on one symmetry boundary with the corresponding nodes on the opposite symmetry boundary in all degrees-of-freedom (radial, axial and circumferential). The contact will be modeled with CONTA174 surface-to-surface contact elements with a contact stiffness of 1E+10. Again, the penetration amounts will be checked in order to ensure that this is an appropriate value. Figure 2.5 shows the finite element mesh that will be used for the 50% percent material removed, 16 tab case.

Figure 2.5 – Finite Element Mesh used for the Three-Dimensional Analysis (shown is the 50% mat’l removed, 16 tab case)

2.3.3 Boundary Conditions

The boundary conditions will be iterated in the two-dimensional axisymmetric model in order to generate a contact load on the order of 100,000 lbs for the full circumference. The 1st Disk will be fixed at the inner diameter in the axial direction and the 2nd Disk will be fixed at the inner diameter in the radial and axial directions. The rotation speed will be iterated in order to come up with a value that meets the load criteria.

Figure 2.6 – Boundary Conditions to be applied to the Models

After some iteration, a value of 12,000 RPM was chosen for the rotational speed. This is on the order of magnitude of the operation of a commercial jet engine high turbine rotor. Also, it provides on the order of 100,000 lbs of interface load which it typical of an HPT rotor interface load.

3. Results and Discussion

3.1 Model Validation

3.1.1 Two-Dimensional Model

3.1.1.1 Free-Body Diagram

In order to validate the model behavior, a free-body diagram was created of both the components. The main loads acting on the two disk are the centrifugal load due to the angular rotation (Fcentrif), the radial constraint due to the circumferential strains (Fhoop), the contact load (Finterface) and the radial constraint (Fconstraint). The centrifugal load due to the angular rotation was approximated by Equation 3.1.