DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE NOZZLE USING 3D CRACK MESHES

Size: px
Start display at page:

Download "DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE NOZZLE USING 3D CRACK MESHES"

Transcription

1 DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE Greg Thorwald, Ph.D. Principal Consulting Engineer, Quest Integrity Group, USA Michael Rock Engineering Project Manager, Mighty River Power Limited, New Zealand THEME Durability, Fatigue & Fracture KEYWORDS Ductile tearing, crack stability, 3D crack mesh, J-integral, J-R diagram, J-T diagram, fracture mechanics, finite element analysis, FEACrack, Warp3D SUMMARY A ductile tearing analysis of a postulated crack is analyzed to evaluate crack stability and determine the critical crack length. The through-thickness circumferential crack is located in the pipe-to-flange connection in a mixing tee piping component in a geothermal power plant. The pipe-to-flange geometry has an overall cylindrical shape with a 90-degree corner between the pipe and the flange at the outer fillet weld. High stresses are expected at that location, which could initiate a crack and cause it to grow. Material testing data available from another recent project is used to improve this analysis. Twelve 3D crack meshes are generated for a range of crack lengths from short to long, and are used to compute the crack front J-integral values by elastic-plastic finite element analysis. An automated crack mesh generation software is used to reduce the time and effort needed to generate all the crack mesh input files. Many crack meshes are needed to provide enough data points on the applied J result curve to compute an accurate J derivative by simple differences or a polynomial curve-fit. The crack front J values and the material J-R resistance curve are used to compute the tearing modulus and obtain the J-T diagram. The crack ductile instability point is evaluated on the J-T diagram to obtain a critical J value. The critical J value is then used to obtain the critical crack length. The initial crack length to cause the unstable tearing is obtained by shifting the J-R material curve until the tangent instability point intersects with

2 the applied J results curve, and indicates the amount of stable ductile tearing before failure. Compared with using a single toughness value, the ductile tearing analysis takes advantage of stable tearing and the higher J-R resistance values, giving a longer critical crack length, which may be beneficial in deciding upon a course of action for inspecting, maintaining, or repairing a damaged component. 1: INTRODUCTION A ductile tearing analysis is used to examine a postulated circumferential through-thickness crack at the pipe-to-flange fillet weld connection in a piping mixing tee component. The goal of the analysis is to compute the critical crack length that would cause unstable crack growth and structural failure in this piping component. Material testing data is available from a recent analysis of another section of the pipe and is used to improve this analysis (Rowson, 2010). Other items needed for the ductile tearing analysis include the fracture mechanics theory and equations describing ductile crack stability (Anderson, 2005), a 3D crack mesh generator such as FEACrack (Quest Integrity, 2010) to quickly create the finite element analysis (FEA) input files of the pipe-to-flange model, and a non-linear FEA solver with the J-integral calculation such as Warp3D available in the public domain from the University of Illinois (Dodds, et al, 2009). 2: MIXING TEE PIPING COMPONENT The mixing tee is a piping component in the Mighty River Power Rotokawa geothermal power plant (Figure 1). The Rotokawa geothermal field is located in the Taupo Volcanic Zone in New Zealand, roughly 13km northeast of Taupo Township. This resource is a high temperature geothermal field with down hole temperatures of up to 320 C. Rotokawa Geothermal Power Station generates 33 MW and is one of two electricity generating power stations on this field. It is a combined cycle plant with a back pressure topping steam turbine and binary Organic Rankine Cycle bottoming and brine units. Twophase geothermal fluid is piped from the production wells to a centrifugal type separator where the steam and brine phases are separated. The steam phase is used to power the turbine (and subsequently the bottoming units). The brine phase is piped directly to a separate brine binary unit. The cooled brine is then mixed with the condensed steam from the bottoming units. The resultant fluid is then injected back into the ground. Under normal operation, all of the separated brine passes through the brine unit. Under some circumstances, some hot brine bypasses the binary unit and is mixed with the cooled brine. A mix tee is installed where the two fluids combine. The mix tee s purpose is to control how the fluids are mixed so that the likelihood of steam condensation induced water hammer is reduced.

3 Crack location Flow Out: Mixed Brine Flow In: Cooled Brine Region for FEA model Pipe: 250 NPS x 9.27 ASTM A53 Gr B steel Flow In: Bypass Hot Brine Figure 1: Crack located at the pipe-to-flange connection in the mixing tee. The pipe is 250 NPS x 9.27 (Nominal Pipe Size), which has an outside diameter of mm, and a 9.27 mm thickness. The pipe is made of ASTM A53 Gr B steel. The recent material tests give the yield strength of 325 MPa, a tensile strength of 463 MPa, and a modulus of elasticity of 162 GPa at the operating temperature of 230 o C. The pipe is designed for 32 bar internal pressure (3.2 MPa), including additional loads on the pipe of 67 kn axial force and 24.3 MN-mm bending moment. The circular flange plate is 50 mm thick with a 560 mm outside diameter, and is made of AS R steel (similar to ASTM A662 Gr B). The flange material was not tested, so the minimum specified values are used for the yield strength of 119 MPa, tensile strength of 198 MPa, and modulus of elasticity of 190 GPa. The pipe is connected to the flange by internal and external circumferential fillet welds. Since the connection forms a square corner, higher stresses are expected near the outer fillet weld, which could cause a crack to initiate and grow. 3: CRACK MESHES Stress intensity or J values are generally known only for cracks in standard geometric shapes like plates, cylinders, and spheres. To account for the pipeto-flange geometry in the ductile tearing analysis, custom 3D crack meshes are needed. The crack meshes for this analysis includes the pipe and flange on the left side of the mixing tee. The crack meshes are half symmetric with appropriate symmetry constraints, internal pressure, crack face pressure, and axial loads. Weld residual stress was not included in this analysis to keep the example concise, but could be included if desired (Thorwald, 2008).

4 The user-defined geometry method in the FEACrack software is used with a definition mesh to quickly generate the needed crack meshes. The definition mesh describes the desired pipe-to-flange geometry as a general 6-sided volume, and the elements within the definition mesh are used to transform the crack mesh primitive into the final shape (Thorwald, 2006), (Figure 2). Since the definition mesh is used only to create the analysis crack mesh, refinement is needed only along surface curvatures, such as around the circumference for this model. A single element is sufficient across the flange or along the pipe to describe the flat surface geometry in those regions. Use many elements to capture surface curvature around circumference Flange: 560 mm OD 50 mm thickness Pipe: 250 NPS x 9.27 Single element is sufficient if no surface curvature Figure 2: Definition mesh for the pipe-to-flange pipe geometry. The pipe-to-flange 3D crack meshes are shown with color-coded mesh zones, which are used to help adjust the mesh refinement near the crack (Figure 3). The circumferential crack is located in the pipe at the toe of the fillet weld. The crack front uses the typical focused mesh pattern needed to support the J- integral contour calculations. A ductile tearing analysis reveals some of the typical crack meshing challenges: needing many crack meshes, putting the crack into the component geometry, creating the focused mesh at the crack front, and post processing and tabulating the numerous crack front results. Using automated crack mesh generation software reduces the modelling effort. Twelve pipe-to-flange crack meshes were generated with crack lengths from 25 mm to 275 mm. The crack meshes use 20-node brick elements. Hiding the pipe region gives a cut-away view that reveals the crack plane and crack front location in the mesh (Figure 4). The half-symmetric model

5 includes half of the through-thickness crack length, measured around the circumference on the pipe outside diameter. The mesh zone sizes near the crack plane were adjusted to follow the fillet welds and give a mesh line at the weld-to-flange junction. Fix x DOF Symmetry plane, fix y DOF Pressure, axial loads Crack tip focused mesh Figure 3: Views of the through-thickness 3D crack mesh and a close-up of the crack tip focused mesh. Flange Half crack length, c Ligament Symmetry plane Crack front Figure 4: Crack plane in the pipe (light blue) Remove the pipe to view the through-thickness crack plane. 4: FEA RESULTS The FEA results show that the flange plate stiffens the end of the pipe and the crack has opening and shearing displacement (Figure 5). The color scale bar

6 upper limit has been set to the yield strength of 325 MPa to show the high stress region at the toe of the fillet weld at the maximum loading. The elasticplastic FEA used 20 analysis steps with equal increments to increase the applied loading to its maximum value, and for equilibrium convergence. A comparison analysis of the pipe alone with a through-thickness crack shows the crack opening, but does not have the shear displacement (Figure 6), which helps to understand the effect of the flange plate. The pipe-only models use quarter symmetric cylinder through-thickness crack meshes with the same pipe dimensions, materials, and loads. YS = 325 MPa Crack opening and shear displacement 5x displacement scale Figure 5: Pipe-to-flange Warp3D Von Mises stress results, 2c = 100 mm case. Symmetry YS = 325 MPa Crack opening displacement Symmetry 5x displacement scale Figure 6: Cylinder model Warp3D Von Mises stress results, 2c = 100 mm. The left plot in Figure 7 shows the crack front J values versus the distance through the pipe thickness (from the pipe outside diameter through the

7 Crack front J-integral (N/mm) Max crack front J-integral (N/mm) DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE thickness to the inside diameter) in the pipe-to-flange model at the maximum load. The right plot in Figure 7 shows the maximum crack front J values versus the half crack length, c, and compares the pipe-to-flange results with the cylinder results. Each data point is from a crack mesh FEA at the given crack length. The higher stress at the pipe-to-flange connections appears to increase the crack front J values for shorter cracks compared with the cylinder model. The extra stiffness from the flange appears to reduce the crack front J values by limiting the displacement of the back crack face at the longer crack lengths compared with the pipe-only cylinder model Pipe to flange through crack, J results, step J results: pipe to flange and cylinder cylinder c = 275 mm 2c = 25 mm pipe OD distance through thickness (mm) pipe ID J versus distance through the pipe wall thickness Pipe to flange c, half crack length (mm) pipe to flange, max J (N/mm), step 20 cylinder, max J (N/mm), step 20 Max J versus half crack length, c Figure 7: Crack front J-integral results for a range of crack lengths. 5: TEARING RESISTANCE The material testing data provides the J-R resistance curve for the ASTM A53 pipe material (Figure 8). The data points between the exclusion lines are curve-fit to a power-law equation with coefficients C 1 and C 2, Equation (1), (Anderson, pp ). The crack length difference (a-a 0 ) gives the crack extension in the specimen from an initial crack length a 0 during the testing. J R C C2 a a 174. a a (1) The J 1C value on the J-R plot indicates the nominal material toughness of 93.4 N/mm. The single toughness value could be used in a linear elastic fracture mechanics (LEFM) evaluation to obtain a critical crack size. The tearing modulus, T, is a non-dimensional value computed using the modulus of elasticity, E, yield stress, 0, and the derivative of a J curve, Equation (2). The tearing modulus is computed for both the material resistance and crack front curves.

8 J-Integral (N/mm) DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE E T 2 0 dj da (2) The tearing resistance, T R, from the J-R material curve, is computed using a chain-rule derivative of the power-law equation to get T R in terms of J R and the curve-fit exponent, Equation (3). T R E C J 2 R 2 0 a a0 (3) J-Integral Tearing Resistence Curve Test result for ASTM A53 ASTM E1820 Standard y = x J 1C =93.4 N/mm Crack extension, delta a (mm) Test Data Construction Line 0.15mm Exclusion line 0.2mm Offset line 1.5mm Exclusion line Data within exclusion lines (for trend line) J1C, intersection of 0.2 offset and tend line Power law within exclusion lines Figure 8: J-R material testing results for the pipe ASTM A53 Gr B material. The applied tearing modulus, T app, from the crack front J versus crack length results is computed using either simple differences, J/ c, or a polynomial curve-fit to compute the derivative of J. The 5 th order polynomial curve-fit of the J results in the left plot in Figure 9 provides an easy to compute J derivative, Equation (4), for comparison to the differences (the exponent values have been left as constants in each term to indicate the derivative calculation). dj app dc *7.52E 8 c 4* 2.28E 5 c 3* 2.82E 3 c 2*0.162 c (4) In either approach, sufficient data points are needed for accurate derivative values. More crack meshes at various lengths can be added as needed to provide more data points. The same modulus and yield stress values (from the pipe) in both tearing modulus calculations are used for consistency.

9 Tearing modulus Max crack front J-integral (N/mm) Max crack front J-integral (N/mm) DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE The T R and T app tearing modulus curves are plotted together to get the J-T diagram (Figure 10). A crack length is stable for a tearing modulus value below the T R tearing resistance curve, and unstable above the T R curve. Typically the T app curve will intersect with the T R curve, and the J-T diagram is convenient to identify the intersection at the ductile instability. However, the pipe material test specimen was sub-size, which gives a limited range of values in the T R curve. The extrapolated T R curve (green dashed line) is shown only to suggest where the curves might eventually intersect if more data were available. Since the tearing modulus curves do not intersect, the maximum available material J-R value of 262 N/mm is used as the critical J to determine the critical crack length, since using extrapolated J-R material values may be unreliable Pipe to flange in the mixing tee J results y = 7.52E-08x E-05x E-03x E-01x E+00x R² = 1.00E c, half crack length (mm) pipe to flange, max J (N/mm), step 20 Poly. (pipe to flange, max J (N/mm), step 20) Pipe flange: 5 th order polynomial curve-fit Cylinder through-thickness crack y = 2.56E-05x E-03x E-01x E+00x R² = 9.99E c, half crack length (mm) cylinder, max J (N/mm), step 20 Poly. (cylinder, max J (N/mm), step 20) Cylinder: 4 th order polynomial curve-fit Figure 9: Use polynomial curve-fit to the J versus crack length plots J 1C Tearing modulus, pipe to flange model and cylinder T R ASTM A53 extrapolated J = 262 cylinder pipe to flange J-integral (N/mm) T_R for ASTM A53 pipe T_app pipe to flange, differences T_app cylinder, differences T_R extrapolation using cuve-fit T_app pipe to flange, curve-fit T_app cylinder, curve-fit Figure 10: Look for intersection of T R and T app tearing modulus curves to get the critical J at ductile instability; curves do not intersect in the available data range.

10 Max crack front J-integral (N/mm) 2c total crack length (mm) DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE The applied tearing modulus curves in Figure 10 are computed using both the simple differences and the polynomial curve-fit for comparison. There is close agreement between the two approaches for most of the curve. Additional data points at the higher J values may improve the agreement for the higher J values by generating more crack meshes. The left plot in Figure 11 shows where the critical J max from the J-T diagram intersects with the pipe-to-flange and cylinder J curves. Interpolation gives the pipe-to-flange through-thickness critical crack length of 211 mm. Coincidentally, the pipe-only cylinder model critical crack size is nearly the same when using the J max value. The J result trends in Figure 11 show that for a different critical J material value, the cylinder and pipe-to-flange models would give different critical crack lengths. 300 Interpolate for critical crack size at given J 2c = 211 mm 225 Critical crack length, 2c 250 J max Pipe to flange J 1C Cylinder c, half crack length (mm) pipe to flange, max J cylinder, max J J1C toughness J-R max value c 25 0 pipe to flange cylinder J1C toughness J-R Jmax Figure 11: Use the critical J value to interpolate the critical crack length. If the J 1C single toughness value were used, the critical crack length for the pipe-to-flange model would be 77 mm. The extra effort of a ductile tearing analysis takes advantage of the higher material J-R value at the ductile instability, and gives a larger critical crack size. Knowing these critical crack lengths may help a client decide on a safe but not overly conservative course of action to inspect, maintain, or repair a damaged component. The initial critical crack length, 2c 0, to initiate the unstable ductile tearing is obtained by shifting the material J-R curve on the J versus crack length plot until the tangent instability point just meets the analysis J results curve (Figure 12). With the limited J-R data available, the tangent instability point is approximated by the maximum J-R value. The critical initial crack length 2c 0 is 206 mm, which allows for 5 mm of stable ductile crack growth until the

11 J_app and J_R (N/mm) DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE crack length reaches the ductile instability point and the component is predicted to fail Pipe to flange through-crack, find initial c 0 Approximate tangent instability point pipe to flange max J 2c 0 = 206 mm Pipe to flange c, half crack length (mm) J-R ASTM A53 J-R ASTM A53 data Figure 12: Adjust the initial critical crack length to shift the J-R curve so the tangent instability point meets the applied J results curve. Another consideration is the possible yield rupture failure as the crack length increases. The increasing crack length is reducing the available pipe crosssection to carry the load, which could also cause the component to fail. The limit load calculation is not included in this analysis to keep the example concise. 6: CONCLUSION A postulated circumferential through-thickness crack in the pipe-to-flange connection in the mixing tee was examined using a ductile tearing analysis, and compared with a pipe-only analysis. The ductile tearing analysis used twelve 3D crack meshes with a range of crack lengths, from short to long, to compute the crack front J-integral values by elastic-plastic finite element analysis. The material J-R curve and analysis J results were used to compute the tearing modulus curves to get the J-T diagram. Each crack mesh provides a data point on the applied tearing modulus curve, and enough crack meshes are needed to compute an accurate J derivative. The critical J value for ductile instability was used to interpolate the critical crack length. The initial critical crack length that initiates the unstable ductile tearing was obtained by shifting the J-R curve to match the ductile instability point to the crack front J results curve. Compared with using a single toughness value, the ductile tearing analysis takes advantage of stable tearing and higher J-R values giving a longer critical crack length, which may be beneficial in deciding upon a course of action to inspect, maintain, or repair a damaged component.

12 REFERENCES Rowson, Q. and Rock M., Tearing Analysis Employing Finite Element Analysis With Crack Mesh In Comparison To Standardised Methods. NAFEMS World Congress 2011, Boston, May Anderson, T. L., Fracture Mechanics: Fundamentals and Applications. 3 rd ed. Boca Raton, FL: CRC Press, Taylor & Francis Group. Quest Integrity Group, FEACrack User s Manual, version 3.2. Available at: < [Accessed 7 December 2010]. Dodds, R. et al., WARP3D-Release 16.2: 3-D Dynamic Nonlinear Fracture Analyses of Solids Using Parallel Computers. Available at: < [Accessed 7 December 2010]. Thorwald, G., Necessary Analysis Ingredients For FEA Models With Multiple Cracks West Regional ABAQUS User s Meeting, San Francisco Bay Area, October Thorwald, G Fatigue Analysis Using a Custom Profile 3D Crack Front Including Weld Residual Stress International ANSYS Conference, Pittsburgh, August

3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation

3D Finite Element Software for Cracks. Version 3.2. Benchmarks and Validation 3D Finite Element Software for Cracks Version 3.2 Benchmarks and Validation October 217 1965 57 th Court North, Suite 1 Boulder, CO 831 Main: (33) 415-1475 www.questintegrity.com http://www.questintegrity.com/software-products/feacrack

More information

FEACrack Version History

FEACrack Version History FEACrack Version History Version 3.2.033 December 5, 2017 Fixed a problem in the PRO mesh to assign the weld and HAZ mesh zones to the correct elements when the weld root size is small compared to the

More information

CHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force

CHAPTER 4. Numerical Models. descriptions of the boundary conditions, element types, validation, and the force CHAPTER 4 Numerical Models This chapter presents the development of numerical models for sandwich beams/plates subjected to four-point bending and the hydromat test system. Detailed descriptions of the

More information

A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections

A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections A Multiple Constraint Approach for Finite Element Analysis of Moment Frames with Radius-cut RBS Connections Dawit Hailu +, Adil Zekaria ++, Samuel Kinde +++ ABSTRACT After the 1994 Northridge earthquake

More information

Similar Pulley Wheel Description J.E. Akin, Rice University

Similar Pulley Wheel Description J.E. Akin, Rice University Similar Pulley Wheel Description J.E. Akin, Rice University The SolidWorks simulation tutorial on the analysis of an assembly suggested noting another type of boundary condition that is not illustrated

More information

Revised Sheet Metal Simulation, J.E. Akin, Rice University

Revised Sheet Metal Simulation, J.E. Akin, Rice University Revised Sheet Metal Simulation, J.E. Akin, Rice University A SolidWorks simulation tutorial is just intended to illustrate where to find various icons that you would need in a real engineering analysis.

More information

THE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT

THE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT Journal of MECHANICAL ENGINEERING Strojnícky časopis, VOL 67 (2017), NO 2, 69-76 THE EFFECT OF THE FREE SURFACE ON THE SINGULAR STRESS FIELD AT THE FATIGUE CRACK FRONT OPLT Tomáš 1,2, POKORNÝ Pavel 2,

More information

Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction

Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering. Introduction Revision of the SolidWorks Variable Pressure Simulation Tutorial J.E. Akin, Rice University, Mechanical Engineering Introduction A SolidWorks simulation tutorial is just intended to illustrate where to

More information

3D Finite Element Software for Cracks Version User s Manual

3D Finite Element Software for Cracks Version User s Manual 3D Finite Element Software for Cracks Version 3.2.034 User s Manual 1965 57 th Court North, Suite 100 Boulder, CO 80301, USA Office: +1-303 415-1475 FAX: +1-303 415-1847 http://www.questintegrity.com/software-products/feacrack

More information

Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering

Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Engineering Effects of Boundary Conditions (Fixtures and Temperatures) J.E. Akin, Rice University, Mechanical Engineering Here SolidWorks stress simulation tutorials will be re-visited to show how they

More information

Non-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla

Non-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla Non-Linear Analysis of Bolted Flush End-Plate Steel Beam-to-Column Connection Nur Ashikin Latip, Redzuan Abdulla 1 Faculty of Civil Engineering, Universiti Teknologi Malaysia, Malaysia redzuan@utm.my Keywords:

More information

A Computational Study of Local Stress Intensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens

A Computational Study of Local Stress Intensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens A Computational Study of Local Stress ntensity Factor Solutions for Kinked Cracks Near Spot Welds in Lap- Shear Specimens D.-A. Wang a and J. Pan b* a Mechanical & Automation Engineering, Da-Yeh University,

More information

ASME Verification and Validation Symposium May 13-15, 2015 Las Vegas, Nevada. Phillip E. Prueter, P.E.

ASME Verification and Validation Symposium May 13-15, 2015 Las Vegas, Nevada. Phillip E. Prueter, P.E. VVS2015-8015: Comparing Closed-Form Solutions to Computational Methods for Predicting and Validating Stresses at Nozzle-to-Shell Junctions on Pressure Vessels Subjected to Piping Loads ASME Verification

More information

Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields

Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields Linear Elastic Fracture Mechanics (LEFM) Analysis of Flaws within Residual Stress Fields David Woyak 1, Brian Baillargeon, Ramesh Marrey, and Randy Grishaber 2 1 Dassault Systemés SIMULIA Corporation &

More information

Quarter Symmetry Tank Stress (Draft 4 Oct 24 06)

Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Quarter Symmetry Tank Stress (Draft 4 Oct 24 06) Introduction You need to carry out the stress analysis of an outdoor water tank. Since it has quarter symmetry you start by building only one-fourth of

More information

CHAPTER 4 INCREASING SPUR GEAR TOOTH STRENGTH BY PROFILE MODIFICATION

CHAPTER 4 INCREASING SPUR GEAR TOOTH STRENGTH BY PROFILE MODIFICATION 68 CHAPTER 4 INCREASING SPUR GEAR TOOTH STRENGTH BY PROFILE MODIFICATION 4.1 INTRODUCTION There is a demand for the gears with higher load carrying capacity and increased fatigue life. Researchers in the

More information

Manual for Computational Exercises

Manual for Computational Exercises Manual for the computational exercise in TMM4160 Fracture Mechanics Page 1 of 32 TMM4160 Fracture Mechanics Manual for Computational Exercises Version 3.0 Zhiliang Zhang Dept. of Structural Engineering

More information

Global to Local Model Interface for Deepwater Top Tension Risers

Global to Local Model Interface for Deepwater Top Tension Risers Global to Local Model Interface for Deepwater Top Tension Risers Mateusz Podskarbi Karan Kakar 2H Offshore Inc, Houston, TX Abstract The water depths from which oil and gas are being produced are reaching

More information

TUTORIAL 7: Stress Concentrations and Elastic-Plastic (Yielding) Material Behavior Initial Project Space Setup Static Structural ANSYS ZX Plane

TUTORIAL 7: Stress Concentrations and Elastic-Plastic (Yielding) Material Behavior Initial Project Space Setup Static Structural ANSYS ZX Plane TUTORIAL 7: Stress Concentrations and Elastic-Plastic (Yielding) Material Behavior In this tutorial you will learn how to recognize and deal with a common modeling issues involving stress concentrations

More information

AUTOMATED METHODOLOGY FOR MODELING CRACK EXTENSION IN FINITE ELEMENT MODELS

AUTOMATED METHODOLOGY FOR MODELING CRACK EXTENSION IN FINITE ELEMENT MODELS AUTOMATED METHODOLOGY FOR MODELING CRACK THEME Structural Analysis - Durability, Fatigue & Fracture. James J. Kosloski Senior Engineering Manager - CAE Associates Dr. Michael Bak Senior Engineering Manager

More information

Mixed Mode Fracture of Through Cracks In Nuclear Reactor Steam Generator Helical Coil Tube

Mixed Mode Fracture of Through Cracks In Nuclear Reactor Steam Generator Helical Coil Tube Journal of Materials Science & Surface Engineering Vol. 3 (4), 2015, pp 298-302 Contents lists available at http://www.jmsse.org/ Journal of Materials Science & Surface Engineering Mixed Mode Fracture

More information

The part to be analyzed is the bracket from the tutorial of Chapter 3.

The part to be analyzed is the bracket from the tutorial of Chapter 3. Introduction to Solid Modeling Using SolidWorks 2007 COSMOSWorks Tutorial Page 1 In this tutorial, we will use the COSMOSWorks finite element analysis (FEA) program to analyze the response of a component

More information

WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD. For ANSYS release 14

WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD. For ANSYS release 14 WORKSHOP 6.4 WELD FATIGUE USING HOT SPOT STRESS METHOD For ANSYS release 14 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated.

More information

THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD

THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD THREE DIMENSIONAL DYNAMIC STRESS ANALYSES FOR A GEAR TEETH USING FINITE ELEMENT METHOD Haval Kamal Asker Department of Mechanical Engineering, Faculty of Agriculture and Forestry, Duhok University, Duhok,

More information

ANSYS Element. elearning. Peter Barrett October CAE Associates Inc. and ANSYS Inc. All rights reserved.

ANSYS Element. elearning. Peter Barrett October CAE Associates Inc. and ANSYS Inc. All rights reserved. ANSYS Element Selection elearning Peter Barrett October 2012 2012 CAE Associates Inc. and ANSYS Inc. All rights reserved. ANSYS Element Selection What is the best element type(s) for my analysis? Best

More information

Step Change in Design: Exploring Sixty Stent Design Variations Overnight

Step Change in Design: Exploring Sixty Stent Design Variations Overnight Step Change in Design: Exploring Sixty Stent Design Variations Overnight Frank Harewood, Ronan Thornton Medtronic Ireland (Galway) Parkmore Business Park West, Ballybrit, Galway, Ireland frank.harewood@medtronic.com

More information

2: Static analysis of a plate

2: Static analysis of a plate 2: Static analysis of a plate Topics covered Project description Using SolidWorks Simulation interface Linear static analysis with solid elements Finding reaction forces Controlling discretization errors

More information

Technical Report Example (1) Chartered (CEng) Membership

Technical Report Example (1) Chartered (CEng) Membership Technical Report Example (1) Chartered (CEng) Membership A TECHNICAL REPORT IN SUPPORT OF APPLICATION FOR CHARTERED MEMBERSHIP OF IGEM DESIGN OF 600 (103 BAR) 820MM SELF SEALING REPAIR CLAMP AND VERIFICATION

More information

Simulation of Discrete-source Damage Growth in Aircraft Structures: A 3D Finite Element Modeling Approach

Simulation of Discrete-source Damage Growth in Aircraft Structures: A 3D Finite Element Modeling Approach Simulation of Discrete-source Damage Growth in Aircraft Structures: A 3D Finite Element Modeling Approach A.D. Spear 1, J.D. Hochhalter 1, A.R. Ingraffea 1, E.H. Glaessgen 2 1 Cornell Fracture Group, Cornell

More information

studying of the prying action effect in steel connection

studying of the prying action effect in steel connection studying of the prying action effect in steel connection Saeed Faraji Graduate Student, Department of Civil Engineering, Islamic Azad University, Ahar Branch S-faraji@iau-ahar.ac.ir Paper Reference Number:

More information

ANSYS AIM Tutorial Structural Analysis of a Plate with Hole

ANSYS AIM Tutorial Structural Analysis of a Plate with Hole ANSYS AIM Tutorial Structural Analysis of a Plate with Hole Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Problem Specification Pre-Analysis & Start Up Analytical vs. Numerical Approaches

More information

Chapter 3 Analysis of Original Steel Post

Chapter 3 Analysis of Original Steel Post Chapter 3. Analysis of original steel post 35 Chapter 3 Analysis of Original Steel Post This type of post is a real functioning structure. It is in service throughout the rail network of Spain as part

More information

Computer Life (CPL) ISSN: Finite Element Analysis of Bearing Box on SolidWorks

Computer Life (CPL) ISSN: Finite Element Analysis of Bearing Box on SolidWorks Computer Life (CPL) ISSN: 1819-4818 Delivering Quality Science to the World Finite Element Analysis of Bearing Box on SolidWorks Chenling Zheng 1, a, Hang Li 1, b and Jianyong Li 1, c 1 Shandong University

More information

Some Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact

Some Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact Some Aspects for the Simulation of a Non-Linear Problem with Plasticity and Contact Eduardo Luís Gaertner Marcos Giovani Dropa de Bortoli EMBRACO S.A. Abstract A linear elastic model is often not appropriate

More information

FOUNDATION IN OVERCONSOLIDATED CLAY

FOUNDATION IN OVERCONSOLIDATED CLAY 1 FOUNDATION IN OVERCONSOLIDATED CLAY In this chapter a first application of PLAXIS 3D is considered, namely the settlement of a foundation in clay. This is the first step in becoming familiar with the

More information

Hot Spot Stress Determination for a Tubular T-Joint under Combined Axial and Bending Loading

Hot Spot Stress Determination for a Tubular T-Joint under Combined Axial and Bending Loading IUST International Journal of Engineering Science, Vol. 17, No.3-4, 2006, Page 21-28 Hot Spot Stress Determination for a Tubular T-Joint under Combined Axial and Bending Loading M. Haghpanahi and H. Pirali

More information

IMPROVED SIF CALCULATION IN RIVETED PANEL TYPE STRUCTURES USING NUMERICAL SIMULATION

IMPROVED SIF CALCULATION IN RIVETED PANEL TYPE STRUCTURES USING NUMERICAL SIMULATION 26 th ICAF Symposium Montréal, 1 3 June 2011 IMPROVED SIF CALCULATION IN RIVETED PANEL TYPE STRUCTURES USING NUMERICAL SIMULATION S.C. Mellings 1, J.M.W. Baynham 1 and T.J. Curtin 2 1 C.M.BEASY, Southampton,

More information

ES 128: Computer Assignment #4. Due in class on Monday, 12 April 2010

ES 128: Computer Assignment #4. Due in class on Monday, 12 April 2010 ES 128: Computer Assignment #4 Due in class on Monday, 12 April 2010 Task 1. Study an elastic-plastic indentation problem. This problem combines plasticity with contact mechanics and has many rich aspects.

More information

ES 230 Strengths Intro to Finite Element Modeling & Analysis Homework Assignment 5

ES 230 Strengths Intro to Finite Element Modeling & Analysis Homework Assignment 5 ES 230 Strengths Intro to Finite Element Modeling & Analysis Homework Assignment 5 The GREAT Combined Load Problem Moving on to Principal Stresses and von Mises Failure Criteria Open up your ANSYS model

More information

Embedded Reinforcements

Embedded Reinforcements Embedded Reinforcements Gerd-Jan Schreppers, January 2015 Abstract: This paper explains the concept and application of embedded reinforcements in DIANA. Basic assumptions and definitions, the pre-processing

More information

Creo Simulate 3.0 Tutorial

Creo Simulate 3.0 Tutorial Creo Simulate 3.0 Tutorial Structure and Thermal Roger Toogood, Ph.D., P. Eng. SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following

More information

SDC. Engineering Analysis with COSMOSWorks. Paul M. Kurowski Ph.D., P.Eng. SolidWorks 2003 / COSMOSWorks 2003

SDC. Engineering Analysis with COSMOSWorks. Paul M. Kurowski Ph.D., P.Eng. SolidWorks 2003 / COSMOSWorks 2003 Engineering Analysis with COSMOSWorks SolidWorks 2003 / COSMOSWorks 2003 Paul M. Kurowski Ph.D., P.Eng. SDC PUBLICATIONS Design Generator, Inc. Schroff Development Corporation www.schroff.com www.schroff-europe.com

More information

Simulation of AJWSP10033_FOLDED _ST_FR

Simulation of AJWSP10033_FOLDED _ST_FR Phone: 01922 453038 www.hyperon-simulation-and-cad-services.co.uk Simulation of AJWSP10033_FOLDED _ST_FR Date: 06 May 2017 Designer: Study name: AJWSP10033_FOLDED_STATIC Analysis type: Static Description

More information

CHAPTER 1. Introduction

CHAPTER 1. Introduction ME 475: Computer-Aided Design of Structures 1-1 CHAPTER 1 Introduction 1.1 Analysis versus Design 1.2 Basic Steps in Analysis 1.3 What is the Finite Element Method? 1.4 Geometrical Representation, Discretization

More information

Advanced Professional Training

Advanced Professional Training Advanced Professional Training Non Linea rand Stability All information in this document is subject to modification without prior notice. No part of this manual may be reproduced, stored in a database

More information

EXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY

EXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY EXACT BUCKLING SOLUTION OF COMPOSITE WEB/FLANGE ASSEMBLY J. Sauvé 1*, M. Dubé 1, F. Dervault 2, G. Corriveau 2 1 Ecole de technologie superieure, Montreal, Canada 2 Airframe stress, Advanced Structures,

More information

FRANC3D & BES Benchmarking

FRANC3D & BES Benchmarking FRANC3D & BES Benchmarking Version 2.6 2003 1 Introduction FRANC3D/BES is capable of evaluating stress intensity factors (SIFs) along threedimensional crack fronts and then propagating these cracks. It

More information

Structural Analysis of an Aluminum Spiral Staircase. EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen

Structural Analysis of an Aluminum Spiral Staircase. EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen Structural Analysis of an Aluminum Spiral Staircase EMCH 407 Final Project Presented by: Marcos Lopez and Dillan Nguyen Abstract An old aluminum spiral staircase at Marcos home has been feeling really

More information

CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING

CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING 113 CHAPTER 6 EXPERIMENTAL AND FINITE ELEMENT SIMULATION STUDIES OF SUPERPLASTIC BOX FORMING 6.1 INTRODUCTION Superplastic properties are exhibited only under a narrow range of strain rates. Hence, it

More information

Exercise 1. 3-Point Bending Using the GUI and the Bottom-up-Method

Exercise 1. 3-Point Bending Using the GUI and the Bottom-up-Method Exercise 1 3-Point Bending Using the GUI and the Bottom-up-Method Contents Learn how to... 1 Given... 2 Questions... 2 Taking advantage of symmetries... 2 A. Preprocessor (Setting up the Model)... 3 A.1

More information

The GR3 Method for the Stress Analysis of Weldments

The GR3 Method for the Stress Analysis of Weldments The GR3 Method for the Stress Analysis of Weldments by Aditya Chattopadhyay A thesis presented to the University of Waterloo in fulfillment of the thesis requirement for the degree of Master of Applied

More information

WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD. For ANSYS release 14

WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD. For ANSYS release 14 WORKSHOP 6.3 WELD FATIGUE USING NOMINAL STRESS METHOD For ANSYS release 14 Objective: In this workshop, a weld fatigue analysis on a VKR-beam with a plate on top using the nominal stress method is demonstrated.

More information

CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1

CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1 Outcome 1 The learner can: CITY AND GUILDS 9210 UNIT 135 MECHANICS OF SOLIDS Level 6 TUTORIAL 15 - FINITE ELEMENT ANALYSIS - PART 1 Calculate stresses, strain and deflections in a range of components under

More information

Study of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket

Study of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket RESEARCH ARTICLE OPEN ACCESS Study of Convergence of Results in Finite Element Analysis of a Plane Stress Bracket Gowtham K L*, Shivashankar R. Srivatsa** *(Department of Mechanical Engineering, B. M.

More information

Finite Element modeling for computational Elastic-Plastic Fracture Mechanics: Crack Tip Opening Displacement (CTOD)

Finite Element modeling for computational Elastic-Plastic Fracture Mechanics: Crack Tip Opening Displacement (CTOD) e t International Journal on Emerging Technologies (Special Issue on ICRIET-2016) 7(2): 52-56(2016) ISSN No. (Print) : 0975-8364 ISSN No. (Online) : 2249-3255 Finite Element modeling for computational

More information

Element Order: Element order refers to the interpolation of an element s nodal results to the interior of the element. This determines how results can

Element Order: Element order refers to the interpolation of an element s nodal results to the interior of the element. This determines how results can TIPS www.ansys.belcan.com 鲁班人 (http://www.lubanren.com/weblog/) Picking an Element Type For Structural Analysis: by Paul Dufour Picking an element type from the large library of elements in ANSYS can be

More information

COMPUTER AIDED ENGINEERING. Part-1

COMPUTER AIDED ENGINEERING. Part-1 COMPUTER AIDED ENGINEERING Course no. 7962 Finite Element Modelling and Simulation Finite Element Modelling and Simulation Part-1 Modeling & Simulation System A system exists and operates in time and space.

More information

Set No. 1 IV B.Tech. I Semester Regular Examinations, November 2010 FINITE ELEMENT METHODS (Mechanical Engineering) Time: 3 Hours Max Marks: 80 Answer any FIVE Questions All Questions carry equal marks

More information

Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections

Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections October 25, 2000 Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections Tommi Vanhala Helsinki Institute of Physics 1. INTRODUCTION...2 2. STIFFNESS ANALYSES...2 2.1 ENVELOPE...2 2.2

More information

DESIGN & ANALYSIS OF CONNECTING ROD OF FORMING AND CUTTING DIE PILLAR STATION OF VACUUM FORMING MACHINE

DESIGN & ANALYSIS OF CONNECTING ROD OF FORMING AND CUTTING DIE PILLAR STATION OF VACUUM FORMING MACHINE Research Paper ISSN 2278 0149 www.ijmerr.com Vol. 3, No. 3, July, 2014 2014 IJMERR. All Rights Reserved DESIGN & ANALYSIS OF CONNECTING ROD OF FORMING AND CUTTING DIE PILLAR STATION OF VACUUM FORMING MACHINE

More information

Exercise 1. 3-Point Bending Using the Static Structural Module of. Ansys Workbench 14.0

Exercise 1. 3-Point Bending Using the Static Structural Module of. Ansys Workbench 14.0 Exercise 1 3-Point Bending Using the Static Structural Module of Contents Ansys Workbench 14.0 Learn how to...1 Given...2 Questions...2 Taking advantage of symmetries...2 A. Getting started...3 A.1 Choose

More information

Analysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing

Analysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing Kasetsart J. (Nat. Sci.) 42 : 165-176 (2008) Analysis of Fluid-Structure Interaction Effects of Liquid-Filled Container under Drop Testing Chakrit Suvanjumrat*, Tumrong Puttapitukporn and Satjarthip Thusneyapan

More information

MEEN 3360 Engineering Design and Simulation Spring 2016 Homework #1 This homework is due Tuesday, February 2, From your book and other

MEEN 3360 Engineering Design and Simulation Spring 2016 Homework #1 This homework is due Tuesday, February 2, From your book and other MEEN 3360 Engineering Design and Simulation Spring 2016 Homework #1 This homework is due Tuesday, February 2, 2016 1.0 From your book and other sources, write a paragraph explaining CFD and finite element

More information

Newman-Raju Limits Study. Exceeding Thickness to Diameter Upper Bound. Chad King Robert Pilarczyk James Gyllenskog Joshua Hodges

Newman-Raju Limits Study. Exceeding Thickness to Diameter Upper Bound. Chad King Robert Pilarczyk James Gyllenskog Joshua Hodges Newman-Raju Limits Study Exceeding Thickness to Diameter Upper Bound Chad King Robert Pilarczyk James Gyllenskog Joshua Hodges Issue Approach Overview Finite Element Analysis Solution AFGROW Solution (Implementation)

More information

COLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS

COLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS VOL., NO., NOVEMBER 6 ISSN 8968 6-6 Asian Research Publishing Network (ARPN). All rights reserved. COLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS

More information

AiMT Advances in Military Technology

AiMT Advances in Military Technology AiMT Advances in Military Technology Vol. 13, No. 1 (2018), pp. 119-131 ISSN 1802-2308, eissn 2533-4123 DOI 10.3849/aimt.01230 Critical Crack Size Investigation Method for a Land Launcher A. Yetgin 1*,

More information

Lateral Loading of Suction Pile in 3D

Lateral Loading of Suction Pile in 3D Lateral Loading of Suction Pile in 3D Buoy Chain Sea Bed Suction Pile Integrated Solver Optimized for the next generation 64-bit platform Finite Element Solutions for Geotechnical Engineering 00 Overview

More information

THE COMPUTATIONAL MODEL INFLUENCE ON THE NUMERICAL SIMULATION ACCURACY FOR FORMING ALLOY EN AW 5754

THE COMPUTATIONAL MODEL INFLUENCE ON THE NUMERICAL SIMULATION ACCURACY FOR FORMING ALLOY EN AW 5754 THE COMPUTATIONAL MODEL INFLUENCE ON THE NUMERICAL SIMULATION ACCURACY FOR FORMING ALLOY EN AW 5754 Pavel SOLFRONK a, Jiří SOBOTKA a, Pavel DOUBEK a, Lukáš ZUZÁNEK a a TECHNICAL UNIVERSITY OF LIBEREC,

More information

AN IMPROVED METHOD TO MODEL SEMI-ELLIPTICAL SURFACE CRACKS USING ELEMENT MISMATCH IN ABAQUS

AN IMPROVED METHOD TO MODEL SEMI-ELLIPTICAL SURFACE CRACKS USING ELEMENT MISMATCH IN ABAQUS AN IMPROVED METHOD TO MODEL SEMI-ELLIPTICAL SURFACE CRACKS USING ELEMENT MISMATCH IN ABAQUS R. H. A. Latiff and F. Yusof School of Mechanical Engineering, UniversitiSains, Malaysia E-Mail: mefeizal@usm.my

More information

IJMH - International Journal of Management and Humanities ISSN:

IJMH - International Journal of Management and Humanities ISSN: EXPERIMENTAL STRESS ANALYSIS SPUR GEAR USING ANSYS SOFTWARE T.VADIVELU 1 (Department of Mechanical Engineering, JNTU KAKINADA, Kodad, India, vadimay28@gmail.com) Abstract Spur Gear is one of the most important

More information

ASME Fatigue DOCUMENTATION. ANSYS Mechanical Application. Extension version Compatible ANSYS version

ASME Fatigue DOCUMENTATION. ANSYS Mechanical Application. Extension version Compatible ANSYS version ASME Fatigue ANSYS Mechanical Application DOCUMENTATION Extension version 180.1 Release date 06-Apr-17 Compatible ANSYS version 18.0 www.edrmedeso.com Table of Contents 1 INTRODUCTION... 3 2 PRODUCT RESTRICTIONS...

More information

Analysis and Design of Cantilever Springs

Analysis and Design of Cantilever Springs Analysis and Design of Cantilever Springs Hemendra Singh Shekhawat, Hong Zhou Department of Mechanical Engineering Texas A&M University-Kingsville Kingsville, Texas, USA Abstract Cantilever springs are

More information

Design Verification Procedure (DVP) Load Case Analysis of Car Bonnet

Design Verification Procedure (DVP) Load Case Analysis of Car Bonnet Design Verification Procedure (DVP) Load Case Analysis of Car Bonnet Mahesha J 1, Prashanth A S 2 M.Tech Student, Machine Design, Dr. A.I.T, Bangalore, India 1 Asst. Professor, Department of Mechanical

More information

Case Study- Importing As-Molded Plastic Part Conditions into CAE tools

Case Study- Importing As-Molded Plastic Part Conditions into CAE tools 1 IEI Innova Engineering 1 Park Plaza Suite 980 Irvine, California 92614 Case Study- Importing As-Molded Plastic Part Conditions into CAE tools 2 CONTENTS CONTENTS... 2 EXECUTIVE SUMMARY... 3 APPROACH...

More information

Print Depth Prediction in Hot Forming Process with a Reconfigurable Die

Print Depth Prediction in Hot Forming Process with a Reconfigurable Die Print Depth Prediction in Hot Forming Process with a Reconfigurable Die Jonathan Boisvert* Thibaut Bellizzi* Henri Champliaud Patrice Seers École de Technologie supérieure, Montréal, Québec *Master students,

More information

Introduction to Finite Element Analysis using ANSYS

Introduction to Finite Element Analysis using ANSYS Introduction to Finite Element Analysis using ANSYS Sasi Kumar Tippabhotla PhD Candidate Xtreme Photovoltaics (XPV) Lab EPD, SUTD Disclaimer: The material and simulations (using Ansys student version)

More information

CHAPTER 8 FINITE ELEMENT ANALYSIS

CHAPTER 8 FINITE ELEMENT ANALYSIS If you have any questions about this tutorial, feel free to contact Wenjin Tao (w.tao@mst.edu). CHAPTER 8 FINITE ELEMENT ANALYSIS Finite Element Analysis (FEA) is a practical application of the Finite

More information

Application of a FEA Model for Conformability Calculation of Tip Seal in Compressor

Application of a FEA Model for Conformability Calculation of Tip Seal in Compressor Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 2008 Application of a FEA Model for Conformability Calculation of Tip Seal in Compressor

More information

RELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS

RELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS International Conference on Economic Engineering and Manufacturing Systems Braşov, 26 27 November 2009 RELIABILITY OF THE FEM CALCULATIONS OF THE FRACTURE MECHANICS PARAMETERS Galina TODOROVA, Valentin

More information

Finite Element Course ANSYS Mechanical Tutorial Tutorial 3 Cantilever Beam

Finite Element Course ANSYS Mechanical Tutorial Tutorial 3 Cantilever Beam Problem Specification Finite Element Course ANSYS Mechanical Tutorial Tutorial 3 Cantilever Beam Consider the beam in the figure below. It is clamped on the left side and has a point force of 8kN acting

More information

ANSYS Workbench Guide

ANSYS Workbench Guide ANSYS Workbench Guide Introduction This document serves as a step-by-step guide for conducting a Finite Element Analysis (FEA) using ANSYS Workbench. It will cover the use of the simulation package through

More information

Using three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model

Using three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model Boundary Elements XXVII 245 Using three-dimensional CURVIC contact models to predict stress concentration effects in an axisymmetric model J. J. Rencis & S. R. Pisani Department of Mechanical Engineering,

More information

Figure 30. Degrees of freedom of flat shell elements

Figure 30. Degrees of freedom of flat shell elements Shell finite elements There are three types of shell finite element; 1) flat elements, 2) elements based on the Sanders-Koiter equations and 3) elements based on reduction of a solid element. Flat elements

More information

Solid and shell elements

Solid and shell elements Solid and shell elements Theodore Sussman, Ph.D. ADINA R&D, Inc, 2016 1 Overview 2D and 3D solid elements Types of elements Effects of element distortions Incompatible modes elements u/p elements for incompressible

More information

Difficulties in FE-modelling of an I- beam subjected to torsion, shear and bending

Difficulties in FE-modelling of an I- beam subjected to torsion, shear and bending DEGREE PROJECT, IN STEEL STRUCTURES, SECOND LEVEL STOCKHOLM, SWEDEN 2015 Difficulties in FE-modelling of an I- beam subjected to torsion, shear and bending MIRIAM ALEXANDROU KTH ROYAL INSTITUTE OF TECHNOLOGY

More information

What makes Bolt Self-loosening Predictable?

What makes Bolt Self-loosening Predictable? What makes Bolt Self-loosening Predictable? Abstract Dr.-Ing. R. Helfrich, Dr.-Ing. M. Klein (INTES GmbH, Germany) In mechanical engineering, bolts are frequently used as standard fastening elements, which

More information

Modelling Flat Spring Performance Using FEA

Modelling Flat Spring Performance Using FEA Modelling Flat Spring Performance Using FEA Blessing O Fatola, Patrick Keogh and Ben Hicks Department of Mechanical Engineering, University of Corresponding author bf223@bath.ac.uk Abstract. This paper

More information

Offshore Platform Fluid Structure Interaction (FSI) Simulation

Offshore Platform Fluid Structure Interaction (FSI) Simulation Offshore Platform Fluid Structure Interaction (FSI) Simulation Ali Marzaban, CD-adapco Murthy Lakshmiraju, CD-adapco Nigel Richardson, CD-adapco Mike Henneke, CD-adapco Guangyu Wu, Chevron Pedro M. Vargas,

More information

SETTLEMENT OF A CIRCULAR FOOTING ON SAND

SETTLEMENT OF A CIRCULAR FOOTING ON SAND 1 SETTLEMENT OF A CIRCULAR FOOTING ON SAND In this chapter a first application is considered, namely the settlement of a circular foundation footing on sand. This is the first step in becoming familiar

More information

X-FEM based modelling of complex mixed mode fatigue crack propagation

X-FEM based modelling of complex mixed mode fatigue crack propagation X-FEM based modelling of complex mixed mode fatigue crack propagation Hans Minnebo 1, Simon André 2, Marc Duflot 1, Thomas Pardoen 2, Eric Wyart 1 1 Cenaero, Rue des Frères Wright 29, 6041 Gosselies, Belgium

More information

Example 24 Spring-back

Example 24 Spring-back Example 24 Spring-back Summary The spring-back simulation of sheet metal bent into a hat-shape is studied. The problem is one of the famous tests from the Numisheet 93. As spring-back is generally a quasi-static

More information

OPTIMIZATION OF ENERGY DISSIPATION PROPERTY OF ECCENTRICALLY BRACED STEEL FRAMES

OPTIMIZATION OF ENERGY DISSIPATION PROPERTY OF ECCENTRICALLY BRACED STEEL FRAMES OPTIMIZATION OF ENERGY DISSIPATION PROPERTY OF ECCENTRICALLY BRACED STEEL FRAMES M. Ohsaki (Hiroshima Univ.) T. Nakajima (Kyoto Univ. (currently Ohbayashi Corp.)) Background Difficulty in optimization

More information

Tutorial 1: Welded Frame - Problem Description

Tutorial 1: Welded Frame - Problem Description Tutorial 1: Welded Frame - Problem Description Introduction In this first tutorial, we will analyse a simple frame: firstly as a welded frame, and secondly as a pin jointed truss. In each case, we will

More information

Advanced model of steel joints loaded by internal forces from 3D frame structures

Advanced model of steel joints loaded by internal forces from 3D frame structures Advanced model of steel joints loaded by internal forces from 3D frame structures Lubomír Šabatka, IDEA RS s.r.o František Wald, FSv ČVUT Praha Jaromír Kabeláč, Hypatia Solutions s.r.o Drahoslav Kolaja,

More information

Modeling Foundations in RS

Modeling Foundations in RS Modeling Foundations in RS 3 Piled Raft Modeling in RS 3 Deep foundation piles are commonly used to increase foundation stability and to increase the bearing capacity of structural systems. The design

More information

PREDICTION OF CRACK PROPAGATION DIRECTION FOR HOLES UNDER QUASI-STATIC LOADING

PREDICTION OF CRACK PROPAGATION DIRECTION FOR HOLES UNDER QUASI-STATIC LOADING 2007 Computational & Experimental Mechanics Editors: A. K. Ariffin, N. A. Nik Mohamed and S. Abdullah PREDICTION OF CRACK PROPAGATION DIRECTION FOR HOLES UNDER QUASI-STATIC LOADING Zaleha. M 1., A.K. Ariffin

More information

Application of Finite Volume Method for Structural Analysis

Application of Finite Volume Method for Structural Analysis Application of Finite Volume Method for Structural Analysis Saeed-Reza Sabbagh-Yazdi and Milad Bayatlou Associate Professor, Civil Engineering Department of KNToosi University of Technology, PostGraduate

More information

Modeling Skills Stress Analysis J.E. Akin, Rice University, Mech 417

Modeling Skills Stress Analysis J.E. Akin, Rice University, Mech 417 Introduction Modeling Skills Stress Analysis J.E. Akin, Rice University, Mech 417 Most finite element analysis tasks involve utilizing commercial software, for which you do not have the source code. Thus,

More information

Final project: Design problem

Final project: Design problem ME309 Homework #5 Final project: Design problem Select one of the analysis problems listed below to solve. Your solution, along with a description of your analysis process, should be handed in as a final

More information

MATLAB. Advanced Mathematics and Mechanics Applications Using. Third Edition. David Halpern University of Alabama CHAPMAN & HALL/CRC

MATLAB. Advanced Mathematics and Mechanics Applications Using. Third Edition. David Halpern University of Alabama CHAPMAN & HALL/CRC Advanced Mathematics and Mechanics Applications Using MATLAB Third Edition Howard B. Wilson University of Alabama Louis H. Turcotte Rose-Hulman Institute of Technology David Halpern University of Alabama

More information