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

Size: px
Start display at page:

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

Transcription

1 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 for numerical simulations of conformed mechanical components. Such processes have large permanent deformations, and require material models that account for the relationship between stress and strain, along with the influence of temperature and strain rate.. Important parameters are mesh quality, solver type, contact behavior, boundary conditions and the material model. Also, when the properties are unknown and the data available in the literature is inadequate, lab tests are indispensable. The easiest and most common test is the tension test. It provides information, such as stress-strain curve, Young modulus, yield and ultimate stress. This work proposes to analyze numerical results using MISO and BISO models, with experimental data from a tension test. This problem involves compressing a cylinder against two flat surfaces. It is validated with actual tests, where the load versus axial and radial displacement are measured during load application and elastic return. The importance of the contact method, element type and size are evaluated with respect to final deformation and CPU time. Introduction One of the principal difficulties with finite element modeling is using the correct properties for the materials involved. Frequently, the analyses are performed with material data obtained from the literature. This fact raises the risk of results that do not represent the actual material. Of course that there are other factors, like geometry, mesh, boundary conditions, loads, and contact parameters, that are very important to successful Finite Element Method (FEM) application. Looking back to the material case, the problem becomes more pronounced when the analysis moves from linear (elastic behavior) to non-linear (elasto-plastic behavior). In this situation, the correct characterization of the mechanical behavior of the material is fundamental. Consider a typical stress-strain curve for steel, one of the most common curves in engineering. This curve is obtained from a tension test performed on standard specimens, where the deformation is measured as a function of the applied axial load. Up to a certain magnitude, the deformation in the specimen is elastic and proportional to the load. This point (Sy) is called yield strength or yield point. Beyond it the material enters in the plastic region, and starts to undergo permanent deformation, i.e., the specimen will not return to its initial length. In the literature there are various mathematical models to describe the elasto-plastic behavior of the materials. The used most often are: elastic-perfectly plastic, elasto-plastic with linear or nonlinear hardening, isotropic or kinematic hardening and elasto-viscoplastic, It is becoming more common to apply FEM to simulate the conformation process, such as stamping, extrusion and forging. In those cases, the correctly setting up the contact parameters is essential to the problem solution. It will also aid CPU processing time (convergence) and result accuracy. These two factors, (non-linear material properties and contact), lead to highly complex problems in the numerical point view, demanding considerable theoretical and computational effort to reach the solution. The objective of this work is to present the main steps that should be followed in the numerical simulation of a specimen under compression. In this simulation, besides the geometric simplicity of the model, it involves so complex stages, since the characterization of the stress-strain curve of the material, contact parameters evaluation, including a experimental test to determine the friction coefficient, study of elastoplastic models, influence of the elements and mesh, and at the end a comparison with experimental results.

2 Material properties An initial step for simulations is to know the material properties for the problem. One can not simulate a steel gear using aluminum properties. There are a lot of models to describe the elasto-plastic behavior of the materials. Each model has its characteristic and is appropriate to a certain type of problem. Because of this, it is very important to know the theory before using it. Examples of models are: linear elastic, elastic-perfectly plastic, elasto-plastic with linear or nonlinear hardening, isotropic or kinematic hardening. Several options and models are available for describing plasticity behavior in ANSYS. This work will deal with only the BISO and MISO models. The Bilinear Isotropic Hardening (BISO) option uses the von Mises yield criteria coupled with an isotropic work hardening assumption. It is called bilinear because just two lines define the stress-strain curve: one to describe the linear elastic region and another to the plastic, see Figure 1a. The Multilinear Isotropic Hardening (MISO) is like the previous model, except that a couple of curves are used instead of a bilinear curve, Figure 1b. Figure 1. Uniaxial behavior for a) MISO and b) BISO model. To enter the information in ANSYS, it is necessary to define the material s behavior in both the elastic and plastic region. To accomplish this, standard strength specimens were produced and submitted to a tension test. The experiment uses a grip-gage to collect the axial strain and a load cell measuring the traction force, all connected to a computer. Data used in ANSYS for MISO model are shown in Figure 2, but not adimmensionally as here. The material of the tension test specimens is the same as that for the next experiment.

3 Figure 2. True stress-strain curve. FEM model The objective of the tension test is to collect the material properties and supply the material properties for the simulation of a compression test, the purpose of this paper. The specimen for compression is cylindrical, with 9.0 mm diameter and 18.0 mm height. Figure 3. FEM model with refinement factor of a) 1.0 and b) 3.0. To simplify the analysis, some assumptions are considered: The elements have axisymmetry, so it is a 2D simulation;

4 Poisson coefficient of 0.3; The surfaces that compress the specimen are flat and rigid; Constant friction coefficient among specimen and flat surfaces; The material behavior for compression is the same as for tension. The model is composed by a section of the cylinder and two rigid lines in contact with the body: one is fixed (bottom) and another receives the load (upper), see Figure 3a. The load is applied in steps up to the maximum compression load. Then, a second time step gradually removes it. The specimen has elastoplastic behavior. This whole model allows the simulation of permanent deformations of the body. The complete model is made with ANSYS Parametric Design Language (APDL). This scripting language allows the model to be built in parametric terms. Besides the simple geometry of the model, the language allows that factors like element type, mesh refinement, contact parameters and material behavior be able to be easily changed and analyzed. To make the analysis easier in terms of degrees of freedom (DOF), a parameter called refinement factor is defined, indicating how the mesh is refined with regard to a standard one. In this case, the reference mesh is presented in Figure 3a, and consists of 3 elements in the radius and 12 elements in the height. The sizes are divided to have each element with quadrate shape. Thus, for a refinement factor of 3.0, there are 3*3 elements in the radius and 3*12 elements in the height, Figure 3b. Contact parameters The iterative analysis of two non-adjacent elements is performed with contact elements. Contact elements prevent contacting surfaces from passing through each other and transfer forces between contacting surfaces. Problems involving contact are highly nonlinear and require significant resources to solve. There are methods for contact and also parameters to set up. Pure Penalty, Pure Lagrange and Augmented Lagrange are used the most. Each method has its characteristics, with advantages and disadvantages. In pure penalty, the iteration among the contact surfaces is achieved using a kind of spring. When contact is detected, the spring deflects, creating a contact force that satisfies the equilibrium. This method requires spring stiffness, (also called the normal penalty stiffness factor FKN). This method will converge more readily, but shows small penetration between the contact surfaces and is sensitive to FKN value. Artificially high FKN values can lead to convergence difficulties, while low values yield exaggerated penetration. The Augmented Lagrange method uses a series of penalty functions to guarantee contact compatibility. The contact forces are raised up during the solution. This approach minimizes penetration, is better conditioned than Pure Penalty and is less sensitive to contact stiffness, but might require more iterations. The Pure Lagrange method does not use those virtual springs, but adds an extra DOF (contact pressure) to reach the contact compatibility in order to guarantee the zero penetration. However, it requires direct solves, which means extra computational effort. Moreover, convergence problems can occur due the over constraining phenomenon. The friction between two bodies is set up as a parameter of the contact method. When friction is included, shear forces are added between the bodies. In ANSYS, friction is implemented using a Coulomb model. Contact problems involving friction produce an unsymmetrical stiffness matrix, and using an unsymmetrical equation solver is more computationally expensive than a symmetric solver. For this reason ANSYS uses a symmetrization algorithm by which most contact problems involving friction can be solved. The contact methods used in the simulations are Pure Lagrange, Augmented Lagrange or Pure Penalty. In the last two, the values for FKN are 1.0 and

5 Friction coefficient One important parameter in analysis involving contact is the friction coefficient among the bodies faces. For the case in question, the friction coefficient is measured, using a simple inclined plan. At first, a specimen is placed on the plan surface, and slowly it is inclined, see Figure 4. The tangent of the inclination angle, which provides the initial slid of the body, is the static friction coefficient. Equation bellow is the force sum on the inclined direction. No lubricant is applied among the body and flat surfaces during experimental tests. For this case, the friction coefficient obtained is 0.2. F F friction friction sinβ *Weight = 0 = Normal* µ = cos β *Weight* µ µ = cos β sen β = tan β = Friction coefficient Figure 4. Friction test. Numerical results Figure 5 represents the permanent deformation for the body after applying a compressive force and removing it, in axial and radial directions. The parameters for this analysis are: refinement factor of 3.0, element type PLANE183 (higher order 2-D, 8-node element). The Pure Lagrange method is used to reduce the errors from the contact elements. The friction coefficient is 0.2, the same as obtained at the experimental test. The material model is MISO, with data from the tension test, Figure 2.

6 Figure 5. Axial and radial permanent deformation. Material model: So important as the boundary conditions, the correct set up of the material properties can be deceiving in the accuracy of an analysis. In this chapter it shall be discussed the numerical results obtained for the compressive test simulation, when using MISO and BISO model to characterize the material. The difference between them is that in the former the stress-strain curve is discretized by several line segments. The latter consists of just two lines: one for elastic and another for plastic behavior. In ANSYS, the BISO model can be easy used: it is just necessary to choose the model and inform the Young modulus, the yield stress and the line tangent that defines the plastic field. The BISO model is evaluated, for the problem in question, using two different curves to characterize the material, with different yield stress and line tangent, as shown in Figure 6.

7 Figure 6. True stress-strain curve using BISO model. In curve a, the line that represents the plastic field is established in such way that it can better approximate the whole material behavior, but its yield stress has been increased. The disadvantage of this curve is that it has some distance to the experimental values near the yield region. In the other hand, curve b describes very well the material behavior for small plastic deformations, but turns the model more rigid for large deformations. As a consequence of this difference between the BISO curves for plasticity, there is a result variation for the models, especially in the permanent deformations after the compressive load removal, according to Table 1. In this, it is possible to see that the use of curve a leads to permanent deformations that are very distant to the expected, that would be using the MISO model. The opposite occurs when using curve b, which results have a deviation less than 6 %. Table 1: Comparison of the permanent deformation for different material models Model* Axial permanent deformation [ µ m] Radial permanent deformation [ µ m] MISO BISO with curve a BISO with curve b *Using element type PLANE183, friction coefficient 0.2, refinement factor 3.0 and Pure Lagrange method. An investigation shows that during compression the specimen undergoes small deformations. In the half height of the body, the deformations are about mm/mm, corresponding to a stress of 0.92 (adimenjional), for MISO model.

8 Figure 7. Von Mises stress distribution for maximum load, using BISO curve a and b. With model BISO based on curve a, where the yield stress was increased to better fit the experimental stress-strain curve, there is just plasticity in the corners. In the Figure 7 it is possible to see the stress distribution in the body, using curves a and b. For curve b, the differences in the results are smaller, because it has been approximated a line for the plastic field just for small deformation, which occurs in this problem. For this reason, the use of BISO model requests a lot of care, and the incorrect set up of its parameters can lead to very large differences in the permanent deformations. Contact parameters influence: In models involving contact, the correct set up of the various contact parameters are important for the analysis results, and some times can lead to the non-convergence of the problem. Among the parameters, the principals are the contact method, the contact stiffness, when it is necessary, and for the case in question, the friction coefficient. The influence of this last one can be shown in Figure 8.

9 Figure 8. Influence of the friction coefficient on axial and radial permanent deformation. The friction among the flat surfaces (in axisymmetric represented by two lines) and the specimen is responsible for the reduction of the body material flow in those regions. As consequence, the increase of the friction coefficient provides higher radial permanent deformation in the half height of the body. On the other hand, if there is no friction, the deformed body has a cylinder shape, not a barrel. According to Figure 8, the increase of friction coefficient after 0.3 brings no relevant difference for the radial and axial permanent deformation, less than 4 %, but the opposite occurs for friction coefficient less than 0.3. So, if a lubricant is placed in the experiment or if the friction coefficient were not very well measured before, the deformation shall have a huge change. An attempt was done to simplify the problem, eliminating the contact elements. In the upper body surface a force is distributed and in the bottom face a non-displacement condition. The time necessary to solve the problem is reduced between 30 and 60 %, depending the contact method. The result for this simplification is an axial permanent deformation of 62.2 µ m, similar as that on obtained for a friction coefficient of 0.1. The radial permanent deformation is 9.4 µ m, a little higher than any other result with contact. High variation in the results is observed due to the contact method. It can be explained by the mathematical penetration between two bodies under contact when using stiffness factor. For example, the penetration reaches 2.2 µ m for a friction coefficient 0.2 and FKN equals to 1. Remember that for Pure Lagrange method the penetration is zero. The influence of the mesh quality in the permanent deformation is noted in Figure 9. One can see that for FKN equals to 100 and for Pure Lagrange contact method, the element refinement does not bring significant influence. However, considerable variation is found for FKN value of 1.0. It is important to mention that the results for Figures 8, 9 and 10 are performed using element type PLANE183, and simulations for another element type shall produce different graphs.

10 Figure 9. Influence of the element size on axial and radial permanent deformation. An important thing that needs to take in consideration is the number of iterations to converge the problem. For the simulations with MISO model and element type PLANE183, the number of iterations does not vary so much, from 47 to 66, for FKN values of 1.0 and The change of contact method to Pure Lagrange brings an increase in the iteration number, reaching 108, which is expected. This corresponds to approximately the double of iterations to converge the problem, the same relation found in the CPU time increase, see Figure 10. According to it, the simulation-processing time is a potential function of the number of degrees of freedom (DOF), for MISO model and element type PLANE183. In fact, the potential coefficient is 0.97, and the relation between CPU time and DOF can be assumed linear, which corresponds to a coefficient of 1.0. Figure 10. Influence of the degrees of freedom and contact method on CPU time processing. So, for the same number of DOF, Pure Lagrange contact method takes the double time to converge, compared to Augmented Lagrange or Pure Penalty. Besides time processing is an important factor to take

11 into consideration, results quality should the studied, because it will serve for nothing a coarse mesh that converges relatively fast, but for the wrong place. Element and mesh influence: As mentioned before, element type choice can be determinant for results and time processing. This section analyses the influence of the element type and the mesh quality for the permanent deformations of the body under compression. The element used in the previous simulations is PLANE183, which is bi-dimensional, with two degrees of freedom in each node (translation in x and y axes), and axisymmetric simplification. To compare results with different element types, now it is used quadrilateral elements: PLANE 42, 182, 82 and 183, and the triangular PLANE2. Except to the first two, the other elements are higher order, i.e., have quadratic displacement behavior. In Figure 11, one can see that CPU time for higher order elements (PLANE 2, 82 and 183) is lower than for the others elements. The convergence criteria and value is the same in all simulations. But this can lead to a wrong conclusion if no care is taken. If you use the same element size, the analysis with the first group needs approximately 50 percent more time for convergence. It because those elements have 6 or 8 nodes per element. Consequently, a graph of CPU time versus refinement factor will point to PLANE 42 and 182 as a better element, when looking for time processing. Figure 11. Influence of the degrees of freedom and element type on CPU time processing. On the other hand, PLANE 42 and 182 elements show the worst results for coarse meshes. Figures 12 and 13 present, respectively, the axial and radial permanent deformation after load removal with the refinement factor variation. For very refined meshes, results for all element types converge to the same point. It is also possible to see that elements PLANE 82 and 183 have the smaller variation in the results when changing the element size. It means that even with a coarse mesh the results are not so different to another with very refined mesh. This verification makes possible a gain in time processing, because for refinement factor greater than 3.0 no expressive differences are found for deformations.

12 Figure 12. Variation of axial permanent deformation by the refinement factor. Figure 13. Variation of radial permanent deformation by the refinement factor. Experimental results To validate the numerical model, five cylindrical specimens were submitted to a compression test. In a machine test, a load cell measure the actual load applied, and a sensor gives the relative displacement of the nippers that tighten the device (a punch and a die). The punch and a die are hardened to guaranty plastic deformation just in the specimen. In addition, a linear sensor has been installed to collect diametral displacement, during load appliance and elastic return. See the whole apparatus in Figure 14.

13 Figure 14. Device to compression test. Figure 15. Diametral increase measurement on half height body by compression force. Good concordance between numerical and experimental results are achieved, according to Figure 15 that shows a graph of diametral displacement at the half height versus applied force. Similar results are found in Figure 16, which plots the axial displacement along load appliance. In the first case, the numerical model has a significant distance to the experimental in the region after yield point, which does not occur in the axial direction.

14 Figure 16. Axial displacement by compression force. A more accurate measurement of radial and diametral plastic deformation is made using a micrometer, taking the dimensions before and after test, see table 2. It indicates that a mean experimental diametral permanent deformation of 16 µ m, against 18 µ m from numerical results. This corresponds to a difference of 12 %, passing to 16 % when analyzed the axial deformation. Table 2: Specimens dimension before and after experiment Specimen SP1 SP2 SP3 SP4 SP5 Mean Initial length [mm] Initial diameter [mm] Axial permanent deformation [mm] Diametral permanent deformation [mm] One can note that the diametral and axial deformations measured with a micrometer, Table 2, are a little different to those collected by the test machine, in Figures 15 and 16, after removal the load. This can be due to small gaps in the test machine, in the axial direction. Another factor that can influence the experimental results is that the edges of the sensors in contact to the specimen, that collect diametral displacements, are rounded. A flat face would be better. Conclusion

15 The problem used to analyze the influence some parameters for a simulation of plasticity and contact consists in a compression of a cylinder against two flat surfaces, involving plasticity and contact. Some simplifications are made to reduce the time necessary to process the simulation. Between all parameters analyzed on this work, the most influence for the results is the material model and its properties. Some care should be taken when using BISO model instead MISO. Depending the aspect of the stress-strain curve and the range of use, the condition of plasticity can vary, i.e., for the same load, a simulation with MISO model can pass the elastic region, and with BISO model not. It is very important to choose a proper contact method, and also set up the parameters. According to the results, the choice of the contact method is more determinant for the results than the element type and size, for the problem in question. The friction coefficient has a very influence on the results in a range of 0 to 0.3. After it, the change in the axial and radial permanent deformation is not significant. The simplification of the contact elements by non-displacement conditions is not suitable for the problem in question, because there are a huge variation on the results. As expected, elements of higher order (PLANE 82 and 183) showed better results compared to those of with linear interpolation (PLANE 42 and 182). For the second group, there is a great variation in the results when elements have big sizes. For very refined meshes, results for all element types converge to the same point. The choice of the PLANEXXX elements and the mesh quality has more influence in the CPU time processing than in the results. Good correlation between numerical and experimental is found, with differences from 12 to 16 %, talking about the radial and axial deformations. The factors that can influence in the experimental results are: The edge of the diametral displacement sensors are rounded, but should be flat; The diametral displacement sensors can be not very well aligned; There are deviations in the tension test results, which have big influence to the numerical material model; The experimental determination of friction coefficient can show small variations, that represents a large difference in the permanent deformation values, because it is lower than 0.3. Reference 1) ZAHAVI, Eliahu, & BARLAM, David. Nonlinear Problems in Machine Design. CRC Press, New York, ) BOSCO Jr., Raul. Structural Analysis of a Sandwich Valve System for Hermetic Compressors ANSYS Latin American Users Conference (Presentation): São Paulo, ) ANSYS User Guide Manual.

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

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

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

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

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

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

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

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

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

Contents Metal Forming and Machining Processes Review of Stress, Linear Strain and Elastic Stress-Strain Relations 3 Classical Theory of Plasticity

Contents Metal Forming and Machining Processes Review of Stress, Linear Strain and Elastic Stress-Strain Relations 3 Classical Theory of Plasticity Contents 1 Metal Forming and Machining Processes... 1 1.1 Introduction.. 1 1.2 Metal Forming...... 2 1.2.1 Bulk Metal Forming.... 2 1.2.2 Sheet Metal Forming Processes... 17 1.3 Machining.. 23 1.3.1 Turning......

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

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

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

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

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

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

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

Guidelines for proper use of Plate elements

Guidelines for proper use of Plate elements Guidelines for proper use of Plate elements In structural analysis using finite element method, the analysis model is created by dividing the entire structure into finite elements. This procedure is known

More information

Non-Linear Analysis of Base Plates in Automated Storage Systems

Non-Linear Analysis of Base Plates in Automated Storage Systems Non-Linear Analysis of Base Plates in Automated Storage Systems Ph.D. Juan José del Coz Díaz, Fco. Suarez Domínguez, Paulino J.Garcia Nieto University of Oviedo. Construction and Applied Mathematics Area.

More information

Finite Element Method. Chapter 7. Practical considerations in FEM modeling

Finite Element Method. Chapter 7. Practical considerations in FEM modeling Finite Element Method Chapter 7 Practical considerations in FEM modeling Finite Element Modeling General Consideration The following are some of the difficult tasks (or decisions) that face the engineer

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

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

Coupled analysis of material flow and die deflection in direct aluminum extrusion

Coupled analysis of material flow and die deflection in direct aluminum extrusion Coupled analysis of material flow and die deflection in direct aluminum extrusion W. Assaad and H.J.M.Geijselaers Materials innovation institute, The Netherlands w.assaad@m2i.nl Faculty of Engineering

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

Non-Linear Finite Element Methods in Solid Mechanics Attilio Frangi, Politecnico di Milano, February 3, 2017, Lesson 1

Non-Linear Finite Element Methods in Solid Mechanics Attilio Frangi, Politecnico di Milano, February 3, 2017, Lesson 1 Non-Linear Finite Element Methods in Solid Mechanics Attilio Frangi, attilio.frangi@polimi.it Politecnico di Milano, February 3, 2017, Lesson 1 1 Politecnico di Milano, February 3, 2017, Lesson 1 2 Outline

More information

Finite Element Course ANSYS Mechanical Tutorial Tutorial 4 Plate With a Hole

Finite Element Course ANSYS Mechanical Tutorial Tutorial 4 Plate With a Hole Problem Specification Finite Element Course ANSYS Mechanical Tutorial Tutorial 4 Plate With a Hole Consider the classic example of a circular hole in a rectangular plate of constant thickness. The plate

More information

3-D Numerical Simulation of Direct Aluminum Extrusion and Die Deformation

3-D Numerical Simulation of Direct Aluminum Extrusion and Die Deformation 3-D Numerical Simulation of Direct Aluminum Extrusion and Die Deformation ABSTRACT W.A.Assaad, University of Twente Enschede, The Netherlands H.J.M. Geijselaers, University of Twente Enschede, The Netherlands

More information

Orbital forming of SKF's hub bearing units

Orbital forming of SKF's hub bearing units Orbital forming of SKF's hub bearing units Edin Omerspahic 1, Johan Facht 1, Anders Bernhardsson 2 1 Manufacturing Development Centre, AB SKF 2 DYNAmore Nordic 1 Background Orbital forming is an incremental

More information

Aufgabe 1: Dreipunktbiegung mit ANSYS Workbench

Aufgabe 1: Dreipunktbiegung mit ANSYS Workbench Aufgabe 1: Dreipunktbiegung mit ANSYS Workbench Contents Beam under 3-Pt Bending [Balken unter 3-Pkt-Biegung]... 2 Taking advantage of symmetries... 3 Starting and Configuring ANSYS Workbench... 4 A. Pre-Processing:

More information

Module 1.5: Moment Loading of a 2D Cantilever Beam

Module 1.5: Moment Loading of a 2D Cantilever Beam Module 1.5: Moment Loading of a D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing 9 Loads

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

Simulation of metal forming processes :

Simulation of metal forming processes : Simulation of metal forming processes : umerical aspects of contact and friction People Contact algorithms LTAS-MCT in a few words Laboratoire des Techniques Aéronautiques et Spatiales (Aerospace Laboratory)

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

Module 3: Buckling of 1D Simply Supported Beam

Module 3: Buckling of 1D Simply Supported Beam Module : Buckling of 1D Simply Supported Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing 9 Solution

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

Modeling Strategies for Dynamic Finite Element Cask Analyses

Modeling Strategies for Dynamic Finite Element Cask Analyses Session A Package Analysis: Structural Analysis - Modeling Modeling Strategies for Dynamic Finite Element Cask Analyses Uwe Zencker, Günter Wieser, Linan Qiao, Christian Protz BAM Federal Institute for

More information

Module 1.6: Distributed Loading of a 2D Cantilever Beam

Module 1.6: Distributed Loading of a 2D Cantilever Beam Module 1.6: Distributed Loading of a 2D Cantilever Beam Table of Contents Page Number Problem Description 2 Theory 2 Geometry 4 Preprocessor 7 Element Type 7 Real Constants and Material Properties 8 Meshing

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

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

Recent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA

Recent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA 14 th International LS-DYNA Users Conference Session: Simulation Recent Advances on Higher Order 27-node Hexahedral Element in LS-DYNA Hailong Teng Livermore Software Technology Corp. Abstract This paper

More information

FORMING SIMULATION USING RIGID-PLASTIC MATERIAL MODEL IN MARC

FORMING SIMULATION USING RIGID-PLASTIC MATERIAL MODEL IN MARC SESSION TITLE WILL BE COMPLETED BY MSC SOFTWARE FORMING SIMULATION USING RIGID-PLASTIC MATERIAL MODEL IN MARC Gary Huang, Simufact-Americas LLC April 8, 2013 SUMMARY When simulating large deformation in

More information

CHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA

CHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA DYNAMIC SIMULATION USING LS-DYNA CHAPTER-10 10.1 Introduction In the past few decades, the Finite Element Method (FEM) has been developed into a key indispensable technology in the modeling and simulation

More information

Module 1.3W Distributed Loading of a 1D Cantilever Beam

Module 1.3W Distributed Loading of a 1D Cantilever Beam Module 1.3W Distributed Loading of a 1D Cantilever Beam Table of Contents Page Number Problem Description 2 Theory 2 Workbench Analysis System 4 Engineering Data 5 Geometry 6 Model 11 Setup 13 Solution

More information

The Finite Element Method for the Analysis of Non-Linear and Dynamic Systems. Prof. Dr. Eleni Chatzi, J.P. Escallo n Lecture December, 2013

The Finite Element Method for the Analysis of Non-Linear and Dynamic Systems. Prof. Dr. Eleni Chatzi, J.P. Escallo n Lecture December, 2013 The Finite Element Method for the Analysis of Non-Linear and Dynamic Systems Prof. Dr. Eleni Chatzi, J.P. Escallo n Lecture 11-17 December, 2013 Institute of Structural Engineering Method of Finite Elements

More information

Best Practices for Contact Modeling using ANSYS

Best Practices for Contact Modeling using ANSYS Best Practices for Contact Modeling using ANSYS 朱永谊 / R&D Fellow ANSYS 1 2016 ANSYS, Inc. August 12, 2016 ANSYS UGM 2016 Why are these best practices important? Contact is the most common source of nonlinearity

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

A Sensitivity Analysis On The Springback Behavior Of The Unconstrained Bending Problem

A Sensitivity Analysis On The Springback Behavior Of The Unconstrained Bending Problem A Sensitivity Analysis On The Springback Behavior Of The Unconstrained Bending Problem T. Meinders 1,2, A.W.A. Konter 1, S.E. Meijers 1, E.H. Atzema 3, H. Kappert 4 1 Netherlands Institute for Metals Research,

More information

Static and dynamic simulations for automotive interiors components using ABAQUS

Static and dynamic simulations for automotive interiors components using ABAQUS Static and dynamic simulations for automotive interiors components using ABAQUS Mauro Olivero, Vincenzo Puleo, Massimo Barbi, Fabrizio Urbinati, Benedetta Peyron Fiat Research Centre Giancarlo Luciani,

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

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

Exercise 1: 3-Pt Bending using ANSYS Workbench

Exercise 1: 3-Pt Bending using ANSYS Workbench Exercise 1: 3-Pt Bending using ANSYS Workbench Contents Starting and Configuring ANSYS Workbench... 2 1. Starting Windows on the MAC... 2 2. Login into Windows... 2 3. Start ANSYS Workbench... 2 4. Configuring

More information

Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint

Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint Finite Element Model for Axial Stiffness of Metal-Plate-Connected Tension Splice Wood Truss Joint Jose M. Cabrero Assistant Professor University of Navarra, Department of Structural Analysis and Design,

More information

CHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS

CHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS CHAPTER 7 BEHAVIOUR OF THE COMBINED EFFECT OF ROOFING ELEMENTS 7.1 GENERAL An analytical study on behaviour of combined effect of optimised channel sections using ANSYS was carried out and discussed in

More information

Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses

Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses Exercise 2: Mesh Resolution, Element Shapes, Basis Functions & Convergence Analyses Goals In this exercise, we will explore the strengths and weaknesses of different element types (tetrahedrons vs. hexahedrons,

More information

A pipe bend is subjected to a concentrated force as shown: y All dimensions in inches. Material is stainless steel.

A pipe bend is subjected to a concentrated force as shown: y All dimensions in inches. Material is stainless steel. Problem description A pipe bend is subjected to a concentrated force as shown: y 15 12 P 9 Displacement gauge Cross-section: 0.432 18 x 6.625 All dimensions in inches. Material is stainless steel. E =

More information

SolidWorks. An Overview of SolidWorks and Its Associated Analysis Programs

SolidWorks. An Overview of SolidWorks and Its Associated Analysis Programs An Overview of SolidWorks and Its Associated Analysis Programs prepared by Prof. D. Xue University of Calgary SolidWorks - a solid modeling CAD tool. COSMOSWorks - a design analysis system fully integrated

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

Finite Element Analysis Prof. Dr. B. N. Rao Department of Civil Engineering Indian Institute of Technology, Madras. Lecture - 36

Finite Element Analysis Prof. Dr. B. N. Rao Department of Civil Engineering Indian Institute of Technology, Madras. Lecture - 36 Finite Element Analysis Prof. Dr. B. N. Rao Department of Civil Engineering Indian Institute of Technology, Madras Lecture - 36 In last class, we have derived element equations for two d elasticity problems

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

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

NEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN

NEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN Vol 4 No 3 NEW WAVE OF CAD SYSTEMS AND ITS APPLICATION IN DESIGN Ass Lecturer Mahmoud A Hassan Al-Qadisiyah University College of Engineering hasaaneng@yahoocom ABSTRACT This paper provides some lighting

More information

Influence of geometric imperfections on tapered roller bearings life and performance

Influence of geometric imperfections on tapered roller bearings life and performance Influence of geometric imperfections on tapered roller bearings life and performance Rodríguez R a, Calvo S a, Nadal I b and Santo Domingo S c a Computational Simulation Centre, Instituto Tecnológico de

More information

An Overview of Computer Aided Design and Finite Element Analysis

An Overview of Computer Aided Design and Finite Element Analysis An Overview of Computer Aided Design and Finite Element Analysis by James Doane, PhD, PE Contents 1.0 Course Overview... 4 2.0 General Concepts... 4 2.1 What is Computer Aided Design... 4 2.1.1 2D verses

More information

Through Process Modelling of Self-Piercing Riveting

Through Process Modelling of Self-Piercing Riveting 8 th International LS-DYNA User Conference Metal Forming (2) Through Process Modelling of Self-Piercing Riveting Porcaro, R. 1, Hanssen, A.G. 1,2, Langseth, M. 1, Aalberg, A. 1 1 Structural Impact Laboratory

More information

Predicting the mechanical behaviour of large composite rocket motor cases

Predicting the mechanical behaviour of large composite rocket motor cases High Performance Structures and Materials III 73 Predicting the mechanical behaviour of large composite rocket motor cases N. Couroneau DGA/CAEPE, St Médard en Jalles, France Abstract A method to develop

More information

IDENTIFYING WORST CASE DESIGNS THROUGH A COMBINED STRATEGY OF COMPUTATIONAL MODELING, STATISTICAL METHODS, AND BENCH TOP TESTS

IDENTIFYING WORST CASE DESIGNS THROUGH A COMBINED STRATEGY OF COMPUTATIONAL MODELING, STATISTICAL METHODS, AND BENCH TOP TESTS IDENTIFYING WORST CASE DESIGNS THROUGH A COMBINED STRATEGY OF COMPUTATIONAL MODELING, STATISTICAL METHODS, AND BENCH TOP TESTS Payman Afshari Andrew Dooris Pat Fatyol DePuy Synthes Spine, a Johnson and

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

TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS.

TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS. Ex_1_2D Plate.doc 1 TWO-DIMENSIONAL PROBLEM OF THE THEORY OF ELASTICITY. INVESTIGATION OF STRESS CONCENTRATION FACTORS. 1. INTRODUCTION Two-dimensional problem of the theory of elasticity is a particular

More information

Module 1.2: Moment of a 1D Cantilever Beam

Module 1.2: Moment of a 1D Cantilever Beam Module 1.: Moment of a 1D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry Preprocessor 6 Element Type 6 Real Constants and Material Properties 7 Meshing 9 Loads 10 Solution

More information

ME 442. Marc/Mentat-2011 Tutorial-1

ME 442. Marc/Mentat-2011 Tutorial-1 ME 442 Overview Marc/Mentat-2011 Tutorial-1 The purpose of this tutorial is to introduce the new user to the MSC/MARC/MENTAT finite element program. It should take about one hour to complete. The MARC/MENTAT

More information

Code_Aster. SSNV209 Interface in contact rubbing with X-FEM

Code_Aster. SSNV209 Interface in contact rubbing with X-FEM Titre : SSNV209 - Interface en contact frottant avec X-FEM Date : 21/07/2015 Page : 1/34 SSNV209 Interface in contact rubbing with X-FEM Summary: This problem corresponds to a quasi-static analysis of

More information

A rubber O-ring is pressed between two frictionless plates as shown: 12 mm mm

A rubber O-ring is pressed between two frictionless plates as shown: 12 mm mm Problem description A rubber O-ring is pressed between two frictionless plates as shown: Prescribed displacement C L 12 mm 48.65 mm A two-dimensional axisymmetric analysis is appropriate here. Data points

More information

A Locking-free Smoothed Finite Element Formulation (Modified Selective FS/NS-FEM-T4) with Tetrahedral Mesh Rezoning for Large Deformation Problems

A Locking-free Smoothed Finite Element Formulation (Modified Selective FS/NS-FEM-T4) with Tetrahedral Mesh Rezoning for Large Deformation Problems A Locking-free Smoothed Finite Element Formulation (Modified Selective FS/NS-FEM-T4) with Tetrahedral Mesh Rezoning for Large Deformation Problems Yuki ONISHI, Kenji AMAYA Tokyo Institute of Technology

More information

Generative Part Structural Analysis Fundamentals

Generative Part Structural Analysis Fundamentals CATIA V5 Training Foils Generative Part Structural Analysis Fundamentals Version 5 Release 19 September 2008 EDU_CAT_EN_GPF_FI_V5R19 About this course Objectives of the course Upon completion of this course

More information

Engineering Analysis with

Engineering Analysis with Engineering Analysis with SolidWorks Simulation 2013 Paul M. Kurowski SDC PUBLICATIONS Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com Visit the following websites

More information

Minimizing Run Time of Finite Element Analyses: Applications in Conformable CNG Tank Modeling

Minimizing Run Time of Finite Element Analyses: Applications in Conformable CNG Tank Modeling Michigan Technological University Digital Commons @ Michigan Tech Dissertations, Master's Theses and Master's Reports 2017 Minimizing Run Time of Finite Element Analyses: Applications in Conformable CNG

More information

Learning Module 8 Shape Optimization

Learning Module 8 Shape Optimization Learning Module 8 Shape Optimization What is a Learning Module? Title Page Guide A Learning Module (LM) is a structured, concise, and self-sufficient learning resource. An LM provides the learner with

More information

Engineering Analysis with SolidWorks Simulation 2012

Engineering Analysis with SolidWorks Simulation 2012 Engineering Analysis with SolidWorks Simulation 2012 Paul M. Kurowski SDC PUBLICATIONS Schroff Development Corporation Better Textbooks. Lower Prices. www.sdcpublications.com Visit the following websites

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

Die Wear Profile Investigation in Hot Forging

Die Wear Profile Investigation in Hot Forging Die Wear Profile Investigation in Hot Forging F. R. Biglari, M Zamani Abstract In this study, the wear profile on the die surface during the hot forging operation for an axisymmetric cross-section is examined.

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

D DAVID PUBLISHING. Stability Analysis of Tubular Steel Shores. 1. Introduction

D DAVID PUBLISHING. Stability Analysis of Tubular Steel Shores. 1. Introduction Journal of Civil Engineering and Architecture 1 (216) 563-567 doi: 1.17265/1934-7359/216.5.5 D DAVID PUBLISHING Fábio André Frutuoso Lopes, Fernando Artur Nogueira Silva, Romilde Almeida de Oliveira and

More information

Abaqus CAE Tutorial 6: Contact Problem

Abaqus CAE Tutorial 6: Contact Problem ENGI 7706/7934: Finite Element Analysis Abaqus CAE Tutorial 6: Contact Problem Problem Description In this problem, a segment of an electrical contact switch (steel) is modeled by displacing the upper

More information

Chapter 1 Introduction

Chapter 1 Introduction Chapter 1 Introduction GTU Paper Analysis (New Syllabus) Sr. No. Questions 26/10/16 11/05/16 09/05/16 08/12/15 Theory 1. What is graphic standard? Explain different CAD standards. 2. Write Bresenham s

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

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

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

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

ANSYS AIM Tutorial Stepped Shaft in Axial Tension

ANSYS AIM Tutorial Stepped Shaft in Axial Tension ANSYS AIM Tutorial Stepped Shaft in Axial Tension Author(s): Sebastian Vecchi, ANSYS Created using ANSYS AIM 18.1 Contents: Problem Specification 3 Learning Goals 4 Pre-Analysis & Start Up 5 Calculation

More information

LETTERS TO THE EDITOR

LETTERS TO THE EDITOR INTERNATIONAL JOURNAL FOR NUMERICAL AND ANALYTICAL METHODS IN GEOMECHANICS, VOL. 7, 135-141 (1983) LETTERS TO THE EDITOR NUMERICAL PREDICTION OF COLLAPSE LOADS USING FINITE ELEMENT METHODS by S. W. Sloan

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

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

Comparative Study of Topological Optimization of Beam and Ring Type Structures under static Loading Condition

Comparative Study of Topological Optimization of Beam and Ring Type Structures under static Loading Condition Comparative Study of Topological Optimization of Beam and Ring Type Structures under static Loading Condition Vani Taklikar 1, Anadi Misra 2 P.G. Student, Department of Mechanical Engineering, G.B.P.U.A.T,

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

Workshop 15. Single Pass Rolling of a Thick Plate

Workshop 15. Single Pass Rolling of a Thick Plate Introduction Workshop 15 Single Pass Rolling of a Thick Plate Rolling is a basic manufacturing technique used to transform preformed shapes into a form suitable for further processing. The rolling process

More information

Strength of Overlapping Multi-Planar KK Joints in CHS Sections

Strength of Overlapping Multi-Planar KK Joints in CHS Sections Strength of Overlapping Multi-Planar KK Joints in CHS Sections Peter Gerges 1, Mohamed Hussein 1, Sameh Gaawan 2 Structural Engineer, Department of Structures, Dar Al-Handasah Consultants, Giza, Egypt

More information

Scientific Manual FEM-Design 17.0

Scientific Manual FEM-Design 17.0 Scientific Manual FEM-Design 17. 1.4.6 Calculations considering diaphragms All of the available calculation in FEM-Design can be performed with diaphragms or without diaphragms if the diaphragms were defined

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

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

Numerical simulation of tunnel construction in volcanic rocks

Numerical simulation of tunnel construction in volcanic rocks Numerical simulation of tunnel construction in volcanic rocks G. Beer, Ch. Duenser Graz University of Technology, Graz, Austria ABSTRACT: For the design of tunnels, numerical simulation plays an important

More information