THREE-DIMENSIONAL VS. TWO-DIMENSIONAL FINITE ELEMENT MODELING OF FLIP CHIP PACKAGES
|
|
- Lionel Stephens
- 6 years ago
- Views:
Transcription
1 THREE-DIMENSIONAL VS. TWO-DIMENSIONAL FINITE ELEMENT MODELING OF FLIP CHIP PACKAGES Qizhou Yao and Jianmin Qu G.W. Woodruff School of Mechanical Engineering Georgia Institute of Technology Atlanta, GA Revised December 1998 To Appear in J. Electronic Packaging 1
2 THREE-DIMENSIONAL VS. TWO-DIMENSIONAL FINITE ELEMENT MODELING OF FLIP CHIP PACKAGES Qizhou Yao and Jianmin Qu G.W. Woodruff School of Mechanical Engineering Georgia Institute of Technology Atlanta, GA Abstract In this study, both two-dimensional and three-dimensional finite element analyses were used to study the stress distribution in and deflection of the flip chip assembly under thermal loading. It is found that the three-dimensional results compared favorably with experimental measurements, while the two-dimensional results consistently overestimate both stresses and deflection. Among the two-dimensional models, the plane stress assumption seems to yield results closer to the full three-dimensional predictions. Furthermore, three-dimensional models were used to investigate the effect of printed wiring board size on the overall deflection of the flip-chip assembly. This size effect of the printed wiring board has significant implications on the design of multi-chip modules. The results indicate that a square array placement pattern is preferable to a staggered array for multiple chip modules in order to reduce mechanical interaction between chips. For square arrays, such mechanical interaction between chips can be neglected when the minimum distance between adjacent chips is more than 2 times the chip size. Introduction Flip chip attach (FCA) technology is expected to grow at an accelerated rate in the near future, and it is going to constitute a large portion of the microelectronics industry as the next century comes (Wesselmann, 1996). More and more evidence shows that FCA is an appealing way to implement multi-chip module (MCM) technology (Baker, 1996). However, the 2
3 coefficient of thermal expansion (CTE) mismatch between the printed wiring board (PWB) and the silicon chip introduces a new concern. Under processing or operating conditions, the CTE mismatch not only subjects the solder joints to extremely large strains, but it also causes the overall bending of the flip chip assembly. Such CTE mismatch-induced stresses, manifested by the increasing die size and temperature excursions, poses a great challenge to the thermomechanical reliability of FCA packages. Although the introduction of a rigid encapsulant layer between the chip and the substrate has considerably enhanced the solder fatigue life, thermomechanical reliability issues still exist. Failure analysis of flip chip devices subjected to thermal shock testing has revealed that the typical failure mode is delamination at the encapsulant/chip interface, followed shortly by fatigue failure of the flip chip solder joints. It should be noted that failure often initiates at the outside perimeter of the chip. Once adhesion between these two surfaces is lost, the flip chip joints are subjected directly to the strain resulting from the thermal mismatch of the chip and the board. Electrical failure is the result of solder fatigue cracking. The number of thermal shock cycles that can be tolerated before this failure mechanism occurs has been found to vary and to be dependent on the materials in the assembly and their respective mechanical and chemical properties. And more importantly, it depends on the stresses in the FCA assembly. There are at least two major systems of thermal stresses and strains acting on the solder joints and encapsulant. The first system is due to the local CTE mismatch between the adjacent components. This is of particular concern at the chip-encapsulant and PWB-encapsulant interfaces where the large interfacial shear stresses act as a driving force for encapsulant delamination. The second system is due to the global CTE mismatch between the silicon chip and the PWB. The overall bending stems largely from this global CTE mismatch. To prevent 3
4 premature thermomechanical failure and to ensure the reliability of a FCA package, these thermomechanical stresses, which are the primary driving force to failure, must be understood. Furthermore, design and processing technologies must be developed to minimize such stresses. Due to its geometrical and material complexity, analytical solutions to the stress distribution in a FCA assembly are often unattainable. Numerical methods, such as the finite element method (FEM), have been used extensively to analyze the stresses, strains and deformations in FCA (LeGall, 1996; Schubet, 1997; Iannuzzelli, 1996). However, very few of these studies used three-dimensional (3D) FEM models (Lee, 1997). For example, Dasgupta et. al. (1997) compared 3D model with both sector model and 2D model, found that stress results for the sector model are not comparable with those for the 3D 1/8 model when PWB warpage is a significant factor, and the solder joint fatigue life predicted by 2D model is several times higher than that predicted by 3D models. In most cases, either the plane stress or the plane strain assumption is used to simplify the calculation. Inevitably, the use of such two-dimensional simplifications introduces errors in the predicted results. For example, within the framework of 2D modeling, it is well known that the thermal stress and deformation of silicon die are independent of the PWB size. However, this is not true in a real 3D assembly, since the deformation resistance increases with increasing PWB size due to the 3D constrain effects. This PWB size dependency of the stress and deformation is of great interest, for it is necessary to understand the mechanical interactions between adjacent chips mounted on the same board, so that a guideline for multi-chip design may be provided. The objectives of this paper are (1) to develop a 3D FEM model for the flip-chip assembly and validate the model with experimental data, (2) to investigate the difference between the 2D 4
5 and 3D FEM predictions, and (3) to understand the PWB size effect on the overall wrapage, and its implications on packaging design. Finite Element Modeling The model assembly used in this study consists of a Sandia ATC04 (SNL, 1993; Peterson, 1997) stress chip directly attached to a FR-4 substrate. The chip is a 6.35x6.35 mm 2 silicon die with 35 I/O's. For the baseline model schematically shown in Fig. 1, the substrate is a 9x9 mm 2 FR-4 PWB. To compare the 2D and 3D results, three FEM models were constructed, namely, 2D plane stress, 2D plane strain and full 3D. Due to symmetry, only one-half and one-eighth of the assembly (see Figs. 2-3) were needed for the 2D and 3D models, respectively. The 4-node plane strain elements and the plane stress quadrilateral elements were used, respectively, in the 2D plane strain and plane stress analyses, while the 4-node linear tetrahedron elements were used in the 3D analysis. Mesh refinement was conducted to ensure the convergence of numerical results. It was found that satisfactory accuracy can be achieved using elements with nodes in the 2D case and elements with 5305 nodes in the 3D case. The finite element calculations were carried out by ABAQUS Standard version 5.5. Six different materials were considered in the finite element models. They are the silicon chip, FR-4 substrate (PWB), encapsulant (underfill, Hysol 4520), solder mask, eutectic solder (63Sn/37Pb, wt.%) and copper solder pads. Although the materials were assumed linearly elastic, their properties were considered to be temperature dependent, as given in Tables 1-6 (LeGall, 1996). Furthermore, silicon chip, underfill, solder, copper and solder mask were assumed to be isotropic, while the FR-4 substrate was treated as an orthotropic material. The silica filler loaded in the Hysol 4520 underfill makes the underfill a composite material in nature. However, due to the fine spherical silica particle size, it is justifiable to treat the underfill as 5
6 isotropic material with calculated effective properties. More comprehensive evaluation of the underfill properties can be found in ref. (Hu, 1997). For the purpose of the comparison of 2D and 3D modeling, the complicated filler settling effect is not considered. Caution should be taken when the main interest is in the underfill material, as a resin rich top layer and a filler rich bottom layer result in different local material properties. To study the PWB size effect, two additional 3D models were constructed with the same die size (6.35x6.35 mm 2 ), but with different PWB sizes of 16x16 mm 2 and 24x24 mm 2, respectively. In those models, the silicon die, the PWB and the solder mask were treated the same as in the baseline models discussed in previous paragraphs. The under-die material, however, was considered as an homogeneous material with its effective properties determined from the mixiture of underfill and solder joints by using the Mori-Tanaka Method (Mura, 1991) and the rule of mixture, see the Appendix. Values of the effective properties are listed in Table 7. It is seen that the effective properties of the underfill-solder mixture are not much different from those of the underfill itself, for the solder constitutes less than 10% of the total under-die material volume. By using such effective properties, the computational time is significantly reduced since modeling of individual solder joints is avoided. Although such simplification may not yield accurate results for stress distribution within the individual solder joints, it will not affect the overall deformation of the assembly. Therefore, it is justifiable to homogenize the under-die solder/underfill mixiture, since our interest for this portion of the study is to investigate the overall warpage of the assembly. In all finite element models, the assembly was assumed stress-free at the typical reflow temperature of C. Thermal load is applied by cooling the assembly from C to 20 0 C. For comparison with experimental data, stress distributions at the intermediate temperatures 74 6
7 0 C and 36 0 C were also obtained. For simplicity, uniform temperature distribution was assumed throughout the analysis. Validation of the FEM Results To validate the FEM model, numerical predictions of the stress distribution during cool down were compared with experimental data (Palaniappan, 1997). Figs. 4a - 4b show the comparison between the 3D FEM results and experimental measurements for stress components σ xx, σ yy and σ xy at 74 0 C and 36 0 C post-underfill cure, respectively. The comparison was made at particular locations corresponding to points of experimental measurement near the active surface on the silicon die. It is seen from these figures that the numerical results compare very well with the experimental data, considering that not a single parameter was used to adjust any of the data. This comparison of the stress distributions indicates that the 3D FEM model developed here provides a reasonably accurate prediction of the actual stress distribution and overall deformation of the FCA assembly. Before closing this section, it needs to be pointed out that, although every effort has been made to mimic the ACT04 test vehicle, some approximations had to be made. One is to idealize the shape of the encapsulant fillet which seems to affect the stress distribution in the assembly to a certain extent. The other is to assume that the silicon die is at a stress-free state before the encapsulant starts to cure at C. This seems to be reasonable because of the large compliance of the eutectic solder joints at the temperature close to its melting point, C. It is also worth mentioning that after the encapsulant is applied and cured, solder joints are no longer the dominant load bearer to couple the thermal mismatch between the die and the PWB. Instead, the rigid underfill encapsulant takes over. This is because the solder joints constitute less than 10% of the total under-die material (solder and underfill) volume. Therefore, the effective 7
8 properties of the under-die material are very similar to those of the underfill itself, see Table 5 and Table 7. 2D vs. 3D FEM Modeling To investigate the applicability and limitations of the 2D finite element analysis, comparisons were made between the stress distributions predicted by the 2D plane stress, the 2D plane strain and the full 3D finite element calculations. Figs. 5a - 5b show the contour plots of the distribution of the von Mises effective stress predicted by various models at 40 o C. For the 3D model, both normal and diagonal cross-sections are shown. The extreme values of the stresses are shown in Table 8. It is observed from these results that both the 2D plane strain and plane stress models yield an overall higher stress level than the 3D model does. The von Mises stress obtained from the 2D plane strain model is much higher than that obtained from the 3D model. Furthermore, in the 2D models, the 'hot spots', meaning locations with high stresses, are limited to silicon-solder interfaces. However, in the 3D models, the hot spots are found not only in the silicon-solder interface, but also in the encapsulant, at the corners of the silicon die, and the silicon-underfill interface. Therefore, results from the 3D model can better explain the observed failure modes in flip chip assemblies, such as cracks in silicon die and encapsulant, delamination in the siliconunderfill interface, and cracks in the silicon-solder interfaces. As for the von Mises stress, it seems that results from the plane stress model are closer to the 3D results than to the plane strain results. Since von Mises stress is a good characterization parameter for plastic deformation, one may therefore conclude that plane stress should yield better prediction for plasticity induced failure in comparison with plane strain assumptions. 8
9 In addition to the differences in stress distributions, the 2D and 3D models also predict significantly different overall deformation of the FCA assembly (warpage). Such comparisons are shown in Fig. 6 for the assembly at 20 0 C, where the deflection of the lower surface of the PWB along both a normal cross-section and a diagonal cross-section are plotted. It is seen that the 2D models give an overestimated deformation, which is consistent with the overestimated stresses discussed earlier. Between the 2D plane stress and 2D plane strain models, the results are not very different, although the former seems to be a slightly better approximation. Effects of the PWB Size To investigate the effect of PWB size on the overall assembly warpage, the deformation of three assemblies with PWB sizes ranging from 9x9, 16x16 to 24x24 mm 2 was considered. Shown in Fig. 7a is the deflection curve along a normal cross-section of the die for different PWB sizes. It is seen that the die deflection is almost identical for all the PWB sizes considered. One may then conclude that as far as the stresses in the silicon die are concerned, PWB size effects may be negligible. However, deformation of the PWB outside the die is significantly affected by the overall PWB size. Shown in Figs. 7b 7c are the deflection curves of the PWB along a normal crosssection and a diagonal cross-section, respectively. It is seen that the portion outside the silicon die deforms differently for different PWB sizes, while the portion under the die is almost identical for all PWB sizes. The 3D deformed shape of the PWB is shown in Fig. 8a for the 9x9 mm 2 and in Fig. 9a for the 24x24 mm 2. These deformed surfaces are obtained by plotting the deformed z-coordinates of all nodes located on the lower surface of the PWB. 9
10 Note that there is an inflection region near the corners. This can be seen from the diagonal cross section deflection curve in Fig. 6 and the deformed shape in Fig 9a. The particular shape of the encapsulant at corners of the silicon die is believed to be responsible for this inflection. Two encapsulant fillets on two perpendicular sides of the silicon die join at this point forming an extended sharp ridge, which prevents the overhang of the PWB from free bending in the z- direction while the shrinkage in the x-y plane still exists. The cause of this inflection is the substantial z-direction CTE mismatch between the encapsulant and PWB. Finally, it is observed that the contour density beyond the silicon die area is much more uniform in the normal direction than in the diagonal direction, as seen from Fig 8b and Fig. 9b. This indicates that the curvature is greater in the diagonal direction. Therefore, for designing multi-chip modules, placing multiple chips in staggered array should be avoided because this type of placement produces maximum mechanical interaction between the chips. In addition, to avoid mechanical interaction, the minimum distance between adjacent dies should be approximately 1.8 times the die size (for the PWB used in this study). If other design specifics require a staggered array or closer distances between chips, then the mechanical interaction must be considered. That is, the influence of the deformation of the PWB produced by one die on the reliability of other chips needs to be considered. Concluding Remarks In this study, both two-dimensional and three-dimensional finite element analyses were used to study the stress distribution in and deflection of the flip chip assembly under thermal loading. The following conclusions were drawn. 10
11 (i) By comparing the numerical results with experimental data, it is demonstrated that the 3D finite element analysis based on thermoelasticity theory provides a reasonably accurate tool for stress analysis in FCA. (ii) 2D plane stress and plane strain models yield similar results. Both over estimate the deformation and stresses in FCA, although plane stress seems to be a better model. (iii) As far as single chip modules are concerned, the size of the PWB has very little influence on the assembly stress and deformation. (iv) To reduce mechanical interaction between chips, a square array is preferable to a staggered array for multiple chip modules. For square arrays, such mechanical interaction between chips can be neglected when the minimum distance between two chips is more than 2 times the chip size. Acknowledgments The research was supported by the National Science Foundation through the Packaging Research Center at Georgia Tech. References Baker, D. and Kao, V., 1996, MCMs Take Off, Advanced Packaging, January/February, pp Dasgupta, A., et. al., 1997, Miscellaneous Modeling Issues in Thermomechanical Stress Analysis of Surface-Mount Interconnects, INTERPACK 97, Proc., EEP-Vol. 19-2, Ed. Suhir et. al., pp Hu, K.X., et al., 1997, Electo- thermo-mechanical responses of conductive adhesive systems, IEEE CPMT-A, Vol.20, pp Iannuzzelli, R. J., et al., 1996, Solder Joint Reliability Prediction by the Integrated Matrix Creep Method, J. of Electronic Packaging, Vol.118, pp
12 Lee, S. B. and Kim, J. K., 1997, A Mechanistic Model for Fatigue Life Prediction of Solder Joints for Electronic Packages, Int. J. Fatigue, Vol. 19, No. 1, pp LeGall, C.A., 1996, Thermalmechanical Stress Analysis of Flip Chip Packages, Master s thesis, School of Mechanical Engineering, Georgia Institute of Technology, Atlanta, GA. ed. Mura, T., 1991, Micromechanics of Defects in Solids, Kluwer Academic Publishers, 2nd Palaniappan, P. and Baldwin, D.F., 1997, Preliminary In-Process Stress Analysis of Flip- Chip Assemblies During Underfill, 30th International Symposium on Microelectronics, Philadelphia, PA. Peterson, D. W., et al., 1997, Stresses From Flip-Chip Assembly and Underfill; Measurements with the ATC4.1 Assembly Test Chip and Analysis by Finite Element Method, Proceedings of the 47th Electronic Components and Technology Conference, San Jose, CA, pp Qu, J., 1993, "Effects of Slightly Weakened Interfaces on the Overall Elastic Properties of Composite Materials," Mechanics of Materials, 14, pp Schubert, A., et al., 1997, Materials Mechanics and Mechanical Reliability of Flip Chip Assemblies on Organic Substrates. Proceedings of International Symposium on Advanced Packaging Materials, pp SNL (Sandia National Laboratories), 1993, Assembly Test Chip Ver. 04 (ACT04) Description and User s Guide. Wesselmann, C., 1996, Flip Chip Off the Dime?, Advanced Packaging, March/April, pp.7. 12
13 Table 1. Material properties of silicon Temperature ( 0 C) Tensile Modulus (GPa) α (10-6 / 0 C) Poisson s Ratio, ν
14 Table 2. Material properties of FR-4 PWB Property 30 0 C 95 0 C C C E 1 (GPa) E 2 (GPa) E 3 (GPa) G 12 (GPa) G 13 (GPa) G 23 (GPa) ν ν ν α 1 (10-6 / 0 C) α 2 (10-6 / 0 C) α 3 (10-6 / 0 C)
15 Table 3. Material properties of solder (63 Sn/37Pb) Temperature ( 0 C) Tensile Modulus (GPa) α (10-6 / 0 C) Poisson s Ratio, ν
16 Table 4. Material properties of copper pad Temperature ( 0 C) Tensile Modulus (GPa) α (10-6 / 0 C) Poisson s Ratio, ν
17 Table 5. Material properties of underfill (Hysol 4520) Temperature ( 0 C) Tensile Modulus (GPa) α (10-6 / 0 C) Poisson s Ratio, ν
18 Table 6. Material properties of solder mask Temperature ( 0 C) Tensile Modulus (GPa) α (10-6 / 0 C) Poisson s Ratio, ν
19 Table 7. Effective properties of the under-die solder-underfill mixture Temperature ( 0 C) Tensile Modulus (GPa) α (10-6 / 0 C) Poisson s Ratio, ν
20 Table 8. Maximum stresses and their corresponding locations Stresses (MPa) 2D Plane Strain (xy) 2D Plane Stress (xy) σ xx Location B A B A B A σ yy Location F E all all B A σ zz Location D C B C H, E C τ xz Location B A G A E H τ yz Location I E τ xy 16 Location σ (Mises) Location E B A, B A Solder side of die-solder interface B Die side of die-solder interface C Upper corner of the encapsulant fillet D Solder joints E Copper pads F Solder mask G Underfill side of die-underfill interface near the joints H Lower corner of the die I Upper corner of the die 3D B 20
21 Appendix: Effective Properties of the Under-Die Solder-Underfill Mixture The mixture of underfill and solder joints between the die and the substrate can be viewed as a composite material. The solders can be considered cylindrical with the axis in the z-direction. Therefore, effective properties of the mixture can be assumed transversely isotropic with the axis of symmetry in the z-direction. Making use of the Mori-Tanaka method (Mura, 1991), the effective properties in the x-y plane can be estimated as 9Kµ E =, 3K + µ 1 E ν = -, (A.1) 2 6K where µ = µ 0 Ø Œ1 + º µ 0 + c( µ 1 - µ 0) 2δ (1- c)( µ 1 - ø µ ) œ 0 ß, (A.2) K = K 0 Ø Œ1 + º K 0 + c( K1 - K0) 3γ (1- c)( K - 1 ø K ) œ 0 ß, (A.3) µ n = En (1+ ν ), 2 n K n = En (1-2ν ), n = 0, 1. (A.4) 3 n In the above equations, c is the solder volume fraction of the entire under-die mixture, and ν n are, respectively, the Young's modulus and Poisson's ratio for the underfill material (n = 0) and for the solder materials (n = 1). The non-dimensional constants δ and γ are related to the underfill properties through (Qu, 1993) E n, 3+ 4ν 0 3 4ν 0 δ =, γ =. (A.5) 24(1 ν ) 8(1 ν )
22 The values listed in Table 7 were computed from (A.1). As for the effective properties in the z-direction, the rule of mixture can be used, E = ce ( - E, (A.6) c) 0 ν = cν ( ν. (A.7) c) 0 22
23 Figure Captions Fig. 1 Fig. 2 Fig. 3 Fig. 4a Fig. 4b Baseline configuration of the flip-chip under consideration. Two-dimensional finite element model (one half). Three-dimensional finite element model (one eighth). Comparison of stresses between numerical results and experimental measurements at 74 0 C. Comparison of stresses between numerical results and experimental measurements at 36 0 C. Fig. 5a von Mises stress contour from 2D analysis at 40 0 C. Fig. 5b von Mises stress contour from 3D analysis at 40 0 C. Fig. 6 Fig. 7a Fig. 7b Fig. 7c Fig. 8a Deflection of the lower surface of the PWB along either a normal cross-section or a diagonal cross-section at 20 0 C. Top surface deflection of the silicon die along a normal cross-section for various PWB sizes at 20 0 C. Lower surface deflection of the PWB along a normal cross-section for various PWB sizes at 20 0 C. Lower surface deflection of the PWB along a diagonal cross-section for various PWB sizes at 20 0 C. Deformed shape of the PWB of 9x9 mm 2 at 20 0 C Fig. 8b z-contour plot (µm) for the lower surface of the PWB of 9x9 mm 2 at 20 0 C. Fig. 9a Deformed shape of the PWB of 24x24 mm 2 at 20 0 C. Fig. 9b z-contour plot (µm) for the lower surface of the PWB of 24x24 mm 2 at 20 0 C. 23
24 Fig. 1 Baseline configuration of the flip-chip under consideration. 24
25 3.175 mm 0.60 mm z 0.61 mm x 4.50 mm Fig. 2 Two-dimensional finite element model (one half). 25
26 Z X Y Fig. 3 Three-dimensional finite element model (one eighth). 26
27 Stress (MPa) σ xx, Num. σ xx, Exp. σ yy, Num. σ yy, Exp. σ xy, Num. σ xy, Exp. chip A B C D E F G Location A B C G D E F Fig. 4a Comparison of stresses between numerical results and experimental measurements at 74 0 C. 27
28 Stress (MPa) σ xx, Num. σ xx, Exp. σ yy, Num. σ yy, Exp. σ xy, Num. σ xy, Exp. chip A B C D E F G A B C G D E F Location Fig. 4b Comparison of stresses between numerical results and experimental measurements at 36 0 C. 28
29 plane strain plane stres Fig. 5a von Mises stress contour from 2D analysis at 40 0 C. 29
30 diagonal cross-section normal cross Fig. 5b von Mises stress contour from 3D analysis at 40 0 C. 30
31 0 Deflection (µm) D Normal 3D Diagonal 2D Plane Strain 2D Plane Stress Distance from the Chip Center (mm) Fig. 6 Deflection of the lower surface of the PWB along either a normal cross-section or a diagonal cross-section at 20 0 C. 31
32 0-2 Deflection (µm) -4-6 PWB Size = 9X9 mm 2 PWB Size = 16X16 mm 2 PWB Size = 24X24 mm Distance from the Chip Center (mm) Fig. 7a Top surface deflection of the silicon die along a normal cross-section for various PWB sizes at 20 0 C. 32
33 0 Deflection (µm) PWB Size = 9X9 mm 2 PWB Size = 16X16 mm 2 PWB Size = 24X24 mm Distance from the Chip Center (mm) Fig. 7b Lower surface deflection of the PWB along a normal cross-section for various PWB sizes at 20 0 C. 33
34 0 Deflection (µm) PWB Size = 9X9 mm 2 PWB Size = 16X16 mm 2 PWB Size = 24X24 mm Distance from the Chip Center (mm) Fig. 7c Lower surface deflection of the PWB along a diagonal cross-section for various PWB sizes at 20 0 C. 34
35 Deflection (µm) x-coordinate (mm) y-coordinate (mm) Fig. 8a Deformed shape of the PWB of 9x9 mm 2 at 20 0 C. 35
36 6 y-coordinate (mm) x-coordinate (mm) Fig. 8b z-contour plot (µm) for the lower surface of the PWB of 9x9 mm 2 at 20 0 C. 36
37 0-20 Deflection (µm) x-coordinate (mm) y-coordinate (mm) Fig. 9a Deformed shape of the PWB of 24x24 mm 2 at 20 0 C. 37
38 y-coordinate (mm) x-coordinate (mm) Fig. 9b z-contour plot (µm) for the lower surface of the PWB of 24x24 mm 2 at 20 0 C. 38
Improvement of ELK Reliability in Flip Chip Packages using Bond-on-Lead (BOL) Interconnect Structure
Improvement of ELK Reliability in Flip Chip Packages using Bond-on-Lead (BOL) Interconnect Structure by Eric Ouyang, MyoungSu Chae, Seng Guan Chow, Roger Emigh, Mukul Joshi, Rob Martin, Raj Pendse STATS
More informationCHAPTER 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 informationCorrelated Model For Wafer Warpage Prediction of Arbitrarily Patterned Films
2018 IEEE 68th Electronic Components and Technology Conference Correlated Model For Wafer Warpage Prediction of Arbitrarily Patterned Films Gregory T. Ostrowicki gtostrowicki@ti.com Siva P. Gurum sgurrum@ti.com
More informationChapter 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 informationNumerical analysis on thermal characteristics for chip scale package by integrating 2D/3D models
INTERNATIONAL JOURNAL OF NUMERICAL MODELLING: ELECTRONIC NETWORKS, DEVICES AND FIELDS Int. J. Numer. Model. 2009; 22:43 55 Published online 1 September 2008 in Wiley InterScience (www.interscience.wiley.com)..694
More informationRevised 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 informationTHE 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 information2D Finite Element Analysis ofigbt Solder Joint
2D Finite Element Analysis ofigbt Solder Joint Hua Lui", Chris Bailey Department of Mathematical Sciences, University of Greenwich 30 Park Row, London, SElO 9L S, UK. Email: H.Lu@gre.ac.uk Abstract-2D
More information3D 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 informationME 475 FEA of a Composite Panel
ME 475 FEA of a Composite Panel Objectives: To determine the deflection and stress state of a composite panel subjected to asymmetric loading. Introduction: Composite laminates are composed of thin layers
More informationModularized & parametric modeling methodology.
Modularized & parametric modeling methodology. Active Device Passive Device Vias Foot print Lid Wall floor PWB Ceramic Taxonomy Technique Mechanical Component Library Analysis model Thermal Structural
More informationThermo Mechanical Modeling of TSVs
Thermo Mechanical Modeling of TSVs Jared Harvest Vamsi Krishna ih Yaddanapudi di 1 Overview Introduction to Through Silicon Vias (TSVs) Advantages of TSVs over wire bonding in packages Role of TSVs in
More informationAssignment in The Finite Element Method, 2017
Assignment in The Finite Element Method, 2017 Division of Solid Mechanics The task is to write a finite element program and then use the program to analyse aspects of a surface mounted resistor. The problem
More informationES 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 information3-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 informationCHAPTER 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 informationA 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 informationDie 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 informationFINITE ELEMENT MODELLING AND ANALYSIS OF WORKPIECE-FIXTURE SYSTEM
FINITE ELEMENT MODELLING AND ANALYSIS OF WORKPIECE-FIXTURE SYSTEM N. M. KUMBHAR, G. S. PATIL, S. S. MOHITE & M. A. SUTAR Dept. of Mechanical Engineering, Govt. College of Engineering, Karad, Dist- Satara,
More informationKrzysztof Dabrowiecki, Probe2000 Inc Southwest Test Conference, San Diego, CA June 08, 2004
Structural stability of shelf probe cards Krzysztof Dabrowiecki, Probe2000 Inc Southwest Test Conference, San Diego, CA June 08, 2004 Presentation Outline Introduction Objectives Multi die applications
More informationEmbedded 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 informationExercise 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 informationA 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 informationValidation Report: Additional Data Mapping to Structural Analysis Packages
Autodesk Moldflow Structural Alliance 2012 Validation Report: Additional Data Mapping to Structural Analysis Packages Mapping process-induced stress data from Autodesk Moldflow Insight Dual Domain and
More informationANSYS 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 informationVOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL
VOLCANIC DEFORMATION MODELLING: NUMERICAL BENCHMARKING WITH COMSOL The following is a description of the model setups and input/output parameters for benchmarking analytical volcanic deformation models
More informationENHANCED STRUCTURE CAE SOLUTION WITH MOLDING EFFECT FOR AUTOMOTIVE PARTS
ENHANCED STRUCTURE CAE SOLUTION WITH MOLDING EFFECT FOR AUTOMOTIVE PARTS Allen Y. Peng*, Wen-Hsien Yang, David C. Hsu CoreTech System Co., Ltd., HsinChu, Taiwan, ROC Abstract An increasing number of automotive
More informationA 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 informationQuantifying Three-Dimensional Deformations of Migrating Fibroblasts
45 Chapter 4 Quantifying Three-Dimensional Deformations of Migrating Fibroblasts This chapter presents the full-field displacements and tractions of 3T3 fibroblast cells during migration on polyacrylamide
More informationTOOLS TO ASSESS THE ATTACHMENT RELIABILITY OF MODERN SOLDERED ASSEMBLIES (BGA, CSP...)
TOOLS TO ASSESS THE ATTACHMENT RELIABILITY OF MODERN SOLDERED ASSEMBLIES (BGA, CSP...) by Jean-Paul Clech, EPSI Inc., Montclair, NJ, USA, (973)746-3796, jpclech@aol.com [Paper appeared in Proceedings,
More informationExample 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 informationPurdue e-pubs. Purdue University. Jeongil Park Samsung Electronics Co. Nasir Bilal Purdue University. Douglas E. Adams Purdue University
Purdue University Purdue e-pubs International Compressor Engineering Conference School of Mechanical Engineering 26 Development of a Two-Dimensional Finite Element Model of a Suction Valve for Reduction
More informationLGA vs. BGA: WHAT IS MORE RELIABLE? A2 nd LEVEL RELIABILITY COMPARISON
LGA vs. BGA: WHAT IS MORE RELIABLE? A2 nd LEVEL RELIABILITY COMPARISON Ahmer Syed and Robert Darveaux Amkor Technology 1900 S. Price Road Chandler, AZ 85226 (480)821-5000 asyed@amkor.com ABSTRACT A recent
More informationMicro to Macro Thermo- Mechanical Simulation of Wafer Level Packaging
Chang-An Yuan Research Assistant Kou-Ning Chiang Professor e-mail: knchiang@pme.nthu.edu.tw Department of Power Mechanical Engineering, National Tsing Hua University, 101, Sec. 2, Kuang-Fu Rd., HsinChu
More informationCHAPTER 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 informationAufgabe 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 informationENGINEERING TRIPOS PART IIA FINITE ELEMENT METHOD
ENGINEERING TRIPOS PART IIA LOCATION: DPO EXPERIMENT 3D7 FINITE ELEMENT METHOD Those who have performed the 3C7 experiment should bring the write-up along to this laboratory Objectives Show that the accuracy
More informationModule 1.7: Point Loading of a 3D Cantilever Beam
Module 1.7: Point Loading of a D Cantilever Beam Table of Contents Page Number Problem Description Theory Geometry 4 Preprocessor 6 Element Type 6 Material Properties 7 Meshing 8 Loads 9 Solution 15 General
More informationThe 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 informationEffect of Substrate Flexibility on Solder Joint Reliability
CHAPTER IV Effect of Substrate Flexibility on Solder Joint Reliability 4.1 Introduction Flex substrate is very popular in electronics industry. Flex circuit packaging, a wellestablished technology that
More informationME 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 informationAkrometrix Testing Applications
Akrometrix Optical Techniques: Akrometrix Testing Applications Three full-field optical techniques, shadow moiré, digital image correlation (DIC), and fringe projection (performed by the DFP) are used
More informationIJMH - 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 informationAutodesk Moldflow Insight AMI Undeerfill Encapsulation
Autodesk Moldflow Insight 2012 AMI Undeerfill Encapsulation Revision 1, 22 March 2012. This document contains Autodesk and third-party software license agreements/notices and/or additional terms and conditions
More informationStress analysis of toroidal shell
Stress analysis of toroidal shell Cristian PURDEL*, Marcel STERE** *Corresponding author Department of Aerospace Structures INCAS - National Institute for Aerospace Research Elie Carafoli Bdul Iuliu Maniu
More informationFully-Coupled Thermo-Mechanical Analysis
Fully-Coupled Thermo-Mechanical Analysis Type of solver: ABAQUS CAE/Standard Adapted from: ABAQUS Example Problems Manual Extrusion of a Cylindrical Aluminium Bar with Frictional Heat Generation Problem
More informationFE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS
Proceedings of ICAD26 FE ANALYSES OF STABILITY OF SINGLE AND DOUBLE CORRUGATED BOARDS ICAD-26-43 Enrico Armentani enrico.armentani@unina.it University of Naples P.le V. Tecchio, 8 8125 Naples Italy Francesco
More informationCase 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 informationAdaptive Power Blurring Techniques to Calculate IC Temperature Profile under Large Temperature Variations
Adaptive Techniques to Calculate IC Temperature Profile under Large Temperature Variations Amirkoushyar Ziabari, Zhixi Bian, Ali Shakouri Baskin School of Engineering, University of California Santa Cruz
More information2: 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 informationEXACT 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 informationSimulation 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 informationSOLIDWORKS Simulation Avoiding Singularities
SOLIDWORKS Simulation Avoiding Singularities What is a Singularity? A singularity is a function s divergence into infinity. SOLIDWORKS Simulation occasionally produces stress (or heat flux) singularities.
More informationTop Layer Subframe and Node Analysis
Top Layer Subframe and Node Analysis By Paul Rasmussen 2 August, 2012 Introduction The top layer of the CCAT backing structure forms a critical interface between the truss and the primary subframes. Ideally
More informationCOMPUTER 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 informationChapter 7 Practical Considerations in Modeling. Chapter 7 Practical Considerations in Modeling
CIVL 7/8117 1/43 Chapter 7 Learning Objectives To present concepts that should be considered when modeling for a situation by the finite element method, such as aspect ratio, symmetry, natural subdivisions,
More informationFinite Element Analysis and Optimization of I.C. Engine Piston Using RADIOSS and OptiStruct
Finite Element Analysis and Optimization of I.C. Engine Piston Using RADIOSS and OptiStruct Vivek Zolekar Student M. Tech. Mechanical (CAD/CAM) SGGSIE&T Nanded - 431 606 Dr. L.N. Wankhade Professor Department
More informationANSYS 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 informationAn optimization method for generating self-equilibrium shape of curved surface from developable surface
25-28th September, 2017, Hamburg, Germany Annette Bögle, Manfred Grohmann (eds.) An optimization method for generating self-equilibrium shape of curved surface from developable surface Jinglan CI *, Maoto
More informationTWO-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 informationComparative 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 informationExercise 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 informationExercise 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 informationA NUMERICAL SIMULATION OF DAMAGE DEVELOPMENT FOR LAMINATED WOVEN FABRIC COMPOSITES
A NUMERICAL SIMULATION OF DAMAGE DEVELOPMENT FOR LAMINATED WOVEN FABRIC COMPOSITES Tetsusei Kurashiki 1, Yujiro Momoji 1, Hiroaki Nakai 1, and Masaru Zako 1 1 Department of Management of Industry and Technology,
More informationExercise 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 informationNon-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 informationSIMULATION OF A DETONATION CHAMBER TEST CASE
SIMULATION OF A DETONATION CHAMBER TEST CASE Daniel Hilding Engineering Research Nordic AB Garnisonen I4, Byggnad 5 SE-582 10 Linköping www.erab.se daniel.hilding@erab.se Abstract The purpose of a detonation
More information1. Carlos A. Felippa, Introduction to Finite Element Methods,
Chapter Finite Element Methods In this chapter we will consider how one can model the deformation of solid objects under the influence of external (and possibly internal) forces. As we shall see, the coupled
More informationCONTACT STATE AND STRESS ANALYSIS IN A KEY JOINT BY FEM
PERJODICA POLYTECHNICA SER. ME CH. ENG. VOL. 36, NO. 1, PP. -15-60 (1992) CONTACT STATE AND STRESS ANALYSIS IN A KEY JOINT BY FEM K. VARADI and D. M. VERGHESE Institute of Machine Design Technical University,
More informationEffectiveness of Element Free Galerkin Method over FEM
Effectiveness of Element Free Galerkin Method over FEM Remya C R 1, Suji P 2 1 M Tech Student, Dept. of Civil Engineering, Sri Vellappaly Natesan College of Engineering, Pallickal P O, Mavelikara, Kerala,
More informationGuidelines 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 informationFinite Element Modal Analysis and Mesh Optimization of a Typical Turbo Fan Engine Fan Hub Frame
Finite Element Modal Analysis and Mesh Optimization of a Typical Turbo Fan Engine Fan Hub Frame Charles.G.Martin 1 and Dr. A. Arokkiaswamy 2 1,2 Department of Aeronautical Engg, DSCE, Shavige Malleshwara
More informationAn Efficient Sequential Approach for Simulation of Thermal Stresses in Disc Brakes
An Efficient Sequential Approach for Simulation of Thermal Stresses in Disc Brakes Asim Rashid 1, Niclas Strömberg 1 1 Jönköping University, SE-55111 Jönköping, Sweden Abstract In this paper an efficient
More informationPrint 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 informationAXIAL OF OF THE. M. W. Hyer. To mitigate the. Virginia. SUMMARY. the buckling. circumference, Because of their. could.
IMPROVEMENT OF THE AXIAL BUCKLING CAPACITY OF COMPOSITE ELLIPTICAL CYLINDRICAL SHELLS M. W. Hyer Department of Engineering Science and Mechanics (0219) Virginia Polytechnic Institute and State University
More informationModule 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 informationOptimal Support Solution for a Meniscus Mirror Blank
Preliminary Design Review Optimal Support Solution for a Meniscus Mirror Blank Opti 523 Independent Project Edgar Madril Scope For this problem an optimal solution for a mirror support is to be found for
More informationLocking-Free Smoothed Finite Element Method with Tetrahedral/Triangular Mesh Rezoning in Severely Large Deformation Problems
Locking-Free Smoothed Finite Element Method with Tetrahedral/Triangular Mesh Rezoning in Severely Large Deformation Problems Yuki ONISHI, Kenji AMAYA Tokyo Institute of Technology (Japan) P. 1 P. 1 Motivation
More informationMulti-Step Analysis of a Cantilever Beam
LESSON 4 Multi-Step Analysis of a Cantilever Beam LEGEND 75000. 50000. 25000. 0. -25000. -50000. -75000. 0. 3.50 7.00 10.5 14.0 17.5 21.0 Objectives: Demonstrate multi-step analysis set up in MSC/Advanced_FEA.
More informationASME 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 informationOffshore 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 informationBiography of Authors. September 5, 2014 ASTR 2014, Sep 10-12, St. Paul, MN 1
Biography of Authors Jingshi Meng is a PhD candidate from CALCE (Center for Advanced Life Cycle Engineering), University of Maryland. His doctoral research, advised by Professor Abhijit Dasgupta, focuses
More informationSimilar 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 informationScienceDirect. Vibration Response Prediction of the Printed Circuit Boards using Experimentally Validated Finite Element Model
Available online at www.sciencedirect.com ScienceDirect Procedia Engineering 144 (2016 ) 576 583 12th International Conference on Vibration Problems, ICOVP 2015 Vibration Response Prediction of the Printed
More informationMEAM 550 Modeling and Design of MEMS Spring Solution to homework #3. In our notation and values, k = = =
MEAM 550 Modeling and Design of MEMS Spring 004 Solution to homework # Problem 1 A fixed-guided beam (length = l, width = b, depth = h ) with a transverse tip load of F has the following formulas for maximum
More informationSimulation of a Steel Wire Straightening Taking into Account Nonlinear Hardening of Material
ETASR - Engineering, Technology & Applied Science Research Vol. 2, No. 6, 2012, 320-324 320 Simulation of a Steel Wire Straightening Taking into Account Nonlinear Hardening of Material Ilya Khromov Dept.
More informationIntroduction to the Finite Element Method (3)
Introduction to the Finite Element Method (3) Petr Kabele Czech Technical University in Prague Faculty of Civil Engineering Czech Republic petr.kabele@fsv.cvut.cz people.fsv.cvut.cz/~pkabele 1 Outline
More informationModule 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 informationCrane Hook Design and Analysis
Crane Hook Design and Analysis G Bhagyaraj 1, K Suryaprakash 2, K Subba Rao 3 1M.Tech. CAD/CAM, Godavari Institute of Engineering and Technology, Rajahmundry 2Associate Professor, Godavari Institute of
More informationISSN: ISO 9001:2008 Certified International Journal of Engineering and Innovative Technology (IJEIT) Volume 2, Issue 3, September 2012
Mitigation Curves for Determination of Relief Holes to Mitigate Concentration Factor in Thin Plates Loaded Axially for Different Discontinuities Shubhrata Nagpal, S.Sanyal, Nitin Jain Abstract In many
More informationNEW 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 informationTOLERANCE ALLOCATION IN FLEXIBLE ASSEMBLIES: A PRACTICAL CASE
TOLERANCE ALLOCATION IN FLEXIBLE ASSEMBLIES: A PRACTICAL CASE Pezzuti E., Piscopo G., Ubertini A., Valentini P.P. 1, Department of Mechanical Engineering University of Rome Tor Vergata via del Politecnico
More informationModule 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 informationThe Ohio State University Columbus, Ohio, USA Universidad Autónoma de Nuevo León San Nicolás de los Garza, Nuevo León, México, 66450
Optimization and Analysis of Variability in High Precision Injection Molding Carlos E. Castro 1, Blaine Lilly 1, José M. Castro 1, and Mauricio Cabrera Ríos 2 1 Department of Industrial, Welding & Systems
More informationLinear 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 informationUsing 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 informationChallenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure
Challenge Problem 5 - The Solution Dynamic Characteristics of a Truss Structure In the final year of his engineering degree course a student was introduced to finite element analysis and conducted an assessment
More informationStatic And Modal Analysis Of Rotating Wheel Rim Using Ansys
International Journal of Engineering Science Invention ISSN (Online): 2319 6734, ISSN (Print): 2319 6726 Volume 3 Issue 9 ǁ September 2014 ǁ PP.18-23 Static And Modal Analysis Of Rotating Wheel Rim Using
More informationCE Advanced Structural Analysis. Lab 4 SAP2000 Plane Elasticity
Department of Civil & Geological Engineering COLLEGE OF ENGINEERING CE 463.3 Advanced Structural Analysis Lab 4 SAP2000 Plane Elasticity February 27 th, 2013 T.A: Ouafi Saha Professor: M. Boulfiza 1. Rectangular
More informationApplication Note 5363
Surface Laminar Circuit (SLC) Ball Grid Array (BGA) Lead-free Surface Mount Assembly Application Note 5363 Introduction This document outlines the design and assembly guidelines for surface laminar circuitry
More information