Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections
|
|
- Martin Stewart
- 5 years ago
- Views:
Transcription
1 October 25, 2000 Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections Tommi Vanhala Helsinki Institute of Physics 1. INTRODUCTION STIFFNESS ANALYSES ENVELOPE BRACKET BOLT CONNECTIONS BRACKET TO TUBE BRACKET TO FOOT FOOT TO HCAL CONCLUSIONS REFERENCES...12 APPENDIX
2 1. Introduction The Tracker support tube is supported at its ends by four aluminium brackets that locate at the horizontal symmetry plane. The outer end of the bracket is attached to HCAL. The brackets must bear the load caused by the mass of the Tracker (estimated to be 4t) and the dimensional changes of HCAL due to its thermal expansion. The space for the bracket is very limited due to the ECAL, cooling pipes, cables etc. Therefore, the shape of the bracket cannot be optimized as one would probably like. The support bracket is made of three entities, Figure 1. The entities: banana, bracket and the foot are connected together with stainless A4-70 steel. The bolt joint must provide stable connection in all circumstances. The bolt joints are needed, because the components are mounted to CMS in different phases of assembly. The joints are also needed because of required assembly clearances. Figure 1. The entities of the Tracker support bracket. The components are not in scale. 2. Stiffness analyses The stiffness of the support bracket was analysed with finite element (FE) models in Ansys. The analysis was done in two parts. The preliminary stiffness calculations were done with the bracket envelope model. Later, the displacement was calculated with the more detailed bracket model. The different approach to defining the model was used. The geometry of the envelope model was created with 3D-modeling software. Instead of that, the bracket model was defined with keypoints in Ansys. The two modelling methods should give equivalent results despite the different look of the model. The bracket was modelled in both analyses as a single structure. Therefore, the stiffness calculations of the bolt connection between pieces are presented separately later in this paper. 2.1 Envelope The FE-model of the bracket envelope was based on the Euclid database drawing TL012287MQ made by Mr. Pierre-Benoit Brouze. The bracket is according to drawing an assembly of two aluminium pieces. The connection between the bracket and the Tracker support tube was not yet designed. The bracket was modelled as one solid piece for the FE-analysis. The shape of the envelope was simplified by neglecting small details such as curvatures, rounds etc. 2
3 The geometry of the bracket was modelled in Pro/Engineer 3D-modelling software, Figure 2. The dimensions were given in millimetres. An IGES-file containing the envelope surfaces was exported from ProE. Figure 2. The bracket envelope model in Pro/Engineer. The IGES-file was then imported into Ansys 5.6. Ansys creates a solid model of the imported model. It deletes small areas and merges coincident keypoints. The element type was chosen (SOLID95). SOLID95 is a 3-D 20-node structural solid element. It is a higher order version of the 3- D 8-node solid element (SOLID45). According to Ansys element manual the chosen element type tolerates irregular shapes without as much loss of accuracy. SOLID95 elements have compatible displacement shapes and are well suited to model curved boundaries. The element is defined by 20 nodes having three degrees of freedom per node: translations in the nodal x, y, and z directions. For the analysis, material properties for the aluminium bracket were defined (see Table 1) and the model was meshed, Figure 3. The rather coarse element mesh was used (smart element level 7). Table 1. Bracket material properties (aluminium) used in FE-model. Variable Symbol Young's modulus E [N/mm 2 ] Poisson's ratio Q 0.25 Density J 2700*10-9 [kg/mm 3 ] 3
4 Figure 3. A meshed bracket in Ansys. Then, boundary conditions, gravity and estimated load (a 10 kn load at the end of the bracket) were applied. All degrees of freedom (DOF) on the nodes at two attachment surfaces were fixed. The tube end of the bracket was free. The force was equally divided between 10 nodes at the end of the bracket. Finally, the FE-model was analysed. The solution was done without error notices. The displacement of the bracket envelope with the given load is presented in figures 4 and 5. The displacement is in millimetres. The nodal forces point to the negative Y-axis. The co-ordinate system of the bracket in the FE-analysis is illustrated in Figure 3. Please note that the system differs from the global co-ordinate system of the CMS Tracker. Figure 4. The total displacement of the bracket envelope in millimetres. 4
5 Figure 5. The vertical displacement of the bracket envelope in mm. 2.2 Bracket The further finite element study of the bracket stiffness was done with the more precise dimensions of the bracket. The geometry of the bracket model differs from the envelope model at the tube end of the bracket. The bracket is to be connected to the tube with three via a stiff aluminium banana. The banana was not modelled, but only its reaction force with the bracket is defined. The bracket displaces in the Y-direction due to the mass of the Tracker. HCAL and the Tracker support tube are assumed to have infinite stiffness. Due to the symmetry of the Tracker, the tube end of the bracket cannot displace either in the X- or in the Z-direction. These boundary conditions did not exist in the envelope model. The foot and the bracket were modelled again as a single solid piece. The geometry of the model was created by first defining keypoints, then connecting these by lines and finally creating areas from the lines. The element type used was SHELL63. The thickness of the bracket was defined to be 55 mm at the foot, 45 mm in the inclined part and 35 mm at the end of the bracket. The mass of the bracket without banana was calculated to weigh about 30 kg. All DOFs on the nodes at two attachment surfaces were fixed. Then, the vertical load was applied and the displacement at the tube end of the bracket in the X- and Z-directions were fixed. The support forces at the tube end of the bracket are -1.1 kn in the X-direction and 0.9 kn in the Z- direction. The effect of the thermal expansion of the HCAL on the forces in the bracket was also analysed. The bracket should adapt dimensional changes of HCAL, because the Tracker support tube should not be 5
6 stretched or squeezed. HCAL is mostly made of bras, whose coefficient of the thermal expansion is 20 Pm/mqC. The temperature change of the HCAL was estimated to be r2.5qc, at maximum. The 2.5qC temperature change would increase or decrease the total length of HCAL (6.090 m) by 304 Pm. Therefore, one half of HCAL expands 152 Pm. Correspondingly, the temperature change mentioned above increases the inner radius of HCAL (1.836 m) by 92 Pm. The displacement of the tube end of the bracket with respect to the foot was defined with the displacement boundary conditions. A 2.5qC thermal expansion creates 3.9 kn in the X- and -3.0 kn in the Z-direction support forces at the end of the bracket. The displacement of the bracket with HCAL thermal expansion is presented in Figures 6 and 7. Figure 6. Total displacement of the bracket. Gravity, Tracker mass and HCAL thermal expansions included. Displacement is in mm. 6
7 Figure 7. Displacement of the bracket in the direction of gravity. Displacement is in mm. The stresses in the bracket structure were also calculated. The computed stresses in the bracket structure are presented in Figure 8. The maximum stress (97 MPa) gives the safety factor to stresses more than 2. In addition, the stresses in the final bracket are slightly smaller than the computed values, thanks to round corners. Figure 8. Stresses in the bracket [MPa]. 7
8 3. Bolt connections The strength and the margin of safety (MoS) of the bolt connections were calculated. A bolt joint is normally designed in such way that the friction force caused by the axial force of the bolt [1] transfers the shear force from a structure to another. Thus, the key property of the functional joint is the sufficient tension stiffness of the bolt. The coefficient of friction between the components to be connected is estimated to be P=0.3. Stainless steel will be used to connect bracket components together. The characteristics of the are presented in Table 2. The material properties of the bolt are presented in Table 3. The components that are squeezed together are made of aluminium whose Young's modulus is Ep=70000 Mpa. The stress in the bolt should not exceed the yield strength value. Table 2. Characteristics of the. M12 M14 M16 d (mm) P (mm) d 2 (mm) d 3 (mm) R min (mm) A 3 (mm 2 ) A s (mm 2 ) Table 3. Material properties of a stainless steel bolt. Young's modulus, Es [MPa] Yield strength Vty [MPa] 480 The formulas to dimension a bolt joint are given in [1]. To calculate bolt connection one must first describe the joint. The required parameters are introduced in Table 4. The parameters of the bolt connections are defined in Chapters Table 4. Parameters of the bolt connection. Variable Unit Description li mm Length of the bolt in the connection lk mm Height of connection Da mm Diameter of connection Db mm Diameter of hole for a bolt P - Coefficient of friction between the contact surfaces n - Dimensionless factor of the connection [1, Fig ] First, the spring coefficient of the bolt and the spring coefficient of the elements to be connected are calculated. The combined spring coefficient of the bolt and nut (ks) is calculated with the equation [1, ]. 8
9 ks ª ««0.8 d Es S d 2 4 ¹ 0.5 d Es A3 li Es S d 2 4 º»» ¼ 1 (1) The spring coefficient of the elements to be connected (kp) can be calculated with the equation [1, ]. ª «1 kp dk 2 Db 2 Da dk 2 ( ) x 2 º» ¼ x Ep S lk 4 (2), where x is the dimensionless variable of the joint defined by the dimensions of the joint. The value for x is calculated with the equation 3 [1, ] 3 lk dk x ( dk lk) 2 (3) The required normal force of the joint i.e. tension force of the bolt (Fkr) is calculated with the wellknown friction equation 4. If there is more than one bolt, the force is assumed to divide equally to all i.e. the joint is symmetrical. Thus, two in the joint divide the required tensions force of the bolt by two. Fkr Fq friction (4),where Fkr is the minimum tension force of the bolt and Fq the shear force at the joint The additional force ratio, I, for the definition of the maximum tension force of the bolt, is now defined [1, ]. I ks n ks kp (5) The required pre-strain of the bolt (Fv) is [1, ] Fa Fv Fkr 1 I (6), where Fa is the exterior axial load of the joint. The maximum force that will stretch the bolt is finally [1, ] Fsmax Fv I Fa (7) 9
10 The strength of the bolt i.e. the maximum force the bolt can bear (Fty) is calculated with the equation 8 Fty As Vty (8),where Vty is yield strength of the bolt. The margin of safety (MoS) can be calculated as a ratio between the maximum stretching force of the bolt and the strength of the bolt. MoS Fty Fsmax (9) The stiffness calculations of the bolt connections were done in Mathcad 2000 and they are all presented in Appendix Bracket to tube The bracket was planned to be attached to the banana with a single M12 bolt. The connection must bear the quarter mass of the Tracker (=1000kg) and a 3.9-kN horizontal force due to thermal expansion of HCAL. The total shear force at the connection would be thus 10.6 kn. In addition, there is a 3.0-kN force in the axial direction of the bolt. First, the joint with a single M12 bolt was calculated. The margin of safety was MoS=1.1. The margin was found too small, because it does not meet the earthquake safety requirements for example. An M16 bolt would yield MoS=2.0. However, an M16 bolt would require too much space. Therefore, the bracket should not be attached to the banana with a bolt joint that relies only on friction, but the shape of the components must reinforce the joint. The feasible joint could be made of a M12 bolt with a solid pin sticking out of the banana, Figure 9. Figure 9. An improved design of the banana. The banana is connected to tube with three M12. The margin of safety of the joint is MoS=3.2 assuming that the load is divided equally between the. The length of a thread in the insert should be 16 mm [1,Table ], at least. The sufficient thread guarantees that the thread does not rip of the bolt. 10
11 3.2 Bracket to foot The bracket was preliminarily designed to be attached to the foot with four parallel M12. Due to the shape of a bracket, both shear and axial forces load the joint. The distance between the four and the Tracker support tube is 550 mm in the X-direction and 350 mm in the Z-direction. The maximum shear force the M12 bolt is able to transfer with friction (12.14 kn) was calculated with equations presented in Appendix 1. The equilibrium of a four-bolt joint without structural support (Fig. 10 at left) was calculated first. Then, the forces were calculated with the five-bolt design. In case of five, the outermost remain their positions and the distance between the was decreased. The results of calculations with MoS of the connection are presented in Table 5. As one can notice, the joint cannot bear the load. The bracket would rotate until the bracket corner touches the foot. Table 5. Shear forces in the different bolt connections. Bolts Shear X (kn) Shear Y (kn) Shear total (kn) Axial force (kn) MoS Figure 10. Preliminary designed bolt connection between the bracket and the foot. If the structural support could be guaranteed in all circumstances with shim sheets for example (Fig. 10 at right) the margin of safety of the connection with four M12 would yield MoS=1.1 and five MoS=1.3. However, keeping the shim sheet at their places without extra components turned out to be complicated. Therefore, the two-directional bolt connection should be considered in this joint, Figure
12 Figure 11. An improved bolt connection between the bracket and the foot. The stiffness of the two-directional bolt connection was calculated. The forces in the joint due to thermal expansions of HCAL were also included. The margin of safety was calculated taking into account only the axial support the give. Therefore, the results of calculations are conservative. The 1 and 2 (Fig. 11) carry the moment around the Z-axis and 3 and 4 around the X-axis. The margin of safety of the connection is 1.4. The size of the can be increased if the safety margin is found insufficient. 3.3 Foot to HCAL The foot is to be connected to HCAL with two patterns of four M14. The distance between the centres of the patterns is 404 mm. The equilibrium was calculated with M12. Then, the margin of safety yields 1.8. M14 would yield the margin of safety more than Conclusions According to the bracket FE-analysis, the maximum displacement of the aluminium bracket equals 1.3 mm taking into account the mass of the Tracker and the loads caused by the thermal expansion of HCAL. The stresses in the bracket do not exceed the yield strength of the aluminium alloys. The envelope model yielded larger displacement. The results do not fully correspond. This is due to different boundary conditions at the end of Tracker support tube. The boundary conditions used in the bracket model are more realistic. The forces in the bracket due to thermal expansion of HCAL are relatively high. The forces can be diminished by reducing the thickness of the bracket at its bend. The bracket was modelled as a single solid piece instead of two pieces. Therefore, the screw connections between the components were analysed separately. All proposed bolt connections fulfil the load requirements. 5. References 1. Airila M., Ekman K., et al. Koneenosien suunnittelu. WSOY, Porvoo, Finland, p. ISBN
13 Appendix 1: Calculations of bracket bolt connections A ) Bracket to tube The bracket was planned to be connected to the banana by one M12-bolt. The joint between the bracket and the banana eliminates the moment in the bolt connection. Therefore, the bolt must bear the shear force caused by the mass of the Tracker (1000 kg), shear forces caused by the thermal expansion of the HCAL radius (app N) and the axial forces caused by the mass of the Tracker in an inclined tunnel and the thermal expansion of HCAL in longitudunal direction. The total axial force is 3009 N. Dimensions of the M12-bolt from the bolt standard SFS 4497 d := 12mm P := 1.75mm d2 := d3 := mm 9.853mm Rmin := 0.219mm A3 := 76.2mm 2 As := 84.3mm 2 dk := 17.5mm Diameter of the bolt's head (measured) Elastic modulus of the bolt and the pieces to be connected. Es := Pa Elastic modulus of the bolt Ep := Pa Elastic modulus of the connected materials Description of the connection := 1 Number of in the connection li := := 81.5mm Length of the bolt in the connection from Autocad drawing
14 lk := 81.5mm Length of the connecion Da := 30mm Outer diameter of the connection Db := 13.5mm Diameter of the hole friction := 0.3 n := 0.5 Coefficient of friction Dimensionless factor of the connection (Figure ) Forces in the connection Fq := Fa := 10575N 3009N Shear force in the connection Axial force in the connection There isn't momentum in the bolt connection due joint Spring coefficient of the bolt ks := 0.4 d Es π d li Es π d ks kg = s 2 Spring coefficient of the pieces to be connected Dimensionless factor x: x := lk Da 0.2 ( ) 1 kp := dk 2 Db 2 x = dk ( Da dk ) ( x + 2) x Ep π lk 4 kp kg = s 2 Required normal force of the joint (tension force of the bolt) Fkr := Fq friction Fkr = N "Additional force ratio" phi := ks n ks + kp phi = 0.212
15 Pre-strain required: Fa Fv := Fkr + ( 1 phi) Fv = N Maximum force in the bolt connection Fa Fsmax := Fv + phi Fsmax = N Maximum force the bolt can bear (Yield strength of stainless steel bolt A4-70 is 480N/mm 2 ) N Fty12 := As 480 mm 2 Fty12 = N Margin of safety (MoS) of the bolt connection. MoS := Fty12 Fsmax MoS = Margin of Safety does not meet the common engineering requirements. Therefore, either the size of the bolt should be increased or more bolt should be used in the connection. The corresponding joint with M16 bolt Dimensions of the M16-bolt from the bolt standard SFS 4497 d := 16mm P := 2mm d2 := d3 := mm mm Rmin := 0.250mm A3 := 144mm 2 As := 157mm 2 dk := 21.5mm Diameter of the bolt's head
16 Spring coefficient of the bolt ks := 0.4 d Es π d li Es π d ks kg = s 2 Spring coefficient of the pieces to be connected Dimensionless factor x: x := lk Da 0.2 ( ) 1 kp := dk 2 Db 2 x = dk ( Da dk ) ( x + 2) x Ep π lk 4 kp kg = s 2 "Additional force ratio" phi := ks n ks + kp phi = Pre-strain required: Fa Fv := Fkr + ( 1 phi) Maximum force in the bolt connection Fv = N Fa Fsmax := Fv + phi Fsmax = N Maximum force the bolt can bear (Yield strength of stainless steel bolt A4-70 is 480N/mm 2 ) N Fty16 := As 480 mm 2 Fty16 = N Margin of safety (MoS) of the bolt connection. MoS := Fty16 Fsmax MoS = 1.97
17 B ) Bracket to foot The bracket was designed to attach to the foot with four parallel M12. The forces in the joint is calculated with moment equilibrium equation around z-axis that is the most crirical one. The shear force is transferred to the foot with the axial force of a bolt. All four are assumed to carry equal shear force. b1 ) no structural support Forces Fy := Fx := Fz := 9810N 3950N 3009N 4 as designed := 4 Moment around z-axis Fsx ( ( mm mm ) := 9810N 550mm Fsx := ( 9810N 550mm) 360mm Fsx = N Additional horizontal shear force due to Fx Fsxe := Fx Fsxe = 987.5N Vertical shear force Fsy Fsy := Fy Fsy = N Total shear force Fs Fstot := ( Fsx + Fsxe) 2 + Fsy 2 Fstot = N Axial force of the bolt Fa := Fz Fa = N
18 Margin of Safety of the connection Required normal force of the joint (tension force of the bolt) Fkr := Fstot friction Fkr = N Maximum force in the bolt connection Fmax := Fkr + Fz Fmax = N Mos := Fty12 Fmax Mos = The outermost bolt maintain their positions. The distance between the is 67.5 mm := 5 Moment around z-axis Fsx ( ( mm mm ) := 9810N 550mm Fsx := ( 9810N 550mm) 405mm Fsx = N Additional horizontal shear force due to Fx Fsxe := Fx Fsxe = 790N Vertical shear force Fsy Fsy := Fy Fsy = N Total shear force of the bolt, Fs Fstot := ( Fsx + Fsxe) 2 + Fsy 2 Fstot = N Axial force of the bolt
19 Fz Fa := Fa = N Margin of Safety of the connection Required normal force of the joint (tension force of the bolt) Fkr := Fstot friction Fkr = N Maximum force in the bolt connection Fmax := Fkr + Fz Fmax = N Mos := Fty12 Fmax Mos = b2 ) structural support Forces Fy := Fx := Fz := 9810N 3950N 3000N 4 as designed := 4 Moment equilibrium around z-axis Fsx ( ( )mm := 9810N 550mm N 150mm Fsx := ( 9810N 550mm N 150mm) ( )mm Fsx = N Additional horizontal shear force due to Fx Fsxe := Fx Fsxe = 987.5N Vertical shear force Fsy
20 Fy Fsy := Fsy = N Total shear force Fs of each bolt Fstot := ( Fsx + Fsxe) 2 + Fsy 2 Fstot = N Axial force of the bolt Fa := Fz Fa = 750 N Margin of Safety of the connection Required normal force of the joint to transfer shear force (tension force of the bolt) Fkr := Fstot friction Fkr = N Maximum axial force of the bolt Fmax := Fkr + Fz Fmax = N Mos := Fty12 Fmax Mos = := 5 Moment equilibrium around z-axis Fsx ( ( )mm := 9810N 550mm N 150mm Fsx := ( 9810N 550mm N 150mm) ( )mm Fsx = N Additional horizontal shear force due to Fx Fsxe := Fx Fsxe = 790N Vertical shear force Fsy
21 Fy Fsy := Fsy = N Total shear force Fs of each bolt Fstot := ( Fsx + Fsxe) 2 + Fsy 2 Fstot = N Axial force of the bolt Fa := Fz Fa = 600 N Margin of Safety of the connection Required normal force of the joint to transfer shear force (tension force of the bolt) Fkr := Fstot friction Fkr = N Maximum axial force of the bolt Fmax := Fkr + Fz Fmax = N Mos := Fty12 Fmax Mos = b3 ) 2 dimensional bolt connection Forces Fy := Fx := Fz := 9810N 3950N 3000N 2 in the 2 directions The joint is calculated to be carried only with the axial forces of the. := 4
22 Moment equilibrium (z-axis) Fa1 ( ) mm := Fy 550mm + Fx 150mm Fa1 := ( Fy 550mm + Fx 150mm) 300mm Fa1 = N Moment equilibium (x-axis) Fa2 ( ) mm := Fy 350mm + Fz 150mm Fa2 := ( Fy 350mm + Fz 150mm) 300mm Fa2 = N Margin of Safety of the connection Required normal force of the joint (tension force of the bolt) Shear force in the Y-direction Fsy := Fkr := Fy Fsy friction Fsy = N Fkr = N Maximum tension forces in the bolt connection The axis of the bolt in the direction of x-axis Fmax1 := Fkr + Fa1 Fmax1 = N Mos := Fty12 Fmax1 Mos = The axis of the bolt in the direction of x-axis Fmax2 := Fkr + Fa2 Fmax2 = N Mos := Fty12 Fmax2 Mos = B ) Foot to HCAL The foot is connected to HCAL with two patterns of four M14. The
23 distance between the centres of the patterns is 404 mm. The shear force is transferred to HCAL with the axial force of a bolt. All are assumed to carry equal shear force. The stiffness was calculated with M12. Forces Fy := Fx := Fz := 9810N 3950N 3000N Moment equilibrium (x-axis), shear forces Fsm ( ( mm ) := Fy 350mm 350mm Fsm := Fy ( 8 202mm) Fy Fsy := 8 Fz Fsz := 8 Fsm = N Fsy = N Fsz = 375N Total shear force Fs of each bolt Fstot := ( Fsm + Fsz) 2 + Fsy 2 Fstot = N Moment equilibrium (z-axis), axial forces Fas ( ( 4 15 mm mm ) := Fx 350mm + Fz 550mm Fas := ( Fx 350mm + Fz 550mm) 220mm Fas = N Margin of Safety of the connection Required normal force of the joint to transfer shear force (tension force of the bolt) Fkr := Fstot friction Fkr = N Maximum axial force of the bolt := +
24 Fmax := Fkr + Fas Fmax = N Fty12 Mos := Mos = Fmax
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 informationTechnical Report Example (1) Chartered (CEng) Membership
Technical Report Example (1) Chartered (CEng) Membership A TECHNICAL REPORT IN SUPPORT OF APPLICATION FOR CHARTERED MEMBERSHIP OF IGEM DESIGN OF 600 (103 BAR) 820MM SELF SEALING REPAIR CLAMP AND VERIFICATION
More 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 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 informationDESIGN & ANALYSIS OF CONNECTING ROD OF FORMING AND CUTTING DIE PILLAR STATION OF VACUUM FORMING MACHINE
Research Paper ISSN 2278 0149 www.ijmerr.com Vol. 3, No. 3, July, 2014 2014 IJMERR. All Rights Reserved DESIGN & ANALYSIS OF CONNECTING ROD OF FORMING AND CUTTING DIE PILLAR STATION OF VACUUM FORMING MACHINE
More informationComputer 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 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 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 informationDeep Beam With Web Opening
Deep Beam With Web Opening Name: Path: Keywords: DeepBeamWithWebOpening/deepbeam /Examples//DeepBeamWithWebOpening/deepbeam analys: linear static. constr: suppor. elemen: cq16m ct12m pstres. load: force
More informationSimulation of Connector Assembly C
Simulation of Connector Assembly C Date: Sunday, March 6, 2016 Designer: Solidworks Study name: Horizontal Stress Test on C inner bend Analysis type: Static Table of Contents Model Information... 2 Study
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 informationSimulation of Connector Assembly AA
Simulation of Connector Assembly AA Date: Tuesday, March 1, 2016 Designer: Solidworks Study name: Horizontal Stress in AA inner tab fold Analysis type: Static Table of Contents Model Information... 2 Study
More informationElastic Analysis of a Deep Beam with Web Opening
Elastic Analysis of a Deep Beam with Web Opening Outline 1 Description 2 Finite Element Model 2.1 Units 2.2 Geometry definition 2.3 Properties 2.4 Boundary conditions 2.4.1 Constraints 2.4.2 Vertical load
More informationGlobal to Local Model Interface for Deepwater Top Tension Risers
Global to Local Model Interface for Deepwater Top Tension Risers Mateusz Podskarbi Karan Kakar 2H Offshore Inc, Houston, TX Abstract The water depths from which oil and gas are being produced are reaching
More informationME Optimization of a Frame
ME 475 - Optimization of a Frame Analysis Problem Statement: The following problem will be analyzed using Abaqus. 4 7 7 5,000 N 5,000 N 0,000 N 6 6 4 3 5 5 4 4 3 3 Figure. Full frame geometry and loading
More informationASSIGNMENT 1 INTRODUCTION TO CAD
Computer Aided Design(2161903) ASSIGNMENT 1 INTRODUCTION TO CAD Theory 1. Discuss the reasons for implementing a CAD system. 2. Define computer aided design. Compare computer aided design and conventional
More informationCITY 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 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 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 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 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 informationLateral 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 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 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 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 informationANSYS 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 informationCOLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS
VOL., NO., NOVEMBER 6 ISSN 8968 6-6 Asian Research Publishing Network (ARPN). All rights reserved. COLLAPSE LOAD OF PIPE BENDS WITH ASSUMED AND ACTUAL CROSS SECTIONS UNDER IN-PLANE AND OUT-OF-PLANE MOMENTS
More informationTutorial 1: Welded Frame - Problem Description
Tutorial 1: Welded Frame - Problem Description Introduction In this first tutorial, we will analyse a simple frame: firstly as a welded frame, and secondly as a pin jointed truss. In each case, we will
More 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 informationDesign of a Precision Robot Wrist Interface. Patrick Willoughby Advisor: Alexander Slocum MIT Precision Engineering Research Group
Design of a Precision Robot Wrist Interface Patrick Willoughby Advisor: Alexander Slocum MIT Precision Engineering Research Group Project Summary Problem: Current bolted robot wrist replacements are inaccurate,
More informationmachine design, Vol.9(2017) No.1, ISSN pp
machine design, Vol.9(2017) No.1, ISSN 1821-1259 pp. 29-34 Research paper DYNAMIC ANALYSIS AND PARAMETRIC OPTIMISATION OF THE CONNECTING ROD USING AUTODESK INVENTOR Vasile George CIOATĂ 1, * - Imre KISS
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 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 informationBackground CE 342. Why RISA-2D? Availability
Background CE 342 RISA-2D RISA-2D is a structural analysis program, which can model: Beams, frames, trusses and plates. Any linear elastic structural material. Typical supports, such as pins, rollers and
More informationGeneral modeling guidelines
General modeling guidelines Some quotes from industry FEA experts: Finite element analysis is a very powerful tool with which to design products of superior quality. Like all tools, it can be used properly,
More informationStress Concentration Factors
CONSEIL INTERNATIONAL DES MACHINES A COMBUSTION INTERNATIONAL COUNCIL ON COMBUSTION ENGINES CO-ORDINATING WORKING GROUP "CLASSIFICATION SOCIETIES DIESEL" (WG2) Proposal by CIMAC WG4 11th May 2012 IACS
More informationRevision 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 informationmidas Civil Advanced Webinar Date: February 9th, 2012 Topic: General Use of midas Civil Presenter: Abhishek Das Bridging Your Innovations to Realities
Advanced Webinar Date: February 9th, 2012 Topic: General Use of midas Civil Presenter: Abhishek Das Contents: Overview Modeling Boundary Conditions Loading Analysis Results Design and Misc. Introduction
More informationFINITE ELEMENT ANALYSIS AND DYNAMIC ANALYSIS OF THE OUTER BEARING BUSH FROM THE BLADE ADJUSTMENT MECHANISM OF KAPLAN TURBINES
The 4th International Conference Computational Mechanics and Virtual Engineering COMEC 2011 20-22 OCTOBER 2011, Brasov, Romania FINITE ELEMENT ANALYSIS AND DYNAMIC ANALYSIS OF THE OUTER BEARING BUSH FROM
More informationTUTORIAL 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 informationD 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 informationLesson 6: Assembly Structural Analysis
Lesson 6: Assembly Structural Analysis In this lesson you will learn different approaches to analyze the assembly using assembly analysis connection properties between assembly components. In addition
More informationChapter 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 informationAnalysis of Crank End of Connecting Rod using Finite Element Method
Analysis of Crank End of Connecting Rod using Finite Element Method Mohammad Umair Zaki Faculty of Mechanical Engineering Noida International University Greater Noida, India e-mail-umairzaki@yahoo.com
More informationVARIOUS APPROACHES USED IN THE SEISMIC QUALIFICATION OF THE PIPING SYSTEMS IN NUCLEAR FACILITIES. Introduction
VARIOUS APPROACHES USED IN THE SEISMIC QUALIFICATION OF THE PIPING SYSTEMS IN NUCLEAR FACILITIES A. Musil, P. Markov Stevenson&Associates, Pilsen, Czech Republic Introduction In the firm Stevenson&Associates
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 informationEngineering 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 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 informationAnalysis of ANSI W W 6x9-118,
Page 1 of 8 Analysis of ANSI W W 6x9-118,110236220472 Author: Analysis Created: Analysis Last Modified: Report Created: Introduction Administrator, 08:29:09, 08:29:09 09:26:02 Database: Z:\ENGENHARIA\ESTUDOS
More informationFinite Element Analysis Using NEi Nastran
Appendix B Finite Element Analysis Using NEi Nastran B.1 INTRODUCTION NEi Nastran is engineering analysis and simulation software developed by Noran Engineering, Inc. NEi Nastran is a general purpose finite
More informationANSYS 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 informationDesign Analysis Of Industrial Gear Box Casing.
Design Analysis Of Industrial Gear Box Casing. Balasaheb Sahebrao Vikhe 1 1 Assistant Professor, Dept. of Mechanical Engineering, SVIT College Nasik, Maharashtra, India ---------------------------------------------------------------------***---------------------------------------------------------------------
More informationMSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook
MSC/PATRAN LAMINATE MODELER COURSE PAT 325 Workbook P3*V8.0*Z*Z*Z*SM-PAT325-WBK - 1 - - 2 - Table of Contents Page 1 Composite Model of Loaded Flat Plate 2 Failure Criteria for Flat Plate 3 Making Plies
More informationLearning 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 informationRecent 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 informationFEA and Topology Optimization of an Engine Mounting Bracket
International Journal of Current Engineering and Technology E-ISSN 2277 4106, P-ISSN 2347 5161 2016 INPRESSCO, All Rights Reserved Available at http://inpressco.com/category/ijcet Research Article Sanket
More informationTopology optimization of engine and gearbox mount castings
Topology optimization of engine and gearbox mount castings Peter Hougardy, AUDI AG 1 1 Table of contents > Overview AUDI powertrain mounting system > General approach using topology optimization > Examples
More informationStructural static analysis - Analyzing 2D frame
Structural static analysis - Analyzing 2D frame In this tutorial we will analyze 2D frame (see Fig.1) consisting of 2D beams with respect to resistance to two different kinds of loads: (a) the downward
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 informationWorkshop 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 informationModule 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 informationReinforced concrete beam under static load: simulation of an experimental test
Reinforced concrete beam under static load: simulation of an experimental test analys: nonlin physic. constr: suppor. elemen: bar cl12i cl3cm compos cq16m interf pstres reinfo struct. load: deform weight.
More informationStress Analysis of Bolted Joints Part II. Contact and Slip Analysis of a Four Bolt Joint
Modern Mechanical Engineering, 2014, 4, 46-55 Published Online February 2014 (http://www.scirp.org/journal/mme) http://dx.doi.org/10.4236/mme.2014.41006 Stress Analysis of Bolted Joints Part II. Contact
More informationMODELLING OF AN AUTOMOBILE TYRE USING LS-DYNA3D
MODELLING OF AN AUTOMOBILE TYRE USING LS-DYNA3D W. Hall, R. P. Jones, and J. T. Mottram School of Engineering, University of Warwick, Coventry, CV4 7AL, UK ABSTRACT: This paper describes a finite element
More informationInstitute of Mechatronics and Information Systems
EXERCISE 4 Free vibrations of an electrical machine model Target Getting familiar with the fundamental issues of free vibrations analysis of a simplified model of an electrical machine, with the use of
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 informationSimulation of Overhead Crane Wire Ropes Utilizing LS-DYNA
Simulation of Overhead Crane Wire Ropes Utilizing LS-DYNA Andrew Smyth, P.E. LPI, Inc., New York, NY, USA Abstract Overhead crane wire ropes utilized within manufacturing plants are subject to extensive
More informationIntroduction 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 informationModelling 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 informationDesign and development of optimized sprocket for Track hoe
Design and development of optimized sprocket for Track hoe Mr. Laxmikant P.Sutar 1, Prof. Prashant.G. Karajagi 2, Prof. Rahul Kulkarni 3 1 PG Student, Siddhant College of Engineering, Pune, India 2 Assistant
More informationEnhancing Productivity of a Roller Stand through Design Optimization using Manufacturing Simulation
Enhancing Productivity of a Roller Stand through Design Optimization using Manufacturing Simulation B.R. Krishna Tej 1, N.Sasank Sai 1 and S.Deepak kumar* 1 Engineering Design and Research Center (EDRC)
More informationTHE 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 informationChapter 5 Modeling and Simulation of Mechanism
Chapter 5 Modeling and Simulation of Mechanism In the present study, KED analysis of four bar planar mechanism using MATLAB program and ANSYS software has been carried out. The analysis has also been carried
More informationSIDDHARTH GROUP OF INSTITUTIONS :: PUTTUR Siddharth Nagar, Narayanavanam Road QUESTION BANK (DESCRIPTIVE) UNIT I ARCHES
SIDDHARTH GROUP OF INSTITUTIONS :: PUTTUR Siddharth Nagar, Narayanavanam Road 517583 QUESTION BANK (DESCRIPTIVE) Subject with Code : SA-II (13A01505) Year & Sem: III-B.Tech & I-Sem Course & Branch: B.Tech
More informationWhat makes Bolt Self-loosening Predictable?
What makes Bolt Self-loosening Predictable? Abstract Dr.-Ing. R. Helfrich, Dr.-Ing. M. Klein (INTES GmbH, Germany) In mechanical engineering, bolts are frequently used as standard fastening elements, which
More informationComputations of stresses with volume-elements in rectangular and HE sections
CT3000: Bachelor Thesis Report, Izik Shalom (4048180) Computations of stresses with volume-elements in rectangular and HE sections Supervisors: dr. ir. P.C.J. Hoogenboom en Ir. R. Abspoel June 2013 Preface
More informationAdvanced model of steel joints loaded by internal forces from 3D frame structures
Advanced model of steel joints loaded by internal forces from 3D frame structures Lubomír Šabatka, IDEA RS s.r.o František Wald, FSv ČVUT Praha Jaromír Kabeláč, Hypatia Solutions s.r.o Drahoslav Kolaja,
More informationANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis
R50 ANSYS 5.6 Tutorials Lecture # 2 - Static Structural Analysis Example 1 Static Analysis of a Bracket 1. Problem Description: The objective of the problem is to demonstrate the basic ANSYS procedures
More informationAn 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 informationTerrain settlement analysis
Engineering manual No. 21 Updated: 02/2018 Terrain settlement analysis Program: File: FEM Demo_manual_21.gmk This example contains the solution to terrain settlement under surcharge loading using the Finite
More informationE and. L q. AE q L AE L. q L
STRUTURL NLYSIS [SK 43] EXERISES Q. (a) Using basic concepts, members towrds local axes is, E and q L, prove that the equilibrium equation for truss f f E L E L E L q E q L With f and q are both force
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 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 informationGuangxi University, Nanning , China *Corresponding author
2017 2nd International Conference on Applied Mechanics and Mechatronics Engineering (AMME 2017) ISBN: 978-1-60595-521-6 Topological Optimization of Gantry Milling Machine Based on Finite Element Method
More informationOptimization of hanger arrangement of network arch bridges
IABSE-JSCE Joint Conference on Advances in Bridge Engineering-II, August 8-10, 2010, Dhaka, Bangladesh. ISBN: 978-984-33-1893-0 Amin, Okui, Bhuiyan (eds.) www.iabse-bd.org Optimization of hanger arrangement
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 informationBeams. Lesson Objectives:
Beams Lesson Objectives: 1) Derive the member local stiffness values for two-dimensional beam members. 2) Assemble the local stiffness matrix into global coordinates. 3) Assemble the structural stiffness
More informationBolt Toolkit Extension
Bolt Toolkit Extension DOCUMENTATION Extension version 180.8 Release date 28-Apr-17 Compatible ANSYS version 18.0 www.edrmedeso.com Table of Contents Bolt Toolkit toolbar... 3 Bolt Toolkit Help... 3 News
More information3. Check by Eurocode 3 a Steel Truss
TF 3. Check by Eurocode 3 a Steel Truss Applicable CivilFEM Product: All CivilFEM Products Level of Difficulty: Moderate Interactive Time Required: 40 minutes Discipline: Structural Steel Analysis Type:
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 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 informationAnalysis of Detroit Seismic Joint System
Analysis of Detroit Seismic Joint System for EMSEAL Corporation Prepared by Haig Saadetian, P.Eng. Senior Consultant ROI Engineering Inc. 50 Ronson Drive, Suite 120 Toronto ON M9W 1B3 26-April-2009 1 Contents
More informationstudying 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 informationEngineering 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 informationSolidWorks. 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 informationDUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE NOZZLE USING 3D CRACK MESHES
DUCTILE TEARING ANALYSIS OF A CUSTOM PIPE TO FLANGE Greg Thorwald, Ph.D. Principal Consulting Engineer, Quest Integrity Group, USA Michael Rock Engineering Project Manager, Mighty River Power Limited,
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 informationOrbital 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 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 informationME Optimization of a Truss
ME 475 - Optimization of a Truss Analysis Problem Statement: The following problem will be analyzed using Abaqus and optimized using HEEDS. 4 5 8 2 11 3 10 6 9 1 7 12 6 m 300 kn 300 kn 22 m 35 m Figure
More information