Pre-tensioning techniques in LS-DYNA implicit. Anders Jonsson with contributions from Nils Karjan, Thomas Borrvall and Anders Jernberg
|
|
- Rosalind Edwards
- 5 years ago
- Views:
Transcription
1 Pre-tensioning techniques in LS-DYNA implicit Anders Jonsson with contributions from Nils Karjan, Thomas Borrvall and Anders Jernberg
2 Pre-tensioning techniques in implicit LS-DYNA Implicit set up the basics Bolt modelling in general See For an extensive description of bolts modelling, see Karajan, N., et al., Modeling bolts in LS-DYNA using explicit and implicit time integration, 15 th Int. LS-DYNA Users Conf. ( Bolt pre-tensioning Solid bolts Beam bolts Procedures for applying the pre-tensioning Some remarks on bending stiffness Contact issues Press-fit in contacts MORTAR contact INTERFERENCE contact Initial stresses in simulation of processes Spring back Summary and conclusions 3
3 Basic implicit set-up in LS-DYNA LS-DYNA is a versatile multi-physics solver. Many different analysis types are possible. But many settings are left to the user... Control cards, telling LS-DYNA how to solve the task Element formulations (many different formulations available) Contact definitions (many different formulations and options to chose from) Material models (over 250 to chose from) Based on the Guideline for implicit analyses, this may (in many cases) be greatly simplified. The objective of the Guideline is to reduce the time it takes to make these choices, so that the time can be spent on solving the actual task. The Guideline for implicit analyses is available for download from The Appendix P of the LS-DYNA keyword manual (R9.0 and later) also provides some recommendations, background and motivation to implicit control card settings. 5
4 Implicit set-up in LS-DYNA Control cards Identify analysis type and select appropriate control card include file. In many cases, *CONTROL_TERMINATION is the only required additional control card. Use an include file structure! Then the control card include files of the Guideline package can be used directly. Material data 7
5 Pre-processing GUI dedicated for implicit set up is available in LS-PrePost from V4.6 Including convenient support for Pre-stressing 10
6 BOLT PRE-TENSIONING 11
7 Bolt pre-tensioning - general Main keywords in LS-DYNA *INITIAL_AXIAL_FORCE_BEAM for pre-tension of beam-style bolts. Applies a force. Requires a spotweld beam (elform 9) with *MAT_SPOTWELD. To obtain an elastic beam bolt, specify a high yield stress. *INITIAL_STRESS_SECTON for solid element bolts. Applies a stress. Works for the common solid elements ±1, ±2, 16 Both keywords require a load curve to apply the pre-tensioning. It is recommended to let the curve end when the initialization is completed. For example, for pre-tensioning in implicit: *DEFINE_CURVE_TITLE Bolt pre-tensioning force 100, 0.,0. 1.,75. Pre-tensioning techniques in LS-DYNA-implicit
8 Bolt pre-tensioning Load curves In order to end the pre-tensioning, let the load curve end Should a constant force be required, let the load curve continue on a constant level *DEFINE_CURVE_TITLE Bolt pre-tensioning force 100, 0.,0. 1.,75. Pre-tensioning techniques in LS-DYNA-implicit
9 Bolt pre-tensioning Beam bolts Initialization of a normal force as pre-tension in the spot weld beam *INITIAL_AXIAL_FORCE_BEAM for pre-tension of beam-style bolts. Applies a force. NOTE! Spotweld beam (elform 9) with *MAT_SPOTWELD must be used. Make sure that all DOFs of the beam end nodes are connected! Avoid release conditions on CNRB:s! If *CONSTRAINED_INTERPOLATION is used, set DDOF = *INITIAL_AXIAL_FORCE_BEAM $# bsid lcid scale kbend *DEFINE_CURVE $# lcid sidr sfa sfo offa offo dattyp lcint 100 &dtprestr &BltForce $# a1 o BltForce force dtprestr end curve after pre-tension! time bsid: beam set ID containing the spot weld beams to be pre-tensioned dtprestr: parameter defining the initialization time of the pre-tension BltForce: parameter defining the pre-tension force Bending stiffness of bolt during initialization kbend=0: no bending stiffness kbend=1: beam has bending stiffness (starting with R10) Pre-tensioning techniques in LS-DYNA-implicit 14
10 Bolt pre-tensioning Solid bolts Initialization of a normal stress in a cross section of the solid elements *INITIAL_STRESS_SECTION $# issid csid lcid psid vid izshear *DEFINE_CURVE $# lcid sidr sfa sfo offa offo dattyp lcint 100 &dtprestr &BltStrss $# a1 o *DATABASE_CROSS_SECTION_PLANE_ID $# csid title 100 Cross Section Bolt $# psid xct yct zct xch ych zch radius $# xhev yhev zhev lenl lenm id itype BltStrss stress σ normal vector cross section with radius end curve after pre-tension! time psid: part set ID containing the solid elements to be pre-stressed {x,y,z}ct {x,y,z}ch: head and tail coordinate of normal vector of the cross section BltStress: the (normal) stress to be applied (provide reasonable value!) izshear: flag to activate shear stiffness during pre-stressing phase dtprestr Pre-tensioning techniques in LS-DYNA-implicit 15
11 Bolt pre-tensioning Solid bolts izshear: Allow shear stresses to develop during the pre-stressing phase Yields more realistic distribution of the normal stresses Normal stress distribution in the bolt at equilibrium using LS-DYNA implicit (in coming versions) izshear=0: yields homogeneous normal stress of 0.38 GPa izshear=2: yields inhomogeneous normal stresses averaging 0.38 GPa over the cross section izshear=0 izshear=1 Revised for implicit in current development versions (in coming versions) For explicit analysis this will be available as izshear=2 For implicit izshear=1 and izshear=2 are synonymous Pre-tensioning techniques in LS-DYNA-implicit 16
12 Bolt pre-tensioning Solid bolts Avoid pentahedron elements in the shank Normal stress distribution might be disturbed Cause convergence problems during implicit simulations with some LS-DYNA releases (R9.2, R10) Allow for large enough elements to account for initial contraction Elements with a pre-stress application shrink until equilibrium is reached Head and nut need to travel far enough to be in contact with the sheets hexahedrons only Best to account for this such that the deformed configuration leads to a nice mesh hexas & pentahedrons before pre-stress initialization after initialization at equilibrium Pre-tensioning techniques in LS-DYNA-implicit 17
13 Bolt pre-tensioning - recommendations If a beam bolt consists of many beam elements, apply *INITIAL_AXIAL_FORCE_BEAM to one beam element per bolt. Set KBEND = 1 to account also for the bending stiffness of the beam Add *DATABASE_HISTORY_BEAM_SET for the beam elements which are being pre-tensioned. Use an individual *DATABASE_CROSS_SECTION_PLANE for each *INITIAL_STRESS_SECTON for solid element bolts. By this, cross section forces and moments can be evaluated for each bolt individually from secforc. Avoid pentas in the bolt shank for solid bolts! IGS = 1 on *CONTROL_IMPLICIT_GENERAL (active in User s guide control cards) normally aid convergence for pre-tensioning of solid bolts. Beware that if the elements are initially (very) small and/or the structure surrounding the bolt is weak, there is a risk of ending up with Error termination due to Negative volume in solid element. The remedy is often simply to mesh the pre-tension section a bit coarser. 18
14 Possible procedures for applying the pre-tensioning in implicit Implicit static, in physical time, for example from t = 0 to t = 1. In case the assembly has initial rigid-body modes, implicit dynamics can be applied initially Using dynamic relaxation (DR) Implicit, static or dynamic Explicit 19
15 Pre-tensioning using implicit statics Implicit static, in physical time, for example from t = 0 to t = 1. Pre-tensioning is applied just like normal load application. Don t use a too small first time step size. Statics should work well for beam bolts connected to the structure by constrained nodal rigid bodies. Make sure that all DOFs of the beam nodes are connected! Avoid release conditions on CNRB:s! If *CONSTRAINED_INTERPOLATION is used, set DDOF = If the assembly only is connected by the (solid) bolts and contacts, the model will have rigid body modes at t = 0. LS-DYNA will print negative eigenvalue warnings. *** Warning (IMP+124) 11 negative eigenvalues detected Still, the pre-tensioning may converge. 20
16 Pre-tensioning using implicit dynamics Initial rigid body modes will be taken care of by the dynamics. Note that when dynamics is active, time means physical time. This means that the time to ramp up the pre-tensioning becomes important. Dynamic effects can then be ramped down, as the contacts establish, and the rest of the analysis can be performed as static. *CONTROL_IMPLICIT_DYNAMICS $ IMASS GAMMA BETA TDYBIR TDYDTH TDYBUR IRATE Settings for quasi-statics 21
17 Pre-tensioning using implicit dynamic relaxation (DR) The analysis is split in two stages, and bolt pre-tensioning takes place before t = 0. Implicit dynamic relaxation can be static and/or dynamic. Set SIDR = 1 on the pre-tension load curve to activate DR Output for 3D-plotting of states from the dynamic relaxation can be specified by *DATABASE_BINARY_D3DRLF. Note! Interval is cycles, not time! It is possible to specify separate implicit settings for the DR *CONTROL_IMPLICIT_AUTO_DYN *CONTROL_IMPLICIT_DYNAMICS_DYN *CONTROL_IMPLICIT_SOLUTION_DYN 22
18 Pre-tensioning using implicit dynamic relaxation (DR) Set SIDR = 1 on the pre-tension load curve Also other load curves that are to be active during DR should have SIDR = 1 for example to specify variation of max time step *DEFINE_CURVE_TITLE Bolt pre-tension 600 MPa $ LCID SIDR ,.0 1.,.6 *CONTROL_DYNAMIC_RELAXATION Pre-tensioning is ramped up $ NRCYCK DRTOL DRFCTR DRTERM TSSFDR IRELAL EDTTL IDRFLG *CONTROL_IMPLICIT_AUTO_DYN $ IAUTO ITEOPT ITEWIN DTMIN DTMAX DTEXP *CONTROL_IMPLICIT_DYNAMICS_DYN $ IMASS GAMMA BETA TDYBIR TDYDTH TDYBUR IRATE Pre-tensioning techniques in LS-DYNA-implicit
19 Pre-tensioning using explicit dynamic relaxation (DR) Dynamic relaxation analysis is split in two stages. The bolt pre-tensioning takes place before t = 0 using explicit dynamics. Can be very efficient for structures with many loose parts. Add contact damping to aid convergence (VDC = 20-40) of explicit DR. Set SIDR = 1 on the pre-tension load curve and IDRFLG = 1 to activate explicit DR. *CONTROL_TIMESTEP is also recommended. Use moderate mass scaling (< %) by dt2ms < 0. *DEFINE_CURVE_TITLE Bolt pre-tension 600 MPa $ LCID SIDR ,.6 1.,.6 *CONTROL_TIMESTEP Pre-tensioning is constant $ TDINT TSSFAC ISDO TSLIMT DT2MS E-04 *CONTROL_DYNAMIC_RELAXATION $ NRCYCK DRTOL DRFCTR DRTERM TSSFDR IRELAL EDTTL IDRFLG Pre-tensioning techniques in LS-DYNA-implicit
20 Procedures for applying the pre-tensioning in implicit Performance overview for the pipe example. Run on 4 cores, mpp-ls-dyna R10.1 double precision Option Time (relative) Comment Keyword file Dynamic Static implicit 1 No negative eigenvalues pretens002.key Implicit DR 0.97 No negative eigenvalues pretens004.key Explicit DR 1.19 No gain in this case pretens003.key Implicit static 1.26 Negative eigenvalues during first time step pretens001b.key Pre-tensioning techniques in LS-DYNA-implicit
21 Bolt pre-tensioning bending stiffness By default, LS-DYNA applies the pre-tensioning only in the axial direction. Stress gradients are not considered. 27
22 Bolt pre-tensioning bending stiffness By default, LS-DYNA applies the pre-tensioning only in the axial direction. Stress gradients are not considered. kbend = 0 MAT_24 in the bolt Pre-tensioning techniques in LS-DYNA-implicit
23 Bolt pre-tensioning bending stiffness For *INITIAL_AXIAL_FORCE_BEAM this is resolved from R10. Set the bending stiffness flag KBEND = 1 to account also for the bending stiffness of the beam during initialization. *INITIAL_AXIAL_FORCE_BEAM $# bsid lcid scale kbend For*INITIAL_STRESS_SECTON the bending issue is resolved from R9.1 for *MAT_ELASTIC. So one workaround is to specify a slice of elastic material where the pre-tensioning takes place. In coming LS-DYNA versions, the option IZSHEAR = 2 will prescribe the average stress over the cross section of each bolt. Then also the bending stiffness can be accounted for. *INITIAL_STRESS_SECTION $ isid csid lcid psid vid izshear Pre-tensioning techniques in LS-DYNA-implicit
24 Bolt pre-tensioning bending stiffness For beam bolts, this is resolved in R10. For solid bolts, add a slice of elastic material where the pre-tensioning takes place. KBEND = 1, rev MAT_24 in the bolt, but one layer of elastic material added Pre-tensioning techniques in LS-DYNA-implicit
25 Bolt pre-tensioning bending stiffness For beam bolts, this is resolved in R10. In coming versions, use IZSHEAR = 2 for solid bolts. KBEND = 1, rev MAT_24 in the bolt, IZSHEAR = 2 Pre-tensioning techniques in LS-DYNA-implicit
26 Possible procedures for applying the pre-tensioning in implicit Larger example. Pretension of 9 (5 M20, 4 M14) bolts in 2 directions, using explicit Dynamic Relaxation. Time for pre-tensioning: 12.5 minutes on 4 cores. 36
27 PRESS-FIT 37
28 Press fit in contacts It is strongly recommended to use *CONTACT_..._MORTAR_ID for implicit analyses. Mortar contact can also handle press-fit, using IGNORE = 3 ( small penetrations) or 4 (finite penetrations), and MPAR1 to specify time to resolve the initial penetrations, and MPAR2 to specify search distance for penetrating nodes. The solid contact thickness (PENMAX from R10) may require adjustment The contact surface is adjusted at t = 0 so that no initial penetrations exist The contact surface is then moved out using a linear ramp, to coincide with the meshed surface at t = MPAR1 It is possible to parametrize the grip by contact surface augmentation. For solids, this is most conveniently done in R10, where the parameter SLDTHK (optional card B of the contact definition) can be used to directly specify the thickness increase. 39
29 Contacts Press-fit Mortar example for large penetration / press-fit *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_MORTAR_ID $# cid title 1interference $# ssid msid sstyp mstyp sboxid mboxid spr mpr $# fs fd dc vc vdc penchk bt dt $# sfs sfm sst mst sfst sfmt fsf vsf MPAR1 4is the time when the press-fit should be resolved $# soft sofscl lcidab maxpar sbopt depth bsort frcfrq $# penmax thkopt shlthk snlog isym i2d3d sldthk sldstf $# igap ignodprfac/mpadtstif/mpar2 unused unused flangl cid_rcf Set IGNORE = 4 for finite interference MPAR2 is the search distance 40
30 Contacts Press-fit Mortar example for large penetration / press-fit 41
31 Contacts Press-fit Mortar example for large penetration / press-fit 42
32 Contacts Press-fit Mortar example for large penetration / press-fit 43
33 Press fit in contacts In some cases for press-fit (often finite penetrations, IGNORE = 4) analyses using the Mortar contact may run into (convergence) problems. An option to try out is then *CONTACT_SURFACE_TO_SURFACE_INTERFERENCE_ID $# cid title 1014Bellow - locking ring $# ssid msid sstyp mstyp sboxid mboxid spr mpr $# fs fd dc vc vdc penchk bt dt 0.6 $# sfs sfm sst mst sfst sfmt fsf vsf Curve for scaling penalty stiffness. Start at (0., 0.) end at (t, 1.) $# lcid1 lcid $# soft sofscl lcidab maxpar sbopt depth bsort frcfrq $# penmax thkopt shlthk snlog isym i2d3d sldthk sldstf 1.0 $# igap ignodprfac/mpadtstif/mpar2 unused unused flangl cid_rcf 2 Set IGAP = 2 to disable sticky contact Pre-tensioning techniques in LS-DYNA-implicit
34 Press fit in contacts In some cases for press-fit (often finite penetrations, IGNORE = 4) analyses using the Mortar contact may run into (convergence) problems. An option to try out is then *CONTACT_SURFACE_TO_SURFACE_INTERFERENCE_ID A curve - starting at (0., 0.) - is given for scaling the penalty stiffness up to 1. May need some iterations to find the right curve. Start with linear ramp This contact has the sticky option on by default. Set IGAP = 2 to disable. Pre-tensioning techniques in LS-DYNA-implicit
35 Contacts Press-fit In some cases for press-fit (often finite penetrations, IGNORE = 4) analyses using the Mortar contact may run into (convergence) problems. An option to try out is then *CONTACT_SURFACE_TO_SURFACE_INTERFERENCE_ID 46
36 Press fit in contacts *CONTACT_..._MORTAR_ID Developed for implicit No sticky option, it is always off Contact surface is moved away until no initial penetrations exist, then moved back to the original position Cannot be used with Dynamic Relaxation (in current versions) *CONTACT_.._INTERFERENCE_ID Developed for explicit Separate option to resolve interference in Dynamic Relaxation Sees all penetrations. Contact stiffness is ramped up to resolve them. This contact has the sticky option on by default. Set IGAP = 2 to disable. Pre-tensioning techniques in LS-DYNA-implicit
37 Contacts Press-fit It is possible to parametrize the grip by contact surface augmentation. For solids, this is most conveniently done in R10, where the parameter SLDTHK (optional card B of the contact definition) can be used to directly specify the thickness increase. Note that both master and slave side will be augmented! Contact surface augmentation in R10 Pre-tensioning techniques in LS-DYNA-implicit
38 STRESS INITIALIZATION 49
39 Stress initialization This is the classical application of implicit: Springback after forming Use *INTERFACE_SPRINGBACK_LSDYNA to request dynain file ASCII keyword format or LSDA Binary format LS-DYNA will output the deformed geometry and residual stresses. Keywords: *NODE, *ELEMENT_..., *INITIAL_STRESS_... Note: Hyperelastic materials, like rubbers (MAT_77, MAT_181 ) and foams, are initialized by *INITIAL_FOAM_REFERENCE_GEOMETRY May be useful for multi-step simulations, assembly in several steps May require re-pretension of bolts to obtain correct pre-tension, due to loss of information regarding contact status Contact status will be included in the dynain file in coming versions 50
40 Stress initialization example Bolt pre-tensioning followed by loading dynain Stage 1: Bolt pre-tension *INITIAL_STRESS_SECTION (ramp) *INTERFACE_SPRINGBACK_LSDYNA Stage 2: Loading *INITIAL_STRESS_SECTION (constant) *LOAD_NODE_SET 51
41 Stress initialization example Bolt pre-tensioning followed by loading Stress history comparison: dynain w. solid lines, all-in-one with dashed 52
42 Stress initialization example Bolt pre-tensioning followed by loading dynain Stresses after pre-tension Stresses after re-pre-tension and standstill (1 s) 53
43 Summary Main keywords in LS-DYNA for bolts pre-tensioning *INITIAL_AXIAL_FORCE_BEAM for pre-tension of beam-style bolts. Applies a force. Requires a spotweld beam (elform 9) with *MAT_SPOTWELD. To obtain an elastic beam bolt, specify a high yield stress. *INITIAL_STRESS_SECTON for solid element bolts. Applies a stress. Works for the common solid elements ±1, ±2, 16 For press-fit in contacts, use MORTAR contact with IGNORE = 3 ( small penetrations) or 4 ( finite penetrations ) *CONTACT_...INTERFERENCE may be an option in some cases for finite penetrations Stress initialization can be used in a staged simulation process, using dynain files (*INTERFACE_SPRINGABACK_LSDYNA) 54
44 Implicit analyses in LS-DYNA Other sources of useful information regarding implicit analyses in LS-DYNA: search conference papers DYNAmore / LSTC also gives courses in implicit analyses: Non-linear implicit analysis in LS-DYNA (T. Borrvall) NVH & Frequency domain analysis in LS-DYNA (A. Jonsson) See also: Please report bugs and errors! To support@dynamore.se 55
45 Thank you! Your LS-DYNA distributor and more 56
46 Alternative procedures for applying bolt pre-tensioning Apply thermal loading to strain the bolt. Model the bolt too short. Stretch the bolt to nominal length using for example *BOUNDARY_PRESCRIBED_MOTION. Let the contact be born. Model the pre-tensioning as a press-fit. Use IGNORE = 3 (or 4) on the MORTAR contact, or alternatively INTERFERENCE contact. Either model the bolt too short as above, or use contact surface augmentation in MORTAR. By these methods, some iterations will be needed to find the right pretensioning. 57
47 Bolt pre-tension issues (IZSHEAR) From R10.0, a new feature is added on *INITIAL_STRESS_SECTION: IZSHEAR Add shear resistance to the cross section In the dev version, the average stress is prescribed instead of constant per integration point. MAT_24 bolt R10.1 dev Pre-tensioning techniques in LS-DYNA-implicit
48 Bolt pre-tension issues (IZSHEAR) From R10.0, a new feature is added on *INITIAL_STRESS_SECTION: IZSHEAR Add shear resistance to the cross section In the dev version, the average stress is prescribed instead of constant per integration point. The temporary remedy for R10 may be to switch to *MAT_ELASTIC in the bolt Original geo R10.1, MAT_24 R10.1, MAT_ELASTIC Pre-tensioning techniques in LS-DYNA-implicit
49 Troubleshooting convergence problems Start out with the suggested control card settings. Check the model integrity Element quality, element types, un-intended cracks in the mesh, element connectivity (beams attached directly to solids by common node(s)) etc. Also beware of element connectivity when coupling *ELEMENT_BEAM elform 6 to other elements. Many pre-processors have built-in tools for model checking Check model connectivity Perform eigenvalue analysis - *CONTROL_IMPLICIT_EIGENVALUE In ANSA: Check > Connectivity > Detect unconnected assemblies Avoid the use of release conditions on Constrained nodal rigid bodies (use joints instead) Also, if possible, on beam elements (use joints or trusses instead) Check that consistent units are used (for materials, loadings, accelerations etc.) Use a moderate (not too small) initial time step. The automatic time step control can only decrease time step size upon RETRY. Check material models 60
Preloads in LS-DYNA. Introduction Analysis Techniques (General) Dynamic Relaxation. Explicit Implicit. Bolt Preload Techniques
Preloads in LS-DYNA Introduction Analysis Techniques (General) Dynamic Relaxation Explicit Implicit Transient Explicit with Mass Damping Implicit Analysis Bolt Preload Techniques Thermal Interference Contact
More informationModeling bolts in LS-DYNA using explicit and implicit time integration
Modeling bolts in LS-DYNA using explicit and implicit time integration Nils Karajan 1, Alexander Gromer 1, Thomas Borrvall 2, Kishore Pydimarry 3 1 DYNAmore Corporation, 565 Metro Place South, Suite 300,
More informationRecent Development of LSDYNA in Stamping Applications. Xinhai Zhu, Li Zhang, Houfu Fan, Yuzhong Xiao LSTC
Recent Development of LSDYNA in Stamping Applications Xinhai Zhu, Li Zhang, Houfu Fan, Yuzhong Xiao LSTC Enhancement in OneStep Method First introduced back in 2011, all quadrilateral elements in the model
More informationUltimate capacity analyses in LS-DYNA. Anders Jonsson,
Ultimate capacity analyses in LS-DYNA Anders Jonsson, anders.jonsson@dynamore.se Ultimate capacity analyses in LS-DYNA A simplified cab frame roof crush load case Dimensions and model data Roof crush load
More informationInput Parameters for Metal Forming Simulation Using LS-DYNA
Input Parameters for Metal Forming Simulation Using LS-DYNA Bradley N. Maker Livermore Software Technology Corporation 7374 Las Positas Road Livermore, CA 94550 (925) 449-2500 maker@lstc.com Xinhai Zhu
More informationTutorial #1 Introduction to LSDyna: Simple Cantilever By C. Daley
Engineering 9093 Ice Class Ship Structures Tutorial #1 Introduction to LSDyna: Simple Cantilever By C. Daley Overview LSDyna is a special type of finite element program produced by Livermore Software Technology
More informationLS-DYNA Implicit Workshop. Problem #1: Tensile Test
LS-DYNA Implicit Workshop Problem #1: Tensile Test Objectives Learn how to activate LS-DYNA s implicit mode. Learn how to select linear or nonlinear analysis. Problem Description A static tensile test
More informationRobuste und effiziente Kontaktmodellierung in LS-DYNA: Wie gut sind die neuen Optionen? Dr.-Ing. Ulrich Stelzmann CADFEM Service
Robuste und effiziente Kontaktmodellierung in LS-DYNA: Wie gut sind die neuen Optionen? Dr.-Ing. Ulrich Stelzmann CADFEM Service Introduction For implicit solution methods nonlinear contact is mostly a
More informationEfficient Topology, Topometry and Sizing Optimisation for LS-DYNA Analysis Problems. Coupling LS-DYNA to VR&D GENESIS
Efficient Topology, Topometry and Sizing Optimisation for LS-DYNA Analysis Problems Coupling LS-DYNA to VR&D GENESIS Martin Gambling Managing Director GRM Consulting Ltd, Leamington Spa, UK Summary: For
More informationContact in LS-DYNA. Feapublications.com. The series is contained in the August, September, October, and December D 2001 newsletters.
Contact in LS-DYNA A good overview of contact is presented in a four part series in archived FEA Information newsletters available at www.feapublications Feapublications.com The series is contained in
More informationNumerical Simulation of Aircraft Seat Compliance Test using LS-DYNA Implicit Solver
Numerical Simulation of Aircraft Seat Compliance Test using LS-DYNA Implicit Solver Satish Pathy LSTC, Livermore, CA Thomas Borrvall DYNAmore Nordic AB, Linköping, Sweden Abstract With the possibility
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 informationQuasi-Static Simulations using Implicit LS-DYNA
14 th International LS-DYNA Users Conference Session: Simulation Quasi-Static Simulations using Implicit LS-DYNA Satish Pathy LSTC, Livermore, CA Thomas Borrvall DYNAmore Nordic AB, Linköping, Sweden Abstract
More informationA Quadratic Pipe Element in LS-DYNA
A Quadratic Pipe Element in LS-DYNA Tobias Olsson, Daniel Hilding DYNAmore Nordic AB 1 Bacground Analysis of long piping structures can be challenging due to the enormous number of shell/solid elements
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 informationLS-DYNA features: Staged Construction
LS-DYNA features: Staged Construction *CONTROL_STAGED_CONSTRUCTION etc This presentation is a basic introduction to Staged Construction in LS-DYNA. See also the Remarks for *CONTROL_STAGED_CONSTRUCTION
More informationLS-DYNA Smooth Particle Galerkin (SPG) Method
LS-DYNA Smooth Particle Galerkin (SPG) Method C.T. Wu, Y. Guo, W. Hu LSTC Element-free Galerkin (EFG) meshless method was introduced into LS-DYNA more than 10 years ago, and has been widely used in the
More informationIntroduction to ANSYS LS-DYNA
Lecture 12 Introduction to ANSYS LS-DYNA Extension 14.5 Release Introduction to ANSYS LS-DYNA 2012 ANSYS, Inc. November 8, 2012 1 Release 14.5 What is ANSYS LS-DYNA Extension ANSYS LS-DYNA in Workbench
More informationBest Practices for Contact Modeling using ANSYS
Best Practices for Contact Modeling using ANSYS 朱永谊 / R&D Fellow ANSYS 1 2016 ANSYS, Inc. August 12, 2016 ANSYS UGM 2016 Why are these best practices important? Contact is the most common source of nonlinearity
More informationContact Modeling in LSDYNA Part 1: Some Recommendations Suri Bala - August, 2001 Livermore Software Technology Corporation
Contact Modeling in LSDYNA Part 1: Some Recommendations Suri Bala - August, 2001 Livermore Software Technology Corporation 1.0 Introduction Contact treatment forms an integral part of many large-deformation
More informationCHAPTER-10 DYNAMIC SIMULATION USING LS-DYNA
DYNAMIC SIMULATION USING LS-DYNA CHAPTER-10 10.1 Introduction In the past few decades, the Finite Element Method (FEM) has been developed into a key indispensable technology in the modeling and simulation
More informationUsing MSC.Nastran for Explicit FEM Simulations
3. LS-DYNA Anwenderforum, Bamberg 2004 CAE / IT III Using MSC.Nastran for Explicit FEM Simulations Patrick Doelfs, Dr. Ingo Neubauer MSC.Software GmbH, D-81829 München, Patrick.Doelfs@mscsoftware.com Abstract:
More informationA Roadmap to Linear and Nonlinear Implicit Analysis in LS-DYNA
A Roadmap to Linear and Nonlinear Implicit Analysis in LS-DYNA George Laird 1, Satish Pathy 2 1 Predictive Engineering, Munich, Germany 2 LSTC, Livermore, USA 1 Abstract The default LS-DYNA settings are
More informationLS-DYNA s Linear Solver Development Phase1: Element Validation Part II
LS-DYNA s Linear Solver Development Phase1: Element Validation Part II Allen T. Li 1, Zhe Cui 2, Yun Huang 2 1 Ford Motor Company 2 Livermore Software Technology Corporation Abstract This paper continues
More informationVehicle Load Area Division Wall Integrity during Frontal Crash
Vehicle Load Area Division Wall Integrity during Frontal Crash H. Türkmen TOFAS Türk Otomobil Fabrikasi A.S. Abstract : This study addresses design efforts of a vehicle load area division wall and the
More informationCurrent Status of Isogeometric Analysis in LS-DYNA
Current Status of Isogeometric Analysis in LS-DYNA Stefan Hartmann Developer Forum, September 24 th, 2013, Filderstadt, Germany Development in cooperation with: D.J. Benson: Professor of Applied Mechanics,
More informationRecent Developments in LS-DYNA II
9. LS-DYNA Forum, Bamberg 2010 Keynote-Vorträge II Recent Developments in LS-DYNA II J. Hallquist Livermore Software Technology Corporation A - II - 7 Keynote-Vorträge II 9. LS-DYNA Forum, Bamberg 2010
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 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 informationDEVELOPMENT OF GUIDELINES FOR DEFORMABLE AND RIGID SWITCH IN LS- DYNA SIMULATION
University of Nebraska - Lincoln DigitalCommons@University of Nebraska - Lincoln Mechanical (and Materials) Engineering -- Dissertations, Theses, and Student Research Mechanical & Materials Engineering,
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 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 informationPresentation of PAM-CRASH v2004. Part 1: Solver News
Presentation of PAM-CRASH v2004 Part 1: Solver News. 1 Overview New Options Elements Materials Others Quality Numerical precision and robustness 2 CRASH/SAFE 2G Evolution V2002: Basic reengineering Common
More informationAdvances in LS-DYNA for Metal Forming (I)
Advances in LS-DYNA for Metal Forming (I) Xinhai Zhu, Li Zhang, Yuzhong Xiao, and HouFu Fan Livermore Software Technology Corporation Abstract The following will be discussed: Enhancements in *CONTROL_FORMING_ONESTEP
More informationEfficient Shape Optimisation of an Aircraft Landing Gear Door Locking Mechanism by Coupling Abaqus to GENESIS
Efficient Shape Optimisation of an Aircraft Landing Gear Door Locking Mechanism by Coupling Abaqus to GENESIS Mark Arnold and Martin Gambling Penso Consulting Ltd GRM Consulting Ltd Abstract: The objective
More informationANSYS LS-DYNA in Mechanical APDL
Lecture 6 Contact Surfaces 14.5 Release ANSYS LS-DYNA in Mechanical APDL 2012 ANSYS, Inc. February 5, 2013 1 Release 14.5 Objectives This lecture covers contact surfaces. The different algorithms are presented,
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 2 nd -order Lagrangian Element in LS-DYNA
Introduction to 2 nd -order Lagrangian Element in LS-DYNA Hailong Teng Livermore Software Technology Corporation Nov, 2017 Motivation Users are requesting higher order elements for implicit. Replace shells.
More informationAdvances in LS-DYNA Metal Forming (II)
Advances in LS-DYNA Metal Forming (II) Xinhai Zhu, Li Zhang & Yuzhong Xiao Livermore Software Technology Corporation Abstract Some of the new features developed since the last conference will be discussed.
More informationRecent European Developments in LS-DYNA
Recent European Developments in LS-DYNA Thomas Borrvall Anders Jernberg Jesper Karlsson DYNAmore Nordic AB Thomas Klöppel Tobias Erhart Stefan Hartmann DYNAmore GmbH Mortar Contact for Classical FEM Goal
More informationCrashbox Tutorial. In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0
Crashbox Tutorial In this tutorial the focus is on modeling a Formula Student Racecar Crashbox with HyperCrash 12.0 (Written by Moritz Guenther, student at Altair Engineering GmbH) 1 HyperMesh* 1. Start
More informationHourglass (HG) Modes. Hourglass (HG) Modes
Hourglass (HG) Modes Hourglass modes are nonphysical modes of deformation that occur in underintegrated elements and produce no stress. By underintegrated, we mean Solid elements with a single integration
More informationSpringback Calculation of Automotive Sheet Metal Sub-assemblies
13 th International LS-DYNA Users Conference Session: Simulation Springback Calculation of Automotive Sheet Metal Sub-assemblies Volker Steininger, Xinhai Zhu, Q. Yan, Philip Ho Tiwa Quest AG, LSTC Abstract
More informationixcube 4-10 Brief introduction for membrane and cable systems.
ixcube 4-10 Brief introduction for membrane and cable systems. ixcube is the evolution of 20 years of R&D in the field of membrane structures so it takes a while to understand the basic features. You must
More informationDURABILITY ADD-ONS FOR ANSA AND µeta
DURABILITY ADD-ONS FOR ANSA AND µeta Dr. Dietmar Fels Ford Werke GmbH / Germany KEYWORDS Durability, Scripting, Pre and Postprocessing ABSTRACT - The functionality of ANSA and µeta has reached an outstanding
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 informationExample 12 - Jumping Bicycle
Example 12 - Jumping Bicycle Summary The purpose of this example is to illustrate how to use the RADIOSS description when resolving a demonstration example. The particularities of the example can be summarized
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 informationManufacturing Simulation of an Automotive Hood Assembly
4 th European LS-DYNA Users Conference Metal Forming III Manufacturing Simulation of an Automotive Hood Assembly Authors: Chris Galbraith Metal Forming Analysis Corporation Centre for Automotive Materials
More informationStiffness Analysis of the Tracker Support Bracket and Its Bolt Connections
October 25, 2000 Stiffness Analysis of the Tracker Support Bracket and Its Bolt Connections Tommi Vanhala Helsinki Institute of Physics 1. INTRODUCTION...2 2. STIFFNESS ANALYSES...2 2.1 ENVELOPE...2 2.2
More informationSpotweld Failure Prediction using Solid Element Assemblies. Authors and Correspondence: Abstract:
Spotweld Failure Prediction using Solid Element Assemblies Authors and Correspondence: Skye Malcolm Honda R&D Americas Inc. Email smalcolm@oh.hra.com Emily Nutwell Altair Engineering Email enutwell@oh.hra.com
More informationThrough Process Modelling of Self-Piercing Riveting
8 th International LS-DYNA User Conference Metal Forming (2) Through Process Modelling of Self-Piercing Riveting Porcaro, R. 1, Hanssen, A.G. 1,2, Langseth, M. 1, Aalberg, A. 1 1 Structural Impact Laboratory
More 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 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 informationA GUIDE TO DEVELOP FEA MODEL. 2D Model (Shell Element) In LS-DYNA
A GUIDE TO DEVELOP FEA MODEL 2D Model (Shell Element) In LS-DYNA By Dr. Rakhmad Arief Siregar CAED Lab. Mechanical Eng. Program Universiti Malaysia Perlis Problem 1: Preprocessing by LS-PREPOST 2.1 1.
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 informationIntroduction to Abaqus. About this Course
Introduction to Abaqus R 6.12 About this Course Course objectives Upon completion of this course you will be able to: Use Abaqus/CAE to create complete finite element models. Use Abaqus/CAE to submit and
More informationNeuerungen in LS-PrePost für das Pre- und Postprocessing von Composites
Neuerungen in LS-PrePost für das Pre- und Postprocessing von Composites Thomas Klöppel DYNAmore GmbH Stuttgart Anders Jernberg DYNAmore Nordic AB Linköping LS-PrePost für Composites - Thomas Klöppel -
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 informationLS-DYNA s Linear Solver Development Phase 1: Element Validation
LS-DYNA s Linear Solver Development Phase 1: Element Validation Allen T. Li 1, Zhe Cui 2, Yun Huang 2 1 Ford Motor Company 2 Livermore Software Technology Corporation Abstract LS-DYNA is a well-known multi-purpose
More informationMAE Advanced Computer Aided Design. 01. Introduction Doc 02. Introduction to the FINITE ELEMENT METHOD
MAE 656 - Advanced Computer Aided Design 01. Introduction Doc 02 Introduction to the FINITE ELEMENT METHOD The FEM is A TOOL A simulation tool The FEM is A TOOL NOT ONLY STRUCTURAL! Narrowing the problem
More informationLS-DYNA s Linear Solver Development Phase 2: Linear Solution Sequence
LS-DYNA s Linear Solver Development Phase 2: Linear Solution Sequence Allen T. Li 1, Zhe Cui 2, Yun Huang 2 1 Ford Motor Company 2 Livermore Software Technology Corporation Abstract This paper continues
More informationStamp a Part Perfectly on the Very First Hit.
Stamp a Part Perfectly on the Very First Hit. Using the right software tool it is possible. DYNAFORM allows you to accurately simulate the stamping of parts to predict formability issues, validate die
More informationLecture 5 Modeling Connections
Lecture 5 Modeling Connections 16.0 Release Introduction to ANSYS Mechanical 1 2015 ANSYS, Inc. February 27, 2015 Chapter Overview In this chapter, we will extend the discussion of contact control begun
More informationAnalyzing Elastomer Automotive Body Seals Using LS-DYNA
7 th International LS-DYNA Users Conference Methods Development Analyzing Elastomer Automotive Body Seals Using LS-DYNA Linhuo Shi TG North America Corporation 95 Crooks Road Troy, MI 4884 Tel: (248) 28-7348
More informationModule 1: Introduction to Finite Element Analysis. Lecture 4: Steps in Finite Element Analysis
25 Module 1: Introduction to Finite Element Analysis Lecture 4: Steps in Finite Element Analysis 1.4.1 Loading Conditions There are multiple loading conditions which may be applied to a system. The load
More informationUsing LS-DYNA from ANSYS Workbench Environment
10 th International LS-DYNA Users Conference Pre/Post and Data Management Using LS-DYNA from ANSYS Workbench Environment Dr.-Ing. Matthias Hörmann CADFEM GmbH, Grafing b. München, Germany mhoermann@cadfem.de
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 informationDevelopment and Validation of Bolted Connection Modeling in LS-DYNA for Large Vehicle Models
14 th International LS-DYNA Users Conference Session: Connections Development and Validation of Bolted Connection Modeling in LS-DYNA for Large Vehicle Models Michalis Hadjioannou, David Stevens, Matt
More informationIntroduction to ANSYS Mechanical
Lecture 6 Modeling Connections 15.0 Release Introduction to ANSYS Mechanical 1 2012 ANSYS, Inc. February 12, 2014 Chapter Overview In this chapter, we will extend the discussion of contact control begun
More informationShape and parameter optimization with ANSA and LS-OPT using a new flexible interface
IT / CAE Prozesse I Shape and parameter optimization with ANSA and LS-OPT using a new flexible interface Korbetis Georgios BETA CAE Systems S.A., Thessaloniki, Greece Summary: Optimization techniques becomes
More informationFirst Order Analysis for Automotive Body Structure Design Using Excel
Special Issue First Order Analysis 1 Research Report First Order Analysis for Automotive Body Structure Design Using Excel Hidekazu Nishigaki CAE numerically estimates the performance of automobiles and
More informationA Topology Optimization Interface for LS-Dyna
A Topology Optimization Interface for LS-Dyna Dipl.-Ing. Nikola Aulig 1, Dr.- Ing. Ingolf Lepenies 2 Optimizer LS-Dyna 1 nikola.aulig@honda-ri.de Honda Research Institute Europe GmbH, Carl-Legien-Straße
More informationStep Change in Design: Exploring Sixty Stent Design Variations Overnight
Step Change in Design: Exploring Sixty Stent Design Variations Overnight Frank Harewood, Ronan Thornton Medtronic Ireland (Galway) Parkmore Business Park West, Ballybrit, Galway, Ireland frank.harewood@medtronic.com
More 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 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 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 informationAppendix A: Mesh Nonlinear Adaptivity. ANSYS Mechanical Introduction to Structural Nonlinearities
Appendix A: Mesh Nonlinear Adaptivity 16.0 Release ANSYS Mechanical Introduction to Structural Nonlinearities 1 2015 ANSYS, Inc. Mesh Nonlinear Adaptivity Introduction to Mesh Nonlinear Adaptivity Understanding
More informationInvestigating the influence of local fiber architecture in textile composites by the help of a mapping tool
Investigating the influence of local fiber architecture in textile composites by the help of a mapping tool M. Vinot 1, Martin Holzapfel 1, Christian Liebold 2 1 Institute of Structures and Design, German
More informationVALIDATE SIMULATION TECHNIQUES OF A MOBILE EXPLOSIVE CONTAINMENT VESSEL
VALIDATE SIMULATION TECHNIQUES OF A MOBILE EXPLOSIVE CONTAINMENT VESSEL David Karlsson DYNAmore Nordic AB, Sweden KEYWORDS Hexa, Map, Explosive, LS-DYNA ABSTRACT A Mobile Explosive Containment Vessel (MECV)
More informationLinear and Nonlinear Analysis of a Cantilever Beam
LESSON 1 Linear and Nonlinear Analysis of a Cantilever Beam P L Objectives: Create a beam database to be used for the specified subsequent exercises. Compare small vs. large displacement analysis. Linear
More informationNUMERICAL INVESTIGATION OF SELF-PIERCING RIVETED DUAL LAYER JOINT. A Thesis by UMA SHANKAR KRISHNAPPA. Bachelor of Engineering, UVCE, India, 2004
NUMERICAL INVESTIGATION OF SELF-PIERCING RIVETED DUAL LAYER JOINT A Thesis by UMA SHANKAR KRISHNAPPA Bachelor of Engineering, UVCE, India, 2004 Submitted to the Department of Mechanical Engineering and
More informationEngineering Analysis
Engineering Analysis with SOLIDWORKS Simulation 2018 Paul M. Kurowski SDC PUBLICATIONS Better Textbooks. Lower Prices. www.sdcpublications.com Powered by TCPDF (www.tcpdf.org) Visit the following websites
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 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 informationScientific Manual FEM-Design 17.0
Scientific Manual FEM-Design 17. 1.4.6 Calculations considering diaphragms All of the available calculation in FEM-Design can be performed with diaphragms or without diaphragms if the diaphragms were defined
More 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 informationThe Immersed Smoothed Particle Galerkin Method in LS-DYNA for Material Failure Analysis of Fiber-Reinforced Solid Structures
The Immersed Smoothed Particle Galerkin Method in LS-DYNA for Material Failure Analysis of Fiber-Reinforced Solid Structures Wei Hu, C. T Wu Livermore Software Technology Corporation, 7374 Las Positas
More informationDesign Verification Procedure (DVP) Load Case Analysis of Car Bonnet
Design Verification Procedure (DVP) Load Case Analysis of Car Bonnet Mahesha J 1, Prashanth A S 2 M.Tech Student, Machine Design, Dr. A.I.T, Bangalore, India 1 Asst. Professor, Department of Mechanical
More informationR15.0 Structural Update
R15.0 Structural Update 1 Tim Pawlak R&D Fellow ANSYS Structural Update Topics Geometry and Mesh Material Behavior Numerical Methods Composites Dynamics Submodeling Multiphysics Solvers User Interface
More informationModeling Bolted Connections. Marilyn Tomlin CAE COE / Siemens Corporation
Modeling Bolted Connections Marilyn Tomlin CAE COE / Siemens Corporation Overview Bolted Connection Engineering Judgment Modeling Options Summary Typical Bolted Connection Gasket Bolt Nut Washer Technology
More informationRecent developments in OASYS Primer
Recent developments in OASYS Primer October 2004 Miles Thornton Engineering consultancy 7000 staff worldwide Arup is our founder s name, Ove Arup Oasys = Ove Arup Systems 2004 Copyright by DYNAmore GmbH
More informationValidation of blast simulation models via drop-tower tests
Validation of blast simulation models via drop-tower tests Master s Thesis in Engineering Physics Author Joakim Rydman June 16, 2018 Supervisor: Jörgen Vedin, BAE Systems Hägglunds Examiner: Staffan Schedin,
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 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 informationEPILYSIS. The new FEA solver
EPILYSIS The new FEA solver The most promising and dynamically developed solver for our contemporary needs EPILYSIS serves as a contemporary solution in the field of Finite Element Analysis, embodying
More informationPractical Examples of Efficient Design Optimisation by Coupling VR&D GENESIS and LS-DYNA
Practical Examples of Efficient Design Optimisation by Coupling VR&D GENESIS and LS-DYNA David Salway, GRM Consulting Ltd. UK. Paul-André Pierré, GRM Consulting Ltd. UK. Martin Liebscher, Dynamore GMBH,
More informationUsing LS-DYNA from ANSYS Workbench Environment
Using LS-DYNA from ANSYS Workbench Environment Dr.-Ing. Matthias Hörmann, M.Sc Madhukar Chatiri CADFEM GmbH, Grafing b. München, Germany mhoermann@cadfem.de, mchatiri@cadfem.de Abstract Numerical simulations
More informationOptimization of turbine blade fir-tree root geometry utilizing LS-Prepost in pre- and post-processing
Optimization of turbine blade fir-tree root geometry utilizing LS-Prepost in pre- and post-processing Jiří Jankovec 1 1 Research and Testing Institute Plzen, Czech Republic Abstract The turbine blade fir-tree
More informationImproving Crash Analysis Through the Estimation of Residual Strains Brought About by Forming Metal
7 th International LS-DYNA Users Conference Crash/Safety () Improving Crash Analysis Through the Estimation of Residual Strains Brought About by Forming Metal William Broene, PE Manager of Engineering
More information