Contents. 1 Introduction. 2 Theoretical Background

Transcription

1 Contents 1 Introduction Introduction Analysis Capabilities Main Analysis Features Load Excitation Base Excitation Damping Response Calculations Stress Calculation Theoretical Background Introduction Normal Mode Analysis Damping Effects Rayleigh Damping Modal Damping Concentrated Dampers Composite Modal Damping Solution Accuracy Considering Mode Truncation Force Excitation Problems Base Excitation Problems COSMOSM Advanced Modules i

2 Contents Modal Acceleration Method (MAM) in Time History Missing Mass Correction Technique in Response Spectrum Excitation Due to Base Motion Uniform Translational Base Motion Multi-Base Motion Time History Analysis Solution Accuracy Loading Options Available Concentrated Dampers and Gap Elements Response Spectrum Analysis Definition of Response Spectrum Modal Maximum Response Structure Maximum Response Multiple Response Spectra Response Spectra Generation Random Vibration Analysis Basic Definitions Analysis Procedure Methods of Integration Partial (Spatial) Correlation Steady State Harmonic Analysis Analysis Procedure Direct Spectrum Generation Time History Generation Description of Elements Introduction Brief Description of Commands Introduction ii COSMOSM Advanced Modules

3 Part 1 ASTAR Advanced Dynamics Analysis Main POST_DYN Menu PD DAMP/GAP Submenu PD CURVES Submenu PD BASE EXCITATION Submenu PD OUTPUT Submenu Postprocessing of Dynamic Results XY-Plot of Response Plot of Response XY-Plot of Stresses Plot of Stresses Other Postprocessing Options Post Dynamic Input Procedure Typical Input Procedure Detailed Description of Examples Introduction Dynamic Analysis of a Cantilever Beam Analysis Types Statement of the Problem Frequency Analysis of the Problem Modal Time History Random Vibration Dynamic Analysis of a Culvert Analysis Types Given GEOSTAR Commands Modal Time History Analysis Response Spectrum Generation Harmonic Analysis Random Vibration Analysis Response Spectrum Analysis COSMOSM Advanced Modules iii

4 Contents Multi-Base Motion Application with Composite Material Damping Dynamic Analysis of a Plate Analysis Type Statement of the Problem GEOSTAR Inputs Verification Problems Index iv COSMOSM Advanced Modules

5 First Edition COSMOSM 2.9 August 2004 Copyright Structural Research and Analysis Corp. is a Dassault Systemes S.A. (Nasdaq: DASTY) company. This software product is copyrighted and all rights are reserved by Structural Research and Analysis Corporation. (SRAC) Copyright Structural Research and Analysis Corporation. All Rights Reserved. The distribution and sale of this product is intended for the use of the original purchaser only and for use only on the computer system specified. The software product may be used only under the provisions of the license agreement that accompanies the product package. COSMOSM manuals may not be copied, photocopied, reproduced, translated or reduced to any electronic medium or machine readable form in whole or part wit prior written consent from Structural Research and Analysis Corporation. Structural Research and Analysis Corporation makes no warranty that COSMOSM is free from errors or defects and assumes no liability for the program. Structural Research and Analysis Corporation disclaims any express warranty or fitness for any intended use or purpose. You are legally accountable for any violation of the License Agreement or of copyright or trademark. You have no rights to alter the software or printed materials. The COSMOSM program is constantly being developed, modified and checked and any known errors should be reported to Structural Research and Analysis Corporation. Disclaimer The authors have taken due care in preparing this manual and the examples presented herein. In no event shall SRAC assume any liability or responsibility to any person or company for direct or indirect damage resulting from the use of the information contained herein or any discrepancies between this information and the actual operation of the software. Licenses & Trademarks Use by Structural Research and Analysis Corporation of ANSYS Input Commands and Command Structure herein is licensed under agreement with Swanson Analysis Systems, Inc. All rights reserved. COSMOSM and COSMOS are registered trademarks of Structural Research and Analysis Corporation. All other COSMOSM module names are trademarks of Structural Research and Analysis Corporation. ABAQUS is the registered trademark of Hibbitt, Karlsson & Sorensen, Inc. ANSYS is a registered trademark of Swanson Analysis Systems. AutoCAD is registered in the U.S. Patent and Trademark Office by Autodesk, Inc. DXF and AutoSolid are the registered trademarks of Autodesk, Inc. CenBASE/ Mil5 is the registered trademark of Information Indexing, Inc. DECStation is the registered trademark of Digital Equipment Corporation. EPSON is the registered trademark of Epson Computers. HP is the registered trademark of Hewlett-Packard. IBM is the registered trademark of International Business Machines Corporation. MSC/NASTRAN is the registered trademark of MacNeal-Schwendler Corp. PATRAN is the registered trademark of PDA Engineering. PostScript, Acrobat, and Acrobat Reader are registered trademarks of Adobe Systems, Inc. SINDA/G is a registered trademark of Network Analysis Associates, Inc. Sun is the registered trademark of Sun Microsystems, Inc. SGI is the trademark of Silicon Graphics, Inc. SoliWorks is a registered trademark of SolidWorks Corporation. Helix Design System is a trademark of MICROCADAM Inc. SDRC I-DEAS is a trademark of Structural Dynamics Research Corporation. MicroStation Modeler is a registered trademark of Bentley Systems, Incorporated. Solid/Edge is a trademark of Intergraph Corporation. Eureka is a trademark of Cad.Lab. All other trade names mentioned are trademarks or registered trademarks of their respective owners.

6 ii COSMOSM Advanced Modules

7 1 Introduction Introduction The Advanced Dynamic module, ASTAR or POST DYNAMIC, has three principal functions. The first is to perform linear dynamic analysis of systems subject to different categories of forcing functions; the second is to carry out stress calculations subsequent to a dynamic analysis; and finally to accommodate plot files required for graphic evaluations of the system response at specific nodes and/or solution steps. The various dynamic capabilities of the program are based on the normal mode method. It is therefore essential that the frequency and mode shape calculations are done prior to the application of this module (except for the curve transformation problems) for the solution of the desired dynamic response problem. Note that the GEOSTAR program controls the complete operations of the COSMOSM package and all modules are accessed from there. In the Post Dynamic analysis, after running for frequencies, the POST_DYNAMIC submenu can be accessed from the main ANALYSIS menu in order to set up the input required for any of the several different analysis options listed in the next section. COSMOSM Advanced Modules 1-1

8 Chapter 1 Introduction Analysis Capabilities The Advanced Dynamic module is used for the solution of dynamic response problems listed below: Modal Time History Response Spectra Response Spectra Generation Random Vibration Steady State Harmonic Curve Transformation As stated earlier, these analyses options are based on the normal mode method for which modes and frequencies must be determined in advance (except for curve transformation problems). This can be accomplished through GEOSTAR in which the model is initially created and then analyzed for its modes and frequencies based on the lumped or consistent mass options using DSTAR. Each of these analysis options can then be performed by considering any combination of the four excitation types noted below: Concentrated Forces specified in any coordinate system Pressure Loads specified in any coordinate system Uniform Base Motion defined in the global or local Cartesian system Multi-Base Motion defined in the global or local Cartesian system A brief theoretical description of the different analysis types is provided in Chapter 2. Main Analysis Features 1. Modal Time History Analysis Response of structures excited by time varying forces or base excitations may be evaluated using this option. The uncoupled modal equations of motion are solved by using the step-by-step integration technique of the Wilson-Theta or the Newmark Method. 1-2 COSMOSM Advanced Modules

9 Part 1 ASTAR Advanced Dynamics Analysis All structural elements available in the COSMOSM element library are supported. Linear gap elements may also be created. Concentrated dampers at specified nodes are available for Time History analysis in addition to Modal damping, Rayleigh and composite dampings options. The evaluated response consists of displacements, velocities and accelerations as well as stresses (internal forces for 1D elements). Options available for postprocessing are discussed in Chapter 4 under Postprocessing of Dynamic Results. A detailed description of solution techniques is available in Chapter Response Spectra Analysis The maximum response of a structure can be evaluated for a specified base spectrum. Several options are available for mode combination techniques including the Absolute Sum, Square Root Sum of Squares (SRSS), Complete Quadratic Combination (CQC), and the Naval Research Laboratory (NRL) methods. The evaluated response consists of maximum displacements, velocities, and accelerations as well as stresses at each node. Modal, Rayleigh and composite material damping options are available for this type of analysis. Options available for postprocessing are discussed in Chapter 4 under postprocessing of dynamic results. A detailed description of solution techniques is available in Chapter Response Spectra Generation The response spectrum curves at a specified node are evaluated by using the already calculated modal time response of the structure at that node. The evaluated spectra represents the maximum response amplitude of a single degree of freedom system at various oscillating frequencies for a specified damping ratio. The response spectra can be generated for specified nodal displacements, velocities and/or accelerations. Options available for postprocessing are discussed in Chapter 4 under Postprocessing of Dynamic Results. A detailed description of solution techniques is available in Chapter Random Vibration Analysis The response of structures to random excitations is evaluated using this option. The input may be in the form of Power Spectra Densities (PSD) of applied loads or base excitations versus frequency. The output includes response in the form of PSD of displacements, velocities, accelerations and stresses. In addition, the RMS of response (which for stationary, Gaussian excitation with mean value of zero, is equivalent to one standard deviation of the response, i.e., the actual response can be assumed to be at or below this one standard deviation value about 68% of the time) is evaluated in order to completely determine the statistical behavior of the response. Modal, Rayleigh and composite material COSMOSM Advanced Modules 1-3

10 Chapter 1 Introduction damping options are available for this type of analysis. Options available for postprocessing are discussed in Chapter 4 under Postprocessing of Dynamic Results. A detailed description of solution techniques is available in Chapter Steady State Harmonic Analysis In this case, the response of structures to harmonic forces or base excitations for a range of frequencies is evaluated, i.e., the amplitude of the resulting system response as well as the phase angle of the response (relative to the applied force) are calculated. The system response is evaluated for displacements, velocities, accelerations and stresses. Modal, Rayleigh and composite material damping options are available for this type of analysis. Options available for postprocessing are discussed in Chapter 4 under Postprocessing of Dynamic Results. A detailed description of solution techniques is available in Chapter Curve Transformation The curve transformation option is used to perform the following analyses: a. Direct Spectrum Generation b. Time History Generation Frequency analysis is not required prior to performing these analyses. The objective of Direct Spectrum Generation is to evaluate spectra curves for a given time history curve, whereas, the Time History Generation, evaluates time history records from the user defined acceleration response spectra curve. Options available for postprocessing are discussed in the on-line Help for the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command. Load Excitation Load excitations may be applied as concentrated loads at specified nodes or as distributed pressure applied to specified element faces. Depending on the type of analysis, loads may have arbitrary patterns in the time or frequency domain. You may define up to 100 time or frequency curves and associate them with loads as desired. Force and pressure loading is applicable to all the above mentioned types of analyses except the Response Spectra analysis and curve transformation problems. Forces can be defined in global or local coordinates. 1-4 COSMOSM Advanced Modules

11 Part 1 ASTAR Advanced Dynamics Analysis Base Excitation The excitation to the structure may be specified in terms of base motion (displacement, velocity or acceleration) instead of or in addition to the applied mechanical loads. In this case the previously constrained nodes of the structure (during frequency analysis) are assumed to have motions which follow certain patterns described in the time or frequency domains. You may define up to 100 patterns by creating time or frequency curves and associating them with all the constrained nodes in a certain direction to define uniform base excitation, or associating them with a subset of the nodes constrained in a given direction to define multi-base motion. Base motions are supported in all types of analyses in ASTAR. Both uniform and multi-base motions can be defined in local and global Cartesian coordinates. For a theoretical review of the subject, please refer to Chapter 2. Damping There are several options for consideration of structural damping in linear dynamic analysis using the ASTAR module. 1. Rayleigh damping, where the damping matrix is assumed to be proportional to the modal mass and the modal stiffness matrices (applicable to all types of analysis excluding curve transformation problems). 2. Modal damping, where you directly define the modal damping ratio for each mode (applicable to all types of analysis). 3. Concentrated dampers, where you specify damping between two nodes of the structure (applicable only to Time History). 4. Composite modal damping, where you specify damping as a material property before performing frequency analysis, and the program evaluates the equivalent modal damping ratios for each mode (applicable to all types of analysis excluding curve transformation problems). For a detailed review of this subject, please refer to the appropriate section of Chapter 2. COSMOSM Advanced Modules 1-5

12 Chapter 1 Introduction Response Calculations For all available analysis options, the response of structures at certain nodes may be calculated for the displacement, velocity and acceleration versus time (in Modal Time History) or versus frequency (in PSD of Random Vibration, Harmonic Analysis, and Response Spectra Generation) or simply as the maximum value (in Response Spectra Analysis) or RMS (in Random Vibration). The user may request to have these results written in the output file or have them written in plot files for graphical display (see the postprocessing of dynamic results section of Chapter 4). Stress Calculation For all the analysis options except Response Spectra Generation and Curve Transformation problems, the stresses can be calculated for all element groups supported by DSTAR. Both nodal and element stresses are evaluated. Stresses versus time or frequency (similar to the response) can be requested and if so will be available in both the output file and plot file. 1-6 COSMOSM Advanced Modules

13 2 Theoretical Background Introduction In this chapter, a brief theoretical discussion on the various linear dynamic response analysis options supported by the Post Dynamic module (ASTAR) is presented. In the nonlinear module (NSTAR), the equations of motion for both linear and nonlinear systems are solved by direct integration. However, problems with a large number of equations or degrees of freedom (DOF) often require less computation time if the dynamic behavior of the linear structure can be approximated with sufficient accuracy by only the first few modes (nf), where nf<<dof. The trade-off between computational economy and accuracy revolves around the necessity of calculating the eigenvalues of the system of equations. The process of approximating the solution of the equations of motion by considering only the first few modes of the system's natural frequencies is called normal mode or modal superposition analysis and in the Advanced Dynamic Module, all forced-vibration response problems are based on this procedure. Normal Mode Analysis The equations of motion for a linear dynamic system are: COSMOSM Advanced Modules 2-1

14 Chapter 2 Theoretical Background (2-1) where: [M] [C] [K] {f(t)} = mass matrix = damping matrix = stiffness matrix = time varying load vector are the displacement, velocity, and acceleration vectors, respec- and tively. For linear dynamic problems, the system of equations of motion (Eq. 2-1) can be decoupled into nf single degree of freedom equations in terms of the modal displacement vector {x}, where: (2-2) and [Φ] is the matrix of the lowest nf eigenvectors obtained from the solution of: (2-3) Substituting for {u} from (Eq. 2-2) into (Eq. 2-1) and premultiplying it by [Φ] T, will yield: (2-4) With the mode shapes satisfying the orthogonality conditions, Eq. (2-4) becomes: (2-5) Eq. (2-5) represents nf uncoupled single degree of freedom (second-order differential) equations as shown below: (2-6) 2-2 COSMOSM Advanced Modules

15 Part 1 ASTAR Advanced Dynamics Analysis These equations can be evaluated using step-by-step integration or other techniques, and the displacements {u} and other system responses can then be determined by performing the transformation shown in Eq. (2-2). Damping Effects The damping matrix [C] is assumed to satisfy the orthogonality conditions. It should be noted that in the majority of cases, (a) the exact damping matrix is unknown, and (b) the effect of any non-orthogonality is usually small. In the Post Dynamic module, the following damping options are available. Rayleigh Damping Rayleigh damping is of the form: [C] = α [M] + β [K] (2-7) This form of [C] is orthogonal with respect to the system eigenvectors, and the modal damping coefficient for the i th mode C i may be calculated: C i = 2 ξ i ω i = α + β ω i 2 (2-8) and in terms of the modal critical damping ratio ξ i = α / (2 ω i ) + β ω i / 2 (2-9) where α and β are the Rayleigh damping coefficients. Modal Damping Modal damping is defined as a fraction of critical damping ξ i = C i / C c (2-10) COSMOSM Advanced Modules 2-3

16 Chapter 2 Theoretical Background Concentrated Dampers Concentrated dampers can be defined between any two nodes or any one node and the ground for only the modal time history analysis option. The damping coefficients are defined in terms of their components in the global X, Y, and Z-directions as shown in Figure 2-1. Figure 2-1. Concentrated Dampers Node_1 Y DY Z X Node_2 Composite Modal Damping Composite modal damping allows for the definition of the damping coefficient as a material property. Thus, different element groups representing different materials can be assigned different damping coefficients during a post dynamic analysis. This option provided on the basis of NRC recommendation, is defined below in the form of equivalent modal damping ratios: (2-11) where: = equivalent modal damping ratio of the j th mode = j th normalized modal eigenvector = modified structural mass matrix constructed from element matrices formed by the product of the damping ratio for the element and its mass matrix 2-4 COSMOSM Advanced Modules

17 Part 1 ASTAR Advanced Dynamics Analysis Gap-Friction Element The Gap-Friction element is defined by two nodes representing the distance between any two points in a two- or three-dimensional model. The actual gap separation is defined independent of the node locations and can assume any value including the distance between the nodes. The element resists either compression or tension depending on whether the gap distance is positive or negative. Figure 2-2 illustrates the element and its force-deflection relationship in both compressive and tensile modes. Figure 2-2. Gap-Friction Element Node_1 F s F n Compressive Gap Force V (+) Gdist rel (+) S Gstiff Displacement Node_2 F s 1 F n F n Fs = Friction force in s-direction > G fic * Fn Fn = Comprehensive or tensile gap force in the n-direction and proportional to Vrel Vrel = Relative velocity in the s-direction F s Node_1 V rel Force (-) S 1 Gstiff Displacement Node_2 F s (-) Gdist F n Tensile Gap COSMOSM Advanced Modules 2-5

18 Chapter 2 Theoretical Background As shown in Figure 2-2, the element is assumed to be a compressive gap when the gap distance is positive, and only compressive forces result from its closure. Conversely, it is characterized as a tensile gap element when the distance (G dist ) is negative and tensile forces are produced at the closing stage. An iterative procedure is adopted in the solution of problems involving gap elements. The iteration is performed at the end of each time step on gap elements closed, to ensure convergence of the force in the element to its correct value corresponding to the relative displacement between the two nodes. Frictional forces may also be considered in conjunction with gap elements if the coefficient of friction is supplied. This effect is currently accounted for in the X-Y plane only, along the direction normal to the element axis. Sliding resistance develops once the gap is closed. Maximum force of friction at each time step is equal to the product of normal force Fn and the coefficient of friction. In the program, no arbitrary stiffness value is assigned to the friction element. Instead, the frictional force effects are computed on the basis of relative velocities of the two nodes defining the gap element during each time step. Solution Accuracy Considering Mode Truncation The solution accuracy of dynamic problems based on the normal mode method depends to a large extent on the number of modes considered. Below a few possible options as well as certain remedial steps available in the Interface to improve the solution accuracy are discussed for the various analysis types and loading conditions. Force Excitation Problems In the case of systems under the influence of force excitations, it is essential that all modes which contribute to the static deformation shape of the structure are considered. The following example shows that at least five modes should be included for this case. 2-6 COSMOSM Advanced Modules

19 Part 1 ASTAR Advanced Dynamics Analysis Figure 2-3. Mode Shapes of a Simply-Supported Beam Requires Five Modes Mode 1 Mode 3 Mode 4 Mode 2 Mode 5 Base Excitation Problems In dynamic problems under the influence of base excitations, usually the number of modes considered must contribute to a total mass participation factor of at least 80% of the system mass in the direction of the base motion. For harmonic and random vibration problems, in addition to the 80% mass participation factor requirement, the range of natural frequencies considered for the analysis must cover the highest frequency in the excitation. Modal Acceleration Method (MAM) in Time History The process of mode truncation, as was explained before, introduces some error in the response. The Modal Acceleration Method (MAM), in the Time History Analysis, approximates the effects of the truncated modes by their equivalent static effects. This approximation can be expressed for the displacement by: U c = [K] -1 {R c } COSMOSM Advanced Modules 2-7

20 Chapter 2 Theoretical Background where, K is the structural stiffness matrix and R c represents the static loading. It can be shown that this static load vector can be computed in terms of the included modes, according to: R c = [I - M Φ Φ T ] {P(t)} where, M and Φ are the mass matrix and modal matrix, respectively, {P(t)} is the applied dynamic load, and Φ T is the mass matrix transpose. For a demonstration of the MAM on the improvement of the accuracy, please refer to Chapter 5. Thus by considering only a few number of modes, for even very complicated geometry, you are able to evaluate the response accurately. Missing Mass Correction Technique in Response Spectrum Truncation of higher modes in the modal analysis always introduces some error in the results. This truncation means that some mass of the system is ignored. The distribution of this missing mass is such that the inertia forces associated with it will usually produce only small displacements and stresses. However, these ignored inertia forces will often produce significant displacements (stresses) for stiff systems or at the close proximity of the structural supports. The Missing Mass Correction technique is incorporated in the ASTAR program for Response Spectrum analysis in order to estimate the error introduced by the ignored higher modes and to improve the results. This correction is presented as a factor in the output file immediately after the printed accelerations. The user may apply this factor to improve the accuracy of the results obtained for accelerations or stresses. Excitation Due to Base Motion The various analysis modes available in ASTAR may be considered in conjunction with either uniform base motion, multi-base motion, or both. Uniform Translational Base Motion The equations of motion for a linear dynamic system with uniform base acceleration, can be written as: 2-8 COSMOSM Advanced Modules

21 Part 1 ASTAR Advanced Dynamics Analysis (2-12) where {u r } is the structure displacement relative to the base, and {f e (t)} is an effective load due to the base motion: (2-13) The vector {I b } is an influence vector relating base motion to rigid body structure displacements according to: {U} = {u r } + {I b } u b (t) (2-14) The equations of motion Eq. (2-12) can be transformed into uncoupled equations in terms of the modal displacements {x} where: {u r } = [Φ] {x} (2-15) and the equation of motion Eq. (2-12) becomes (2-16) where [Γ] is the modal participation factor for the lowest nf eigenvectors, i.e., (2-17) Therefore for each mode i, the participating factor is: (2-18) and the participation mass for each mode i is Γ i 2. Thus: ΣΓ i 2 = total participating (effective) mass in the direction of motion. COSMOSM Advanced Modules 2-9

22 Chapter 2 Theoretical Background Uniform Rotational Base Motion In the presence of rotational motion, the base motion is not the same at each base point and cannot be described by a constant ü b as done in the case of uniform translational base motion (Eq. 2-13). Consider the absolute displacement of a base point p where position is specified by vector r p with respect to a moving frame of reference with origin o. Let the translation of the origin o with respect to the absolute frame of reference be g o, and let the rotation of the point o in respect to the absolute frame of reference be θ, then the total acceleration of base point p is specified by: (2-19) The acceleration term,, indicates that superposition of base rotations cannot be used. Further, the Coriollis acceleration term, ν p ; making the problem nonlinear., includes the response The assumption made here is that these two terms are negligible, and that for rotational base motion only the tangential acceleration term, needs to be included. Thus for rotational (and translational) base motion. (2-20) With this approximation, ü for point p can be found from Eq as: (2-21) Where x p, y p, and z p are the coordinates of the point p with respect to the rotating frame of reference with origin o COSMOSM Advanced Modules

23 Part 1 ASTAR Advanced Dynamics Analysis In Eq. 2-13, the right hand term, then is replaced by, where it consists of the acceleration at all base points calculated by the above equation. Multi-Base Motion The application of different support motions to different groups of constrained nodes or supports may also be considered. In this case, the equations of motion can be written as: (2-22) where a denotes structure degrees of freedom and b refers to support degrees of freedom. The superscript t signifies that these displacements are total or absolute displacements differentiating them from relative displacements. In the above equations, the effect of damping may have also been considered. Next, we will examine the response of the system when the support displacements u b are applied in a static manner associated with a single time function, i.e., (2-23) The static application of u b means that the time variation is absent and the applied displacement vector is equal to. Eq. (2-22) are then reduced to: (2-24) in which are the structure displacements and represent support forces. Eq. (2-24) gives: (2-25) COSMOSM Advanced Modules 2-11

24 Chapter 2 Theoretical Background or (2-26) On multiplying both sides of Eq. (2-26) by f(t), the quasi-static part of the response is obtained. (2-27) The total displacement u a t can be expressed by the superposition of the quasi-static and the relative displacements, so that: (2-28) Substitution of Eq. (2-28) into the first part of Eq. (2-22) give: (2-29) Now because, (2-30) Eq. (2-29) reduces to: (2-31) Eq. (2-31), written in terms of the relative displacements {u a }, is equivalent to equations of motion (2-12) (ignoring damping), with the forcing function being a function of the base motion ü b. It can therefore be solved by the application of the mode super-position method as described before. A major simplification results when the motion is assumed to be identical for all the supports, in which case Eq. (2-31) will reduce to undamped form of Eq. (2-16) following the mode superposition application COSMOSM Advanced Modules

25 Part 1 ASTAR Advanced Dynamics Analysis Time History Analysis In time history analysis problems, the equations of motion for multi degree-of-freedom systems are solved considering different dynamic loadings and base excitation functions. The normal mode method is first used to obtain the uncoupled equations of motion as discussed earlier and shown by Eq. (2-6), i.e., Next, one of two step-by-step integration methods available in COSMOSM, that is either (a) the Wilson-Theta method or (b) the Newmark method (see Reference 6), is used to evaluate the response of each mode. These techniques use the results obtained in one previous step to solve for those in the next step. The integration is performed in the time domain starting from time at the last step and ending with the time at the current step (which is equal to the time-step increment). Thus, by reducing the time increment between consecutive steps, accuracy of the solution can be improved. The system response is then determined at each time step using the following transformation: {u} = [Φ] {x} In Figure 2-4, some typical loading functions are shown. Figure 2-4. Known Functions of Time F(t) F(t) F(t) Time Time Time Harmonic Loading Periodic Loading Shock Loading Solution Accuracy The solution accuracy in time-history analysis problems, as in all cases, depends on: 1. Number of modes considered. 2. Now, accurately, the modes are calculated (i.e., accuracy in modeling). COSMOSM Advanced Modules 2-13

26 Chapter 2 Theoretical Background 3. Integration increment or time-step size, (smaller than 1/10 th of the last mode period is recommended). Loading Options Available 1. Force or pressure loadings associated with time curves. 2. Uniform base motion, i.e., the entire constraint portion of the model is subjected to the same motion specified by a time curve. (See PD_BASEFAC [Analysis > POST_DYNAMIC > PD BASE EXCITATION > Base Excitation Factor) commands.] 3. Multi-base motion application, i.e., different groups of constraint nodes are subjected to motions defined by different time curves. (See PD_SPPRT [Analysis > POST_DYNAMIC > PD BASE EXCITATION > Support Level) commands.] 4. Initial conditions can be specified in the form of initial displacements, velocities, or accelerations to a group of nodes. [See INITIAL (LoadsBC > LOAD_OPTIONS > Initial Condition) command.]. Concentrated Dampers and Gap Elements Concentrated dampers and gap elements can be modeled only in conjunction with the time history analysis option. Gap elements are introduced in modal analysis as truss elements which can resist either tension or compression, once a certain distance between two nodes is reached. Also, concentrated dampers can be defined between two nodes or between one node and the ground. Their effect is considered in the modal analysis by applying forces at the proper nodes. The forces, due to gap elements, are proportional to gap distances while the forces resulting from dampers are in proportional with differential nodal velocities. More detailed information on these two features is provided in the earlier parts of this chapter. Response Spectrum Analysis The capability to perform response spectrum analysis of linear elastic structures subject to base motion, is included in the ASTAR module of the COSMOSM program. The normal mode method is first used to transform the problem into uncou COSMOSM Advanced Modules

27 Part 1 ASTAR Advanced Dynamics Analysis pled generalized modal coordinates. The maximum modal responses are then determined from the input response spectrum, and the structure response is found by summing the contributions from each mode. Definition of Response Spectrum A response spectrum is the maximum response of a single degree of freedom system subjected to a particular base motion plotted as a function of the natural frequency of the single DOF system. Different curves are usually plotted for different values of the modal damping ratio of the single DOF system as shown in Figure 2-5. The usual values plotted are the maximum displacement S d (ω i,ξ i ), the maximum pseudo-velocity S v (ω i,ξ i ), and the maximum pseudo-acceleration S a (ω i,ξ i ) responses. These three responses are related by: S a = ω S v = ω 2 S d (2-32) and all can be plotted as a single curve on appropriately scaled graph paper. Figure 2-5. Response Spectrum Curves S d ξ 3 ξ 2 ξ 1 Modal Damping ω Modal Maximum Response As each mode is a single DOF system, the maximum modal response can be obtained from the input response spectrum curve as shown below. (2-33) COSMOSM Advanced Modules 2-15

28 Chapter 2 Theoretical Background (2-34) (2-35) where Γ i is the modal participation factor for each mode i (see Eq. 2-17) and i=1, 2,...nf. Then for each mode i, the structure maximum response can be found from Eq. (2-15), i.e., or (2-36) (2-37) and (2-38) Structure Maximum Response The maximum modal responses cannot be simply added to obtain the structure maximum response because the occurrences of the maximum modal response in the time domain are not known. However, several recommended approaches exist and the following mode combination techniques are available in the Interface. Absolute Sum This is a conservative approach in which it is assumed that all of the modes have their maximum response in the same direction at the same time, i.e., (2-39) 2-16 COSMOSM Advanced Modules

29 Part 1 ASTAR Advanced Dynamics Analysis Square Root Sum of Squares (SRSS) This is a more rational (and not necessarily conservative) approach where the modal responses are summed using the square root of sum of the squares. (2-40) In COSMOSM, the Absolute Sum method will only be used in conjunction with the SRSS technique if the modal frequency spacing is less than or equal to the cluster factor multiplied by the lowest frequency in the cluster. The cluster factor (clusf) is specified by the PD_ATYPE (Analysis > POST_DYNAMIC > P_Analysis Type command when defining Response Spectra Analysis options. Complete Quadratic Combination (CQC) The complete quadratic combination technique considers the effects of damping in combining the mode responses, i.e., (2-41) where ρ ij is the cross-mode correlation coefficient (2-42) and,, and ξ i, ξ j are modal damping coefficients for modes i and j. COSMOSM Advanced Modules 2-17

30 Chapter 2 Theoretical Background Naval Research Laboratory (NRL) The mode combination technique recommended by NRL takes the absolute value of the maximum response among all specified modes and adds it to the SRSS response of the remaining modes for each degree of freedom as noted below: (2-43) where {u j } represents the maximum response among responses of all nf modes. Multiple Response Spectra The structure response to multiple response spectra is found by the square root of the sum of the squares of the individual spectra responses. The output file lists the RMS values of relative displacements and velocities as well as the absolute accelerations. The accelerations at fixed nodes are not listed. Response Spectra Generation This dynamic analysis option allows the generation of response spectrum curves at any point of the structure for any displacement degree of freedom. The curve is generated for a single degree of freedom oscillator and represents the maximum response amplitudes as a function of oscillator frequency for a specified damping ratio. The excitation input required for this analysis is a curve defining accelerations versus time at the desired point of the structure. The program uses the results obtained from a modal time-history analysis to generate the spectrum curve at the specified node. Thus, a response spectra generation is possible only after a modal time history analysis is performed. The response spectrum generated can then be used as base excitation input for a response spectra analysis. This is particularly useful for studying the effect of structure s response on a secondary system attached to a point in the structure COSMOSM Advanced Modules

31 Part 1 ASTAR Advanced Dynamics Analysis In order to generate a response spectra for an available time-dependent curve, use the following procedure: 1. Model a single DOF oscillator (Figure 2-6), such as a truss element with a lumped mass attached to one node and the other node fixed, and perform a frequency analysis. 2. Subject the model to the base acceleration Ä(t) defined by the time-dependent curve (Figure 2-7) in a modal time-history analysis. 3. Use this analysis type (response spectrum generation) to generate a response spectrum curve (Figure 2-8) for the fixed node. Figure 2-6. Single DOF Oscillator C A m k.. A(t) Figure 2-7. Base Acceleration.. A(t) t t t COSMOSM Advanced Modules 2-19

32 Chapter 2 Theoretical Background Figure 2-8. Generated Response Spectrum Curve.. a max (ω) ω Random Vibration Analysis In COSMOSM, the random vibration analysis is available for linear elastic systems when subjected to a random excitation. The excitation is assumed to be stationary, Gaussian, with a mean value of zero, and one-sided (defined for positive frequencies only). The random excitation input required for this analysis consists of curves defining values of power spectral densities (PSD) versus frequencies, which can be associated with base motion, nodal forces, or element pressure. The curves frequencies as well as the lower and upper frequency limits are input in radians per second or in cycles per second, and the units of PSD functions will be interpreted accordingly. Thus, the PSD units are either (Force) 2 /freq, (disp) 2 /freq, (vel) 2 /freq, or (accel) 2 /freq. Also, the exciting power spectral densities of nodal forces can be specified as fully correlated, partially correlated, or fully uncorrelated. For the base motions, the power spectral density can be either fully correlated or fully uncorrelated. In the case of element pressure, the power spectral density can only be defined as fully correlated. Finally, this analysis outputs the root mean square (RMS) responses of displacements, velocities, accelerations, and stresses which for stationary, Gaussian excitation with mean value of zero, is equivalent to one standard deviation of response, i.e., the actual response can be assumed to be at or below this one standard deviation value about 68% of the time. The output of modal PSD's at selected frequencies is optionally available. Also, curves of power spectral density of response versus exciting frequencies at nodes (Q-plots) can be requested COSMOSM Advanced Modules

33 Part 1 ASTAR Advanced Dynamics Analysis Basic Definitions In the analysis of random vibration problems, the effects of such physical phenomena as the intensity of an earthquake or the noise from a jet engine, where the value of the variables describing the phenomena at some future time cannot be predicted, are considered. In view of the nondeterministic or random nature of these types of phenomena, it is necessary to abandon the explicit description of the applied excitations and their corresponding responses in terms of time and work with quantities that are based on certain averages. A few of the relevant average quantities used in the following discussions are described below: Autocorrelation Functions The autocorrelation function provides information concerning the dependence of the values of a random variable f(t) at different times on one another, given by the relation: (2-44) where (2-45) is known as the mean square value of the random variable which is equivalent to the maximum value of the autocorrelation function obtained at τ = 0. Power Spectral Density The power spectral density function defines properties of a random variable, similar to autocorrelation, in the frequency domain, i.e., (2-46) The autocorrelation function can, therefore, be expressed by the Inverse Fourier Transform of the power spectral density function: COSMOSM Advanced Modules 2-21

34 Chapter 2 Theoretical Background (2-47) The function S f (ω) has properties that render the evaluation of certain averages easier. Analysis Procedure The equations of motion for a linear dynamic system, Eq. (2-1), are: With certain restrictions on the form of the structure damping matrix [C], this system of equations was decoupled into nf modal equations as mentioned before. (2-48) for n=1, 2,..., nf, with: (2-49) and the vector of modal loads {r(t)} defined as: (2-50) Mean Square Response Considering that in the analysis of random vibration problems, the applied excitations are expressed by their power spectral density functions, a frequency domain solution is used. Therefore, if {f(t)} has the known PSD matrix [S f (ω)], then {r(t)}, as defined in Eq. (2-50), would have its PSD matrix defined as: (2-51) Now the PSD of the modal displacement response, [S x (ω)], can be obtained by, 2-22 COSMOSM Advanced Modules

35 Part 1 ASTAR Advanced Dynamics Analysis (2-52) where [H(ω)] is the modal transfer function matrix, and [H*(ω)] is its complex conjugate. For normal modes, the transfer function matrix is diagonal with diagonal elements H n (ω) (2-53) and (2-54) The structure displacement response PSD, [S u (ω)], can then be found from Eq. (2-49), i.e., (2-55) Similarly, the structure velocity and acceleration PSD responses can be written as: (2-56) (2-57) Now, the modal velocity PSD can be expressed in terms of the modal displacement PSD with individual matrix elements: (2-58) and hence, the structure velocity and acceleration response PSD's can be written as: (2-59) COSMOSM Advanced Modules 2-23

36 Chapter 2 Theoretical Background (2-60) Next, the zero delay modal autocorrelation responses for τ = 0 in terms of PSD of modal response (directly from Eq. 2-52) are: (2-61) (2-62) (2-63) and from these, the mean square responses are determined as the diagonal terms of the matrices: (2-64) (2-65) (2-66) Random Base Motion The equation of motion for a linear dynamic system with base motion v b (t) can be written: (2-67) (2-68) If the base motions have p.s.d. matrix [S b (ω)], then the p.s.d. of the equivalent vector is [S p (ω)] is: (2-69) 2-24 COSMOSM Advanced Modules

37 Part 1 ASTAR Advanced Dynamics Analysis Then the p.s.d. of the modal load is: (2-70) Once the p.s.d. of the modal loads S r (ω) has been calculated the analysis for the relative displacement response proceeds as for the random nodal load problem with the following considerations. a. In the case of Uniform Base Motion, {I b } contains 1 in the direction(s) of motion and 0 elsewhere (at all nodes). b. In the case of Multi-Base Motion, {I b } corresponds to the static displacement resulting from the static application of support displacements for each one of the support levels. Stress Mean Square Response The element stresses {σ} are determined from the nodal displacements {u e } of the element, or in terms of modal displacements, (2-71a) (2-71) where [Φ e ] are the eigenvectors corresponding to the nodal displacements {u e }. The stress response correlation matrix, [R σ ] for each element is written as: (2-71b) (2-72) Methods of Integration Two methods of integration are available. One is the so called standard method and the second is the approximate method, as briefly discussed below: COSMOSM Advanced Modules 2-25

38 Chapter 2 Theoretical Background Standard Method The standard integration method performs a classical random vibration analysis. This method proceeds in the following steps: 1. Certain frequency points are selected around each natural mode as requested. Locations of these points are based on the value of biasing parameters which is input. A biasing value of one results in points uniformly distributed between the natural frequencies; while a value greater than one helps to bias point locations toward natural frequencies. The default values for these parameters are given in Table 2-1, below, as a function of the modal damping ratio ξ at the first mode. 2. Modal PSD s of response are evaluated at each of the selected frequency points. The cross-mode cut-off ratio (RATIO) defines a limit on the ratio of each two natural frequencies (ω i / ω j, i > j). This means for each two modes with ω i / ω j > RATIO, the cross-spectral density terms are neglected. Cross-mode effects are not considered if RATIO = l. 3. The modal PSD s are then numerically integrated over the specified frequency range to yield the mean squared values and covariances of the modal response. The integration is carried out numerically using Gauss integration of orders two or three over each frequency interval, based on a log-log relation. The mean squared response is obtained by summing the interval contributions. 4. Finally, transformation from modal to nodal yields the RMS displacements, velocities, and accelerations of the system. Table 2-1. Default Values for Parameters num_freq_points and Bias as a Function of ξ Modal Damping Ratio Default for num_freq_points Default for Bias ξ < < ξ < ln (ξ / 0.01) ln (ξ / 0.01) ξ > Approximate Method The standard random vibration analysis can be computationally expensive due to the numerical integration of matrices. The approximate integration method performs a simplified solution by considering the following assumptions: 2-26 COSMOSM Advanced Modules

39 Part 1 ASTAR Advanced Dynamics Analysis Neglecting the cross-mode response, S x (ω), that is the effect of one mode on another, i.e., Forcing PSD's are considered constant around each normal mode. Thus, each mode is assumed to be excited by white noise with power spectral density S n, where (2-73) (2-74) and ω n is the natural frequency of mode n = 1,2,...,nf. For white noise, the mean square response can be determined analytically for the modal response and they are: (2-75) (2-76) (2-77) By combining the two assumptions, the structure mean square responses can be found. Partial (Spatial) Correlation The excitation between two nodes could be fully correlated, fully uncorrelated or partially correlated. In COSMOSM, the partial correlation is based on the spatial distance between two nodes. If the partial (spatial) correlation is used depending on the distance between the two nodes (i) and (j) (R ij ), one of the following three situations will prevail: a. If the distance R ij is smaller than a user defined R MIN, then the two nodes are considered fully correlated. b. If the distance R ij is larger than a user defined R MAX, then the two nodes are considered fully uncorrelated. c. If the distance R ij is between R MIN and R MAX, then the excitation is partially correlated and the degree of correlation is linearly proportional to the COSMOSM Advanced Modules 2-27

40 Chapter 2 Theoretical Background distance. The above conditions can be illustrated in the following figure where nodes 1 and 2 are fully correlated, nodes 1 and 3 are partially correlated, and nodes 1 and 4 are fully uncorrelated. Figure 2-9. Sphere of Influence for the Degree of Correlation α i j Node 3 1 Node 4 Node 2 R MIN Node 1 Distance (R ) i j R MAX The effect of the distance on the cross-correlation terms (off-diagonal terms) of the part of the PSD matrix related to the two nodes (i) and (j) and a single degree of freedom k can be written as: (2-78) where: Currently, partial correlation is only available for force excitations COSMOSM Advanced Modules

41 Part 1 ASTAR Advanced Dynamics Analysis Steady State Harmonic Analysis The steady state harmonic analysis evaluates the maximum structural response due to harmonic excitations of varying magnitudes and varying frequencies. Maximum nodal response is evaluated at different exciting frequencies in the range specified. The excitation input required for this analysis consists of curves defining amplitudes versus frequencies of a harmonic forcing function, which can be associated with nodal forces, element pressures, or base motion. Also, a phase angle can be defined for each base motion curve or nodal force. Note that element pressures are currently associated with zero phase angles. The input curve s frequencies as well as the lower and upper frequency limits can be specified either in radians per second or cycles per second. Curves of maximum nodal response magnitude versus exciting frequencies (Q-plots) may be requested for any node in the structure. Analysis Procedure The frequency response analysis of the structure is determined by using the normal mode method. Let the nodal force vector {P} be harmonic and defined as: (2-79) or, (2-80) where P k is the magnitude of the force in the k th degree of freedom direction, ω is the exciting frequency, and γ k is the phase angle of the force. Considering that for linear systems, the structure equations of motion are decoupled into nf modal equations, (2-81) the substitution of the force vector {P} into Eq. (2-81) will give: COSMOSM Advanced Modules 2-29

42 Chapter 2 Theoretical Background (2-82) where: The steady state solution to Eq. (2-82) is: (2-83) Taking the real part of Eq. (2-83) will result in, (2-84) where 2-30 COSMOSM Advanced Modules

43 Part 1 ASTAR Advanced Dynamics Analysis Now the structure displacement, u, is given by: or (2-85) The magnitude of the structure displacement and its corresponding phase angle for the k th degree of freedom are: (2-86) (2-87) The structure velocity and acceleration response can be found by taking the derivatives of Eq. (2-85). The amplitude of the structure velocity and acceleration are: (2-88) (2-89) where the velocity and the acceleration are 90 and 180 advanced from the displacement in terms of their phase angles, respectively. COSMOSM Advanced Modules 2-31

44 Chapter 2 Theoretical Background Direct Spectrum Generation This analysis evaluates different types of spectra curves for a given frequency range when a time history curve is used as input. For this analysis there is no need to perform frequency analysis. The following spectrums are calculated and can be viewed both in output and in terms of Q-plots. Pseudo acceleration Pseudo velocity Relative displacement Relative velocity Absolute acceleration The direct spectrum generation analysis is based on the central difference time integration procedure where the maximum response of a Single Degree of Freedom system for different frequencies is calculated. This analysis is more accurate, more time consuming and has shorter input than the Response Spectra Generation analysis noted earlier. Finally, this direct generation approach is highly recommended in cases where random time history excitation records (i.e., earthquake) are used as input. The input time history must be defined as an acceleration base excitation curve. The results are written also in a form which can be used as input curves to other problems (see PD_ATYPE command notes in the Command Reference Manual). Time History Generation The objective of this analysis is to generate time history records from the user defined acceleration response spectra curve. For this analysis there is no need to perform frequency analysis. The method is based on the use of summation of a series of sine terms with selected amplitudes and frequencies. The spacing of the frequencies is chosen in such a manner that the half power points of response spectra due to a single frequency input will overlap. In order to obtain time histories that resemble the proper excitation record (i.e., earthquake at a given site), a modulating profile is introduced which has the shape of a given time dependent excitation record (i.e., trapezoidal, box or El-Centro N-S earthquake record). Also, the peak value of acceleration in the time history record can be limited to a specified amount defined for a particular site COSMOSM Advanced Modules

45 Part 1 ASTAR Advanced Dynamics Analysis A maximum of two time histories with relatively low correlation between them can be generated. To develop the second time history, a method based on shifting the frequencies of the first record to the adjoining midfrequencies is used. Also, the Base Line Correction method is used in order to modify the generated time histories such that the final velocity and displacement will be equal to zero. The method used in the Time History Generation analysis is an iterative procedure where the values of the spectra and generated time history curves can be printed at the user specified print intervals, however, plot is available only for the last step). This iterative algorithm will be terminated either at the time where the calculated spectrum converges to the target spectrum, within the user specified tolerance, or when the iteration number is equal to the maximum permitted number of iterations. In case of convergence, the results will be given both in the output and also in terms of Q-plots (spectrum and corresponding time-history curves). It should be noted that once the iterative procedure is used to develop the first time history, the second record and corrected curves will be generated at the final iteration number. The input target spectrum curve must be defined as frequency dependent acceleration base excitation curve, where the unit of frequency must be in Hertz. The profile or envelope curve should also be defined as a time dependent acceleration base excitation curve. The program will assume the El-Centro earthquake envelope if the default value of zero is taken as the profile curve label. The results are written also in a form which can be used as input to other problems (see PD_ATYPE command notes in the Command Reference Manual.) References 1. Clough, R. W. and Penzien, J., Dynamics of Structures, McGraw-Hill Book Company, New York, Cook, R. D., Malkus, D. S. and Plesha, M. E., Concepts and Applications of Finite Element Analysis, Third Edition, John Wiley & Sons, Inc., Fung, Y. C., Foundations of Solid Mechanics, Prentice-Hall, Inc., Englewood Cliffs, Zienkiewicz, O. C., The Finite Element Method, McGraw-Hill Book Company, New York, COSMOSM Advanced Modules 2-33

46 Chapter 2 Theoretical Background 5. Meirovitch, L., Elements of Vibration Analysis, McGraw-Hill Book Company, New York, Bathe, K.J., Wilson, E. L., Numerical Methods in Finite Element Analysis, Prentice Hall, Englewood Cliffs, Numar, J. L., Dynamics of Structures, Prentice-Hall, Inc., Englewood Cliffs, COSMOSM Advanced Modules

47 3 Description of Elements Introduction The entire set of structural elements furnished in the COSMOSM element library can be used in conjunction with the Advanced Dynamic Analysis module. The table below provides a complete list of the available elements. For detailed descriptions of each element, you are referred to Chapter 4 of the COSMOSM User Guide Manual. COSMOSM Advanced Modules 3-1

48 Chapter 3 Description of Elements Table 3-1. Elements for Linear Structural Dynamics Analysis (STAR, DSTAR and ASTAR) Element Type Element Name 2D Spar/Truss TRUSS2D 2D Elastic Beam BEAM2D 3D Elastic Beam BEAM3D 3D Spar/Truss TRUSS3D 2D 4- to 8-node Plane Stress, Strain, Body of Revolution PLANE2D 3D 3- to 6-node Plane Stress, Strain, Body of Revolution TRIANG Triangular Thin Shell SHELL3 6-Node Triangular Thin Shell SHELL6 Quadrilateral Thin Shell SHELL4 Triangular Thick Shell SHELL3T Quadrilateral Thick Shell SHELL4T 6-Node Triangular Thick Shell SHELL6T Triangular Composite Shell SHELL3L Quadrilateral Composite Shell SH3LL4L 8 or 9-node Isoparametric Shell Element SHELL9 8 or 9-node Isoparametric Composite Shell SHELL9L Axisymmetric Shell SHELLAX 3D 8- to 20-node Continuum Brick SOLID 8-node Composite Solid SOLIDL 3D 4-node Tetrahedron Solid TETRA4 3D 4-node Tetrahedron Solid with Rotation TETRA4R 3D 10-node Tetrahedron Solid TETRA10 Spring Element SPRING General Stiffness GENSTIF 2-node Rigid Bar RBAR Elastic Straight Pipe PIPE Boundary Element BOUND General Mass Element MASS Elastic Curved Pipe ELBOW 3D 8- to 20-Node Isoparametric Piezoelectric Solid SOLIDPZ 2-Node Gap with Friction GAP 3-2 COSMOSM Advanced Modules

49 Part 1 ASTAR Advanced Dynamics Analysis COSMOSM Advanced Modules 3-3

50 4 Brief Description of Commands Introduction The commands grouped together in the menu for Post Dynamic analysis provide the options required to set up and run Post Dynamic analysis problems following frequency and mode shape calculations. The steps required to generate various results and system response quantities are also briefly discussed. Detailed description of all commands associated with Post Dynamic analysis is given in the COSMOSM Command Reference Manual. Main POST_DYN Menu The commands of this menu provide general guidelines on the various analyses options available according to the following: POST_DYN PD_ATYPE PD_ALIST R_DYNAIMC PD_PREPARE PD_DAMP/GAP PD_CURVES PD_BEXCIT PD_OUTPUT COSMOSM Advanced Modules 4-1

51 Chapter 4 Brief Description of Commands Command (Path) PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) PD_ALIST (Analysis > POST_DYNAMIC > List PD Analysis Options) Command (Path) R_DYNAMIC (Analysis > POST_DYNAMIC > Run Post Dynamic) PD_PREPARE (Analysis > POST_DYNAMIC > Prepare PD Plot) PD DAMP/GAP (Analysis > POST_DYNAMIC >) PD CURVES (Analysis > POST_DYNAMIC >) PD BASE EXCITATION (Analysis > POST_DYNAMIC >) PD OUTPUT (Analysis > POST_DYNAMIC >) Intended Use Specifies the analysis type and related inputs. Lists the assignments made by PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type). Runs dynamic analysis. Intended Use Makes preparation for extreme/relative response calculations. Submenu related to management of damping and gap elements. Submenu related to the excitation curves. Submenu related exclusively to base excitation. Submenu, specifying options generating output and plot files. A more detailed description of each submenu is provided in the following: PD DAMP/GAP Submenu The Rayleigh, modal and composite damping coefficients specified by the first three commands can be used in conjunction with all the post-dynamic analysis options available. The concentrated damper and gap elements, however, are applicable only in the case of modal time history problems. PD_DAMP/GAP PD_RDAMP PD_MDAMP PD_DAMPREAD PD_DAMPLIST PD_CDAMP PD_CDDEL PD_CDLIST PD_GAP 4-2 COSMOSM Advanced Modules

52 Part 1 ASTAR Advanced Dynamics Analysis Concentrated Damper Element Damper elements can be considered between any two nodes or any one node and the ground as shown in Figure 4-1. The damping coefficient is defined in terms of its components along the global X-, Y-, and Z-directions. The commands in this submenu define, list and delete concentrated dampers (damper elements). Figure 4-1. Concentrated Damper Element Between Two Nodes Node_1 Y DY Z X Node_2 Gap-Friction Element The Gap-Friction element is defined by two nodes representing the distance between any two points in a two- or three-dimensional model. The actual gap separation is defined independent of the node locations and can assume any value including the distance between the nodes. The element resists either compression or tension depending on whether the gap distance is positive or negative (see Chapter 2 for more details). PD CURVES Submenu The commands assembled in this menu are used exclusively for defining, modifying, deleting, or listing different curve types used in conjunction with the analysis options of the Post Dynamic module. Each curve can be defined by at least two and at most 5,000 points. In addition, if a curve is harmonic time dependent, it can be specified by its amplitude and frequency instead of curve points. PD_CURVES PD_CURTYPE PD_CURDEF PD_CURDEL PD_CURLIST Note that at least one curve is usually required for any of the dynamic analyses types, and up to 100 different curves can be defined. COSMOSM Advanced Modules 4-3

53 Chapter 4 Brief Description of Commands The time or frequency curves should be activated prior to defining nodal forces, element pressures, or base excitations. The dynamic loads imposed to the system are then defined by the product of the applied loads and the corresponding curve values at each time or frequency step. The command used for the activation of both time and frequency curves is the ACTSET (Control > ACTIVATE > Set Entity) command. PD BASE EXCITATION Submenu The commands of this submenu define parameters related to uniform base motion and multiple support excitations. In the case of multiple support excitations, the following conditions can be considered: PD_BEXCIT PD_BASEFAC PD_BSLIST PD_SPPRT PD_SPPRTLIST PD_SPPRTDEL May define up to 100 support levels (a support level consists of nodes which move in the same direction with the same amplitude). May consider up to 100 excitation curves. May use both multi-base motion and uniform motion at the same time. Is available for all Post Dynamic analysis options. PD OUTPUT Submenu The PD_OUTPUT (Analysis > POST_DYNAMIC) submenu provides an extensive array of commands for the automatic generation of plot files representing time-history response of various result quantities, deformed shape and stress contour plots, and other related postprocessing information. These files can be formed for any desired time or frequency step within the defined range and for any element and direction in the specified model. Printing of results in the ASCII output file can also be controlled. All plot units will correspond to units used in defining the in-put excitations. The response plots can be obtained in terms of either absolute or relative displacements and velocities, and absolute accelerations only. PD_OUTPUT PD_PRINT PD_PLOT PD_NRESP PD_PLTINT PD_RELRESP PD_SXYSET PD_PLTLIST PD_MAXMIN PD_MAXLIST Commands PD_PRINT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Print Options), PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options), and PD_NRESP (Analysis > POST_DYNAMIC > PD OUTPUT > Set Response Options) must be given prior to the R_DYNAMIC (Analysis > POST_ 4-4 COSMOSM Advanced Modules

54 Part 1 ASTAR Advanced Dynamics Analysis DYNAMIC > Run Post Dynamic) command for the program to write the requested print and plot information. These commands are in general required if detailed postprocessing results are to be generated for graphical evaluations. The PD_SXYSET (Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph) command should be issued before executing the stress module to generate a file that stores stress components for specified elements as a function of time or frequency. The PD_PLTINT (Analysis > POST_DYNAMIC > PD OUTPUT > Specify Interval) command can be used both before or after R_DYNAMIC (Analysis > POST_ DYNAMIC > Run Post Dynamic) and R_STRESS (Analysis > STATIC > Run Stress Analysis) commands. To obtain information on the relative response between any two nodes (or a node and the base), first you are required to submit the PD_RELRESP (Analysis > POST_DYNAMIC > PD OUTPUT > Relative Response) command and then the PD_PREPARE (Analysis > POST_DYNAMIC > Prepare PD Plot) which will result in the computation of the relative response values and their writing in the output file. Finally the combination of PD_MAXMIN (Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Response) and PD_PREPARE (Analysis > POST_DYNAMIC > Prepare PD Plot) commands will initiate the search for nodes with highest response values among a set of nodes and within a given time (or frequency) domain and will list the peak responses for the specified number of nodes. Other GEOSTAR commands such as PRINT_NDSET (Analysis > OUTPUT OPTIONS > Set Nodal Range) and PRINT_ELSET (Analysis > OUTPUT OPTIONS > Set Element Range) can be used if the printout of displacements, velocities, accelerations [using PRINT_NDSET (Analysis > OUTPUT OPTIONS > Set Nodal Range)] and stresses [using PRINT_ELSET (Analysis > OUTPUT OPTIONS > Set Element Range)] is desired for limited number of nodes and/or elements. Postprocessing of Dynamic Results Postprocessing of the system response to the different dynamic loading conditions of this module can be performed with commands provided in the various submenus of the RESULT menu. Graphical depiction or numerical listing of the time or frequency dependent responses can readily be obtained for any part of the structure or for any time or frequency step. COSMOSM Advanced Modules 4-5

55 Chapter 4 Brief Description of Commands Several detailed examples involving the thorough coverage of the pre- and postprocessing features available for Post Dynamic analysis are presented in the next chapter. XY-Plot of Response Graphs of system response (displacement, velocity, and acceleration) versus time or frequency may be requested at specified nodes. The XY-plots available for various types of analyses options are listed below: Time History Harmonic Analysis Random Vibration Response Spectra Generation Response Spectra Analysis Plots of system response versus time. Plots of amplitude and phase of system response versus frequency. Plots of PSD of response versus frequency. Plot of the spectra versus frequency. Not applicable. For all the above analyses except for Spectra Generation, you need to specify the nodes at which XY-plots are required using the following commands: Command (Path) PD_NRESP (Analysis > POST_ DYNAMIC > PD OUTPUT > Set Response Options) PD_PLTINT (Analysis > POST_DYNAMIC > PD OUTPUT > Specify Interval) To select nodes. Intended Use To specify the range and step interval (otherwise (optional) the entire range will be considered) The first command must be used prior to running the analysis. However, the second command can be used both before and after the R_DYNAMIC (Analysis > POST_DYNAMIC > Run Post Dynamic) command. If it is used before, it limits the information in data base for plot to those steps requested, whereas, using it after, limits the display only to the requested steps and range. For Response Spectra Generation the node and range assignments are made by using the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command. To plot the response use the commands in the XY_PLOTS submenu available under the DISPLAY menu. Use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List 4-6 COSMOSM Advanced Modules

56 Part 1 ASTAR Advanced Dynamics Analysis Plot Info) command to list all requested outputs including the XY-plots. For the proper application of these options, please refer to the examples in Chapter 5. Plot of Response Contour plots representing the response of the structure (displacement, velocity, and acceleration) at specified time or frequency steps are available for: Time History Harmonic Analysis Random Vibration Response Spectra Analysis Plot of response at specified time steps. Plot of the amplitude and phase at specified frequency steps. Plot of the PSD of response at specified frequency steps and the RMS of response. Plot of the maximum response. For random vibration the N requested PSD steps are saved at the first N steps of plot file and at the step N+1 the RMS of response is saved as default. For response spectra analysis, the maximum response is always saved at step number one. Use the PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options) command to specify the desired steps prior to executing the dynamic program. To display the results choose the ACTDIS (Results > PLOT > Displacement) command to activate a solution step and then choose DISPLOT (Results > PLOT > Displacement) command to display the response, or use DEFPLOT (Results > PLOT > Deformed Shape) of the same submenu to plot the deformed shape. Use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) command to list all requested outputs including the requested plots. The RESULTS (Results > Available Result) command also lists available steps in the plot file. For the proper application of these options, please refer to the examples in Chapter 5. XY-Plot of Stresses Stresses can be plotted versus time or frequency for the specified elements. This option is available for: Time History Harmonic Analysis Random Vibration Plot of the stress components versus time. Plot of the stress component amplitude versus frequency. Plot of the PSD stress components versus frequency. COSMOSM Advanced Modules 4-7

57 Chapter 4 Brief Description of Commands Response Spectra Analysis Response Spectra Generation Not applicable. Not available. For all the above analyses options you need to use the following two commands prior to running the stress module: Command (Path) PD_SXYSET (Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph) PD_PLTINT (optional) (Analysis > POST_DYNAMIC > PD OUTPUT > Specify Interval) Intended Use Specify element number and stress component. Specify the range and step interval (otherwise the entire range will be considered). For one-dimensional elements such as beams, trusses, pipes, elbows, and springs, the internal forces are plotted instead of stresses. To display XY-plots use XY_PLOT submenu of DISPLAY menu to activate postprocessing for Post Dynamic then the following set of commands may be issued: Command (Path) INITXYPLOT Display > XY PLOTS > Initialize) ACTXYPOST (Display > XY PLOTS > Activate Post-Proc) XYPLOT (Display > XY PLOTS > Plot Curves) Other commands (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) Intended Use To initialize the XY-plot buffer. To activate the desired components. To generate the plot. To setup the graph, specify the range, etc., are also available. Use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) command to list all requested outputs including the XY-plots. For the proper application of these options, please refer to the detailed examples described in Chapter COSMOSM Advanced Modules

58 Part 1 ASTAR Advanced Dynamics Analysis Plot of Stresses Contour plot of stresses are available at specified time or frequency steps. This option is available for: Time History Harmonic Analysis Random Vibration Response Spectra Analysis Plot of the stress components at specified time steps. Plot of stress component amplitude at specified frequency steps. Plot of the PSD of stress components at specified frequency steps and the RMS of stresses. Plot of the maximum stress components. For random vibration the N requested PSD of the stress components are saved at the first N steps of the stress file (provided that the appropriate option in the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command is activated) and at the step N+1 the RMS value of the stress component is saved by default. For the Response Spectra Analysis, the maximum response is saved at step one (provided that the appropriate options in PD_ATYPE (Analysis > POST_ DYNAMIC > Sel PD Analysis Type) command is activated). Use PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options) command to specify the desired steps prior to executing the stress program. To display the stresses use the ACTSTR (Results > PLOT > Stress) command to specify the step number and the desired stress component, then use the STRPLOT (Results > PLOT > Stress) command to display the stress. Use the PD_PLTLIST (Analysis > POST_ DYNAMIC > PD OUTPUT > List Plot Info) command to list all requested outputs including the stress plots. For the proper application of these options, please refer to the detailed example in Chapter 5. Other Postprocessing Options GEOSTAR provides additional postprocessing tools for the better comprehension of results, such as: 1. Plot Animation: The response (displacement, velocity, and acceleration) as well as stresses can be animated in time or frequency domain using this option. After you plot for certain step, use ANIMATE (Results > PLOT > Animate) command to animate within a desired range. COSMOSM Advanced Modules 4-9

59 Chapter 4 Brief Description of Commands 2. Section Animation: You may use LSECPLOT (Results > PLOT > Path Graph) and ANIMATE (Results > PLOT > Animate) to animate the results along a specified section. 3. Extreme Values of Results: You may use the EXTREMES menu to find the maximum response (or the maximum stress) at a desired solution step or across all solution steps. 4. Sorting Nodes with Maximum Response: Using the commands PD_MAXMIN (Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Response), PD_PREPARE (Analysis > POST_DYNAMIC > Prepare PD Plot) and PD_MAXLIS (Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Value), the user can request a list of nodes with highest responses within a range of time or frequency. 5. Response of a Node Relative to Another Node: Using commands PD_RELRES (Analysis > POST_DYNAMIC > PD OUTPUT > Relative Response) and PD_PREPARE (Analysis > POST_DYNAMIC > Prepare PD Plot) the user may request the calculation of relative responses between two nodes or one node relative to the base. The results will be written in the output file. Since most of these analyses generate RMS or ABS types of responses, therefore the relative response calculations are carried at the mode level where the modal displacements are first calculated. 6. Combining Responses: Combining the static response (displacement and stresses) with dynamic response of a specified time or frequency step. Options 4 and 5 are only available for responses, (displacement, velocities, and acceleration, they are not available for stresses). For the proper application of these options, please refer to the example in Chapter 5. Post Dynamic Input Procedure The input commands for Post Dynamic module may either be given directly from the terminal (interactively) or read from a file (in a batch mode) with the use of FILE (File > Load...) command. In the following a typical input procedure is discussed COSMOSM Advanced Modules

60 Part 1 ASTAR Advanced Dynamics Analysis Typical Input Procedure In general, a specific command sequence is not required for setting up a dynamic response problem for the ASTAR module. However, some logic should be observed in the order in which commands are issued to prepare the problem input. The following instructions are applicable to all solution options available through GEOSTAR. Note that this is only a suggested order which does not have to be strictly followed. Before using the ASTAR module, the finite element model must have been developed in GEOSTAR and processed for frequency analysis to store modes and frequencies essential to the normal mode method (except for curve transformation problems). 1. From the ANALYSIS-POST_DYNAMIC menu tree, select the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command to specify the type of Post Dynamic analysis option, the number of modes to be used, and other relevant solution parameters. 2. The program provides complete freedom in the selection of the response information for printing or plotting. Commands like PD_PRINT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Print Options), PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options) and others from the PD OUTPUT submenu that control printing and plotting of output results, can be issued for this purpose. 3. The time or frequency-dependent load functions associated with the analysis type under consideration are subsequently defined in conjunction with base motion commands, nodal force or element pressure multipliers to define excitation for the analysis using the PD_CURTYP (Analysis > POST_DYNAMIC > PD CURVES > Curve Type) and PD_CURDEF (Analysis > POST_DYNAMIC > PD CURVES > Define) commands. The data can be specified interactively or may be read from an external file. 4. Next, using the PD_RDAMP (Analysis > POST_DYNAMIC > PD DAMP/GAP > Rayleigh Damp) or PD_MDAMP (Analysis > POST_DYNAMIC > PD DAMP/GAP > Modal Damp) commands, Rayleigh or Modal damping coefficients may be defined before issuing the R_DYNAMIC (Analysis > POST_DYNAMIC > Run Post Dynamic) command to perform the postdynamic analysis. Also, damping coefficients due to material (composite) COSMOSM Advanced Modules 4-11

61 Chapter 4 Brief Description of Commands damping can be read into modal damping locations using the PD_DAMPREAD (Analysis > POST_DYNAMIC > PD DAMP/GAP > Read Material Damp) command if damping is specified as a material property prior to frequency calculation. 5. With ASTAR analysis performed, the requested output results can be graphically animated. The deformed shapes or nodal response graphs can be plotted for the specified solution steps and nodes. 6. The corresponding dynamic stresses can then be computed by issuing the R_STRESS (Analysis > STATIC > Run Stress Analysis) command. Prior to that PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options) and PD_SXYSET (Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph) commands should be used to specify the time steps for stress contour plots and the elements for which stresses are to be stored as a function of time or frequency for stress plots. 7. Finally the PD_PREPARE (Analysis > POST_DYNAMIC > Prepare PD Plot) command will provide the option to obtain relative response information as well as extreme nodal response. This command must be used in conjunction with the PD_RELRESP (Analysis > POST_DYNAMIC > PD OUTPUT > Relative Response) and PD_MAXMIN (Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Response) commands to assign the nodes and other relevant parameters. The detailed examples described in Chapter 5 will provide step-by-step instructions on the application of the ASTAR module to the solution of various dynamic response problems. For curve transformation problems, please review the verification problems D13, D14 and D15 for the typical inputs as well as the notes corresponding to the command description of PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) for the postprocessing of these options COSMOSM Advanced Modules

62 5 Detailed Description of Examples Introduction This section covers several examples illustrating the Advanced Dynamic analysis capabilities. Dynamic Analysis of a Cantilever Beam Analysis Types Modal Time History Analysis Random Vibration Analysis Statement of the Problem Determine the response of a cantilever beam subjected to: A time varying concentrated load in the Y-direction at the free end (Figure 5-1). Ground acceleration in the Y-direction, defined by its power spectral density (Figure 5-2). COSMOSM Advanced Modules 5-1

63 Chapter 5 Detailed Description of Examples Figure 5-1. Problem with Time Varying Load Node 22 is at the tip of the cantilever Value 10,000 Time Curve Time Figure 5-2. Ground Acceleration P.S.D. 1.g 2 White Noise Frequency Given E = 30 x 10 6 psi g = in/sec 2 h = 1 in Thickness = 1 in L = 10 in DENS = lb sec 2 /in 4 Modal damping coefficient= COSMOSM Advanced Modules

64 Part 1 ASTAR Advanced Dynamics Analysis Frequency Analysis of the Problem 1. The advanced dynamic analysis of the COSMOSM program is based on the normal mode method. Therefore, it is essential that the frequency and mode shape calculations are done prior to the application of the Advanced Dynamic Module. By issuing the following set of commands, the fundamental frequencies and mode shapes are evaluated: Geo Panel: Propsets > Element Group (EGROUP) EGROUP,, PLANE2D; Geo Panel: Propsets > Real Constant (RCONST) RCONST,,,,,1; (thickness is 1.0) Geo Panel: Propsets > Material Property (MPROP) MPROP,,EX,30E6,DENS, 7.3e-4; rconstgeo Panel:Geometry > SURFACES > Draw w/4 Coord (SF4CORD) SF4CORD,,0,0,0,0,1,0,10,1,0,10,0,0 Use AUTO scale icon SCALE,0, Geo Panel: Control > ACTIVATE > Entity Label (ACTNUM) ACTNUM,ND,1, Geo Panel: Meshing > PARAMETRIC MESH > Surfaces (M_SF) M_SF,,,,,1,10; Geo Panel: LoadsBC > STRUCTURAL > DISPLACEMENT > Define Nodes (DND) DND,1,UX,,2; DND,1,UY; Geo Panel: Analysis > FREQUENCY/BUCKLING > Frequency Options (A_FREQUENCY) A_FREQUENCY,10,S; Geo Panel: Analysis > FREQUENCY/BUCKLING > Run Frequency (R_FREQUENCY) R_FREQUENCY Using the calculated frequencies and mode shapes, we are ready to apply the Advanced Dynamic Module in order to find the response of the beam to the two aforementioned types of loading in the following parts: COSMOSM Advanced Modules 5-3

65 Chapter 5 Detailed Description of Examples If you intend to solve the problem for several different types of dynamic analysis, it is recommended that you save the data base of the frequency part of the problem in another file to avoid running that again. Modal Time History This part is divided into three steps. In Step 1, the response (displacement, velocity and acceleration) is evaluated. In Step 2, the postprocessing of the response is explained in detail. In Step 3, stress evaluations and subsequent postprocessing are discussed. Evaluation of Response 1. In this step, the response (displacement, velocity or acceleration) can be evaluated at different time steps. For all post dynamic analyses, the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command should be issued first, so that subsequent commands are prompted properly. Therefore, to start, define the type of analysis by issuing the command: Geo Panel: Analysis > POST_DYNAMIC > Sel PD Analysis Type (PD_ATYPE) Post dynamic type > 2:Modal time history analysis Click Continue No. of frequency > 10 Use 10 modes (all available modes. In general, you can use less modes) No. of time steps in the solution > 50 Starting time [0] > Time step size [0.1]> Time integration method > Newmark method First integration parameter > 0.5 Correspond to delta parameter of Newmark method Second Integration Parameter > 0.25 Correspond to theta, parameter of Newmark method Type of response print out > Rel displ and rel vel Load case for initial conditions > 0 No static displacement is considered as initial conditions Dead load step > COSMOSM Advanced Modules

66 Part 1 ASTAR Advanced Dynamics Analysis No static results will be added to dynamic response Dead load multi-factor > 1 Click OK 2. You may use the PD_ALIST (Analysis > POST_DYNAMIC > List PD Analysis Options) command to review your inputs or reissue the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command to modify them. Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Print Options (PD_PRINT) Displacement print flag > On Velocity print flag > Off Acceleration print flag > Off Phase Angle print flag > Off Missing mass correction flag > Off Response print interval > 1 Beginning step for stress print > 1 Print stresses at all steps Ending step for stress print > 50 Increment > 1 Click OK In the above command the prompt for Missing Mass Correction)" is not effective for this analysis. It is only applicable to the Response Spectra Analysis. 3. The type of curve to be used in the time history analysis is defined by the following command: Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Curve Type (PD_CURTYP) Curve label > 1 Click Continue Type of curve > Time Excitation type > Force/pressure Click OK 4. The curve defining the time variation pattern of the load is defined by the following command. The defined function is used as a multiplier to the associated loading. Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Define Curve Label > 1 Starting point number > 1 COSMOSM Advanced Modules 5-5

67 Chapter 5 Detailed Description of Examples Time at point 1 > 0 Define three points on the curve according to the force diagram Curve value at point 1 > 0 Time at point 2 >.1 Curve value at point 2 > Time at point 3 > 1 Curve value at point 3 > Terminate the command 5. To modify any point, reissue the command with the Starting Point Number" same as the desired point. To review your input, use PD_CURLIST (Analysis > POST_DYNAMIC > PD CURVES > List). To define forces related to curve 1, issue the following two commands: Geo Panel: Control > ACTIVATE > Set Entity (ACTSET) Set label> TC: Time curve Click Continue Time Curve > 1 Click OK Geo Panel: LoadsBC > STRUCTURAL > FORCE > Define by Nodes (FND) Beginning node > 22 Force label > FY Value >0.1 (associated with time curve 1, max. force = 1000) Endind node > 22 Increment > 1 Click OK Plotting Assignments 1. You must specify the time steps for which you are interested to have response plot (for displacement, velocity, and acceleration) or response animation by issuing the following command. Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options (PD_PLOT) Set 1 beginning step > 1 Set 1 ending step > 40 Set 1 step increment > 1 Click OK 5-6 COSMOSM Advanced Modules

68 Part 1 ASTAR Advanced Dynamics Analysis Use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) to list the requested plots. 2. You could specify the nodes for which you need XY-plots (response versus time). The PD_PLTINT (Analysis > POST_DYNAMIC > PD OUTPUT > Specify Interval) command may be used to specify the range and increment of solution steps for XY-plotting, otherwise the whole range will be considered. Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Response Options (PD_NRESP) Starting location > 1 Node 1 > 22 Node 2 > 10 Click OK You may specify up to 50 nodes by issuing the above command. Use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) to list the requested XY-plots. 3. Now you may run the problem by issuing the following command: Geo Panel: Analysis > POST_DYNAMIC > Run Post Dynamic (R_DYNAMIC) Perform Time History analysis Other Applications Applying Initial Conditions: In some problems you may need to assign initial conditions for displacement, velocity or acceleration at particular nodes. This can be accomplished in GEOSTAR by using the INITIAL (LoadsBC > LOAD OPTIONS > Initial Condition) command or you may use the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command to assign the displacement results of certain static program load case as initial displacement condition. Applying Base Motion: If you wish to consider base motion, instead of applied loads, then you should input 1 instead of 0 for uniform base motion) for the third prompt of the PD_CURTYP (Analysis > POST_DYNAMIC > PD CURVES > Curve Type) command as well as replacing the above defined nodal forces with the base motion using the PD_BASE (Analysis > POST_ DYNAMIC > PD BASE EXCITATION > Base Excitation) command. (Additionally, you have to use the PD_SPPRT (Analysis > POST_DYNAMIC > PD BASE EXCITATION > Support Level) command for multi-base motion.) COSMOSM Advanced Modules 5-7

69 Chapter 5 Detailed Description of Examples You may review the results by looking at the output file (with extension.out) or using the GEOSTAR graphic capabilities to have response versus time plots or deformation plots at designated time steps. You may have both force excitation and base excitation on the same model. Postprocessing of the Response XY-Plot of Response 1. Activate the XY-plotting for displacements: Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) Graph number [1] > X-variable > Time Y-variable > UX Node number > 22 Graph color > 12 Graph line style > Solid Graph symbol style > 1 Graph id > 22X Click OK 2. Similarly activate graph number 2 for node 22 along the Y-direction (set id to 22Y) 3. Use the XYPLOT (Display > XY PLOTS > Plot Curves) command to plot the graphs: Geo Panel: Display > XY PLOTS > Plot Curves (XYPLOT) Plot graph > 1: Yes Plot graph 2 > 1: Yes Click OK The resulting plot is shown in Figure Similarly plot velocity and acceleration versus time by activating them as: Geo Panel: Display > XY PLOTS > Initialize (INITXYPLOT) Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) 5-8 COSMOSM Advanced Modules

70 Part 1 ASTAR Advanced Dynamics Analysis Figure 5-3. Displacement Versus Time (Node 22) 5. Plot the desired graphs using the XYPLOT (Display > XY PLOTS > Plot Curves) command. For other type of analysis such as Harmonic Analysis" you may plot, in a similar manner, the response versus frequency. Deformation and Contour Plots 1. Clear screen using Clear icon. Issue the DEFPLOT (Results > PLOT > Deformed Shape) command to have a deformation plot at desired time steps. Geo Panel: Results > PLOT > Deformed Shape (DEFPLOT) Time step number > 15 Beginning element > 1 Ending element > 10 Increment > 1 Scale factor > Default Click OK The result is shown in Figure 5-4. Activate the desired component and time step and then issue the ACTDIS (Results > PLOT > Displacement), DISPLOT (Results > PLOT > Displacement) command COSMOSM Advanced Modules 5-9

71 Chapter 5 Detailed Description of Examples to have the contour plot of displacement, velocity, and acceleration at desired time steps. Figure 5-4. Deformation Plot Animation of Response 1. To have an animation of (displacement, velocity or acceleration) use the following command. Geo Panel: Results > PLOT > Animate (ANIMATE) Beginning time step > 20 Ending time step number > 40 Time step increment > 1 Animation type > Two-way animation Delay > 0 Scale factor > Default Click OK List of Nodes with Highest Response Values 1. The PD_MAXMIN (Analysis > POST_DYNAMIC > PD_OUTPUT > List Peak Response) command sets flags for searching nodes with extreme response values among a set of nodes and in a given time (frequency in Harmonic Analysis), and lists the picked responses at those nodes. Geo Panel: Analysis > POST_DYNAMIC > PD_OUTPUT > List Peak Response (PD_MAXMIN) Max. flag > Displacement Maximums dirn. flag > Y-translation Number of maximum > 5 For the top 5 values 5-10 COSMOSM Advanced Modules

72 Part 1 ASTAR Advanced Dynamics Analysis Starting node label > 1 Search among all nodes Ending node label > 300 Starting time > 0 For the time range of 0 to 0.3 Ending time > Issue the PD_PREPARE (Analysis > POST_DYNAMIC > Prepare PD Plot) command to search for max/min response values: Geo Panel: Analysis > POST_DYNAMIC > Prepare PD Plot (PD_PREPARE) Option > Maxmin Click OK 3. List the max/min responses by using the PD_MAXLIS (Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Value) command: Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Value (PD_MAXLIS) There are other postprocessing options such as contour plot and section plot. (Refer to the next example "Dynamic Analysis of a Culvert"). Stress Analysis and Related Postprocessing To have a record of the stress results (in the output file) for designated time steps, select R_STRESS (Analysis > STATIC > Run Stress Analysis). If you intend to plot stress results, you should proceed as follows: XY-Plot of Stresses 1. First, specify the elements and directions for which you desire to have Stress/ Force versus Time plots (in the Harmonic analysis, Stress/Force versus Frequency plots). You may also reduce computations by specifying a reduced pattern of solution steps using the PD_PLTINT (Analysis > POST_DYNAMIC > PD OUTPUT > Specify Interval) command. Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph (PD_SXYSET) Graph number [1] > 1 COSMOSM Advanced Modules 5-11

73 Chapter 5 Detailed Description of Examples Element label > 1 Direction flag > 4 Force/moment location for plot 1 > 1 Use PD_PLTLIST (Analysis > POST_DYNAMIC > PD_OUTPUT > List Plot Info) to list the requested XY-plots. For multi-layer elements, the A_STRESS (Analysis > STATIC > Stress Analysis Options) command must be used to select the layer number. It can also be used to select the face for which the stresses will be computed. You may specify other elements/directions with the repeated use of the PD_SXYSET (Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph) command. After specifying all the desired locations and directions, then, you may issue the R_STRESS (Analysis > STATIC >Run Stress Analysis) command: Geo Panel: Analysis > STATIC > Run Stress Analysis (R_STRESS) Run stress module Geo Panel: Display > XY PLOTS > Initialize (INITXYPLOT) (Initialize XY-plot information) Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) Activate XY-plot of time versus stress for element 1 direction 4 (select Stress for the Y variable. Direction 4 is the Txy component) Geo Panel: Display > XY PLOTS > Plot Curves (XYPLOT) Plot the activated stress versus time The resulting plot is shown in Figure 5-5 (note that the XYRANGE (Display > XY PLOTS > Set Plot Range) command can be used to set the X- and Y-ranges) COSMOSM Advanced Modules

74 Part 1 ASTAR Advanced Dynamics Analysis Figure 5-5. Stress Versus Time (Element 1 Direction 4) Stress Contours at Specified Time Step(s) Similar to the deformation plots (explained earlier), you can produce stress profiles at certain time steps: Geo Panel: Results > PLOT > Stress (ACTSTR) Activate von Mises stresses for time step 15 Plot stress profile The resulting plot is shown in Figure 5-6. Since PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options) was issued previously for a response plot of desired time step, it was not repeated again here. You may use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) commands to identify the requested plots or the RESULTS (Results > Available Result) command to list the available steps in the plot file. COSMOSM Advanced Modules 5-13

75 Chapter 5 Detailed Description of Examples Figure 5-6. Stress Profile Other Postprocessing Options You may use the ANIMATE (Results > PLOT > Animate) command to animate stress plots at different time steps. You may use the LSECPLOT (Results > PLOT > Path Graph) command to animate stress along a section. You can use the STRMAX (Results > EXTREMES > Stress) command to find the maximum stresses at certain time steps or all available steps in plot file. For Harmonic Analysis, postprocessing is similar but uses frequency instead of time. Random Vibration At this stage, first run a new problem with calculating the frequency first or retrieve the data base for the frequency solution as was recommended previously or use the same data base, but undo carefully all the dynamic commands issued for previous analyses. This part is divided into three steps. In Step 1, the response is evaluated. In Step 2 the postprocessing of the response is described. In Step 3, the stress evaluation process and subsequent postprocessing are outlined COSMOSM Advanced Modules

76 Part 1 ASTAR Advanced Dynamics Analysis Evaluation of Response 1. In this step, the response (displacement, velocity or acceleration) is evaluated at different frequency steps. To start, first define the type of analysis by issuing the following command: Geo Panel: Analysis > POST_DYNAMIC > Sel PD Analysis Type (PD_ATYPE) Post dynamic type > 4 Random Vibration Analysis No. of frequency > 4 Units of exciting freqs. > Rad/sec Starting frequency > 10 Ending frequency > 4000 Correlation flag > Fully correlated Analysis method flag > Standard No. of frequency points > 11 Number of frequencies to be selected between two adjacent natural frequencies Gauss integration order > 2 point Integration points for Power Spectral Density Biasing parameter > 3 Used to select the location of frequency points Cross-mode cut-off ratio > 1E+10 Limit on the ratio of any two mode frequencies PSD stress computation flag > Yes Click OK The default values for "Number of Frequency Points" and "Biasing Pararameters" are based on the modal critical damping ratio. The unit of PSD results (unit of response) 2 / frequency is consistent with the frequency units specified in the above command. Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Print Options (PD_PRINT) Displacement print flag > On Velocity print flag > On Acceleration print flag > On Phase angle print flag > Off Missing mass correction flag > Off COSMOSM Advanced Modules 5-15

77 Chapter 5 Detailed Description of Examples Accept default for the remaining entries Click OK 2. Next define the modal damping: Geo Panel: Analysis > POST_DYNAMIC >PD DAMP/GAP > Modal Damp (PD_MDAMP) Mode set number > 1 First mode > 1 Last mode > 4 Damping constant > 0.1 Consider modal damping of 0.1 for the first four modes Click OK 3. The type of curve to be used in this analysis is defined by the following command: Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Curve Type (PD_ CURTYP) Curve label > 1 Press Continue Type of curve > Frequency Consider frequency Excitation type > Uniform base Click OK 4. In some other applications you may wish to apply loads instead of the base motion. That can be accomplished by entering 0 instead of 1 for the third prompt of the above command and using the FND (LoadsBC > STRUCTURAL > FORCE > Define Nodes) or similar commands. 5. The random excitation input required for this analysis consists of a curve defining values of Power Spectral Densities (PSD) versus frequencies: Geo Panel: Analysis > POST DYNAMIC > PD CURVES > Define (PD_CURDEF) Associated curve label > 1 Starting point number > 1 Frequency at point 1 > 0 Curve value at point 1 > 1 Frequency at point 2 > 4000 Curve value at point 2 > COSMOSM Advanced Modules

78 Part 1 ASTAR Advanced Dynamics Analysis Click OK [To define more than one curve, use the "ACTSET,TC,..." (Control > ACTIVATE > Set Entity) command] If you like to read the curve data from an external file, input "0" for the "Starting Point Number" prompt. You will then be asked to specify the file name. Refer to the on-line help for the PD_CURDEF (Analysis > POST_DYNAMIC > PD CURVES > Define) command for the format of the file. 6. Define the type and direction of the uniform base excitation by issuing the PD_BASEFAC (Analysis > POST_DYNAMIC > PD BASE EXCITATION > Base Excitation Factor) command: Geo Panel: Analysis > POST_DYNAMIC > PD BASE EXCITATION > Base Excitation Factor (PD_BASEFAC) Curve label > 1 Base excitation type > Acceleration Base_Cur multx. X comp. > 0 Base_Cur multx. Y comp. > g 2 as the curve multiplier in Y-direction Base_Cur multx. Z comp. > 0 Phase angle > 0 Accept Defaults... You may also define Base multipliers in local Cartesian coordinates by activating the desired coordinate system prior to issuing the PD_BASEFAC (Analysis > POST_DYNAMIC > PD BASE EXCITATION > Base Excitation Factor) command. 7. To review your input so far, use the PD_ALIST (Analysis > POST_DYNAMIC > List PD Analysis Options), PD_CURLIST (Analysis > POST_DYNAMIC > PD CURVES > List), and PD_BSLIS (Analysis > POST_DYNAMIC > PD BASE EXCITATION > List Base Excitation) commands. To modify the above input, reissue the corresponding command (to modify any curve point, reissue the PD_CURDEF (Analysis > POST_DYNAMIC > PD CURVES > Define) command with the Starting Point Number" same as the desired point). Plotting Assignments 1. You may specify the frequency steps for which you want to have plots of PSD of response (only with the standard method). COSMOSM Advanced Modules 5-17

79 Chapter 5 Detailed Description of Examples Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options (PD_PLOT) Accept defaults... [RMS of response will be considered irrespective of PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options]. You may also utilize the animation facilities of GEOSTAR here as well. 2. You could also specify the nodes for which you desire XY-plots (PSD of response versus frequency). You may reduce the range of computation by using the PD_PLTINT (Analysis > POST_DYNAMIC > PD OUTPUT > Specify Interval) command. Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Response Options (PD_NRESP) Starting location > 1 Node 1 > 22 Node 2 > 10 Click OK You may use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) to list all the requested outputs. 3. Issue the R_DYNAMIC (Analysis > POST_DYNAMIC > Run Post Dynamic) command to calculate the response: Geo Panel: Analysis > POST_DYNAMIC > Run Post Dynamic (R_DYNAMIC) Postprocessing of the Response XY-Plot of Response Plots of power spectral density of response (displacement, velocity or acceleration) versus exciting frequencies at certain nodes (Q-plots) can be obtained by issuing the following commands: 1. Activate the XY-plot for accelerations: Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) Graph number > 1 X-variable > Freq Y-variable > AY 5-18 COSMOSM Advanced Modules

80 Part 1 ASTAR Advanced Dynamics Analysis Node number > 22 Graph color > 12 Graph line style > Solid COSMOSM Advanced Modules 5-19

81 Chapter 5 Detailed Description of Examples Graph symbol style > 1 Graph id > 22N 2. Use the XYPLOT (Display > XY PLOTS > Plot Curves) command to plot: Geo Panel: Display > XY PLOTS > Plot Curves (XYPLOT) Plot graph > Yes The resulting plot is shown in Figure 5-7. Figure 5-7. Response PSD Versus Frequency In a similar manner, you may also plot the PSD of displacement and velocity versus frequency. Deformation and Contour Plot of Response 1. Use the DEFPLOT (Results > PLOT > Deformed Shape) command to plot deformation at the desired frequency step. 2. Use ACTDIS, DISPLOT (Results > PLOT > Displacement) commands to plot displacement, velocity or acceleration at a desired frequency COSMOSM Advanced Modules

82 Part 1 ASTAR Advanced Dynamics Analysis List of Nodes with Highest Response Values 1. The PD_MAXMIN (Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Response) command sets flags for searching nodes with highest response PSD values among a set of nodes and in a given frequency range, and lists the picked responses at those nodes. Geo Panel: Geo Panel:Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Response (PD_MAXMIN) Max. flag > Acceleration Maximums direction > Y-direction Number of maximums > 5 Starting node label > 1 Ending node label > 300 Starting frequency > 0 Ending frequency > Issue the PD_PREPARE (Analysis > POST_DYNAMIC > Prepare PD Plot) command to search for max/min response values: Geo Panel: Analysis > POST_DYNAMIC > Prepare PD Plot (PD_PREPARE) Option 1 > MaxMin 3. List the max/min responses by using the PD_MAXLIS (Analysis > POST_ DYNAMIC > PD OUTPUT > List Peak Value) command: Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Value (PD_MAXLIS) Stress Analysis and Related Postprocessing If you wish to have XY-plot or contour plot of PSD of stresses, you may use PD_SXYSET (Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph) and PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options) commands prior to running stresses with proper flag in PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command. Geo Panel: Analysis > STATIC > Run Stress Analysis (R_STRESS) COSMOSM Advanced Modules 5-21

83 Chapter 5 Detailed Description of Examples XY-Plot of Stresses You may use actxypost (Display > XY PLOTS > Activate Post-Proc) and XYPLOT (Display > XY PLOTS > Plot Curves) commands to display the XY-plot of PSD stresses. RMS of Stress Response 1. You may plot the RMS of the stresses by issuing the following sequence of commands: Geo Panel: Results > SETUP > Set to Post Process Type (ACTPOST) Select Post Dynamic Analysis Geo Panel: Results > PLOT > Stress (ACTSTR, STRPLOT) The RMS stresses are stored in step "N+1" (default step in ACTSTR), where N is the number of steps reserved for PSD values. The resulting plot is shown in Figure 5-8. You may also display the contour plots of PSD of stresses for which you requested plots (prior to running stresses) in a similar manner. Figure 5-8. RMS of Stress Profile The STRLIST (Results > LIST > Stress Component) and STRMAX (Results > EXTREMES > Min/Max Stress) commands are also available for reviewing the results COSMOSM Advanced Modules

84 Part 1 ASTAR Advanced Dynamics Analysis Dynamic Analysis of a Culvert Analysis Types Modal Time History Response Spectrum Generation Harmonic Analysis Random Vibration Response Spectrum Analysis Multi-base Motion Application (with composite material damping) Figure 5-9 Given E = 30,000,000 psi L = 200 in H = 80 in Density = 1 lb sec 2 /in 4 Poisson ratio = 0.3 GEOSTAR Commands These commands cover the modeling and frequency analysis of the problem to find the first five modes. You can directly type them in the console window. The control panel to cryptic commands are also indicated. Geo Panel: Geometry > GRID > Plane (PLANE) PLANE,Z,0,1, COSMOSM Advanced Modules 5-23

85 Chapter 5 Detailed Description of Examples Use View icon to set X-Y view VIEW,0,0,1,0, Geo Panel: Geometry > CURVES > Draw Line/Arc (CRSPOLY) CRSPOLY,1,80,0,0,L, 100,0,0,L, 80,40,0,L, 20,40,0,L, 0,0,0,L, 20,0,0, N,80,0,0, Geo Panel: Geometry > CURVES > MANIPULATION MENU > Break (equally) (CRBRK) CRBRK,2,4,1,2,0, CRBRK,7,6,1,3,0, Geo Panel: Geometry > SURFACES > Define by 2 Cr (SF2CR) SF2CR,1,2,14,0, SF2CR,2,8,13,0, SF2CR,3,3,7,0, SF2CR,4,9,12,0, SF2CR,5,4,11,0, SF2CR,6,10,6,0, Geo Panel: Propsets > Element Group (EGROUP) EGROUP,1,PLANE2D,0,1,2,0,0,0,0,0, Geo Panel: Propsets > Material Property (MPROP) MPROP,1,EX,30E6, MPROP,1,NUXY,.3, MPROP,1,DENS,1., Geo Panel: Meshing > PARAMETRIC MESH > Surfaces (M_SF) M_SF,1,6,1,4,2,2,1,1, Geo Panel: Geometry > CURVES > MANIPULATION MENU > Merge (CRMERGE) CRMERGE,1,20,1,0.0001,1,1,0, Geo Panel: LoadsBC > STRUCTURAL > DISPLACEMENT > Define Curves (DCR) DCR,1,UX,0,5,4,UY,, Geo Panel: LoadsBC > STRUCTURAL > DISPLACEMENT > Define Nodes (DND) 5-24 COSMOSM Advanced Modules

86 Part 1 ASTAR Advanced Dynamics Analysis DND,1,UZ,0,54,1,, Geo Panel: Meshing > NODES > Merge (NMERGE) NMERGE,1,54,1,0.0001,0,1,0, Geo Panel: Analysis > FREQUENCY/BUCKLING > Frequency Options (A_FREQUENCY) A_FREQUENCY,5,S,16,0,0,0,0,1e-05,0,1e-06,0,0,0,0; Geo Panel: Analysis > FREQUENCY/BUCKLING > Run Frequency (R_FREQUENCY) R_FREQUENCY Modal Time History Analysis (You may save the data base of the frequency run in another file for later use with a different analysis type.) With a time varying pressure load on the top of the structure (pressure increases linearly from 0 to 10 psi within 0.1 sec and remains constant thereafter). GEOSTAR Commands for Evaluation of Response Geo Panel: Analysis > POST_DYNAMIC > Sel PD Analysis Type (PD_ATYPE) Post dynamic analysis type > Modal time history analysis Number of frequencies > 5 Number of time steps in the solution > 50 Starting time > 0.0 Time step size > Time integration method > Newmark-Beta COSMOSM Advanced Modules 5-25

87 Chapter 5 Detailed Description of Examples First integration parameter > 0.5 Second integration parameter > 0.25 Type of response print out > Rel displ and rel vel Load case for initial condition > 0 Accept defaults... Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT> Set Print Options (PD_PRINT) Displacement print > On Beginning step for stress print > 1 Ending step for stress print > 50 Increment > 1 Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Curve Type (PD_CURTYP) Curve label > 1 Type of curve > Time Excitation type > Force/pressure Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Define (PD_CURDEF) Curve label > 1 Starting point number > 1 Time at point 1 > 0.0 Curve value at point 1 > 0.0 Time at point 2 > 0.1 Curve value at point 2 > 1.0 Time at point 3 > 10 Curve value at point 3 > 1.0 You may read the excitation curve directly from an ASCII file; refer to on-line help. Geo Panel: LoadsBC > STRUCTURAL > PRESSURE > Define by Curves (PCR) Beginning curve > 3 Pressure magnitude > 10 Ending curve > 9 Increment > 6 Accept defaults COSMOSM Advanced Modules

88 Part 1 ASTAR Advanced Dynamics Analysis Geo Panel: Analysis > POST_DYNAMIC > PD DAMP/GAP > Modal Damp (PD_MDAMP) Mode set number > 1 First mode > 1 Last mode > 5 Damping ratio > 0.03 Response Calculation Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options (PD_PLOT) PD_PLOT,1,50,1; Specify the desired time steps for response plots. You may use the PD_PLTINT (Analysis > POST_DYNAMIC > PD OUTPUT > Specify Interval) command to reduce the range of plot Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Response Options (PD_NRESP) PD_NRESP,1,21; Specify the desired nodes for XY-plot, response versus time All the desired plots must be assigned above prior to issuing the R_DYNAMIC (Analysis > POST_DYNAMIC > Run Post Dynamic) command. You may use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) command to list all requested outputs. Geo Panel: Analysis > POST_DYNAMIC > Run Post Dynamic (R_DYNAMIC) Evaluate the response, print the results and prepare plot files Postprocessing of the Response (displacement, velocity or acceleration) In the following the response is plotted only for the pre-assigned nodes and the preassigned time steps of part b. Furthermore, the response plots are either absolute or relative (relative to the uniform base motion, if any) depending on the flag set in the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command (these conditions apply to all upcoming analysis types). COSMOSM Advanced Modules 5-27

89 Chapter 5 Detailed Description of Examples XY-Plot of Response (response versus time) To have the XY-plot of response (displacement, velocity or acceleration), issue the following commands: Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) ACTXYPOST,,time,UY,21; Assign displacement in Y-direction at node 21 Geo Panel: Display > XY PLOTS > Plot Curves (XYPLOT) XYPLOT,1; Plot the response Figure 5-10 [By repeating ACTXYPOST (Display > XP PLOTS > Activate Post-Proc) command for other nodes and directions, you can plot all the graphs together.] Deformation Plot To have the deformation plot of the model at a pre-assigned time step: Use Clear icon to clear the screen CLS; 5-28 COSMOSM Advanced Modules

90 Part 1 ASTAR Advanced Dynamics Analysis Geo Panel: Results > PLOT > Deformed Shape (DEFPLOT) DEFPLOT,6; Plot the deformation shape for step 6 Figure 5-11 Contour Plot For any type of response (displacement, velocity, or acceleration) and any component of the response (including rotational) at a pre-assigned time step: Geo Panel: Results > PLOT > Displacement (ACTDIS, DISPLOT) ACTDIS,19,VY;, DISPLOT Activate and plot Time step 19 for velocity in Y-direction Figure 5-12 COSMOSM Advanced Modules 5-29

91 Chapter 5 Detailed Description of Examples Animation Deformed shape animation: Use Clear icon to clear the screen CLS; Geo Panel: Results > PLOT > Deformed Shape (DEFPLOT) DEFPLOT; Geo Panel: Results > PLOT > Animate (ANIMATE) ANIMATE,5,10,1; [You may also use other GEOSTAR capabilities to have a better view of your results by issuing commands such as SHADE (Display > DISPLAY OPTION > Shaded Element Plot), HIDDEN (Display > DISPLAY OPTION > Hidden Element Plot), etc., prior to DEFPLOT (Results > PLOT > Deformed Shape).] Response Animation Geo Panel: Results > PLOT > Displacement (ACTDIS, DISPLOT) ACTDIS,,UY;, DISPLOT Geo Panel: Results > PLOT > Animate (ANIMATE) ANIMATE,5,10,1; (You can also animate the contour plot on the deformed shape.) Other Animations of Response You may also use commands like LSECPLOT (Results > PLOT > Path Graph), to animate along a section. Maximum and Minimum of Response The extreme values of response at a specified time step can be found and listed according to: Geo Panel: Results > EXTREMES > Min/Max Displacement (DISMAX) DISMAX,12,UY,10,0,1; For step 12, list the maximum Y-displacement; displacements within 10% of the maximum value are also listed 5-30 COSMOSM Advanced Modules

92 Part 1 ASTAR Advanced Dynamics Analysis In addition to the above mentioned postprocessing features you may utilize the following options at any node (not necessarily for the pre-assigned nodes or time steps) in your model: List of Nodes with Highest Response Values Within a Range Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Response (PD_MAXMIN) PD_MAXMIN,1,2,5,1,300,,.5; For the assigned parameters in the above command, the program searches among all the nodes within the requested time range, 0 to.5, and lists the picked vertical displacements for the five nodes with the highest responses: Geo Panel: Analysis > POST_DYNAMIC > Prepare PD Plot (PD_PREPARE) PD_PREPARE,1 Prepare the results Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Value (PD_MAXLIS) PD_MAXLIS; List the results [Notice that this option evaluates the extremes within a range of time steps contrary to the DISMAX (Results > EXTREMES > Min/Max Displacement) command which does that only for a specified step or all available steps in the plot file.] Response of a Node Relative to Another Node Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Relative Response (PD_RELRESP) PD_RELRES,21,27, Consider nodes 21 and 27 Geo Panel: Analysis > POST_DYNAMIC > Prepare PD Plot (PD_PREPARE) PD_PREPARE,2 Calculate and print in the output file the response of node 21 relative to node 27 for all time steps COSMOSM Advanced Modules 5-31

93 Chapter 5 Detailed Description of Examples Stress Calculation Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph (PD_SXYSET) PD_SXYSET,1,12,1,1, For element 12, consider XY-plot of the normal stress in x-direction. (You may use the same command to delete a requested graph by an entry of zero for element label.) Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options (PD_PLOT) PD_PLOT,1,20,1; Not needed if steps remain the same as for response plot) All the desired plots must be assigned in the above, prior to issuing R_STRESS (Analysis > STATIC > Run Stress Analysis). Geo Panel: Analysis > STATIC > Run Stress Analysis (R_STRESS) R_STRESS Evaluate the stresses Postprocessing of Stress For the above pre-assigned elements and time steps: XY-Plot of Stresses (stress versus time) Geo Panel: Results > SET UP > Set to Post Process Type (ACTPOST) ACTPOST,8 Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) ACTXYPOST,1,time stress,12,1; SX for element 12 Geo Panel: Display > XY PLOTS > Plot Curves (XY PLOT) XYPLOT; 5-32 COSMOSM Advanced Modules

94 Part 1 ASTAR Advanced Dynamics Analysis Figure 5-13 Contour plot Stress plots at Specified Time Step(s): Geo Panel: Results > SET UP > Set to Post Process Type (ACTPOST) ACTPOST,8, Geo Panel: Results > PLOT > Stress (STRPLOT) ACTSTR,19,SX, STRPLOT Activate and plot for step 19 and normal stress in X-direction Figure 5-14 COSMOSM Advanced Modules 5-33

95 Chapter 5 Detailed Description of Examples Animation of Stress Plots Contour plots of stress components for a range of time steps: Geo Panel: Results > PLOT > Stress (ACTSTR, STRPLOT) ACTSTR,20,SX;, STRPLOT Activate and plot SX component of stress Geo Panel: Results > PLOT > Animate (ANIMATE) ANIMATE,10,20,2; Animate the stress field for steps 10 to 20 with interval of 2 [By giving deformed shape option in the STRPLOT (Results > PLOT > Stress) command, you can get animation of contour plots on the deformed shape as it is deforming.] You may use commands like LSECPLOT (Results > PLOT > Path Graph) also to animate stress along a section. Maximum Stress You may use command STRMAX (Results > EXTREMES > Min/Max Stress) to find the maximum stress at a desired time step: Geo Panel: Results > EXTREMES > Min/Max Stress (STRMAX) STRMAX,20; List the maximum nodal von Misses stress at time step 20 Response Spectrum Generation To find the spectra of response at certain node and direction due to a time dependent excitation. (Re-run a new problem with the frequency part first, or retrieve the saved data base frequency solution if you have done so, or undo all the dynamics commands issued for the previous analysis.) 5-34 COSMOSM Advanced Modules

96 Part 1 ASTAR Advanced Dynamics Analysis Pre-Analysis (Running the Time History Analysis) It is necessary to run a time history prior to the actual Response Spectrum analysis since the input to the Response Spectrum analysis is the output of the Time History analysis (the time varying acceleration response at the desired node and direction) Let's consider a time varying uniform base excitation in the vertical direction: (to find the time varying acceleration response at node 21, X-direction) Geo Panel: Analysis > POST_DYNAMIC > Sel PD Analysis Type (PD_ATYPE) PD_ATYPE,2,5,50,0,.005,0,0.5,0.25,0; Specify the analysis parameters for modal time history Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Print Options (PD_PRINT) PD_PRINT,1,0,0,0,0,1,1,1,1, Print displacement only Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Curve Type (PD_CURTYP) PD_CURTYP,1,0,1, Specify uniform base excitation for a time dependent curve Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Define (PD_CURDEF) PD_CURDEF,1,1,0.,0.,.1,1.,10.,1, Define the curve Geo Panel: Analysis > POST_DYNAMIC > PD BASE EXCITATION > Base Excitation Factor (PD_BASEFAC) PD_BASEFAC,1,0,0,1,0,0; Define a velocity type base excitation in vertical direction Geo Panel: Analysis > POST_DYNAMIC > Run Post Dynamic (R_DYNAMIC) R_DYNAMIC Run the Modal Time History COSMOSM Advanced Modules 5-35

97 Chapter 5 Detailed Description of Examples Calculation of the Spectra (at Node 21, X-Direction) Geo Panel: Analysis > POST_DYNAMIC > Sel PD Analysis Type (PD_ATYPE) Post dynamic analysis type > Response Spectra Generation Number of frequencies > 5 Starting frequency > 2 Ending frequency > 50 Frequency scale > Logarithmic Number of points to be used > 50 Node label > 21 Damping ratio > 0.03 X translation flag > Generate response Specify the Response Spectra Generation analysis parameters such as desired node and direction, range of frequency and number of points Geo Panel: Analysis > POST_DYNAMIC > Run Post Dynamic (R_DYNAMIC) R_DYNAMIC Run the Response Spectra Generation The results obtained for this problem are written in files with formats compatible with the "external files" which can be read by other problems as input files through the PD_CURDEF (Analysis > POST_DYNAMIC > PD CURVES > Define) command. [See the notes for the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command]. XY-Plot of Response (Spectra Versus Frequency) Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) ACTXYPOST,,freq,UX,21; Activate node 21, X-direction for plot Geo Panel: Display > XY PLOTS > Plot Curves (XYPLOT) XYPLOT; 5-36 COSMOSM Advanced Modules

98 Part 1 ASTAR Advanced Dynamics Analysis Figure 5-15 Stress Calculation Stress calculation may be done only for time history analysis of this model. Harmonic Analysis Considering a harmonic excitation with constant amplitude within the desired range of frequency (Re-run a new problem with the frequency part first, or retrieve the saved data base frequency solution if you have done so, or use the same data base and undo carefully all the dynamics commands issued for the previous analysis.) GEOSTAR Commands for Evaluation of Response Geo Panel: Analysis > POST_DYNAMIC > Sel PD Analysis Type (PD_ATYPE) Post dynamic analysis type > Harmonic analysis COSMOSM Advanced Modules 5-37

99 Chapter 5 Detailed Description of Examples Number of frequencies > 5 Units of exciting frequencies > Rad/sec Starting frequency > 1E-11 Ending frequency > 350 Number of output frequencies > 50 Frequency scale > Linear Type of response print out > Abs disp and abs vel Geo Panel: Analysis > POST_DYNAMIC > PD DAMP/GAP > Modal Damp (PD_MDAMP) PD_MDAMP,1,1,5,0.01, Define modal dampings Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Print Options (PD_PRINT) PD_PRINT,1,1,1,1,0,1,1,50,1, Specify types of response for printing as well as desired frequency steps for stress printout Geo Panel: Control > ACTIVATE > Set Entity (ACTSET) ACTSET,TC,1, Activate curve 1 Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Curve Type (PD_CURTYP) PD_CURTYP,1,1,0, Specify a load type of excitation for a frequency dependent curve Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Define (PD_CURDEF) PD_CURDEF,1,1,0.,1.,30000,1., Define excitation curve; curve data may be read from an external file, refer to on-line help Geo Panel: LoadsBC > STRUCTURAL > PRESSURE > Define Curves (PCR) PCR,3,1.,9,6,1; Specify the pressure loads 5-38 COSMOSM Advanced Modules

100 Part 1 ASTAR Advanced Dynamics Analysis Response Calculation Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options (PD_PLOT) PD_PLOT,45,55,1; Specify the desired frequency steps for response plots Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Response Options (PD_NRESP) PD_NRESP,1,21; Specify the desired nodes for XY-plotting, response versus frequency; use the PD_PLTINT (Analysis > POST_DYNAMIC > PD OUTPUT > Specify interval) command to reduce the range of the plot All the desired plots must be assigned prior to issuing the R_DYNAMIC (Analysis > POST_DYNAMIC > Run Post Dynamic) command. Use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) command to list all requested outputs. Geo Panel: Analysis > POST_DYNAMIC > Run Post Dynamic (R_DYNAMIC) DYNAMIC Evaluate the response, print the results and prepare plot files Postprocessing of the Response (displacement, velocity or acceleration) For the above pre-assigned nodes and the pre-assigned frequency steps: XY-Plot of Response (response versus frequency) To have the XY-plot of the amplitude of response, issue the following commands: Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) ACTXYPOST,,freq,VY,21,0; Assign node 21 and direction 2, for plot of velocity amplitude COSMOSM Advanced Modules 5-39

101 Chapter 5 Detailed Description of Examples Geo Panel: Display > XY PLOTS > Plot Curves (XYPLOT) XYPLOT; Plot the response Figure 5-16 In a similar manner the XY-plotting of the phase of response can be plotted for all components: Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) ACTXYPOST,,freq,VY,21,1; Assign node 21 and direction 2, for plot of velocity phase Geo Panel: Display > XY PLOTS > Plot Curves (XYPLOT) XYPLOT; 5-40 COSMOSM Advanced Modules

102 Part 1 ASTAR Advanced Dynamics Analysis Figure 5-17 Deformation Plot To have the plot of maximum deformation (amplitude of harmonic motion) at a desired frequency: Geo Panel: Results > PLOT > Deformed Shape (DEFPLOT) DEFPLOT,55; Plot the maximum deformation at the frequency step 55 Figure 5-18 COSMOSM Advanced Modules 5-41

103 Chapter 5 Detailed Description of Examples Contour Plot For any type of response (displacement, velocity or acceleration) and any component of the response: Geo Panel: Results > PLOT > Displacement (ACTDIS, DISPLOT) ACTDIS,50,AY;, DISPLOT Activate frequency step 50 for vertical component of acceleration and plot For Harmonic analysis, the natural frequencies of the system that fall in the requested frequency range are automatically added to the sequence of frequencies requested by the user. The actual frequency at each step may be listed using the PD_ALIST (Analysis > POST_DYNAMIC > List PD Analysis Options) command. Figure 5-19 Animation: Animation of response in frequency domain (see Time History analysis for more details) Maximum deformed shape animation: Geo Panel: Results > PLOT > Deformed Shape (DEFPLOT) DEFPLOT; Geo Panel: Results > PLOT > Animate (ANIMATE) ANIMATE,45,55,1; Animate for steps 45 to COSMOSM Advanced Modules

104 Part 1 ASTAR Advanced Dynamics Analysis Response animation: Geo Panel: Results > PLOT > Displacement (ACTDIS, DISPLOT) ACTDIS,,UY;, DISPLOT Geo Panel: Results > PLOT > Animate (ANIMATE) ANIMATE,45,55,1; Animate the displacement field for steps 45 to 55 Maximum and Minimum of Response Similar to the Time History analysis, the extreme values of the response at a specified step can be found and listed according to: Geo Panel: Results > EXTREMES > Min/Max Displacement (DISMAX) DISMAX,50,UY,5,1,1; For step 50, list the maximum Y-displacement; displacements within 5% of the maximum value are also listed For any node in the model: List of Nodes with Highest Response Values Within a Range Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Response (PD_MAXMIN) PD_MAXMIN,2,2,8,1,300x,10.,300.0; For the assigned parameters in the above command, the program searches among all the nodes within the requested frequency range, 10 to 300, and lists the peak vertical velocities for the 8 nodes with the highest responses: Geo Panel: Analysis > POST_DYNAMIC > Prepare PD Plot (PD_PREPARE) PD_PREPARE,1 Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Value (PD_MAXLIS) PD_MAXLIS; List the results [Notice that this option evaluates the specified extreme response within a range of frequency steps contrary to the DISMAX (Results > EXTREMES > Min/Max Displacement) command which does that only for a specified step or all the available steps in the plot file]. COSMOSM Advanced Modules 5-43

105 Chapter 5 Detailed Description of Examples Response of a Node Relative to Another Node Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Relative Response (PD_RELRES) PD_RELRES,21,27, Consider nodes 21 and 27 Geo Panel: Analysis > POST_DYNAMIC > Prepare PD Plot (PD_PREPARE) PD_PREPARE,2 Calculate and print in the output file the response of node 21 relative to node 27 for all steps Stress Calculation Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options (PD_PLOT) PD_PLOT,43,48,1; Plot for steps 43 to 48 Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph (PD_SXYSET) PD_SXYSET,1,12,1,1; XY-plot for element 12, for SX Geo Panel: Analysis > STATIC > Run Stress Analysis (R_STRESS) R_STRESS Run stress You may use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) command to list all requested outputs. Postprocessing of Stress For the above pre-assigned elements and frequency steps: XY-Plot of Stresses (stress versus frequency) Geo Panel: Results > SET UP > Set to Post-Process Type (ACTPOST) ACTPOST, COSMOSM Advanced Modules

106 Part 1 ASTAR Advanced Dynamics Analysis Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) ACTXYPOST,,freq,stress,12,1; SX for element 12 Geo Panel: Display > XY PLOTS > Plot Curves (XYPLOT) XYPLOT; Plot the stress component Figure 5-20 Contour Plot Stress plots at specified frequency step(s): Geo Panel: Results > SET UP > Set to Post Process Type (ACTPOST) ACTPOST,8, Geo Panel: Results > PLOT > Stress (ACTSTR, STRPLOT) ACTSTR,48,SX;, STRPLOT Activate for step 48 and normal stress in X-direction and plot COSMOSM Advanced Modules 5-45

107 Chapter 5 Detailed Description of Examples Figure 5-21 Animation of Stress Plots Contour plots of stress components for a range of frequency steps: Geo Panel: Results > PLOT > Stress (ACTSTR, STRPLOT) ACTSTR,48,SX;, STRPLOT Activate SX component of stress and plot Geo Panel: Results > PLOT > Animate (ANIMATE) ANIMATE,43,48,1; Animate the stress field for steps 43 to 48 [By giving deformed shape option in the STRPLOT (Results > PLOT > Stress) command, you can get animation of contour plots on the deformed shape as it is deforming.] You may use commands like LSECPLOT (Results > PLOT > Path Graph) also to animate stress along a section. Maximum Stress You may use command STRMAX (Results > EXTREMES > Min/Max Stress) to find the maximum stress at a desired frequency step or across all frequency steps. Random Vibration Analysis Consider a vertical force at the top center, defined by its power spectral density with characteristic of a white noise (re-run a new problem with the frequency part first, or retrieve the saved frequency solution if you have done so, or use the same 5-46 COSMOSM Advanced Modules

108 Part 1 ASTAR Advanced Dynamics Analysis data base and undo carefully all the dynamics commands issued for the previous analysis). GEOSTAR Commands for Evaluation of Response Geo Panel: Analysis > POST_DYNAMIC > Sel PD Analysis Type (PD_ATYPE) Post dynamic analysis type > Random vibration analysis Number of frequencies > 5 Units of exciting frequencies > Rad/sec Starting frequency > 1E-11 Ending frequency > 350 Correlation flag > Fully correlated Analysis method flag > Standard Number of frequency points > 11 Gauss integration order > 2-point Gaussian Biasing parameter > 0 Cross-mode cut-off ratio > 1.e10 PSD stress computation flag 0=No 1=Yes > 1 Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Print Options (PD_PRINT) PD_PRINT,1,0,1,0,0, Print displacement and acceleration only Geo Panel: Analysis > POST_DYNAMIC > PD DAMP/GAP > Modal Damp (PD_MDAMP) PD_MDAMP,1,1,5,.02, Define modal damping Geo Panel: Control > ACTIVATE > Set Entity (ACTSET) ACTSET,TC,1, Activate curve 1 Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Curve Type (PD_CURTYP) PD_CURTYP,1,1,0, Define excitation type, force Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Define (PD_CURDEF) PD_CURDEF,1,1,0.,1.,10000,1., Define the excitation curve COSMOSM Advanced Modules 5-47

109 Chapter 5 Detailed Description of Examples For curves with many data points, it is easier to read the data from an external file; refer to on-line help. Geo Panel: LoadsBC > STRUCTURAL > FORCE > Define Nodes (FND) FND,21,FY,1.,21,1, Define the nodal forces For proper application of PSD in units of "g 2 /freq" use the previous example of a beam. To read the curves from the external file, look at the description for the PD_CURDEF (Analysis > POST_DYNAMIC > PD CURVES > Define) command. Response Calculation The following plot pre-assignments are applicable for the Standard method application where the PSD of response is evaluated at different frequencies (RMS values are always written in the plot file). With the Standard method flag on (command PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) and with consideration of the number of frequency points between any two adjacent natural frequencies: Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options (PD_PLOT) PD_PLOT,1,30,1; Specify the desired frequencies steps for plot of PSD of response Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Response Options (PD_NRESP) PD_NRESP,1,21; Specify the desired nodes for XY-plotting, PSD of response versus frequency; use PD_PLTINT (Analysis > POST_DYNAMIC > PD OUT- PUT > Specify Interval) command to reduce the range of the XY-plot For RMS of response there is no need for pre-assignment. Use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) command to list all requested outputs. Geo Panel: Analysis > POST_DYNAMIC > Run Post Dynamic (R_DYNAMIC) R_DYNAMIC Evaluate the response, print the results and prepare plot files 5-48 COSMOSM Advanced Modules

110 Part 1 ASTAR Advanced Dynamics Analysis The unit of PSD results (unit of response) 2 /frequency is consistent with the frequency unit specified in PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type) command. Postprocessing of the Response (displacement, velocity or acceleration) The response PSD plot is possible only for the above pre-assigned nodes and the above pre-assigned frequency steps. However, the RMS of the results are always calculated and is available for plotting: XY-Plot of Response (PSD of response versus frequency) To have the XY-plot of response issue the following commands: Geo Panel: Display > XY PLOTS > Activate Post-Proc (ACTXYPOST) ACTXYPOST,,freq,AY,21; Assign acceleration in Y-direction at node 21 Geo Panel: Display > XY PLOTS > Plot Curves (XYPOST) XYPLOT Plot the response Figure 5-22 COSMOSM Advanced Modules 5-49

111 Chapter 5 Detailed Description of Examples Deformation plot PSD deformation of the model at a desired frequency: Use Clear icon to clear the screen CLS; Geo Panel: Results > PLOT > Deformed Shape (DEFPLOT) DEFPLOT,9; Plot the deformation at frequency step 9 Figure 5-23 RMS deformation of the model: Use Clear icon to clear the screen CLS; Geo Panel: Results > PLOT > Deformed Shape (DEFPLOT) DEFPLOT; Default is the last calculated frequency step for PSD plus 1 which corresponds to the RMS 5-50 COSMOSM Advanced Modules

112 Part 1 ASTAR Advanced Dynamics Analysis Figure 5-24 Contour Plot For any type of response (displacement, velocity or acceleration) and any component of the response, for both RMS and PSD: Geo Panel: Results > PLOT > Displacement (ACTDIS, DEFPLOT) ACTDIS,,UY;, DISPLOT Activate for RMS, default frequency step and plot Figure 5-25 Geo Panel: Results > PLOT > Displacement (ACTDIS, DEFPLOT) ACTDIS,7,AY;, DISPLOT Activate frequency step 7 and plot acceleration COSMOSM Advanced Modules 5-51

113 Chapter 5 Detailed Description of Examples Figure 5-26 Animation: Animation of PSD in frequency domain (see Time History analysis for more details) Deformed shape PSD animation: Geo Panel: Results > PLOT > Displacement (DEFPLOT) DEFPLOT;1 Geo Panel: Results > PLOT > Animate (ANIMATE) ANIMATE,5,12,1; Animate for steps 5 to 12 Response PSD animation: Geo Panel: Results > PLOT > Displacement (ACTDIS, DEFPLOT) ACTDIS,,AY;, DISPLOT Geo Panel: Results > PLOT > Animate (ANIMATE) ANIMATE,5,12,1; Animate the displacement PSD for steps 5 to 12 Maximum and Minimum of Response Similar to the Time History analysis, the extreme values of the response at a specified step can be found and listed according to: 5-52 COSMOSM Advanced Modules

114 Part 1 ASTAR Advanced Dynamics Analysis Geo Panel: Results > EXTREMES > Min/Max Displacement (DISMAX) DISMAX,15,AY,5,0,1; For step 15, list the maximum Y-acceleration; accelerations within 5% of the maximum value are also listed Geo Panel: Results > EXTREMES > Min/Max Displacement (DISMAX) DISMAX,,AY,3,0,1; For response RMS, list the maximum For any node in the model: List of Nodes with Highest Response PSD Values Within a Range Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Response (PD_MAXMIN) PD_MAXMIN,3,2,5,1,300,30.,300.0; For the frequency range, 30 to 300, find the peak accelerations for the 5 nodes with the highest responses Geo Panel: Analysis > POST_DYNAMIC > Prepare PD Plot (PD_PREPARE) PD_PREPARE,1 Prepare the results Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > List Peak Value (PD_MAXLIS) PD_MAXLIS; List the results Response of a Node Relative to Another Node Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Relative Responses (PD_RELRES) PD_RELRES,21,27, Consider nodes 21 and 27 Geo Panel: Analysis > POST_DYNAMIC > Prepare PD Plot (PD_PREPARE) PD_PREPARE,2 Calculate and print in the output file the response of node 21 relative to node 27 for all frequency steps COSMOSM Advanced Modules 5-53

115 Chapter 5 Detailed Description of Examples Stress Calculation If you wish to have XY-plot or contour plot of PSD stresses you must use PD_SXYSET (Analysis > POST_DYNAMIC > PD OUTPUT > Stress Graph) and PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options) commands prior to running stresses with proper flags in PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type). Use the PD_PLTLIST (Analysis > POST_DYNAMIC > PD OUTPUT > List Plot Info) command to list all requested outputs. Geo Panel: Analysis > STATIC > Run Stress Analysis (R_STRESS) R_STRESS Postprocessing of Stress XY-Plot of Stresses You may use ACTXYPOST (Display > XY PLOTS > Activate Post-Proc) and XYPLOT (Display > XY PLOTS > Plot Curves) commands to display the XY-plot of PSD stresses. Contour plot RMS of stresses: Geo Panel: Results > SET UP > Set to Post Process Type (ACTPOST) ACTPOST,8, Activate advanced dynamics postprocessing Geo Panel: Results > PLOT > Stress (ACTSTR, STRPLOT) ACTSTR,,SX;, STRPLOT Use the default for the step number, and activate normal component of stress in X-direction and plot PSD of Stresses: In a similar manner to RMS you can display contour plots of stresses for requested steps [using PD_PLOT (Analysis > POST_DYNAMIC > PD OUTPUT > Set Plot Options) prior to running stresses] COSMOSM Advanced Modules

116 Part 1 ASTAR Advanced Dynamics Analysis Figure 5-27 Animation of Stress Plots You may animate the PSD of stresses. Maximum Stress You may use command STRMAX (Results > EXTREMES > Min/Max Stress) to find the maximum RMS stresses or maximum PSD stresses. Geo Panel: Results > EXTREMES > Min/Max Stress (STRMAX) STRMAX,12,SX; List maximum RMS stresses (default step for RMS) Response Spectrum Analysis (Re-run a new problem with the frequency part first, or retrieve the saved frequency solution if you have done so, or use the same data base and undo carefully all the dynamics commands issued for the previous analysis.) Uniform base motion in vertical direction defined by its response spectrum curve. GEOSTAR Commands for Evaluation of Response Geo Panel: Analysis > POST_DYNAMIC > Sel PD Analysis Type (PD_ATYPE) Post dynamic analysis type > Response spectra analysis COSMOSM Advanced Modules 5-55

117 Chapter 5 Detailed Description of Examples Number of frequencies > 5 Mode combination method > SRSS Cluster factor > 0.0 Units of exciting frequency > Rad/sec Unused > Unused > Mode displacement flag > No Response print out type > Both and plot Geo Panel: Analysis > POST_DYNAMIC > PD OUTPUT > Set Print Options (PD_PRINT) PD_PRINT,1,0,0,0,0 Desired types of response for printing and plotting Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Curve Type (PD_CURTYP) PD_CURTYP,1,1,1, Define base type of excitation Geo Panel: Analysis > POST_DYNAMIC > PD CURVES > Define (PD_CURDEF) PD_CURDEF,1,1,0.,1.,150,1.,200,.2, Define the excitation curve For curves with many data points, it is easier to read the data from an external file; refer to on-line help. Geo Panel: Analysis > POST_DYNAMIC > PD BASE EXCITATION > Base Excitation Factor (PD_BASEFAC) Curve label > 1 Base excitation type > Velocity Curve multiplier X comp > 0.0 Curve multiplier Y comp > 1 Curve multiplier Z comp > 0.0 Phase angle (degrees) > 0.0 Specify a velocity type of base excitation in Y direction and a curve multiplier of 1 [To read the curve values from an external file, look at the description for the PD_CURDEF (Analysis > POST_DYNAMIC > PD CURVES > Define) command.] 5-56 COSMOSM Advanced Modules

118 Part 1 ASTAR Advanced Dynamics Analysis Response Calculation To have the RMS plot of response, assign 2 for the last prompt of the PD_ATYPE (Analysis > POST_DYNAMIC > Sel PD Analysis Type), in above. There is no other pre-assignments for plotting. Geo Panel: Analysis > POST_DYNAMIC > Run Post Dynamic (R_DYNAMIC) R_DYNAMIC Evaluate the response, print the results, and prepare the plot file Postprocessing of the Response (displacement, velocity or acceleration) XY-Plot of Response (not applicable) Deformation Plot RMS deformation of the model: Use Clear icon to clear the screen CLS; Geo Panel: Results > PLOT > Deformed Shape (DEFPLOT) DEFPLOT,1; Plot the deformation COSMOSM Advanced Modules 5-57

119 Chapter 5 Detailed Description of Examples Figure 5-28 Contour Plot For any type of response (displacement, velocity or acceleration) and any component of the response, RMS: Geo Panel: Results > PLOT > Displacement (ACTDIS, DISPLOT) ACTDIS,1,VY;, DISPLOT Activate for RMS of vertical velocity and plot Figure 5-29 Animation (not applicable) 5-58 COSMOSM Advanced Modules