Transient Dynamic Analysis

Transient Dynamic Analysis
Module 4 Transient Dynamic Analysis ANSYS Dynamics

Module 4 Transient Dynamic Analysis
A. Define transient dynamic analysis and its purpose. B. Learn basic terminology and concepts underlying transient analysis. C. Learn how to do a transient analysis in ANSYS. D. Work on a transient analysis exercise. January 30, 2001 Inventory #001447 4-2 ANSYS Dynamics

Transient Analysis A. Definition & Purpose
What is transient dynamic analysis? A technique to determine the response of a structure to arbitrary time-varying loads such as an explosion. Input Loads as a function of time. Output Time-varying displacements and other derived quantities such as stresses and strains. January 30, 2001 Inventory #001447 4-3 ANSYS Dynamics

Transient Analysis … Definition & Purpose
Transient dynamic analysis is used in the design of: Structures subjected to shock loads, such as automobile doors and bumpers, building frames, and suspension systems. Structures subjected to time-varying loads, such as bridges, earth moving equipment, and other machine components. Household and office equipment subjected to “bumps and bruises,” such as cellular phones, laptop computers, and vacuum cleaners. January 30, 2001 Inventory #001447 4-4 ANSYS Dynamics

Transient Analysis B. Terminology & Concepts
Topics covered: Equation of motion Solution methods Integration time step January 30, 2001 Inventory #001447 4-5 ANSYS Dynamics

Transient Analysis - Terminology & Concepts Equation of Motion
Equation of motion for a transient dynamic analysis is the same as the general equation of motion. This is the most general form of dynamic analysis. Loading may be any arbitrary function of time. Depending on the method of solution, ANSYS allows all types of nonlinearities to be included in a transient dynamic analysis - large deformation, contact, plasticity, etc. January 30, 2001 Inventory #001447 4-6 ANSYS Dynamics

Transient Analysis - Terminology and Concepts Solution Methods
Solving the equation of motion Direct Integration Mode Superposition Implicit Explicit Full Reduced January 30, 2001 Inventory #001447 4-7 ANSYS Dynamics

Transient Analysis - Terminology and Concepts … Solution Methods
Two methods of solving the equation of motion: Mode superposition (discussed in Module 6) Direct integration Equation of motion is directly integrated step by step over time. At each time point ( time = 0, Dt , 2Dt, 3Dt,….) a set of simultaneous, static equilibrium equations (F=ma) is solved. An assumption (integration scheme) is made regarding how displacement, velocity and acceleration will vary over Dt Various integration schemes are available in literature such as Central difference, Average acceleration, Houbolt, WilsonQ, Newmark etc. January 30, 2001 Inventory #001447 4-8 ANSYS Dynamics

ANSYS uses Newmark integration scheme. Varying values of a and d causes integration scheme to change (implicit / explicit / average acceleration ). Newmark is an implicit scheme. ANSYS/LS-DYNA uses explicit scheme. See module 1 for a discussion of implicit and explicit. January 30, 2001 Inventory #001447 4-9

Solution can use either reduced or full structure matrices. Reduced matrices Used to speed up the solution. No nonlinearities (except gap) allowed. [K], [C], and [M] are written in terms of master DOF, which form a subset of the full DOF set. Reduced [K] is exact, but reduced [C] and [M] are approximate. There are other disadvantages also, not discussed in this seminar. Full matrices No reduction. Uses full [K], [C], and [M]. All nonlinearities allowed. All discussions in this seminar assume this approach. January 30, 2001 Inventory #001447 4-10 ANSYS Dynamics

Transient Analysis - Terminology and Concepts Integration Time Step
An important concept in time integration techniques is the integration time step (also ITS or Dt). ITS = time increment Dt from one time point to the next. Determines solution accuracy, so its value should be chosen carefully. ANSYS allows only a constant value of ITS for reduced and mode superposition transient analyses. In a FULL transient analysis, ANSYS can automatically vary the time step size within limits set by user (discussed later). January 30, 2001 Inventory #001447 4-11 ANSYS Dynamics

Transient Analysis - Terminology and Concepts … Integration Time Step
The integration time step ( ITS) size should be small enough to capture the following: the response frequency the contact frequency (if applicable) wave propagation effects (if applicable) Nonlinear response (plasticity, creep, contact status) January 30, 2001 Inventory #001447 4-12

Response frequency Different types of loads excite different natural frequencies of the structure. Response frequency is the weighted average of all frequencies excited by a given load. The ITS should be small enough to capture the response frequency . Twenty time points per cycle should be sufficient, i.e, Dt = 1/20f where f is the response frequency. Response period January 30, 2001 Inventory #001447 4-13 ANSYS Dynamics

Response frequency (continued) During solution, the full transient method (discussed in this seminar) prints the response frequency and the number of points per cycle at every time point. The goal is to maintain about 20 points per cycle. By default, ANSYS automatically increases or decreases ITS to maintain about 20 points per cycle at the response frequency. January 30, 2001 Inventory #001447 4-14

Contact frequency When two objects come in contact, the gap or contact surface is usually represented by a stiffness (gap stiffness). The ITS should be small enough to capture the frequency of the gap “spring.” Thirty points per cycle are recommended. This is sufficient to capture the momentum transfer between the two objects. A larger ITS might result in energy loss, and the impact may not be perfectly elastic. The response frequency printed during solution includes contact frequency. January 30, 2001 Inventory #001447 4-15 ANSYS Dynamics

Wave propagation Caused by impact. More prominent in slender structures (such as a thin rod dropped on one end). Requires a very small ITS and a fine mesh along the direction of the wave. Explicit method (available in ANSYS-LS/DYNA) may be better suited for this. January 30, 2001 Inventory #001447 4-16 ANSYS Dynamics

Nonlinear response A full transient analysis can include any type of nonlinearity. Nonlinearities can be classified into 3 types: Material nonlinearity (plasticity , creep, hyperelasticity …) Geometric nonlinearity (large strain , large rotation, buckling) Element nonlinearity (contact , cable) Nonlinearities require an iterative solution at each time point. These iterations are called equilibrium iterations. January 30, 2001 Inventory #001447 4-17

Nonlinear response (continued) Smaller ITS sizes generally help equilibrium iterations to converge quickly. Nonlinearities such as plasticity, creep and friction are non-conservative in nature and require the load history to be followed accurately. A small ITS size helps in following the load history accurately. A small ITS size is also required to capture changes in contact status. January 30, 2001 Inventory #001447 4-18

Nonlinear response (continued) Example of ball hitting a plate With large Dt the ball goes through the plate. If ball goes through too far then contact will not be detected (beyond pinball radius). At time = t At time = t+Dt January 30, 2001 Inventory #001447 4-19

So how do you choose an ITS? Recommended way is to activate automatic time stepping (AUTOTS), then provide Dtinitial , Dtmin , and Dtmax. ANSYS uses an automatic time stepping algorithm (AUTOTS) to determine the optimum Dt value for a given problem. Example: If AUTOTS is on with Dtinitial= 1 sec, Dtmin= 0.01 sec, and Dtmax= 10 sec; then ANSYS starts with an ITS= 1 sec and allow it to vary between 0.01 and 10 depending on the structure’s response. January 30, 2001 Inventory #001447 4-20

AUTOTS is on by default for full transient analyses and is not available for reduced and mode superposition methods. AUTOTS will reduce the ITS (up to Dtmin) if: less than 20 points are being used at the response frequency solution is diverging solution takes a large number of equilibrium equations (slow convergence) plastic strain is accumulated in one time step exceeds 15% Creep ratio exceeds 0.1 if contact status is about to change ( controlled by KEYOPT(7) of most contact elements) January 30, 2001 Inventory #001447 4-21

Transient Analysis C. Procedure
We will discuss the Full method only in this section. Five main steps: Build the model Choose analysis type and options Specify BC’s and initial conditions Apply time-history loads and solve Review results January 30, 2001 Inventory #001447 4-22 ANSYS Dynamics

Transient Analysis Procedure Build the Model
All nonlinearities are allowed. Remember density! See also Modeling Considerations in Module 1. Typical commands: /PREP7 ET,... MP,EX,... MP,DENS,… ! Geometry … ! Mesh January 30, 2001 Inventory #001447 4-23 ANSYS Dynamics

Transient Analysis Procedure Choose Analysis Type & Options
Build the model Choose analysis type and options: Enter Solution and choose transient analysis. Choose Full transient Solution options - discussed next. Damping - discussed next. Typical commands: /SOLU ANTYPE,TRANS,NEW January 30, 2001 Inventory #001447 4-24 ANSYS Dynamics

Transient Analysis Procedure … Choose Analysis Type & Options
Solution options Choose large displacement transient or small displacement transient . When in doubt, choose large displacement transient Specify time at end of load step. Automatic time stepping (discussed next) Specify initial, min and max values of Dt for this load step. Specify output controls (discussed next) Typical commands: TRNOPT,FULL NLGEOM,… SSTIF,… NROPT,… LUMPM,… EQSLV,... January 30, 2001 Inventory #001447 4-25 ANSYS Dynamics

Automatic time stepping An algorithm that automatically calculates appropriate ITS sizes during the transient. Recommendation is to activate it and also specify minimum and maximum values of ITS. If nonlinearities are present, use the “Program Chosen” option. Note: The global solution controls switch [SOLCONTROL] is ON by default. We recommend leaving it as is. More importantly, do not turn this switch on and off between load steps. January 30, 2001 Inventory #001447 4-26 ANSYS Dynamics

Output controls Used to determine what is written to the results file. Use the OUTRES command or choose Solution > Sol’n Control.. > Basic in the menu Typical choice is to write all items at every substep to the results file. Allows smooth plots of results vs. time. Might cause results file to be large. Typical commands: OUTRES,ALL,ALL January 30, 2001 Inventory #001447 4-27 ANSYS Dynamics

Turn transient effects on/off useful for setting up initial conditions (discussed later) Ramp or Step apply load Specify damping (discussed next) Use default values for time integration parameters January 30, 2001 Inventory #001447 4-28

Damping Both alpha damping and beta damping are available. In many cases, alpha damping (viscous damping) is ignored and only beta damping (damping due to hysteresis) is specified: b = 2/w where x is the damping ratio and w is the dominant response frequency (rad/sec). Material damping (e.g. rubber) and element damping (e.g. shock absorber) are also available. Typical commands: ALPHAD,… BETAD,… January 30, 2001 Inventory #001447 4-29 ANSYS Dynamics

Choose solver By default ANSYS chooses Sparse solver For large problems (> dofs) use PCG solver January 30, 2001 Inventory #001447 4-30

Transient Analysis Procedure Specify BC’s & Initial Conditions
Build the model Choose analysis type and options Specify BC’s and initial conditions BC’s in this case are loads or conditions that remain constant throughout the transient, e.g: Fixed points (constraints) Symmetry conditions Gravity Initial conditions are discussed next. Typical commands: DK,… ! or D or DSYM DL,… DA,… ACEL,… OMEGA,... January 30, 2001 Inventory #001447 4-31 ANSYS Dynamics

Transient Analysis Procedure … Specify BC’s & Initial Conditions
Transient analyses require initial displacement (u0) and initial velocity(v0) to be specified. By default, u0= v0 = a0 = 0. Examples where non-zero initial conditions may be required: Aircraft landing gear (v00). A golf club striking a ball (v00). Drop test of an object (u0= v0 =0 , a00). January 30, 2001 Inventory #001447 4-32 ANSYS Dynamics

Two ways to apply initial conditions: Start with a static load step Useful when initial conditions need to be applied on only a portion of the model, such as “plucking” the end of a cantilever beam with an imposed displacement (u0 is known , v0 =0) Required for applying a non-zero initial acceleration. Use the IC command Solution >Loads- Apply > Initial Condit’n > Define + Useful when a non-zero initial displacement or velocity needs to be applied on the entire body. January 30, 2001 Inventory #001447 4-33 ANSYS Dynamics

Example - Dropping an object from rest In this case a0=g (gravitational acceleration) and u0 = v0=0. Use the static load step method. Load step 1: Transient effects OFF. Use TIMINT,OFF command or Solution > Sol’n Control > Transient > Transient Effects Small time interval, e.g, 2 substeps, stepped loads. (If ramped or with one substep, v0 will be non-zero.) Hold the object at rest, i.e, fix all DOFs on the object. Apply acceleration of g. SOLVE. Typical commands: ! Load step 1 TIMINT,OFF ! Transient effects OFF TIME,0.001 ! Small time interval NSEL,… ! Select all nodes on the dropped object… D,ALL,ALL,0 ! … and fix them in all directions (temporarily) NSEL,ALL ACEL,… ! Acceleration value NSUBST,2 ! Two substeps KBC,1 ! Stepped loads SOLVE January 30, 2001 Inventory #001447 4-34 ANSYS Dynamics

Load step 2: Transient effects ON. Release the object, i.e, delete DOF constraints on the object. Specify ending time and continue with the transient. Application of Temporal Acceleration Acel 0.0005 0.001 t Load step 1 Typical commands: ! Load step 2 TIMINT,ON ! Transient effects ON TIME,… ! Actual time value at end of load step NSEL,… ! Select all nodes on the dropped object… DDELE,ALL,ALL ! … and release them NSEL,ALL SOLVE ... January 30, 2001 Inventory #001447 4-35 ANSYS Dynamics

Example - “Plucking” the free end of a cantilever beam In this case u00 at one end of the beam, and v0=0. Use the static load step method. Load step 1: Transient effects OFF. Use TIMINT,OFF command or Solution >Sol’n Control > Transient > Transient Effects Small time interval, e.g, 2 substeps, stepped loads. (If ramped or with one substep, v0 will be non-zero.) Apply the desired non-zero displacement at the free end of the beam. SOLVE. Typical commands: ! Load step 1 TIMINT,OFF ! Transient effects OFF TIME,0.001 ! Small time interval D,… ! Imposed displacement at desired node(s) NSUBST,2 ! Two substeps KBC,1 ! Stepped loads SOLVE January 30, 2001 Inventory #001447 4-36 ANSYS Dynamics

Load step 2: Transient effects ON. Delete the imposed displacement. Specify ending time and continue with the transient. Typical commands: ! Load step 2 TIMINT,ON ! Transient effects ON TIME,… ! Actual time value at end of load step DDELE,… ! Delete the imposed displacement ... SOLVE January 30, 2001 Inventory #001447 4-37 ANSYS Dynamics

Example - Initial velocity on a golf club head Assuming that only the club head is modeled and that the entire head moves, we have v00. We will also assume that u0 = a0 = 0. The IC command method is convenient for this case. Select all nodes on the club. Use the IC command to apply initial velocity, or Choose Solution > Loads- Apply > Initial Condit’n > Define + Pick all nodes. Select direction and enter velocity value. Activate all nodes. Specify ending time, apply other loading conditions (if any), and solve. Typical commands: NSEL,… IC,… NSEL,ALL TIME,… … SOLVE January 30, 2001 Inventory #001447 4-38 ANSYS Dynamics

Example - A stationary plate subjected to an impulse load In this case u0 = v0 = a0 = 0. These are the default initial conditions in ANSYS, so there is no need to specify them! Simply apply the boundary conditions and the impulse load, then solve. January 30, 2001 Inventory #001447 4-39 ANSYS Dynamics

Transient Analysis Procedure Apply Time-History Loads & Solve
Build the model Choose analysis type and options Specify BC’s and initial conditions Apply time-history loads and solve Time-history loads are loads that vary with time. Three ways to apply them: Function tool Tabular input Multiple load steps Load t Load t Load t January 30, 2001 Inventory #001447 4-40 ANSYS Dynamics

Transient Analysis Procedure … Apply Time-History Loads & Solve
Function Tool Allows you to apply complicated boundary conditions. To access the function editor, choose Solution > Loads-Apply > Functions-Define/Edit Recommendation: do not use the Function Tool if the boundary conditions can be expressed directly with tabular input For more information refer to “Applying Loads Using Function Boundary Conditions” in the Basic Analysis Guide. Typical commands: ! First define a load-vs-time array *DIM,FORCE,TABLE,5,1,,TIME ! Array of type table FORCE(1,0)=0,0.5,1,1.01,1.5 ! Time values FORCE(0,1)=0,22.5,10,0,0 ! Force values ! Then apply the array to desired nodes NSEL,… ! Select desired nodes F,ALL,FZ,%FORCE% ! Apply table at all selected nodes NSEL,ALL ... January 30, 2001 Inventory #001447 4-41 ANSYS Dynamics

Tabular input Allows you to define a table of load vs. time (using array parameters) and apply the table as a load. Very convenient, especially if there are several different loads, each with its own time history. For example, to apply the force-vs-time curve shown: 1. Choose Solution > Loads- Apply > Force/Moment > On Nodes, then pick desired nodes. 0.5 Force t 22.5 10 1.0 1.5 Typical commands: ! First define a load-vs-time array *DIM,FORCE,TABLE,5,1,,TIME ! Array of type table FORCE(1,0)=0,0.5,1,1.01,1.5 ! Time values FORCE(0,1)=0,22.5,10,0,0 ! Force values ! Then apply the array to desired nodes NSEL,… ! Select desired nodes F,ALL,FZ,%FORCE% ! Apply table at all selected nodes NSEL,ALL ... January 30, 2001 Inventory #001447 4-42 ANSYS Dynamics

2. Choose the force direction and “New table”, then OK. 3. Enter table name and no. of rows (no. of time points), then OK. 4. Fill in time and load values, then File > Apply/Quit. January 30, 2001 Inventory #001447 4-43 ANSYS Dynamics

5. Specify ending time and integration time step. Solution > Time/Frequenc > Time - Time Step… There is no need to specify the stepped or ramped condition. It is implied by the load curve. 6. Activate automatic time stepping, specify output controls, and solve (discussed later.) Typical commands: TIME,… ! Ending time DELTIM,0.002,0.001,0.1 ! Starting, minimum, and maximum ITS AUTOTS,ON OUTRES,… SOLVE January 30, 2001 Inventory #001447 4-44 ANSYS Dynamics

Multiple load step method Allows you to apply each segment of the load-vs-time curve in a separate load step. No need to use array parameters. Simply apply each segment and either solve the load step or write it to a load step file (LSWRITE). January 30, 2001 Inventory #001447 4-45 ANSYS Dynamics

For example, to apply the same force-vs-time curve as before: 1. Plan the approach. We will need three load steps in this case: one for the up-ramp load, one for the down-ramp load, and one for the step removal of the load. Force t 22.5 10 0.5 1.0 1.5 2. Define load step 1: Apply force = 22.5 units at the desired nodes. Specify the ending time (0.5), integration time step, and ramped loads. Activate automatic time stepping, specify output controls*, and either solve or write the load step to a load step file. *Discussed later Typical commands: ! Load step 1 F,… ! 22.5 force at desired nodes TIME,0.5 ! Ending time DELTIM,… ! Integration time step KBC,0 ! Ramped loading AUTOTS,ON OUTRES,… SOLVE ! or LSWRITE January 30, 2001 Inventory #001447 4-46 ANSYS Dynamics

3. Define load step 2: Change force values to 10.0. Specify the ending time (1.0). No need to respecify the integration time step or ramped condition. Solve or write the load step to a load step file. 4. Define load step 3: Delete the forces or set their values to zero. Specify the ending time (1.5) and stepped loads. Typical commands: ! Load step 2 F,… ! 10.0 force at desired nodes TIME,1.0 ! Ending time SOLVE ! or LSWRITE ! Load step 3 FDELE,… ! Delete the forces TIME,1.5 ! Ending time KBC,1 ! Stepped loading January 30, 2001 Inventory #001447 4-47 ANSYS Dynamics

Solution Use SOLVE command (or LSSOLVE if load step files were written). At each time step, ANSYS calculates load values based on the load-vs-time curve. Typical commands: SOLVE ! or LSSOLVE FINISH January 30, 2001 Inventory #001447 4-48 ANSYS Dynamics

Transient Analysis Procedure Review Results
Build the model Choose analysis type and options Specify BC’s and initial conditions Apply time-history loads and solve Review Results Consists of three steps: Plot results vs. time at specific points in the structure. Identify critical time points. Review results over entire structure at those time points. Use POST26, the time-history postprocessor Use POST1, the general postprocessor January 30, 2001 Inventory #001447 4-49 ANSYS Dynamics

Transient Analysis Procedure Review Results - POST26
To plot results vs. time: First define POST26 variables. Tables of nodal or element data. Identified by a number  2. Variable 1 contains time-points and is predefined. January 30, 2001 Inventory #001447 4-50 ANSYS Dynamics

Transient Analysis Procedure … Review Results - POST26
Define variables (cont'd) Pick nodes that might deform the most, then choose the DOF direction. List of defined variables is updated. January 30, 2001 Inventory #001447 4-51 ANSYS Dynamics

Once the variables are defined, you can graph them or list them. A Graphed Response in the Time Domain Typical commands: /POST26 NSOL,… PLVAR,... January 30, 2001 Inventory #001447 4-52 ANSYS Dynamics

Identify critical time points Use the List Extremes menu. Note down the time points at which the minimum and maximum values occur. Typical commands: EXTREM,… FINISH January 30, 2001 Inventory #001447 4-53 ANSYS Dynamics

Transient Analysis Procedure Review Results - POST1
Review results over entire structure at critical time points Enter POST1, read results “By Time/Freq...”, and enter appropriate time value. Plot deformed shape and stress contours. Typical commands: /POST1 SET,,, ,, ! Read results at time = January 30, 2001 Inventory #001447 4-54 ANSYS Dynamics

Typical commands: PLDISP,… ! Deformed shape PLNSOL,… ! Contours January 30, 2001 Inventory #001447 4-55 ANSYS Dynamics

Typical commands: /DSCALE,,1 ! True displacement scaling PLDISP,… January 30, 2001 Inventory #001447 4-56 ANSYS Dynamics

Transient Analysis Procedure
Build the model Choose analysis type and options Specify BC’s and initial conditions Apply time-history loads and solve Review Results January 30, 2001 Inventory #001447 4-57 ANSYS Dynamics

Lesson D: Workshop - Transient Analysis
In this workshop, you will examine the transient response of a block bouncing on a beam. See your Dynamics Workshop supplement for details (Transient Analysis Workshop - Bouncing Block, Page W-28 ). January 30, 2001 Inventory #001447 4-58 ANSYS Dynamics

Transient Dynamic Analysis

Similar presentations

Presentation on theme: "Transient Dynamic Analysis"— Presentation transcript:

Similar presentations

About project

Feedback

Log in

Auth with social network:

Transient Dynamic Analysis

Similar presentations

Presentation on theme: "Transient Dynamic Analysis"— Presentation transcript:

Similar presentations

About project

Feedback