Skip to content

13. Step

Analysis-related commands primarily include *Step and *PostStep. The *Step command specifies the stages for performing the actual analysis, while *PostStep is used to organize and process the analyzed results.

In the *Step command, you can specify analysis types such as Static, Dynamic, Frequency, and Buckling. By designating a sequence of steps prior to *Step, simulations can be structured into multiple analysis phases. Subcommands within *Step include *Activate and *Inactivate for specifying or altering elements, loads, and constraints, as well as *Solver, *SolutionAlgorithm, *Convergency, *RayleighDamping, and *Modal for setting analysis options. For output specifications, commands such as *Output, *Print, *History, and *Check are available.

When the *Step command is executed, an output step named ResultStep is created in the HDB file(.hdb), where results specified by *Output are stored. *PostStep operates on an existing ResultStep to extract specific results, calculate maximum/minimum values, combine results, and generate a new ResultStep.

Names used in *Step and *PostStep must be unique and non-duplicated.

*Step

Defines an analysis step.

*Step, Type=type,...  Name=name[, PREV=prevStep, ...]
 ...
Keyword line
  • Type=step_type,...: Analysis type and additional options
    • Static: Static analysis
    • Dynamic: Dynamic analysis
    • Frequency: Frequency analysis
  • Name=name: Name of the analysis
  • PREV=prevStep: Previous analysis step. If not specified, analysis begins from the initial state.

This categorizes the analysis types as follows:

▪ Standard Analysis Steps

  • Static Analysis Steps

    • Standard load-displacement controlled static analysis step
    • Arclength-controlled static analysis step
    • Quasi-static analysis step (time-dependent static analysis)

  • Dynamic Analysis Steps

    • Time-domain analysis step

▪ Eigen Analysis Steps

  • Frequency extraction analysis step

The way time is handled depends on the analysis type:

▪ Standard Load-Displacement Controlled Static Analysis Step

The given time represents a pseudo-time, interpreted as a load factor.

▪ Arclength-Controlled Static Analysis Step

The time is normalized to a pseudo-time based on the arclength occurring when the load factor is 1 in a linear response. Thus, applying Arclength control in a linear analysis yields the same time increments as the standard method.

▪ Quasi-Static Analysis Step

A static analysis that considers time dependency without mass effects, where the given time represents real time. Time dependency arises in load cases with time functions and in time-dependent material models. To account for time dependency in static analysis, a time-dependent analysis must be performed.

▪ Dynamic Analysis Step

Considers both mass effects and time dependency, with time represented in real terms. Supported time integration methods include Newmark and Hilbert-Hughes-Taylor (HHT) methods, specified in *TimeIntegration. The default integration method is the Newmark method (or average acceleration method) with coefficients \(\small\gamma=0.5\) and \(\small\beta=0.25\). When using the HHT method, the default value for \(\small\alpha\) is -0.05.

Example
*Step, Type=Static, Name=Case2
 EquiTime, 0.1, 10
*Activate, Type=Element
 ALL
*Activate, Type=Constraint
 BC
*Activate, Type=Load
 LC2, SelfWeight
*Output
 D,FN,BSF,SSF


*Step, Type=Frequency, Name=Case7
 10
*Activate, Type=Element
 ALL 
*Activate, Type=Constraint
 BC

*Step, Type=Static

Specifying a Static Analysis Step

*Step, Type=Static,Standard|Arclength|Quasi,  Name=name, PREV=prevStep, NLGeom=ON|OFF
 {EquiTime, dtime,ntime}|{GivenTime, t1,t2,...}|{AutoTime, t0,tmax,dtmin,dtmax,maxInc}
Keyword line
  • Standard: Standard load-displacement controlled static analysis step (optional, can be omitted)
  • Arclength: Arclength-controlled static analysis step
  • Quasi: Quasi-static analysis step (time-dependent static analysis)
  • NLGeom=On|Off: Specifies geometric nonlinearity (optional, default is Off). [Reserved. Currently Unused]
First dataline
  • EquiTime, dtime, ntime: Specifies equal time increments for the analysis. It is equivalent to specifying the times as dtime, 2*dtime, ..., ntime*dtime.
  • GivenTime, t1, t2,...: Specifies the analysis time using given time values.
  • AutoTime, t0, tmax, dtmin, dtmax, maxInc: Defines the time increment with automatic increment settings. maxInc represents the maximum increments (default values: 1, 1, 1, 1, 1000).

*Step, Type=Dynamic

Specifies a dynamic analysis.

*Step, Type=Dynamic, Name=name, PREV=prevStep, NLGeom=ON|OFF
 EquiTime, dtime,ntime
Keyword line
  • NLGeom=On|Off: Specifies geometric nonlinearity (optional, default is Off). [Reserved. Currently Unused]
First dataline
  • EquiTime, dtime, ntime: Specifies equal time increments for the analysis. It is equivalent to specifying the times as dtime, 2*dtime, ..., ntime*dtime.
  • GivenTime, t1, t2,...: Specifies the analysis time using given time values.
  • AutoTime, t0, tmax, dtmin, dtmax, maxInc: Defines the time increment with automatic increment settings. maxInc represents the maximum increments (default values: 1, 1, 1, 1, 1000).

Currently, the equal interval option (EquiTime, t0, tmax) should be used.

*Step, Type=Frequency

Specifies a frequency analysis.

*Step, Type=Frequency, Name=name[, PREV=prevStep]
 nmode, shift
First dataline
  • nmode: Number of modes to be extracted (default is 10)
  • shift: Shifting frequency (Hz). (default is 0). If specified, calculates the natural frequency corresponding to the eigenvalue closest to 4 * π² * shift². Applicable only when the eigenvalue solver is Arpack.

*Activate

Activates elements, loads, and constraints targeted by the step.

*Activate, Typ={Element|Load|Constraint}
 target, ...
 ...
Keyword line for *Activate
  • Type=type
    • Element: Target to be activated is an element
    • Load: Target to be activated is a load
    • Constraint: Target to be activated is a constraint
First dataline and subsequent datalines
  • target: Target determined by the specified type, such as Elset, Load, or Constraint
Example
*STEP, TYPE=Static, Name=stage2 Prev=stage1
*Inativate, TYPE=ELEMENT
 slab
*Activate, TYPE=Element
 10, new_slab
*Inativate, TYPE=Load
 pointLoad
*Activate, TYPE=Load
 lineload

*Inactivate

Deactivates elements, loads, and constraints targeted by the step.

*Inactivate, Type={Element|Load[,Ramp]|Constraint}
 target, ...
 ...
Keyword line
  • Type=type
    • Element: Target element to be deactivated
    • Load[, Ramp]: Target load to be deactivated. If Ramp is specified, it is removed immediately at the start of the step.
    • Constraint: Target constraint to be deactivated
First dataline and subsequent datalines
  • target: Target determined by the specified type, such as Elset, Load, or Constraint

*Solver

Changes the default solver to be applied in the analysis step.

*Solver, TYPE=LinearSolver
 Pardiso|BiCG|BiCGStab|CGS, solverOption

*Solver, TYPE=EigenSolver
 Arpack|Subspace
Keyword line
  • Type=LinearSolver: Specifies the linear solver. The default solver is Pardiso.
  • Type=EigenSolver: Specifies the eigenvalue solver, with Arpack as the default.
First dataline for TYPE=LinearSolver
  • Pardiso|BiCG|BiCGStab|CGS: Solver to be applied
  • solverOption: Options for the solver, specified as a string (optional)

▪ For Pardiso:

  • IteractiveOff|IteractiveOn-TryPositiveDefinite|PositiveDefinite|Indefinite
  • IteractiveOff|IteractiveOn: Toggle iterative solver combination (default is IterativeOff)
  • TryPositiveDefinite|PositiveDefinite|Indefinite: Specifies matrix handling for positive definite or indefinite matrices (default is TryPositiveDefinite)

▪ For BiCG, BiCGStab, CGS:

  • None|Jacobi|SSOR|ILU0|ILUT|PardisoS|PardioD|PardioDC-TryPositiveDefinite|PositiveDefinite|Indefinite
  • None|Jacobi|SSOR|ILU0|ILUT|PardisoS|PardioD|PardioDC: Specifies the preconditioner (default is None)
  • TryPositiveDefinite|PositiveDefinite|Indefinite: Specifies matrix handling for positive definite or indefinite matrices (default is TryPositiveDefinite)
First dataline for TYPE=EigenSolver
  • ARPACK|Subspace: Solver to be applied

The linear solver is used to solve a linear system of the form \(\small Kx = f\), where \(K\) is a sparse matrix. The default solver is the direct sparse solver Pardiso, but iterative sparse solvers such as BiCG, BiCGStab, and CGS are also available.

The eigenvalue solver is used to solve standard or generalized eigenvalue problems. The default is ARPACK, with Subspace iteration solver as an alternative. Both solvers use the linear sparse solver Pardiso internally. Eigenvalue solvers used in finite element methods are optimized to calculate only a few low-order modes rather than all eigenvalues. Available eigenvalue solvers include subspace iteration and ARPACK, with ARPACK as the default. The Subspace iteration solver is applicable only to symmetric matrices, while ARPACK can handle both symmetric and asymmetric matrices.

The subspace size for the Subspace iteration solver is determined by \(\small ncv = \text{min}(\text{min}(2 \times nev, nev + 8), n)\). For ARPACK, in the case of symmetric matrices, \(\small nev < ncv \leq n\) must be satisfied, and \(\small ncv = 2 \times nev\) is recommended. Therefore, it is advisable to set \(\small nev\) to be less than \(\small n/2\). The maximum allowable \(\small nev\) is \(\small nev = n - 1\). Here, \(\small n\) is the actual degree of freedom of the mass matrix, \(\small ncv\) is the size of the required subspace or Lanczos vectors for computation, and \(\small nev\) is the number of required eigenvalues.

*Convergency

Imposing convergence criteria for the standard analysis step

*Convergency, Monitor={ON|OFF}
 Force, ftol1, ftol2, fmin
 or Displacement, dtol1, dtol2, dmin
 ...
Keyword line
  • monitor: monitoring option. ON or OFF. Default OFF.
First dataline for FORCE criteria
  • ftol1, ftol2: primary and seconary tolerances for force criteria (default 1E-4, 0.01)
  • fmin: minimum allowable unbalanced force (default 0.01)
First dataline for Displacement criteria
  • dtol1, dtol2: primary and secondary tolerances for displacement criteria (default 0.01,0.01)
  • dmin: mimimum allowable displacement (default 1E-4)

Specifies convergence criteria for nonlinear analysis. These criteria are ignored in linear analysis or eigenvalue analysis (FrequencyStep and BucklingStep). Convergence criteria for energy, load, and displacement can be applied selectively and in combination. Convergence tolerances include primary and secondary tolerances. The primary tolerance applies when the iteration count is low, while the secondary tolerance applies when nonlinearity is significant, and the iteration count is high. The iteration threshold distinguishing primary and secondary tolerances (\(\small I_p\)) is 9. In other words, up to 8 iterations, the primary tolerance is applied, and beyond that, the secondary tolerance is used. The following are the default values.

  • Force/Moment criteria
\[\small || { R}_{n+1} ^i || <= \epsilon_F ~ \max (|| { R}_{n+1} ^1 || ,R_{min} ) \]
  • Displacement/Rotation criteria (applies from the second iteration onward)
\[\small || \delta U_{n+1}^i || \le \epsilon_D \max(||U_{n+1} ^{i+1} ||, D_{min} ) \]

For the load criterion, \(\small \epsilon_F\) is 1E-4 for iteration counts less than \(\small I_p\) and 1E-2 otherwise, with \(\small R_{min} = 0.01\). For the displacement criterion, \(\small \epsilon_D\) is set to 0.01, and \(\small D_{min}\) is set to 1E-4.

Example
*Step, Type=Static Name=1
...
*Convergency, Monitor=ON

*Step, Type=Static, Name=2
...
*Convergency
 Force,1E-5
*SolutionControl, Type=SolutionAlgorithm
 BFGS, 8
*SolutionControl, Type=LineSearch
 Bracketed
*SolutionControl, Type=MaxIteration
 20

*SolutionControl

Specifies options related to nonlinear analysis.

*SolutionControl, Type=MaxIteration
 maxIteration

*SolutionControl, Type=SolutionAlgorithm
 Newton|BFGS|Secant|MNewton, kernelUpdateIter

*SolutionControl, Type=LineSearch
 Bracketed, N, tol, amp, smax | Backtracking, N, tol
Keyword line
  • Type=MaxIteration|Algorithm|LineSearch: Applies maximum iteration count, algorithm, and line search methods
First dataline for MaxIter
  • maxIter: Maximum number of iterations
First dataline for Algorithm
  • Newton|BFGS|Secant|MNewton: Nonlinear analysis algorithm applied during each iteration
  • kernelUpdate: Iteration count at which the kernel matrix is rebuilt in quasi-Newton methods such as MNewton, Secant, and BFGS (optional, default is 8). Ignored in Newton method.
First dataline for LineSearch, Bracketed
  • N: Maximum allowable number of line search iterations (default is 6)
  • tol: Tolerance for line search (default is 0.8)
  • amp: Amplification factor to prevent dangerous extrapolation (default is 5.0)
  • smax: Maximum allowable scaling factor (default is 25.0)
First dataline for LineSearch, Backtracking
  • N: Maximum allowable number of line search iterations (default is 6)
  • tol: Tolerance for line search (default is 0.5)

The solution algorithm specifies the method applied to determine the equilibrium equation during iterations in nonlinear analysis. Algorithms such as Newton and BFGS can be specified, and line search techniques can be applied to ensure convergence.

Example
*Step, Type=Static, Name=step2
...
*SolutionControl, Type=SolutionAlgorithm
 BFGS, 8
*SolutionControl, Type=LineSearch
 Bracketed
*SolutionControl, Type=MaxIteration
 20

*TimeIntegration

Defines the time integration method for dynamic analysis.

*TimeIntegration, Type=Newmark,gamma,beta

*TimeIntegration, Type=HHT,alpha
Keyword line for Type=Newmark
  • Type=Newmark, gamma, beta: Newmark 시간 적분을 적용. gamma와 beta는 optional이며 디폴트는 0.5, 0.25.
Keyword line for Type=HHT
  • Type=HHT, alpha: HHT 시간 적분을 적용. alpha는 optional이며 디폴트는 –0.05

If *TimeIntegration is not specified separately, the default is set to Newmark with parameters 0.5 and 0.25.

In the Newmark method, coefficients \(\small\beta\) and \(\small\gamma\) are determined based on numerical stability and accuracy. When \(\small\gamma=1/2\), no numerical damping is introduced, whereas if \(\small\gamma>1/2\), numerical damping is introduced. Typically, values of \(\small\gamma=1/2\) and \(\small 1/6 \le \beta \le 1/4\) are chosen. With \(\small\gamma=1/2\) and \(\small\beta=1/4\), the acceleration is assumed constant within the time interval, a method known as the average acceleration method. When \(\small\gamma=1/2\) and \(\small\beta=1/6\), the acceleration is assumed to vary linearly within the time interval, known as the linear acceleration method. For numerical stability, the following condition must be satisfied:

\[\small \frac{\Delta t}{T_n} <= \frac{1}{\pi \sqrt 2} \frac{1}{\sqrt {\gamma-2\beta}}, ~~ \rm , where, T_n is natural frequency \]

Thus, using the average acceleration method ensures unconditional stability, while the linear acceleration method requires satisfying \(\frac{\Delta t}{T_n}\) for stability. In finite element problems involving multiple degrees of freedom, it is challenging to meet this stability condition up to higher modes with shorter natural periods (higher natural frequencies). Consequently, the average acceleration method is generally used for its unconditional stability, even if it sacrifices some precision.

The Hilbert-Hughes-Taylor (HHT or \(\small\alpha\)-method) extends the Newmark method by introducing controllable numerical damping while maintaining solution accuracy. It is unconditionally stable for values within \(\small -1/3 \le \alpha \le 0\). When \(\small \alpha = 0\), it is equivalent to the Newmark method with the average

Example
*Step, Type=Dynamic, Name==analysis1
 EquiTime, 0.02, 24 
*TimeIntegration, Type=HHT, -0.05
...

*RayleighDamping

Specifies Rayleigh damping values during a dynamic analysis (DynamicStep).

*RayleighDamping
 Direct, alpha,beta, targetElset
 Equivalent, fm, fn, xim, xin, targetElset
 ...
First dataline and subsequent datalines
  • Direct, alpha, beta: Specifies Rayleigh damping constants alpha and beta. Alpha and beta represent mass and stiffness proportional damping, respectively. (Both alpha and beta are optional, default values are 0, 0)
  • Equivalent, fm, fn, xim, xin: Specifies equivalent damping ratios xim and xin, along with the corresponding natural frequencies of the structure fm and fn (in Hz), usually set to the 1st and 2nd natural frequencies. Typically, xim and xin are set to the same value (all are required).
  • targetElset: Specifies the target elset, which must be an active elset in the current analysis step (optional). If omitted, Rayleigh damping applies to all active elsets in the current step.

When equivalent damping ratios are specified, Rayleigh damping coefficients alpha and beta are calculated and set using the following relation:

\[ \small \left[ \begin{matrix} \xi_m \\ \xi_n \\ \end{matrix} \right] = \frac{1}{2} \left[ \begin{matrix} 1/\omega_m & \omega_m\\ 1/\omega_n & \omega_n\\ \end{matrix} \right] \left[ \begin{matrix} \alpha \\ \beta \\ \end{matrix} \right] \]

In the above, \(\small \omega_m = 2\pi f_m\) and \(\small \omega_n = 2\pi f_n\), and the determined values of \(\small \alpha\) and \(\small \beta\) are constants in the Rayleigh damping matrix, defined as \(\small C^R = \alpha M + \beta K\).

Example
*Step, Type=Dynamic, Name=1
*Activate, Type=Element
 ELSET1, ELSET2
*RayleighDamping
 Direct, 0.5, 0.1    # Specifies all elsets in Step 1, such as ELSET1, ELSET2

*Step, Type=Dynamic, Name=2
*Activate, Type=Element
 ELSET1, ELSET2
*RayleighDamping
 Direct, 0.5, 0.1, ELSET2    # Sets a damping ratio of 0.5, 0.1 for ELSET2
 Equivalent,2.3, 5.7, 0.05, 0.05, ELSET2  # Specifies an equivalent damping ratio of 0.5 for ELSET2

Specifies the modal analysis method and its damping ratio during dynamic analysis (DynamicStep).

*MODAL, [ELSet=targetElset]
 imode,dampingRatio
 fromMode, toMode, dampingRatio
 ...
Keyword line
  • ELSET=targetElset: Specifies the elset participating in the modal analysis (optional). By default, all elements in the analysis step are included.
First dataline and subsequent datalines
  • imode, dampingRatio: Mode and damping ratio
  • fromMode, toMode, dampingRatio: Range of modes and damping ratio

Modal analysis is a special technique for performing dynamic analysis on linear systems.

  1. When specified with *Modal, *RayleighDamping is ignored.
  2. Only the Newmark method is allowed as the integration method with *Modal. If HHT or Frequency is specified as the integration method, an error occurs.
  3. Only the specified modes participate in the modal analysis. If the specified modes cannot be computed through eigenvalue analysis, an error is raised.
  4. *Load, Type=Displacement cannot be applied in modal analysis.
  5. Reaction forces in modal analysis do not consider the effects of modal damping.
  6. Modal analysis can only be applied to linear elsets.
  7. If targetElset is not specified, modal analysis is conducted on the entire model, which must be a linear system.
  8. When targetElset is specified, a partial modal analysis is performed on that specific elset using the given modes. Only the specified targetElset needs to satisfy linear conditions. This feature is especially useful in vehicle-bridge interaction analyses where nonlinearities arise due to contact point changes.
Example
*Step, Type=DYNAMIC, Name=1
 EquiTime=0.1, 2.5
*Activate, Type=Element
 Bridge
*Activate, Type=Constraint
 Boundary
*Activate, Type=Load
 ConcentricLoad
*MODAL
 1,0.001       # Mode 1 with a damping ratio of 0.001
 2,5,0.0005    # Modes 2, 3, 4, 5 with a damping ratio of 0.0005
 6,0.007       # Mode 6 with a damping ratio of 0.007
 10,15,0.001   # Modes 10 through 15 with a damping ratio of 0.001 (Modes 7, 8, and 9 are not used)

*Step, Type=DYNAMIC, Name=2
 EquiTime=0.1, 2.5
*Activate, Type=Element
 Bridge, Truck
*Activate, Type=Constraint
 Boundary
*MODAL, ELSet=Bridge  # Apply modal analysis only to Bridge
 1,10,0.01

*Field

Specifies the state field of an element.

*Field, Type={TendonStress|TendonStressHold|CableLength|MovingSpringSpeed}
 target, value
 ...
Keyword line
  • Type=type: Type of the field to specify (required)
    • TendonStress: Tendon stress
    • TendonStressHold: Tendon hold stress
    • CableLength: Cable length
    • MovingSpringSpeed: Speed of the moving spring
First dataline and subsequent datalines
  • target: Element or elset (required). TendonStress and TendonStressHold apply to Tendon elements, CableLength to Cable elements, and MovingSpringSpeed to MovingSpring elements.
  • value: Value to specify (required)
Example
*STEP, TYPE=STATIC, NAME=step1
*Activate,TYPE=ELEMENT
 tendon, conc
*Activate,TYPE=Constraint
 BC
*Field, TYPE=TendonStress
 1001 200E6
*OUTPUT
 D, FN, FK, FE, BSF
*History, Name=rebarPretension1
 step1
 BSE.Ex@1-1 BSF.Nx@1-1  BSE.Ex@1-2 BSF.Nx@1-2
 E.11@1001-1 S.11@1001-1

*Output

Specifies the output values to be saved in the HDB file(.hdb).

*Output[, ELSET=elset1, elset2, ..., Constraint=constraint1, constraint2, ..., Frequency=freqeuncy]
 field|sensorName,...
 ...
Keyword line
  • ELSET=elset1, elset2, ...: Target elsets for which results will be output in the HDB file(.hdb). If not specified, the elsets designated in *Activate, TYPE=Element are used.
  • Constraint=constraint1, constraint2, ...: Target constraints for which results will be output in the HDB file(.hdb). If not specified, constraints designated in *Activate, TYPE=Constraint are used.
  • Frequency=frequency: Output interval, default is 1. For example, if set to 3 and there are 100 increments, outputs will be generated at increments 3, 6, ..., 99, and always at the last increment (100). If frequency is set to 0, only the last increment will be output (optional).
First dataline and subsequent datalines (optional for FrequencyStep)
  • field, ...: Name of the field
  • sensorName: Name of the sensor for output

*Output specifies the node or element field values or sensor values to be output to the HDB file(.hdb). Target elsets or constraints can be specified using Element or Constraint. If the target elset or constraint is not specified, the elsets or constraints designated in *Activate, TYPE=Element/Constraint are used. The target nodes are determined by these elsets and constraints. In other words, the target elset is defined by the specified elset, and the target nset is determined by both the specified elset and constraints. Specifying a sensor for output in the dataline is independent of the target specified by Element or Constraint.

The HDB file(.hdb) creates an *ResultStep corresponding to each *Step and outputs *TargetElements, *TargetConstraints, and *TargetLoads. Here, *TargetElements and *TargetConstraints correspond to the target elsets and constraints specified in *Output. If no target elset or constraint is specified in *Output, these match the elsets or constraints specified in *Activate, TYPE=Element/Constraint. *TargetLoads always corresponds to *Activate, TYPE=Load.

Field values can be distinguished by node or element units as field values.

▪ Node-Level Fields

  • FN, FE: Equivalent nodal loads for applied loads and element loads at nodes
  • FK, FC, FM: Internal forces including elastic, damping, and inertial forces
  • D: Degree of freedom field (displacements, temperature, etc., at nodes; represents modes in frequency analysis)
  • V: First time derivative of the degree of freedom field (e.g., velocity for displacement, temperature rate, etc.)
  • A: Second time derivative of the degree of freedom field (e.g., acceleration for displacement, temperature acceleration, etc.)

The relationship for nodal loads is satisfied as FN + FE = FK + FC + FM.

▪ Element-Level Fields

  • BSF, BSE, BST: Cross-sectional force, strain, and temperature for beam elements (including truss/cable elements)
  • SSF, SSE, SST: Cross-sectional force, strain, and temperature for shell elements
  • ISF, ISE: Cross-sectional force and strain for interface elements
  • SF, SE, DF, DE: Cross-sectional force and strain for spring elements, and force and strain for damper sections
  • S, E, PE: Stress, strain, and plastic strain
  • SB: Back stress
  • IEC, IET: Compressive and tensile inelastic strain
  • ECUN, ETUN: Last committed compressive/tensile unloading strain
  • PEEQ, PEEQT, PEEQC: Equivalent plastic strain, and tensile/compressive equivalent plastic strain
  • TEMP: Temperature
  • TIME: Material time
  • ECR, ESH: Creep strain and shrinkage strain
  • EP: Element pressure
  • EW: Volumetric strain

▪ Notes 1. In frequency analysis steps (*Step, Type=Frequency), frames are output for each mode in the HDB file(.hdb). Each frame corresponds to one mode, with the mode shape output in D. The remaining field values represent values induced by this D. 2. Fields may have subcomponents. For example, D includes subcomponents such as D.X, D.Y, D.Z, etc. For details on subcomponents, refer to *History.

Example
*Step, Type=Static, Name=Case1
*Activate, TYPE=Element
 dam, water, farField
*Output
 D, SF, S, mySensor
*Print File=Case1.prn 
 D@Left, SF@Bearing

*Step, Type=Frequency, Name=FRQ
 10
*Output
 D, SSF
*Print, File=FRQMode.prn

*Print

Specifies the output values to be saved in a separate file.

*Print[, Frequency=frequency, File=file 
 field@target|sensorName...
 ...
Keyword line
  • Frequency=frequency: Output interval, default is 1. For example, if set to 3 and there are 100 increments, outputs are generated at increments 3, 6, ..., 99, and always at the last increment (100). If frequency is set to 0, only the last increment is output (optional).
  • File=file: Name of the output file in the *Print command (optional). If not specified, it is automatically named as filename-stepname-P#.csv (where filename is the name without extension, and # is a sequential number). If <DB> or <STEP> is included in the filename, they are replaced with the current DB name (name without extension from the input file) and the current step name, respectively.
First dataline and subsequent datalines
  • field@target: Field and target for output. For fields defined at nodes, target can be a node number, node number pattern, or nset; for fields defined at elements, target can be an element number, element number pattern, or elset.
  • sensorName: Name of the sensor for output

The *Print command is similar to *Output but outputs the results as text values for the specified node or elsets.