Skip to content

Analysis Types

FrontISTR provides multiple analysis types covering both structural and thermal physics, from static equilibrium through time evolution and periodic steady state to extraction of intrinsic characteristics. This page describes the phenomena addressed by each analysis type, its scope of application, and how to select among them. For input-file syntax, see the keyword reference; for mathematical details of the formulation, see the theory manual.

Overview

FrontISTR analysis types are characterized by combinations of the following three axes.

  • Target physics: Structural (displacement and stress), thermal (temperature and heat flux), or coupling between them
  • Treatment of motion: Whether inertia terms are included and whether time evolution is followed. These are independent axes
    • No inertia and no time evolution → static equilibrium
    • No inertia, but time evolution is followed → quasi-static (viscoelasticity, creep, etc.)
    • Inertia included and time evolution followed → transient dynamic response
    • Treated in the frequency domain as a periodic steady state → harmonic response
    • No external force; extract properties intrinsic to the system → intrinsic characteristics
  • Linearity: Linear (small deformation and linear material) or nonlinear (large deformation, nonlinear material, or contact)

The implemented combinations of these axes correspond to the analysis types described below. In the input, !SOLUTION specifies the broad category of analysis type, while !DYNAMIC, !EIGEN, !HEAT, and similar keywords specify associated properties in more detail. The time-step size and increments for analyses involving time evolution are controlled with !STEP.

How to Choose an Analysis Type

When selecting an analysis type, begin by organizing the phenomenon to be treated and the result you want to obtain. Even for the same object, the appropriate analysis type changes depending on what you want to know. Considering the following points in order leads to an analysis type suited to the objective.

  1. What do you want to obtain? — Displacement and stress, temperature distribution, vibration modes, or frequency response. The desired quantity determines the broad analysis category
  2. Does inertia need to be considered? — Select dynamic analysis when the load changes rapidly and acceleration affects the response. Static analysis is sufficient when changes are slow and inertia can be neglected
  3. Does time evolution need to be followed? — Even when inertia can be neglected, time-dependent material response such as viscoelasticity or creep is solved by advancing time within the static-analysis framework (quasi-static analysis)
  4. Is the assumption of linearity valid? — Linear analysis is sufficient for small deformation with linear materials. Select nonlinear analysis if large deformation, nonlinear materials, or contact is included

Typical problems and their corresponding analysis types are shown in the following table.

What you want to know Analysis type
Stress and displacement under static load Static analysis (linear or nonlinear)
Time response involving viscoelasticity or creep Static analysis (quasi-static)
Transient response such as impact or earthquake response Dynamic analysis
Natural frequencies and mode shapes Modal analysis
Frequency characteristics under harmonic excitation Frequency response analysis
Temperature distribution and heat flux Heat conduction analysis
Thermal stress due to a temperature field Thermo-mechanical coupled analysis

Static Analysis

Static analysis solves equilibrium equations while neglecting inertia terms. This framework includes not only steady equilibrium without time evolution, but also quasi-static analysis in which equilibrium at each time is tracked sequentially while advancing time when treating time-dependent material response such as viscoelasticity or creep, or nonlinearities with history. The distinction from dynamic analysis is whether inertia terms are present, not whether time evolution is present.

Linear static analysis assumes small deformation and linear materials and solves the equilibrium equation with a single linear-system solution. It has the lowest computational cost and is used for stress evaluation and studies in the early stages of design.

Nonlinear static analysis is used when any of large deformation (geometric nonlinearity), nonlinear materials (elastoplasticity, hyperelasticity, viscoelasticity, or creep), or contact is included. Because the equilibrium equation is nonlinear, the load is divided into multiple increments and applied stepwise, with iterative solution by the Newton-Raphson method within each increment. When time-dependent materials such as viscoelasticity or creep are treated, the same incremental and iterative process is performed while sequentially tracking equilibrium at each time.

In the input, specify !SOLUTION, TYPE=STATIC, and add the NONLINEAR parameter when treating nonlinearity. Time stepping, increment control, and convergence criteria are specified with !STEP. For details of increment control, see Step Control.

Dynamic Analysis

Dynamic analysis solves equations of motion including inertia terms as a time-evolution problem and obtains the response to the time history of external forces as a time history. It targets phenomena such as impact loading, earthquake response, and vibration propagation, where acceleration of the system significantly affects the response.

Time-integration methods are broadly divided into implicit and explicit methods. The choice depends on the time scale of the phenomenon, problem size, and stability requirements on the time step. Implicit methods are suitable when low-frequency components dominate and relatively large time steps are desired, while explicit methods are suitable for high-frequency phenomena such as impact and wave propagation that inherently require small time steps.

Implicit Method

The implicit method (Newmark-β method) solves a system of simultaneous equations at each time step to obtain displacement, velocity, and acceleration at the next time. There is no stability restriction on the time-step size, so for structural responses dominated by low-frequency components (such as earthquake response and mechanical vibration), relatively large time steps can be used to reduce the number of steps, making the method efficient. On the other hand, the cost of solving simultaneous equations is incurred at every step, so it is not suitable for phenomena requiring an extremely large number of steps.

Explicit Method

The explicit method (central difference method) directly calculates the state at the next time using only information from the previous step. Because it does not solve a simultaneous system, the cost per step is small, but the time-step size is limited by a condition based on the minimum natural period of the system (the CFL condition). It is advantageous for problems such as impact, wave propagation, and high-speed contact, where small time steps are inherently required.

In the input, specify !SOLUTION, TYPE=DYNAMIC, and use !DYNAMIC to select the solution method and specify integration parameters such as those for the Newmark-β method. Use !STEP when switching boundary-condition or load groups across multiple steps, or when specifying increment control for each step. In implicit nonlinear dynamic analysis, automatic increment control and cutback according to convergence behavior are also available.

Modal analysis solves the generalized eigenvalue problem formed by the mass and stiffness matrices without applying external forces, extracting the natural frequencies and natural mode shapes intrinsic to the system. It is performed to evaluate the vibration characteristics of structures, identify resonance points, and as a preliminary step when modal superposition is used in frequency response analysis.

The Lanczos method is used to efficiently extract a specified number of lower modes. A lumped mass matrix is used for the mass matrix.

In the input, specify !SOLUTION, TYPE=EIGEN, and use !EIGEN to specify the number of modes to extract, shift values, and other parameters.

Frequency Response Analysis

Frequency response analysis determines the periodic steady-state response reached by a system subjected to harmonic (sinusoidal) external forces while varying the excitation frequency. Unlike dynamic analysis that follows a time history, it solves directly in the frequency domain and is therefore suitable for evaluating resonance characteristics and designing for steady-state vibration.

The solution is based on the modal superposition method, constructing the response by superposing the natural modes obtained beforehand by modal analysis. Therefore, modal analysis must be performed for the same system before frequency response analysis. Only linear models are supported; the analysis cannot be executed when geometric or material nonlinearity is enabled.

In the input, it is treated as a form of dynamic analysis: specify !SOLUTION, TYPE=DYNAMIC, then specify frequency response using subordinate parameters of !DYNAMIC. Excitation conditions are specified with !FLOAD.

Heat Conduction Analysis

Heat conduction analysis solves the heat-conduction equation to obtain the temperature distribution and heat flux. It uses the same finite element mesh as structural analysis, but each node has only one degree of freedom, temperature, and the material properties handled are limited to thermal conductivity, specific heat, and density. Boundary conditions also differ from structural analysis and include prescribed temperature, heat flux, convection, and radiation.

By temporal behavior, heat conduction analysis is classified into steady heat conduction, which determines a time-independent equilibrium state, and transient heat conduction, which follows the time evolution of the temperature field. The choice depends on whether the desired result is the equilibrium temperature ultimately reached or how temperature changes over time.

In the input, specify !SOLUTION, TYPE=HEAT, and use !HEAT to specify steady or transient analysis and the time step.

Thermo-Mechanical Coupled Analysis

Thermo-mechanical coupled analysis applies the temperature distribution obtained by heat conduction analysis as a thermal-strain load in structural analysis to determine stresses and deformation caused by the temperature field. The standard FrontISTR workflow is one-way coupling: thermal analysis and structural analysis are executed independently, and the temperature field is passed in one direction through a result file.

The procedure is first to perform heat conduction analysis and obtain a result file containing the temperature distribution. Then, when performing structural analysis, read that temperature field as a temperature load with !TEMPERATURE, READRESULT. The structural-analysis framework itself is the same as ordinary static or dynamic analysis, and no special analysis type needs to be specified for coupling.

Two-way coupling in which structural deformation affects heat conduction (for example, changes in thermal boundary conditions due to deformation) is outside the scope of this version of the documentation.