SOL 402 Multi-Step Nonlinear Kinematics

SOL 402 Multi-Step Nonlinear Kinematics is a structural analysis solution that supports large strains and large displacements, large rotations, and nonlinear materials. An example application for SOL 402 in the automotive industry is analyzing tires or engine mounts (hyperelastic materials). In the aerospace industry, an example application is analyzing vibration dampers between a rocket body and its boosters or composite panels. You can also use SOL 402 to perform a structural analysis of an assembly that contains moving parts. For information on using SOL 402 on models that contain moving parts, see SOL 402 structural analysis with kinematics.

At the subcase level, SOL 402 supports the following analysis types. You can define a combination of these analysis types within the same solution.

• Nonlinear static analysis

• Nonlinear dynamic analysis

• Normal modes, complex modes, cyclic modes, and Fourier normal modes

• Buckling modesNote: Buckling analysis can follow a static analysis but not a dynamic analysis.

• Bolt preload

For output, SOL 402 supports only SORT1 data.

SOL 402 Multi-Step Nonlinear Kinematics provides the same classical nonlinear features as SOL 401 Multi-Step Nonlinear but with the differences outlined in Simcenter Nastran Multi-Step Nonlinear User's Guide (SOL 401 and SOL 402).

Nonlinear control parameters

You can define the SOL 402 nonlinear control parameters at the solution and subcase levels.

• At the solution level, you set the solver type, matrix symmetry and stiffness, and whether you want to perform an initial static or steady-state computation.

• At the subcase level, you set parameters for time steps, iterations and convergence, integration scheme, load ramping, plasticity and creep effects, contact (to apply to all contact pairs), and the .f06 output file.

Geometric nonlinear effects

In addition to material nonlinearities, SOL 402 supports the following geometric nonlinearities:

• Large strains and large displacements

• Small strains and large displacements

The material and geometric nonlinearity parameters are global for all subcases. If material nonlinearity is turned on, plasticity and creep can be turned off at the subcase level.

Stress-strain measures and material nonlinearity

When you define a nonlinear material, you can enter hardening curves (stress-strain data) in a stress/strain table (assuming there is no temperature dependency). For the same material, you can use different inputs depending on the stress/strain measure type, which is commonly engineering or true. You can select the measure type when you define the material.

SOL 402 supports small strains and large strains, and the default stress-strain measure depends on whether your analysis is for small or large strains.

• If your analysis is for small strains (Large Strains (LGSTRN) check box is cleared), the default stress-strain measure is Biot Strain, Biot Stress (Engineering).No conversion is applied because in a small strain context, all the measures give approximately the same result.

• If your analysis is for large strains (Large Strains (LGSTRN) check box is selected), the default stress-strain measure is Log Strain, Cauchy Stress (True) and the hardening laws are assumed to be in that measure.If, however, you specify the hardening law in the Biot Strain, Biot Stress (Engineering) measure, a conversion of the law from engineering to true measure is performed in the solver, along with Young's modulus.

For more information, see SOL 401 and 402 - Stress-strain measures.

The recommended workflow for setting up your solution for stress-strain and material nonlinearity is as follows:

1. In the FEM file , select the material law and specify the appropriate stress-strain measure (engineering or true). You can select these in the following options in the material dialog boxes.Stress-Strain Input Data****Stress-Strain (H) (hardening curves table)Type of Nonlinearity (TYPE)

2. In the simulation file, set one of the following on the Solution dialog box, Parameters page:For small strains, clear the Large Strains (LGSTRN) check box.For large strains, select the Large Strains (LGSTRN) check box.

3. Solve the solution.Pre/Post writes the following to the input file:Stress-strain as it exists in the stress-strain tables. No conversion is done except for plastic stress-total strain (PLASTIC) to stress-plastic strain (PLSTRN) and vice versa.The MATS1 material stress dependence bulk entry with the STRMEAS field, which contains the measure of the hardening curve.

4. View the results in post-processing.Post-processing displays the measure of the results as follows:If your analysis is for small strains (Large Strains (LGSTRN) check box is cleared), the results are in engineering measure.If your analysis is for large strains (Large Strains (LGSTRN) check box is selected), the results are in true measure.Note: The following exceptions apply to beam and shell elements:For multi-layered shell elements, results are output in the Green Strain, PK2 Stress measure.For CBAR/CBEAM beam elements, results are output in the Green Strain, PK2 Stress measure.

If necessary, you can set the following advanced options by updating the Nonlinear Control Parameters - Global modeling object.

• To change the solver measure, set Stress-Strain Measure for All Material Laws (STRMEAS).

• To change the stress/strain output, set Output Label for Element Stress-Strain Measures (STROUT).

• To change the method used to convert the stress-strain curves, set Stress-Strain Conversion Method (STRCONV).

For information on these advanced options, see Advanced Parameters page (SOLs 401 and 402) / Additional Parameters tab (SOL 414) on the Nonlinear Control Parameters - Global dialog box.

Boundary conditions

SOL 402 supports the following boundary conditions:

• Loads — Mechanical (force, moment, gravity, pressure, bolt preload, and kinematic driver) and thermal (time independent or dependent, or external from another solution).

• Constraints — Single-point constraints and multi-point constraints, including joint time constraints for kinematic models.

• Simulation objects — Flexible sliders for kinematic models, surface-to-surface and edge-to-edge contact, surface-to-surface and edge-to-edge gluing, cyclic symmetry, coupling 3D cyclic symmetry and 2D axisymmetric components, protective layers (thermal barrier coating), material override, and report (displacement tracking).Note: Pre/Post does not support edge-to-surface gluing, but you can define edge-to-surface gluing in your Simcenter Nastran input file. Contact defined for use in SOL 402 cannot be used in other Simcenter Nastran solutions unless you modify the contact parameters modeling object.For information on coupling 3D cyclic symmetry and 2D axisymmetric components, see 2D axisymmetric and 3D cyclic symmetry analysis (SOL 402).For information on adding thermal barrier coatings, see Protective Layers.

Elements

SOL 402 supports the following elements:

• 0D elements: CELAS1, CELAS2, CMASS1, CMASS2, CDAMP1, CDAMP2

• 1D elements: CBAR, CBEAM, CROD, CONROD, and CJOINTFor information on the kinematic joint elements, see Kinematic joints (SOL 402).

• 2D elementsShell elements: CQUAD4, CQUAD8, CTRIA3, CTRIA6Plate elements: CQUADR, CTRIAR2D Plane Strain elements: CPLSTN3, CPLSTN4, CPLSTN6, CPLSTN82D Plane Stress elements: CPLSTS3, CPLSTS4, CPLSTS6, CPLSTS82D Axisymmetric (Fourier): CQUADX4, CQUADX8, CTRAX3, and CTRAX6

• 3D elementsCHEXA, CPYRAM, CTETRA, CPENTA3D Axisymmetric elements: CTRAX3, CTRAX6, CTRIAX, CQUADX4, CQUADX8, CQUADX3D Cohesive elements: CHEXCZ, CPENTCZ3D Rigid elements: RBAR, RBE2, RBE3

• Special element types: CBUSH, CONM1, CONM2, CBUSH1D, CGAP

Materials

SOL 402 supports user-defined materials (UMAT) and the following material behaviors (with optional temperature dependencies):

• Isotropic

• Orthotropic

• Anisotropic

• Hyperelastic

• Creep

• Ply failure

• Strain rate

• Material for cohesive elements

• Gasket

Subcase sequencing and time steps

SOL 402 supports sequentially dependent (SEQDEP) subcases. Sequential dependency causes a subcase to use the end state (displacement, stress, strain, and so on) from a specified subcase as its starting state. You can set the dependency to any subcase, including the first subcase. Setting the dependency to the first subcase is useful in restart solutions to ensure that the first subcase starts with the end state of the last specified subcase in the initial run solution. For more information, see the SEQDEP case control command.

You can control time steps in SOL 402 with the TSTEP or TSTEP1 bulk entries, but TSTEP1 is recommended. For more information, see the TSTEP1 bulk entry.

If your analysis includes modal subcases that are sequentially dependent to nonlinear subcases, you can control how the computed contact stiffness in the nonlinear subcase is applied to the sequentially dependent modal subcase. For more information, see Tangential Contact Stiffness in Linear Perturbation Subcase (KMODTN) in Nonlinear Control Parameters - Subcase dialog box (Simcenter Nastran SOLs 402 and 414,129).

Monitoring solves

While a SOL 402 is solving, you can monitor progress, request results, and stop the solution in the Solution Monitor.

• To view the status of the solve, click the following:Simcenter Nastran tab, which shows general status.SOL 402 tab, which shows the time steps and iterations.

• To view graphs of the solve progress, click Graphs . You can view the built-in graphs as well as nodal displacement graphs that you request using the Reports simulation object. You must request the nodal displacement graphs before you start the solve.

• To request intermediate results, click Get Results

• To stop a solve, click Stop .

Where do I find it?

Application	Pre/Post, Simcenter Nastran
Prerequisite	A Simulation file as the work part and displayed partSimcenter Nastran as the specified solverStructural as the specified analysis type
Command Finder	Solution
Simulation Navigator	Right-click the Simulation file→New Solution
Location in dialog box	Solution dialog box→Solution Type list

Learn more

SOL 401 Multi-Step Nonlinear

SOL 401 Multi-Step Nonlinear workflow

SOL 402 Multi-Step Nonlinear Kinematics workflow

Modeling thermal strain

Controlling plasticity and creep effects

Controlling the sequence of bolt pre-loads (SOL 401)

Element Add/Remove (SOL 401)

Simcenter Nastran SOL 401 Co-simulation with Simcenter STAR-CCM+

Complex modes analysis (SOL 402)

Displaying graphs in the Solution Monitor using the Report simulation object

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

SOL 402 Multi-Step Nonlinear Kinematics, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });