SOL 402 Multi-Step Nonlinear Kinematics workflow

Step	Summary	Detailed help topic
1.	Build the finite element (FE) model and Simulation file.	In Pre/Post, define the geometry, material properties, and meshes as you would for other structural solutions.	Create new FEM and Simulation filesMaterial typesMeshingBoundary conditions
2.	Create the Simcenter Nastran solution.	In the Solution dialog box, set the Analysis Type to Structural and the Solution Type to SOL 402 Multi-Step Nonlinear Kinematics.Note: If you plan to create kinematic joints using universal connections, you can create the Simulation file and solution after step 3.	Create or modify a solution
3.	If your model contains moving parts, create kinematic joint connections.	Create the kinematic joint connections between the components of your model using one of the following methods:Universal connections (recommended)1D connections (manual)If necessary, create a flexible slider joint in the Simulation file.Note: If you want to use a joint multiple times in an assembly FEM (AFEM) file, create the joint once at the FEM or subassembly FEM level. Then duplicate this FEM or subassembly FEM at the AFEM level.	Add joints to your kinematics model using universal connections1D connection elements for kinematic jointsFlexible slider jointCreate a flexible slider jointAssembly FEM file
4.	Create boundary conditions.	Create loads, constraints, simulation objects, and drivers (kinematics).If your model contains moving parts, you can use the following to drive or constrain a joint:Kinematic Driver****Joint Time ConstraintIn Pre/Post, SOL 402 supports surface-to-surface and edge-to-edge contact and glue simulation objects. Note: To define edge-to-surface gluing, you must edit your Simcenter Nastran input file before solving. Pre/Post does not export the edge-to-surface bulk entries.SOL 402 uses different contact parameters than other nonlinear solutions such as SOL 401 and SOL 601. Therefore, if you are using a model for which you previously defined contact, or you want to use this model with these other solutions, you must update the contact parameters modeling object.	Contact and glue conditionsSurface-to-Surface Contact (Simcenter Nastran, Simcenter 3D Multiphysics, Abaqus, ANSYS)Defining parameters for contact conditions (Simcenter Nastran)Contact modeling (Samcef documentation)Contact (Samcef documentation)BCTPAR2 (contact)Defining parameters for glue conditionsBGPARM (glue)Kinematic Driver dialog boxJoint Time Constraint dialog box
5.	Configure the solution parameters.	Determine whether you want to solve for large strains, large displacements, and material nonlinearities. On the Parameters page:To solve for large strains and/or large displacements, select the appropriate Large Strains and Large Displacements check boxes.To include plasticity effects, creep effects, damage material properties, and progressive ply failure in the solution, select the Material Nonlinearity check box.Note: You must also define the nonlinear materials.	Solution dialog box (Nastran), Parameters pageCreate a materialControlling plasticity and creep effectsNastran creep material properties
6.	Set the global nonlinear control parameters.	The Nonlinear Control Parameters - Global modeling object includes settings for the solver type, matrix symmetry, stress-strain measure, and computation state.	Solver-specific modeling objectsNonlinear Control Parameters - Global dialog box (Simcenter Nastran)
7.	Create subcases.	Select the analysis types, determine how you want to sequence the subcases, and define the time steps. For each subcase, you can define load ramping (LVAR) for time-unassigned loads, or temperature ramping (TVAR).	Create or modify a solution step or subcaseSolution Step/Subcase dialog box (Nastran)Subcase sequencingDefining solution time steps
8.	Set subcase-level nonlinear control parameters.	The Nonlinear Control Parameters - Subcase modeling object includes settings for analysis control (maximum displacement, rotation, and deformation; time-unassigned ramping; displacement prediction; and so on), disabling creep and plasticity effects, time integration, automatic time stepping, equilibrium iteration, convergence criteria, contact options, and so on.	Solver-specific modeling objectsNonlinear Control Parameters - Subcase dialog box (Simcenter Nastran SOLs 402 and 414,129)
9.	Request output for contact, glue, creep, strain, kinematic joints, and so on.	Create Structural Output Requests modeling objects. For example, in the Structural Output Requests dialog box:To request contact output, click the Contact Result page and select the Enable BCRESULTS Request check box.To request output for kinematic joints, click the Joint Result or Flexible Slider Result page and select the corresponding check box.	Requesting output for Nastran analysesStructural, FRF, and Thermal Output Requests dialog boxes (Nastran)
10.	Solve the model and view the progress of the solve.	The Solution Monitor displays information about the progress of the solve. You can use it to stop the solve, or you can request an intermediate results file.	Solve the modelSolution MonitorSimcenter Nastran graphs
11.	Review the .f06 results file.	The Simcenter Nastran .f06 output file contains time step entries for checking convergence; contact conditions; error, warning, and information messages; and all requested results. To locate the Simcenter Nastran .f06 file, right-click the solution and select Browse.	Convergence difficulties (Samcef documentation)
12.	Post process the results.	Use the Post-Processing Navigator and the Results tab to manage and view results. To view result curves for models with kinematic joint results, in the Post-Processing Navigator, expand the Graphs node.Note: If your model contains contact, set the deformed scale to 1.0. Otherwise, the results may show penetration between objects.If your model contains kinematic joints, set the deformed scale to 1.0 to see the true movement of the model.	Post-processingControl the display of deformation

Learn more

SOL 401 Multi-Step Nonlinear

SOL 401 Multi-Step Nonlinear workflow

SOL 402 Multi-Step Nonlinear Kinematics

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 workflow, 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 } });