SOL 402 structural analysis with kinematics

Using SOL 402 Multi-Step Nonlinear Kinematics, you can define kinematic joints in your model to perform a structural analysis of an assembly that contains moving parts. This capability lets you solve complex models such as the ones found in aerostructures, helicopters, deployable structures in space, gas turbines, and machine tools.

A kinematic joint connects two nodes. You can create the kinematic joints from kinematic universal connections, or from 1D element connections.

• Creating universal connections is the recommend method for creating joints. Using a kinematic universal connection is quicker than creating 1D connections, and it is more automatic because the spider meshes are created for you. In addition, universal connections are solver independent. Thus, you can use the same model with different solvers. You do not need to recreate the connections. The universal connections are not exported to any solver. Only the mesh that you create (when you realize the universal connections) is exported. You can realize (mesh) kinematic universal connections into CJOINT and RBE2 or RBE3 Simcenter Nastran elements

• Creating 1D connections is the manual method for creating joints. The 1D connection consists of a CJOINT element and a set of physical properties (PJOINT and optionally PJOINT2) that define that joint. The CJOINT element is specific to the Simcenter Nastran solver.

If you want to use a joint multiple times in an assembly FEM file, create it once at the FEM or a subassembly AFEM level. Then duplicate this FEM or subassembly AFEM at the AFEM level.

For a complete list of the supported joints, see Kinematic joints for SOL 402.

Boundary conditions for kinematic joints

The following boundary conditions are specific to a kinematic analysis:

• To apply displacement, force, rotation, or torque to a joint, use the Kinematic Driver load.You can add the Kinematic Driver at the solution level or to Nonlinear Dynamics and Nonlinear Statics subcases.You can add the Kinematic Driver to revolute, inline, cylindrical, slider, and slider-universal joints.You can apply displacement or force to inline, cylindrical, slider, and slider-universal joints.You can apply rotation or torque to revolute and cylindrical joints.

• To specify the time at which you want to free or constrain a joint, use the Joint Time Constraint. If you need both types of constraints, you must first free the joint, and then constrain it using two different Joint Time Constraints.You can use the Joint Time Constraint at the solution level only. The joint time constraint applies to the entire solution, not to the subcases. You can free or constrain revolute, inline, cylindrical, slider, and slider-universal joints. You can free specified translational and/or rotational degrees of freedom for a fixed joint.

• To define a flexible slider joint, use the Flexible Slider simulation object. A flexible slider joint is similar to a slider joint except that the track is flexible and made of beam elements. The track can be curvilinear.You can use the Flexible Slider simulation object at the solution level only.You can use the Flexible Slider simulation object with different joint types depending on how you want to control the relative rotations of the nodes around the track: spherical, cylindrical, slider, or slider-universal.You can use a flexible slider joint, for example, to drive displacement of parts along beams, such as a model of a track.

Output requests for kinematic joints

To request the output for your kinematic analysis, use the following structural output requests:

• Joint ResultYou can request output for force, moment, displacement, angle, velocity, and angular velocity, or any combination of those. You can use the Joint Result output request with all joints.

• Flexible Slider ResultThe Flexible Slider Result outputs the relative displacement along the curvilinear abscissa for flexible slider joints.

To enable these output requests by default, use the Customer Defaults settings.

To set the number of maximum kinematic modes to include in the output, set Number of Kinematic Modes to Save as Output (NKINE) in the Nonlinear Control Parameters - Global dialog box.

Where do I find it?

Kinematic Driver load

Application	Pre/Post
Prerequisite	Simulation file as the work part and displayed partSimcenter Nastran as the specified solverStructural as the specified analysis typeSOL 402 Multi-Step Nonlinear Kinematics as the specified solution type
Command Finder	Kinematic Driver
Simulation Navigator	Right-click Load Container→New Load→Kinematic Driver

Joint Time Constraint constraint

Application	Pre/Post
Prerequisite	Simulation file as the work part and displayed partSimcenter Nastran as the specified solverStructural as the specified analysis typeSOL 402 Multi-Step Nonlinear Kinematics as the specified solution type
Command Finder	Joint Time Constraint
Simulation Navigator	Right-click Constraint Container→New Constraint→Joint Time Constraint

Flexible Slider simulation object

Application	Pre/Post
Prerequisite	Simulation file as the work part and displayed partSimcenter Nastran as the specified solverStructural as the specified analysis typeSOL 402 Multi-Step Nonlinear Kinematics as the specified solution type
Command Finder	Flexible Slider
Simulation Navigator	Right-click Simulation Object Container→New Simulation Object→Flexible Slider

Requesting output for a kinematic analysis

Application	Pre/Post
Prerequisite	Simcenter Nastran as the specified solverStructural as the specified analysis typeSOL 402 Multi-Step Nonlinear Kinematics as the specified solution type
Command Finder	Modeling Object
Location in dialog box	Modeling Objects Manager dialog box→Type list→Structural Output Requests→Create→Flexible Slider Result page→Enable FLXRESULTS Request Joint Result page→Enable JRESULTS Request

Setting output request customer defaults

Application	Pre/Post
Command Finder	Customer Defaults
Location in dialog box	Simulation→Pre/Post→Nastran→Output Requests tab:Flexible Slider Joint

Creating joints using the kinematic universal connection

Application	Pre/Post
Prerequisite	A FEM or assembly FEM file as the work part and displayed partSimcenter Nastran as the specified solverStructural as the specified analysis typeSOL 402 Multi-Step Nonlinear Kinematics as the specified solution type
Command Finder	Kinematic
Simulation Navigator	Right-click a FEM file→New Universal Connection→Kinematic
Location in dialog box	DOFs page→Connection Type list

How do I

Add joints to your kinematics model using universal connections

Create a flexible slider joint

Create and assign control nodes

Learn more

1D connection elements for kinematic joints

Kinematic Driver boundary condition

Joint Time Constraint boundary condition

Flexible slider joint

Control nodes

Look up more details

Kinematic joints for SOL 402

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

SOL 402 structural analysis with 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 } });