Add joints to your kinematics model using universal connections

This procedure uses universal connections to create kinematic joints in your model for a SOL 402 Multi-Step Nonlinear Kinematics analysis.

1. Make the FEM or assembly FEM file the work part and the displayed part.

2. Choose Home tab→Universal Connections group→Kinematic .

3. In the Kinematic Connection dialog box, complete the following pages to identify the joint type, set its coordinate system, and so on. To name the joint and create or select a folder to store it in the Simulation Navigator, use the General page.To select the point or spider targets that will be connected by the joint, use the Targets page.For joints, Target 1 is linked to node 1 of the joint, and Target 2 is linked to node 2. For multipoint constraints (MPC), Target 1 is the dependent degrees of freedom and Target 2 is the independent degrees of freedom.To select the coordinate system for the joint, use the Axis Type page. To select the joint type, use the DOFs page.To add friction to the joint, use the Physicals page.Note: If you realize (mesh) the kinematic connection using CJOINT+RBE2 spider(s) or CJOINT+RBE3 spider(s), the values you enter are added to the PJOINT physical property table.If you plan to realize (mesh) the kinematic connection using MPC+RBE2 spider(s), the friction information does not apply because it is not exported to the solver. For information, see Kinematic / Rigid Connection dialog box.

4. Click OK to create the connection.The connection appears in the Universal Connections container in the folder that you designated. Its status is Not realized, which indicates that the connection is not meshed yet.

5. Right-click the Universal Connections container and choose Automatic Connection Elements.Note: The Automatic Connection Elements command lets you realize all of your kinematic joints with the same elements. If you want to use different elements for some joints, use the Connection Elements command to mesh the joints individually.

6. In the Automatic Connection Elements dialog box, make sure that the Kinematic Connection check box is selected, and from the list, select how you want to mesh the connection, and then click OK.To connect the two targets with a kinematic joint, select CJOINT+RBE2 spider(s) or CJOINT+RBE3 spider(s).Note: When you realize a kinematic joint universal connection with CJOINT+RBE3, the six degrees of freedom of the leg nodes drive only the translation of the core node. This can lead to problems when you connect shell elements to a joint using RBE3. To avoid the problems, set the three rotational degrees of freedom of the core node to On. You can set the core node and leg node degrees of freedom in the mesh associated data for the RBE3 meshes.The status is now Up-to-date, and the 1D Collectors container is added or updated with two solver-specific collectors:Cjoint Collector, which contains the meshed kinematic connection. For a description of CJOINT and the PJOINT physical property tables, see 1D connection elements for kinematic joints. To view a description of how the kinematic connection information is represented in the Simcenter Nastran element, right-click the kinematic connection and choose Information.RBE2 Collector or RBE3 Collector, which contains the spider elements for the meshed kinematic connection.

7. (Optional) For CJOINT elements, add additional friction, spring, and damping.Note: If you added friction to the kinematic universal connection, the Friction Coefficient and Tightening Force for Friction Calculation values are automatically added to the PJOINT physical property table.Right-click the Cjoint Collector and choose Edit.In the Mesh Collector dialog box, for the Cjoint Property, click Edit .In the PJOINT dialog box, add friction, stiffness, and damping as explained in PJOINT dialog box.Note: If you change the Joint Type and then later update and realize the kinematic universal connections, the original value for Joint Type is restored.Click OK.

8. (Optional) Create a control node for the CJOINT element.For more information, see Control nodes and Create and assign control nodes.

9. To add boundary conditions to the joints, do the following:Make the Simulation file the work part and displayed part.Create the following as necessary for your model:To create a driver, choose Home tab→Loads and Conditions group→Load Type→Kinematic Driver and complete the Kinematic Driver dialog box.To free (move) or constrain (fix) a joint, choose Home tab→Loads and Conditions group→Constraint Type→Joint Time Constraint and complete the Joint Time Constraint dialog box.If you realized (meshed) the connection using MPC+RBE2 spider(s), do the following:Choose Home tab→Loads and Conditions group→Constraint Type→Manual Coupling.In the Manual Couplingdialog box, from the Type list, select Multi MPC.In the Simulation Navigator, click 1D Collectors→Constraint Equation Collector→Kinematic mesh.Click OK.

10. To request output, do the following:Choose Home tab→Properties group→Modeling Objects .In the Modeling Objects Manager dialog box, from the Type list, select Structural Output Requests and click Create.On the Structural Output Requests dialog box, click the Joint Result page and complete the dialog box as explained in Structural, FRF, and Thermal Output Requests dialog boxes (Nastran).

11. If you are using a joint multiple times in an assembly FEM file, duplicate the FEM or subassembly FEM at the AFEM level wherever the joint is needed.For more information, see Assembly FEM file.

12. Make sure that boundary conditions and output requests are added to your solution, and solve it as you usually do.For information on monitoring the solve progress, see Solution Monitor and Simcenter Nastran graphs.

How do I

Create a flexible slider joint

Create and assign control nodes

Learn more

SOL 402 structural analysis with kinematics

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

Add joints to your kinematics model using universal connections, 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 } });