Submodel constraint (Abaqus)

Use the Submodel Constraint command to perform node-based submodeling in the Abaqus environment. Submodeling lets you analyze a local area of a larger model. The software drives the submodel using the nodal results, such as displacements, from a global solution. You use the Submodel tab of the Solution dialog box to define the source of the global solution results. You can enter the name of the global results (.fil) or output database (.odb) file.

The options in the Submodel Constraint dialog box correspond to the Abaqus *SUBMODEL keyword. For more information, see:

• Submodeling in the Abaqus Analysis User's Guide

• *SUBMODEL in the Abaqus Keywords Reference Guide.

Example

In this example, to analyze a region near a concentrated load, two submodel constraints constrain the edge nodes. Results from the global analyses are interpolated to the two edges.

For the submodel constraint that constrains edge 1, the DOF values are:

• DOF1 = Free

• DOF2 = Fixed

• DOF3 = Free

• DOF4 = Fixed

• DOF5 = Free

• DOF6 = Fixed

For the submodel constraint that constrains edge 2, the DOF values are:

• DOF1 = Free

• DOF2 = Fixed

• DOF3 = Fixed

• DOF4 = Free

• DOF5 = Free

• DOF6 = Free

The boundary parameters for both constraints are:

• Exterior Tolerance = 0.05

• Step Number = 1

• Scale = 1

In the Submodel tab of the Solution dialog box, the global analysis associated with the submodel analysis is defined as:

• Submodel Analysis

• Name of the Global Model Results = pnchcyl_global.odb

Limitations

All submodel constraints in a given step must have the same global steps, increments, and scales. Therefore, the submodel boundary parameters, Step Number, Increment Number, and the Scale and Adjust the Time Variable for Driven Nodes Amplitude Functions check box, must be the same across all submodel constraints in a step. The solver does not issue a warning if the parameters are different and it generates an input file.

Note that parameters Absolute Exterior Tolerance and Exterior Tolerance can be different for submodel constraints because the solver writes them to a separate *SUBMODEL card with the associated node sets.

Where do I find it?

Application	Pre/Post
Prerequisite	A Simulation file as the work part and displayed partAbaqus as the specified solverStructural or Explicit Dynamic as the analysis type
Command Finder	Submodel Constraint

How do I

Define submodel constraint and solution (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Submodel constraint (Abaqus), 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 } });