Define submodel constraint and solution (Abaqus)

Define a submodel constraint

1. Choose Home tab→Loads and Conditions group→Submodel Constraint .

2. In the Model Objects group, click Select Object and select the geometry or FE entity to which to apply the constraint.

3. In the Direction group, specify the displacement coordinate system to use.

4. Set the DOF values to Free, Fixed, or define a displacement value.

5. In the Submodel Boundary Parameters group, set the parameters for the submodel:To specify the amount by which a driven node of the submodel can lie outside the region of the elements of the global model, type a value in the Absolute Exterior Tolerance box. To specify the fraction of the average element size in the global model by which a driven node of the submodel can lie outside the region of the elements of the global model, type a value in the Exterior Tolerance box.To specify the step of the global model history that is to be used for the driven variables in the current submodel analysis step, type a value in the Step Number box. To specify the increment number of the global model history that is to be used for the driven variables in the current submodel analysis step, type a value in the Increment Number box.To specify the value by which the driven variables read from the global analysis are to be scaled, type a value in the Scale box.

6. If the submodel analysis step time is different from the global analysis step time, to scale the driven node's amplitude function to match the submodel analysis step time, select the Adjust the Time Variable for Driven Nodes Amplitude Functions check box.

Set up the submodel solution

1. In the Simulation Navigator, right-click the Simulation file, and choose New Solution.

2. In the Solution dialog box, set up the solution, either Structural or Dynamic Explicit.

3. In the Submodel tab, do the following:Select the Submodel check box. In the File Browser box, type the name of the results (.fil) or database (.odb) file containing the global results to drive the submodel analysis.

4. Click OK.

Learn more

Submodel constraint (Abaqus)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Define submodel constraint and solution (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 } });