Initial stress (LS-DYNA)

Use the Initial Stress command to preload a cross section of solid elements to a prescribed stress value. The software applies the preload stress values normal to the cross section using a loading curve that defines the stress values over time. For example, you can use the Initial Stress command to define preload stress values for a set of bolts that clamp together two sheet metal parts.

You can use options in the Initial Stress dialog box to specify:

• The cross section that defines the set of elements to which to apply the stress.

• The load curve that defines the preload stress over time.

• Options, such as whether shear and bending stresses are allowed to develop during the time that the curve is acting to prescribe normal stress.

The Initial Stress command corresponds to the LS-DYNA *INITIAL_STRESS_SECTION keyword.

Supported elements and materials for initial stresses

You can use the Initial Stress command to apply initial stress values to certain types of solid elements that are assigned certain material types. You can apply initial stress values to elements with:

• Solid element types 1, 2, 3, 4, 9, 10, 13, 15, 16, 17, and 18 only. ALE elements are not supported.

• Assigned materials that the software incrementally updates during the solve, such as elastic, viscoelastic, and elastoplastic materials.

Defining the cross section

You must create a Cross-Section Region type of Region to define the physical location of the cross section. LS-DYNA uses the Cross-Section Region to determine the resultant forces to write to the ASCII secforc file during the solve. LS-DYNA requires that a cross section consist of the nodes that define the cutting surface of the plane and the deformable elements to one side of that plane that also touch that cutting surface. The physical property tables that you specify in the Initial Stress dialog box together with the elements associated with the cross section identify the elements that are subject to the prescribed preload stress.

You can use options in the Region dialog box to define the planar cross section. The cross section:

• Can be rectangular or circular.

• Should cut through deformable elements only and not through rigid bodies.

The Cross-Section Region type of Region corresponds to the *DATABASE_CROSS_SECTION_PLANE keyword.

Defining the load curve for the stress values

You can create a DEFINE_CURVE modeling object to specify how the software should apply the stress values to the Cross-Section Region over time. Typically:

• You define the data with a ramp function, starting at the origin, to increase the stress to the desired value. The time duration of the ramp should produce a quasi-static response. When the end of the load curve is reached, or when the value of the load decreases from its maximum value, the initialization stops. If you do not use a ramp function and simply begin the load curve at the desired stress value, the solution can take longer to converge.

• You select the (1) Dynamic Relaxation option from the Load curve used in (SDIR) list to apply the preload during the dynamic relaxation phase of the analysis.

For more information, see Defining XY data for LS-DYNA solutions.

Defining shear and bending stress options

You can use options in the Initial Stress dialog box to

• Use the Shear Stress Flag option to control whether you want to allow shear stresses and bending stresses to develop during the initialization phase of the analysis.

• Use the Artificial Stiffness option to simulate additional linearly elastic ghost elements in the cross section. These elements prevent mesh distortion by adding stiffness to the structure.

Where do I find it?

Application	Pre/Post
Prerequisite	An active Simulation file with LS-DYNA as the specified solver
Command Finder	Initial Stress

Learn more

Contact interference (Abaqus)

Constrained keywords for rigid body creation (LS-DYNA)

Enforced acceleration constraint (ANSYS)

Fixed and free boundary degrees of freedom (Nastran, ANSYS, and Abaqus)

Initial forces on beam element axes (LS-DYNA)

Initial velocity (LS-DYNA)

Rigid wall definition (LS-DYNA)

Single point constraints for boundary nodes (LS-DYNA)

Enforced velocity constraint (ANSYS)

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Initial stress (LS-DYNA), 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 } });