22.2.2 No compression or no tension

Abaqus Analysis User's Guide

22.2.2 No compression or no tension

Products: Abaqus/Standard Abaqus/CAE

Warning: Except when used with truss or beam elements, Abaqus/Standard does not form an exact material stiffness for this option. Therefore, the convergence can sometimes be slow.

References

Overview

The no compression and no tension elasticity models:

are used to modify the linear elasticity of the material so that compressive stress or tensile stress cannot be generated; and
can be used only in conjunction with an elasticity definition.

Defining the modified elastic behavior

The modified elastic behavior is obtained by first solving for the principal stresses assuming linear elasticity and then setting the appropriate principal stress values to zero. The associated stiffness matrix components will also be set to zero. These models are not history dependent: the directions in which the principal stresses are set to zero are recalculated at every iteration.

The no compression effect for a one-dimensional stress case such as a truss or a layer of a beam in a plane is illustrated in Figure 22.2.2–1. No compression and no tension definitions modify only the elastic response of the material.

Figure 22.2.2–1 A no compression elastic case with an imposed strain cycle.

Input File Usage:	Use one of the following options:
	NO COMPRESSION NO TENSION

Abaqus/CAE Usage:

Property module: material editor: MechanicalElasticityElastic: No compression or No tension

Stability

Using no compression or no tension elasticity can make a model unstable: convergence difficulties may occur. Sometimes these difficulties can be overcome by overlaying each element that uses the no compression (or no tension) model with another element that uses a small value of Young's modulus (small in comparison with the Young's modulus of the element using modified elasticity). This technique creates a small “artificial” stiffness, which can stabilize the model.

Material options

No compression and no tension definitions can be used only in conjunction with an elasticity definition. These definitions cannot be used with any other material option.

Elements

The no compression and no tension elasticity models can be used with any stress/displacement element in Abaqus/Standard. However, they cannot be used with shell elements or beam elements if section properties are pre-integrated using a general section definition.

Abaqus Analysis User's Guide