Progressive Element Activation

You must first define the elements that can be used for activation in the model in the same way that you define regular elements. Then you must assign the elements to a specific progressive element activation feature.

ELEMENT PROGRESSIVE ACTIVATION, NAME=activation_name, ELSET=element_set_name

Elements that are assigned to a specific progressive element activation can be activated only in steps in which the feature is switched on.

ACTIVATE ELEMENTS, ACTIVATION=activation_name

To activate elements within a step, you must assign the volume fraction of the material to the element in user subroutine UEPACTIVATIONVOL, which is called at the beginning of each increment. If a table collection has been specified for this activation, the data from parameter tables can be accessed from the user subroutine (see Accessing Abaqus Table Collections).

By default, elements that are inactive do not contribute to the overall response of the model and their degrees of freedom are not part of the solution (except for degrees of freedom at nodes shared with active elements). In stress-displacement analyses this approach works only if displacements are relatively small. If this is not the case, the inactive elements may become excessively distorted before they are activated, which may cause convergence difficulties or produce poor results. In this case you can allow the inactive elements to follow the deformation, which prevents excessive element deformation.

ELEMENT PROGRESSIVE ACTIVATION, FOLLOW DEFORMATION=YES

ELEMENT PROGRESSIVE ACTIVATION, FOLLOW DEFORMATION=NO

When an element is activated, the initial thermal strains, ${ϵ}_0^{th}$, are computed with respect to the initial temperature. This might result in large values of strains applied instantaneously, which is equivalent to applying instantaneous loads. Such loads might cause convergence problems that will not be resolved by reducing the time increment. Abaqus avoids these convergence problems by specifying that thermal strains are ramped up by default instead of being applied instantaneously.

The initial thermal strains are ramped up over time according to the formula

where ${ϵ}^{th}$ is the thermal strain applied, ${ϵ}_0^{th}$ is the value of the thermal strain at the end of the increment at which the element is activated, $t_{act}$ is the activation time, and ${\tau }_{th}$ is a user-specified expansion time constant. The default value of ${\tau }_{th}$ is 2 times the initial time increment. Specifying ${\tau }_{th}$=0 causes the thermal strains to be applied instantaneously.

*ACTIVATE ELEMENTS, EXPANSION TIME CONSTANT=${\tau }_{th}$

Eigenstrain is a generic name given to inelastic strains such as thermal strain, plastic strain, phase transformation strain, and others. These strains can develop during various manufacturing processes such as welding, thermo-mechanical treatments, or additive manufacturing due to mechanical and thermal loads to which a material is subjected. If the distribution of these eigenstrains is known, it can be used to estimate the distortion and residual stresses in the body. In Abaqus, eigenstrains can be prescribed in user subroutine UEPACTIVATIONVOL to the new material that is added to an element. In addition, for solid elements the local orientation can be updated when the element is first activated.

As in the case of thermal strains, a sudden application of eigenstrains could lead to convergence problems. Therefore, Abaqus allows the eigenstrains to be ramped up linearly according to the formula:

where ${ϵ}^{eig}$ is the eigenstrain applied, ${ϵ}_0^{eig}$ is the value of the eigenstrain at the beginning of the increment at which the element is activated, $t_{act}$ is the activation time, and ${\tau }_{eig}$ is a user-specified time constant. The default value of ${\tau }_{eig}$ is zero.

*ACTIVATE ELEMENTS, EIGEN TIME CONSTANT=${\tau }_{eig}$

In a static analysis the position of the nodes that are shared by active and inactive elements in general will change before the elements are activated. In this case the configuration at the time of element activation is different from the original element configuration. This new configuration is assumed to be stress free, and the deformation from this configuration determines the stress in the element.