Progressive Element Activation

You can activate elements in each increment of a step. You must first define the elements that can be activated during an analysis and then refer to them in each analysis step in which they can be activated. Elements for which the activation feature is turned on in a step can be activated by assigning a volume fraction of material to an element at the beginning of each increment.

Both full and partial element activation are supported. For full activation the material volume fraction added must be equal to 0 or 1 (that is, the status of an element can change only from inactive to fully active). For partial activation the material volume fraction added can be arbitrary; however, in practice the volume fraction in an element should not be too small to prevent numerical singularity problems.

In stress-displacement analyses it is assumed that the material added to an element is stress free. Therefore, for full activation the configuration at which an element is activated is the stress-free configuration from which the strains used to compute the material response are measured. For partial activation the newly added material and the material already present are at different states. To obtain the material response, Abaqus/Standard uses the rule of mixtures to compute homogenized state variables.

Specifying Elements for 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.

Switching Off/On Progressive Element Activation in a Step

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

Activating Elements

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).

Controlling the Behavior of Inactive Elements

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.

Scaling the Material Properties of the Inactive Elements

When you specify that inactive elements should follow the deformation, all the elements in the model contribute to the response. However, you can scale the material properties of the inactive elements by specifying a preactivation coefficient. If the value of the scaling coefficient is sufficiently small, the contribution from the inactive elements does not markedly affect the solution and at the same time the elements follow the deformation and do not deform excessively. The default value of the preactivation coefficient is 10^–4.

Applying Initial Thermal Strains

When an element is activated, the initial thermal strains, $ϵ_{0}^{t h}$ , 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

ϵ^{t h} = {\begin{matrix} \frac{t - t_{a c t}}{τ_{t h}} ϵ_{0}^{t h}, & t_{a c t} \leq t \leq t_{a c t} + τ_{t h} \\ ϵ_{0}^{t h}, & t > t_{a c t} + τ_{t h} \end{matrix}

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

Applying Eigenstrains

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:

ϵ^{e i g} = {\begin{matrix} \frac{t - t_{a c t}}{τ_{e i g}} ϵ_{0}^{e i g}, & t_{a c t} \leq t \leq t_{a c t} + τ_{e i g} \\ ϵ_{0}^{e i g}, & t > t_{a c t} + τ_{e i g} \end{matrix},

where $ϵ^{e i g}$ is the eigenstrain applied, $ϵ_{0}^{e i g}$ is the value of the eigenstrain at the beginning of the increment at which the element is activated, $t_{a c t}$ is the activation time, and $τ_{e i g}$ is a user-specified time constant. The default value of $τ_{e i g}$ is zero.

Initial Configuration

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.

Procedures

Progressive element activation is supported only with the uncoupled heat transfer (see Uncoupled Heat Transfer Analysis) and static (see Static Stress Analysis) procedures.

Initial conditions

Abaqus allows the initial volume fraction of material in an element to be specified. In addition, the initial temperatures are handled in a special way when progressive element activation is used in an analysis.

Defining Initial Volume Fraction

You can specify the initial values of volume fraction for elements that can be progressively activated. The volume fraction must be equal to 0 or 1, which means that the element can be either inactive or fully active at the beginning of an analysis.

Initial Temperatures

In general, when elements are activated their state is set to the state at the beginning of the analysis. However, special handling is required for temperatures in a heat transfer analysis. In this case the temperatures at the integration points are interpolated from the nodal temperatures. Since inactive and active elements might share nodes, the nodal temperatures and, consequently, the temperatures at the integration points might be different from the specified initial values of the temperatures. In this case Abaqus generates a body heat flux at an integration point to compensate for this difference.

Boundary conditions

If you specify that inactive elements should follow the deformation, the boundary conditions are applied to inactive nodes (since the degrees of freedom at these nodes are part of the solution). Otherwise, the boundary conditions are not applied to the inactive nodes until the elements to which they belong are activated.

Loads

Loads are not applied when an element is inactive; however, they are applied as soon as an element is activated. The load magnitude at activation has the value corresponding to the time at activation, which means that the load magnitude can increase suddenly, what might cause convergence problems.

Elements

Progressive element activation is supported only for solid continuum elements and shell elements. However, for shell elements only full activation is supported. If a volume fraction of material smaller than one is assigned to a shell element, Abaqus automatically changes the value to one.

Output

In addition to the standard output identifiers available in Abaqus/Standard, the following variable has special meaning when progressive element activation is specified:

EACTIVE: Volume fraction of the material in the current element.
EEIG: All components of the eigenstrain.
UACT: All physical displacement components, including rotations at nodes with rotational degrees of freedom, measured from the time the node is activated.
URACT: All rotational displacement components measured from the time the node is activated.
UTACT: All translational displacement components measured from the time the node is activated.