Element progressive activation

Element progressive activation:

  • can be used to activate elements during an analysis;

  • can be used only with solid elements; and

  • can be used only in heat transfer or static analyses.

The following topics are discussed:

Related Topics
In Other Guides
*ACTIVATE ELEMENTS
*ELEMENT PROGRESSIVE ACTIVATION
UEPACTIVATIONVOL
Accessing Abaqus table collections

ProductsAbaqus/Standard

Element progressive 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 in the element at the beginning of each increment. Elements cannot be partially activated; therefore, the material volume fraction added that you specify must be equal to zero or one, which means that the status of the element can change only from inactive to fully active.

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 element progressive activation feature.

Input File Usage

Use the following option to define elements that can be activated during an analysis:

ELEMENT PROGRESSIVE ACTIVATION, NAME=activation_name, ELSET=element_set_name

Switching off/on element progressive activation in a step

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

Input File Usage

Use the following option to switch on element progressive activation is a step and optionally specify the table collection name:

ACTIVATE ELEMENTS, ACTIVATION=activation_name

By default, element progressive activation is switched off in the step. You can repeat the option in each step as many times as necessary to turn on multiple activations.

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). Only full activation of elements is supported; therefore, the volume fraction of material must be either zero for inactive elements or one for active elements.

Procedures

Element progressive activation is supported only with the uncoupled heat transfer (see Uncoupled heat transfer analysis) and static (see Static stress analysis) procedures.

Initial conditions

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 temperatures at the beginning of the analysis. In this case Abaqus generates a body heat flux at an integration point to compensate for this difference. 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 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 will determine the stress in the element.

Boundary conditions

The boundary conditions can be specified on inactivate elements; however, they are not applied until the element is activated. If nonzero displacement boundary conditions are specified on nodes of inactive elements in a static analysis, they are applied at the time of element activation and they will determine the new stress free configuration of the element.

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, which might result in convergence problems.

Elements

Element progressive activation is supported only for solid continuum elements.

Constraints

Specifying constraints on elements activated during an analysis may cause convergence problem if the nodes involved in the same constraint definition belong to elements that are not activated at the same time. In general, defining constraints in such cases should be avoided.

Output

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

EACTIVE
Volume fraction of the material in the current element.