Eigenstrain-Based Simulation of Additive Manufacturing Processes

A trajectory-based eigenstrain analysis activates elements and applies eigenstrains based upon a specified trajectory of new material being fused or bonded to the underlying layer. For example, the trajectory of a powder bed fusion process is the same as the heat source scan path, and the trajectory for directed energy deposition and material extrusion processes is the nozzle path. The trajectory is defined using an event series (in the form of time, spatial coordinates, and user-defined data of events; see Event series for more details) and processed directly by the toolpath-mesh intersection module. In user subroutine UEPACTIVATIONVOL, you can call the relevant toolpath-mesh intersection utilities to obtain information about the change of volume fraction of material and the eigenstrain values to assign to each element in each increment. Optionally, you can update the material orientation to align it with the trajectory. The analysis is similar to the stress analysis in thermomechanical simulations, except that it is driven by eigenstrain loadings instead of temperature results for the thermal analysis.

A pattern-based eigenstrain analysis activates elements layer by layer and applies eigenstrain based on a specified in-plane eigenstrain pattern for each layer. An eigenstrain pattern is a domain that is partitioned by a "quilt" of one or more patches. Each patch is an area that contains a specific value of eigenstrains or a rotation angle of eigenstrains as a result of a specific trajectory in that area. For example, the eigenstrain patterns for powder bed fusion processes are related to the in-plane scan pattern of the heat source, and the eigenstrain patterns for directed energy deposition processes and material extrusion processes are related to the in-plane moving pattern of the nozzle. A pattern-based eigenstrain analysis does not require you to define a trajectory. The analysis considers layer-by-layer building sequences and ignores the detailed sequences of material deposition or scanning within layers. You define parameters and properties of eigenstrain patterns using table collections (see Table Collections, Parameter Tables, and Property Tables) and access them using user subroutine UEPACTIVATIONVOL. In the user subroutine you can activate elements in a layer-by-layer fashion, call the toolpath-mesh intersection utilities to identify which eigenstrain patch an element in the last activated layer belongs to, and apply the eigenstrains to the element. You can also update the material orientation, such as aligning it with the rotation angle of the eigenstrain of the patch.

Eigenstrain-based simulations in Abaqus/Standard are supported with full and partial element activation. In the case of partial element activation the volume fraction of material added can be arbitrary; however, in practice the value should be larger than a small threshold value to avoid numerical singularity problems. Full activation is a special case of partial activation when the volume fraction of material added is restricted to 1.0.

For partial activation, when new material is added in an increment, both the old and new material contribute to the stress response of the material. In general, the two materials might be in different states; therefore, the homogenized values of state variables are used to compute stresses. Abaqus homogenizes the variables using the rule of mixtures in which the variables are computed using the volume weighed average values. For example, for the linear elastic material model the response is computed from:

where

${\mathit{V}}^{\mathit{f}}$ is the volume fraction of the material in the element; and

${\epsilon }^{el}$ is the homogenized elastic strain.

In general, the new material is added with the eigenstrain prescribed. In this case the homogenized elastic strain is computed from the relation

where

$V_t^f$ is the volume fraction of the material in the element in the previous increment;

$\mathrm{\Delta }{\mathit{V}}^{\mathit{f}}$ is the volume fraction of the material added to the element ($\mathrm{\Delta }{\mathit{V}}^{\mathit{f}}={\mathit{V}}^{\mathit{f}}-V_t^f$);

$\mathrm{\Delta }\epsilon$ is the total strain increment;

$\mathrm{\Delta }{\epsilon }^{*}$ is the eigenstrain in the material added; and

${\epsilon }_t^{el}$ is the elastic strain at the end of the previous increment.

The configuration at which the new material is added is stress free only if no eigenstrain is prescribed. If the eigenstrain is specified, it causes a sudden increase of stress that does not decrease when the time increment is cut. This behavior can cause convergence difficulties, particularly when geometric nonlinearities are taken into account and nonlinear material models, such as the elastic-plastic model, are used. In such cases Abaqus provides the option of ramping up the eigenstrain linearly in the specified time interval (see Progressive Element Activation). However, you must use caution when choosing the ramping time value; it should be small relative to the analysis so that the results are not strongly affected.

When using progressive element activation in Abaqus/Standard, you can control the behavior of inactive elements to follow or not follow the deformation of active elements in the model (see Controlling the Behavior of Inactive Elements). The two behaviors are expected to produce similar results in the limit of small deformation, with the exception of displacements and rotations (U, UT, and UR).

An inactive element that follows the deformation, also referred to as a "quiet" element, is always present in the model and participates in the solution, but it produces a negligible contribution to the overall response. In this case a node attached to inactive elements can experience nonzero displacements before any of its attached elements are activated. The nodal output variables U, UT, and UR represent displacements and rotations measured from the beginning of an analysis, containing contributions of displacements during both inactive and active periods of a node. Abaqus/Standard also provides nodal output variables UACT, UTACT, and URACT corresponding to the displacements and rotations measured from the time when an element attached to the node is first activated.

An inactive element not following the deformation does not contribute to the stiffness of the model and does not participate in the solution. Any nodes attached to inactive elements remain in their initial position. In this case the nodal output variables UACT, UTACT, and URACT are the same as the output variables U, UT, and UR, respectively.

Regardless of the behavior chosen for inactive elements, the configuration of an element upon activation is usually different from the original configuration because nodes shared by active and inactive elements undergo displacements (see Initial Configuration). When an element becomes active, the configuration at the time of activation is the reference for subsequent element calculations. Therefore, the output variable E represents strains measured from the time an element is activated.

The time increment used in eigenstrain analyses can influence the final results. Assume that two eigenstrain analyses are performed to activate a row of elements using different time increments: a small time increment activating one element per increment and a large time increment activating two elements per increment. The initial configuration of every second element is different between the two analyses, leading to different results of residual stresses and distortions. You can choose an appropriate time increment for a trajectory-based eigenstrain analysis by performing a time stepping convergence study. For a pattern-based eigenstrain analysis, it is recommended that you use a time increment less than the time taken to process one element layer.