Abaqus/Standard supports eigenstrain-based analysis of additive manufacturing processes through two
approaches: the pattern-based method and the trajectory-based method.
When you use the trajectory-based method, you define the tool path (for example, movement of
the laser spot) explicitly using an event series. Abaqus/Standard uses this event series to determine the time of activation of an element and the
eigenstrain to apply to the element at the time of its activation. Optionally, you can also
include the tool orientation and the dimensions of the deposition bead (height and width) in
the event series definition used to specify the tool trajectory.
When you use the pattern-based method, you define a scan pattern that represents an idealized
motion of the laser. Abaqus/Standard uses this scan pattern to determine the time of activation of an element and the
eigenstrain to assign to that element (see Scan Pattern–Mesh Intersection).
Specifying Element Activation and Eigenstrain Using the Pattern-Based Method
To use the pattern-based eigenstrain method, you must complete the following steps: :
Create a table collection with a name that
begins with "ABQ_EIG". The table collection must contain a
parameter table of type "ABQ_AM_EigenStrain_Method" as well as the other
parameter tables listed below.
Define parameters of rectangular patches that make up a rectangular unit cell (see Scan Pattern–Mesh Intersection), which is repeated to cover the cutting plane or a layer,
in a parameter table of type "ABQ_AM_EigenStrain_PatternBased_Define". You can
define the following parameters: a local angle, ; the extents of a patch and ; and a label of the parameter table defining an eigenstrain to apply to
this patch.
Alternatively, use a parameter table of type "ABQ_AM_EigenStrain_PatternBased_ScanStrategy_Define_Elset" to assign a
particular scan-pattern strategy directly to an element set. Element set–based
assignments of scan-pattern strategies have precedence over bounding box–based
assignments.
You can combine both assignment types under the same table collection.
Refer to the table collection in the
progressive element activation.
A dedicated collection of parameter table, property table, and event series types is
available to include all the definitions required by special-purpose techniques for additive
manufacturing. These special-purpose parameter table, property table, and event series type
definitions are generated internally. You need to explicitly include them in your model only
if you output the results of your additive manufacturing simulation in
SIM format. If needed, you can use the
abaqus fetch utility to obtain the file containing all the type
definitions of parameter tables, property tables, and event series required by the
special-purpose techniques for additive manufacturing as follows:
abaqus fetch job=ABQ_am_special_purpose_types.inp
Input File Usage
Use the following options to define scan pattern parameters and eigenstrains:
A scan pattern can be visualized over the part geometry by requesting element
solution-dependent field variables for output and plotting them as contours over the finite
element mesh. For a pattern-based eigenstrain analysis, the first two element
solution-dependent field variables are internally set to the patch
ID and scan region ID,
respectively (see Figure 1). For a trajectory-based eigenstrain analysis, the first
element solution-dependent field variable is internally set to the rule
ID.
Input File Usage
Use the following options to visualize a scan pattern:
The tool location and active strain definition as a function of time, a
time-dependent tool orientation, and time-dependent bead cross-section
dimensions
All event series types allow you to change the active eigenstrain
definition along the tool path, if needed. Using "0" for the active eigenstrain
definition rule has a special meaning and corresponds to turning the tool off. When the
tool is active (that is, it has a nonzero eigenstrain rule
ID), the tool direction cannot be parallel to the
event series segment.
You can include
multiple parameter tables of this type in the table collection, each defining a separate
set of components of the eigenstrain tensor. You must assign a unique label to each
table.
You must assign a unique label to
the scan rule, and you must list all the scan rules defined in the table collection in a
parameter table of type "ABQ_AM_EigenStrain_TrajectoryBased_Rules".
Figure 2. Position of the deposition bead relative to the tool path.
Abaqus/Standard assumes the eigenstrain components to be defined with respect to a local (orthonormal)
coordinate system , as shown in Figure 3.Figure 3. Local orientation along the tool trajectory when activating solid elements. For solid elements the local coordinate system follows the tool trajectory and depends
on the tool (build) orientation, such that
is along the current tool trajectory segment,
is computed based on the cross-product between the current tool
direction vector, , and (that is, ), and
is computed using .
For shell elements, a different local orientation is computed that depends on the average shell element normal, (and ), such that
For solid elements, if the material assigned to the elements to be activated
includes an initial orientation, Abaqus/Standard updates that orientation with the local orientation shown in Figure 3 at the moment of element activation; otherwise, Abaqus/Standard transforms the eigenstrain to the global coordinate directions. For shell elements, Abaqus/Standard cannot update the orientation; instead, Abaqus/Standard transforms the eigenstrain to the local shell orientation.
Input File Usage
Use the following options to define trajectory-based activation in an
eigenstrain-based analysis:
The eigenstrain-based simulation method for additive manufacturing does not support
material models with hyperelastic, hyperfoam, or low-density foam constitutive responses. If
elements assigned any of these material behaviors are activated during the analysis, Abaqus/Standard does not apply the eigenstrains defined in the model to those elements.