Thermomechanical Simulation of Additive Manufacturing Processes

A sequential thermal-stress analysis of an additive manufacturing process consists of a transient heat transfer analysis of thermal loads introduced by the process on a printing part followed by a static structural analysis that is driven by the temperature field from the thermal analysis. The analysis can also include support structures (if required for the build) and a substrate where the part and support are built to consider their influences on thermal conduction, part distortions, and residual stresses.

For the heat transfer analysis, the following aspects of the process must be included in the simulation:

• Progressive material deposition: every additive manufacturing process adds new material with time.
• Progressive heating of the deposited material: for some additive manufacturing processes, the newly deposited layer of material gets heated up to the melting point, causing the material to fuse to an underlying layer or a substrate.
• Progressive cooling of the printing part: as a part is printed, its cooling surface is continuously evolving with time.

For the stress analysis,

• Temperatures from the heat transfer analysis are used to drive the stress analysis.
• Similar techniques of progressive material deposition as the heat transfer analysis can be used.
• Temperature-dependent material properties can be used for accurate stress results.

Progressive material deposition in additive manufacturing processes can be modeled using progressive element activation in Abaqus/Standard (see Progressive Element Activation). The parts and support structures can be activated progressively. During the analysis, any element that is defined as progressively activated is filled with material (completely or partially) or remains empty (inactive). You can control the activation and the volume fraction of the material for each element in each increment during an analysis with user subroutine UEPACTIVATIONVOL.

The material deposition sequence is defined in an event series (for example, in the form of time and spatial coordinates of a recoater sequence of events; see About Event Series for more details) and processed using user subroutine UEPACTIVATIONVOL to define how much material is added to an element in a given time increment. To simplify this process, you can access toolpath-mesh intersection utilities from within UEPACTIVATIONVOL to compute the change of the volume fraction of the material in each element and time increment taking into account the intersection of the finite element mesh with the specified event series data for material deposition (see Toolpath-Mesh Intersection Module). Optionally, you can update the material orientation to align it with the trajectory.

In addition, Abaqus/Standard provides a number of streamlined solutions for some of the most common additive manufacturing processes that do not require you to write user subroutines. These techniques are described in Special-Purpose Techniques for Additive Manufacturing.

With the deposition of new material during the additive manufacturing process, previously exposed material surfaces are covered, and new free surfaces are created with time. You can define surface convection and radiation on continuously evolving free surfaces (see Specifying Element-Based Film Conditions on Evolving Faces of an Element in Abaqus/Standard and Specifying Element-Based Radiation Conditions on Evolving Faces of an Element in Abaqus/Standard). Abaqus/Standard continually tracks the evolving free surfaces that reflect the current shape of a printing part at any given time in the build and applies film and radiation loadings only to those surfaces.

Many types of additive manufacturing processes involve the application of a moving heat source (laser, electron beam, welding torch, etc.) to fuse the raw material. You can define one or multiple nonuniform distributed heat sources in user subroutine UMDFLUX (see Defining Moving or Stationary Nonuniform Heat Flux in User Subroutine UMDFLUX).

The scanning path of a moving heat source is defined in an event series (for example, in the form of time, spatial coordinates and power of the heat source; see About Event Series for more details) and processed using user subroutine UMDFLUX to define each heating event that occurs on a given element in a given time increment. To simplify this process, you can access toolpath-mesh intersection utilities from within UMDFLUX to compute heat fluxes received by each element in each increment (see Toolpath-Mesh Intersection Module).

In addition, Abaqus/Standard provides a number of streamlined solutions to specify heat events that correspond to some of the most common heat sources in additive manufacturing processes that do not require you to write user subroutines. These techniques are described in Special-Purpose Techniques for Additive Manufacturing.

Additive manufacturing process simulation is a multiscale problem in both time and space. You can control the scale of the simulation and the solution fidelity by choosing an appropriate time incrementation and mesh size. In general, you can consider two types of simulation at different ends of the fidelity spectrum: process-level simulations (high fidelity) versus part-level simulations (lower fidelity).

A detailed process-level simulation is performed by using a small time increment and a fine mesh with at least one element per printing layer thickness and a few elements across an action zone where active melting or fusion occurs. The simulation captures the rapidly evolving temperature and high-temperature gradients typically found within and near action zones and, thus, provides accurate predictions for both residual stresses and distortions. You can specify temperature-dependent thermal and mechanical material properties. You can model thermal energy release and absorption during melting and solidification in heat transfer analyses using latent heat definitions (see Latent Heat). For processes that use metallic materials, you can also model annealing effects or melting at a certain temperature in stress analyses (see Annealing or Melting). In addition, precise simulations of temperature histories facilitate the modeling of material phase transformations and microstructure evolutions during printing, which can be achieved with user subroutines (such as UMAT, UMATHT or USDFLD). For example, you can specify material properties for different phases of materials (such as powder, liquid, or different solid-phases) as functions of field variables or solution-dependent variables representing the material phase and evaluated inside USDFLD as a function of the temperature history (see Specifying Field Variable Dependence and Specifying Material Data as Functions of Solution-Dependent Variables). A process-level simulation can model detailed physics of additive manufacturing processes and provide accurate results, but it typically has a high computational cost and can be affected by convergence difficulties due to the use of temperature-dependent nonlinear material properties under rapidly changing temperature conditions.

A part-level simulation is performed by appropriately averaging (lumping) the time sequence of events and using coarser meshes. For example, the model could have an element size that is a few times larger than the physical printing layer thickness and use only one or several time increments for printing one element layer. The heat transfer analysis can usually capture far-field temperature evolutions (away from action zones) as long as the thermal energy balance of progressive heating and cooling is modeled correctly. However, the simulation may not capture local rapid temperature evolutions properly because the specified sequence of concentrated, fast-moving heat sources is lumped over both time and space. In other words, the temperature results do not usually contain an accurate history of melting and solidification. In this case, to model the annealing or melting effects in the stress analysis correctly, you must assign an initial temperature representing a relaxation temperature above which thermal straining induces negligible thermal stress in the printing part. Upon element activation, the relaxation temperature is the temperature from which the initial thermal contraction occurs. This relaxation temperature can be calibrated from experiments or detailed process-level simulations. The part-level simulation is computationally efficient for the prediction of distortions and stresses in printing parts with reasonable accuracy.

Thermomechanical simulations of additive manufacturing processes are usually nonlinear due to temperature-dependent material behavior, progressive element activation, or other factors. Common convergence issues and recommendations on how to resolve them are discussed below.

In the heat transfer analysis, convergence difficulties are usually caused by the nonlinearity of material properties.

• If temperature-dependent conductivity is specified for the material, the system of equations is unsymmetric. In this case using the unsymmetric matrix storage and solution scheme (see Matrix Storage and Solution Scheme in Abaqus/Standard) may help to improve convergence.

• When latent heat effects are considered, they can introduce severe nonlinearity in the analysis and have a negative impact on convergence. Abaqus provides options to reduce the nonlinearity by specifying a smooth transition or extending the solidus-liquidus temperature interval (see Defining a Smooth Latent Heat Transition).

In the stress analysis, convergence difficulties can be encountered during the activation of elements.

• Elements may distort excessively before they are activated and cause convergence difficulties. In such situations you should specify that inactive elements follow the deformation to prevent excessive element distortion (see Controlling the Behavior of Inactive Elements).

• The initial thermal strain experienced by an element upon activation (due to the difference between the current temperature and the specified initial temperature) can lead to convergence difficulties that cannot be resolved by reducing the time increment. To overcome this issue, Abaqus provides an option to ramp the thermal strains over a period of time instead of applying them instantaneously upon activation (see Applying Initial Thermal Strains). Ramping thermal strains can influence the accuracy of the analysis results. For example, if the thermal strains of elements in a layer are not fully ramped when the next layer of elements is activated, the strain-free configuration of the newly activated elements is different from the case when thermal strains are fully ramped. You should use a ramping time constant smaller than the required time for processing one layer.

• If the material definition includes plasticity, the analysis may iterate excessively due to the extrapolation scheme used to speed up the solution. You can prevent this issue by turning off extrapolation (see Incrementation in Abaqus/Standard).