With Abaqus, different physical domains can be coupled with each other. In addition to the pure structural-mechanical analysis of components using static or dynamic stress analysis, electromagnetic phenomena can also be simulated. These can be coupled using a suitable coupled procedure or co-simulation. The co-simulation solution technique uses a segregated solution approach in which the multiphysics or multiscale problem is divided into two or more subsystems, with each subsystem solved independently and the solution data exchanged as the analysis progresses. An Abaqus analysis can be coupled with another Abaqus analysis or with another analysis program to solve multiphysics and multiscale simulations. This blog post will focus on how to set up an electromagnetic-structural analysis with a suitable procedure in Abaqus.
In general, there are three different types of simulations to couple together as part of a co-simulation. The first is the "uncoupled analysis" (see Fig. 1). It can be simulated using a mapping strategy where the results from one analysis are used as a starting value for another analysis. In our case, an electromagnetic analysis would be carried out first and the result would then be used as input for a structural analysis. The second variant is the "sequentially coupled analysis" (see Fig. 1). In this case, the two simulations are coupled in such a way that the electromagnetic forces of each time step have an influence on the stress analysis of the next time step. The third variant is the "fully coupled analysis" (see Fig. 1). This analysis is a simulation in which both the electromagnetic forces and the voltage influence each other.
Figure 1: The three different types of coupled simulation (1)
The topic of "coupled simulation" is used in various fields such as fluid-structure analysis (simulation of transverse flow induction heating), electromagnetic-mechanical analysis (simulation of magnetic impulse deformation), thermal-electrical-mechanical analysis (heat transfer analysis of a socket). An article has been published on the subject of "thermal-electrical-mechanical analysis" (2). In our contribution, we will focus on the "EM-mechanical analysis", which we consider to be a sequentially coupled analysis.
An electromagnetic to transient implicit dynamic analysis is useful for applications such as electromagnetic reshaping, where the Lorentz body forces from an electromagnetic analysis drive a transient dynamic analysis. Co-simulation between a transient electromagnetic analysis and a static or transient implicit dynamic analysis is supported. In this case, the coupling is only one-sided, i.e. the effects of the deformation of parts of the domain on the electromagnetic fields are not taken into account. Therefore, such an analysis should only be used if the effects of the deformation on the electromagnetic fields are small (3).
Electromagnetic forming is mainly used to stretch, compress or shape tubular components. Occasionally, it is also used to form flat sheet metal. These three different types of electromagnetic forming - expansion, compression and flat coil - are shown in Figure 2. The process is a high-speed forming process in which electromagnetic forces are used to deform the workpieces. It can be used, for example, to punch holes or to form thin-walled components such as pipes. The forces required for forming and punching are generated by the electromagnetic interaction between the coil and the workpiece. The component, e.g. a tube, is deformed depending on the shape of the core.
Figure 2: The three different types of magnetic pulse forming (4)
The described co-simulation is carried out according to the workflow shown in Figure 3.
Figure 3: The workflow of this co-simulation
In the following, we consider an aluminum tube in an electromagnetic simulation that is deformed with a steel core in a structural analysis. The electromagnetic simulation model consists of three parts (surrounding space, coil and aluminum tube), while the mechanical analysis model consists of two parts (aluminum tube and core), which are shown in Fig. 4.
In these analyses, the two physical phenomena of magnetism and mechanics are coupled together. In the electromagnetic simulation, the magnetic field is generated by the current flow in the coil, which creates magnetic forces. These forces are used in the second simulation to compress or deform the aluminum tube. The following steps must be followed to set up the models.
In the first step, the components for the simulation are created, positioned and assigned suitable material properties. The thickness of the aluminum tube for this process is typically between 0.1 mm and 3 mm. For the electromagnetic simulation, a simulation space is defined as "air" to analyze the propagation of the magnetic field during the simulation. In addition, a coil for the flowing current and the aluminum tube are modeled (see Fig. 4). For this purpose, the "magnetic permeability" and the "electrical conductivity" are taken into account. For the mechanical simulation, only the aluminum tube and the steel core are modeled. The "elastic and plastic behavior" of the materials is modeled.
Figure 4: The components for the electromagnetic and mechanical simulation
Before entering the parameters in Abaqus, a uniform system of units should be defined. The unit system "mm-t-s" is chosen for this analysis. In our model, the isotropic material copper is defined based on the material properties from the literature.
Linear elements with electromagnetic degrees of freedom (EMC3D8) are used for the meshing strategy of the electromagnetic simulation. Linear elements with mechanical degrees of freedom (C3D8) are used in the mechanical simulation.
Three procedures were implemented in Abaqus for the EM simulations:
In this case, the procedure "Low Frequency Transient Eddy Current Analysis" is used. This procedure is supported by keywords in Abaqus. However, only the "Low Frequency Time Harmonic Eddy Current" step is available in Abaqus CAE. The customized keyword should look like this:
*Step, name=Electromagnetic
*Electromagnetic, low frequency, transient, STABILIZATION=100
The stabilization is used to control singularities, as the formulation of the magnetic vector potential in the Maxwell equation can lead to singularities. The maximum value for stabilization is 100, which is used in this case. There are various options for the electrical load in Abaqus. In this case, the current is applied as a "body current" with suitable boundary conditions for the EM simulation. Extremely high currents flow through the coil during the process, as it is a high-speed forming process that requires strong magnetic forces. The current strength depends on the specific requirements of the process, such as the size of the workpiece, the type of material and the desired deformation. The peak current is typically between 50,000 and 1,000,000 amperes. Suitable mechanical boundary conditions are also defined for the mechanical analysis in order to ensure the static determinacy of the model.
An identical element-based region is defined for both simulations and its behavior is investigated. This is supported in Abaqus by the keyword "*CO-SIMULATION REGION". In this case, the aluminum tube is the co-simulation region. In addition, the region is defined depending on the field variables by specifying which variables are imported or exported in which analysis. Here, the electromagnetic forces are exported from the EM simulation and imported as mechanical forces in the structural analysis. The customized keyword should look like this:
The appropriate coupling scheme is defined for the next step. The coupling step determines the frequency of exchange between the analyses in a co-simulation and directly influences the stability and accuracy of the coupled solution. The size of the coupling step is defined at the beginning of each coupling step and is used to calculate the next target time point. For this purpose, the "increment size" and the "negotiation scheme" must be defined. The SIMULIA Co-Simulation Engine is used to determine the increment size and the negotiation scheme.
There are two methods for determining the increment size. One method is called "subcycling" or automatic method. Depending on the process, Abaqus can adjust the increment size. For non-linear events that require a reduction in the increment size, subcycling allows Abaqus to reduce the increment size. The other method is "Lockstep". In this case, Abaqus can be forced to use a fixed time step size. This allows both solvers to use the same time step size and avoid interpolation of quantities during the coupling step. However, with lockstep, Abaqus is not able to reduce the time increment to resolve non-linear events and terminates the simulation in these cases.
The SIMULIA co-simulation engine offers several negotiation methods, such as "Constant Coupling Step Size", "Minimum Coupling Step Size", "Maximum Coupling Step Size", "Having a Solver Dictate the Coupling Step Size" and "Constant Multiple". Detailed explanations can be found in the Abaqus online documentation (5). In this case, "Constant Multiple" is used. With this method, the coupling step size is determined by the solver, in addition to the step size preferred by the user.
To start a co-simulation, a configuration file is required to couple the two simulations together. Both input files must be created and saved for this purpose. The configuration file is written as an .xml file. This .xml file can be either detailed or simplified. Typically, a simplified version of the file is used when two procedures are linked together within Abaqus to prevent the user from making unnecessary changes. The detailed .xml file, on the other hand, is used when an Abaqus solver is to be linked to another program. The fetch function (abaqus fetch job=exa_em_std_export) can be used to create a pattern for the .xml file. The .xml file is written as follows:
Then the co-simulation is started by the following command window:
abaqus cosimulation job=em_job_name,st_job_name cosimjob=Co-simulation_job_name config=config_name
Here, "em_job_name" is replaced by the name of the EM simulation and "st_job_name" by the name of the structure simulation. The name of the co-simulation task is defined as "co-simulation_job_name" and the configuration file has the name "config_name".
After running the simulations, the outputs such as the magnetic flux density (EMB) and the magnetic forces of the body in conducting regions (EMBF) are analyzed vectorially from the EM simulation. EMB shows the magnetic field in the defined environment as vectors, while EMBF shows the magnetic forces in the aluminum tube as vectors (see Fig. 5). The EMBF output has the unit of 𝐹𝑇-1𝐿-3 in the selected unit system. This output is imported in the structural analysis as input CF, which has the unit 𝐹 in the same system of units. The unit conversion is carried out easily by the detailed configuration file so that the user does not have to make any manual adjustments in this case.
Figure 5: Two important outputs of the EM simulation; a) EMB, b) EMBF
Next, the deformation of the aluminum tube is considered in the mechanical simulation. Depending on the shape of the core, the aluminum tube is deformed. The stress of the tube will increase considerably (see Fig. 6). The mechanical forces are shown in Figure 7.
Figure 6: Two important outputs of structural analysis; a) deformation, b) stress
Figure 7: CF from the structural analysis of two different views
In Abaqus, different physical domains can be coupled with each other. As an example, a coupling of electromagnetic and mechanical simulation was considered in this blog. A magnetic pipe deformation was used as a model for this. Both simulations illustrate how a thin aluminum tube is quickly deformed by an electromagnetic field. In this high-speed forming process, high currents of between 50 kA and 1 MA flow through the coil, generating a magnetic field. The tube can be severely deformed and the stress of the tube can increase up to 67,360 GPa. The EM simulation can also be carried out with another program for a more detailed analysis and then coupled with Abaqus.