Advanced Simulation
Abaqus offers the possibility to couple different physical domains with each other. In addition to the pure structural-mechanical analysis of components using static or dynamic stress analysis, thermal simulations and electrical phenomena can also be simulated. This can be done using a suitable coupled procedure or co-simulation. This blog post is about setting up a thermal-electrical-mechanical multiphysics simulation with a suitable procedure in Abaqus.
Types of coupled multiphysics simulation
In general, there are three types of these simulations. The first is the "uncoupled analysis" (see Fig. 1). It can be simulated with a mapping strategy or as a single heat transfer analysis. In this case, a single thermal analysis can be performed and the result subsequently used as input for a structural analysis. The second variant is the "sequentially coupled analysis" (see Fig. 1). With this type of coupling, a thermal deformation analysis, a thermal-electrical analysis or a thermal-electrical-mechanical analysis can be performed. In this case, it can be simulated so that the temperature of each time step has an influence on the stress analysis of the next time step. An article on magnetic deformation has been published on the subject of "sequentially coupled analysis" (Source 1). The third variant is the "fully coupled analysis" (see Fig. 1). This analysis is a simulation in which both the temperature and the stress influence each other.
a) uncoupled analysis
b) Sequentially coupled analysis
c) Fully coupled analysis
Figure 1: The three different types of coupled simulation [1]
Heat transfer with a relevant example in Abaqus
One of the most important goals of thermal-electrical-mechanical simulation is to calculate the temperature change due to electric current.
Heat transfer distinguishes between three types of heat flow: "conduction", "convection" and "radiation". Conduction is the transfer of heat energy in solids or stationary liquids through molecular interactions (see Fig. 2). Convection is the transfer of thermal energy between a surface and a moving fluid (see Fig. 2). Radiation is the transfer of thermal energy through media or vacuum by means of electromagnetic waves (see Fig. 2).
a) Conduction
b) Convection
c) Radiation
Figure 2: Three types of heat transfer
A simple plug or flat plug is considered below. This serves as an illustrative example of a classic plug/socket connection, see Fig. 3. The simple model of a flat plug consists of two parts - the pin and the plug (see Fig. 4). The red dot on the plug indicates the measuring point of the temperature of the plug, which is used to calculate the minimum step size. This is explained in more detail in the next section.
Figure 3: A schematic representation of the socket and the plug
Figure 4: A simple model of a flat plug
In this model, the three physical phenomena of heat transfer, mechanics and electrical conduction come together. In the first step, the mechanics are considered by inserting the flat plug. Subsequently, current is applied and the extent to which the plug heats up is investigated.
The following points are to be implemented for the construction of the model:
1. Thermal, electrical and mechanical material properties
Depending on the procedure, material properties are defined. For example, "density" and "specific heat" must be specified for transient processes. For this simulation, "density", "elastic behavior", "specific heat", "thermal-electrical conductivity" and "Joule heat content" are used. The specific heat capacity indicates the amount of heat that must be added to a substance per unit mass in order to increase the temperature by one Kelvin. This must be defined in a transient analysis. The Joule heat fraction is used to indicate the proportion of dissipated electrical energy that is released as heat in thermal-electrical coupled problems. It is an optional parameter with a default value of 1.
Before entering the parameter, a uniform system of units should be selected, which is listed in Table 1. The unit system "mm-t-s" is selected for our analysis. In our model, the isotropic material copper was selected according to the material properties of the literature values.
Table 1: The selected system of units in Abaqus/CAE
2. The meshing and procedure of the model
After defining the material properties, the components should be meshed. Linear brick elements with thermal, electrical and mechanical degrees of freedom (Q3D8) were used for the meshing.
Models that take thermal degrees of freedom into account can be simulated as transient or stationary. In the transient simulation, the temporal course of the temperature change is calculated, while the stationary simulation represents the final temperature course that occurs after a long period of time. Both cases are examined below. Each of the simulations consists of two "steps". The first simulates the movement of the pin and the resulting mechanical load. For this step, the procedure "static general" or "thermal-electrical-structural" can be used. The second step calculates the thermal-electrical effect. For this step, "thermal-electrical-structural" was used.
One of the parameters entered for the procedure is the minimum increment size. For transient heat conduction problems, it is important that the time increment is not too small in order to avoid instabilities. This time increment depends on the mesh fineness and is calculated using the following formula:
Where p is the density, c is the specific heat, Δl is the distance between the nodes of the element near the surface with the highest temperature (Fig. 5) and k is the thermal conductivity.
Figure 5: The distance between the nodal points of the element near the surface with the highest temperature gradient
3. Contact surfaces and the heat transfer to the environment
Interactions must be defined for this simulation. One of the interactions of this model refers to the contacted surfaces. Here, either the "general contact" or a "contact-pairs" contact between surfaces or nodes can be defined. In this simulation, the surface contact option is selected. In this case, the contact surfaces have no friction and should have thermal-electrical properties. The properties of the contact surfaces are listed in Table 2.
Table 2: The literature values of interaction properties of the model
The other interaction of this model relates to convection between the environment and the components. For heat transfer to the environment, any surfaces should be selected and suitable properties defined. The properties are listed in Table 4.
Table 3: Literature values of convection properties with the environment
Convection with the environment should be defined as "surface film condition". The setting is shown in Fig. 6. For the coupled thermal-electrical-mechanical step, the amplitude should be defined as "instantaneous" (see Fig. 7) for the "sink temperature", as the temperature of the parts decreases with the change of the steps.
Figure 6: The surface film state of pin and connector
Figure 7: The amplitude for the "sink temperature" as a tabular amplitude
To make the model realistic, the initial temperature should be set as the ambient temperature. This is defined under "Predefined Field" and is 25°C (see Fig. 8).
Figure 8: The initial temperature as ambient temperature
Analysis of the simulation results
To check the validity of our model, we first examined the current through the cross-section of the component. For this reason, "SOE" - total current through the section - must be selected as the "history output". To analyze the SOE, "integrated output section" must be defined. If the radiation properties play a role in the simulation, the arbitrary surface for the integrated output section should not have any radiation properties. SOE is not available in Abaqus/CAE for the coupled thermal-electrical-structural step and must be requested via the Keyword Editor as follows:
*Output, history
*Integrated Output, section=I-section-name
SOE
For the connector in the application, the permissible continuous load for an electrical current is 141.4 amperes and the permissible short-term load for this is 282.7 amperes. The simulation was carried out with the two different surface currents.
Figure 9: SOE or the total current over the section of the two simulations
The result of SOE is plotted by the connector as a graph in Figure 9, which shows the amount of current through a selected surface. As mentioned above, this option helps the user to compare the current in a simulation and that of the experiment. Fig. 9 shows the results of four simulations; transient at 141.4 amps, transient at 282.7 amps, steady state at 141.4 amps and steady state at 282.7 amps.
Figure 10: The result of the node temperature of this simulation with 141.4 amps
Figure 11: The result of the node temperature of this simulation with 282.7 amps
The result of the maximum node temperature of this simulation with 141.4 amperes is approx. 36 °C and the result with 282.7 amperes is approx. 67 °C (Fig. 10 and Fig. 11). The temperature curve during the four simulations is shown as a diagram in Fig. 11. This also explains why 282.7 amperes are permissible for a short-term load. For a duration of less than 20 s, a maximum temperature of 35 °C is reached; for a longer duration, the temperature rises up to 67 °C.
Figure 12: The result of the node temperature of four simulations as a diagram
From our experience
In Abaqus, different physical domains can be coupled together. As an example, a coupling of thermal, electrical and mechanical simulation was considered in this blog. A flat connector was used as a model for this. The multiphysics simulation illustrates how hot a plug or blade terminal becomes at a certain current. The permissible short-term and continuous load of such a plug are 282.7 amperes and 141.4 amperes respectively. While a maximum temperature of 36 °C is reached with the continuous load current, a current twice as high can lead to temperatures of up to 67 °C. However, if the intended short load duration of 20s is adhered to, the temperatures remain within a reasonable range of below 36 °C. For further considerations, ventilation or cooling systems can be added in order to find a design that is also suitable for higher currents.
Bibliography:
- Zarei, Naghmeh. 2024, Multiphysics Simulation with Abaqus Magnetic Deformation [Online]. Available: https://blog.technia.com/en/multiphysics-simulation-with-abaqus-magnetic-deformation
- Dassault Systèmes, "Online Companion," [Online]. Available:
https://widgetfactoryext.extranet.3ds.com/api/download/ENOVIA/file/service/3DXU.
PRDEXT/param/value/action/enovia/skilldevelopment/COMPANION_SCORM/Launch.
html?authentication=4&AICC_SID=-5951777581260773852izihj&sSourcePath=https
%3A%2F%2Feduspace.3ds.com%3A
