Structural-to-Structural Co-Simulation

Co-simulation between Abaqus/Standard and Abaqus/Explicit is a multiple domain analysis approach, where each Abaqus analysis operates on a complementary section of the model domain where it is expected to provide the more computationally efficient solution. For example, Abaqus/Standard provides a more efficient solution for light and stiff components, while Abaqus/Explicit is more efficient for solving complex contact interactions. In addition, when a portion of the Abaqus/Standard model is linear, you can use substructures to further reduce the computational cost .

You can use the following Abaqus/Standard analysis procedures:

• Static Stress Analysis

• Implicit Dynamic Analysis Using Direct Integration

You can use the following Abaqus/Explicit analysis procedure:

• Explicit Dynamic Analysis

The domains modeled in each Abaqus analysis are complementary, and the interaction between the models takes place through a common interface region. You can specify an interface region using either node sets or surfaces when coupling Abaqus/Standard to Abaqus/Explicit. However, you must be consistent in your region definition in Abaqus/Standard and Abaqus/Explicit. If you define a co-simulation region with a node set or node-based surface in one analysis, you must use the same type of co-simulation region definition in the other analysis. For node-based surfaces the nodes must be coincident because no topology information is provided to conservatively map fields between the models. Likewise, if you define a co-simulation region with an element-based surface in one analysis, you must define your co-simulation region with an element-based surface in the other analysis.

You can have dissimilar meshes in regions shared in the Abaqus/Standard and Abaqus/Explicit model definitions. In some cases you can improve solution stability and accuracy by ensuring that you have matching nodes at the interface (see Dissimilar Mesh-Related Limitations). In these cases you can use the modeling practice described in Ensuring matching nodes at the interface regions to ensure these matching nodes.

In the step definition, you declare a co-simulation step, define the interface region, and specify the solution fields to exchange. When coupling Abaqus/Standard to Abaqus/Explicit, you can declare only a single interface region; if there are multiple regions, you must combine them into a single region. The fields exchanged depend on the interface method and whether or not rotational degrees of freedom are active at the interface.

CO-SIMULATION, PROGRAM=MULTIPHYSICS
CO-SIMULATION REGION, IMPORT, TYPE=SURFACE (default)
element-based or node-based surface, comma-separated list of fields
CO-SIMULATION REGION, EXPORT, TYPE=SURFACE (default)
element-based or node-based surface, comma-separated list of fields

CO-SIMULATION, PROGRAM=MULTIPHYSICS
CO-SIMULATION REGION, IMPORT, TYPE=NODE
node set, comma-separated list of fields
CO-SIMULATION REGION, EXPORT, TYPE=NODE
node set, comma-separated list of fields

The enhanced subcycling method is the preferred method for coupling Abaqus/Standard to Abaqus/Explicit. This method ensures velocity compatibility at the interface, where calculations are performed by an interface service; stiffness and mass properties of the underlying structure are exchanged in the form of a dynamic interface operator providing robust and accurate solutions for strongly coupled physics. Abaqus/Explicit subcycles (that is, takes one or more increments) per Abaqus/Standard increment to ensure a cost-effective solution of both domains. This method allows constraints to exist on the co-simulation interface region. Table 1 and Table 2 provide descriptions of fields exchanged and their causality (whether the field is imported or exported). Fields associated with a rotational degree of freedom should be exchanged only when the elements underlying the interface are structural elements with rotational degrees of freedom.

An interface solve is performed in Abaqus/Explicit for every Abaqus/Explicit increment. This solve can be costly because the interface matrix used for the interface solve is dense, and its size scales with the number of interface nodes.

CO-SIMULATION, PROGRAM=MULTIPHYSICS
CO-SIMULATION REGION, IMPORT, TYPE=NODE or SURFACE
node set or surface name, IFORCE, IMOMENT
CO-SIMULATION, EXPORT, TYPE=NODE or SURFACE
node set or surface name, VT, VR, H

CO-SIMULATIONPROGRAM=MULTIPHYSICS
CO-SIMULATION REGION, IMPORT, TYPE=NODE or SURFACE
node set or surface name, VTINTRF, VRINTFRF
CO-SIMULATION, EXPORT, TYPE=NODE or SURFACE
node set or surface name, IFORCE, IMOMENT

Similar to the enhanced subcycling method, the "original" subcycling method ensures velocity compatibility at the interface and provides a robust and accurate solution for strong coupled physics.

Table 3 and Table 4 provide descriptions of fields exchanged and their causality. You must specify rotational fields even if they are not active at the interface.

An interface solve is performed in Abaqus/Standard for every Abaqus/Explicit increment. This solve can be costly for two reasons. First, the interface matrix used for the interface solve is dense, and its size scales with the number of interface nodes. Second, the interface matrix changes every Abaqus/Explicit increment, requiring factorization in Abaqus/Standard for every Abaqus/Explicit increment. You can reduce the impact of this cost by approximating the interface matrix and factorizing it typically once for the duration of an Abaqus/Standard increment, rather than for eachAbaqus/Explicit increment. However, if the Abaqus/Explicit stable time increment changes significantly, the interface matrix is refactored for stability reasons.

Factorizing the interface matrix every Abaqus/Explicit increment is the default. When the number of interface nodes is large, using this approach reduces the cost of the interface factorization. Only the interface matrix factorization is performed once per Abaqus/Standard increment; the interface solve is performed every Abaqus/Explicit increment using this factorized interface matrix. Because this approach approximates the interface matrix, it might slightly increase the drift in the displacement solution at the co-simulation interface. The performance gain with this method depends on the number of interface nodes, the subcycling ratio (which is the ratio between Abaqus/Standard and Abaqus/Explicit increments), and the size of the models. For models with greater than 100 interface nodes and a subcycling ratio greater than 50, this method typically reduces the analysis time by a factor between 1.2 and 3.0. The performance gain increases for larger subcycling ratios and decreases for larger models.

You can also automate the selection of the fields for both Abaqus/Standard and Abaqus/Explicit models.

CO-SIMULATION, PROGRAM=MULTIPHYSICS
CO-SIMULATION REGION, IMPORT, TYPE=NODE or SURFACE
node set or surface name, VTINTRF, VRINTFRF, MASSINV, RICUR
CO-SIMULATION REGION, EXPORT, TYPE=NODE or SURFACE
node set or surface name, IFORCE, IMOMENT, VT, VR

CO-SIMULATION, PROGRAM=MULTIPHYSICS
CO-SIMULATION REGION, IMPORT, TYPE=NODE or SURFACE
node set or surface name, IFORCE, IMOMENT, VTINIT, VRINIT
CO-SIMULATION REGION, EXPORT, TYPE=NODE or SURFACE
node set or surface name, VT, VR, MASS, RICUR

CO-SIMULATION CONTROLS, FACTORIZATION FREQUENCY=STANDARD INCREMENT

CO-SIMULATION, PROGRAM=ABAQUS
CO-SIMULATION REGION, TYPE=NODE or SURFACE
node set or surface name

The time incrementation that you choose for coupling affects the solution computational cost, accuracy, and stability. The enhanced subcycling method is frequently the more robust, accurate, and cost effective method because Abaqus/Standard time increments, free of any forced co-simulation time incrementation constraints, are commonly much longer than Abaqus/Explicit time increments. However, this subcycling method might be less cost effective when a large portion of the nodes in the model are at the co-simulation interface. This is because stabilization operations at the interface (a “free solve”) for each increment in the Abaqus/Explicit analysis is performed. These free-solve operations require an implicit solution of a dense system of equations that scale with the number of interface nodes. In cases with a large number of interface nodes, the computational cost of this interface solve can exceed any cost savings seen due to subcycling. Therefore, for a model where a significant share of the nodes are at the co-simulation interface, performance might be poorer with the subcycling scheme. In such a case, you can use the lockstep method, where Abaqus/Standard is forced to use the time increment size of the Abaqus/Explicit analysis. This approach enforces displacement compatibility at the interface.

Table 5 and Table 6 provide descriptions of the fields exchanged and their causality. You must specify rotational fields even if there are no rotational degrees of freedom active at the interface.

The selection of the fields for both Abaqus/Standard and Abaqus/Explicit models are automated.

CO-SIMULATION CONTROLS, NAME=controls name, TIME INCREMENTATION=LOCKSTEP
CO-SIMULATION, PROGRAM=ABAQUS
CO-SIMULATION REGION,  TYPE=NODE or SURFACE
node set or surface name

You can use predefined templates to create a configuration file for the coupling schemes described above. Table 7 describes the two predefined templates available for Abaqus/Standard to Abaqus/Explicit co-simulation and lists example configuration files that you can review.

To obtain an example configuration file, you can use the abaqus fetch utility. For example, to obtain the example for Abaqus/Standard to Abaqus/Explicit subcycling, use the following command:

abaqus fetch job=GandC_contbeam_mixDofs

You can then modify the configuration by modifying the replaceable text (rotation degrees of freedom active at interface, job names, Abaqus/Explicit interface region name and duration).

<?xml version="1.0" encoding="utf-8"?>
<CoupledMultiphysicsSimulation>
   <template_std_xpl_subcycleEnhanced rotation="true or false">
      <Standard_Job>standard_job_name</Standard_Job>
      <Explicit_Job>explicit_job_name</Explicit_Job>
      <Explicit_Interface>region_name</Explicit_Interface>
      <duration>duration_value</duration>
   </template_std_xpl_subcycleEnhanced>
</CoupledMultiphysicsSimulation>

In certain cases you might need to use co-simulation configuration features that are not described in the predefined templates. For example, you might want to change the dissimilar mesh mapping search tolerances; these tolerances are available generally in the configuration file but are not described in the predefined templates. For these cases, you must create an elaborated configuration file; for more information, see Using Elaborated Configuration Files.

You execute the co-simulation interactively in Abaqus/CAE or from the command line, as described in Executing a Co-Simulation.