17.2.1 Preparing an Abaqus analysis for co-simulation
Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD
References
Overview
Preparing an Abaqus analysis for co-simulation involves the following:
identifying an Abaqus analysis step for co-simulation analysis;
identifying the co-simulation interface regions in the Abaqus model; and
identifying the fields exchanged during the co-simulation.
This section provides an overview of preparing an Abaqus analysis for a co-simulation. The discussion in this section is general and may not apply to every product pairing. “Co-simulation between Abaqus solvers,” Section 17.3, provides setup, execution, and limitation details for co-simulation between Abaqus solvers. For co-simulation between Abaqus and third-party analysis programs, consult the appropriate User’s Guide.
Identifying an Abaqus step for co-simulation analysis
The co-simulation event need not begin at the start of the first step in an Abaqus analysis. However, it does need to start with the beginning of an analysis step and end within that analysis step. Hence, you need to define the step durations in Abaqus such that the start of the co-simulation event falls at the beginning of an Abaqus analysis step and to define that particular step so that the co-simulation event ends by the end of that step. Regular loads and boundary conditions for the Abaqus model are specified as usual.
Communication with the coupled analysis is initiated as the co-simulation event begins and is terminated when the co-simulation event time is reached. Abaqus may terminate the co-simulation event when the end of the analysis step is reached prior to the co-simulation event time or when the analysis cannot proceed any further; for example, due to convergence problems. In such a case, a warning message is issued to all clients, and the co-simulation is terminated.
Co-simulation is supported by the following Abaqus procedures:
“Implicit dynamic analysis using direct integration,” Section 6.3.2
“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
| Input File Usage: | Use the following option within a step definition to indicate the beginning of a co-simulation event: |
*CO-SIMULATION, NAME=name |
Identifying the analysis program communicating with Abaqus during the co-simulation
You can couple Abaqus with another Abaqus analysis or Abaqus with certain third-party analysis programs using the SIMULIA Co-Simulation Engine. For details on coupling with third-party analysis programs, see the respective User's Guides.
| Input File Usage: | Use the following option to couple Abaqus analyses (except Abaqus/Standard to Abaqus/Explicit) and Abaqus to third-party analysis programs: |
*CO-SIMULATION, NAME=name, PROGRAM=MULTIPHYSICS Use the following option to couple Abaqus/Standard to Abaqus/Explicit: *CO-SIMULATION, NAME=name, PROGRAM=ABAQUS |
Identifying the co-simulation interface region
Interaction between two Abaqus models or between an Abaqus model and a third-party analysis model takes place through a common interface region referred to as the co-simulation interface region. The co-simulation interface region may be a set of discrete points, a surface region, or a volume region. You must be consistent in your interface region definition; if you define a surface co-simulation region in one analysis, then you must define a surface co-simulation region in the other analysis. Furthermore, these co-simulation regions need to be co-located and have the same region boundaries.
Interacting through discrete points
Interaction can occur through a set of discrete points where only nodal position information without element topology information (e.g., tributary area) defines the co-simulation interface region. In this case the spatial mapping is limited to point-to-point mapping, and you must ensure that there are matching nodes between the models.
In Abaqus you can use a node set or a node-based surface to define a co-simulation interface region consisting of discrete points.
| Input File Usage: | Use the following option to define a node set as a co-simulation region in an Abaqus model: |
*CO-SIMULATION REGION, TYPE=NODE nodeset_A Use the following options to define a node-based surface as a co-simulation region in an Abaqus model: *SURFACE, TYPE=NODE nodeset_A *CO-SIMULATION REGION, TYPE=SURFACE node-based surface name |
Interacting through a surface
Interaction between distinct domains occurs through a common interface surface. For example, when a fluid interacts with a solid without penetrating it, the fluid-solid interface is defined through a surface. In this case both nodal position and element topology information define the co-simulation interface, and appropriate spatial mapping between dissimilar surface meshes is performed to conservatively map fields.
| Input File Usage: | Use the following option to define an element-based surface as a co-simulation region in an Abaqus model: |
*CO-SIMULATION REGION, TYPE=SURFACE (default) element-based surface name |
Interacting through a volume
Interaction between overlapping domains occurs through a volume. In this case both nodal position and element topology information define the co-simulation region, and appropriate spatial mapping between dissimilar volume meshes is performed to conservatively map fields.
The interface region is defined by an element set.
| Input File Usage: | Use the following option to define a volume as a co-simulation region in an Abaqus model: |
*CO-SIMULATION REGION, TYPE=VOLUME elset_A |
Identifying the fields exchanged across a co-simulation interface
The coupling of the domain models can be through loads and/or boundary conditions prescribed at the co-simulation interface. In addition, mass, rotary inertia, and heat capacitance terms can also be exchanged. Based on the physics and the interaction type and its enforcement, you must specify the fields that are imported and/or exported in an Abaqus analysis during the co-simulation.
The co-simulation interface can consist of a group of discrete points (nodes), a surface region, or a volume region. Not all fields can be exchanged across all region types.
This section provides a general overview of all fields available in Abaqus. For detailed information on the fields exchanged between two Abaqus solvers, see “Structural-to-structural co-simulation,” Section 17.3.1, and “Fluid-to-structural and conjugate heat transfer co-simulation,” Section 17.3.2. For detailed information on fields exchanged by Abaqus and a third-party analysis program, see the respective User’s Guides.
| Input File Usage: | Use the following option to import field data over a region into Abaqus: |
*CO-SIMULATION REGION, IMPORT region_A, import_field_1 region_A, import_field_2 Use the following option to export data from Abaqus: *CO-SIMULATION REGION, EXPORT region_A, export_field_1 region_A, export_field_2 |
Procedures involving mechanical degrees of freedom
Table 17.2.1–1 lists the fields that can be exchanged for procedures supporting mechanical degrees of freedom (degrees of freedom 1–6), their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–1 Exchanging fields for procedures supporting mechanical degrees of freedom.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
|---|---|---|---|---|---|
| Import | Export | ||||
| UT or U | Displacement | P, S, V | S, E, C | S, E | L |
| VT or V | Velocity (transient procedures) | P, S, V | S, E, C | S, E |  |
| AT or A | Acceleration (transient procedures) | P, S, V | S | S, E |  |
| UR | Rotations | P, S | S, E | S, E | radians |
| VR | Angular velocity (transient procedures) | P, S | S, E | S, E | radians  |
| AR | Angular acceleration (transient procedures) | P, S | S | S, E | radians  |
| COORD | Current coordinates | P, S, V | S, E | ||
| CF | Concentrated forces | P, S, V | S, E | S, E | F |
| CM | Concentrated moments | P, S | S, E | S, E |  |
| TRSHR | Traction vector | S | C |  | |
| PRESS | Pressure normal to element surface | S | S | | |
| 1 P (points), S (surface region), V (volume region) | |||||
| 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
“Implicit dynamic analysis using direct integration,” Section 6.3.2
“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
Displacements
Displacements (field ID UT or U) for the translational degrees of freedom can be exported by Abaqus/Standard and Abaqus/Explicit. Displacements can be imported by Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD. When imported, displacements are ramped from the values of the previous exchange time point to those of the next target time point. In an implicit dynamic analysis, velocity and acceleration must be imported when importing displacement. The displacements are in the global coordinate system.
Displacements are available for points, surface regions, and volume regions in Abaqus/Standard and Abaqus/Explicit and for surface regions in Abaqus/CFD.
Displacements can be viewed in the Visualization module of Abaqus/CAE.
Velocity and acceleration
Velocity (field ID VT or V) and acceleration (field ID AT or A) for the translational degrees of freedom can be imported and exported by Abaqus/Standard for transient procedures and by Abaqus/Explicit. In an implicit dynamic analysis, when importing velocity or acceleration, all three fields—displacement, velocity, and acceleration—must be imported. Velocity can be imported by Abaqus/CFD. Velocity and acceleration are in the global coordinate system.
Velocity and acceleration are available for points, surface regions, and volume regions in Abaqus/Standard and Abaqus/Explicit and for surface regions in Abaqus/CFD.
Rotations
Rotations (field ID UR) can be imported and exported by Abaqus/Standard and Abaqus/Explicit. In an implicit dynamic analysis, rotational velocity and rotational acceleration must be imported when importing rotations. Rotations are in the global coordinate system.
Rotations are available for points and surface regions.
Rotations can be viewed in the Visualization module of Abaqus/CAE.
Rotational velocity and rotational acceleration
Rotational velocity (field ID VR) and rotational acceleration (field ID AR) can be imported and exported by Abaqus/Standard for transient procedures and by Abaqus/Explicit. In an implicit dynamic analysis, when importing rotational velocity or rotational acceleration, all three fields—rotation, rotational velocity, and rotational acceleration—must be imported. Rotational velocity and rotational acceleration are in the global coordinate system.
Rotational velocity and rotational acceleration are available for points and surface regions.
Current coordinates
Current nodal coordinates (field ID COORD) can be exported by Abaqus/Standard and Abaqus/Explicit. The coordinates are the current coordinates of the deformed structure whether small- or large-displacement analysis is performed. In general, it is preferred to export displacements (field ID UT or U) rather than current coordinates when results are mapped between dissimilar interface regions. In cases where the partner client does not retain the original coordinates, it may be necessary to send current coordinate values rather than displacements.
Current coordinates are available for points, surface regions, and volume regions in Abaqus/Standard and Abaqus/Explicit.
Concentrated forces
Concentrated forces (field ID CF), if imported, are ramped from the values of the previous exchange time point to those of the next target time point in Abaqus/Standard and are kept constant over the exchange interval in Abaqus/Explicit. The concentrated forces are in the global coordinate system.
When exporting concentrated forces, Abaqus/Standard transfers reaction forces at interface nodes that have prescribed displacements. The reaction forces are exported in the global coordinate system.
Concentrated forces are available for points, surface regions, and volume regions in Abaqus/Standard and Abaqus/Explicit.
Concentrated normal forces can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CF.
Concentrated moments
Concentrated moments (field ID CM), if imported, are ramped from the values of the previous exchange time point to those of the next target time point in Abaqus/Standard and are kept constant over the exchange interval in Abaqus/Explicit. The concentrated moments are in the global coordinate system.
Concentrated moments are available for points and surface regions in Abaqus/Standard and Abaqus/Explicit.
Concentrated moments can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CM.
Traction vector
The traction vector (field ID TRSHR), supported by Abaqus/CFD, exports the fluid total traction (normal and shear components) on the interface surface. Usually, the exported traction vector is integrated to concentrated forces (field ID CF) when imported into Abaqus/Standard or Abaqus/Explicit in a fluid-structure simulation.
The traction vector is a force vector in the global Cartesian coordinate system.
The traction vector is available for surface regions in Abaqus/CFD.
Normal pressure
Normal pressure (field ID PRESS), supported for import by Abaqus/Standard, is the traction normal component to the surface. Pressure values are ramped from the values of the previous exchange time point to those of the next target time point when imported into Abaqus/Standard. In most cases it is preferred to import concentrated forces (field ID CF) since these contain both the normal and shear traction components. For membrane-like structures it might be preferable to import pressures.
Normal pressure can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable P.
Procedures involving thermal degrees of freedom
Table 17.2.1–2 lists the thermal fields available for co-simulation exchange, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–2 Exchanging fields for procedures supporting thermal degrees of freedom.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
|---|---|---|---|---|---|
| Import | Export | ||||
| NT | Temperature as a nodal degree of freedom | P, S, V | S, E | S, E |  |
| CFL | Concentrated heat flux at a node | P, S, V | S, E |  | |
| HFL | Heat flux normal to element surface | S | S | C |  |
| CFILM | Film properties | S | S |  | |
| FILM | Film properties (MpCCI only) | S | S |  | |
| TEMP | Temperature as a nodal degree of freedom | P, S, V | C | | |
| LUMPEDHEATCAPACITANCE | Lumped heat capacitance | P, S, V | S, E | C |  |
| 1 P (points), S (surface region), V (volume region) | |||||
| 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
Nodal temperature
Nodal temperature (field ID NT) can be imported and exported by Abaqus/Standard and Abaqus/Explicit and imported by Abaqus/CFD (as field ID TEMP). Temperature values are ramped from the values of the previous exchange time point to those of the next target time point when imported into Abaqus/Standard and Abaqus/CFD.
Temperature values can be exchanged either on the top surface (SPOS) or the bottom surface (SNEG) of structural elements. Temperatures cannot be exchanged on double-sided surfaces. When exchanging temperatures on both the top and bottom faces, define two different regions; one to exchange temperature on the top face and the other to exchange temperature on the bottom face. For volume regions, only degree of freedom NT11 is used, and it should not be used for exchanging temperature values over volumes discretized by nonthermal element types.
Nodal temperature values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable NT.
Heat flux
Use concentrated heat flux (field ID CFL) for heat entering at a node in Abaqus/Standard and Abaqus/Explicit. Concentrated heat flux is available for points, surface regions, and volume regions.
Heat flux values can be exchanged either on the top surface (SPOS) or the bottom surface (SNEG) of structural elements. Heat flux cannot be exchanged on double-sided surfaces. When exchanging heat flux on both the top and bottom faces, define two different regions; one to exchange heat flux on the top face and the other to exchange heat flux on the bottom face.
Concentrated heat flux values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CFL.
Use surface heat flux (field ID HFL) for a distributed heat flux entering the surface in Abaqus/Standard or distributed heat flux leaving a surface in Abaqus/CFD. Distributed heat flux is available only for surface regions.
Film properties
Use surface film properties (field ID FILM) or concentrated (nodal) film properties (field ID CFILM) to model convection governed by
is the wall temperature, and 
is the fluid or ambient temperature. The film coefficient is computed from the heat flux and fluid temperature obtained from the computational fluid dynamics analysis and the wall temperature from the Abaqus/Standard analysis computed during the previous exchange interval, according to
Film properties are available only for surface regions in Abaqus/Standard.
Procedures involving pore fluid pressure
Table 17.2.1–3 lists additional fields that can be exchanged for a coupled pore fluid diffusion/stress analysis, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–3 Exchanging fields for a coupled pore fluid diffusion/stress analysis.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
|---|---|---|---|---|---|
| Import | Export | ||||
| POR | Pore fluid pressure at a node | P, S, V | S | S | |
| CFF | Concentrated fluid flow at a node | P, S, V | S |  | |
| RVF | Reaction fluid volume flux due to prescribed pressure | P, S, V | S | | |
| 1 P (points), S (surface region), V (volume region) | |||||
| 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
Pore pressure
Nodal pore pressure (field ID POR) can be imported and exported by Abaqus/Standard for points, surface regions, and volume regions.
Nodal pore pressure values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable POR.
Concentrated fluid flow
Fluid flow (field ID CFF) defines the seepage flow at a node. Concentrated fluid flow can be imported by Abaqus/Standard for points, surface regions, and volume regions.
Concentrated fluid flow values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CFF.
Reaction fluid volume flow
Reaction fluid volume flux (field ID RVF) defines the rate at which fluid volume is entering or leaving the model through the node to maintain the prescribed pore pressure. Reaction fluid volume flux can be exported by Abaqus/Standard for points, surface regions, and volume regions.
Procedures involving electromagnetic response
Table 17.2.1–4 lists additional fields that can be exchanged for an electromagnetic analysis, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–4 Exchanging fields for a electromagnetic analysis.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
|---|---|---|---|---|---|
| Import | Export | ||||
| EMJH | Joule heating flux due to flow of current | V | S |  | |
| EMBF | Magnetic body force intensity vector due to flow of current | V | S |  | |
| 1 P (points), S (surface region), V (volume region) | |||||
| 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
Joule heating flux
The Joule heating flux (field ID EMJH) can be exported by Abaqus/Standard for volume regions. It can be imported in a downstream heat transfer analysis as concentrated nodal heat flux (field ID CFL).
Values for the Joule heating flux can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable EMJH.
Magnetic body force intensity vector
The magnetic body force intensity vector (field ID EMBF) can be exported by Abaqus/Standard for volume regions. It can be imported in a downstream stress analysis as concentrated force (field ID CF).
Magnetic body force intensity vector values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable EMBF.
Temperature and independent field variables
Field variables are time-dependent, predefined fields that exist over the spatial domain of the model (see “Predefined fields,” Section 34.6.1). Field variables in conjunction with the co-simulation technique extend the possibilities of multiphysics by allowing material point dependencies on an external field defined by another application.
Field variables must be numbered consecutively starting with one. Field variables can be defined:
by entering the data directly,
by reading an Abaqus results file or output database file,
in an Abaqus/Standard user subroutine, and
through the co-simulation interface.
If field variables are defined by multiple methods, Abaqus processes them in the order defined above. Care needs be taken when field variables are used with structural elements, such as membranes and shells. In this case only the top or bottom face forming the interface region receives a value.
Table 17.2.1–5 lists the temperature and independent field variables available for co-simulation exchange, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–5 Exchanging temperature and independent field variables.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
|---|---|---|---|---|---|
| Import | Export | ||||
| TEMP | Temperature as field variable | V | S | | |
| FV1 | Field variable 1 | V | S | ||
| FV2 | Field variable 2 | V | S | ||
| FV3 | Field variable 3 | V | S | ||
| 1 P (points), S (surface region), V (volume region) | |||||
| 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
“Implicit dynamic analysis using direct integration,” Section 6.3.2
“Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
Temperature
Temperature (field ID TEMP) can be imported by Abaqus/Standard for procedures that allow material properties to be defined as a function of an external temperature field. When imported, temperature values are ramped from the values of the previous exchange time point to those of the next target time point. Use field ID NT instead of field ID TEMP to import temperature values for thermal procedures (procedures using degrees of freedom 11, 12, etc.).
Temperature can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting element output variable TEMP.
Independent field variables
Independent field variables (field IDs FV1, FV2, and FV3) can be imported by Abaqus/Standard, allowing material properties to be defined as a function of the external fields. When imported, independent field variable values are ramped from the values of the previous exchange time point to those of the next target time point.
Field variables can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variables FV1, FV2, and/or FV3.
Miscellaneous fields
Table 17.2.1–6 lists miscellaneous fields available for co-simulation exchange, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–6 Exchanging miscellaneous fields.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
|---|---|---|---|---|---|
| Import | Export | ||||
| MASS or LUMPEDMASS | Mass | P, S | S, E | S, E, C | M |
| RI | Rotary inertia | P, S | S | E |  |
| 1 P (points), S (surface region), V (volume region) | |||||
| 2 S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
Defining the coupling and rendezvousing scheme
Different types of analyses have different time integration requirements that will influence or dictate the frequency of interaction between the analyses in a co-simulation to obtain an accurate and robust solution. For example, consider the difference in time integration between an implicit and an explicit dynamic analysis. Furthermore, Abaqus/Standard can adjust the increment sizes automatically to obtain an economical and accurate solution for transient problems (see “Incrementation” in “Defining an analysis,” Section 6.1.2). For example, consider a transient heat transfer analysis modeling a diffusive process; here the analysis may use small time increments at the beginning of the analysis where there is a high gradient in the solution and large time increments toward the end of the analysis when steady state is reached.
The parameters that you use to control these co-simulation exchanges depend on the co-simulation interface that you are using.
You define the co-simulation algorithm and related exchange parameters in a co-simulation configuration file.
For structural-to-structural co-simulation using Abaqus/Standard and Abaqus/Explicit, you must also provide co-simulation controls parameters in the input file.
Using the SIMULIA Co-Simulation Engine configuration file
The SIMULIA Co-Simulation Engine employs an independent software component, termed the “director,” which defines all aspects of the interaction for co-simulation between analysis programs and provides the necessary instructions to implement the coupling and rendezvousing schemes. You provide the director with relevant parameters for your scheme choices through the co-simulation configuration file. When you use Abaqus/CAE to execute the co-simulation, the configuration file is created for you automatically.
The configuration file must be in Extensible Markup Language (XML) format, which uses the file extension xml. You can define a configuration file through a predefined template, or you can create a fully elaborated form of the configuration file.
Using predefined configuration templates
For the co-simulation analysis cases described in “Co-simulation between Abaqus solvers,” Section 17.3, predefined templates that define common coupling and rendezvousing schemes are available. To use one of the predefined templates, you must create a configuration file with the structure shown below.
<?xml version="1.0" encoding="utf-8"?>
Required XML declaration line
<CoupledMultiphysicsSimulation>
Required XML root element; identifies file as describing a multiphysics simulation
<template_name>
<template_parameter_1>parameter_1_name</template_parameter_1>
<template_parameter_2>parameter_2_name</template_parameter_2>
<template_parameter_3>parameter_3_name</template_parameter_3>
</template_name>
Closure of the template element
</CoupledMultiphysicsSimulation>
Closure of the XML root elementYou enter the template name and a short list of parameter settings, such as the names of the two analysis jobs and the duration of the analysis. Details of the predefined templates are provided in “Structural-to-structural co-simulation,” Section 17.3.1; “Fluid-to-structural and conjugate heat transfer co-simulation,” Section 17.3.2; and “Electromagnetic-to-structural and electromagnetic-to-thermal co-simulation,” Section 17.3.3; as well as information on how to obtain an example configuration file for each template, such as the example shown below for a fluid-to-structural co-simulation.<?xml version="1.0" encoding="utf-8"?>
<CoupledMultiphysicsSimulation>
<template_std_cfd_fsi>
<Standard_Job>StandardJobName</Standard_Job>
<Cfd_Job>CfdJobName</Cfd_Job>
<duration>duration</duration>
</template_std_cfd_fsi>
</CoupledMultiphysicsSimulation>Using elaborated configuration files
At run time, the SIMULIA Co-Simulation Engine director applies your parameter settings to the template, creating an elaborated configuration file that is then used in the co-simulation analysis. An elaborated configuration file is defined as a configuration file that provides all details of the configuration explicitly without referring to a template.
In cases where predefined templates are not available (such as coupling with an in-house or third-party code) or are insufficient (for example, you want to exchange more variables at the co-simulation interface region or adjust mapping tolerances), you must create an elaborated configuration file. For tips on working with elaborated configuration files, see “Advanced Uses of the SIMULIA Co-Simulation Engine Configuration File” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base. For detailed information about the elaborated configuration file, see the SIMULIA Co-Simulation Engine Application Programing Interface (API) documentation.
Coupling and rendezvousing schemes for elaborated configuration files
You define the co-simulation coupling and rendezvousing schemes in an elaborated configuration file.
Coupling scheme
The coupling scheme defines the sequence of exchanges between analysis programs and whether a coupled simulation can be run in a serial, parallel, or implicit iterative manner. When deciding on the coupling scheme, you should consider solution stability issues as well as the utilization impact on your computing resources
Parallel explicit coupling scheme (Jacobi)
In a parallel explicit coupling scheme, both simulations are executed concurrently, exchanging fields to update the respective solutions at the next target time. The parallel coupling scheme may make more efficient use of computing resources; however, it is considered less stable than the sequential scheme and should be employed only for weakly coupled physics simulations using small coupling steps. The co-simulation partner analysis must also specify a Jacobi coupling algorithm.
Sequential explicit coupling scheme (Gauss-Seidel)
In a sequential explicit coupling scheme, the simulations are executed in sequential order. One analysis leads while the other analysis lags the co-simulation. The co-simulation partner analysis must also specify a Gauss-Seidel coupling algorithm.
The sequential explicit coupling scheme should be employed only for weakly coupled physics simulations using small coupling steps.
Iterative coupling scheme
In an iterative coupling scheme, the simulations are executed in sequential order. One analysis leads while the other analysis lags the co-simulation. Multiple exchanges per coupling step are performed until termination criteria are met.
The termination criteria depend on the analyses in the co-simulation; for co-simulation between Abaqus and third-party analysis products, consult the appropriate User’s Guide.
Coupling step size
The coupling step is the period between two consecutive exchanges and consequently defines the frequency of exchange between the analyses in a co-simulation. The coupling step size is established at the beginning of each coupling step and is used to compute the target time (the time when the next synchronized exchange occurs).
The methods available in Abaqus for computing the coupling step size are described in the sections below. To determine the methods available for a co-simulation partner analysis, consult the appropriate third-party program documentation.
Constant coupling step size
A constant user-defined coupling step size is the most basic method of defining a coupling step size. Both analyses advance while exchanging data at target points according to
is a value that defines the coupling step size to be used throughout the coupled simulation, 
is the target time, and 
is the time at the start of the coupling step. Minimum coupling step size
This method selects the minimum of the coupling step sizes suggested by each analysis. Abaqus always uses the next increment suggested by its automatic incrementation as its suggested coupling step size.
Maximum coupling step size
This method selects the maximum of the coupling step sizes suggested by each analysis. Abaqus always uses the next increment suggested by its automatic incrementation as its suggested coupling step size.
Time incrementation scheme
Abaqus may take multiple increments per coupling step, or you can force Abaqus to use a single increment per coupling step.
Typically, Abaqus may perform several increments (referred to as “subcycling”) during the coupling step. During subcycling, Abaqus/Standard ramps the loads and boundary conditions (with the exception of film properties) from the values at the end of the previous coupling step to the values at the target time, while in Abaqus/Explicit the loads are applied at the start of the coupling step and kept constant over the coupling step.
Subcycling allows Abaqus to use its own time incrementation to reach the target coupling time; specifically, it allows Abaqus to cut back the increment size if there are nonlinear events that require the increment size to be reduced.
In certain cases you may force Abaqus to use a time increment size dictated by the coupling step size (i.e., no subcycling). This allows both solvers to use the same time incrementation and avoid interpolation of quantities during the coupling step. When proceeding in this “lockstep” manner, Abaqus will not be able to reduce the time increment to resolve nonlinear events and, consequently, will terminate the simulation in cases where the nonlinear events require that the increment size be reduced.
Model dimension and coordinate systems
Two-dimensional and three-dimensional Abaqus models are fully supported. Axisymmetric Abaqus models are supported only for Abaqus/Standard to Abaqus/Explicit co-simulation. For co-simulations that do not support two-dimensional and axisymmetric models, you can represent these models as a three-dimensional slice of unit thickness (or wedge element) with the appropriate boundary conditions applied.
Vector quantities are defined according to Abaqus conventions; the first component represents the quantity along the x-axis, the second quantity represents the quantity along the y-axis, and the third quantity represents the quantity along the 
-axis (for three-dimensional models). For axisymmetric models in Abaqus the axis of revolution is about the y-axis. These conventions apply to both the exported and the imported vector quantities.
All exported vector quantities are expressed in the global coordinate system of the Abaqus model, ignoring any transformation definitions. Similarly, the third-party program must provide vector quantities that are imported into Abaqus in the global coordinate system of the Abaqus model.
The third-party analysis program may use different conventions, please refer to the appropriate third-party program documentation for further modeling details and/or limitations.
Unit system
Abaqus does not require that the analysis be run with a particular unit system. In general, the unit system used in creating the Abaqus model may not be the same as that used with the third-party program model. When the two unit systems differ, the fields exchanged between the two programs must go through a transformation of units. Refer to the appropriate third-party program documentation for further modeling details.
Restarting a co-simulation
Field imported into Abaqus/Standard, Abaqus/Explicit, or Abaqus/CFD are not saved to the Abaqus restart database. Thus, to restart a co-simulation, the coupled analysis must send the fields at the start of the restart analysis. These fields must balance the conjugate fields computed by the Abaqus analysis such that equilibrium is maintained. You must synchronize the restart information written between the analyses to ensure that the simulation is restarted at the same solution (step) time. For more information, see “Synchronizing restart information written in a co-simulation” in “Restarting an analysis,” Section 9.1.1. Specifically, the solution time for the particular step/increment number from which Abaqus is restarted must correspond to the coupled analysis solution.
Limitations
The following limitations apply:
The steps in the Abaqus model must be defined such that the co-simulation fits entirely within a single Abaqus step. Further, there can be only one co-simulation in the Abaqus job. You can use the restart capability to perform multiple co-simulations for an analysis (see “Restarting an analysis,” Section 9.1.1).
A co-simulation surface or volume defined over beam, pipe, and truss elements or defined over the edges of three-dimensional elements cannot be used as an interface region. You should use discrete points to transfer loads and boundary conditions.
A co-simulation surface or volume defined over modified triangular elements or modified tetrahedral elements cannot be used as an interface region.
Quadratic coupled temperature-displacement elements cannot be used as an interface region in a co-simulation using the coupled temperature-displacement procedure.
When performing a co-simulation, output at specified time points may not be satisfied at the requested times, depending on the synchronization parameters.