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, particularly away from the interface regions, are specified as usual.

Communication with a third-party analysis program is initiated as the co-simulation event begins and is terminated when the co-simulation event is ended by either program. Abaqus may terminate the co-simulation event when the end of the analysis step is reached or when the analysis cannot proceed any further; for example, due to convergence problems.

*CO-SIMULATION, NAME=name

The Abaqus co-simulation technique provides several interfaces, such as SIMULIA interfaces for coupling Abaqus to Abaqus and Abaqus to third-party analysis programs and a general open interface through the multiphysics code coupling interface, MpCCI.

*CO-SIMULATION, PROGRAM=ABAQUS 

*CO-SIMULATION, PROGRAM=MULTIPHYSICS 

*CO-SIMULATION, PROGRAM=DCI

*CO-SIMULATION, PROGRAM=MULTIPHYSICS

*CO-SIMULATION, PROGRAM=MPCCI 

*CO-SIMULATION, PROGRAM=MADYMO 

Interaction between the two Abaqus models or between the Abaqus model and the third-party analysis program model takes place through a common interface region.

*CO-SIMULATION REGION, TYPE=NODE
nodeset_A

*CO-SIMULATION REGION, TYPE=SURFACE
surface_A

*CO-SIMULATION REGION, TYPE=SURFACE
surface_A

*CO-SIMULATION REGION
surface_A, quantity

*CO-SIMULATION REGION, REGION ID=n
surface_A,
surface_B,

The coupling of the domain models can be through loads, boundary conditions, or contact conditions prescribed at the interface; for example, continuous heat flux across the interface or continuity of a temperature field at the interface. Based on the interaction type and its enforcement, you can specify the fields that need to be exchanged during the simulation.

The methods for identifying the fields exchanged across an interface vary depending on the program with which Abaqus is coupling. In Abaqus/Standard to Abaqus/Explicit co-simulation you do not define the fields exchanged; they are determined automatically according to the procedures and co-simulation parameters used. In co-simulation with Abaqus/CFD, the fields exchanged are determined automatically by Abaqus/CAE. For co-simulation with MADYMO the list of fields to be exported and imported over a co-simulation region is predetermined by the MADYMO interface.

Identifying the fields exchanged across an interface with a third-party analysis program

Table 14.1.2–1 lists all the fields and their associated field identifiers that are available for co-simulation exchange. The choice of appropriate fields depends on the Abaqus analysis procedure and the coupling analysis program. Fields that can be imported into and exported from Abaqus/Standard or Abaqus/Explicit depend on the analysis procedure as defined in Table 14.1.2–2. For fields available for a particular third-party analysis program, consult the third-party program documentation.

Table 14.1.2–1 Fields and identifiers available for co-simulation exchange.

Field ID	Fields	Units
CF	Traction vector at a node	F
CFILM	Film properties	,
CFL	Concentrated heat flux at a node
CFLOW	Concentrated flow at a node
COORD	Current coordinates	L
FILM	Film properties	,
FLOW	Flow normal to element surface
FVi	General field variables (FV1, FV2, …)
HFL	Heat flux normal to element surface
NT	Temperature as a nodal degree of freedom
POR	Pore fluid pressure
PRESS	Pressure normal to element surface
TEMP	Temperature as a field variable in Abaqus
U	Displacement	L
V	Velocity

Table 14.1.2–2 Fields available for import to and export from Abaqus for particular procedures.

Procedure description	Import	Export
Static	CF	CF
	FVi	COORD
	PRESS	PRESS
	TEMP	U
	U
Implicit dynamic	CF	CF
	FVi	COORD
	PRESS	PRESS
	TEMP	U
	U	V
	V
Explicit dynamic	CF	CF
	U	COORD
	V	V
Heat transfer	CFL	NT
	CFILM
	FILM
	FVi
	HFL
	NT
Coupled temperature-displacement (implicit)	CF	CF
	CFILM
	CFL	COORD
	FILM	NT
	FVi	U
	HFL
	NT
	PRESS
	U
Coupled pore fluid diffusion/stress (soils)	CF	CFLOW
	CFLOW	COORD
	FLOW	FLOW
	FVi	POR
	POR	U
	PRESS
	TEMP
	U
Quasi-static (visco)	CF	COORD
	FVi	U
	TEMP
	U

Each region can have a separate list of fields to be imported and exported.

Input File Usage:	Use the following option to import data into Abaqus:
	*CO-SIMULATION REGION, IMPORT surface_A, import_field_1 surface_A, import_field_2 surface_B, import_field_3 Use the following option to export data from Abaqus: *CO-SIMULATION REGION, EXPORT surface_A, export_field_1 surface_A, export_field_2 surface_B, export_field_3 For a unidirectional co-simulation specify one of the above options. For a bidirectional co-simulation specify both options.

Abaqus/CAE Usage:

Coupling with third-party analysis programs is not supported in Abaqus/CAE.

Concentrated forces and normal pressure

Both concentrated forces (CF) and normal pressure (PRESS, supported for Abaqus/Standard only), 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 expected in the global coordinate system.

When exporting concentrated forces, Abaqus/Standard transfers reaction forces at interface nodes that have prescribed displacements. The forces are exported in the global coordinate system.

Concentrated normal forces can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CF.

Displacements and current coordinates

Displacements (U) and current coordinates (COORD) can be exported by Abaqus/Standard and Abaqus/Explicit. The displacements are exported in the global coordinate system. The coordinates are the current coordinates of the deformed structure whether small- or large-displacement analysis is performed.

Displacements can be imported into Abaqus/Standard and are ramped from the values of the previous exchange time point to those of the next target time point.

Pore fluid pressure and flow

Pore fluid pressure (POR) and concentrated flow (CFLOW) can be imported and exported for coupled diffusion stress analysis. Fluid flow normal to the element (FLOW) can be exported. The fluid flow exported represents the volume flux at the nodes where pore pressure is prescribed. Both pore pressure and fluid flow are ramped from the values of the previous exchange time point to those of the next target time point in Abaqus/Standard.

Heat flux and film properties

Use surface heat flux (HFL) for a distributed heat flux entering the surface, and use concentrated heat flux (CFL) for a heat source at a node. Both concentrated and distributed heat flux are applicable for transient problems. For steady-state problems you may use film properties (FILM) to model convection governed by

where q is the heat flux entering the surface, h is a film coefficient, 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 analysis computed during the previous exchange interval, according to

Both the film coefficient and fluid temperature are passed into Abaqus and are kept constant over the subsequent exchange interval. When the fluid and wall temperatures coincide, an arbitrary small value for the heat transfer coefficient is passed into Abaqus. To obtain reasonable film properties for the first exchange interval, you should ensure that the wall temperatures are initialized properly in Abaqus and that you provide a good estimate for the initial fluid temperature. Abaqus should initiate the coupling process by initially sending the wall temperatures to the third-party analysis program.

Field variables

Field variables are time-dependent, predefined fields that exist over the spatial domain of the model (see “Predefined fields,” Section 30.6.1, and “Sequentially coupled multiphysics analyses using predefined fields,” Section 14.2.1). The usage and treatment of a field variable is analogous to that of temperature. An example of a field variable is an electromagnetic field. Abaqus has no way of solving such a field; rather, a third-party electromagnetic analysis could be coupled to Abaqus to prescribe the magnitude and time variation of the field over the interface region. Combined with user subroutines, field variables can extend the possibilities of the co-simulation beyond multiphysics.

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.

Different types of analyses have different time integration requirements that will influence or dictate the frequency of interaction between the analysis programs to obtain an accurate and robust solution. For information on defining the rendezvousing scheme for co-simulation, see the following sections:

• “Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 14.1.4

• “Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 14.1.5

• “Rendezvousing schemes for coupling Abaqus to third-party analysis programs,” Section 14.1.6

• For coupling using MpCCI, refer to the Abaqus User's Guide for Multiphysics Simulation Using Abaqus and MpCCI (available from Answer 2420 in the SIMULIA Online Support System).

• For coupling between Abaqus/Explicit and MADYMO, refer to the Abaqus User's Guide for Crash Safety Simulation Using Abaqus/Explicit (available from Answer 2721 in the SIMULIA Online Support System).

The model in Abaqus can be either two-dimensional, three-dimensional, or axisymmetric.

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.

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.

For the coupling with MADYMO you can specify a set of conversion factors for the basic units of mass, length, and time. If a field with the units of length is exported, Abaqus multiplies this quantity by the length unit conversion factor prior to exporting the value to the third-party program. Similarly, if a field with the units of length is imported, Abaqus divides this quantity from the third-party program by the length unit conversion factor prior to using the field in the Abaqus model. The conversion factors are constructed for the various fields that are exchanged based on the conversion factors for the basic units.

*CO-SIMULATION, PROGRAM=MADYMO
mass unit conversion factor, length unit conversion factor, time unit conversion factor

Global convergence of a coupled simulation is assumed when the individual analyses have converged to their specified tolerances, referred to as local convergence. Local convergence for nonlinear Abaqus/Standard problems is discussed in “Solving nonlinear problems,” Section 7.1.1. These Abaqus/Standard criteria are unaffected by the co-simulation interaction with third-party programs and are met before the coupled simulation proceeds to the next coupling step in Abaqus.

The coupling schemes provided are globally explicit; that is, the loads and boundary conditions for the next coupling step are determined based on the solution of the previous coupling step. Hence, the overall convergence of a coupled solution is expected to behave similarly to that of an explicit algorithm; transient problems require a suitable rendezvousing scheme such that data are exchanged with a frequency that ensures overall solution stability.

Interface loads imported into Abaqus/Standard or Abaqus/Explicit are not saved to the Abaqus restart database. Thus, to restart a co-simulation, the third-party analysis program must send the loads at the start of the restart analysis. These loads from the third-party analysis program must balance the current deformation of the Abaqus analysis such that the structure is in equilibrium. It is your responsibility to synchronize the restart information written between the analyses. Furthermore, you must ensure that the simulation is restarted at the same solution (step) time. For example, to restart an FSI co-simulation, the solution time for the particular step/increment number from which Abaqus is restarted must correspond to the third-party analysis solution.