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 a general open interface through the Mesh-based Parallel Code Coupling Interface and a direct coupling interface for coupling to third-party analysis programs.

*CO-SIMULATION, PROGRAM=MPCCI 

*CO-SIMULATION, PROGRAM=ACUSOLVE 

*CO-SIMULATION, PROGRAM=MADYMO 

*CO-SIMULATION, PROGRAM=ABAQUS 

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

*CO-SIMULATION REGION
surface_A, quantity

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

*CO-SIMULATION REGION, TYPE=NODE
nodeset_A

*CO-SIMULATION REGION, TYPE=SURFACE
surface_A

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 solution quantities that need to be exchanged during the simulation. Table 14.1.2–1 lists all the solution quantities and the associated quantity identifiers that can be exchanged during a co-simulation.

Table 14.1.2–1 Solution quantity identifiers and quantity types.

Quantity ID	Description	Units
CF	Concentrated force at a node when imported into Abaqus. Reaction force at a node when exported from Abaqus/Standard.	F
CFL	Concentrated heat flux at a node when imported into Abaqus/Standard.
CFLOW	Concentrated pore fluid flow at a node when imported into Abaqus/Standard. Reaction volume flux at a node when exported from Abaqus/Standard.
COORD	Nodal coordinates	L
FILM	Film coefficient and ambient temperature (fluid temperature)	,
FLOW	Pore fluid flow normal to the surface of an element
FV1–FV19	Field variables 1–19 at a node
HFL	Heat flux normal to the surface of an element
NT	Wall temperature at a node
POR	Pore fluid pressure at a node
PRESS	Normal pressure normal to the surface of an element
TEMP	Temperature at a node in a stress analysis
U	Displacements	L
V	Velocities

The choice of appropriate quantities depends on the Abaqus analysis procedure and the third-party analysis program. Solution quantities that can be imported and exported into/from Abaqus depend on the analysis procedure as defined in Table 14.1.2–2. Consult the appropriate User's Guide for solution quantities available for particular third-party analysis programs.

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

*CO-SIMULATION REGION, IMPORT
surface_A, quantity_I1
surface_A, quantity_I2
surface_B, quantity_I3 	

*CO-SIMULATION REGION, EXPORT
surface_A, quantity_E1
surface_A, quantity_E2
surface_B, quantity_E3

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.

For co-simulation using MpCCI and the coupling between Abaqus and AcuSolve, refer to “Performing a co-simulation using MpCCI or coupling Abaqus and AcuSolve,” Section 14.1.4. For coupling between Abaqus/Explicit and MADYMO, refer to the Abaqus User's Guide for Crash Safety Simulation Using Abaqus/Explicit and MADYMO. For coupling between Abaqus/Standard and Abaqus/Explicit, refer to “Performing an Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 14.1.3.

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 User's Guide for further modeling details.

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 solution quantities exchanged between the two programs must go through a transformation of units. Refer to the appropriate User's Guide 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 solution quantity 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 solution quantity 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 solution quantity in the Abaqus model. The conversion factors are constructed for the various solution quantities 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 or actuators imported into Abaqus 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.