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 a step and end within that 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 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. The co-simulation technique can be used with the following procedure types in ABAQUS:

*CO-SIMULATION, NAME=name

You can choose either the MpCCI, typically for fluid-structure interaction (FSI) problems, or the MADYMO program, typically for crash safety simulation problems, to communicate with ABAQUS during a co-simulation.

*CO-SIMULATION, PROGRAM=MPCCI

*CO-SIMULATION, PROGRAM=MADYMO

Interaction between the ABAQUS model and the third-party analysis software model takes place through a common interface region. In ABAQUS the interface region can consist of one or more element-based surfaces (see “Defining element-based surfaces,” Section 2.3.2).

The model data defining the interface region, such as the surface name and user-given element and node labels of the underlying region, are exported to the third-party analysis software. You can use these data to pair the interface regions between ABAQUS and the third-party analysis software. For further information about pairing interface regions with the third-party analysis software, consult the ABAQUS User's Guide for Fluid-Structure Interaction Using ABAQUS and FLUENT or the ABAQUS User's Guide for Crash Safety Simulation Using ABAQUS/Explicit and MADYMO.

*CO-SIMULATION REGION 
surface_A,
surface_B, 

The coupling of the subdomain 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 13.1.2–1 lists the solution quantities and the quantity identifiers that can be exchanged during a co-simulation.

Table 13.1.2–1 Solution quantity identifiers and quantity types.

Quantity ID	Description	Units
CF	Concentrated nodal force	F
COORD	Current nodal coordinates	L
FILM	Film coefficient and ambient temperature (fluid temperature)	,
FV1–FV19	Field variables 1–19
HFL	Surface heat flux
NT	Wall temperature (or nodal temperature)
PRESS	Normal pressure
TEMP	Nodal temperature for a stress analysis
U	Nodal displacement	L
VEL	Nodal velocities	L/T

Each region can have a separate list of solution quantities to be imported and exported. For coupling between ABAQUS/Explicit and MADYMO, ABAQUS needs to export only the coordinates and import only the concentrated nodal force (see “The solution quantities exchanged with MADYMO” in “Co-simulation with MADYMO,” Section 13.1.4).

*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. 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.

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.

Any vector quantity that is exported is 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.

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 software model. When the two unit systems differ, the solution quantities exchanged between the two programs must go through a transformation of units.

In the case of co-simulation using MpCCI, the unit transformation is performed by MpCCI (see the MpCCI User's Manual for further details).

In the case of co-simulation with MADYMO, ABAQUS provides a method for conversion between the unit systems (see “Co-simulation with MADYMO,” Section 13.1.4).