7.9.2 Preparing an ABAQUS analysis for co-simulation

Products: ABAQUS/Standard ABAQUS/Explicit

References

Overview

Preparing an ABAQUS analysis job for co-simulation involves the following:

defining the co-simulation step,
defining the interface region or regions, and
defining the physical quantities to be exchanged during the analysis.

Each of these steps is described in detail below.

Defining a co-simulation step

The ABAQUS co-simulation interface is used in conjunction with existing ABAQUS procedures. In steps where you wish to define a co-simulation, you specify a valid ABAQUS procedure, loads, and boundary conditions irrespective of coupling considerations. You then indicate that the step should be performed as a co-simulation step in which solution quantities will be exchanged with a third-party code. The following procedure types can be used with the ABAQUS co-simulation interface:

Communication with the MpCCI server is initiated at the beginning of the co-simulation step and is terminated at the end of the co-simulation step.

Because a co-simulation involves real-time communication between ABAQUS and a third-party code, with actions required to start and stop the third-party process, you can define only one co-simulation step per analysis job.

Input File Usage:	Use the following option within a step definition to indicate that the step should be a co-simulation:
	*CO-SIMULATION

Defining the interface region

The interface region is a surface that adjoins the domains of a multidisciplinary problem. The surface must be an element-based surface (“Defining element-based surfaces,” Section 2.3.2). Any element type available for the supported procedures can be used in a co-simulation step. Only those element types listed in Table 7.9.2–1 can underlie the interface region.

Table 7.9.2–1 Element types supported by the ABAQUS co-simulation interface.

Description	Element Types
Continuum elements	CPE3(H)(T), CPE4(R)(I)(H)(T), CPS3, CPS4(R)(I)(T),CAX3(H), CAX4(R)(H)(T),C3D4(H), C3D6(H), C3D8(R)(H)(T), C3D10(H), C3D15(H), C3D20(R)(H)(T),DC2D3, DC2D4,DCAX3, DCAX4,DC3D4, DC3D6, DC3D8, DC3D10, DC3D15, DC3D20
Membrane elements	M3D3, M3D4(R), M3D6, M3D8(R), MAX1, MAX2
Shell elements	S3(R), STRI65, S4(R), S4R5, S8R, S8R5, S9R5
Continuum shell elements	SC6R, SC8R

Defining the physical quantities to be exchanged during the co-simulation

For each interface region you must specify the physical quantities that are to be exchanged with the third-party code. Table 7.9.2–2 lists the physical quantities that can be exchanged during a co-simulation and provides the quantity identifier and a description of the quantity.

Table 7.9.2–2 Physical quantity identifiers and quantity types.

Quantity ID	Description	Units
CF	Concentrated nodal force
COORD	Current nodal coordinates
FILM	Film coefficient and ambient temperature (fluid temperature)	,
HFL	Surface heat flux
NT	Wall temperature (or nodal temperature)
PRESS	Normal pressure
U	Nodal displacement

The quantities that can be imported and exported depend on the analysis procedure as defined in Table 7.9.2–3.

Table 7.9.2–3 Physical quantities that can be imported/exported for a particular ABAQUS procedure.

Procedure	Import	Export
“Static stress analysis,” Section 6.2.2	CF, PRESS	COORD, U
“Implicit dynamic analysis using direct integration,” Section 6.3.2	CF, PRESS	COORD, U
“Explicit dynamic analysis,” Section 6.3.3	CF, PRESS	COORD, U
“Uncoupled heat transfer analysis,” Section 6.5.2	HFL, FILM	NT
“Fully coupled thermal-stress analysis,” Section 6.5.4 (ABAQUS/Standard only)	CF, HFL, FILM, PRESS	COORD, U, NT

Input File Usage:

Use the following option to specify the data to be received from the third-party code:

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

Use the following option to specify the data to be sent to the third-party code:

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

Current nodal coordinates and displacements

Use current nodal coordinates (COORD) rather then nodal displacements (U) for FSI simulations, since typical CFD codes do not maintain the original structural geometry.

The definition of COORD is the current nodal coordinates, irrespective of whether small- or large-deformation analysis is performed. This definition differs from the usual ABAQUS convention, in which the original coordinates are not updated in small-deformation analysis.

Displacements are always exchanged in the global coordinate system. If a local transformation (“Transformed coordinate systems,” Section 2.1.5) exists at a node, ABAQUS will transform the displacements to the global coordinate system prior to sending them to the MpCCI server.

Concentrated forces and normal pressure

Use concentrated nodal forces (CF) rather than normal pressure (PRESS) when viscous shear forces are important in the FSI simulation. Both concentrated forces and normal pressure are ramped from the end of the previous coupling step to the target time in ABAQUS/Standard and are kept constant over the coupling step in ABAQUS/Explicit.

Concentrated forces are always exchanged in the global coordinate system. If a local transformation (“Transformed coordinate systems,” Section 2.1.5) exists at a node, ABAQUS transforms the concentrated loads to a local coordinate system prior to applying them.

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

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

is the heat flux entering the surface,

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 CFD analysis and the wall temperature from the ABAQUS analysis computed during the previous coupling step, according to

Both the film coefficient and fluid temperature are passed into ABAQUS and are kept constant over the subsequent coupling step. 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 coupling step, 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.

Unit system

ABAQUS does not require that the analysis be run with a particular unit system. However, in a co-simulation the unit system used by ABAQUS must coincide with the internal unit system of the third-party code. The MpCCI configuration file provides a mechanism to perform unit transformations; see the MpCCI User's Manual for further details.

Model dimension and coordinate systems

Vector quantities are transferred according to ABAQUS conventions; the first component represents the quantity along the -axis, the second quantity represents the quantity along the -axis, and the third quantity represents the quantity along the -axis (for three-dimensional models).

Care must be taken for axisymmetric models. In ABAQUS the axis of revolution is about the -axis, which may not be the case for the third-party code. MpCCI provides a mapping tool to transform results between different coordinate systems; see the MpCCI User's Manual for further details.

Limitations

A restart of a co-simulation step may not be performed if ABAQUS is receiving loads from the third-party code. Such loads are not applied at the beginning of the increment and, thus, may lead to convergence problems.
Double-sided surfaces on shell elements are not allowed. Specify two surfaces representing the top and bottom interface regions instead.