Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE
“Rendezvousing schemes for coupling Abaqus to third-party analysis programs,” Section 16.1.3
“Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 16.1.4
“Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 16.1.5
Preparing an Abaqus analysis for co-simulation involves the following:
identifying the Abaqus analysis step for a co-simulation analysis;
identifying the analysis program, which may be a separate Abaqus analysis, that is communicating with Abaqus during the co-simulation analysis;
identifying the interface regions in the Abaqus model;
identifying the fields exchanged during the co-simulation event; and
defining the rendezvousing scheme.
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 the coupled analysis 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.
| Input File Usage: | Use the following option within a step definition to indicate the beginning of a co-simulation event: |
*CO-SIMULATION, NAME=name |
| Abaqus/CAE Usage: | Use the following option for an Abaqus/Standard to Abaqus/Explicit co-simulation: |
Interaction module: Create Interaction: Standard-Explicit co-simulation: Name: name Use the following option for an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation: Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary: 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.
You can couple an Abaqus/Standard analysis to an Abaqus/Explicit analysis.
| Input File Usage: | *CO-SIMULATION, PROGRAM=ABAQUS |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Standard-Explicit co-simulation |
You can couple Abaqus/CFD with Abaqus/Standard or with Abaqus/Explicit using the SIMULIA Co-Simulation Engine.
| Input File Usage: | *CO-SIMULATION, PROGRAM=MULTIPHYSICS |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary |
You can couple Abaqus with certain third-party analysis programs using the direct coupling interface or the SIMULIA Co-Simulation Engine. Consult the third-party program documentation for information regarding the option to specify.
| Input File Usage: | Use the following option when coupling Abaqus using the direct coupling interface: |
*CO-SIMULATION, PROGRAM=DCI Use the following option when coupling Abaqus using the SIMULIA Co-Simulation Engine: *CO-SIMULATION, PROGRAM=MULTIPHYSICS |
| Abaqus/CAE Usage: | Coupling with third-party analysis programs is not supported in Abaqus/CAE. |
You can use MpCCI to communicate with any third-party analysis program that is MpCCI compliant. MpCCI is a third-party connectivity program for general multidisciplinary simulation and is distributed by the Fraunhofer-Institute for Algorithms and Scientific Computing. In this case Abaqus communicates with the MpCCI server, which in turn communicates with the third-party analysis program.
| Input File Usage: | *CO-SIMULATION, PROGRAM=MPCCI |
| Abaqus/CAE Usage: | Coupling with third-party analysis programs is not supported in Abaqus/CAE. |
You can couple Abaqus/Explicit with the MADYMO program for crash safety simulation problems. MADYMO is distributed by TNO, MADYMO BV.
| Input File Usage: | *CO-SIMULATION, PROGRAM=MADYMO |
| Abaqus/CAE Usage: | Coupling with third-party analysis programs is not supported in Abaqus/CAE. |
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.
You can specify an interface region using either node sets or surfaces when coupling Abaqus/Standard to Abaqus/Explicit. You must, however, be consistent in your region definition in Abaqus/Standard and Abaqus/Explicit; if you define a co-simulation region with a node set or node-based surface in one analysis, you must use the same type of co-simulation region definition in the other analysis. Likewise, if you define a co-simulation region with an element-based surface in one analysis, you must define your co-simulation region with an element-based surface in the other analysis.
You may have dissimilar meshes in regions shared in the Abaqus/Standard and Abaqus/Explicit model definitions. In some cases, however, you can improve solution stability and accuracy by ensuring that you have matching nodes at the interface (see “Dissimilar mesh-related limitations” in “Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 16.1.4). In these cases you can use the modeling practice described in “Ensuring matching nodes at the interface regions,” Section 26.4 of the Abaqus/CAE User's Manual, to ensure these matching nodes.
| 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 option to define an element-based or node-based surface as a co-simulation region in an Abaqus model: *CO-SIMULATION REGION, TYPE=SURFACE (default) surface_A Only one *CO-SIMULATION REGION option can be defined in each Abaqus analysis. In addition, only one node set or surface can be defined. |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Standard-Explicit co-simulation: Surface or Node Region: select region |
You specify an interface region using surfaces when coupling Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit. You must define an element-based surface, and you can specify only one surface to be used as the interface region in the analysis. You may have dissimilar meshes in regions shared in the model definitions.
| Input File Usage: | Use the following option to define an element-based surface as a co-simulation region: |
*CO-SIMULATION REGION, TYPE=SURFACE surface_A |
| Abaqus/CAE Usage: | Interaction module: Create Interaction: Fluid-Structure Co-simulation boundary: select surface region |
In Abaqus the interface region can consist of one or more element-based surfaces (see “Element-based surface definition,” Section 2.3.2).
The model data defining the interface region, such as the surface name and element and node labels of the underlying region, are exported to the third-party analysis program. You can use these data within the third-party analysis program model definition to pair the interface regions of the two models. For further information about pairing interface regions with a third-party analysis program, consult the third-party program documentation.
| Input File Usage: | Use the following option to identify the interface regions and the quantities being imported or exported: |
*CO-SIMULATION REGION surface_A, quantity |
| Abaqus/CAE Usage: | Coupling with third-party analysis programs is not supported in Abaqus/CAE. |
When coupling with MADYMO, an integer identifier can be assigned to each interface region in the Abaqus model. These identifiers, and not the surface names, are used when defining the interface regions exported to MADYMO. You can define groups in the MADYMO model by selecting the desired region identifiers, the node numbers, and/or the element numbers from the Abaqus model.
| Input File Usage: | Use the following options to define a co-simulation region in an Abaqus model using an integer identifier: |
*CO-SIMULATION REGION, REGION ID=n surface_A, surface_B, Repeat the *CO-SIMULATION REGION option to define interface regions with different integer identifiers. |
| Abaqus/CAE Usage: | Coupling with third-party analysis programs is not supported in Abaqus/CAE. |
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. Table 16.1.2–1 lists all the fields and their associated field identifiers that are available for co-simulation exchange. Fields that can be imported into and exported from Abaqus depend on the analysis procedure as defined in Table 16.1.2–2.
For 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.
For Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation, see Table 16.1.2–2. When using Abaqus/CAE, the fields exchanged are determined automatically by Abaqus/CAE.
For co-simulation with third-party analysis programs, the fields that can be imported into and exported from Abaqus/Standard or Abaqus/Explicit depend on the analysis procedure as defined in Table 16.1.2–2. For fields available for a particular third-party analysis program, consult the third-party program documentation.
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.
Table 16.1.2–1 Fields and identifiers available for co-simulation exchange.
| Field ID | Fields | Units |
|---|---|---|
| CF | Force 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 |  |
| LUMPEDHEATCAPACITANCE | Lumped heat capacitance at a node |  |
| LUMPEDMASS | Lumped mass at a node | M |
| 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 | |
| TRSHR | Traction vector | F |
| U | Displacement | L |
| V | Velocity | |
Table 16.1.2–2 Fields available for import to and export from Abaqus for particular procedures.
| Procedure description | Import | Export |
|---|---|---|
| Static | CF FVi PRESS TEMP U | CF COORD PRESS U |
| Implicit dynamic | CF FVi LUMPEDMASS PRESS TEMP U V | CF COORD PRESS U V |
| Explicit dynamic | CF LUMPEDMASS U V | CF COORD V |
| Heat transfer | CFL CFILM FILM FVi HFL LUMPEDHEATCAPACITANCE NT | NT |
| Coupled temperature-displacement (implicit) | CF CFILM CFL FILM FVi HFL NT PRESS U | CF COORD NT U |
| Incompressible fluid dynamic (for fluid-structure interaction) | U V | LUMPEDMASS TRSHR |
| Incompressible fluid dynamic (for conjugate heat transfer) | TEMP | HFL LUMPEDHEATCAPACITANCE |
| Coupled pore fluid diffusion/stress (soils) | CF CFLOW FLOW FVi POR PRESS TEMP U | CFLOW COORD FLOW POR U |
| Quasi-static (visco) | CF FVi TEMP U | COORD U |
| 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 Use the following option to export data from Abaqus: *CO-SIMULATION REGION, EXPORT surface_A, export_field_1 surface_A, export_field_2 When using the direct coupling interface, each region can have a separate list of fields to be imported and exported. For a unidirectional co-simulation specify one of the options below. For a bidirectional co-simulation specify both options. *CO-SIMULATION REGION, IMPORT surface_A, import_field_1 surface_A, import_field_2 surface_B, import_field_3 *CO-SIMULATION REGION, EXPORT surface_A, export_field_1 surface_A, export_field_2 surface_B, export_field_3 |
| Abaqus/CAE Usage: | The fields exchanged during a co-simulation with Abaqus/CFD are determined automatically in Abaqus/CAE. Coupling with third-party analysis programs is not supported in Abaqus/CAE. |
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 and normal pressure can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variables CF and P, respectively.
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 (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.
Concentrated fluid flow can be viewed in the Visualization module of Abaqus/CAE for a coupled diffusion stress analysis by requesting output variable CFF.
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
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
Concentrated heat flux values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CFL.
Field variables are time-dependent, predefined fields that exist over the spatial domain of the model (see “Predefined fields,” Section 32.6.1, and “Sequentially coupled multiphysics analyses using predefined fields,” Section 16.2.1). The usage and treatment of a field variable is analogous to that of temperature. Temperature (TEMP) can be imported as a field variable. 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.
Predefined field variables and temperature (as a field variable) can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variables FV and NT, respectively.
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:
“Rendezvousing schemes for coupling Abaqus to third-party analysis programs,” Section 16.1.3
“Abaqus/Standard to Abaqus/Explicit co-simulation,” Section 16.1.4
“Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation,” Section 16.1.5
For coupling using MpCCI, refer to “Abaqus User's Guide for Fluid-Structure Interaction (FSI)” in the Dassault Systèmes DSX.ECO Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com.
For coupling between Abaqus/Explicit and MADYMO, refer to “Using coupling between Abaqus/Explicit and MADYMO in Abaqus” in the Dassault Systèmes DSX.ECO Knowledge Base at www.3ds.com/support/knowledge-base or the SIMULIA Online Support System, which is accessible through the My Support page at www.simulia.com.
Three-dimensional Abaqus models are fully supported. Two-dimensional and axisymmetric Abaqus models are supported only for Abaqus/Standard to Abaqus/Explicit co-simulation and coupling using MpCCI. 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.
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.
| Input File Usage: | Use the following option to specify unit conversion factors when there is a mismatch in unit systems between the Abaqus/Explicit model and the MADYMO model: |
*CO-SIMULATION, PROGRAM=MADYMO mass unit conversion factor, length unit conversion factor, time unit conversion factor |
| Abaqus/CAE Usage: | Coupling with third-party analysis programs is not supported in Abaqus/CAE. |
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, 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 loads at the start of the restart analysis. These loads must balance the current deformation of the Abaqus analysis such that the structure is in equilibrium. 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. 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 coupled analysis solution.
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).
For co-simulation based on surface coupling, the following additional limitations apply:
A surface defined over beam, pipe, and truss elements or defined over the edges of three-dimensional elements cannot be used as an interface region.
Use of mixed geometric primitives underlying the interface region (i.e., use of triangles and quadrilaterals or use of bricks and tetrahedrals) is not supported when communicating with the SIMULIA Co-Simulation Engine.
A surface defined over modified triangular elements or modified tetrahedral elements cannot be used as an interface region.
There may be further limitations depending on the third-party analysis program being used. For more information, refer to the appropriate third-party program documentation.