Specifying Co-Simulation Settings in Abaqus

Add co-simulation commands to the Abaqus input file, to specify the co-simulation step, the coupled Abaqus surfaces or nodes, and the fields that are exchanged during the co-simulation.

You can specify the co-simulation settings by either modifying the Abaqus input (*.inp) file manually, or by using the Write Abaqus Keywords option in Simcenter STAR-CCM+. This option instructs Simcenter STAR-CCM+ to automatically add the co-simulation definitions to the Abaqus input (*.inp) file, based on the co-simulation set up in the Simcenter STAR-CCM+ simulation.

To manually specify co-simulation settings in the Abaqus input (*.inp) file:

Open the Abaqus input (*.inp) file with a text editor of your choice.
Include co-simulation to the analysis step, by adding the following options in the history section of the input file:
```
*CO-SIMULATION, NAME=<name>, PROGRAM=MULTIPHYSICS
```
Communication between Abaqus and Simcenter STAR-CCM+ initiates during the co-simulation step and terminates when either program ends the co-simulation. Abaqus terminates the co-simulation event when it reaches the end of the analysis step or when the analysis cannot proceed any further; for example, due to convergence problems.

Define co-simulation regions to specify the Abaqus surfaces or nodes that couple with Simcenter STAR-CCM+ and the fields exchanged across the co-simulation interface.

In the Abaqus .inp file, include separate *CO-SIMULATION REGION definitions to specify the fields that are imported and exported by Abaqus across the coupled surface/node. For each co-simulation region, set TYPE to either SURFACE or NODE and specify the name of the Abaqus coupled surface/node:

For coupling between Simcenter STAR-CCM+ boundaries and Abaqus surfaces, include the following *CO-SIMULATION REGION definitions:

*CO-SIMULATION REGION, TYPE=SURFACE, IMPORT
<surface>, <field_identifier>
<surface>, <field_identifier>

*CO-SIMULATION REGION, TYPE=SURFACE, EXPORT
<surface>, <field_identifier>
<surface>, <field_identifier>

where <surface> is the name of the Abaqus surface (see "Element-based surface definition," Section 2.3.2 of the Abaqus Analysis User’s Guide). In the first co-simulation region definition, <field_identifier> designates the field that Abaqus imports from Simcenter STAR-CCM+ during the co-simulation. In the second co-simulation region definition, <field_identifier> designates the field that Abaqus exports to Simcenter STAR-CCM+ during the co-simulation.

注	For each coupling zone defined in the Simcenter STAR-CCM+ simulation, specify a single unique surface name. This surface can be defined as the union of multiple disconnected surfaces. The same surface name can be specified on multiple lines when defining the imported/exported fields.

For coupling between Simcenter STAR-CCM+ boundaries and Abaqus nodes, include the following *CO-SIMULATION REGION definitions:

*CO-SIMULATION REGION, TYPE=NODE, IMPORT
<node>, <field_identifier>

*CO-SIMULATION REGION, TYPE=NODE, EXPORT
<node>, <field_identifier>

where <node> is the name of a node set, containing a single node, defined on the Abaqus model and the <field_identifier> designates the field that is imported or exported during the co-simulation.

注	For each coupling zone defined in the Simcenter STAR-CCM+ simulation, specify a single unique node name. Coupling between Simcenter STAR-CCM+ boundaries and an Abaqus node is only available when you select Simcenter STAR-CCM+ to be the mapper code.

For more information on the fields that are available for exchange, see 协同仿真交界面和交换场.

Optionally, you can write restart frames during the Abaqus analysis so that you can restart the co-simulation in case of termination of the analysis due to a power outage, etc. The time points in which Abaqus saves a restart frame must be synchronized with the Auto Save settings in Simcenter STAR-CCM+ to provide a consistent state from which to restart the co-simulation.

In the co-simulation step definition, add the following keyword to write n equally spaced (in time) restart frames to the Abaqus restart file during the co-simulation:

*RESTART, WRITE, NUMBER INTERVAL=<n>

注 In Abaqus 2023, when the time-step in Abaqus is smaller than the coupling time interval, Abaqus may ignore the NUMBER INTERVAL keyword specified for the *RESTART command in the Abaqus input (*.inp) file. Therefore, Abaqus may not write the restart frames at the interval specified using the NUMBER INTERVAL keyword.

Additionally, to save only the latest restart frame on the restart file (analogous to setting Max Autosaved Files to 1 in Simcenter STAR-CCM+) use:
```
RESTART, WRITE, NUMBER INTERVAL=<n>, OVERLAY
```