MultiPhysicsVault/.raw/AbaqusAnalysisUserGuide2/AbaqusAnalysisUserGuide2_141.md

Defining the rendezvousing scheme

For structural-to-structural co-simulation, you must specify co-simulation controls for each analysis and create a configuration file; the consistency of the parameters is confirmed during execution. The SIMULIA Co-Simulation Engine configuration file is used to define the time incrementation process and the frequency of exchange between the two Abaqus analyses. Abaqus/CAE automatically creates and uses this configuration file. If you are not using Abaqus/CAE to perform the co-simulation, you must create the configuration file manually.

Predefined templates are available for the following co-simulation schemes:

• You can force Abaqus/Standard to use the same increment size as Abaqus/Explicit, or
• you can allow the increment sizes in Abaqus/Standard to differ from those in Abaqus/Explicit (subcycling).

You refer to these predefined templates when you create your configuration files.

Input File Usage: Use both of the following options to specify co-simulation controls:

*CO-SIMULATION, PROGRAM=ABAQUS, CONTROLS=name

*CO-SIMULATION CONTROLS, NAME=name

Abaqus/CAE Usage: Interaction module: Create Interaction: Standard-Explicit co-simulation

Time incrementation scheme

You can force Abaqus/Standard to use the same increment size as Abaqus/Explicit, or you can allow the increment sizes in Abaqus/Standard to differ from those in Abaqus/Explicit (subcycling). The time incrementation scheme that you choose for coupling affects the solution computational cost and accuracy but not the solution stability.

The subcycling scheme is frequently the most cost effective since Abaqus/Standard time increments, free of any forced co-simulation time incrementation constraints, are commonly much longer than Abaqus/Explicit time increments. The subcycling scheme, however, may be less cost effective when a large portion of the nodes in the model are at the co-simulation interface. This is because Abaqus/Standard performs a set of stabilization operations at the interface (a “free solve”) for each increment in the Abaqus/Explicit analysis. These free-solve operations require an implicit solution of a dense system of equations that scale with the number of interface nodes. In cases of a large number of interface nodes the computational cost of this interface solve can exceed any cost savings seen due to subcycling. Hence, for a model where a significant share of the nodes are at the co-simulation interface performance may be poorer with the subcycling scheme.

Forcing Abaqus/Standard to use the same increment size as Abaqus/Explicit

You can force Abaqus/Standard to match the increment size of Abaqus/Explicit, and fields will be exchanged at each of the shared increments.

Input File Usage: Use the following option in the Abaqus/Standard analysis and in the Abaqus/Explicit analysis:

*CO-SIMULATION CONTROLS, TIME INCREMENTATION=LOCKSTEP

Abaqus/CAE Usage: Use the following input in the Abaqus/Standard analysis and in the Abaqus/Explicit analysis:

Interaction module: Create Interaction: Standard-Explicit co-simulation: Incrementation control: Lock time steps

Allowing the increment sizes in Abaqus/Standard to differ from those in Abaqus/Explicit

You can allow the Abaqus/Standard increment size to differ from those in Abaqus/Explicit (subcycling). In this case fields will be exchanged as needed.

Input File Usage: Use the following option in the Abaqus/Standard analysis and in the Abaqus/Explicit analysis:

*CO-SIMULATION CONTROLS,TIME INCREMENTATION=SUBCYCLE

Abaqus/CAE Usage: Use the following input in the Abaqus/Standard analysis and in the Abaqus/Explicit analysis:

Interaction module: Create Interaction: Standard-Explicit co-simulation: Incrementation control: Allow subcycling

Controlling interface matrix factorization frequency

For the subcycling time incrementation scheme an interface solve is performed, by default, in Abaqus/Standard for every Abaqus/Explicit increment. This solve can be significantly costly for two reasons. First, the interface matrix used for the interface solve is dense and its size scales with the number of interface nodes. Second, the interface matrix changes every Abaqus/Explicit increment, requiring factorization in Abaqus/Standard for every Abaqus/Explicit increment. You can reduce the impact of this cost by approximating the interface matrix and factorizing it typically once for the duration of an Abaqus/Standard increment, rather than for each Abaqus/Explicit increment. However, if the Abaqus/Explicit stable time increment changes significantly, the interface matrix is refactored for stability reasons.

Allowing Abaqus/Standard to factorize the interface matrix every Abaqus/Explicit increment

Factorizing the interface matrix every Abaqus/Explicit increment is the default approach.

Input File Usage: Use the following option in the Abaqus/Standard analysis:

*CO-SIMULATION CONTROLS,FACTORIZATION FREQUENCY=EXPLICIT INCREMENT

Abaqus/CAE Usage: Factorizing the interface matrix every Abaqus/Explicit increment is used by default in Abaqus/CAE.

Forcing Abaqus/Standard to factorize the interface matrix once per Abaqus/Standard increment

When the number of interface nodes is large, the cost of the interface factorization can be significantly reduced by using this approach. Only the interface matrix factorization is performed once per

Abaqus/Standard increment; the interface solve is performed every Abaqus/Explicit increment using this factorized interface matrix. Since this approach approximates the interface matrix, it may slightly increase the drift in the displacement solution at the co-simulation interface. The performance gain with this method depends on the number of interface nodes, the subcycling ratio (which is the ratio between Abaqus/Standard and Abaqus/Explicit increments), and the size of the models. For models with greater than 100 interface nodes and a subcycling ratio greater than 50, this method typically reduces the analysis time by a factor between 1.2 and 3.0. The performance gain increases for larger subcycling ratios and decreases for larger models.

Input File Usage: Use the following option in the Abaqus/Standard analysis:

\mathrm { ^ { * } C O - S I M U L A T I O N \ C O N T R O L S } ,

\mathrm { F A C T O R I Z A T I O N F R E Q U E N C Y = S T A N D A R D \ I N C R E M E N T }

Abaqus/CAE Usage: Factorizing the interface matrix once per Abaqus/Standard increment is not supported in Abaqus/CAE.

Coupling step size

The coupling step size is the period between two consecutive co-simulation data exchanges between Abaqus/Standard and Abaqus/Explicit and always equals the current Abaqus/Explicit increment size.

When using the subcycling method, this data exchange does not represent a constraint on Abaqus/Standard incrementation; the Abaqus/Standard analysis advances in time using its normal time incrementation logic.

Creating a configuration file

You can use predefined templates to create a configuration file for the coupling schemes described above. Table 17.3.1–1 describes the two predefined templates available for Abaqus/Standard to Abaqus/Explicit co-simulation and lists example configuration files that you can review.

Table 17.3.1–1 Templates for structural-to-structural co-simulation.

Structural-to-structural co-simulation: subcycling	Coupling scheme: Allow Abaqus/Explicit to subcycle
	template_std_xpl_subcycle
	Example file: exa_std_xpl_subcycle.xml
Structural-to-structural co-simulation: lockstep	Coupling scheme: Abaqus/Standard and Abaqus/Explicit use a single increment per coupling step (lockstep)
	template_std_xpl_lockstep
	Example file: exa_std_xpl_lockstep.xml

To obtain an example configuration file, you can use the abaqus fetch utility. For example, to obtain the example for Abaqus/Standard to Abaqus/Explicit subcycling, use the following command:

abaqus fetch job=exa_std_xpl_lockstep

The example file exa_std_xpl_lockstep.xml is shown below.

<?xml version="1.0" encoding="utf-8"?>
<CoupledMultiphysicsSimulation>
    <template_std_xpl_subcycle>
    <Standard_Job>standard_job_name</Standard_Job>
    <Explicit_Job>explicit_job_name</Explicit_Job>
    <duration>duration_value</duration>
    </template_std_xpl_subcycle>
</CoupledMultiphysicsSimulation> 

In certain cases you may need to use co-simulation configuration features that are not described in the predefined templates. For example, you may wish to change the dissimilar mesh mapping search tolerances; these tolerances are available generally in the configuration file but are not described in the predefined templates. For these cases, you must create an elaborated configuration file; for more information, see “Using elaborated configuration files” in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1.

Executing the coupled analysis

You execute the co-simulation interactively in Abaqus/CAE or from the command line, as described in “Executing a co-simulation,” Section 17.3.4.

Diagnostics information

The Abaqus/Standard job provides detailed descriptions of co-simulation operations in the message (.msg) file. For the subcycling scheme the status (.sta) file provides summary information indicating when the interface calculations followed by re-solve of the increment are made, as shown in the following example status file. The E suffix in the attempt-count entry (column 3) indicates an increment performing interface calculations. An increment without the E suffix indicates re-solve of the increment.

SUMMARY OF JOB INFORMATION:
STEP	INC	ATT	SEVERE	EQUIL	TOTAL	TOTAL	STEP	INC OF	DOF	IF
			DISCON	ITERS	ITERS	TIME/	TIME/LPF	TIME/LPF	MONITOR	RIKS
			ITERS			FREQ
1	1	1E	0	1	1	0.000	0.000	0.001000
1	1	1	0	3	3	0.00100	0.00100	0.001000
1	2	1E	0	1	1	0.00100	0.00100	0.001000
1	2	1	0	3	3	0.00200	0.00200	0.001000
1	3	1E	0	1	1	0.00200	0.00200	0.001000
1	3	1	0	2	2	0.00300	0.00300	0.001000
1	4	1E	0	1	1	0.00300	0.00300	0.001000
1	4	1	0	3	3	0.00400	0.00400	0.001000

The Abaqus/Explicit job provides summary descriptions of co-simulation operations in the status (.sta) file.

The following limitations apply to Abaqus/Standard to Abaqus/Explicit co-simulation in addition to the limitations discussed in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1.

General limitations

• Displacement compatibility at the co-simulation interface is not maintained when you allow the Abaqus/Standard increment size to differ from that in Abaqus/Explicit (i.e., when you specify subcycling as a co-simulation time incrementation control). In this case velocity compatibility is maintained, but you may see small amounts of displacement mismatch between Abaqus/Standard and Abaqus/Explicit as the simulation advances in time. This “drift” is more pronounced if severe nonlinearity such as plastic deformation occurs at the co-simulation interface. You can control this drift by adjusting Abaqus/Standard solution parameters so that the Abaqus/Standard increment size is reduced (e.g., by limiting the maximum time increment size or specifying a smaller half-increment residual tolerance for implicit dynamic analyses).
• Nodal transformations are not permitted on the co-simulation region nodes.
• The ALE technique may not be used in elements attached to co-simulation region nodes.
• Fully coupled temperature-displacement elements can be used, but no temperature quantities are exchanged.
• An Abaqus/Standard static stress analysis cannot be used with the lockstep time incrementation scheme in Abaqus/Standard to Abaqus/Explicit co-simulation.
• Only points and surface regions are allowed; coupling volume regions is not supported.
• Only a single region can be defined as the interface region; multiple interface regions are not supported.

Dissimilar mesh-related limitations

When your Abaqus/Standard and Abaqus/Explicit co-simulation region meshes differ, the following limitations apply:

• Solution accuracy may be affected when your co-simulation region meshes are not uniform in the presence or absence of rotational degrees of freedom; for example, if a continuum element mesh is locally reinforced with beam or shell elements at the co-simulation region interface.
• In cases where the stress state near the co-simulation interface is significant (approaching 1% or more) relative to the material stiffness, you may observe appreciable irregular mesh distortion if the mesh density adjacent to the co-simulation region differs greatly between the Abaqus/Explicit and Abaqus/Standard models. For example, this effect is common with large deformation of hyperelastic materials. You can minimize this effect by choosing a similar or finer mesh at the Abaqus/Standard co-simulation region when using the subcycling time integration scheme or by choosing a similar or finer mesh at the Abaqus/Explicit co-simulation region when using the lockstep time integration scheme.

Abaqus/Standard analysis limitations

Abaqus/Standard elements that have no equivalent degree-of-freedom counterpart in Abaqus/Explicit cannot be connected to co-simulation region nodes. These elements include

• Axisymmetric elements with twist degrees of freedom (the CGAX element family)
• Axisymmetric solid elements with asymmetric deformation (the CAXA element family)
• Generalized plane strain elements (the CPEG element family)
• Coupled pore pressure-displacement elements
• Heat transfer and thermal-electrical elements
• Acoustic elements
• Piezoelectric elements

The following specific limitations also apply:

• A co-simulation region node cannot be a slave node in a tie constraint, an MPC constraint, or a kinematic coupling constraint.

Abaqus/Explicit analysis limitations

Stability and accuracy of the co-simulation solution may be adversely affected when the following model features are defined at or near the co-simulation region:

• Connector elements connected to co-simulation region nodes.
• Co-simulation region nodes that participate in a tie constraint, an MPC constraint, or a kinematic coupling constraint.

When using these features, you should compare the Abaqus/Standard and Abaqus/Explicit solutions (e.g., compatibility of the displacement history) at the co-simulation interface as an indicator of solution accuracy.

17.3.2 FLUID-TO-STRUCTURAL AND CONJUGATE HEAT TRANSFER CO-SIMULATION

Products: Abaqus/Standard Abaqus/Explicit Abaqus/CFD Abaqus/CAE

References

• “Co-simulation: overview,” Section 17.1.1
• “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1
• *CO-SIMULATION
• *CO-SIMULATION CONTROLS
• Chapter 26, “Co-simulation,” of the Abaqus/CAE User’s Guide

• “Defining a fluid-structure co-simulation interaction,” Section 15.13.15 of the Abaqus/CAE User’s Guide, in the HTML version of this guide

Overview

This section discusses analysis setup, execution, and limitation details specific to fluid-to-structural cosimulation and conjugate heat transfer using Abaqus/CFD and Abaqus/Standard or Abaqus/Explicit.

Refer to “Conjugate heat transfer analysis of a component-mounted electronic circuit board,” Section 6.1.1 of the Abaqus Example Problems Guide, for an example of conjugate heat transfer.

Identifying the Abaqus step for the co-simulation analysis

The following Abaqus/CFD analysis procedure can be used for co-simulation with Abaqus/Standard or Abaqus/Explicit:

• “Incompressible fluid dynamic analysis,” Section 6.6.2

The following Abaqus/Standard analysis procedures can be used for co-simulation with Abaqus/CFD:

• “Implicit dynamic analysis using direct integration,” Section 6.3.2

• “Uncoupled heat transfer analysis,” Section 6.5.2

The following Abaqus/Explicit analysis procedures can be used for co-simulation with Abaqus/CFD:

• “Explicit dynamic analysis,” Section 6.3.3
• “Fully coupled thermal-stress analysis in Abaqus/Explicit” in “Fully coupled thermal-stress analysis,” Section 6.5.3

Input File Usage: Use the following option within a step definition for an Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation:

*CO-SIMULATION, PROGRAM=MULTIPHYSICS

Abaqus/CAE Usage: 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

Identifying the co-simulation interface 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

Identifying the fields exchanged across a co-simulation interface

For Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation, see the tables in “Identifying the fields exchanged across a co-simulation interface” in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1, for lists of fields that are available for co-simulation exchange. When using Abaqus/CAE, the fields exchanged are determined automatically by Abaqus/CAE.

Defining the rendezvousing scheme

The SIMULIA Co-Simulation Engine configuration file is used to define the time incrementation process and the frequency of exchange between the two Abaqus analyses. Abaqus/CAE automatically creates and uses this configuration file. If you are not using Abaqus/CAE to perform the co-simulation, you must create the configuration file manually.

Predefined templates are available for commonly used coupling schemes. You refer to these templates when you create configuration files. This section describes the rendezvous scheme settings and predefined configuration file templates.

Defining the coupling scheme

The sequential explicit coupling scheme (also referred to as the Gauss-Seidel coupling algorithm) is the only coupling scheme available for Abaqus/CFD to Abaqus/Standard or to Abaqus/Explicit co-simulation. In all of the predefined templates, the Abaqus/CFD analysis lags the co-simulation and the Abaqus/Standard or Abaqus/Explicit analysis leads the co-simulation. For conjugate heat transfer, the Abaqus/CFD analysis can either lag or lead the co-simulation. For fluid-structure interaction, the Abaqus/CFD analysis must lag the co-simulation and the Abaqus/Standard or Abaqus/Explicit analysis must lead the co-simulation.

Coupling step size

The coupling step size is the period between two consecutive co-simulation data exchanges. The coupling step size is determined automatically based on the type of analysis and is used to obtain time-accurate solutions for the coupled physics problem. For fluid-structure interaction (FSI) and conjugate heat transfer (CHT) analyses that couple Abaqus/CFD and Abaqus/Standard, the coupling step size is the minimum of the time step sizes determined by the automatic time incrementation schemes of the individual analyses. For FSI problems that couple Abaqus/CFD and Abaqus/Explicit, Abaqus/Explicit imports the coupling step size from Abaqus/CFD; consequently, Abaqus/CFD exports the coupling step size to Abaqus/Explicit.

Time incrementation scheme

Depending on the type of analysis, Abaqus may either perform one increment (referred to as “lockstep”) or several increments (referred to as “subcycling”) per coupling step. For FSI analyses that couple Abaqus/CFD and Abaqus/Explicit, Abaqus/Explicit typically uses subcycling while Abaqus/CFD uses lockstep behavior.

Creating a configuration file

You can use predefined templates to create a configuration file for the coupling schemes described above. Table 17.3.2–1 describes the predefined templates available for fluid-to-structural co-simulation and conjugate heat transfer and lists example configuration files that you can review.

To obtain an example configuration file, you can use the abaqus fetch utility. For example, to obtain the example for Abaqus/Standard to Abaqus/CFD conjugate heat transfer, use the following command:

abaqus fetch job=exa_std_cfd_cht 

The example file exa_std_cfd_cht is shown below.

<?xml version="1.0" encoding="utf-8"?>
<CoupledMultiphysicsSimulation>
    <template_std_cfd_cht>
    <Standard_Job>standard_job_name</Standard_Job>
    <Cfd_Job>cfd_job_name</Cfd_Job>
    <duration>duration_value</duration>
    </template_std_cfd_cht>
</CoupledMultiphysicsSimulation> 

In certain cases you may need to use co-simulation configuration features that are not described in the predefined templates. For example, you may wish to change the dissimilar mesh mapping search tolerances; these tolerances are available generally in the configuration file but are not described in the predefined templates. For these cases, you must create an elaborated configuration file; for more information, see “Using elaborated configuration files” in “Preparing an Abaqus analysis for co-simulation,” Section 17.2.1.

Table 17.3.2–1 Templates for fluid-to-structural co-simulation and conjugate heat transfer.

Fluid-to-structural co-simulation: Abaqus/Standard and Abaqus/CFD	Coupling scheme:·Abaqus/Standard analysis leads·Coupling step size is based on the minimum of both analyses·Allow Abaqus/Standard to subcycle; Abaqus/CFD uses a single increment per coupling step (lockstep)
	template_std_cfd_fsi
	Example file: exa_std_cfd_fsi
Fluid-to-structural co-simulation: Abaqus/Explicit and Abaqus/CFD	Coupling scheme:·Abaqus/Explicit analysis leads·Abaqus/CFD defines the coupling step size·Allow Abaqus/Explicit to subcycle; Abaqus/CFD uses a single increment per coupling step (lockstep)
	template_xpl_cfd_fsi
	Example file: exa_xpl_cfd_fsi
Conjugate heat transfer: Abaqus/Standard and Abaqus/CFD	Coupling scheme:·Abaqus/Standard analysis leads·Coupling step size is based on the minimum of both analyses·Allow Abaqus/Standard to subcycle; Abaqus/CFD uses a single increment per coupling step (lockstep)
	template_std_cfd_cht
	Example file: exa_std_cfd_cht
Conjugate heat transfer: Abaqus/Explicit and Abaqus/CFD	Coupling scheme:·Abaqus/Explicit analysis leads·Abaqus/CFD defines the coupling step size·Allow Abaqus/Explicit to subcycle; Abaqus/CFD uses a single increment per coupling step (lockstep)
	template_xpl_cfd_cht
	Example file: exa_xpl_cfd_cht