김경종
21 KiB
point. Use field ID NT instead of field ID TEMP to import temperature values for thermal procedures (procedures using degrees of freedom 11, 12, etc.).
Temperature can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting element output variable TEMP.
Independent field variables
Independent field variables (field IDs FV1, FV2, and FV3) can be imported by Abaqus/Standard, allowing material properties to be defined as a function of the external fields. When imported, independent field variable values are ramped from the values of the previous exchange time point to those of the next target time point.
Field variables can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variables FV1, FV2, and/or FV3.
Miscellaneous fields
Table 17.2.1–6 lists miscellaneous fields available for co-simulation exchange, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–6 Exchanging miscellaneous fields.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
| Import | Export | ||||
| MASS or LUMPEDMASS | Mass | P, S | S, E | S, E, C | M |
| RI | Rotary inertia | P, S | S | E | ML2 |
| 1P (points), S (surface region), V (volume region) | |||||
| 2S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
Lumped mass
Lumped mass values (field ID MASS or LUMPEDMASS) at nodes can be exported by Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD and can be imported by Abaqus/Standard and Abaqus/Explicit.
Lumped mass is available for points and surface regions.
Rotary inertia
Nodal (lumped) rotary inertia (field ID RI) can be imported by Abaqus/Standard and exported by Abaqus/Explicit over points or surface regions for models using structural elements.
Defining the coupling and rendezvousing scheme
Different types of analyses have different time integration requirements that will influence or dictate the frequency of interaction between the analyses in a co-simulation to obtain an accurate and robust solution. For example, consider the difference in time integration between an implicit and an explicit dynamic analysis. Furthermore, Abaqus/Standard can adjust the increment sizes automatically to obtain an economical and accurate solution for transient problems (see “Incrementation” in “Defining an analysis,” Section 6.1.2). For example, consider a transient heat transfer analysis modeling a diffusive process; here the analysis may use small time increments at the beginning of the analysis where there is a high gradient in the solution and large time increments toward the end of the analysis when steady state is reached.
The parameters that you use to control these co-simulation exchanges depend on the co-simulation interface that you are using.
• You define the co-simulation algorithm and related exchange parameters in a co-simulation configuration file.
• For structural-to-structural co-simulation using Abaqus/Standard and Abaqus/Explicit, you must also provide co-simulation controls parameters in the input file.
Using the SIMULIA Co-Simulation Engine configuration file
The SIMULIA Co-Simulation Engine employs an independent software component, termed the “director,” which defines all aspects of the interaction for co-simulation between analysis programs and provides the necessary instructions to implement the coupling and rendezvousing schemes. You provide the director with relevant parameters for your scheme choices through the co-simulation configuration file. When you use Abaqus/CAE to execute the co-simulation, the configuration file is created for you automatically.
The configuration file must be in Extensible Markup Language (XML) format, which uses the file extension xml. You can define a configuration file through a predefined template, or you can create a fully elaborated form of the configuration file.
Using predefined configuration templates
For the co-simulation analysis cases described in “Co-simulation between Abaqus solvers,” Section 17.3, predefined templates that define common coupling and rendezvousing schemes are available. To use one of the predefined templates, you must create a configuration file with the structure shown below.
<?xml version="1.0" encoding="utf-8"?>
Required XML declaration line
<CoupledMultiphysicsSimulation>
Required XML root element; identifies file as describing a multiphysics simulation
<template_name>
<template_parameter_1>parameter_1_name</template_parameter_1>
<template_parameter_2>parameter_2_name</template_parameter_2>
<template_parameter_3>parameter_3_name</template_parameter_3>
</template_name>
Closure of the template element
</CoupledMultiphysicsSimulation>
Closure of the XML root element
You enter the template name and a short list of parameter settings, such as the names of the two analysis jobs and the duration of the analysis. Details of the predefined templates are provided in “Structural-to-structural co-simulation,” Section 17.3.1; “Fluid-to-structural and conjugate heat transfer co-simulation,” Section 17.3.2; and “Electromagnetic-to-structural and electromagnetic-to-thermal co-simulation,” Section 17.3.3; as well as information on how to obtain an example configuration file for each template, such as the example shown below for a fluid-to-structural co-simulation.
<?xml version="1.0" encoding="utf-8"?>
<CoupledMultiphysicsSimulation>
<template_std_cfd_fsi>
<Standard_Job>StandardJobName</Standard_Job>
<Cfd_Job>CfdJobName</Cfd_Job>
<duration>duration</duration>
</template_std_cfd_fsi>
</CoupledMultiphysicsSimulation>
Using elaborated configuration files
At run time, the SIMULIA Co-Simulation Engine director applies your parameter settings to the template, creating an elaborated configuration file that is then used in the co-simulation analysis. An elaborated configuration file is defined as a configuration file that provides all details of the configuration explicitly without referring to a template.
In cases where predefined templates are not available (such as coupling with an in-house or third-party code) or are insufficient (for example, you want to exchange more variables at the co-simulation interface region or adjust mapping tolerances), you must create an elaborated configuration file. For tips on working with elaborated configuration files, see “Advanced Uses of the SIMULIA Co-Simulation Engine Configuration File” in the Dassault Systèmes Knowledge Base at www.3ds.com/support/knowledge-base. For detailed information about the elaborated configuration file, see the SIMULIA Co-Simulation Engine Application Programing Interface (API) documentation.
Coupling and rendezvousing schemes for elaborated configuration files
You define the co-simulation coupling and rendezvousing schemes in an elaborated configuration file.
Coupling scheme
The coupling scheme defines the sequence of exchanges between analysis programs and whether a coupled simulation can be run in a serial, parallel, or implicit iterative manner. When deciding on the
coupling scheme, you should consider solution stability issues as well as the utilization impact on your computing resources
Parallel explicit coupling scheme (Jacobi)
In a parallel explicit coupling scheme, both simulations are executed concurrently, exchanging fields to update the respective solutions at the next target time. The parallel coupling scheme may make more efficient use of computing resources; however, it is considered less stable than the sequential scheme and should be employed only for weakly coupled physics simulations using small coupling steps. The co-simulation partner analysis must also specify a Jacobi coupling algorithm.
Sequential explicit coupling scheme (Gauss-Seidel)
In a sequential explicit coupling scheme, the simulations are executed in sequential order. One analysis leads while the other analysis lags the co-simulation. The co-simulation partner analysis must also specify a Gauss-Seidel coupling algorithm.
The sequential explicit coupling scheme should be employed only for weakly coupled physics simulations using small coupling steps.
Iterative coupling scheme
In an iterative coupling scheme, the simulations are executed in sequential order. One analysis leads while the other analysis lags the co-simulation. Multiple exchanges per coupling step are performed until termination criteria are met.
The termination criteria depend on the analyses in the co-simulation; for co-simulation between Abaqus and third-party analysis products, consult the appropriate User’s Guide.
Coupling step size
The coupling step is the period between two consecutive exchanges and consequently defines the frequency of exchange between the analyses in a co-simulation. The coupling step size is established at the beginning of each coupling step and is used to compute the target time (the time when the next synchronized exchange occurs).
The methods available in Abaqus for computing the coupling step size are described in the sections below. To determine the methods available for a co-simulation partner analysis, consult the appropriate third-party program documentation.
Constant coupling step size
A constant user-defined coupling step size is the most basic method of defining a coupling step size. Both analyses advance while exchanging data at target points according to
t _ {i + 1} = t _ {i} + \Delta t _ {c},
where \Delta t _ { c } is a value that defines the coupling step size to be used throughout the coupled simulation, t _ { i + 1 } is the target time, and t _ { i } is the time at the start of the coupling step.
Minimum coupling step size
This method selects the minimum of the coupling step sizes suggested by each analysis. Abaqus always uses the next increment suggested by its automatic incrementation as its suggested coupling step size.
Maximum coupling step size
This method selects the maximum of the coupling step sizes suggested by each analysis. Abaqus always uses the next increment suggested by its automatic incrementation as its suggested coupling step size.
Importing the coupling step size
Abaqus can import a coupling step size suggested by the co-simulation partner analysis.
Exporting the coupling step size
Abaqus can export a suggested coupling step size to the co-simulation partner analysis.
Time incrementation scheme
Abaqus may take multiple increments per coupling step, or you can force Abaqus to use a single increment per coupling step.
Typically, Abaqus may perform several increments (referred to as “subcycling”) during the coupling step. During subcycling, Abaqus/Standard ramps the loads and boundary conditions (with the exception of film properties) from the values at the end of the previous coupling step to the values at the target time, while in Abaqus/Explicit the loads are applied at the start of the coupling step and kept constant over the coupling step.
Subcycling allows Abaqus to use its own time incrementation to reach the target coupling time; specifically, it allows Abaqus to cut back the increment size if there are nonlinear events that require the increment size to be reduced.
In certain cases you may force Abaqus to use a time increment size dictated by the coupling step size (i.e., no subcycling). This allows both solvers to use the same time incrementation and avoid interpolation of quantities during the coupling step. When proceeding in this “lockstep” manner, Abaqus will not be able to reduce the time increment to resolve nonlinear events and, consequently, will terminate the simulation in cases where the nonlinear events require that the increment size be reduced.
Model dimension and coordinate systems
Two-dimensional and three-dimensional Abaqus models are fully supported. Axisymmetric Abaqus models are supported only for Abaqus/Standard to Abaqus/Explicit co-simulation. 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.
Unit system
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.
Restarting a co-simulation
Field 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 fields at the start of the restart analysis. These fields must balance the conjugate fields computed by the Abaqus analysis such that equilibrium is maintained. 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. Specifically, the solution time for the particular step/increment number from which Abaqus is restarted must correspond to the coupled analysis solution.
Limitations
The following limitations apply:
• 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).
• A co-simulation surface or volume defined over beam, pipe, and truss elements or defined over the edges of three-dimensional elements cannot be used as an interface region. You should use discrete points to transfer loads and boundary conditions.
• A co-simulation surface or volume defined over modified triangular elements or modified tetrahedral elements cannot be used as an interface region.
• Quadratic coupled temperature-displacement elements cannot be used as an interface region in a co-simulation using the coupled temperature-displacement procedure.
• When performing a co-simulation, output at specified time points may not be satisfied at the requested times, depending on the synchronization parameters.
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.
17.3 Co-simulation between Abaqus solvers
• “Structural-to-structural co-simulation,” Section 17.3.1
• “Fluid-to-structural and conjugate heat transfer co-simulation,” Section 17.3.2
• “Electromagnetic-to-structural and electromagnetic-to-thermal co-simulation,” Section 17.3.3
• “Executing a co-simulation,” Section 17.3.4
17.3.1 STRUCTURAL-TO-STRUCTURAL CO-SIMULATION
Products: Abaqus/Standard Abaqus/Explicit 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
• “Defining a Standard-Explicit co-simulation interaction,” Section 15.13.14 of the Abaqus/CAE User’s Guide, in the HTML version of this guide
• Chapter 26, “Co-simulation,” of the Abaqus/CAE User’s Guide
Overview
Co-simulation between two structural solvers (solvers exchanging displacements and/or rotations and the conjugate fields’ force and/or moments) represents a very strong physics coupling and requires special treatment at the co-simulation interface. Abaqus supports co-simulation between Abaqus/Standard and Abaqus/Explicit by providing specialized interface handling. Although you can perform a structure-to-structure co-simulation between two Abaqus/Standard analyses or between two Abaqus/Explicit analyses, it is not recommended due to the lack of proper handling at the interface.
This section discusses analysis setup, execution, and limitation details specific to Abaqus/Standard to Abaqus/Explicit co-simulation.
Refer to “Dynamic impact of a scooter with a bump,” Section 2.4.1 of the Abaqus Example Problems Guide, for an example of Abaqus/Standard to Abaqus/Explicit co-simulation.
Identifying the Abaqus step for the co-simulation analysis
The following Abaqus/Standard analysis procedures can be used for an Abaqus/Standard to Abaqus/Explicit co-simulation:
• “Static stress analysis,” Section 6.2.2
• “Implicit dynamic analysis using direct integration,” Section 6.3.2
The following Abaqus/Explicit analysis procedure can be used for an Abaqus/Standard to Abaqus/Explicit co-simulation:
• “Explicit dynamic analysis,” Section 6.3.3
Input File Usage: Use the following option within a step definition for an Abaqus/Standard to Abaqus/Explicit co-simulation:
*CO-SIMULATION, PROGRAM=ABAQUS
Abaqus/CAE Usage: Use the following option for an Abaqus/Standard to Abaqus/Explicit co-simulation:
Interaction module: Create Interaction: Standard-Explicit co-simulation
Identifying the co-simulation interface region
Interaction between the Abaqus/Standard and Abaqus/Explicit models 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. For node-based surfaces the nodes have to be co-incident since no topology information is provided to conservatively map fields between the Abaqus/Standard and Abaqus/Explicit models. 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 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 Guide, to ensure these matching nodes.
Input File Usage: 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
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
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
Identifying the fields exchanged across a co-simulation interface
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.