김경종
24 KiB
In Abaqus you can use a node set or a node-based surface to define a co-simulation interface region consisting of discrete points.
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 options to define a node-based surface as a co-simulation region in an Abaqus model: *SURFACE, TYPE=NODE nodeset_A *CO-SIMULATION REGION, TYPE=SURFACE node-based surface name
Interacting through a surface
Interaction between distinct domains occurs through a common interface surface. For example, when a fluid interacts with a solid without penetrating it, the fluid-solid interface is defined through a surface. In this case both nodal position and element topology information define the co-simulation interface, and appropriate spatial mapping between dissimilar surface meshes is performed to conservatively map fields.
Input File Usage: Use the following option to define an element-based surface as a co-simulation region in an Abaqus model: *CO-SIMULATION REGION, TYPE=SURFACE (default) element-based surface name
Interacting through a volume
Interaction between overlapping domains occurs through a volume. In this case both nodal position and element topology information define the co-simulation region, and appropriate spatial mapping between dissimilar volume meshes is performed to conservatively map fields.
The interface region is defined by an element set.
Input File Usage: Use the following option to define a volume as a co-simulation region in an Abaqus model: *CO-SIMULATION REGION, TYPE=VOLUME elset_A
Identifying the fields exchanged across a co-simulation interface
The coupling of the domain models can be through loads and/or boundary conditions prescribed at the cosimulation interface. In addition, mass, rotary inertia, and heat capacitance terms can also be exchanged. Based on the physics and the interaction type and its enforcement, you must specify the fields that are imported and/or exported in an Abaqus analysis during the co-simulation.
The co-simulation interface can consist of a group of discrete points (nodes), a surface region, or a volume region. Not all fields can be exchanged across all region types.
This section provides a general overview of all fields available in Abaqus. For detailed information on the fields exchanged between two Abaqus solvers, see “Structural-to-structural co-simulation,” Section 17.3.1, and “Fluid-to-structural and conjugate heat transfer co-simulation,” Section 17.3.2. For detailed information on fields exchanged by Abaqus and a third-party analysis program, see the respective User’s Guides.
Input File Usage: Use the following option to import field data over a region into Abaqus:
*CO-SIMULATION REGION, IMPORT
region_A, import_field_1
region_A, import_field_2
Use the following option to export data from Abaqus:
*CO-SIMULATION REGION, EXPORT
region_A, export_field_1
region_A, export_field_2
Procedures involving mechanical degrees of freedom
Table 17.2.1–1 lists the fields that can be exchanged for procedures supporting mechanical degrees of freedom (degrees of freedom 1–6), their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–1 Exchanging fields for procedures supporting mechanical degrees of freedom.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
| Import | Export | ||||
| UT or U | Displacement | P, S, V | S, E, C | S, E | L |
| VT or V | Velocity (transient procedures) | P, S, V | S, E, C | S, E | $LT^{-1}$ |
| AT or A | Acceleration (transient procedures) | P, S, V | S | S, E | $LT^{-2}$ |
| UR | Rotations | P, S | S, E | S, E | radians |
| VR | Angular velocity (transient procedures) | P, S | S, E | S, E | radians $T^{-1}$ |
| AR | Angular acceleration (transient procedures) | P, S | S | S, E | radians $T^{-2}$ |
| COORD | Current coordinates | P, S, V | S, E | ||
| CF | Concentrated forces | P, S, V | S, E | S, E | F |
| Field ID | Fields | Interface Type $^{1}$ | Abaqus Solver $^{2}$ | Units | |
| Import | Export | ||||
| CM | Concentrated moments | P, S | S, E | S, E | $FL$ |
| TRSHR | Traction vector | S | C | $FL^{-2}$ | |
| PRESS | Pressure normal to element surface | S | S | $FL^{-2}$ | |
| $^{1}$ P (points), S (surface region), V (volume region) | |||||
| $^{2}$ S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
The following procedures support co-simulation using mechanical degrees of freedom:
• “Static stress analysis,” Section 6.2.2
• “Quasi-static analysis,” Section 6.2.5
• “Implicit dynamic analysis using direct integration,” Section 6.3.2
• “Explicit dynamic analysis,” Section 6.3.3
• “Fully coupled thermal-stress analysis,” Section 6.5.3
• “Incompressible fluid dynamic analysis,” Section 6.6.2
• “Piezoelectric analysis,” Section 6.7.2
• “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
Displacements
Displacements (field ID UT or U) for the translational degrees of freedom can be exported by Abaqus/Standard and Abaqus/Explicit. Displacements can be imported by Abaqus/Standard, Abaqus/Explicit, and Abaqus/CFD. When imported, displacements are ramped from the values of the previous exchange time point to those of the next target time point. In an implicit dynamic analysis, velocity and acceleration must be imported when importing displacement. The displacements are in the global coordinate system.
Displacements are available for points, surface regions, and volume regions in Abaqus/Standard and Abaqus/Explicit and for surface regions in Abaqus/CFD.
Displacements can be viewed in the Visualization module of Abaqus/CAE.
Velocity and acceleration
Velocity (field ID VT or V) and acceleration (field ID AT or A) for the translational degrees of freedom can be imported and exported by Abaqus/Standard for transient procedures and by Abaqus/Explicit. In an implicit dynamic analysis, when importing velocity or acceleration, all three fields—displacement, velocity, and acceleration—must be imported. Velocity can be imported by Abaqus/CFD. Velocity and acceleration are in the global coordinate system.
Velocity and acceleration are available for points, surface regions, and volume regions in Abaqus/Standard and Abaqus/Explicit and for surface regions in Abaqus/CFD.
Rotations
Rotations (field ID UR) can be imported and exported by Abaqus/Standard and Abaqus/Explicit. In an implicit dynamic analysis, rotational velocity and rotational acceleration must be imported when importing rotations. Rotations are in the global coordinate system.
Rotations are available for points and surface regions.
Rotations can be viewed in the Visualization module of Abaqus/CAE.
Rotational velocity and rotational acceleration
Rotational velocity (field ID VR) and rotational acceleration (field ID AR) can be imported and exported by Abaqus/Standard for transient procedures and by Abaqus/Explicit. In an implicit dynamic analysis, when importing rotational velocity or rotational acceleration, all three fields—rotation, rotational velocity, and rotational acceleration—must be imported. Rotational velocity and rotational acceleration are in the global coordinate system.
Rotational velocity and rotational acceleration are available for points and surface regions.
Current coordinates
Current nodal coordinates (field ID COORD) can be exported by Abaqus/Standard and Abaqus/Explicit. The coordinates are the current coordinates of the deformed structure whether small- or large-displacement analysis is performed. In general, it is preferred to export displacements (field ID UT or U) rather than current coordinates when results are mapped between dissimilar interface regions. In cases where the partner client does not retain the original coordinates, it may be necessary to send current coordinate values rather than displacements.
Current coordinates are available for points, surface regions, and volume regions in Abaqus/Standard and Abaqus/Explicit.
Concentrated forces
Concentrated forces (field ID CF), 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 in the global coordinate system.
When exporting concentrated forces, Abaqus/Standard transfers reaction forces at interface nodes that have prescribed displacements. The reaction forces are exported in the global coordinate system.
Concentrated forces are available for points, surface regions, and volume regions in Abaqus/Standard and Abaqus/Explicit.
Concentrated normal forces can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CF.
Concentrated moments
Concentrated moments (field ID CM), 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 moments are in the global coordinate system.
Concentrated moments are available for points and surface regions in Abaqus/Standard and Abaqus/Explicit.
Concentrated moments can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CM.
Traction vector
The traction vector (field ID TRSHR), supported by Abaqus/CFD, exports the fluid total traction (normal and shear components) on the interface surface. Usually, the exported traction vector is integrated to concentrated forces (field ID CF) when imported into Abaqus/Standard or Abaqus/Explicit in a fluidstructure simulation.
The traction vector is a force vector in the global Cartesian coordinate system.
The traction vector is available for surface regions in Abaqus/CFD.
Normal pressure
Normal pressure (field ID PRESS), supported for import by Abaqus/Standard, is the traction normal component to the surface. Pressure values are ramped from the values of the previous exchange time point to those of the next target time point when imported into Abaqus/Standard. In most cases it is preferred to import concentrated forces (field ID CF) since these contain both the normal and shear traction components. For membrane-like structures it might be preferable to import pressures.
Normal pressure can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable P.
Procedures involving thermal degrees of freedom
Table 17.2.1–2 lists the thermal 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.The following procedures support co-simulation using thermal degrees of freedom:
• “Uncoupled heat transfer analysis,” Section 6.5.2
• “Fully coupled thermal-stress analysis,” Section 6.5.3
• “Incompressible fluid dynamic analysis,” Section 6.6.2
• “Coupled thermal-electrical analysis,” Section 6.7.3
Table 17.2.1–2 Exchanging fields for procedures supporting thermal degrees of freedom.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
| Import | Export | ||||
| NT | Temperature as a nodal degree of freedom | P, S, V | S, E | S, E | $\theta$ |
| CFL | Concentrated heat flux at a node | P, S, V | S, E | $JT^{-1}$ | |
| HFL | Heat flux normal to element surface | S | S | C | $JT^{-1}L^{-2}$ |
| CFILM | Film properties | S | S | $JT^{-1}\theta^{-1}$ | |
| FILM | Film properties (MpCCI only) | S | S | $JT^{-1}L^{-2}\theta^{-1}$ | |
| TEMP | Temperature as a nodal degree of freedom | P, S, V | C | $\theta$ | |
| LUMPEDHEATCAPACITANCE | Lumped heat capacitance | P, S, V | S, E | C | $JM^{-1}\theta^{-1}$ |
| $^1$ P (points), S (surface region), V (volume region) | |||||
| $^2$ S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
Nodal temperature
Nodal temperature (field ID NT) can be imported and exported by Abaqus/Standard and Abaqus/Explicit and imported by Abaqus/CFD (as field ID TEMP). Temperature values are ramped from the values of the previous exchange time point to those of the next target time point when imported into Abaqus/Standard and Abaqus/CFD.
Temperature values can be exchanged either on the top surface (SPOS) or the bottom surface (SNEG) of structural elements. Temperatures cannot be exchanged on double-sided surfaces. When exchanging temperatures on both the top and bottom faces, define two different regions; one to exchange temperature on the top face and the other to exchange temperature on the bottom face. For volume regions, only degree of freedom NT11 is used, and it should not be used for exchanging temperature values over volumes discretized by nonthermal element types.
Nodal temperature values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable NT.
Heat flux
Use concentrated heat flux (field ID CFL) for heat entering at a node in Abaqus/Standard and Abaqus/Explicit. Concentrated heat flux is available for points, surface regions, and volume regions.
Heat flux values can be exchanged either on the top surface (SPOS) or the bottom surface (SNEG) of structural elements. Heat flux cannot be exchanged on double-sided surfaces. When exchanging heat flux on both the top and bottom faces, define two different regions; one to exchange heat flux on the top face and the other to exchange heat flux on the bottom face.
Concentrated heat flux values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CFL.
Use surface heat flux (field ID HFL) for a distributed heat flux entering the surface in Abaqus/Standard or distributed heat flux leaving a surface in Abaqus/CFD. Distributed heat flux is available only for surface regions.
Film properties
Use surface film properties (field ID FILM) or concentrated (nodal) film properties (field ID CFILM) to model convection governed by
q = - h (\theta_ {w a l l} - \theta_ {f l u i d}),
where q is the heat flux entering the surface, h is a film coefficient, \theta _ { w a l l } is the wall temperature, and \theta _ { f l u i d } 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/Standard analysis computed during the previous exchange interval, according to
h = q / (\theta_ {f l u i d} - \theta_ {w a l l}).
Both the film coefficient and fluid temperature are passed into Abaqus/Standard and are kept constant over the subsequent exchange interval. 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 exchange interval, you should ensure that the wall temperatures are initialized properly in Abaqus and that you provide a good estimate for the initial fluid temperature.
Film properties are available only for surface regions in Abaqus/Standard.
Heat capacitance
Nodal (lumped) heat capacitance (field ID LUMPEDHEATCAPACITANCE) can be exported by Abaqus/CFD in models in which heat capacitance is defined. Nodal heat capacitance can be imported into Abaqus/Standard and Abaqus/Explicit.
Procedures involving pore fluid pressure
Table 17.2.1–3 lists additional fields that can be exchanged for a coupled pore fluid diffusion/stress analysis, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–3 Exchanging fields for a coupled pore fluid diffusion/stress analysis.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
| Import | Export | ||||
| POR | Pore fluid pressure at a node | P, S, V | S | S | $FL^{-2}$ |
| CFF | Concentrated fluid flow at a node | P, S, V | S | $L^{3}T^{-1}$ | |
| RVF | Reaction fluid volume flux due to prescribed pressure | P, S, V | S | $L^{3}T^{-1}$ | |
| 1P (points), S (surface region), V (volume region) | |||||
| 2S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
The following procedure involving pore fluid pressure supports co-simulation:
• “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
Pore pressure
Nodal pore pressure (field ID POR) can be imported and exported by Abaqus/Standard for points, surface regions, and volume regions.
Nodal pore pressure values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable POR.
Concentrated fluid flow
Fluid flow (field ID CFF) defines the seepage flow at a node. Concentrated fluid flow can be imported by Abaqus/Standard for points, surface regions, and volume regions.
Concentrated fluid flow values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable CFF.
Reaction fluid volume flow
Reaction fluid volume flux (field ID RVF) defines the rate at which fluid volume is entering or leaving the model through the node to maintain the prescribed pore pressure. Reaction fluid volume flux can be exported by Abaqus/Standard for points, surface regions, and volume regions.
Procedures involving electromagnetic response
Table 17.2.1–4 lists additional fields that can be exchanged for an electromagnetic analysis, their associated field identifiers, the supported co-simulation interface region types, and which Abaqus solvers support import and export of the field values.
Table 17.2.1–4 Exchanging fields for a electromagnetic analysis.
| Field ID | Fields | Interface Type1 | Abaqus Solver2 | Units | |
| Import | Export | ||||
| EMJH | Joule heating flux due to flow of current | V | S | $JT^{-1}L^{-3}$ | |
| EMBF | Magnetic body force intensity vector due to flow of current | V | S | $FT^{-1}L^{-3}$ | |
| $^1$ P (points), S (surface region), V (volume region) | |||||
| $^2$ S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
The following procedure involving electromagnetics supports co-simulation:
• “Eddy current analysis,” Section 6.7.5
Joule heating flux
The Joule heating flux (field ID EMJH) can be exported by Abaqus/Standard for volume regions. It can be imported in a downstream heat transfer analysis as concentrated nodal heat flux (field ID CFL).
Values for the Joule heating flux can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable EMJH.
Magnetic body force intensity vector
The magnetic body force intensity vector (field ID EMBF) can be exported by Abaqus/Standard for volume regions. It can be imported in a downstream stress analysis as concentrated force (field ID CF).
Magnetic body force intensity vector values can be viewed in the Visualization module of Abaqus/CAE for an Abaqus/Standard simulation by requesting output variable EMBF.
Temperature and independent field variables
Field variables are time-dependent, predefined fields that exist over the spatial domain of the model (see “Predefined fields,” Section 34.6.1). Field variables in conjunction with the co-simulation technique extend the possibilities of multiphysics by allowing material point dependencies on an external field defined by another application.
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.
Table 17.2.1–5 lists the temperature and independent field variables 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 17.2.1–5 Exchanging temperature and independent field variables.
| Field ID | Fields | Interface Type $^{1}$ | Abaqus Solver $^{2}$ | Units | |
| Import | Export | ||||
| TEMP | Temperature as field variable | V | S | $\theta$ | |
| FV1 | Field variable 1 | V | S | ||
| FV2 | Field variable 2 | V | S | ||
| FV3 | Field variable 3 | V | S | ||
| $^{1}$ P (points), S (surface region), V (volume region) | |||||
| $^{2}$ S (Abaqus/Standard), E (Abaqus/Explicit), C (Abaqus/CFD) | |||||
The following Abaqus/Standard procedures support import of temperature and independent field variables:
• “Static stress analysis,” Section 6.2.2
• “Quasi-static analysis,” Section 6.2.5
• “Implicit dynamic analysis using direct integration,” Section 6.3.2
• “Fully coupled thermal-stress analysis,” Section 6.5.3
• “Piezoelectric analysis,” Section 6.7.2
• “Eddy current analysis,” Section 6.7.5
• “Coupled pore fluid diffusion and stress analysis,” Section 6.8.1
Temperature
Temperature (field ID TEMP) can be imported by Abaqus/Standard for procedures that allow material properties to be defined as a function of an external temperature field. When imported, temperature values are ramped from the values of the previous exchange time point to those of the next target time