김경종
265 lines
26 KiB
Markdown
265 lines
26 KiB
Markdown
<!-- source-page: 671 -->
|
||
|
||
be allowed to continue only if all the elements being imported are coupled temperature-displacement elements; however, the field variables are not imported. If the original analysis uses initial temperature (“Defining initial temperatures” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) and field variable (“Defining initial values of predefined field variables” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,” Section 34.2.1) conditions, the import analysis will be allowed to continue only if all the elements being imported are coupled temperature-displacement elements.
|
||
|
||
In addition, specification of initial conditions for temperatures and field variables is not allowed in an import analysis, unless all the elements being imported are coupled temperature-displacement elements. In this case initial conditions for temperatures and field variables can be specified on the imported nodes if the reference configuration is updated and the material state is not imported. Initial temperatures can be specified in the import analysis if it is an adiabatic analysis.
|
||
|
||
# Material options
|
||
|
||
All material property definitions and the orientations associated with imported elements are imported by default. Material properties can be changed by respecifying the material property definitions with the same material name. All relevant material properties must be redefined since the old definitions that were imported by default will be overwritten. Material orientations associated with imported elements can be changed only if the reference configuration is updated and the material state is not imported; the material orientations associated with imported elements cannot be redefined for other combinations of the reference configuration and material state.
|
||
|
||
# Hyperelastic materials
|
||
|
||
When hyperelastic materials are imported, the state must be imported if the configuration is not updated; if the state is not imported, the configuration must be updated.
|
||
|
||
# Connector elements
|
||
|
||
When connector elements are imported, any associated connector behavior definitions are imported by default. The imported connector behavior definitions can be modified only if the state is not imported.
|
||
|
||
# Mass scaling
|
||
|
||
If mass scaling (“Mass scaling,” Section 11.6.1) is used in Abaqus/Explicit, the scaled masses will not be transferred to the subsequent import analysis in Abaqus/Standard. The mass of the model for the Abaqus/Standard analysis will be based on either the imported or the redefined density definitions.
|
||
|
||
# Material damping
|
||
|
||
The material model must be redefined in the import analysis if changes to material damping are required.
|
||
|
||
# Changes to material definitions
|
||
|
||
When material definitions are changed, care must be taken to ensure that a consistent material state is maintained. It may sometimes be possible to simplify the material definition. For example, if a Mises
|
||
|
||
<!-- source-page: 672 -->
|
||
|
||
plasticity model was used in the Abaqus/Explicit analysis and no further plastic yielding is expected in the Abaqus/Standard analysis (as is generally the case for springback simulations), a linear elastic material can be used for the Abaqus/Standard analysis. However, if further nonlinear material behavior is expected, no changes to the existing material definitions should be made. The history of the state variables will not be maintained if the material models are not the same in both the original analysis and the import analysis.
|
||
|
||
# Elements
|
||
|
||
The import capability is available for first-order continuum, modified triangular and tetrahedral elements, conventional shell, continuum shell, membrane, beam (both linear and quadratic), pipe (linear), truss, connector, rigid, and surface elements that are common to both Abaqus/Explicit and Abaqus/Standard, as defined in Table 9.2.2–2.
|
||
|
||
Table 9.2.2–2 Common element types that can be transferred between Abaqus/Explicit and Abaqus/Standard.
|
||
|
||
<table><tr><td>Common element types</td></tr><tr><td>CPS3, CPS3T, CPS4R, CPS4RT, CPS6M, CPS6MT</td></tr><tr><td>CPE3, CPE3T, CPE4R, CPE4RT, CPE6M, CPE6MT</td></tr><tr><td>CAX3, CAX3T, CAX4R, CAX4RT, CAX6M, CAX6MT</td></tr><tr><td>C3D4, C3D4T, C3D6, C3D6T, C3D8, C3D8R, C3D8T, C3D8RT, C3D10M, C3D10MT</td></tr><tr><td>M3D3, M3D4, M3D4R</td></tr><tr><td>R2D2</td></tr><tr><td>R3D3, R3D4</td></tr><tr><td>RAX2</td></tr><tr><td>S4, S4R, S3R, S4RT, S3RT</td></tr><tr><td>SC8R, SC8RT, SC6R, SC6RT</td></tr><tr><td>SAX1</td></tr><tr><td>SFM3D3, SFM3D4R</td></tr><tr><td>T2D2</td></tr><tr><td>T3D2</td></tr><tr><td>B21, B22, PIPE21</td></tr><tr><td>B31, B32, PIPE31</td></tr></table>
|
||
|
||
<!-- source-page: 673 -->
|
||
|
||
<table><tr><td>Common element types</td></tr><tr><td> $CONN2D2^1$ , $CONN3D2^1$ </td></tr><tr><td>AC2D3, AC2D4R, AC2D4, ACIN2D2</td></tr><tr><td>AC3D4, AC3D6, AC3D8R, AC3D8, ACIN3D3, ACIN3D4</td></tr><tr><td>ACAX3, ACAX4R, ACAX4, ACINAX2</td></tr><tr><td>COH2D4, COHAX4, COH3D6, COH3D8</td></tr><tr><td>MASS, ROTARYI</td></tr><tr><td> $^1$ Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit; but not vice versa.</td></tr></table>
|
||
|
||
When S3R shell elements are imported from Abaqus/Explicit into Abaqus/Standard, they are converted into degenerated S4R elements automatically. However, when S3R shell elements are imported from Abaqus/Standard into Abaqus/Explicit, they remain S3R elements. When C3D6 and C3D6T solid elements are imported from Abaqus/Explicit into Abaqus/Standard, the results at the single point integration are applied to both integration points in Abaqus/Standard and the full integration is used automatically. However, when C3D6 and C3D6T solid elements are imported from Abaqus/Standard into Abaqus/Explicit, only the results at the first integration point are imported and are used in the reduced integration. When quadrilateral and hexahedral acoustic finite elements are imported between Abaqus/Explicit and Abaqus/Standard, they are converted to or from reduced-integration types, as required.
|
||
|
||
The following restrictions apply to the import capability:
|
||
|
||
• Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit but not vice versa. Further, if connector elements are imported, the configuration can be updated provided that the state is not imported and the state can be imported provided that the configuration is not updated.
|
||
• Rebars defined using rebar layers (“Defining reinforcement,” Section 2.2.3) are imported provided the underlying elements are also imported. Rebar reinforcements defined using the embedded element technique (“Embedded elements,” Section 35.4.1) are imported if the host and embedded elements used in this definition are also imported. Rebars defined as an element property (“Defining rebar as an element property,” Section 2.2.4) cannot be imported.
|
||
• Infinite elements and fluid elements cannot be imported.
|
||
• Rigid elements for which the thickness is interpolated from the nodes in an Abaqus/Explicit analysis will not be imported into Abaqus/Standard.
|
||
• A rigid body containing both deformable and rigid elements cannot be imported. A rigid body that includes rigid elements is imported when the element set used to define the rigid body is specified for import. A rigid body that includes deformable elements is imported into Abaqus/Explicit when the element set used to define the rigid body is specified for import. The imported rigid body definition is overwritten if it is respecified using the same element set. When the model is defined in terms
|
||
|
||
<!-- source-page: 674 -->
|
||
|
||
of an assembly of part instances, the reference node of an imported rigid body must belong to an imported instance.
|
||
|
||
• When a rigid body is imported, any associated data such as pin node sets and tie node sets are part of the imported definition. However, these sets as imported contain only those nodes that are connected to the imported elements.
|
||
• Failed elements in Abaqus/Explicit will not be imported into Abaqus/Standard.
|
||
• Elements that are being removed or are inactive (see “Element and contact pair removal and reactivation,” Section 11.2.1) in Abaqus/Standard will not be imported into Abaqus/Explicit.
|
||
• Rigid surfaces will not be imported.
|
||
|
||
When importing results from an Abaqus/Standard analysis to an Abaqus/Explicit analysis, each element set specified can contain only compatible element types listed in Table 9.2.2–3 and can contain at most three different element types.
|
||
|
||
Table 9.2.2–3 Compatible element types.
|
||
|
||
<table><tr><td>ACINAX2, ACIN2D2, ACIN3D3, ACIN3D4</td></tr><tr><td>CPE4R, CPE3, AC2D3, AC2D4</td></tr><tr><td>CPS4R, CPS3</td></tr><tr><td>CAX4R, CAX3, ACAX3, ACAX4</td></tr><tr><td>AC3D4, AC3D6, AC3D8, C3D8, C3D8R, C3D4, C3D6</td></tr><tr><td>M3D4R, M3D3, M3D4</td></tr><tr><td>R3D3, R3D4</td></tr><tr><td>S4R, S3R, SC6R, SC8R, S4</td></tr><tr><td>SFM3D3, SFM3D4R</td></tr><tr><td>CAX6M, C3D10M</td></tr><tr><td>C3D8T, C3D4T, C3D6T</td></tr><tr><td>SC6RT, SC8RT, S4T, S4RT, S3T, S3RT</td></tr><tr><td>MASS, ROTARYI</td></tr></table>
|
||
|
||
# Using section controls in an import analysis
|
||
|
||
When transferring results between Abaqus/Standard and Abaqus/Explicit, it is important that the hourglass forces are computed consistently. The enhanced hourglass control formulation (see “Enhanced hourglass control approach in Abaqus/Standard and Abaqus/Explicit” in “Section controls,” Section 27.1.4) is recommended for computing hourglass forces in the original as well as all subsequent import analyses.
|
||
|
||
<!-- source-page: 675 -->
|
||
|
||
Once section controls have been defined in the original analysis, they cannot be modified in any subsequent Abaqus/Standard or Abaqus/Explicit analysis. Therefore, if section controls are to be used in any one analysis in a series of import analyses, they must be specified in the very first analysis. The section controls specified for an element set in the original analysis will be used for the elements belonging to that element set in all subsequent import analyses.
|
||
|
||
Section controls other than the hourglass control formulation have appropriate defaults depending on the type of analysis and, generally, do not need to be changed. Nondefault values can be chosen subject to certain restrictions.
|
||
|
||
In an Abaqus/Standard analysis only the average strain kinematic formulation and second-order accurate element formulation are available; other kinematic formulations, element formulations, or section controls that are relevant only in an Abaqus/Explicit analysis can be specified in the Abaqus/Standard analysis. Such controls will be ignored in the Abaqus/Standard analysis but retained for the subsequent Abaqus/Explicit import analysis.
|
||
|
||
If a kinematic formulation other than average strain is used for solid elements in the Abaqus/Explicit analysis, the differences in the kinematic formulations may lead to errors in Abaqus/Standard if the elements are distorted or undergo large rotations.
|
||
|
||
Using the first-order accurate element formulation (default) in Abaqus/Explicit and the second-order accurate element formulation (the only available formulation) in Abaqus/Standard is not expected to cause significant errors, since the time increment size in Abaqus/Explicit is inherently small. One exception to this is when the Abaqus/Explicit analysis involves components undergoing several revolutions, in which case it is recommended that the second-order accurate element formulation be used in Abaqus/Explicit.
|
||
|
||
Input File Usage: Use the following options in the original analysis:
|
||
|
||
\*MEMBRANE SECTION, CONTROLS=name1, ELSET=elset1
|
||
|
||
\*SHELL SECTION, CONTROLS=name2, ELSET=elset2
|
||
|
||
\*SHELL GENERAL SECTION, CONTROLS=name3, ELSET=elset3
|
||
|
||
\*SOLID SECTION, CONTROLS=name4, ELSET=elset4
|
||
|
||
Use options similar to the following one in the original analysis:
|
||
|
||
\*SECTION CONTROLS, NAME=name1
|
||
|
||
Abaqus/CAE Usage: Define section controls when you assign the element type in the original analysis:
|
||
|
||
Mesh module: Mesh→Element Type: Element Controls
|
||
|
||
# Membrane and shell element thickness computation
|
||
|
||
The computations for membrane and shell element thicknesses are described below.
|
||
|
||
Shell elements defined using a general shell section
|
||
|
||
For shells defined using a general shell section, the current thickness is computed based on the effective Poisson’s ratio, which is 0.5 by default, in both Abaqus/Explicit and Abaqus/Standard.
|
||
|
||
Input File Usage: \*SHELL GENERAL SECTION, POISSON=
|
||
|
||
<!-- source-page: 676 -->
|
||
|
||
# Abaqus/CAE Usage: Property module: homogeneous or composite shell section editor: Section integration: Before analysis: Advanced: Section Poisson's ratio
|
||
|
||
Shell elements defined using shell sections integrated during analysis and membrane elements
|
||
|
||
For shells defined using shell sections integrated during analysis and for membranes in Abaqus/Standard, the current thickness is computed based on the effective Poisson’s ratio, which is 0.5 by default. In Abaqus/Explicit, on the other hand, the computation of the thickness could be based either on the effective Poisson’s ratio or the through-thickness strains, with the computation based on the through-thickness strains used by default.
|
||
|
||
If you do not specify a section Poisson’s ratio for shell sections integrated during analysis or for membrane sections in an original Abaqus/Explicit or Abaqus/Standard analysis, the thickness computations in the original and all subsequent import analyses are carried out using the default methods. In other words, the thicknesses in all Abaqus/Standard analyses are computed using the default effective Poisson’s ratio of 0.5, while the thicknesses in all Abaqus/Explicit analyses are computed using the through-thickness strains.
|
||
|
||
When the section Poisson’s ratio is assigned a numerical value in an original Abaqus/Standard or Abaqus/Explicit analysis, the thickness computations in the original analysis and all subsequent import analyses are performed using the specified value for the effective Poisson’s ratio.
|
||
|
||
Input File Usage: Use one of the following options:
|
||
|
||
\*SHELL SECTION, POISSON=
|
||
\*SHELL SECTION, POISSON=MATERIAL
|
||
\*MEMBRANE SECTION, POISSON=
|
||
\*MEMBRANE SECTION, POISSON=MATERIAL
|
||
|
||
Abaqus/CAE Usage: Property module:
|
||
|
||
Homogeneous or composite shell section editor: Section integration:
|
||
|
||
During analysis: Advanced: Section Poisson's ratio
|
||
|
||
Membrane section editor: Section Poisson's ratio
|
||
|
||
# Contact angle computation in SLIPRING-type connector elements
|
||
|
||
The contact angle, , made by the belt wrapping around node b (see “Connection-type library,” Section 31.1.5) is computed automatically in Abaqus/Explicit, ignoring the value specified within the Abaqus/Standard analysis.
|
||
|
||
# Constraints
|
||
|
||
Most types of kinematic constraints (including multi-point constraints and surface-based tie constraints) specified in the original analysis are not imported and must be defined again in the import analysis; however, embedded element constraints are imported by default. See “Kinematic constraints: overview,” Section 35.1.1, for a discussion of the various types of kinematic constraints.
|
||
|
||
<!-- source-page: 677 -->
|
||
|
||
# Interactions
|
||
|
||
Contact definitions specified in the original analysis and the contact state are not imported. Contact can be defined again in the import analysis by specifying the surfaces and contact pairs; however, you may not be able to use the exact contact definitions that were used in the original analysis because of differences in the contact capabilities between Abaqus/Standard and Abaqus/Explicit.
|
||
|
||
The contact constraint enforcement may be different in Abaqus/Standard and Abaqus/Explicit. Examples of potential causes for differences include:
|
||
|
||
• Abaqus/Standard typically uses a “pure master-slave” approach, whereas Abaqus/Explicit typically uses a “balanced master-slave” approach.
|
||
• Depending on the contact formulations used, Abaqus/Standard and Abaqus/Explicit sometimes treat shell thicknesses and midsurface offsets differently.
|
||
|
||
Thus, when the contact conditions are defined in the import analysis, the contact state that existed in the previous analysis may not be reproduced at the beginning of the import analysis. This could lead to a redistribution of stresses and an analysis that differs from what you desire. In some cases this problem can be mitigated by using nondefault options, such as ignoring shell thicknesses in the contact calculations, to match behaviors in Abaqus/Standard and Abaqus/Explicit.
|
||
|
||
For a detailed description of the contact capabilities in Abaqus and the differences in the contact capabilities between Abaqus/Standard and Abaqus/Explicit, see “Contact interaction analysis: overview,” Section 36.1.1.
|
||
|
||
# Output
|
||
|
||
Output can be requested for an import analysis in the same way as for an analysis in which the results are not imported. The output variables available in Abaqus/Standard are listed in “Abaqus/Standard output variable identifiers,” Section 4.2.1. The output variables available in Abaqus/Explicit are listed in “Abaqus/Explicit output variable identifiers,” Section 4.2.2.
|
||
|
||
The values of the following material point output variables will be continuous in an import analysis when the material state is imported: stress, equivalent plastic strain (PEEQ), and solution-dependent state variables (SDV) for UMAT and VUMAT. Similarly, for a connector behavior, the plastic relative displacement (CUP), kinematic hardening shift force (CALPHAF), overall damage (CDMG), damage initiation criteria (CDIF, CDIM, CDIP), friction accumulated slip (CASU), and connector status (CSLST, CFAILST) will be continuous.
|
||
|
||
If the reference configuration is not updated, the displacements, strains, whole element variables, section variables, and energy quantities will be reported relative to the original configuration. Accelerations are recomputed at the start of an import analysis in Abaqus/Explicit and may be different from those obtained at the end of an Abaqus/Standard analysis. The differences in accelerations arise from the recalculation of the internal forces created by the imported stresses using the Abaqus/Explicit element formulation algorithms.
|
||
|
||
If the reference configuration is updated, displacements, strains, whole element variables, section variables, and energy quantities will not be continuous in an import analysis and will be reported relative to the updated reference configuration.
|
||
|
||
<!-- source-page: 678 -->
|
||
|
||
Time and step number will not be continuous between the original and the import analyses if the reference configuration is updated. Time and step number will be continuous only if the reference configuration is not updated.
|
||
|
||
# Limitations
|
||
|
||
The import capability has the following known limitations. Where applicable, details are given in the relevant sections.
|
||
|
||
• The same release of Abaqus/Explicit and Abaqus/Standard must be run on computers that are binary compatible.
|
||
• The capability is not available for fluid elements, infinite elements, and spring and dashpot elements. Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit but not vice versa. See the discussion on “Elements” earlier in this section for further details.
|
||
• If connector elements are imported, the configuration can be updated provided that the state is not imported and the state can be imported provided that the configuration is not updated.
|
||
• All elements and nodes must be included in at least one set in the original analysis when importing part instances.
|
||
• Node sets that are generated from existing element sets (see “Node definition,” Section 2.1.1) must be defined in the original analysis.
|
||
• Surface definitions, contact pair definitions, and general contact definitions are not imported. Analytical rigid surfaces will not be imported.
|
||
• If the material state is imported, only stresses will be imported for material models other than those defined by linear elasticity, hyperelasticity, Mullins effect, hyperfoam, viscoelasticity, Mises plasticity (including the kinematic hardening models), extended Drucker-Prager plasticity, crushable foam plasticity, Mohr-Coulomb plasticity, critical state (clay) plasticity, cast iron plasticity, concrete damaged plasticity, damage for cohesive elements, damage for ductile metals, or damage for fiber-reinforced composites. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details.
|
||
• If the state is imported for connector elements with behavior defined, the plastic displacements, the frictional slip, and the damage state are imported and the connector forces are recomputed. Some of the connector output variables, such as CU, are also recomputed on import. The recomputed variables may differ slightly at the point of import due to precision and algorithmic differences between the two solvers across import. See “Importing the material state” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1, for details.
|
||
• Temperatures and field variables at nodes are not imported. If the temperature is a state variable (as in an adiabatic analysis where temperature is an integration point quantity), it will be imported if the material state is imported. See the discussion on “Predefined fields” for details.
|
||
• Loads, boundary conditions, multi-point constraints, and equations are not imported.
|
||
• Kinematic and distributing coupling constraints are not imported. In addition, the reference node of a coupling constraint will not be imported unless the reference node is part of another element definition that is imported.
|
||
|
||
<!-- source-page: 679 -->
|
||
|
||
• The rigid body must be redefined if the element set containing the assigned elements is imported more than once in an Abaqus/Explicit import analysis.
|
||
|
||
• Embedded elements must be redefined if the host element set is imported more than once in an Abaqus/Explicit import analysis.
|
||
|
||
• Element and contact pair removal/reactivation (“Element and contact pair removal and reactivation,” Section 11.2.1) cannot be used in the first step of an import analysis in Abaqus/Standard. It can be used in the subsequent steps.
|
||
|
||
• In a series of Abaqus/Standard and Abaqus/Explicit import analyses in the order Abaqus/Explicit(1) → Abaqus/Standard(1) → Abaqus/Explicit(2) →Abaqus/Standard(2), if elements in an element set are removed in the Abaqus/Standard(1) analysis, the subsequent Abaqus/Standard(2) import analysis does not recognize that this element set was removed in a previous analysis and fails with an error message stating that the element set is not found in the restart file. Such failures can be avoided by using flattened input files and requesting only the active element sets for import.
|
||
|
||
• Section controls must be defined in the original analysis if any of a series of import analyses uses nondefault element formulations since section controls cannot be changed in an import analysis. See the discussion on “Using section controls in an import analysis” earlier in this section.
|
||
|
||
• The symmetric model generation capability (“Symmetric model generation,” Section 10.4.1) cannot be used in an import analysis in Abaqus/Standard.
|
||
|
||
• The results file, restart file, or output database file generated during the import analysis is not appended to the results file, restart file, or output database file of the original analysis.
|
||
|
||
• An Abaqus/Standard import analysis where the reference configuration is not updated is not allowed if the adaptive meshing capability (“ALE adaptive meshing: overview,” Section 12.2.1) was used in the previous Abaqus/Explicit analysis.
|
||
|
||
• Mesh-independent spot welds (see “Mesh-independent fasteners,” Section 35.3.4) and tie constraints (see “Mesh tie constraints,” Section 35.3.1) are not imported. These constraints can be redefined in the import analysis and are formed using the reference configuration of the import model. If the reference configuration is updated, the redefined constraints may not match the old constraints exactly due to the differences in geometry. If new constraints are defined and the reference configuration of the import model is not updated, they may not initially be in compliance if the nodes involved in the constraint have nonzero displacements. This may cause numerical difficulty and potential abort of the import analysis. In this case it is recommended that you update the reference configuration upon import.
|
||
|
||
• The first step after an import when the reference conference is updated should not be used to generate a substructure.
|
||
|
||
• For beam structures that have acute curvatures and undergo large permanent changes in curvatures, slightly different equilibrated configurations will be seen when using import depending on whether or not the reference configuration is to be updated to the imported configuration (see “Updating the reference configuration” in “Transferring results between Abaqus analyses: overview,” Section 9.2.1). This configuration difference is due to beam element formulation differences between Abaqus/Standard and Abaqus/Explicit.
|
||
|
||
<!-- source-page: 680 -->
|
||
|
||
# Transferring results between Abaqus/Explicit and Abaqus/Standard using models that are not defined as assemblies of part instances:
|
||
|
||
Abaqus/Explicit analysis:
|
||
```txt
|
||
*HEADING
|
||
...
|
||
*MATERIAL, NAME=mat1
|
||
*ELASTIC
|
||
Data lines to define linear elasticity
|
||
*PLASTIC
|
||
Data lines to define Mises plasticity
|
||
*DENSITY
|
||
Data line to define the density of the material
|
||
...
|
||
*BOUNDARY
|
||
Data lines to define boundary conditions
|
||
*STEP
|
||
*DYNAMIC, EXPLICIT
|
||
...
|
||
*RESTART, WRITE, NUMBER INTERVAL=n
|
||
*END STEP
|
||
```
|
||
|
||
Abaqus/Standard analysis:
|
||
```txt
|
||
*HEADING
|
||
*IMPORT, STEP=step, INTERVAL=interval, STATE=YES, UPDATE=NO
|
||
Data lines to specify element sets to be imported
|
||
*IMPORT ELSET
|
||
Data lines to specify element set definitions to be imported
|
||
*IMPORT NSET
|
||
Data lines to specify node set definitions to be imported
|
||
**
|
||
*** Optionally redefine the material block
|
||
**
|
||
*MATERIAL, NAME=mat1
|
||
*ELASTIC
|
||
Data lines to redefine linear elasticity
|
||
*PLASTIC
|
||
Data lines to redefine Mises plasticity
|
||
...
|
||
*BOUNDARY
|
||
```
|