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.
If mass scaling (“Mass scaling,” Section 11.7.1) 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.
The material model must be redefined in the import analysis if changes to material damping are required.
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 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), 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.
Common element types CPS3, CPS3T, CPS4R, CPS4RT, CPS6M, CPS6MT CPE3, CPE3T, CPE4R, CPE4RT, CPE6M, CPE6MT CAX3, CAX3T, CAX4R, CAX4RT, CAX6M, CAX6MT C3D4, C3D4T, C3D6, C3D6T, C3D8, C3D8R, C3D8T, C3D8RT, C3D10M, C3D10MT M3D3, M3D4, M3D4R R2D2 R3D3, R3D4 RAX2 S4, S4R, S3R, S4RT, S3RT SC8R, SC8RT, SC6R, SC6RT SAX1 Common element types SFM3D3, SFM3D4R T2D2 T3D2 B21, B22 B31, B32 CONN2D21, CONN3D21 AC2D3, AC2D4R, AC2D4, ACIN2D2 AC3D4, AC3D6, AC3D8R, AC3D8, ACIN3D3, ACIN3D4 ACAX3, ACAX4R, ACAX4, ACINAX2 COH2D4, COHAX4, COH3D6, COH3D8 1Connector elements can be imported from Abaqus/Standard to Abaqus/Explicit; but not vice versa. 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 31.4.1) 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 defined in the original analysis to include an element set (see “Assigning elements to a rigid body” in “Rigid body definition,” Section 2.4.1) can be imported only if the element set exclusively contains rigid elements; if the rigid body contains deformable elements declared as rigid, the rigid body cannot be imported.
? Nodes that are part of a rigid body (defined using tie node sets and pin node sets; see “Assigning nodes to a rigid body” in “Rigid body definition,” Section 2.4.1) cannot be imported.
? 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/Explicit analysis to an Abaqus/Standard 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.
ACINAX2, ACIN2D2, ACIN3D3, ACIN3D4 CPE4R, CPE3, AC2D3, AC2D4