and boundary interaction forces contribute to the initial out-of-balance forces. The boundary forces are the result of interactions from fixed boundary and contact conditions. Any changes in the boundary and contact conditions from the Abaqus/Explicit analysis to the Abaqus/Standard analysis will contribute to the initial out-of-balance forces.
In general the instantaneous removal of the initial out-of-balance forces in a static analysis will lead to convergence problems. Hence, these forces need to be removed gradually until complete static equilibrium is achieved. During this process of removing the out-of-balance forces, the body will deform further and a redistribution of internal forces will occur, resulting in a new stress state. (This is essentially what occurs during “springback,” when a formed product is removed from the worktools.)
When the first step in the Abaqus/Standard import analysis is a static procedure, the following algorithm is used to remove the initial out-of-balance forces automatically:
1. The imported stresses are defined at the start of the analysis as the initial
stresses in the material.
2. An additional set of artificial stresses is defined at each material point. These
stresses are equal in magnitude to the imported stresses but are of opposite sign. The sum of the material point stresses and these artificial stresses, thus, creates zero internal forces at the beginning of the step.
3. The internal artificial stresses are ramped off linearly in time during the first
step. Thus, at the end of the step the artificial stresses have been removed completely and the remaining stresses in the material will be the residual stress state associated with static equilibrium.
Once static equilibrium has been obtained, subsequent steps can be defined using any analysis procedure that would normally follow a static analysis in Abaqus.
When the first step is not a static analysis, no artificial stress state is applied and the imported stresses are used in the internal force computations for the element.
Boundary conditions
Boundary conditions, including any connector motion, specified in the original analysis are not imported. They must be defined again in the import analysis. In some cases nonzero boundary conditions imposed in the original analysis need to be maintained at the same values in the import analysis when the imported configuration is not updated. In such cases you can prescribe a constant (step function) amplitude variation for the analysis step (see “Prescribing nondefault amplitude variations” in “Procedures: overview,” Section 6.1.1) so that the newly applied boundary conditions are applied instantaneously and held at that value for the duration of the step. Alternatively, you can refer to an amplitude curve in the boundary condition definition (see “Amplitude curves,” Section 30.1.2). If boundary conditions in the original analysis are applied in a transformed
coordinate system (see “Transformed coordinate systems,” Section 2.1.5), the same coordinate system should be defined and used in the import analysis.
For a discussion of applying boundary conditions, see “Boundary conditions in Abaqus/Standard and Abaqus/Explicit,” Section 30.3.1.
Loads
Loads, including those applied for connector actuation, defined in the original analysis are not imported. Loads may, therefore, need to be redefined in the import analysis. There are no restrictions on the loads that can be applied when results are imported from one analysis to the other. In cases when the loads need to be maintained at the same values as in the original analysis, you can prescribe a constant (step function) amplitude variation for the analysis step (see “Prescribing nondefault amplitude variations” in “Procedures: overview,” Section 6.1.1) to apply the loads instantaneously at the start of the step and hold them for the duration of the step. Alternatively, you can refer to an amplitude curve in the load definition (see “Amplitude curves,” Section 30.1.2). If point loads in the original analysis are applied in a transformed coordinate system (see “Transformed coordinate systems,” Section 2.1.5) and the loads must be maintained in the import analysis, the load application is simplified if the same coordinate system is defined and used in the import analysis.
See “Applying loads: overview,” Section 30.4.1, for an overview of the loading types available in Abaqus.
Predefined fields
The field variables at nodes are not imported. If the elements being imported are coupled temperature-displacement elements, the temperature is imported if the associated material state is imported. The temperature is also imported for an adiabatic analysis if the associated material state is imported. For all other cases the temperatures at nodes are not imported.
If the original analysis uses predefined temperature fields (“Predefined temperature” in “Predefined fields,” Section 30.6.1) to vary the temperatures at nodes, the import analysis will not be allowed to continue. If the original analysis uses predefined field variable definitions (“Predefined field variables” in “Predefined fields,” Section 30.6.1) to vary the field variables at nodes, the import analysis will 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 30.2.1) and field variable (“Defining initial values of predefined field variables” in “Initial conditions in Abaqus/Standard and Abaqus/Explicit,”
Section 30.2.1) 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.