Product: ABAQUS/Standard
Symmetric results transfer:
reduces the analysis cost of structures that may first undergo symmetric deformation followed by nonsymmetric deformation later during the loading history;
can be used to transfer the solution of an axisymmetric model to a three-dimensional model;
can be used to transfer the solution of the symmetric part of a three-dimensional model to a full three-dimensional model;
must be used in conjunction with the symmetric model generation capability (see “Symmetric model generation,” Section 10.3.1); and
can be used only to transfer the solution of a stress/displacement, heat transfer, coupled temperature-displacement, or coupled acoustic-structural analysis to a new model.
The symmetric results transfer capability can be used to transfer the solution of an axisymmetric model to a three-dimensional model or to transfer the solution of the symmetric part of a three-dimensional model to a full three-dimensional model. The symmetric model generation capability described in “Symmetric model generation,” Section 10.3.1, must be used to generate the three-dimensional model.
The symmetric results transfer capability is not available for models defined in terms of an assembly of part instances.
The solution that is transferred to the new model consists of the deformed configuration and corresponding material state, which includes strains and all state variables. The nodes are imported with their original coordinates. This solution becomes the initial or base state in the new analysis.
You specify the time at which the solution obtained in the original model must be read. The required step and increment or iteration must have been written to the restart files during the original analysis.
| Input File Usage: | Use the following option if the solution is transferred from any analysis other than a direct cyclic procedure: |
*SYMMETRIC RESULTS TRANSFER, STEP=step, INC=increment Use the following option if the solution is transferred from a previous direct cyclic analysis: *SYMMETRIC RESULTS TRANSFER, STEP=step, ITERATION=iteration |
You must ensure that the model is in equilibrium at the beginning of the analysis. It is recommended that an initial step definition be included using boundary conditions and loading that match the state of the model from which the results are transferred. An initial time increment equal to the total time should be used for this step to allow ABAQUS/Standard to try and achieve the equilibrium in one increment. If needed, ABAQUS/Standard can resolve the stress unbalance linearly over the step such that more than one increment is used. You can choose to have the stress unbalance resolved in the first increment of the step instead.
| Input File Usage: | Use the following option to have ABAQUS/Standard resolve the stress unbalance linearly over the step: |
*SYMMETRIC RESULTS TRANSFER, UNBALANCED STRESS=RAMP Use the following option to have ABAQUS/Standard resolve the stress unbalance in the first increment of the step: *SYMMETRIC RESULTS TRANSFER, UNBALANCED STRESS=STEP |
The symmetric results transfer capability uses the restart (.res), analysis database (.stt and .mdl), part (.prt), and output database (.odb) files from the old analysis to transfer the solution data to the new mesh. The name of the restart files from the old analysis must be specified when the new analysis is executed by using the oldjob parameter in the command for running ABAQUS or by answering a request made by the command procedure (see “Execution procedure for ABAQUS/Standard and ABAQUS/Explicit,” Section 3.2.2).
It is recommended that you verify that the new model is generated correctly before results are transferred or any analysis is performed. The model generation capability requires only information stored in the restart files during a data check run to generate the new model, which allows you to verify the new model before the analysis of the original model is performed. A data check analysis is performed by using the datacheck parameter in the command for running ABAQUS (see “Execution procedure for ABAQUS/Standard and ABAQUS/Explicit,” Section 3.2.2).
Once the model has been verified, the analysis of the original model can be performed and the results can be transferred to the new model.
The transferred solution can be written to the results files by requesting output at the beginning of a step (the zero increment; see “Output,” Section 4.1.1). This solution can also be viewed in ABAQUS/CAE.
When results are transferred from an axisymmetric model to a three-dimensional model, a local cylindrical orientation system is used for element output of stress, strain, etc. A default local orientation definition (“Orientations,” Section 2.2.5) is provided if the material in the original axisymmetric model does not contain an orientation definition. This default orientation is defined with the polar axis of the system along the axis of revolution with an additional 90° rotation about the local 1-direction so that the local axes are 1=radial, 2=axial, and 3=circumferential. If shells or membranes are used, the projections of the local 2- and 3-axes onto the surface of the shell or membrane are taken as the local directions on the surface. It is assumed that the material properties are specified in this system. If, on the other hand, an orientation definition is associated with the material in the original model, the orientation in the new three-dimensional model will be that orientation definition revolved about the axis of symmetry.
When results are transferred from a partial three-dimensional model to a full three-dimensional model by reflecting the partial three-dimensional model, a local material orientation is created in the full three-dimensional model based on the corresponding orientation definition in the partial three-dimensional model. However, if the material does not contain an orientation definition in the partial three-dimensional model and the partial three-dimensional model is not created by revolving an axisymmetric model, no local orientation definition is created in the full three-dimensional model. The full three-dimensional model uses a global coordinate system.
When results are transferred from a three-dimensional sector to a periodic three-dimensional model by revolving the three-dimensional sector about its symmetry axis, a local cylindrical orientation system is always used for element output of stress, strain, etc. If an orientation is specified in the original three-dimensional sector, the orientation system in the new model is defined by revolving the original orientation system about the symmetry axis. If shells or membranes are used, the projections of the local 2- and 3-axes onto the surface of the shell or membrane are taken as the local directions on the surface. If the material in the original three-dimensional sector does not contain an orientation definition, a default local orientation definition is provided. This default orientation is defined by revolving the global coordinate system in the original model about the axis of symmetry in the new model.
The displacement and rotational components obtained from the original model are first transformed into a global, rectangular Cartesian axis system before the results are transferred. If local coordinate directions are required in the new model, a nodal transformation (“Transformed coordinate systems,” Section 2.1.5) must be specified in the new model to define this coordinate system.
The following limitations exist for result transfer from an axisymmetric model to a 3-D model:
Result transfer is not available from 8-node reduced-integration axisymmetric elements (CAX8R and CAX8RH) to the corresponding 20-node brick elements (C3D20R and C3D20RH) when the elements are underlying the slave surface in a contact pair.
SAX2 is a finite-strain shell, while S8R is a small-strain shell. Do not use this combination when deformations are large in the original analysis.
Result transfer is not supported for shells with five degrees of freedom per node (STRI65, S8R5, and S9R5).
Initial conditions (see “Initial conditions,” Section 27.2.1) can be specified on all nodes and elements, including the part of the model generated using symmetric model generation (see “Symmetric model generation,” Section 10.3.1). However, in most cases the symmetric results transfer capability will overwrite the initial condition values with the solution obtained from the original model. An exception is initial temperatures and field variables. Initial temperatures and field variables are overwritten only when temperatures and field variables are specified in the original model. If only part of the original model contains a specification for temperatures or field variables, the remaining part of the model is assumed to have initial conditions with a magnitude of zero. This distribution of the field will be transferred to the new model. If temperatures and/or field variables are not defined anywhere in the original model, the initial conditions specified in the new model are applied.
All boundary conditions must be redefined; the symmetric result transfer capability ignores the boundary conditions specified in the original model. You must ensure that the model is in equilibrium at the beginning of the analysis; therefore, an initial step definition should be included using boundary conditions and loading that match the state of the model from which the results are transferred.
All loads must be redefined; the symmetric result transfer capability ignores the loads specified in the original model. You must ensure that the model is in equilibrium at the beginning of the analysis; therefore, an initial step definition should be included using boundary conditions and loading that match the state of the model from which the results are transferred.
All of the material definitions defined in the original model will be transferred to the new model.
Any element or contact pair removal/reactivation definition (see “Element and contact pair removal and reactivation,” Section 11.2.1) that was active in the original model should be respecified.
All of the standard output variables available for stress/displacement elements can be used with the symmetric results transfer capability.
The solution that is transferred to the new model can be written to the results (.fil) file by requesting output at the beginning of a step (the zero increment; see “Output,” Section 4.1.1). It can also be displayed in ABAQUS/CAE.