You can select part instances from your model and associate an initial state field with the instances. An initial state field applies a deformed mesh and its associated material state to the instances using data imported from a previous ABAQUS/Standard or ABAQUS/Explicit analysis. ABAQUS/CAE allows you to select the job name corresponding to the analysis from which the initial state field is imported. You can also specify the particular step and increment of the analysis from which to import data. ABAQUS/CAE imports data from several of the files created by the previous analysis. As a result, the files from the analysis must reside in the directory from which you started the current ABAQUS/CAE session.
You can use this capability to drive an ABAQUS/Explicit analysis with the results of an ABAQUS/Standard analysis and vice versa. This is useful if your problem can be broken down into different stages; for example, you can use ABAQUS/Explicit to analyze a metal forming problem and ABAQUS/Standard to analyze the following springback. You can also use this capability to change the model definition between steps. For more information, see “Transferring results between ABAQUS analyses: overview,” Section 9.2.1 of the ABAQUS Analysis User's Manual.
You can also transfer results and model information from an ABAQUS/Standard analysis to a new ABAQUS/Standard analysis, where you can specify additional model definitions before continuing the analysis. For example, you might first study the local behavior of a particular component during an assembly process and then study the behavior of the assembled product. You can start by analyzing the local behavior of the component in an ABAQUS/Standard analysis. You can then transfer the model information and results from this analysis to a second ABAQUS/Standard analysis, where you can specify additional model definitions for the other components and analyze the behavior of the entire product.
ABAQUS/CAE always imports the material state along with the deformed mesh. If you want to import only the deformed mesh, you can import an orphan mesh from a selected step and increment of an output database. For more information, see “What kinds of files can be imported and exported from ABAQUS/CAE?,” Section 10.1.1.
ABAQUS uses the imported information when you submit a job for analysis; however, ABAQUS/CAE does not update the shape of the selected instances to reflect the applied deformed mesh. As a result, you should be careful when adding new instances to the assembly and positioning them relative to existing part instances. For example, a new part instance may appear to touch one of the instances associated with the initial state field; however, when the analysis applies the imported deformed mesh, the instances may become separated or overclosed.
To avoid this mismatch between the undeformed state and the imported state, you may want to import the deformed mesh from the analysis in the form of an orphan mesh part instead of working with the undeformed part instance. Even if you import the deformed mesh, you must take care that the frame from which you imported the orphan mesh part is the same as the step and increment specified in the initial state field. For more information, see “Importing a part from an output database,” Section 10.7.12. Alternatively, you can create the current model by copying it from the model that generated the previous ABAQUS/Standard or ABAQUS/Explicit analysis. For more information, see “Manipulating models within a model database,” Section 9.8.1.
The reference configuration is the configuration of the model from which displacements (and associated strains) are calculated. By default, ABAQUS/CAE does not use the imported data to update the reference configuration. As a result, displacements and strains are calculated as total values relative to the reference configuration at the start of the original analysis, and the values will be continuous between analyses. You can change the default behavior and configure ABAQUS/CAE to update the reference configuration to be the imported configuration. ABAQUS/CAE now calculates displacements and strains relative to the new imported reference configuration; for example, for a springback analysis.
ABAQUS imposes many restrictions when you try to create an initial state field. For a detailed discussion of these limitations, see “Transferring results between ABAQUS analyses: overview,” Section 9.2.1 of the ABAQUS Analysis User's Manual. For example, the mesh of the part instances that you select from the current model must match the mesh of the part instances that you are importing. You can then, for example, change the material definition, add loads and boundary conditions, and change from an ABAQUS/Standard to an ABAQUS/Explicit step. However, you cannot perform an operation that will change the mesh of a selected part instance; for example, you cannot partition the part instance.
You can transfer results between analyses only if the original analysis used one of the following steps:
Static stress
Dynamic stress
Steady-state transport
In addition, ABAQUS/CAE applies the following limitations:
The selected part instances and the instances from the previous analysis must have the same name.
After you define the initial state field, ABAQUS/CAE will continue to show the undeformed shape of the model.
You cannot use the Assembly module position and constraint tools, such as Translate and Face to Face, to move a part instance associated with an initial field.
ABAQUS/CAE imports only the mesh and the material state from the previous analysis. As a result, you must redefine sets and surfaces in the current model along with all of the prescribed conditions (loads, boundary conditions, predefined fields, interactions, connectors, etc.).
ABAQUS/CAE checks that the files exist that contain data from the previous ABAQUS/Standard or ABAQUS/Explicit analysis; however, it does not check that the specified step and increment number have been written to the files. The job submission fails if the data for the specified step or increment do not exist.
You cannot modify a part instance associated with an initial field (or the part from which you created the instance). In addition, you cannot modify the mesh of a part instance associated with an initial field (or the mesh of the part from which you created the instance).
You cannot assign new sections, material orientations, normals, or beam orientations to the part from which you created the instance associated with an initial field. Similarly, you cannot assign mass or inertia. However, you can edit the material definition (which ABAQUS/CAE imports along with the mesh). The imported material definitions will overwrite any existing material definitions.