Defining an initial state field

You can select part instances from your model and associate an initial state field with the instances. An initial state field defines a deformed mesh and its associated material state using data imported from a previous Abaqus/Standard or Abaqus/Explicit analysis. You can create an initial state field only during the initial step. For more information, see Transferring results between Abaqus analyses, and About transferring results between Abaqus analyses.

Related Topics
Importing a part from an output database
Creating predefined fields
In Other Guides
Importing and transferring results

  1. Display the initial state field editor using one of the following methods:

    • To create a new initial field, follow the procedure outlined in Creating predefined fields (Category: Other; Types for Selected Step: Initial state). You can create an initial state field only during the initial step.

    • To edit an existing initial state field using menus or managers, see Editing step-dependent objects. You can modify an initial state field only during the initial step.

  2. In the Job name field of the editor, enter the name of the job from which Abaqus/CAE will import the deformed mesh and material state. Abaqus/CAE imports data from several of the files created by the original analysis. As a result, the files from the analysis must reside in the directory from which you started the current Abaqus/CAE session.

  3. Choose the step from which to import. Do one of the following:

    • Choose Last step to import data from the last step of the previous analysis.

    • Choose Specify, and enter an integer specifying the step from which to import data from the previous analysis. A value of 1 specifies the first step.

  4. Choose the frame from which to import. Do one of the following:

    • Choose Last to import data from the last frame of the specified step.

    • Choose Specify, and enter an integer specifying the frame of the specified step. A value of 1 specifies the first frame.

  5. 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 analysis and will be continuous from the start of the analysis. Toggle on Update reference configuration to reset the reference configuration to be the imported configuration. Displacements and strains are now calculated relative to the new imported configuration.

  6. Click OK to create the initial state field and to close the dialog box.

    Yellow circles appear on the model representing the initial field that you just created. For more information, see Understanding symbols that represent prescribed conditions. Although Abaqus/CAE checks that the files from the previous analysis exist when you create the initial state field, it imports the deformed mesh and the material state from the specified step and increment only when you analyze the model in the Job module. As a result, you will not see any other changes in the current model after you create the initial state field; for example, Abaqus/CAE does not update the mesh of the current model.