5.1. Transfering Explicit Results to MAPDL

It is possible to initialize a Mechanical APDL implicit analysis from the results of an Explicit Dynamics analysis by using features of the Mechanical APDL command language. You can obtain results from the Explicit analysis by using an Explicit Dynamics Workbench system followed by a Design Assessment system that uses a python script to extract the results and write the additional Mechanical APDL commands to a file. A Commands object can be added to the Transient or Static Structural system to include the execution of the Mechanical APDL commands from the file. A full description of the process follows, and an example has been detailed in the Design Assessment documentation.


Note:  This method is currently limited to cases where there is no change in mesh topology between the start of both the Explicit and Implicit analyses.


Follows these steps to perform the Explicit-to-Implicit analysis:

  1. Add an Explicit Dynamics analysis to the Workbench Project Schematic.

  2. Add a Design Assessment system to the Explicit Dynamics system in the Project Schematic. You will create an XML Definition File for the Design Assessment system that specifies a python script to be run on “solve”. Set your Design Assessment type to be User Defined, and choose the XML Definition File that you created.

  3. Create the python script to write to a file the necessary Mechanical APDL commands to initialize the implicit model. The script should:

    1. Get nodal deformations, stresses, and plastic strains from the end of the Explicit Dynamics analysis using the Design Assessment API.

    2. Write the Mechanical APDL commands:

      1. Enter the preprocessor.

        Command(s): /PREP7

      2. Get initial nodal locations from the Implicit analysis.

        Command(s): *GET, and so on

      3. Redefine Implicit elements to the deformed configuration by adding values from steps 3(a) and 3(b)(ii).

        Command(s): N, and so on

      4. Specify reduced element integration if using solid elements. Workbench automatically converts explicit elements to Implicit elements. However, due to Explicit elements having only one integration point per element, it is necessary to specify this manually for the Implicit elements in order that results can be transferred between the two analyses.


        Note:  Explicit uses SHELL163 for shells and SOLID164 for solids. These get automatically converted to SHELL181 and SOLID185 respectively.


        Command(s): ET, 1, 185, , 1 and so on

      5. Reenter the solution processor.

        Command(s): /SOLU

      6. Set any necessary constraints on the model by modifying or adding to the boundary conditions defined during the Explicit analysis (for example, in a metal forming analysis, you need to constrain the blank).

        Command(s): D, and so on

      7. Import stresses from the Explicit Dynamics analysis. For solids, this will be one set of values per element. For shells, this will be one set of values for every layer within each element.

        Command(s): INISTATE, SET, DTYPE, STRESS

        Command(s): INISTATE, DEFINE, and so on

      8. Import plastic strains and accumulated equivalent plastic strain from Explicit Dynamics analysis

        Command(s): INISTATE, SET, DTYPE, EPPL

        Command(s): INISTATE, DEFINE, and so on

        Command(s): INISTATE, SET, DTYPE, PLEQ

        Command(s): INISTATE, DEFINE, and so on

      9. Solve analysis.

        Command(s): SOLVE

  4. Add an Implicit system, either Static Structural or Transient Structural. In this system include the file that was created with the Design Assessment script by adding a Commands object that reads in the file that was created by the python script.

    Command(s): /INPUT, and so on

  5. When post processing, view results by issuing Mechanical APDL commands in order to view results with the initial deformed mesh. When post processing in the standard Workbench view, results will appear to deform in the opposite direction to the Explicit Dynamics analysis because it has not taken into account the redefined deformed mesh. To create graphic files showing the correctly deformed mesh, add a new Commands object under the Solution branch of the Implicit analysis.

    Command(s): /SHOW, PNG

    Command(s): PLNSOL, and so on

  6. When using shell elements, another step must be included in order to view the results. Shells only accept INISTATE in the element coordinate system, and so when the stresses are initialized they are not in the global coordinate system. Therefore, in order to view the results correctly, you must first change the solution to plot the results in the solution coordinate system.

    Command(s): /VIEW, , , -1

    Command(s): /SHOW, PNG

    Command(s): PLNSOL, and so on


Release 18.2 - © ANSYS, Inc. All rights reserved.