14.1. Performing an Explicit-to-Implicit Sequential Solution

In sheet metal forming operations, springback deformation is an essential parameter that significantly complicates the design of forming tools. Springback deformation is best defined as the dimensional change of the formed part from that of the die which occurs from elastic deformations during unloading. In most dynamic metal forming operations, the highly nonlinear deformation processes tend to generate a large amount of elastic strain energy in the blank material. This elastic energy, which becomes stored in the blank while it is in dynamic contact with the die components, is subsequently released after the forming pressure is removed. This release of energy, which is the driving force for springback, generally causes the blank to deform towards its original geometry. Hence, the final part shape in a sheet metal forming process not only depends upon the contours of the dies, but also on the amount of elastic energy stored in the part while it is being plastically deformed. Since the amount of elastic energy stored in a part is a function of many process parameters such as material properties and interfacial loads, predicting springback during forming is extremely complicated. This poses significant problems to designers and analysts who must accurately assess the amount of springback that will occur during a forming process so that a final desired part shape can be obtained. Herein lies the great advantage of performing an explicit-to-implicit sequential solution. By simulating the dynamic forming process explicitly, and then modeling the springback deformations implicitly, stringent design tolerances can be attained for sheet metal forming operations.

In an explicit-to-implicit sequential solution, you must first run the ANSYS LS-DYNA program to simulate the metal forming process. In the explicit metal forming analysis, the sheet metal blank being deformed must consist of SHELL163 and/or SOLID164 elements. Then the deformed shape, stresses, and thicknesses of these elements only are transferred into the corresponding implicit ANSYS elements (SHELL181 and SOLID185). Once valid boundary conditions are specified on the blank material, implicit simulation of the elastic springback within the workpiece can be performed.


Note:  Only elastic properties are considered in the implicit phase. This implies that the analysis is purely elastic unloading from the formed state (configuration). The displacements are interpreted as the changes in these quantities from the formed configuration.


A detailed description of the explicit-to-implicit solution procedure follows.

  1. Run the explicit analysis as described earlier, using Jobname1. You must use SHELL163 and/or SOLID164 to model the working piece in order to analyze the springback effect in a subsequent ANSYS implicit analysis. In addition, you must use one of the following element formulations for the SHELL163 elements: KEYOPT(1) = 1, 2, 6, 7, 8, 9, 10, 11, or 12 (10 and 12 are recommended). Solve and finish the analysis.

    You should always check your explicit analysis solution from ANSYS LS-DYNA carefully before proceeding with the ANSYS implicit analysis. Specifically, check whether there is any undesirable dynamic effect left in the structure at the end of the explicit run (using POST26).

  2. Save the explicit analysis database to file Jobname1.DB.

    Command(s): SAVE
    GUI: Utility Menu> File> Save as


    Note:  If you do not save your Jobname1.DB file at this point, then the database for this explicit run will not be saved. Only the database file for the subsequent implicit run will be saved.


  3. Change to Jobname2 to prevent the explicit results files from being overwritten.

    Command(s): /FILNAME,Jobname2
    GUI: Utility Menu> File> Change Jobname

  4. Reenter the preprocessor.

    Command(s): /PREP7
    GUI: Main Menu> Preprocessor

  5. Convert explicit element types to corresponding companion implicit element types. (Note that the 2-D explicit element, PLANE162, and composite shell element SHELL163 with KEYOPT(3) = 1, cannot be used in a sequential solution.) The companion explicit-implicit element type pairs are:

    Explicit Element TypeImplicit Element Type
    SHELL163 SHELL181
    SOLID164 SOLID185
    COMBI165 COMBIN14
    MASS166 MASS21

    Although all explicit element types are converted, only SHELL163 and SOLID164 data (stresses and thicknesses for SHELL163, and stresses for SOLID164) are transferred to SHELL181 and SOLID185 (via the RIMPORT command; see step 12).

    Command(s): ETCHG,ETI
    GUI: Main Menu> Preprocessor> Elem Type> Switch Elem Type

  6. Redefine the key options, real constants, material properties, boundary conditions, and loading values on any implicit elements that are converted from explicit element types. (For SHELL163 elements that were converted to SHELL181, you do NOT need to redefine the real constants, but you do need to redefine the other values. For SOLID164 elements that were converted to SOLID185 elements, you need to specify the uniform reduced integration option by setting KEYOPT(2) = 1.) The TYPE, REAL, and MAT numbers from the explicit elements are retained, but the actual key option and real constant values are reset to zero or the default settings.

    Command(s): KEYOPT, R, MP, etc.
    GUI: Main Menu> Preprocessor> Element Type/Real Constants/Material Properties/Loads


    Note:  Only linear elastic material properties (as specified with the MP command) can remain active in the ANSYS implicit phase. Delete any inelastic material properties (as specified with the TB command) from the ANSYS LS-DYNA run.


  7. Turn off shape checking because elements may have undergone considerable deformation during the explicit analysis.

    Command(s): SHPP,OFF
    GUI: Main Menu> Preprocessor> Checking Ctrls> Shape Checking

  8. Redefine the implicit elements to the deformed configuration.

    Command(s): UPGEOM
    GUI: Main Menu> Preprocessor> Modeling> Update Geometry

  9. Unselect or delete any unnecessary elements (mainly those making up any rigid bodies from the explicit analysis), or convert them to null elements. Any explicit elements that are not either unselected, deleted, converted to null elements, or converted to implicit will remain active in ANSYS, which will produce an error and terminate the analysis. Also, if the rigid bodies in the explicit analysis were made up of SHELL163 or SOLID164 elements, these elements must be unselected, deleted, or converted to NULL elements before importing stresses and thicknesses (from SHELL163 to SHELL181, or SOLID164 to SOLID185) by the RIMPORT command (See Step 12); otherwise, the implicit analysis will be terminated.

    Command(s): ESEL, EDELE
    GUI: Utility Menu> Select> Entities or
    Main Menu> Preprocessor> Delete> Elements

  10. Reenter the solution processor.

    Command(s): /SOLU
    GUI: Main Menu> Solution

  11. 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, etc.
    GUI: Main Menu> Solution> Loads> Apply> Structural-Displacement> On Nodes, etc.

  12. Import stresses and changed thicknesses (from SHELL163 to SHELL181, and from SOLID164 to SOLID185). For SOLID164, only the stresses are transferred. For SHELL163, the stresses and thicknesses are transferred. The deformed integration point thicknesses are averaged before being transferred to the implicit analysis. These thicknesses override those defined using real constants.

    Command(s): RIMPORT
    GUI: Main Menu> Solution> Loads> Apply> Structural-Other> Import Stress

  13. Turn large deformation effects on.

    Command(s): NLGEOM,ON
    GUI: Main Menu> Solution> Sol’n Controls

  14. Solve and finish the analysis.

    Command(s): SOLVE, FINISH
    GUI: Main Menu> Solution> Solve> Current LS
    Main Menu> Finish

Once you have solved the analysis, you can use any of the standard ANSYS postprocessing functions to review your results.

The following is a sample input stream for performing an explicit-to-implicit sequential solution.

/batch,list
resume,stamp1,db          ! resume explicit database (explicit
                          ! problem run previously)
/filename,stamp2          ! change jobname so explicit results
                          ! are not overwritten
/prep7
etchg,eti                 ! convert explicit to implicit elements
r,1,.01,.01,.01,.01       ! change real constants (deformed
                          ! thicknesses used by RIMPORT)
ddel,all                  ! delete constraint loads from
                          ! explicit analysis
tbdelete,all,all          ! delete material models (retain
                          ! linear material properties)
upgeom,,,,stamp1,rst      ! redefine the implicit elements
                          ! at the deformed geometry
d,n1,ux,0.0,,,,uy,uz      ! Set necessary constraints on the model
d,n2,ux,0.0,,,,uy         !  (at least 3 non-colinear nodes)
d,n3,ux,0.0
  esel,s,ename,,181       ! Select only corresponding SHELL181
                          ! elements (No “former” rigid bodies)
nsle,s,1                  ! Select only SHELL181 nodes
shpp,off                  ! Turn off shape checking
finish
/solution
nlgeom,on                   ! Turn on nonlinear geometry
rimport,dyna,,,,,stamp1,rst ! Import stresses and thicknesses from
                            ! explicit analysis
save
solve
finish

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