Unlike explicit-to-implicit solutions, which are used only in forming applications, structural implicit-to-explicit sequential solutions can be used for a broad range of engineering problems where a structure's initial stress state affects its dynamic response. The following is a short list of applications in which this type of implicit-to-explicit solution may be useful.
Droptest simulation of prestressed consumer goods
Bird-strike of a rotating engine blade (and blade containment)
Mounting and bearing loads on a turbine
Pressure vessels with initial internal pressure
Golf club striking a preloaded (wound) golf ball
Dynamic response of bolted joints
Dynamic response of a turbine engine under thermal straining
In an implicit-to-explicit sequential solution, you must first run an ANSYS implicit structural analysis to apply a preload to the structure being analyzed. In this implicit analysis, completely constrain all of the nodes of any elements that will only be used in the explicit analysis (e.g., the bird in a bird-strike problem). The nodal displacements and rotations from the ANSYS implicit solution are written to the ANSYS LS-DYNA dynamic relaxation file drelax.
Note: Temperatures from the ANSYS implicit structural solution are also written to the drelax file, but are not used by LS-DYNA. See Special Considerations for Thermal Loading for more information on how temperature loads are handled.
After defining additional loads, initial velocities, different material models (e.g., adding plasticity), etc., the explicit dynamic analysis can be conducted. The first part of this analysis uses the displacement results stored in the drelax file to do a stress initialization to a prescribed geometry. This preload is applied in pseudo time over 101 time steps to damp out any kinetic energy. The transient portion of the analysis then begins at time zero with a stable preloaded structure.
A detailed description of the implicit-to-explicit solution procedure follows.
Run the implicit analysis as described earlier, using Jobname1. Keep in mind that this analysis must be small strain with linear material behavior. The only element types that can be used for an implicit-to-explicit sequential solution are:
| SHELL181 |
| SOLID185 |
| COMBIN14 |
| MASS21 |
Define any additional nodes and elements that are necessary to complete the explicit solution (for example, the bird in a bird-strike simulation, or a rigid surface that a phone would impact in a droptest). These additional nodes and elements may not be part of the implicit analysis, but they need to be defined here nonetheless. These additional nodes must be constrained (using D,ALL,ALL,0).
Solve and finish the analysis.
Save the implicit analysis database to file Jobname1.DB.
Note: If you do not save your Jobname1.DB file at this point, then the database for this implicit run will not be saved. Only the database file for the subsequent explicit run will be saved.
Change to Jobname2 to prevent the implicit results files from being overwritten.
Reenter the preprocessor.
Convert implicit element types to corresponding companion explicit element types. Note that the 2-D explicit element, PLANE162, cannot be used in this type of sequential solution. (PLANE162 is allowed in a thermal implicit-to-explicit sequential solution; see Thermal Implicit-to-Explicit Solution for details.) The corresponding companion implicit-explicit element type pairs are:
| Implicit Element Type | Explicit Element Type |
|---|---|
| SHELL181 | SHELL163 |
| SOLID185 | SOLID164 |
| COMBIN14 | COMBI165 |
| MASS21 | MASS166 |
Implicit elements not listed above can also be used, as long as they are defined by the same number of nodes, but they will not automatically be converted to explicit elements when ETCHG is issued. These elements must be converted manually using EMODIF. Higher-order implicit elements can also be used, but must also be converted manually using EMODIF with the corner nodes only. Do NOT delete or unselect the midside nodes - these nodes must be written to the LS-DYNA input file. The drelax file contains solutions for these nodes, but the ANSYS LS-DYNA explicit elements do not use these nodes in their definition.
Redefine the key options, real constants, boundary conditions, and loading values on the explicit elements. The TYPE, REAL, and MAT numbers from the implicit elements are retained, but the actual key option and real constant values are reset to zero or the default settings.
Remove constraints from the additional nodes or elements defined in Step 2, above.
Reenter the solution processor.
Read nodal displacements, rotations, and temperatures from the implicit results file, and write this information to an ASCII LS-DYNA file, drelax.
Initialize the structure to the prescribed geometry according to the displacements and rotations contained in the drelax file. In this step, LS-DYNA applies the load information (displacements and rotations) from the drelax file to the original geometry and calculates the deformed geometry, which it then uses as a starting point for the explicit analysis.
Apply any necessary loading for the explicit run.
Solve and finish the explicit dynamics analysis. You can then return to the implicit solution, if necessary.
The following is a sample input stream for performing an implicit-to-explicit sequential solution.
/batch,list
resume,drop1,db ! Resume implicit database (implicit
! problem run previously)
/filename,drop2 ! Change jobname so implicit results are
! not overwritten
/prep7
etchg,ite ! Convert implicit to explicit elements
mp,dens,1,.0216 ! Change material properties
ddel,all ! Delete constraint loads from implicit
! analysis
tb,plaw,1,,,8 ! Define explicit dynamics nonlinear
! material models
edmp,rigid,2,7,7 ! Change an existing material to a rigid body
edcgen,assc ! Specify contact algorithms (if any)
nsel,s,loc,x,0 ! Select geometry for new constraints to be
! specified
nsel,a,loc,y,0
d,all,ux,0 ! Set necessary constraints on the rigid
! body, etc.
d,all,uy,0
finish
/solution
rexport,dyna,,,,,drop1,rst ! Create DRELAX file from implicit
! results
eddrelax,ansys ! Specify stress initialization by prescribed
! geometry
edpart,create ! Create parts for loading
edpart,list ! List parts
edvel,… ! Apply initial velocities
edload,add,rbvx,,2,time,load,0 ! Apply phase = 0 loads
save
solve
finishMost types of temperature loads that are applied in the implicit structural analysis will be carried over to the subsequent explicit analysis; these include temperature loads applied with the BF, BFK, BFL, BFA, BFV, LDREAD, TUNIF, BFUNIF, and TREF commands. If you do not want to include the temperature loads in the explicit analysis, you can delete them in the ANSYS structural analysis phase (before you convert the model to explicit elements via ETCHG), or you can delete them in the explicit analysis.
In the explicit analysis phase, you can use the BFLIST command to list the temperature loads mentioned above. You can then use the BFDELE command to delete any temperatures originally defined with the LDREAD command or one of the "BF" type commands listed above. If you do not want to include a uniform temperature carried over by TUNIF (or BFUNIF,TEMP) you should set TUNIF to the reference temperature (which is the temperature specified on the TREF command). Any temperature loads that are not deleted will be written to the LS-DYNA input file, Jobname.K, automatically when the SOLVE or EDWRITE command is issued.
In order for temperature loads to take effect in the explicit analysis, you must use the Temperature Dependent Bilinear Isotropic material model or the Elastic Viscoplastic Thermal material model for portions of the model that are subjected to temperature loading. Note that only the SHELL163 and SOLID164 elements can accept temperature loading in a structural implicit-to-explicit sequential solution.
Note: The temperature loads in the implicit analysis are also written to the drelax file when REXPORT is issued (Step 12 above). However, the temperatures contained in the drelax file are not used in the LS-DYNA calculation.
Appendix D contains a complete example of a thermal/structural preload followed by a structural transient dynamic analysis.
Currently, ANSYS LS-DYNA does not support applying a thermal transient in a model that includes a thermal preload.