RIMPORT, Source, Type, Loc, LSTEP, SBSTEP, Fname, Ext, --, SPSCALE, MSCALE
Imports initial stresses from an explicit dynamics run into ANSYS.

Compatible Products: – | Pro | Premium | Enterprise | Ent PP | Ent Solver | –


The type of analysis run from which stresses are imported.



Ignore initial stresses.



Get initial stresses from an earlier explicit (ANSYS LS-DYNA) run (default).


Type of data imported. Note that this is an ANSYS-defined field; the only valid value is STRESS.


Location where the data is imported. Note that this is an ANSYS-defined field; the only valid value is ELEM (data imported at the element integration points).


Load step number of data to be imported. Defaults to the last load step.


Substep number of data to be imported. Defaults to the last substep.


File name and directory path (248 characters maximum, including the characters needed for the directory path). An unspecified directory path defaults to the working directory; in this case, you can use all 248 characters for the file name.

The file name does not have a default; you must specify a name. It CANNOT be the current Jobname.


Filename extension (eight-character maximum).

The extension must be an RST extension (default).


Unused field.


Stabilization factor. This factor is used in a springback analysis to scale (up or down) the initial stiffness of the applied spring. No default; input a value only if you want to activate stabilization. If SPSCALE is blank, stabilization is not activated.


Acceptable stabilization stiffness (defaults to 1.0 X 10--4). In a springback analysis, iterations will stop when the applied spring stiffness comes down to this value. MSCALE is not used if SPSCALE is blank.


This command imports initial stress information into ANSYS from an earlier explicit (ANSYS LS-DYNA) run. The stress state from SHELL163 and SOLID164 elements in the explicit analysis is imported to the corresponding SHELL181 and SOLID185 implicit elements. For the shell elements, the current shell element thickness is also imported. This command is valid only before the first SOLVE command of the implicit analysis (which comes after the explicit analysis) and is ignored if issued after subsequent SOLVE commands (that is, stresses will not be re-imported).

RIMPORT is typically used to perform springback analysis of sheet metal forming. We recommend that you use SHELL163 elements in the explicit analysis with 3 to 5 integration points through the thickness. This ensures that the through-thickness stress distribution is transferred accurately to the SHELL181 elements. If more than 5 integration points are used, ANSYS imports resultants (forces and moments) to the SHELL181 elements. This implies that linearization of the through-thickness stress distribution is assumed in SHELL181 elements. If SHELL163 uses full integration in the shell plane, stress and thickness data are averaged and then transferred. For the solid elements, the stress at the SOLID164 element centroid is transferred to the SOLID185 element centroid. If SOLID164 has full integration, the stress is averaged and then transferred.

When the SPSCALE argument is specified, artificial springs with exponentially decaying stiffness (as a function of iterations) are applied. This technique is recommended only for those cases in which there are severe convergence difficulties. In general, you should first attempt a springback analysis without using the stabilization factors SPSCALE and MSCALE. (For more information on springback stabilization, see the ANSYS LS-DYNA User's Guide.)

This command is not written to the Jobname.CDB file when the CDWRITE command is issued. Further, the RIMPORT information is not saved to the database; therefore, the RIMPORT command must be reissued if the database is resumed.

This command is also valid in PREP7.

Distributed ANSYS Restriction This command is not supported in Distributed ANSYS.

Menu Paths

Main Menu>Preprocessor>Loads>Define Loads>Apply>Structural>Other>Import Stress
Main Menu>Solution>Define Loads>Apply>Structural>Other>Import Stress

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