Analysis Types

In Abaqus a general static STEP definition without the explicit PERTURBATION option is nonlinear. That means to optimize these models with SIMULIA Tosca Structure an advanced license for SIMULIA Tosca Structure.nonlinear is needed. Otherwise use only *STEP, PERTURBATION in Abaqus input deck.

Geometric Nonlinear Analysis

Geometric nonlinear analysis (parameter NLGEOM) can be used in topology optimization (both, controller and sensitivity based) and shape controller optimization. An excessive deformation of soft elements can occur during topology optimization. This does not occur for a linear analysis. However, in the case of a geometric nonlinear analysis this leads to an adverse effect on the convergence which eventually leads to the termination of the analysis. This has to be considered when applying topology optimization using hyperelastic material.

Optimizing Using Abaqus/Explicit

The use of Abaqus/Explicit is permitted for shape controller optimization of quasi static problems. The ODB result interface must be activated which is also default, see Files and Formats. The result of one explicit analysis step is divided into 20 increments which are interpreted as 20 single sub-steps in SIMULIA Tosca Structure. A step in the finite element input deck has to be divided into several steps if the results of more than 20 substeps should be included in the optimization.

Topology, bead and shape sensitivity optimization in combination with Abaqus/Explicit is not supported.

Allowed Analysis Types for Sensitivity-Based Optimizations

In Abaqus responses from the two following analysis types are allowed:

*STEP
 *STATIC
 ...
*END STEP

and

*STEP, PERTURBATION
 *STATIC
 ...
*END STEP

and

*STEP
 *FREQUENCY
 ...
*END STEP

Note: For sensitivity based shape optimization (SHAPE_SENSITIVITY) and sensitivity based bead optimization (BEAD_SENSITIVITY) the static step is only supported with PERTURBATION.

Remarks

  • If PERTURBATION is added then the step command *STEP will be recognized as a linear static solution in SIMULIA Tosca Structure. If PERTURBATION is not added then the analysis is non-linear. The sensitivity-based algorithm supports geometrical nonlinearities (NLGEOM) and contact for Abaqus.
  • Abaqus has no predefined numbers for the load cases. Therefore, the first defined load case in the INP file is recognized as load case one, the second defined load case in the INP file is recognized as load case two and etc.
  • Computationally, it is recommended that the user defines the static load case in Abaqus using the load case command *LOAD CASE in one *STEP and not be defining more steps using *STEP several times. Hence, using the load case command *LOAD CASE will keep the CPU-time significant lower, e.g. 
    *STEP, PERTURBATION
 *STATIC
 *LOAD CASE
 ...
 *END LOAD CASE
 *LOAD CASE
 ...
 *END LOAD CASE
 ...
*END STEP
  • The results of the finite element analysis can only be read from the ODB file when the command *LOAD CASE is activated (default) and not the FIL file.
  • The user can decide to write to the FIL file only when *STEPS are defined in the Abaqus input deck. Reading from the FIL file instead of ODB file is activated when the following command is added in the CONFIG command: 
    CONFIG
 ...
 ${res_ext} = "fil";
 ...
END_