Analysis Types

Geometric Nonlinear Analysis

Geometric nonlinear analysis (parameter NLGEOM) can be used in topology optimization (both, controller and sensitivity-based), shape and bead (both, controller and sensitivity-based) optimization as well as in sizing 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 must 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 substeps in Tosca Structure. A step in the finite element input file must 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

and

*STEP
*Heat Transfer, steady state
...
*END STEP

Remarks

• If PERTURBATION is added, the step command *STEP will be recognized as a linear static solution in Tosca Structure. If PERTURBATION is not added, the analysis is nonlinear. 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, for example,

  
  *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.