Analysis Types

Geometrically Nonlinear Analysis

Geometrically nonlinear analysis (parameter NLGEOM) is only supported in controller-based topology, bead, and shape optimization.

The same applies for contact formulations and nonlinear material properties.

Allowed Analysis Types for Sensitivity-Based Optimizations

The responses from the two following analysis types in ANSYS® are allowed for sensitivity-based topology optimization:

ANTYPE,0
ANTYPE,2


Solution types	TOPO	SHAPE	BEAD	SIZING
ANTYPE,0 Linear static	C, S	C, S	C, S	S
ANTYPE,2 Modal analysis	C, S	C, S	C, S	S
with nonlinearities	C	C	C

C = controller-based optimizations
S = sensitivity-based optimizations

Only one set of the command LSSOLVE is allowed in each finite element file (CDB). In addition, the load case should be specified in an order starting from 1 and then the numbering should be chronologically increasing. The load case are referred in the parameter file using the number of the load case.

For example, if two static load case (LSSOLVE,1,2,1 and ANTYPE,0 in file_fe_static.s01 and file_fe_static.s02) are defined in the file file_fe_static_1.cdb and two eigenfrequency load case (LSSOLVE,1,2,1 and ANTYPE,2 in file_fe_dynamic.s01 and file_fe_dynamic.s02) are defined in the file_fe_dynamic_1.cdb, they are defined in the parameter file like:


FEM_INPUT
 ID_NAME = Two_files
 FILE = file_fe_static.cdb
 FILE = file_fe_dynamic.cdb
END_

and the two static responses can be referred to as:


DRESP
 ...
 LC_SET = STATIC,1,
 ...
END_

and


DRESP
 ...
 LC_SET = STATIC,2,
 ...
END_

and the two modal frequency responses can be referred to like:


DRESP
 ...
 LC_SET = MODAL,10001,...
 ...
END_

and


DRESP
 ...
 LC_SET = MODAL,10002,.....
 ...
END_

Important:

Significant improvement in the CPU-time is obtained using the following command in each load case:
```
OUTPR,ALL,NONE !No output in ASCII format
```
This ensures that no ASCII information is written as output. Therefore, adding this command in each load case is strongly recommended.
When two or more finite element input files (CDB) are referred in the FEM_INPUT command, the ANSYS® command /FILNAME, <name>, 1 must be added in all finite element input files (CDB) for uniquely defining the load case for each finite element input file (CDB).
When only one finite element input file (CDB) is referred in the command FEM_INPUT, the ANSYS® command /FILNAME, <name>, 1 does not must be added in the finite element input file (CDB). However, then the load case files must be named file.s01, file.s02, file.s03, etc.
In a case of analyses where boundary conditions are read from another ANSYS® analysis (for example, when a TEMPERATURE FILE is included), set the environment variable as
```
ansys_keep_result_requests=1
```
so that Tosca reads all the load cases or timesteps from the first analysis.