Analysis Types

Allowed Analysis Types for Controller-Based and Sensitivity-Based Optimizations

In MSC Nastran®, the responses from the following analysis types are allowed:

Solution types	TOPO	SHAPE	BEAD	SIZING
SOL 101 Linear static	C, S	C, S	C, S	S
SOL 103 Modal analysis	C, S	C, S	C, S	S
SOL 106 Nonlinear analysis	C	C	C

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

SOL 101 and SOL 103 represent the linear static and linear eigenvalue analysis, respectively. Therefore, you must define a finite element file (for example, bdf) containing the SOL 101 and another finite element file (for example, bdf) containing the SOL 103 when both the responses from the static and frequency analysis are applied in the optimization formulation (for example, minimizing the compliance but still ensuring that the first eigenfrequency is higher than a given value).

However, there is a workaround to reduce the finite element analysis CPU-time for MSC Nastran® when responses consist of both static and modal responses. Only the SOL 103 solution can be used when both the responses from the static and frequency analysis are applied in the optimization formulation. This is done by adding static load case in the SOL 103 solution.

Important: The eigenfrequency solutions of the structure are not allowed to be prestressed (then convergence is not guaranteed). Thus, the user should define a dummy load case, which has no stresses and this dummy load case is referenced in the eigenfrequency analysis.

An example of combining several frequency analyses and several static analyses in SOL 103 is given below:

SOL 103
...
SUBCASE 1
$ dynamic loadcase 1
 METHOD=....
 SPC = ....
$ the structure is prestressed.
$ The REFEERED subcase (20) has no stresses !
 STATSUB = 20
SUBCASE 2
$ dynamic loadcase 2
 METHOD=....
 SPC = .....
$ the structure is prestressed.
$ The REFEERED subcase (20) has no stresses !
 STATSUB = 20
.......
SUBCASE 13
$ Static loadcase 1
 SPC = ....
 LOAD = ....
SUBCASE 14
$ Static loadcase 2
 SPC = ...
 LOAD = ...
…………..
SUBCASE 20
$ DUMMY static loadcase, which is stress free !
$ The command load should NOT be present here !
$ Boundary conditions are added for ensuring
$ no singularities of the global stiffness and mass matrix
 SPC = 3
BEGIN BULK
……..
ENDDATA

Important: Remember when defining the command DRESP in the parameter file to distinguish between the different types of load case (STATIC - MODAL) and the number of eigenfrequencies. Generally, laminate materials cannot be used in topology optimization. However, laminate materials as design elements are supported for MAT2, MAT8, and MAT9 in MSC Nastran®.

Temperature Loading

TEMPERATURE(LOAD) or TEMPERATURE(BOTH) in sub cases referring to the following types are supported for temperature loadings using SIMULIA Tosca Structure:

• TEMP
• TEMPD
• TEMPP1
• TEMPRB
• TEMPAX

Important: Different sub case can have different or nonpresent temperature loadings. STRAIN_ENERGY as DRESP when having temperature loading is not allowed for MSC Nastran® because MSC Nastran® is calculating the strain energy without isotropic thermal expansion. For temperature loadings, shell elements (CTRIA3, CTRIA6, CTRIARCQUAD4, CQUAD8, CQUADR ) are not supported within the design domain. However, the elements can be included in the model. The material parameters are not allowed to be a function of the temperature. Thus, TEMPERATURE(MATERIAL) and TEMPERATURE(INITIAL) are not supported. TEMPBC and TEMPF are not supported as boundary conditions and temperature-dependent material, respectively.