About Design variables (DV_SHAPE)

Design variables for shape optimization are defined when assigning a node group to the design area.

Related Topics
Defining Design variables
In Other Guides
DV_SHAPE

Important:

Only surface nodes are allowed as design nodes.

  • The design nodes must define one or more continuous areas, i.e., the individual design areas must consist of at least three design nodes. Single design nodes without neighboring design nodes are not permitted.
  • Only corner nodes (from finite elements) are supported as design nodes. Midside nodes may be included in the design node group but the optimization displacements of the midside nodes of second order elements is interpolated from the optimization displacement of the adjacent corner nodes, which maintains a curvature of the initial design during optimization.

Strictly speaking, design variables are the signed amounts of optimization displacement applied to the design nodes. In unrestricted tasks, the direction of the optimization displacement vector corresponds to the outer surface unit normal on the node and the amount of displacement is determined by the optimization procedure. Restrictions influence the amount and direction of the optimization displacement vector.

Basically there are three cases that may occur:

  • Growth means that a design node is moved outwards (positive amount of displacement).
  • Shrinkage means that a design node is moved inwards (negative amount of displacement).
  • Neutral means that a design node is moved neither outwards nor inwards (zero displacement).

Important:

The optimization displacement vector contains the optimized changes in positions of the nodes and not the displacements of the nodes obtained from the FE analysis.

When unrestricted design nodes lie in component areas in which they have only a little mechanical effect on the system as a whole, an undesirable “shrink effect” may occur. Therefore, design areas should not be selected before the mechanical component behavior is known. It is recommended to analyze the mechanical behavior of the component in a preliminary FE calculation before specifying the design area.

Determination of optimization displacement vectors

  • The optimization displacement vector on the design node is determined by superimposing all external element normal vectors on the boundaries of neighboring elements. In two-dimensional models the normals are formed relative to element edges and in three-dimensional to element surfaces. The only element edges or element surfaces that are taken into consideration are those spanning design nodes. Isolated design nodes (neighboring nodes on the surface are not design nodes) are not permitted and must be removed from the design node group. The optimization displacement direction is a uniform vector.

    Example:

    In a two-dimensional model each design node has two neighboring nodes on the boundary of the component. If both of these neighboring nodes are design nodes, see the figure above on the left, two normal vectors are formed, one each for the respective element edges, and superimposed. If only one of the neighboring nodes is a design node, see the figure above on the right, there is only one normal vector. This is identical with the normal vector of the design node.



  • If the displacement direction of a node is restricted by a design variable constraint (DVCON_SHAPE) the direction of the optimization displacement vectors is correspondingly adjusted.
  • The optimization displacement vector is derived from scaling the optimization displacement direction with the signed amount of displacement calculated by the optimization procedure.
  • The length of the optimization displacement vector may also be influenced by design variable constraints (DVCON_SHAPE).

Note:

  • The optimization displacement vector determined by the optimizer is adjusted to the changed conditions in each design cycle (e.g. shape of the structure, effective restrictions, mesh quality, etc.). The optimization displacement vectors are therefore not constant; they are subject to certain changes in each cycle.
  • With the VECTOR parameter in the optimization settings (command OPT_PARAM) it is possible to control when the optimization displacement vectors are calculated.

Supported elements attached to shape sensitivity design nodes

Valid element types for sensitivity based shape optimization

Abaqus element type

ANSYS® element type

MSC Nastran® element type

Solid elements

  

SOLID_TETRA_4

C3D4

 SOLID285

CTETRA4

SOLID_TETRA_10

C3D10

C3D10I

SOLID148

SOLID187

SOLID92

CTETRA10

SOLID_BRICK_8

C3D8

C3D8I

SOLID185

SOLID45

 CHEXA8