In the optimization task editor, click the
Advanced tab.
Enter values specifying the Growth scale factor
and the Shrink scale factor. The growth scale factor is
applied to the displacement of nodes that are growing (increasing the volume of
the model) as a result of the shape optimization. The shrink scale factor is
applied to the displacements of nodes that are shrinking (decreasing the volume
of the model) as a result of the shape optimization.
It is recommended that you perform an optimization with default scale
factors of 1.0 and examine the results before you attempt an optimization with
modified scale factors. A value greater than 1.0 increases the incremental
displacement of nodes and accelerates the optimization. Conversely, a value
less than 1.0 decreases the incremental displacement of nodes and slows down
the optimization.
You should consider increasing the scale factors if the first few
iterations of the optimization produce little change in the position of the
surface nodes; for example, if you have a dense mesh with small element edge
lengths. Conversely, if the scale factor is too large, mesh quality will
suffer, individual elements may collapse, and the optimization may not be able
to converge on the optimal solution.
You should consider decreasing the scale factors if the original
model is close to being optimal. Decreasing the scale factor and slowing down
the optimization is also beneficial when the optimization includes many
geometric restrictions and when the beginning mesh quality is poor.
To optimize regions that are in contact, you may want to enter a
negative value to reverse the direction of the optimization. As a result, areas
of high stress will shrink and areas of low stress will grow.
Choose whether to update the optimization shape vectors after every
optimization cycle (default) or only after the first cycle.
The
Optimization module
determines an optimization displacement vector for every node in the design
area. The vector lies along the normal to the outer surface at the node and
indicates the direction of displacement during the optimization. If you choose
to update the optimization shape vectors after every optimization cycle, the
Optimization module
adjusts the vectors to account for changing conditions, such as changes in the
shape of the structure, the mesh quality, and design variable restrictions. If
you choose to update the optimization shape vectors only after the first
optimization cycle, the vectors remain fixed in subsequent cycles.
In most cases, the default value of updating the optimization shape
vectors after every optimization cycle provides better results because the mesh
smoothing algorithm is less restricted, resulting in an improved mesh quality.
Choose whether the step size should be determined by the minimum
displacement of the nodes in the design area during the optimization or the
average displacement.
The
Optimization module
examines your mesh and limits the amount of displacement of the nodes in the
design area during each optimization cycle. This limit prevents the large
displacement of one node from causing the collapse of a neighboring element. In
addition, the condition-based optimization algorithm provides control of the
displacement of the nodes in the design area after every design cycle—the step
size. The step size depends on the limit that the
Optimization module
has applied to the nodes. For example, if the
Optimization module
decreases the allowed displacement, the condition-based optimization algorithm
decreases the increment size.
This option allows you to choose which displacement is used by the
condition-based optimization algorithm to determine the step size. You can
choose the average value of the allowed displacement of the nodes in the design
area during the optimization or the minimum value (default). Selecting the
average value results in a larger step size and a faster calculation of the
optimum solution. However, selecting the average value can result in limited
displacement of nodes for which only small displacements are allowed causing
undesirable corners in the design area.
Choose the method that the
Optimization module
will use to interpolate the midside nodes.
If you select Linearly by position (default),
the optimization linearly interpolates the position of the midside node from
the optimized position of the connected corner nodes. If you select
By optimization displacement of corner nodes, the
optimization interpolates the position of the midside node from the
optimization displacement of the connected corner nodes.
If the nodes are in their original position, the midside node sits on
the line between the corner nodes and there is no difference between the two
interpolation methods. However, to prevent element bending, you must select
By optimization displacement of corner nodes.
If desired, toggle on Edge length for movement
vector and enter a value.
The
Optimization module
modifies the displacement of nodes in areas of high curvature to prevent the
mesh from collapsing because of a large volume change. In effect, sharp corners
are smoothed out. The default value of the minimum element edge length that
triggers smoothing is 5.0. A larger value results in a larger radius for the
smoothed region.
The
Optimization module
can use a filter to smooth out local stress peaks. You can define the filter
function by toggling on Max. influence radius for equivalent
stress and entering the following:
-
A value for the maximum distance between nodes that are influenced
by the filter.
-
A value that determines how much the local surface curvature will
be used to adjust the maximum distance between nodes that are influenced by the
filter. The default value is 0.2; a smaller value increases the effect of the
surface curvature.
-
A weighting value that controls the effect of the filter depending
on the distance from the node.
Volume is the only constraint you can apply to a shape optimization,
and you can specify that the volume be reduced to a specified value or to a
fraction of the initial value. The Equality constraint
tolerance specifies the minimum difference between the specified
volume constraint and the calculated volume that results in the
Optimization module
assuming the solution has converged. The
Optimization module
compares the absolute value of the difference with the tolerance value you
enter. The default value is 0.001.