Optimization of a simply supported beam

In this section the optimization of a simply supported beam w.r.t. stress and subject to a non-increasing mass constraint is treated. This example shows how an optimization might be performed, the procedure itself is manually and by no way optimized. For industrial applications one would typically write generally applicable scripts taking care of the manual steps explained here.

This example uses the files opt1.inp, opt1.sh, opt2.fbl and op3.inp, all available in the CalculiX test suite. File opt1.inp contains the geometry and the loading of the problem at stake: the structure is a beam simply supported at its ends (hinge on one side, rolls on the other) and a point force in the middle. The von Mises stresses are shown in Figure 45.

**Figure 45:** von Mises stress in the starting geometry of the beam
$\begin{figure}\epsfig{file=opt1.eps,width=10cm}\end{figure}$

The target of the optimization is to reduce the stresses in the beam. The highest stresses occur in the middle of the beam and at the supports (cf. Figure 45). Since the stresses at the supports will not decrease due to a geometrical change of the beam (the peak stresses at the supports are cause by the point-like nature of the support) the set of design variables (i.e. the nodes in which the geometry of the beam is allowed to change during the optimization) is chosen as all nodes in the beam except for a set of nodes in the vicinity of the supports. These latter nodes are shown in Figure 46.

**Figure 46:** Nodes excluded from the set of design variables
$\begin{figure}\epsfig{file=opt2.eps,width=6cm}\end{figure}$

In order to perform an optimization one has to determine the sensitivity of the objective w.r.t. the design variables taking into account any constraints for every intermediate design step (iteration) of the optimization. The objective and the constraints are generally design responses. First, the sensitity of each design response is determined in a *SENSITIVITY step. Then, one design response is selected as objective and one or more as constraints in a *FEASIBLE DIRECTION step. In the latter step the sensitivity of the unconstrained objective is combined with the sensitity of the constraints in order to obtain the sensitivity of the constrained objective.

The design variables were already discussed and constitute the set of nodes in which the design is allowed to change. In the input deck for the present example this is taken care of by the lines:

*DESIGNVARIABLES,TYPE=COORDINATE
DESIGNNODES

“DESIGNNODES” is a nodal set containing the design nodes as previously discussed. For optimization problems in which the geometry of the structure is to be optimized the type is COORDINATE. Alternatively, one could optimize the orientation of anisotropic materials in a structure, this is covered by TYPE=ORIENTATION.

The objective is the design response one would like to minimize. In the present example the Kreisselmeier-Steinhauser function calculated from the von Mises stress in all design nodes (cf. *DESIGN RESPONSE for the definition of this function) is to be minimized. Again, the support nodes are not taken into account because of the local stress singularity. The objective is taken care of by the lines:

*DESIGN RESPONSE, NAME=STRESS_RESP
MISESSTRESS,DESIGNNODES,10.,100.

in the sensitivity step and

*OBJECTIVE,TARGET=MIN
STRESS_RESP

in the feasible direction step in the input deck. Notice that the node set used to define the Kreisselmeier-Steinhauser function (second entry underneath the *DESIGN RESPONSE card) does not have to coincide with the set of design variables. The third and fourth entry underneath the *DESIGN RESPONSE card constitute parameters in the Kreisselmeier-Steinhauser function. Specifically, the fourth entry is a reference stress value and should be of the order of magnitude of the actual maximum stress in the model. The third parameter allows to smear the maximum stress value in a less or more wide region of the model.

In addition to the objective function (only one objective function is allowed) one or more constraints can be defined in the feasible direction step. In the actual example the mass of the beam should not increase during the optimization. This is taken care of by

*DESIGN RESPONSE, NAME=MASS_RESP
MASS,Eall

in the sensitivity step and

*CONSTRAINT
MASS_RESP,LE,1.,

in the feasible direction step. For the meaning of the entries the reader is referred to *DESIGN RESPONSE and *CONSTRAINT. Notice that for this constraint to be active the user should have defined a density for the material at stake. Within CalculiX the constraint is linearized. This means that, depending on the increment size during an optimization, the constraint will not be satisfied exactly.

In the CalculiX run the sensitivity of the objective and all constraints w.r.t. the design variables is calculated. The sensitivity is nothing else but the first derivative of the objective function w.r.t. the design variables (similarly for the constraints), i.e. the sensitivity shows how the design response changes if the design variable is changed. For design variables of type COORDINATE the change of the design variables (i.e. the design nodes) is in a direction locally orthogonal to the geometry. So in our case the sensitivity of the stress tells us how the stress changes if the geometry is changed in direction of the local normal (similar with the mass CONSTRAINT). If the sensitivity is positive the stress increases while thickening the structure and vice versa. This sensitivity may be postprocessed by using a filter. In the present input deck (opt1.inp) the following filter is applied:

*FILTER,TYPE=EXPLICIT,EDGE PRESERVATION=YES,DIRECTION WEIGHTING=YES
3.

**Figure 47:** Stress sensitivity before filtering
$\begin{figure}\centering \epsfig{file=opt3.eps,width=6cm}\end{figure}$

**Figure 48:** Stress sensitivity after filtering
$\begin{figure}\centering \epsfig{file=opt4.eps,width=6cm}\end{figure}$

**Figure 49:** Mass sensitivity after filtering
$\begin{figure}\centering \epsfig{file=opt5.eps,width=6cm}\end{figure}$

The filter chosen to be explicit. For the filter, which is by default linear, a radius of 3 has been selected (it can be visualized as a cone at each design variable in which the sensitivity is integrated and subsequently smeared), sharp corners should be kept (EDGE PRESERVATION=YES, cf. *FILTER) and surfaces with a clearly different orientation (e.g. orthogonal) are not taken into account while filtering (or taken into account to a lesser degree, DIRECTION WEIGHTING=YES). The filtering is applied to each design response separately. Figure 47 shows the stress sensitivity before filtering, Figure 48 the stress sensitivity after filtering and Figure 49 the mass sensitivity after filtering. All of this information is obtained by requesting SEN underneath the *NODE FILE card.

**Figure 50:** Stress sensitivity taking the mass constraint into account
$\begin{figure}\centering \epsfig{file=opt6.eps,width=6cm}\end{figure}$

After calculating the filtered sensitivities of the objective function and the constraints separately (this is done in the sensitivity step) they are joined by projecting the sensitivity of the active constraints on the sensitivity of the objective function (this is done in the feasible direction step). For a mesh modification size of 1 (parameter underneath the *FEASIBLE DIRECTION card) this results in Figure 50.

The sensitivities calculated in this way allow us to perform an optimization. The simplest concept is the steepest gradient algorithm in which the geometry is changed in the direction of the steepest gradient. In the present calculations only one gradient is calculated (the one in the direction of the local normal) since a geometry change parallel to the surface of the structure generally does not change the geometry at all. So the geometry is changed in the direction of the local normal by an amount to be defined by the user. It is usually a percentage of the local sensitivity, the so-called mesh modification size, to be defined underneath the *FEASIBLE DIRECTION card. Here, a mesh modification size of 10 % was selected (i.e. 0.1).

In order to maintain a good quality mesh the other boundary nodes and the internal nodes should be appropriately moved as well. This is taken care of by a subsequent linear elastic calculation with the sensitivity-based surface geometry change as boundary conditions. The corresponding input deck with the name opt1.equ is automatically generated within the *FEASIBLE DIRECTION step.

This input deck contains the original geometry of the beam. The sensitivity-based surface geometry change is imposed by *BOUNDARY statements.

Furthermore, preservation of sharp edges and corners in the original structure is taken care of by linear equations. In order to obtain a good quality mesh at the free surface the fictitious elastic modulus is decreased with increasing distance from the free surface. Before running opt1.equ it is copied by script opt1.sh into opt2.inp.

**Figure 51:** Deformed mesh after one iteration
$\begin{figure}\centering \epsfig{file=opt7.eps,width=6cm}\end{figure}$

**Figure 52:** Mises stress after one iteration
$\begin{figure}\centering \epsfig{file=opt8.eps,width=10cm}\end{figure}$

The resulting deformed mesh is shown in Figure 51. The beam was thickened in the middle, where the von Mises stresses were highest. This should lead to a decrease of the highest stress value. In order to check this, a new sensitivity calculation was done on the deformed structure. To that end the deformation calculated based on opt2.inp is superimposed on the coordinates (by a call to opt2.fbl in script opt1.sh) and stored as opt3.inc. This file is included in input deck opt3.inp, which apart from the coordinates is a copy of opt1.inp. The resulting von Mises stresses are shown in Figure 52. The von Mises stress in the middle of the lower surface of the beam has indeed decreased from 114 to about 83 (MPa if the selected units were mm, N, s and K). Further improvements can be obtained by running several iterations.