## 1. Introduction

The astronomical instrumentation needs high level of image quality and stability. The quality of images processed by an optical instrument can be referred to the size of the spot and/or the point spread function (p.s.f.), while the stability is related to the displacement of the spot centroid during the observations.

The opto-mechanical elements are designed and manufactured in order to have enough stiffness to minimize shape deformations and flexures due to thermo-gravitational loads. Old traditional design philosophy answered to the problem with high thicknesses and related high masses. Heavier glasses means heavier supports and high gravitational dependent misalignment. The technological research is nowadys devoted to the light weighing of opto-mechanical systems either keeping enough stiffness, or actively correcting optical surfaces and/or positions. Complementary to the technological research, the development of powerful numerical tools added to an huge enlargement of CPU computing capacity have been offered a significant improvement into the engineering design enhancing the complexity and efficiency of the design phase.

Optical lens design refers to the calculation of lens construction parameters (variables) that will meet a set of performance requirements and constraints, including cost and schedule limitations. Construction parameters include surface profile types (spherical, aspheric, holographic, diffractive, etc.), and the parameters for each surface type such as radius of curvature, distance to the next surface, glass type and optionally tilt and decenter. The optical design exploits numerical raytracing techniques to maximize the design efficiency. Ray tracing is a method for calculating the path of waves or particles through a system with regions of varying propagation velocity, absorption characteristics, and reflecting surfaces. Under these circumstances, wavefronts may bend, change direction, or reflect off surfaces, complicating analysis. Ray tracing solves the problem by repeatedly advancing idealized narrow beams called rays through the medium by discrete amounts. Simple problems can be analyzed by propagating a few rays using simple mathematics. More detailed analyses can be performed by using a computer to propagate many rays.

On the other hand, structural design is nowadays mainly based onto The finite element method (FEM). It is a numerical technique for finding approximate solutions of partial differential equations (PDE) as well as of integral equations. The solution approach is based either on eliminating the differential equation completely (steady state problems), or rendering the PDE into an approximating system of ordinary differential equations, which are then numerically integrated using standard techniques such as Euler’s method, Runge-Kutta, etc.

The optimization procedure refers to choosing the best element from some set of available alternatives. In the simplest case, this means solving problems in which one seeks to minimize or maximize a real function by systematically choosing the values of real or integer variables from within an allowed set. This formulation, using a scalar, real-valued objective function, is probably the simplest example; the generalization of optimization theory and techniques to other formulations comprises a large area of applied mathematics. More generally, it means finding “best available” values of some objective function given a defined domain, including a variety of different types of objective functions and different types of domains.

In this chapter we present a possible simplified application of the optimization theory to opto-mechanical design that has been integrated into a multipurpose combined opto-mechanical numerical design process. In particular we will show a single variable optimization routine oriented to minimize mass while keeping the optical displacement below a certain value [12]. In addition considering the general purpose of this book will be briefly shown the modeling techniques used in some application to simulate the performances of functional materials like SHape Memory Alloys and Piezoelectrics. This techniques has been implemented in the optimization algorithm to maximize the efficiency of this devices in the actuation of active Mirrors based onto composite materials.

## 2. Framework

The integrated design procedure proposed exploits the huge power of numerical computation for the design of instrumentations for astronomy. The framework can be ideally seen as “server to client” communication, where a managing server code feeds input data to computing clients and extracts the desired results. The adopted software are:

Matlab® is the server software: it adapts the inputs for the client codes and evaluates their outputs.

MSC-Nastran® is the FEA client code: it receives from the server code proper models and computes mechanical results (thermo-gravitational displacements, eigen-frequencies,...)

ABAQUS® is a FEA client code used alternatively to MSC-Nastran® in case of user defined contitutive laws.

Zemax® is the Raytracing client code: it receives the optical perturbations properly adapted and evaluates the optical performance of the system (image quality, image stability,...).

The procedure obtains image quality and motion of an opto-mechanical system under thermal and/or gravitational loads. A simplified mesh (1d or 2d elements) of a possible opto-mechanical configuration is prepared starting from the optical design. Then Matlab® implement physical properties into the input file and feeds the MSC-Nastran® solver. The displacements are extrapolated and reorganized in order to be compliant with the Zemax® reference systems. Matlab® runs the Zemax® solver and extract the desired data (Spot radius, EE80, p.s.f.,...). In this way a first order estimation of the Instruments mechanical stability is obtained and can be easily implemented an optimization process based onto the smart modification of the physical and mechanical properties depending onto the Zemax® results.

Easy modifications can be introduced to improve the accuracy of the algorithm’s results. A “qr” based Zernike fitting function has been implemented in order to allow the modeling of optical surface deformations introducing surface errors into the Zemax optical layout. This configuration can be used both for overall system analysis and for detailed object analysis like active optical element performances evaluation[11, 13].

### 2.1. FEA

#### 2.1.1. Mesh generator

The opto-mechanical Finite Element modeling starts from the optical model. Masses, Center of Gravity and Optical Centers of each element are extracted from the optical file. A simplified Matlab® discretization function can be used when the instrument is very simple (i.e. two or three elements); in case of complex geometries the preliminary mesh can be prepared through dedicated software (Femap®, Hypermesh®,...); this raw discretization usually models a bench or a box that profiles the optical systems through 2D elements. Due to the high interaction level required we decide to omit the automation of the whole bench meshing.

The opto-mechanical elements are then modeled through semi-rgid elements and concentrated masses. The weight of opto-mechanical subsystem is simplified considering double the optical element mass to include the contribution of mechanical mountings. The semi-rigid element (80%) is used instead of the rigid one in order to simulate the finite stiffness of the mountings; the master node is the optical vertex and the slave are the system’s CoG and the connection points. Depending onto the geometry and the interface of the instruments, sometimes it is necessary to introduce some reinforcement beams or support trusses that can be easily modeled through 1d beam elements. In some cases, in particular with large optics or active optical systems, it is important to model the whole optical surface through 2D elements connected to the main bench via 1D beams.

Matlab® can read the model mesh and writes the input file for the Finite Element processor modifing both the geometry and the properties (thickness of 2D and section of 1D elements) if needed. This feature is the crucial point that helps the designer to optimize the performances of the system.

Different codes can be used for different application. The interaction with ABAQUS[1] is necessary for smart structures applications thanks to the higher performances of the code in presence of user defined constitutive laws. The routines interacts with NASTRAN[6] for opto-mechanical performances prediction and optimization.

#### 2.1.2. Fast extrapolation algorithm

To evaluate the whole performances of an instrument is necessary to verify the performances within all the loading conditions. In particular it should be possible to find situations where the errors tends to auto-compensate or, on the other hand, are magnified by the interaction with other perturbations.

Here is presented a simple extraction algorithm that can be used to reduce the number of FEA analysis required. The basic idea is to perform less analyses as possible and extracts all the displacement fields in an analytical way. Doing this, one can also predict the displacements in every condition of the gravitational load with or without the thermal expansion.

If the *g* vector rotates in the whole 3D space the analytical definition of the displacements is more complex. First of all it is necessary to define how decompose the *g*vector in the three directions *x*, *y* and *z*. We have decided to use that shown in Figure 2. In this way we can simulate the real rotations of the telescope, the *α* angle is the declination and *β* angle represents the rotation of the telescope around the optical axis. Doing this, the components of the g-vector are:

The equation that ties force and displacements can be written as:

Where *D* is the displacements vector, *K* the stiffness matrix, and *F* is the loads vector. If we combine Equations 1 and 2, through some algebraical operations, we obtain the general form:

Where *A*_{1} is the vector of the maximum amplitudes of the displacements when the *g* vector is in the *xy*plane, *A*_{2} is the vector of the maximum amplitudes of the displacements when the *g* vector is orthogonal at the *xy*plane, *α* and *β* are the angles of equation 1 and *ϕ* is a phase vector of the sinusoids. In order to have the whole displacement we need three known points to determinate the three unknown variables: the amplitudes and the phase.

Equation 2 can be further detailed introducing the thermal loads simply by adding the *C* _ *T* term, where *C* C is a vector constant which ties the temperature *T* at the displacement *D*. If we consider *T*_{d} as the the vector of the displacements due to the thermal loads, Equation 3 becomes:

Now with only four known points (for four unknown variables: the two amplitudes, the phase and the thermal displacement) we can have the overall displacements and the possibility to decompose the thermal contribution.

In addition we should note that Equation 4 can be simplified if the known points are wisely taken. In fact if the sampling loading condition are:

*α*= 90,*β*= 0,*δT*= 0: gravity vector along*X*axis, no thermal load.*α*= 90,*β*= 90,*δT*= 0: gravity vector along*Y*axis, no thermal load.*α*= 0,*β*= 0,*δT*= 0: gravity vector along*Z*axis, no thermal load.*g*= 0,*δT*≠0: only thermal load.

The algebraic simplification of Equations 1 and 2

#### 2.1.3. Zernike fitting

The surface Deformations are processed through a Zernike Fitting algorithm. In precision optical manufacturing, Zernike polynomials are used to characterize higher-order errors observed in interferometric analysis, in order to achieve desired system performance. They are commonly used in active and adaptive optics where they can be used to describe wavefront aberrations.

The most general way to express the Zernike polynomials is in the form:

Where the *n* index defines the order of the radial power so an *n* value of 5 would indicate all polynomials whose maximum radial power is *ρ*^{5}. Only certain values for *m* are allowed once *n* is chosen; *n* + *m* must be even, and 0 ≤ *m* ≤ *n*. The surface error is defined as[2]:

where*i*is the node number, *δ*_{i}is FE displacement of *i*_{th}node, *D*_{i} is the polynomial displacement of the *i*_{th}node. The series of *D* can be symbolically written as *D*_{i} = Σ*c*_{j}*f*_{ij}where *c*_{j}are the coefficients of the polynomial. The best fit coefficients can be found minimizing the error *E* respect to *c*_{j}:

This system is then solved finding the best fitting coefficients through an orthogonal-triangular decomposition (Matlab® *qr*function). The first 28 coefficients of the Zernike Polynomial have been taken into account in this application.

### 2.2. Raytracing

#### 2.2.1. Zemax® and Matlab® data exchange

The raytrancing software Zemax® is used to evaluate the optical performances. Zemax® has a very powerful feature which allows another software to establish a communication link to extract lens data. The idea is based onto a program that use Zemax® like a remote application to trace rays through the lenses, and then extracts the data to be sent to other programs for further analysis or computation[17].

The communication between the application and Zemax® is accomplished using Dynamic Data Exchange (DDE). DDE is a protocol defined within the Windows operating system for sharing data between programs. Two programs can establish a DDE link, with one program acting as the “server” and the other the “client”. The client generally requests specific data from the server, and the server sends the data back to the client.

Two main function must be used when exchanging data with Zemax that are the link opening and closing. To establish a DDE link with Zemax®, the client program must broadcast a message to all top level windows that includes a reference to the application name, and the topic name. The topic name indicates to Zemax® what data is being requested.

Zemax® supports a number of capabilities under DDE. Each function/item is given a name, that is passed to the Zemax® server using the proper request protocol. Zemax® responds to each item request with requested data. Most of them are passed from Zemax® back to the application (Matlab® ) in a string that must be properly managed.

#### 2.2.2. Zemax® computations

In the case of thermal and gravitational performances evaluation, it is necessary an adaptation of the optical model. Coordinate Breaks (CB) are introduced before and after each Optical element paying attention to the transformation sequence. This is crucial to realize a feature that allow the introduction of local optical displacements without modifying the remaining optical layout. Matlab® extracts optical displacements from Nastran (global coordinate system), optical coordinate systems from Zemax® and applies the proper transformation matrices to obtain optical displacements in Zemax® local reference systems. In case of surface deformations, the surfaces of Zemax® file are modified from “Standard” to “Zernike Fringe Sag” in order to allow Matlab® to updates the extra data tables with the Zernike coefficients obtained from the fitting algorithm.

After the uploading of mechanical data into the optical file, Zemax® evaluate spot and p.s.f. information through its raytracing engine. If necessary Matlab® request a focusing optimization after having stored the focal plane distance to evaluate the relative focal variation. Finally Matlab® extract from Zemax Spot dimensions (Max and R.M.S. radius) and centroid displacement, eventually of multiple fields.

The results defines respectively the image quality and stability of the overall optical layout and, if necessary can be passed to an optimization algorithm that manage the mechanical properties of the system.

### 2.3. Optimization

Whereas optimization methods are nearly as old as calculus, numerical optimization reached prominence in the digital age. Its systematic application to structural design dates to its advocacy by Schmit in 1960. The success of structural optimization in the 1970s motivated the emergence of multidisciplinary design optimization (MDO) in the 1980s. Here will be presented a simplified single variable optimization approach that has been used as starting point[14].

#### 2.3.1. Problem statement

The general optimization problem (for example minimization) wants to minimize the objective function:

subjected to inequality constraints:

and equality constraints:

and side constraints (if applicable):

where vector *X* is the *n* dimension design variable vector.

In opto-mechanical variable design *X* may consists into the instrument properties (shell thickness, beam diameter,...) while *F*(*X*) is the overall instrument Mass function dependent to design variables. The inequality constraint *p*(*X*) ≤0 is the optical displacement that must be kept within certain specifications.

#### 2.3.2. Iterative procedure

The optimization algorithm requires an initial set of variables *X*_{0}. In the opto-mechanical optimization we consider as staring point the preliminary mesh defined by the user based onto its own experience. The whole integrated analysis is carried out as shown in this chapter extracting from MSC-Nastran® the overall system mass and from Zemax® the first optical displacement set. A small perturbation is applied onto the design variable (*X*_{1} = *X*_{0} + *δX*) and the procedure evaluates a second set of Mass and optical displacements. After the initialization the gradient of Mass and Optical displacement functions are evaluate respect to the design variable and the automatic procedure is started.

The optimization routine is launched:

Evaluate Mass function gradient as ∇

*M*(*X*_{i-1}) = (*M*(*X*_{i-1}) -*M*(*X*_{i-2}))/(*X*_{i-1}-*X*_{i-2});Update the design variable:

*X*_{i}=*X*_{i-1}-*g*_{M}∇*M*(*X*_{i-1}) where*g*_{M}is a gain factor properly set in order to manage iteration number;Evaluate Mass and optical displacement with new variables and update step counter;

Is optical displacement below specification? Yes: go to point 5; No: go to point 6

Is

*M*(*X*_{i}) -*M*(*X*_{i-1}) ≤*Toll*(where*Toll*is a reference value) i.e. the minimization converging? Yes: optimization ended; No: go to point 1Evaluate Displacement function gradient as ∇

*D*(*X*_{i-1}) = (*D*(*X*_{i-1}) -*D*(*X*_{i-2}))/(*X*_{i-1}-*X*_{i-2});Update the design variable:

*X*_{i}=*X*_{i-1}-*g*_{D}∇*D*(*X*_{i-1}) where*g*_{D}is a gain factor properly set in order to manage iteration and go to point 3

## 3. Modeling techniques

In the attitude of this book, following will be presented the modeling technique developed for the build up of the Finite Element Models of the Smart Structures. In particular the techniques adopted for the modeling of PiezoComposites and Shape Memory Alloy will be briefly introduced. It will not be described here the phsyicalbehaviour of the materials, detialed description of the full work and approach can be found in [11] and in [13].

### 3.1. Shape memory alloy Finite Element modeling: the Turner micro-mechanicalapproach

To perform Finite Element analysis regarding SMA is necessary to define the properconstitutive law that describe the material behavior. In this paper will be presented the FEimplementation of three different constitutive law. A further detailed description of the lawsand their application can be found in the references [7].

In physics, a constitutive equation is a relation between two physical quantities (oftendescribed by tensors) that is specific to a material or substance, and approximates the responseof that material to external forces. It is combined with other equations governing physical lawsto solve physical problems, like the flow of a fluid in a pipe, or the response of a crystal to anelectric field.

During the last ten years researchers have been developed several constitutive laws thatcan be classified considering the different approaches used in their formulation such as:micro-mechanical or macro-mechanical and phenomenological or thermodynamic.

The micro-mechanical formulation essentially takes into account the properties of singlecrystals of the material averaging their behavior over a Representative Volume Element(EVE). Micro-mechanical models have been developed using a thermodynamic approachand evaluating the energy involved during a phase transformation. These models also usehomogenization techniques to derive the overall behavior of the SMA.

The real benefit of this class of model lies in their ability to predict the real response of thematerial starting from the lattice parameters for crystalline and crystal and grain level dataderived from martensitic transformation. Nevertheless these models are very complex andrequire a large number of computational operations.

The Turner model has been successfully implemented into the commercial code ABAQUS®[10]. This model defines temperature dependent Young modulus and Thermal expansioncoefficient. Exploiting some peculiar properties of the software it is possible to define a lookup table mapping the variation of material characteristics. As obtained from the calibration ofthe model (Figures 4 and 5), it has been used the definition of Young modulus and ThermalExpansion coefficient as a function of temperature.

Different verification models were performed to select the type of the elements [10]. Thecomparison underlines how a shell model is precise enough with a high gain in terms of CPUtime. Due to this consideration, the final comparison was conducted on a shell-based modelwith composite laminate properties. The NiTiNOL actuators were modeled thickening themesh and considering the material as a “ply” of the lamination sequence. The thermoelasticmodel receives as input the thermal load on the wires and derives the temperature behaviorof all the nodes (Figure 6).

A carbon fiber-reinforced panel with six embedded NiTiNOL wires was modeled andanalyzed using the ABAQUS commercial code. The actual panel was manufactured with12 plies [90/(0)_{2}/90/ + 45/ -45]_{s}and its overall dimensions were: 30 x 170 x 1.2 mm. Theactuators chosen were OWSME wires (*ϕ* = 0.38*mm*) trained using standard heat treatments.They were embedded between the 2^{nd}and the and 3^{rd}plies with a 4% imposed strain. Themanufacturing technolgoy is reported in [3, 10]. The panel was constrained on one sideand activated via Joule effect. The numerical/experimental comparison shows that, after ashort transition, the predicted displacement matches (max. error 20 *μm*) the experimental one(Figure 7).

### 3.2. Piezoelectric numerical modeling:“Structural-scale” modeling technique forMFC

Following will be presented the numerical technique adopted to model The Macro FiberComposites (MFC) that have been developed by NASA Langley Research Center (LARC) in2000 [16]. The components of the MFC are illustrated in Figure 9. The core is made by alignedpiezoceramic fiber included in epoxy resin and joined between two groups of interdigitedelectrodes (IDE) supported by a Kapton film. The MFC have an overall thickness of 0.3*mm* and the dimensions of the region in which are placed PZT fibers called the active area, canvary from an area of 28×14*mm*^{2} to 85×28*mm*^{2}. The spacing of IDE is 0.5*mm*, while the fibershave a width of 350*μm* and a volume fraction above 85%.

The set up of numerical procedure for the performance prediction as the selection of the besttechnology to couple the structure to the actuators are fundamental to design efficient smartstructures. The numerical approach for the design of piezo based smart structures is dealt inthis section. The design of smart structure is mainly oriented to the study of authority andthen to the stress analysis. With the intent of reducing the design time, a technique able topredict the overall performances of the structure through “light-weight” numerical modelswas developed.

The overall smart structure can be conceptually divided into two sub-system: the structureitself consisting into the composite panel and the MFC actuators. The proposed techniqueis developed under the ABAQUS® commercial code [4] environment[1] -and neglect thedetailed analysis of stress state adopting essentially two type of elements: S4R four-nodeshell elements for the host material and C3D20RE twenty-node quadratic bricks (reducedintegration[1] -) for the actuator. The two subsystems are modeled as separated mesh connectedtogether through the *TIE algorithm which introduce a link between the nodes of the twodifferent surfaces evaluating the distances between the two faces and obtaining an adhesionfactor to be applied at each node (Figure 10).

A simple laminate (Figure 11) 200 × 40*mm* made by three layers, with the piezo in themiddle, has been considered to validate the proposed technique. A d.d.p. of 100*V* betweenthe electrodes has been simulated and the transversal motion of the tip has been evaluatedthrough the Classic Lamination Theory (CLT) [4]. Since the laminate is formed by three platesthe TIE algorithm is used twice. Due to the fact that Piezoelement are quadratic, while shellones are linear different mesh densities must be adopted as shown in Figure 12

It is important to pay attention to the constraint conditions, because those nodes are alsoinfluenced by the TIE algorithm which connect elements with six degrees of freedom (d.o.f.)per nodes to other with three d.o.f. per nodes. If compared with the CLT, the results comingfrom those analyses, strongly encourages the use of these techniques in fact the tip deflectionerror obtained is less then 1*e* - 3%.

The proposed technique can be also adopted for the modeling of smart structures withMFC actuators. For an overall performance evaluation is not necessary to model the wholedetailed MFC as a sequence of different layers and subcomponents. A previous comparison[4] between detailed models[1] -confirm in fact, that the displacements resulting from thelight-weighted technique are exceptionally close to the detailed ones.

The MFC have then been modeled through an homogeneous equivalent piezoelectric platesMFC_{EQ} with the same effective coefficients derived from the data-sheets. The dimensions thathave been taken into account are the ones of the active area, while the electrodes have beenmodeled as a voltage equivalent activation[1] -.

The MFC_{EQ} has been then used for the modeling of simple smart panels with bonded orembedded actuators. The simply bonding of the piezo device onto a panel is simulatedthrough the TIE algorithm and have been compared with the detailed one obtaining limitederrors (1*e* - 2%).

## 4. Applications

### 4.1. Shape memory actuated deformable mirrors

This procedure has been used to evaluate optical performances deformable mirrors[7–9] basedonto new technologies known as smart structures. Carbon fiber reinforced Mirrors actuatedby Shape Memory Alloy wires have been modeled to verify their optical capabilities. Imagequality during refocusing oriented activation has been evaluated. Several runs of this codehas been performed, varying the number/position of actuators and the structure laminationsequence in order to have the evaluation of the influence of each ingredient onto the efficiencyof the overall system. In this particular application the routine interact with ABAQUS® thatis a finite element solver more reliable with user defined Constitutive laws. The aim of theanalysis was the evaluation of the authority of the actuators into the variation of the curvatureradius of the shell keeping the image quality within acceptable limits.

In Figure 17 is shown the overall activation sequence: the first part of the process is dominatedby a contraction of the deformable mirror due to the mismatching of the CTE of NiTiNOLrespect to CFRP; when the temperature raise up to the *A*_{S} the phase transition starts and theactuators imposes the recovery strain deploying the deformable mirror. The image qualityhas been evaluated both in terms of focusing spot (Figures 19 and 21) and p.s.f. (Figures 18and 20)

Several analyses have been performed to evaluare the focusing capabilities respect to thenumber of actuators and the stiffness of the substrate (i.e. number of composite plies). Forthe detail and the results of this analyses that are not purpose of this chapter we refer to [8].As an example here we show how the actuators density modify the efficiency of the smartSMA actuated structure. Thus why thw he comparison between two different configurationsthat offer similar variations of focal positions is shown. In Figure 22 is displayed the overallfocusing variation comparing a 48 plies substrate with 14 actuators (blue) and a 36 plies with8 actuators (green). This behavior has been crosschecked with the RMS and max spot sizevariation (respectively Figures 23 and 24).

### 4.2. MFC actuated deformable mirrors

The same approach (paragraph 4.1) has been used to evaluate Carbon fiber reinforced Mirrorsactuated by Piezoelectric MFC actuators.

Analyses have been conducted based on the correlation data obtained by the validation ofsimplified modeling technique presented in Paragraph 3.2. In particular the surface qualityand the curvature radius variation have been verified as functions of the number of actuators,the different configurations and the lamination sequence.

It has been considered the smallest type of actuator even if the analysis framework set upallow the implementation of several type and dimension of them, simply due to the fact thatthey were already available in the laboratory,

Considering this class of actuators the performances are not satisfactory when the MFCare placed onto a single concentric ring. In Figures 27, 28 and 29 the results obtainedwith a population of 15 actuators evaluated as a technological limit are plotted; the radialcoordinates have been parametrically obtained searching for the best performances that havebeen obtained placing the actuators at 0.53% of the mirror radius. With this layout the spotsize goes out of boundary limit with low radius variations (0.37*mm*) while the max spot radiusis always unacceptable.

The performance of the piezo actuated smart deformable mirror are more interesting if weconsider two ring of actuators, with the same angular coordinates (Figure 25). In Figure 26is shown the contour of deformation. The results obtained comparing configurations withrespectively 8 and 10 batteries of actuators (Figures 30, 31 and 32) shows the more interestingperformances, both in terms of higher radius variation and in terms of better image qualityprocessed, with the higher number of actuator that are then limited only by technologicalaspects, mainly related to the crowding of the surface.

Also in this case have been performed analyses to evaluare the focusing capabilities respect tothe number of actuators and the stiffness of the substrate. For the detail and the results of thisanalyses that are not purpose of this chapter we refer to [8].

### 4.3. Opto-mechanical design

Here we show a simple example of the optimization procedure. Within the framework of afeasibility study for a robotic 3m class telescope, equipped with VIS and NIR instruments, ableto react to a satellite trigger in less than 50 sec (with a goal of 30 sec): CODEVISIR (ConceptualDesign for a VISible and nIR telescope), we exploited the optimization procedure to define thethickness of the main bench of the instrumental suite[15].

The instrument includes seven camera able to cover the wavelength range from the Visible(VIS, 0.4 -0.9*μm*) to the Near Infrared (NIR, 1 - 2.5*μm*) during the same exposure. Thiswill be allowed by a multichannel imaging configuration that envisages a detector foreach photometric band, delivered through a dichroic cascade along the optical path. Twoancillary instruments will complete the instrumentation suite, a visible spectrograph and aphoto-polarimeter, fed by rotating the M3 mirror.

The Optimization procedure has been oriented to weight minimizing of the overallsystem keeping the optical displacement[1] -below proper requirements. The design variableconsidered is the thickness of the bench. In Figure 35 can be observed the image displacementbehavior calculated as*μm*) and the optimization variable has been modified starting from 35*mm*. The optimizationroutine converges to a reasonable value (the thickness variation is less than a reasonable value(Δ*th*= 0.016*mm*)) within 10 steps. The final thickness is around 25*mm* and the optimizedweight of the instrument is quite less than 1.2*Ton* and the final displacement is 2.88*μm*. Thisprocedure produce an overall weight saving of 270*Kg*, starting from a very conservative value.

## 5. Conclusions

The aim of this chapter was to present the design procedure developed to the numericalcapabilities of modern softwares and hardwares. The framework is very versatile and can beused simply for performance prediction of optical system or structres and/or for optimizationstrategies. The Matlab® code works as a “server” that interact with the “client” Finite Element(ABAQUS, Nastran,...) solver managing the input file and extracting the results; the dataare modified in order to be handled by the “client” raytracing software that evaluates theoptical performances. The procedure is under development and integration in order toallow a multi-variable optimization. We are planning also to evaluates different optimizationalgorithms exploiting in particular the sensitivities analyses[5] capabilities of both FiniteElement and raytracingsoftwares.

## Notes

- And can be obviously ported to other Finite Element Codes
- the reduced integration is necessary to reduce the so called shear-locking numerical induced effect
- The whole substructure was modeled in detail with 0.2mmmesh pitch
- the electric field between two digit times the number of digit gives the overall electric field and tension.
- of one of the seven arms that is also representative of the performances of all the others