1. Introduction
2. The Experiment

Pre-Processing Stage

Solution Stage

Post-Processing Stage

3. Discussion

Study of Axial Forces

Study of Lateral Forces

Study of Lateral Attachments

Possible Sources of Error

4. Conclusion
5. Acknowledgments
6. References

The Center of Excellence in Information Systems at Tennessee State University (TSU) is building a 2-meter (81-inch) completely automatic telescope for high-dispersion spectroscopy of stars. This instrument will be the largest automatic telescope in existence and the largest telescope wholly owned by any institution in the South (aside from the University of Texas). This telescope is designed around a surplus 81-inch f/1.5 parabolic primary mirror that came with an existing mirror cell having support points already provided. Unfortunately, the hardware to support the mirror at those positions has disappeared over the years, so TSU has been forced to design replacements for it.

The support of the 81-inch primary mirror is crucial in the overall effectiveness of the 2-meter telescope. Proper support would result in a relatively flat optical surface of the mirror (ie., preserving the mirror’s parabolic shape) and thus lead to good reception of the studied stars. The support of the primary mirror may be broken down into two main problematic cases: 1) when the mirror is flat (zenith distance=0^o), the gravitational force pulls in the axial direction; 2) when the mirror is upright (zenith distance=90^o), the gravitational force pulls in the lateral direction. In either of these orthogonal situations, as well as in combinations in between the extremes, the mirror is subject to intolerable variation in deflections without the aid of proper supports applying the right forces. Strategically placed forces will counter the gravitational forces evenly and significantly lower the net displacement. This study of the primary mirror's deflections was prompted by the need to identify the proper method for supporting the telescope mirror with attached weights (invar pucks) by using forces applied by a system of counterweighted levers.

Engineering Goal: To model a proper support design for an 81-inch astronomical telescopic mirror in order to prevent intolerable gravitational deflections of the mirror surface.

The support design for the mirror will be derived from the results of the following first two specific aims of this research:

Specific Aim #1: To determine which forces must be applied to the mirror axially to properly support it at a zenith distance of 0^o (flat position) without a wide-ranging amount of deflections, and to find the tolerance level of the variation of the forces from their optimal values.

Specific Aim #2: To determine which forces must be applied to the mirror laterally to properly support it at a zenith distance of 90^o (upright position) without a wide-ranging amount of deflections, and to find the tolerance level of the variation of the forces from their optimal values.

Specific Aim #3: To determine the difference between the deflections produced by realistic supporting plates and the deflections resulting from the nodal point supports on the mirror model.

An engineering method called finite-element analysis (FEA) was used to conduct this study. FEA uses a complex system of points called nodes, which make a grid called a mesh. This mesh is programmed to contain the material and structural properties that define how the structure will react to certain loading conditions. Static linear FEA and modeling of the 81-inch primary mirror were performed using ANSYS, a software package used for hypothetical engineering simulations. ANSYS was used for several reasons, for example: 1) real testing of the forces cannot be performed on the actual telescope, 2) ANSYS allows users to create, modify, and test new models repeatedly through simulation, and 3) ANSYS has been proven to be a highly accurate engineering tool.

The FEA session consists of three main stages, namely the pre-processing stage, the solution stage, and the post-process stage.

The first step in the pre-processing design of the model was to create the overall geometric shape of the 3-D model. The mirror is basically a thin glass cylindrical disc with a flat bottom and a top surface that has a certain curvature. At f/1.5, the center is roughly 3.4 inches deeper than the rim. The diameter of the mirror is 81 inches, with a 20-inch hole in the center, and it is roughly 9 inches thick at the edge. Using the pre-determined information from the existing mirror (presently located at Washington Camp in Arizona), an ANSYS program was written to generate a realistic gravitational model of the mirror and mesh it into elements. When generating the finite-element model, the program considered various material properties such as Young's modulus (or modulus of elasticity), Poisson's ratio, and density. The geometry of the model included various factors, namely concavity, radii lengths, and size dimensions. The mirror is made of Cervit, a ceramic glass having roughly the same physical properties (Young’s modulus and density) as aluminum, but with a very low coefficient of thermal expansion at normal temperatures. The locations of support points and hard points (constraints) were given from the existing mirror, and their locations were measured to better than 0.1 inch. Another task is to select the most accurate element, which is the basic building unit with a pre-determined number of degrees of freedom (DOF) and material properties. Defining the element type is one of the most crucial parts of the analysis because the accuracy of the results depends heavily on this decision. A brick (hexahedron)-shaped element with 8 nodes was decided for usage, and calculations were first done using half the normal grid size to assess the effect of mesh size on the deflection calculations.

A set of prescribed displacements, where the value of displacement of a nodal freedom is specified as part of the input data, is a convenient boundary condition for this sort of problem. Such prescribed displacements are also referred to as constraints. The most obvious use of a prescribed displacement is to model a "true support," where a structure is fixed to a relatively rigid foundation or adjoining structure. It is necessary in static stress analyses to provide sufficient supports to prevent rigid body motion. When applying the supports, it will be checked that each possible rigid body motion is prevented. According to St. Venant’s principle that providing the reactions at the support are statically equivalent to the real reactions, the stresses away from the supports will be satisfactory.

Constraint equations (also known as multi-point constraints) relate the displacement of a freedom to one or more other freedoms. A typical form is:

where m_n, v_n, and w_n are displacements of node n in the x, y, and z directions, and C_i is a constant or coefficient. The freedom on the left-hand side may be referred to as the "slave" or "dependent" freedom. Since the displacement of this freedom is completely defined by the displacements of the other freedoms in the equation, irrespective of the stiffness of the elements, it can be eliminated from the stiffness matrix. It is important in this finite element analysis to keep in mind that the application of too many constraints is usually unconservative for mechanical loads.

The solution stage of the FEA process is the portion of the research that is wholly computed by the ANSYS software package. It is essentially the calculation of the displacements. If the displacements are prescribed, an assumed solution for those freedoms is being effectively forced. The mirror-modeling program that was inputted into the pre-processor will be used by ANSYS to calculate myriad possible solutions and calculation under various degrees of freedom (DOF). These diverse calculations become options for the user to view numerically or graphically in the post-processing stage. The solution basically completes the task of the gravitational simulation and calculates the resultant force vectors. Although the solution is calculated by the ANSYS software, the theory behind the complex calculations will be discussed.

The following figure is a representation of a typical 8-node brick element, which fits the description of the specific SOLID 45 element used in this research.

Where K_e represents the element (SOLID 45) stiffness matrix, u = translation in a given direction, and the coordinate system above is used,

|K_e| = 1/8 (u_I(1 – s)(1 – t)(1 – r) + u_J(1 + s)(1 – t)(1 – r) + u_K(1 + s)(1 + t)(1 – r)

+ u_L(1 – s)(1 + t)(1 – r) + u_M(1 – s)(1 – t)(1 + r) + u_N(1 + s)(1 – t)(1 + r)

+ u_O(1 + s)(1 + t)(1 + r) + u_P(1 – s)(1 + t)(1 + r)

In general, the equation that is solved for static linear analyses is:

[K]{u} = {F^a} + {F^r}

where: [K] = total stiffness matrix, {u} = nodal degree of freedom (DOF) vector, N = number of elements, [K_e] = element stiffness matrix, and {F^r} = nodal reaction load vector,

{F^a}, the total applied load vector, is defined by:

{F^a} = {F^nd} + {F^e},

where {F^nd} = applied nodal load vector and {F^e} = total of all element load vector effects (pressure, acceleration, thermal, gravity)

The figure below gives a visual representation of applied and reaction load vectors:

The post-processing stage includes all of the analysis of the results produced from the solution. The resulting stress and displacement distributions derived from the computed solution will be analyzed. Stress linearization in the post-process allows a separation through a section into constant (membrane) and linear (bending) stresses.

The "bending" values of the stress components at a specific node N₁ are computed from:

where: t = thickness of section, s_i = stress component I along path from results file (‘total’ stress), and x_s = coordinate along path r.

The resulting equivalent linear stress can then be equated to a value of elastic strain by using the following equation:

where: s_eq = equivalent stress, G = shear modulus, e_eq = equivalent elastic strain, E = Young's modulus, and v = Poisson's ratio.

Finally, the elastic strain can be related to the resulting deformation (deflection) through the following equation:

where: e = elastic strain, d = deformation, and L = unit length.

Degree-of-freedom reaction solutions along the Y- and Z- axis translations will be calculated at the designated nodes and keypoints of the model. The reaction solution reveals the Newtonian action-reaction forces at all selected nodes and is critical in decisions to redesign the model by adding or removing constraints (hard points) and applied forces. The proper application of translational constraints prevents rigid body motion, especially rotation. The rule of thumb for judging whether or not the calculated variation of deflection is acceptable is a quarter of a wavelength of light (l = 0.5 micron, or 2 x 10^-5 inches). If the total range of deflections is approximately less than 5 x 10^-6 inches, the support design assumed in the model will be considered adequate.

The most accurate and realistic element type for the mirror was chosen to be "SOLID 45" (brick-shaped element, 8 nodes, 3 degrees of freedom (DOF), with orthotropic properties). "MASS 21" (point element, 1 node, 6 DOF, no material properties) was selected to represent the attached weights, which were necessary for simulating the invar pucks glued to the side and back of the mirror for attaching the support hardware.

The keypoints defining the supports on the back of the mirror were spread evenly and concentrically and designated in one of three "rings" or "zones" on the model: the outer ring, the middle ring, and the inner ring.

As seen in the figure above (used solely to reveal keypoint locations), the ring patterns of the keypoints (red dots) can be seen clearly.

Initially, uniform axial forces were applied to the back of the mirror at the 36 support keypoints. The positions of these keypoints were determined by measuring the positions in the actual mirror cell, accurate to within 1/8 of an inch. The applied force at each keypoint was determined by dividing the weight of the mirror (3429 lbs.) by the number of concentric keypoints (36), which resulted in 95.25-lb axial forces. Gravitational loading at zd=0^o along the Z-axis translation produced the following nodal displacements:

The range in deflection was 3.02 x 10^-5 inches, which is an unsatisfactory level. The mirror is being warped by the pucks hanging preferentially on its upper and lower edges. The triangular appearance of this figure reflects the three axial hard points.

A lateral, or side view if the identical scenario is shown below, with the force vectors at the 36 keypoints marked on the image:

Next, in order to produce a more realistic and varied applied force on the mirror, a multiplicative factor for each ring was determined by using the reaction solution from the previous case. The average reaction force for any particular ring was divided by the number of keypoints in that ring in order to obtain the multiplicative factor. Due to the difference in nodal displacements, the outer ring was eventually subdivided into the upper outer ring and the lower outer ring.

The average axial forces varied among the three rings, per the following multiplicative factors: inner ring (x 0.919), middle ring (x 1.016), upper outer ring (x 1.060), and lower outer ring (x 0.90). After accounting for the multiplicative factors, the axial forces for the keypoints on the back of the mirror were as follows: 87.5 lbs on inner ring keypoints, 96.8 lbs on the middle ring, 101 lbs on the upper outer ring, and 88 lbs on the lower outer ring. The post-process results at zd=0^o along the Z-axis for this distribution of supporting forces is shown in the figure below:

The deflection variation of the mirror when the axial forces were concentrically varied was 2.2 x 10^-5 inches. There was an improvement compared to the uniform axial forces, but the resulting deformations were still too divergent.

The final and most extreme case of force variance involved determining individual applied forces at each separate support point on the back of the mirror to the nearest pound. To do this, the keypoints corresponding to the 36 support points were constrained in the Z-axis direction (along gravity) to give a smooth front surface to the mirror. Resulting forces ranged from 87 lbs to 108 lbs, with most of the variation coming from the weight of the invar pucks glued to the bottom and side of the mirror to attach the support levers. The nodal solution is revealed in the figure on the next page:

The range in deflections is 2.127 x 10^-6 inches. This favorable result confirms the trend of getting less deflection variation as the force becomes more varied and specific.

Next, random errors in applied axial forces were prescribed in order to test the mirror model under realistic error conditions. The precision tolerance of the lever systems that will be used to deliver the counter-gravitational masses is correct to better than ± 2 lbs. Using a random digit generator, random integer values ranging from –2 to +2 were assigned as applied errors (in lbs) to the existing forces that were determined to flatten the front surface of the mirror. For example, a random error of –2 lbs was assigned to a 90-lb force at keypoint #65. The new force at keypoint #65 is now 88 lbs. The post-process results for one such error-tested model is shown in the figure below (on the next page):

The deflection range for this simulation was 4.16 x 10^-6 inches, a surprisingly favorable result, considering the inclusion of random errors into the formula. Several different cases of 2-pound random errors were run, and all gave similarly acceptable results.

In the study of the lateral support design, the distribution of lateral forces was changed several times to try to reduce the bending of the mirror. The lateral supports at six different nodes were studied: three on the top side ( #541, #941, #1341) and three on the bottom side (#2341, #2741, #3141). The lateral supports were varied by a magnitude of 30 lbs. The variation that produced the optimal results was subtracting the force at the top node (#941) by 30 and adding 30 more lbs to the bottom left node and the bottom right node (#2341, #3141). The nodal solution of the mirror model in the upright position is displayed below:

It can be seen from the figure above that since gravity is pulling downward on the mirror, the bottom supports push upward with a reaction force and cause gaps or displacements at the bottom support nodes. As a direct effect, the areas surrounding the top nodes are deformed upward. The deflection produced by the gravitational simulation at zd=90^o varied with a magnitude of a moderate 5.71 x 10^-6 inches. Also, an extended effort to make the model as realistic as possible is evidenced by the steel rod-shaped "links" to lateral support points on the side of the mirror.

This part of the calculation showed that the errors in setting up the lateral-support levers are not very important. The positions of those lateral support points may be more significant, as experiments done is varying the amount of force applied to nodes at the top and bottom edges of the mirror showed.

Due to the restrictions of element quantity on the University Version of ANSYS, realistic lateral support pucks could not be included with the mirror model. Therefore, a brief exclusive study of lateral attachments was conducted to determine the difference between the stresses produced by the actual supporting plates and the stresses resulting from the nodal point supports on the current mirror model. Using ANSYS, a realistic lateral support puck was modeled, meshed, and attached to a single element from the original mirror model. The result of the a 12 psi (pounds per square inch) gravitational loading on the top of a 6 x 8 x 2 steel puck is shown on the next page:

The back of the 20 x 12 x 9 glass (Cervit) block is tied fixed. Deflections in the area encompassed by the "puck-mirror complex" had a maximum absolute value of about 6.65 x 10^-6 inches.

As a measure of comparison, a more detailed and in-depth view of the nodal solution graphic for the lateral gravitational simulation of the entire mirror model is shown below:

The zoomed-in image of nodal lateral support clearly show the sharp upward displacement mentioned earlier. The maximum deflection, at the apex of the nodal displacement, is 3.59 x 10^-5 inches. This calculation with point supports gives a deflection that is approximately 5 times as large in magnitude as a more realistic calculation gives. This observation will be considered when determining the lateral support design for the mirror.

In the midst of all of the FEA calculations, one possible source of error is the fact that ANSYS is merely a simulation. Although the finite-element method is usually an accurate predictor for structural engineering situations, there may be some discrepancies between the simulation and the actual performance of the telescope prototype. The modestly inaccurate representation of the lateral supports may be another possible source of error in the study of lateral forces. In the FEA calculations, the lateral supports were represented at single nodes (due to the MASS 21 properties). Thus, the exaggeratedly sharp upward displacement can be noticed around the lateral supports on the top side. The actual mechanism for the lateral supports involves the application of a counter-weight to a rectangular metal plate that is attached to the side of the mirror.

The extensive series of similar and diverse finite element analyses (FEA) of the 81-inch telescopic mirror yielded desired results that were conducive to the modeling of a sufficient mirror support design.

Specific Aim #1 was met through several FEA calculations that were made for different scenarios for the axial forces. A noticeable trend is that as the axial forces became more and more varied, the deflection variation became more reduced. Therefore, the optimal results were produced from the axial support design that included individually calculated forces for each separate keypoint on the back of the mirror. With the account of random errors within the precision tolerance of the weight systems, the final axial support design for the mirror included at zd=0^o: (a rough estimate) 87.5 lbs applied to the inner ring of keypoints on the back of the mirror, 96.8 lbs applied to the middle ring, 101 lbs on the upper outer ring, and 88 lbs on the lower outer ring. The individual forces ranged from 87 lbs to 108 lbs. The total range of deflections was 4.16 x 10^-6 inches, approximately less than a quarter of a wavelength of light. For precise force values on each axial keypoint, please consult the "primir7a.in" ANSYS pre-process source code.

Specific Aim #2 was also met successfully through the finite element method. The bulk of the investigation and FEA calculations were performed on the three lateral supports on the top side of the mirror and the three on the bottom side. The forces at the six lateral supports were varied by ± 30 lbs. A comparison of several FEA calculations of varied lateral forces led to the finalization of the lateral support design, which includes: (at zd=90^o) 665 lbs applied on the upper left support, 530 lbs on the upper middle support, 665 lbs on the upper right support, 566 lbs on the bottom left support, 520 lbs on the bottom middle support, and 566 lbs on the bottom right support. Overall, the lateral forces ranged from 520 lbs to 665 lbs. This design produced a moderate net displacement of 5.71 x 10^-6 inches.

The combination of meeting both specific research aims fulfills the overall engineering goal of supporting the astronomical mirror. The prescribed random errors did not have a significant impact on the outcome of the deflections, and therefore the precision tolerance level ( ± 2 lbs) of the lever weight systems will suffice and not produce unwanted stresses.

The investigation of Specific Aim #3 proved that the actual lateral support plates on the mirror edges would produce deflections approximately five times less than the deflections calculated by the mirror model with the unrealistic nodal point supports.

The results of this engineering research have very significant and practical implementations. The desire to know our surrounding celestial bodies is stronger than ever before in our society, partly due to possible future inhabitance in space and mainly due to natural human curiosity. The proper support of the astronomical telescope will find its "real-world" application when the quality of the spectroscopic receptions of the stars becomes a vital part of the telescope user’s space exploration, as well as our own.

Special thanks to Dr. Joel Eaton, for giving me this incredible research opportunity and for his mentoring; and thanks to the Center for Automated Space Science at Tennessee State University, for providing the facility to conduct my research and for providing the necessary ANSYS software.

Beer, Ferdinand P. and Johnston, E. Russell. Mechanics of Materials: Second Edition. NewYork: McGraw-Hill, Inc. (1992).

Monaghan, Dermot. "Notes Giving an Introduction to the Finite Element Method in Engineering Analysis." National Agency for Finite Element Methods and Standards. 1 June 1999 <http://sog1.me.qub.ac.uk/dermot/fam-abaq.html>

Eaton, Joel A. Structural Analysis of the Telescope Mount. < http://coe.tsuniv.edu/eaton/eng_t13_fea.html>

Bathe, K. J., Finite Element Procedures in Engineering Analysis, Prentice-Hall, Englewood Cliffs (1982).

Cook, R. D., Concepts and Applications of Finite Element Analysis, Second Edition, New York: John Wiley and Sons (1981).

Galambos, T. V., Structural Members and Frames, Prentice-Hall, Englewood Cliffs (1968).

Diekmann, Ralf. "Mesh Generation." AG-Monien. http://www.unipaderborn.de/fachbereich/AG/monien/RESEARCH/FEM/netgen.html

ANSYS: Modeling and Meshing Guide (Release 5.3). Houston: ANSYS, Inc. (1996).

ANSYS: Structural Analysis Guide (Release 5.3). Houston: ANSYS, Inc. (1996).

ANSYS: Basic Analysis Procedures Guide (Release 5.3). Houston: ANSYS, Inc. (1996).

ANSYS: Elements Reference (Release 5.3). Houston: ANSYS, Inc. (1996).

ANSYS: Command Reference (Release 5.3). Houston: ANSYS, Inc. (1996).

Kohnke, Peter. ANSYS: Theory Reference (Release 5.3). Houston: ANSYS, Inc. (1996).

Oden, J. T., Mechanics of Elastic Structures. New York: McGraw-Hill (1968).

Przemieniecki, J. S. Theory of Matrix Structural Analysis. New York: McGraw-Hill (1968).