Top Layer Subframe and Node Analysis

Transcription

1 Top Layer Subframe and Node Analysis By Paul Rasmussen 2 August, 2012 Introduction The top layer of the CCAT backing structure forms a critical interface between the truss and the primary subframes. Ideally this interface should impart no displacements or forces to the subframes. This is a near impossible feat for real world structures. Gravity and thermal changes will distort the truss and transfer some of these distortions to the primary subframes. One our goals is to at least minimize the effects of dish tilting and thermal changes on the primary optical surface. On the thermal side we hope to design near zero TCE truss elements to minimize the truss distortion due to differential expansions of individual truss elements. On the structural side we can drive up the truss stiffness only at great expense. Cost constraints will limit truss structure to a design goal of 10 Hz for the fundamental resonate frequency. An active primary surface will be used to provide corrections along a normal ray centered on a subframe optical surface. Three motorized linear actuators will be used on each subframe to provide this correction. Subframe sideways motions will not be actively corrected so we need to understand static deflections of the subframes attachment points before we can design the subframe attachment interface. The limit of subframe sideways motion is limited to 100 μm for a one gravity load in any direction. A previous study analyzed a bridge structure to support the subframe actuators. This method of actuator attachment to the truss has proven to be too weak to support the subframe to the required tolerance. In current analysis we present an alternative to the bridge model. Rather than having the actuator at the same level and centered in the top layer nodes, we propose to place the actuator below and centered on the top layer node. We would then use an auxiliary shaft through the node to transfer the actuator output to the subframe interface. We feel that the advantages of this method are: A more compact node. As the size of the central node gets smaller the node behaves more like an ideal point node. A stiffer node. The central volume of the node only has to provide space for a small diameter rod and a couple of bushings. The top bushing support for the auxiliary rod can be made of Aluminum. There only needs to be invar for the junction of the truss elements. This will reduce the weight of a node. Easy access to the actuator. The actuator mounting bolts will be easier to access. Also, the subframe can be locked into place while the actuator is replaced. This design reduces the actuator shaft moment stiffness requirement. The subframe moment loads will be taken by the node and the actuator will only require high axial stiffness. 1

2 Figure 1 Actuator below the node, bottom view 2

3 Figure 2 Actuator below the node, top view 3

4 Figure 3 Cross section A Analysis Goals For this study we wish investigate the following items: We wish to understand the displacements for the tip of the actuator with respect to the node center when the node is analyzed in the full truss. Tilting of the auxiliary shaft will define how deep into the subframe the interface can extend before we exceed the sideways tolerance. We also wish to analyze this node in a standalone configuration without the full truss. This means that the full truss is removed and the ends of the tubing are fixed. This will allow us to compare the simpler standalone model to the full truss model. The full truss model requires a long time to run and it is easy to break. We wish to show that this concept can be used for the top layer of the truss. We wish to check stresses and distortions in the node to optimize the design of the node truss rod ends for strength to weight of the truss structure. We wish to model a simple subframe with the standalone node to gain an understanding of the subframe lateral displacements as a function of actuator interface height within the subframe. 4

5 Model Construction The truss model is based on a modified version 13c of the evolving truss. This modification has changed the top layer, layer 1, and the intermediate layer 1 to 2.This modification was made because layer 1 of the version 13c was laid out to accommodate the bridges from the previous study. In the version 13c model the layer 1 nodes were not coincident with the subframe actuator locations. For this study the layer 1 was reconstructed to have the nodes coincident with the actuator location. This change also required the rebuilding of the intermediate layer 1 to 2. All other node positions were left unchanged. The same model is used for both the embedded node and the standalone versions of this study. This is largely accomplished by using the simplified representation function within ProEngineer. This functionality allows one to create various configurations of a master model. This functionality was originally intended to facilitate working with large models, but its functionally has expanded to include simulation configuration management. One can turn off components (parts) and various features of parts. The components are no longer displayed or editable, but they still exist in the model. This is different from hiding a part or feature. When one hides a part it is only invisible, it can still be edited. As a consequence of this if a feature in a part is turned off in a simplified representation then the FEA mesher will not mesh that feature. But, if there are simulation entities, such as beams or idealized masses in the feature then these entities will be incorporated into the simulation model. This how one gets a beam simulation model from a solid tubing model. One embeds a beam in the tubing part and then creates a simplified representation that removes the solid tube and leaves the idealized beam between the node points. If one did not remove the solid tube then the mesher would mesh the tube and also include the beam in the simulation. If one constructs these tubes to represent the entire truss then one can setup a simplified representation that strips all the solid tubing and leaves only beams for the simulation model. Embedded Single Node Assembly For both the embedded and standalone simulation models a simplified node was constructed at the inner subframe actuator position for a second ring subframe. The chosen node is in line with the EL axis. Again see figures 1, 2, and 3. See figure 4 to see the node embedded into the full truss. 5

6 Figure 4 Node embedded into full Truss A simplified representation was configured with the following characteristics: The version 13c tubing parts that overlapped the constructed node assembly were excluded. Excluding a part will remove all but references to the part. This has the effect of removing the solids as well as the embedded beams. The actuator was replaced with an idealized mass at the center of gravity of the actuator. This mass is attached to the bottom node flange with a weighted link. The ends of node tubes attach to the truss with weighted links. The solids of the node assembly are left intact for meshing. The solid tubing for the rest of the truss, not the tubing parts, are excluded to leave only beams in their place. After this simplified representation is activated, constraints are placed, loads are configured, and the model is meshed the model is ready for analysis. Standalone Node Assembly As before a simplified representation is configured, but with the following characteristics: 6

7 The version 13c tubing parts that overlapped the constructed node assembly were excluded. Excluding a part will remove all but references to the part. This has the effect of removing the solids as well as the embedded beams. All version 13c tubing parts are excluded from the model. This will leave only the node assembly. The actuator was replaced with an idealized mass at the center of gravity of the actuator. This mass is attached to the bottom node flange with a weighted link. The solids of the node assembly are left intact for meshing. The ends of the node assembly tubes are fully constrained. After this simplified representation is activated, loads are configured, and the model is meshed the model is ready for analysis. The ADS Actuator is used as an Example The ADS actuator is used in the model because ADS has provided an assembly drawing that provides enough detail to construct a reasonably accurate shell with a few internal details. Use in this model does not constitute an endorsement of the ADS design. Analysis Environment This model was constructed and analyzed using PTC s Creo 2.0 date code M10. Materials Refer to figure 5 and table 1 for materials and material properties used in the analysis. The material CFRP_TRANS_1 is a transversely isotropic carbon fiber composite based on a Hexcel IM7 fiber and a TenCate RS-50 matrix. A micromechanical model was used to calculate the bulk properties of a 0 unidirectional CFRP laminate. The volume fraction was adjusted to provide a longitudinal modulus near the value that vendors have cited for low CTE tubing. From these calculations the transverse modulus, shear modulus, and the Poisson s ratios were calculated. The IM7 and RS-50 materials were chosen because they had tensile properties similar materials that RockWest has proposed for the tubing and they had published material properties that allowed the calculations to made. Table 1 Material Density (gm/cm 2 ) Longitudinal Modulus (GPa) Transverse Modulus (GPa) Shear Modulus (Gpa) μ 21 =μ 31 μ 32 CFRP_TRANS_ INVAR n/a n/a STEEL n/a n/a AL n/a n/a 7

8 Figure 5 Material that are used in the analysis Analysis Results See table 2 for the summary comparison of the auxiliary shaft tip local displacements. Local means that the displacement is with respect to a coordinate system at the center of node. In table 2 W/O Truss represents the standalone node model analysis case. And With Truss represents the embedded node analysis case. The reference coordinate system for both the application of gravity and measurement of local displacement that is used has the z direction parallel with the optical axis and the x direction is parallel with the EL axis. One of the conclusions that can be pulled from table 2 is that for the standalone and embedded Y gravity case there is a near factor of two for the displacement magnitude. This can be understood by assuming that the full truss is pushing and pulling the node assembly tubes in a complex pattern. But, the displacement numbers are close enough that the moment stiffness of the nodes will be similar for both the embedded and standalone cases. This allows us the make the important assumption that the standalone analysis case can be used for designing the nodes. The embedded analysis can require 2 hours to run, versus ten minutes to run for the standalone case. 8

9 Measure W/O Truss Y Gravity (mm) With Truss Y Gravity (mm) W/O Truss Z Gravity (mm) W/O Truss X Gravity (mm) Actuator Tip X Disp Actuator Tip Y Disp Actuator Tip Z Disp Displacement Mag Actuator CG X Disp n/a Actuator CG Y Disp n/a Actuator CG Z Disp n/a Notes: 1. All measurements are with respect to the node center. 2. Y gravity simulates the dish pointed to the Horizon. 3. X gravity simulates the dish pointed to the Horizon and a subframe aligned perpendicular to the EL axis. 4. Z gravity simulates the dish pointed to the Zenith. 5. The 'Actuator CG' is a point at the estimated center of gravity of the actuator. Table 2 Node Moment Stiffness The node moment stiffness is essentially the torsional spring constant of the node about the center of the node. This property only has practical value for sideways motions of the subframes. These motions correspond to rotations about the local x or y axis. Subframe Mass Node Actuator CG 40 Kg 7 Kg.15 Meters.24 Meters 68.6 N 392 N Figure 11 The standalone node will be used for the calculation. Also, since the Y gravity case is similar to the X gravity case, but the stiffness is slightly lower, the Y gravity case should be used for general calculations. Figure 11 is a schematic of the weight distribution about the standalone node. The net force about the node is: The moment about the node center is: Net Force = 392 N 68.4 N Net Force = N 9

10 Moment = N.15 M = NM From table 2 the magnitude of the actuator CG displacement for the Y gravity case =.0687mm. This creates an angular displacement of: = tan = R 240 The displacement of the actuator CG is used because it is connected to the node via a weighted link. The weighted link does not bend; it only follows the motion of node attachment point. This motion will produce a moment stiffness of: This is for the Y gravity case. Moment Stiffness = NM R = NM R Embedded Single Node Results See figures 6 and 7 for embedded analysis results. In figure 6 the thin lines surrounding the node assembly are version 13c beams. In figure 7 the surrounding truss has been removed to show displacement results local to the node assembly. In figure 7 the thin blue lines are the truss before deformation. In figures 6 and 7 it can be seen that most of the displacement is from the sagging of the full truss and details of the node tilting are hidden. Other tools are required to pull the local node displacements from the analysis. To get the local displacements simulations measures are placed at the tip of the auxiliary shaft s tip. These measures display the displacement of the tip with respect to the center of the node. These measures were used to obtain the values in table 2. An important result that can be pulled from figure 6 is that the embedded node assembly is not putting any discernible asymmetry into the distortion of the full truss. This can mean one of two things: Removing a single node at the top layer does not change the analysis much. Or, the characteristics of the embedded node assembly are significantly similar to an ideal node that the analysis solution is nearly the same. A stress plot of the truss, (not shown in this report), shows that the version 13c beams that support the embedded node assembly are under similar stresses to the beams in similar positions on the other side of the optical axis. This would tend to support the second conclusion. 10

11 Figure 6 11

12 Figure 7 12

13 Standalone Node Results Figure 8 X gravity standalone 13

14 Figure 9 Y gravity - standalone 14

15 Figure 10 Z gravity - standalone Figures 8, 9, and 10 display the results summarized in table 2. For the z gravity case, at zenith, the actuator tip displacement would probably be less if there were two symmetrically placed layer 1 to 2 truss struts to support the node. For the version 13c truss this would have required changing the layer 2 node placements. 15

16 Subframe Lateral Displacement Simulation The standalone model can be simply extended to a first order standalone subframe displacement model. Using additional beams, masses, springs an idealized subframe can be constructed. Figure 11 shows additional added idealized elements that are used to provide a first order simulation of a subframe. Figure 11 Idealized Subframe Construction A total of 14 beams, 3 masses, and 2 springs were added to create the subframe and two nodes. The wedge shaped beam structure in figure 11 is the idealized subframe. The subframe was constructed from 12 beams and three masses. The beams used in the wedge use the material unobtiaium ; it is ten times stiffer than steel and one tenth the density of Aluminum. Constructing the wedge with these materials makes the wedge extremely stiff and near massless. Because of this only node stiffness will contribute to subframe displacements. The bottom plane of the wedge is at the actuator tip attachment height. The top plane of the wedge is through the estimated center of gravity (CG) of the subframe. Three point masses are used to simulate the mass of the subframe. The masses are shown as dark blue spheres on the top plane of the wedge. The masses are 40 Kg each. The combined mass of 120 kg is 20% more than the ideal mass of a ring 6 subframe. This is the same mass used for the single node analysis presented in the previous sections. 16

17 Two beams and two springs are used to simulate the two nodes that mimic the remaining actuator nodes used to support a subframe. The two beams simulate the actuator shaft used in the preceding single analysis. These beams have a solid 30 mm diameter circular section and steel is used as the material. The two springs are 3 dimension torsion ground springs that have a spring constant equal to the node moment stiffness calculated in the preceding standalone analysis. This analysis was structured as a design study, the subframe CG height was fixed at 300 mm above the node centers and the actuator attachment height was varied from 100 mm to 250 mm above the node centers. The subframe CG height can be varied based on better estimates of the CG, but for this analysis it will be fixed at 300 mm. Results Figure 12 presents the results of this design study. The vertical axis is the lateral displacement of the three actuator tips. Here lateral means the magnitude of the x and y displacement at each actuator tip. The x and y directions are perpendicular to the plane defined by the three node centers. The z direction is parallel to the actuator shafts and would thus be nulled out during normal operations so it is not included. In figure 12 Tip A corresponds to the node from the previous analysis Actuator Tip Displacment vs. Tip Height Lateral Tip Displacement (microns) Actuator Tip Height (mm) Tip A Tip B Tip C Poly. (Tip A) Figure 12 The results for shown in figure 12 are for the Y gravity case. The results from the previous analysis would indicate that similar but more modest displacements would be present for the X gravity case. 17

18 The Y gravity case is equivalent to a subframe radially aligned with the EL axis and the dish pointed to the horizon. The X gravity case is equivalent to a subframe radially aligned perpendicular to the EL axis and the dish pointed to the horizon. The images in figures 13 through 16 present results for actuator tip heights at 100 mm, 150 mm, 200 mm, and 250mm. Figure 13 Tip Height = 100 mm 18

19 Figure 14 Tip Height = 150 mm 19

20 Figure 15 Tip Height = 200 mm 20

21 Figure 16 Tip Height = 250mm Conclusion The distortion scale factor for the previous four figures is fixed at 2000, so the element displacements are multiplied by 2000 before being plotted. From this series it may be apparent that the results presented in figure 12 are a result of the node twisting and the shaft bending. Presumably, the total displacement is a simple addition of node twisting and shaft bending. Without further study it is not clear if the node twisting is linear with applied moment, but for the moment we will assume that it is linear. From analytical beam calculations end displacements of a beam vary as the square of the beam length. The poly (Tip A) curve in figure 12 is a parabolic fit of the Tip A results. The shape of the Tip A curve is very close to parabolic. If the node twisting is near linear with applied moment the parabolic shape of Tip A curve would be due the bending of the actuator shaft. This is important, the subframe lateral displacements roughly scale as the square of the actuator tip heights as simple beam calculations would also indicate. 21