A SPACE APPLICATION OF A DATA RECOVERY PROCEDURE BASED ON DIRECT ENFORCED MOTION USING A MULTI-BODY DYNAMICS SOFTWARE (DCAP)

Transcription

1 A SPACE APPLICATION OF A DATA RECOVERY PROCEDURE BASED ON DIRECT ENFORCED MOTION USING A MULTI-BODY DYNAMICS SOFTWARE (DCAP) André Oliveira (1), Gianluigi Baldesi (2), Donato Sciacovelli (3) (1) ESA / ESTEC, Keplerlaan 1, postbus 299, 2200 AG Noordwijk, The Netherlands, Andre.Oliveira@esa.int (2) AOES, Keplerlaan 1, postbus 299, 2200 AG Noordwijk, The Netherlands, Gianluigi.Baldesi@aoes.nl (2) ESA / ESTEC, Keplerlaan 1, postbus 299, 2200 AG Noordwijk, The Netherlands, Donato.Sciacovelli@esa.int ABSTRACT Future space structures with complex dynamics demand a high degree of versatility from multi-body dynamics simulation tools. Based on its order-n dynamic formulation for both rigid and flexible bodies with the possibility of time varying mass characteristics and its symbolic pre-processor, DCAP is a software tool that can meet the requirements of new projects in terms of computational efficiency. In order to complete the dynamic analysis for flexible elements, the capability to determine the internal loads should be pursued. The idea is to use, as an input, the results from the multi-body dynamics software and direct enforced motion in a Finite Element (FE) program to study the internal loads. Consequently, a data recovery procedure, which postprocesses DCAP results in MSC.Nastran, has been developed, tested and validated. Depending on the particular application, the internal loads analysis can be carried out statically or dynamically. A real life space application of this technique, such as a docking case scenario of the Automated Transfer Vehicle (ATV) with flexible Solar Arrays (SA) to the International Space Station (ISS) is presented. 1. INTRODUCTION When working with multi-body dynamic systems, the first goal is to accurately represent their cinematic and dynamic behaviour. Future space applications have been evolving towards ever more challenging systems involving considerable economic budgets. In order to model and analyse their performances, the simultaneous solution of hundreds or thousands of first-order differential equations is required. This could not have been accomplished a few decades ago, before the development of electronic computers. Recently, greater emphasis has been placed on developing time and computer efficient state-of-art multi-body system codes which are able to describe complex systems in detail. The Dynamic and Control Analysis Package (DCAP), which is currently used at ESTEC s Structures Section is one such code. DCAP is a collection of programs capable of performing the analysis of complex, multi-body, flexible structures and their associated control systems. A DCAP model is usually composed of four parts: structural dynamics, control systems, orbital environment and graphical or physical model. To assemble the model the user must first decompose the spacecraft structure into an assembly of bodies, rigid or flexible, and hinges [2][3]. Many additional components are also available such as devices to constrain cinematic motion, contact dynamics models, manipulators and non-linear springs and dampers. The most common way of modelling flexible structures in DCAP is to import a modal base of the structure from Nastran and represent its degrees of freedom (DOF) through modal coordinates [5]. DCAP assembles the mass matrices taking into account the rigid and flexible contributions from the bodies in the system, the boundary conditions of the flexible bodies and the coupling terms between rigid and flexible DOF. DCAP uses Kane s method and exploits a dedicated symbolic manipulation pre-processor to assemble an Order(n) dynamic model for flexible multibody systems containing tree topologies. The method essentially consists of two parts: a frontal part, in which the inertia and active forces associated with each body are shifted to its inboard body and this process repeated until the core body is reached, and a back substitution part in which all the accelerations are obtained in terms of the core body accelerations and all the external forces acting on the system. A fourth order Runge-Kutta integration scheme is then used to determine the remaining unknowns [4]. Despite its great potential, the fact that DCAP is not a Finite Element (FE) software hinders its capabilities to determine the internal forces, moments and stresses in modelled flexible structures. Since DCAP can include sensors, actuators and control systems, it would be extremely interesting to be able to determine the internal forces present in a structure while in near operating conditions imposed through DCAP. The purpose of this work was to develop and validate a Data Recovery Procedure (DRP) and to demonstrate its capabilities by applying it to a real life space structure. 2. METHODOLOGY

2 As a starting point the method described in [1] was used. It uses the results of a multi-body dynamics simulation run in DCAP as input in a FE software, namely Nastran, to determine the internal forces and stresses in the structure. This was accomplished for a particular time instant and used Matlab functions (some were never coded) to produce a Nastran input file where the motion computed by DCAP was enforced on the structure through the use of a direct matrix abstraction program (DMAP) alter. Considering most multi-body dynamics software simulation capabilities, it would be interesting to develop a similar data recovery module capable of determining the time history of the internal forces during a whole multi-body dynamics simulation. In order to achieve this, two strategies can be followed. The first consists of coding directly in the multi-body software a method for force computation similarly to what happens in FE software. The other is to use already established and proven FE software for the internal forces determination and create an interface between it and the multi-body software, in this case DCAP. The latter has been selected due to its minor complexity. As already mentioned there are several ways to model flexible bodies in DCAP. The most common one is to import a model from Nastran. Being a wellestablished and proven finite element software, and considering that DCAP s flexible models are built using it, Nastran seems to be the natural choice for performing the computation of the internal forces. The motion of a flexible body, which can be obtained from DCAP, can be enforced on the same structure in Nastran. At this point two questions rise: how to obtain the motions in DCAP and how to enforce them in Nastran. Regarding the first question, two strategies were identified: - One was to use a DCAP sensor for each Degree Of Freedom of the structure. Position sensors should be used for translational DOF and integrating gyros for the rotational DOF for deformation outputs. For the position sensors a reference point has to be defined (usually the origin of the body reference frame). This method was used in [1]. It has the disadvantage of increasing the size of the DCAP model substantially since all unconstrained FE nodes should be defined as DCAP nodes and for each of these, a number of sensors equal to the number of DOF should also be defined. For large FE models this strategy becomes unfeasible and leads to very large computation times. Another disadvantage is that the reference frame for the sensors might not be the same as the reference frame in Nastran (the displacement coordinate system) in which the deformations are enforced. This leads to additional transformations from DCAP s chosen frames to Nastran s chosen frames or prior definition of consistent frames for the sensors in DCAP. - The second method is based on the use of modal coordinates, modal velocities and modal accelerations computed in DCAP and the modal shapes matrix imported from Nastran to determine the motions of all DOF of the flexible body. Considering that the modal bases usually used in large structures might consist of up to a few hundred modes and that the structure might have thousands of DOF, recurring to the modal transformations leads to a more elegant solution. The displacements are determined using the transformation from modal coordinates to physical coordinates as stated in expression (1), where x represents the vector of physical coordinates, Φ the matrix of the mode shapes and z the vector of modal coordinates. Similar expressions should be used for the velocities and accelerations. x =Φ z (1) For this work the second strategy using the modal transformations was chosen. Using this technique reduces computation time and prevents the DCAP model from growing exaggeratedly because there is no need for sensors. Another advantage is that, although the solution for the dynamic system is computed through a direct integration scheme (DCAP takes into account the coupling between rigid body motion and elastic motion), the modal coordinates computed by DCAP are output in a way so that they contain only pure elastic motion. As with the first method, there is a disadvantage in using the modal coordinates and it s related to the coordinate system. All matrices in Nastran are assembled in the global coordinate system (the collection of all displacement coordinate systems) and the eigenvectors matrix used in DCAP is represented in the coordinate system of a reference point (usually the basic coordinate system). So if the basic coordinate system differs from the global coordinate system, the physical displacements have to be transformed into the correct global coordinate system. With respect to the second question a careful research was carried out. In [1], the motion was enforced through direct matrix input and a DMAP alter. In [9][10][12] several other methods for enforcing motion are presented. Without using DMAP alters it is possible to enforce motion by the large mass/spring method, the Lagrange Multiplier Technique and through the use of SPCD data bulk entries. The large mass/spring approach is a modelling technique in which elements with large mass or stiffness are placed at points of known accelerations or displacements [10][12][13]. These elements act as constraints on the connected points. If they are sufficiently heavy or stiff, the reactions forces from the structure won t affect the input motions. A typical example of this technique is the earthquake analysis of tall buildings where a single base input is assumed. Despite being very easy to understand and use some considerations should be taken into account. When the enforced motion is applied to a redundant set of boundary points, some fictitious forces and stresses

3 might arise due to the presence of the large masses or springs. In modal formulation, the extra masses cause the occurrence of fictitious low frequency modes. To overcome this the redundant points should be connected with rigid body elements (RBE) to prevent their independent motions. Also, the use of large springs generates high frequency modes that are usually missing from the system and small errors in the loading history may cause large errors in the structural response (through large spurious drifts). This method is therefore recommended for cases in which displacements (large spring) or accelerations (large mass) are known at a single point. The Lagrange multiplier technique (LMT) consists of adding extra degrees of freedom to the matrix solution that are used as force variables for the constraint functions [12][14]. Coefficients are added to the matrices for the equations that couple the constrained displacement variables to the points at which enforced motions are applied. The LMT is an exact method and can be used for all constraints and reduction methods such as single point constraints, multiple point constraints and rigid elements. It provides better accuracy and numerical stability than the large mass method. The main disadvantage is that the LMT is only available through DMAP alters, which were very complicated and costly to upgrade. For these reasons the last version of Nastran for which an LMT alter exists is version 70.7 [14]. The last method of enforcing motions is through the use of SPCD entries [9][13]. These entries define an enforced displacement value for static analysis and an enforced motion value (displacement, velocity or acceleration) for dynamic analysis. This direct method is the recommended by MSC.Nastran. In order to use this technique an SPCD entry should be defined for each DOF where enforced motion is necessary. A dynamic load (TLOADi) entry should also be defined. The time history of the motions should then be introduced in a TABLEDi entry. Finally also loads for all DOF should be added into the same load and selected in the same load case. This method is the most direct method provided by Nastran and presents good results. Its main disadvantage is that the user has to define SPCD, TLOADi and TABLEDi entries for all DOF in the model. For a large model this translates in a very large input file and is impossible to do without some form of automatic generation of the required data bulk entries. In addition to this, a dummy DOF should be defined since, after constraining all DOF, there will be no DOF left in the set assembled in superelement analysis. The SPCD direct method was chosen as the method to implement. 3. IMPLEMENTATION The basic premise behind the SPCD method is to define loading functions for each DOF where enforced motion is desired. For static cases this means creating a number of loading functions equal to the number of DOF of the system. For the dynamic cases there is yet another choice to be made. Nastran gives its users the possibility to enforce displacements, velocities and/or accelerations. In order to insure that the model is run under the same conditions present as in DCAP, only one sort of motion need be enforced in Nastran (either displacements, velocities or accelerations), as the program automatically makes use of its numerical integration schemes to determine the remaining corresponding enforced motions. Nastran 2004 (the version used when this work begun) presented some problems regarding the numerical integration rules used to determine enforced velocities and accelerations. During a normal dynamic analysis Nastran computes the displacements based on the loads and then uses central finite differences to compute the velocities and accelerations. When displacements are enforced, Nastran 2004 uses backwards finite differences to compute the enforced velocities and accelerations instead of central finite differences which translates into a delay of one integration step in the velocity and acceleration time histories. When velocities or accelerations are enforced the expressions are also different leading to displacements different from the ones output by DCAP. Because most finite elements use the displacement-based finite element method it was decided to enforce displacements (which assures the correct values for the displacement are always used). The 2005 version of Nastran claims to have solved this problem by using the same central finite differences that are used for transient analyses and by implementing enforced motion in machine precision [15]. A quick check has shown that indeed the velocities and accelerations computed when displacement is enforced use the correct finite differences but some problems still remain when velocities or accelerations are enforced (leading to different displacements from the expected ones). We are still waiting for a reply from Nastran support regarding this issue. Therefore, to enforce the motion in Nastran, a number of loading functions equal to the number of enforced DOF will have to be defined. These loading functions will represent the time history of the physical displacements output by DCAP. It was thus necessary to code a script that read the eigenvectors matrix from the file used for input in DCAP and the time history of the modal coordinates from the DCAP output files, computed the displacements, determined the corresponding DOF, transformed them into the global coordinate system and then produced an output file with all the SPCD entries as well as the definition of all the dynamic loads where the enforced motion is defined. The developed modules (the dynamic and static Data Recovery pre-processors) follow the basic program flow defined in Fig. 1.a) where the main difference between procedures is that the static pre-processor

4 doesn t run the Timevec routine and it has a different output module. The mesh and element properties defined in the Nastran file used for the DCAP model are the same as the ones that will be used for the data recovery. All kinematic and static boundary conditions should be removed and the SPCD entries from the output file of the data recovery pre-processor should be appended. It was decided to code the data recovery pre-processor in Matlab in order to make use of already available modules that read the time history files of DCAP. The module requires some user inputs namely, the Nastran file that was used to generate the model for DCAP, the file produced by the normal analysis on Nastran and used to build the modal base in DCAP, the number of modes the model is using, the specific mode numbers and the time history file output by DCAP. In order to use this procedure a few simple steps should be followed. The first step is to build a FE model of the desired structure in Nastran. After that the user must run a normal analysis in Nastran to prepare the model for DCAP. The result from this analysis is a file that will be used in DCAP to form the modal basis and in the Data Recovery pre-processor to build the eigenvector matrix. After taking advantage of the full capabilities of DCAP analyses, the user should run the desired Data Recovery Pre-processor (either static or dynamic) which outputs the enforced motion file. A new Nastran analysis should be prepared in order to compute the forces and stresses. For this analysis the user can use the same input file that was used for the aforementioned normal analysis. The user should include in this new file the entries from the output file of the pre-processor. DynSRPrep ParseIn Grids Timevec ReadEigVec discomp dynsrprepout.txt.bdf or.dat files (Nastran input files).nas file (Eigenvector matrix).tod file Fig. 1 Flow chart for: a) the dynamic Data Recovery pre-processor. A few modifications to the Nastran input file should still be made before computing the forces. Since all nodes have been constrained in order to apply the enforced motion, all RBE elements should be eliminated (DOF can t belong simultaneously to the set of degrees of freedom eliminated by multipoint constraints and to the set of DOF eliminated by single point constraints). The multipoint constraint information is implicitly included in the results obtained in DCAP. A dummy DOF must be added to the model. Since all DOF are constrained the solution set is empty. To prevent this, a dummy grid point and a dummy element must be defined. This additional DOF has no influence on the results and serves merely the purpose of opening the l- set and preventing Nastran from generating a fatal error. The last step is to define the type of analysis to run. The user may define a static linear analysis (Sol 101) or a direct transient analysis (Sol 109). A direct transient is used instead of a normal transient because the displacements for the structure are already known and there is no need to compute the eigenmodes again. In addition, because all DOF have enforced motion some mass would have to be added to the dummy DOF which would result in different eigenmodes from the ones used in DCAP. In summary, the steps the user has to take to determine the forces and stresses in the structure are the following: 1. Model the structure in Nastran. 2. Determine the.nas file with the eigenvectors that is to be used in the DCAP analyses, using the DMAP alter for DCAP. 3. Perform the dynamic analysis in DCAP. 4. Run the Data Recovery pre-processor. 5. Prepare the Nastran input file for the data recovery analysis. 6. Remove all RBE and multipoint constraints from the model. 7. Add a dummy degree of freedom to the model. 8. Define the type of analysis to run. It is important to always bear in mind that the model used to obtain the.nas file from which the DCAP is built should be the same as the model used for the Data Recovery afterwards to insure the use of the same modal base. 4. VALIDATION OF THE TECHNIQUE A detailed validation procedure for the data recovery technique was performed. The DRP was validated for static and dynamic analyses and tested for 1D, 2D and 3D models (using some of the most common Nastran elements like CBEAM and CQUAD4). The first step was to analyse the procedure in Nastran alone (Nastran closed loop), i.e., to use the results from a Nastran analysis of a certain structure directly to enforce the displacements and run the DRP. This allowed for the determination of the errors inherent to the procedure (inherent to the way Nastran performs the enforced motion analysis). Analyses on the

5 magnitude of numerical errors were performed and a qualitative measure for the maximum accuracy of the procedure was estimated. This was also an important step because the influence of certain factors like mesh, load type, integration time step and size of the modal base on the results could be studied. These tests also helped establish the main uses of the procedure as a tool. Next a series of tests were performed on simple structures using DCAP results. Due to space constraints only a few results of this phase are presented in this paper D elements dynamic model For the 1-dimensional test case structure, a 1m in length cantilever beam was chosen. The reason for choosing a beam structure is related to the possibility of having simple theoretical references for the internal forces and stresses acting on the structure. The beam was modelled in Nastran through the use of CBEAM elements, PBEAM properties and isotropic MAT1 entries. Its properties are specified in Table 1. Two types of loads were applied: concentrated and uniformly distributed. The concentrated load was applied at the free end of the beam. The uniformly distributed load was applied over the entire beam s length. Two forcing functions were used, a low frequency sine wave and a step function. Table 1 Beam properties. Property Value Beam s length (l) 1.0 m Beam s width (b) 0.05 m Beam s height (h) 0.1 m Transverse area (A) 5.0x10-3 m 2 Moment of inertia (I yy ) x10-6 m 4 Moment of inertia (I zz ) x10-6 m 4 Young Modulus (E) 7.31x10 10 Nm -2 Poisson s ratio (ν) 0.3 Density 7800 kgm -3 d w() t V( x, t) = EI 3 dx d w() t M( x, t) = EI 2 dx 3 2 M ( xtz, ) σ ( x, z, t) = Eε ( x, z, t) = x x I (2) Nastran assumes constant strains, stresses and forces along elements and determines them based on the elements displacements, as shown on expression (3), where G is the rigidity modulus and K z is the factor for computing the transverse shear stiffness, and subscripts a and b refer to both node points of the beam element. In the case of dynamic simulations, Nastran uses the same static formulas although the displacements are computed taking inertia and damping effects into account [7]. 1 3 l l E R = + ; G = ; K = 1 z K AG 12EI 2(1 + ν ) z l l R R R R 2 2 F 2 2 za l EI za yy l l EI u yy R+ R R M ya 4 l 2 4 l θ ya = Fzb l u zb R R M yb 2 θ yb 2 l EI yy Sym R + 4 l (3) Fig. 3 to Fig. 6 present a collection of the most important results obtained. Table 2 summarizes the curves representations. Fig. 2 Loading cases for 1D test case; a) concentrated load applied to the tip of the beam; b) Uniformly distributed load. Six different meshes were used for each of the loading cases: four uniform meshes comprising 2, 4, 20 and 100 elements and two non-uniform meshes comprising 12 and 60 elements. The modal base used consisted of the first 6, 16 and 32 modes of vibration. The theoretical equations used were the following Fig. 3 Internal forces results for a sine load applied to the free end of the 1D beam model.

6 2 4 elements Circle (o), solid line 3 20 elements Plus sign (+), solid line elements Cross (x), dashed line 5 12 elements Square ( ), dotted line 6 60 elements Diamond ( ), solid line Fig. 4 Internal moment results for a sine load applied to the free end of the 1D beam model. Fig. 5 Influence of load type on internal moment results for the finer mesh in the 1D beam model. Fig. 6 Modal base influence on results for uniform 20 element mesh. Table 2 Mesh representations. Mesh ID Representation 1 2 elements Asterisk (*), solid line Results showed that errors (difference between data recovery procedure results and Nastran modal transient results referenced to Nastran modal transient results) were higher close to the free end of beam mainly because of numerical zero representation issues (Nastran modal transient represented zeros as and the data recovery procedure represented them as values of the order of 10-8 ). The errors were also higher for the finer meshes reaching values up to 60% which was unexpected (Fig. 3). The internal moments and stress distribution results presented the same trend. Some research showed that the reason for the existence of the errors in the force, moment and stress distributions (regardless of the mesh) was that, according to [ref], Nastran uses the exact expressions for force, moment and stress determination in simple beam problems. The differences could be explained by the fact that for the DRP, Nastran has no information on the load applied to the structure, which means that it uses expression (3) and not the exact expressions to compute the forces, moments and subsequently the stress. This means that even with complete accuracy on the displacements (which is unlikely, because the machine precision can not be matched unless Nastran 2005 or newer is used) different results would still be obtained due to numerical errors in expression (3) which is just an approximation based on the shaping functions for the beam element. In addition to this, it should be considered that for constant distributions of force and stress, better results were obtained with fewer points because as the number of points increases so do the numerical errors inherent to the process. This however doesn t mean that it s always better to use coarser meshes. It was demonstrated that for other distributions of internal forces and moments, like the linear force distribution and quadratic moment distribution of a typical static pressure loading, the errors decrease as the mesh size decreases. The errors for the coarser meshes were very big because there was no information about the loading conditions. Due to the lack of elements necessary to depict the distribution the differences to the real forces and moments distributions were quite large. These can only be decreased through the use of a finer mesh that represents much more accurately the distribution even if the errors closer to the tip of the beam are somewhat larger. Regarding the increase of the errors as the size of the mesh decreases, it was estimated that these were due to numerical issues (subtraction cancellation) in the use of expression (3). Consider the expressions for the forces at the ends of the beam element in (3). For the smallest mesh used (elements 0.01 in length), the R*l/2 term that multiplies by the rotations is 200 times smaller than the term that multiplies by the

7 difference in end displacements. As the element size decreases the difference in displacements becomes very small (u a -u b 0) which can lead to numerical errors appearing in the force results. These will be less visible near the fixed end because the rotations there can be up to 100 times larger than the displacements leading to the following θa + θb Fi R± O( ua ub) O 200 ua + ub R± O( ua ub) O 2 (4) For very small meshes, there is a loss of significance in the first term of the second member of expression (4) which is not very visible because the second term is dominant. However, close to the tip of the beam the rotations are of the same order of magnitude as the displacements resulting in the following θa + θb Fi R± O( ua ub) O 200 ua + ub R± O( ua ub) O 200 (5) When the mesh is very small both terms of the second member of expression (5) might be of the same order which means that a small error in the first term of the second member will be more visible in the end results. This might explain the reason for the increase in error closer to the tip for finer meshes. A similar reasoning can be used for the moment and stress (that is proportional to the moment). The expressions used are the following 2 l l EI M =± R u u + R + ± i 2 4 l y ( ) ( θ θ ) ( θ θ ) 2 l l EI A = ; B = ; C = 2 4 l b a a b a b y ; (6) For the finer mesh used for the model, A will be 200 times greater than B and approximately 50 times larger than C. Like before, closer to the fixed end, the higher value for the rotations will compensate the difference between A and B and therefore any loss of accuracy in the first and third terms of the second member of (6) will be less visible. On the other hand, close to the free end the first term of the second member will be dominant meaning that any errors might be more noticeable. All results showed that as the time of the simulation grows the errors also increase, mostly due to numerical issues and error accumulation. It was observed that the procedure presents slightly higher errors (still below 1%) for distributed loads than for concentrated loads as shown in Fig. 5. So the load type does not have much influence on the accuracy of the procedure, as expected. Fig. 6 shows that, as the modal base becomes richer the results are better which was also expected. Here the modal gains tool referred in [20] can be particularly effective in helping to determine a modal base capable of characterizing the model without losing performance and accuracy. It was also observed, as intuition would suggest, that as the integration step becomes smaller, the results from the data recovery procedure become more accurate although the increase in accuracy wasn t very noticeable (an integration step 100 times smaller resulted in an increase in accuracy of around 5%, at best) D elements dynamic model For the model with 2D elements, a plate structure was chosen. Its geometric and material properties are shown in Table 3. Table 3 Plate properties. Plate property Value Plate s length (l) 1 m Plate s width (b) 0.6 m Plate s thickness (h) m Transverse Area (A) 6.0x10-4 m 2 Young Modulus (E) 7.31x10 10 Nm -2 Poisson s ratio (ν) 0.3 Density 7800 kgm -3 The plate was modelled with CQUAD4 elements, PSHELL element properties and MAT1 isotropic material entries. The boundary conditions applied to the structure consisted of simply supporting the plate on three sides leaving the last one free. As before, two types of loads were applied. A concentrated load applied to the middle of the free end of the plate, and a distributed load applied uniformly over the plate, as shown in Fig. 7. Figure 7 - Loading cases for 2D test case. For forcing functions, a low frequency sine wave and a step were chosen again. For this test case it was decided to use three different meshes: one consisting of four elements (0.3m by 0.6m, mesh 1), another consisting of sixteen elements (0.15m by 0.25m, mesh 2) and the last one making use of sixty elements (0.1m by 0.1m, mesh 3). Fig. 8 to Fig. 12 present some of the results obtained for the plate model. In Fig. 8 through to Fig. 10 the asterisk curves correspond to mesh 1 (the coarser mesh), the circle curves to the 16 element mesh and the cross curves to the finer mesh (60 element mesh). The modal base comparison was performed for the finer mesh.

8 This test proved that for models different from the simple beam problem, results are much better for finer meshes except at the free end (due to numerical zeros), as would be expected (refer to Fig. 8 to 10). Errors obtained with the enforced motion procedure for internal forces and moments ranged in the order of 0.05%, which indicates that accuracy is limited to numerical precision obtained when enforcing the motion in Nastran. Fig Results for internal moment in the length direction for a concentrated sine load. Fig. 8 Results for internal force in the width direction for a concentrated sine load. It was also established that the influence of the integration step size on the results was minimal (as long as the usual rules for integration step definition are followed). Fig. 11 and 12 show that results present a higher accuracy when the modal base is increased. This led to the conclusion that, in order to increase the accuracy of the force computations using DCAP results, a comprehensive modal base should be used in the dynamic simulations in DCAP. Finally it was also observed that the load type had no significant influence on the results. Fig. 9 - Results for internal force in the length direction for a concentrated sine load. Fig. 11 Influence of modal base on results for internal force in the length direction.

9 Fig Influence of modal base on results for internal moment in the width direction. 5. APPLICATION TO ATV S SA It would of great interest to apply the data recovery procedure for DCAP to a real life space structure to demonstrate its capabilities. To this effect it was decided to apply the DRP to a hypothetical docking case scenario between the Automated Transfer Vehicle (ATV) and the International Space Station (ISS). Specifically, the data recovery procedure was used to recover the internal forces and moments in one of the solar arrays (SA) of the ATV using the modal displacements of the solar array obtained through DCAP non-linear time simulations. In order to have some other results with which to compare the DRP results, a Nastran modal transient analysis was also performed on the ATV s SA. modes were used. The loads were also the same as the ones used in DCAP (they were extracted from DCAP) and they were applied to the same point. The residual vectors option was turned off (because DCAP doesn t use residual vectors) and the mode displacement method was used for data recovery. The first simulations for data recovery were run on a SUN machine using Nastran The results showed a great deal of noise superimposed on the curves. The behaviour was reproduced for a simple beam model and reported to Nastran support that suggested using the Windows version of Nastran 2005 where the noise didn t show up. It is our impression that this noise is related to some machine precision problem. At the date of this paper s publishing, Nastran support has informed us that this issue is indeed an error that will be fixed by development on a later release of Nastran. At first, a DCAP simulation with just one SA attached to the ATV was run and then the data recovery procedure was applied to a single cantilevered SA in Nastran. For comparison, a Nastran modal transient was run on a rigid ATV with one SA attached. On a second iteration the DCAP simulation was run on a rigid ATV with full 4 SA and the resulting data recovery procedure (which was applied to just one SA since the effect of the other three SA on its dynamics were already taken into account in the DCAP results) compared to a Nastran modal transient of a rigid ATV with 4 flexible SA. Fig. 13 and 14 show the Nastran models used and also give an idea of the DCAP models used for this study. 5.1 Modelling In order to keep the model realistic without making it too big and computationally heavy it was decided to model the SA as flexible bodies and the ATV as a rigid body, in DCAP. For that purpose a SA FE model kindly provided by Dutch Space was used to obtain a modal model that was imported into DCAP. This model was repeated four times and attached, through rigid hinges, to a rigid model of the ATV. The ATV model corresponded to a rigid body with the mass and inertia properties of the real ATV. The loads were applied to the ATV through user-defined functions. A time history simulation was run for 60 seconds with a 0.01 integration step. A Nastran equivalent model was also created in order to compare the internal forces and moments results with the ones obtained through the data recovery procedure. The Nastran model consisted the FE model of the SA attached through rigid body elements (RBE) to a concentrated mass element (CONM2) representing the rigid ATV. As in DCAP the first eight flexible Fig. 13 Rigid ATV with 4 flexible SA model used in Nastran and DCAP.

10 Fig. 14 Rigid ATV with single flexible SA model used in Nastran and DCAP. 5.2 Results The modal base of the SA, which was used in DCAP was obtained for a cantilevered SA in a normal modes analysis in Nastran. Table 4 presents a comparison of eigenvalues obtained for the ATV with 4 SA model with DCAP and with the Nastran model for data recovery comparison. As can be seen, the eigenvalues are practically the same showing very small differences. It was also observed that the eigenvectors were approximately the same. This meant that the displacements, internal forces and moments computed by the DRP for DCAP and the Nastran modal transient should be very similar. Table 4 Eigenvalues for the ATV with 4 SA model. DCAP modes (Hz) Nastran modes (Hz) with the DRP for DCAP and the Nastran modal transient for the Rigid ATV with 4 SA model. The values refer to the membrane forces and bending moments in CQUAD elements aligned with the centre axis of the SA and positioned at the base (Fig. 16 to Fig. 18) and at the free tip of the SA (Fig. 19 to 21). Fig. 17 and 20 show the absolute differences between the values of the forces obtained in the Nastran modal transient and the values obtained through the DRP. As can be seen, for forces in the first and third axis the errors are small with values always below 10% (typical values range 5%). The values for the moments are even better (around 2%) which proves that the accuracy of the data recovery procedure for DCAP is quite acceptable. However, for the second axis the internal forces results showed substantially larger differences. These errors were due to differences in the eigenvectors used by the two procedures (DRP and Nastran modal transient) along the axial direction of the SA. Although the modal coordinates were basically the same, by multiplying them by eigenvectors with slight differences along the axial direction of the SA, different displacements and thus forces were obtained. The reason for the different eigenvectors was that, for DCAP these were determined with the SA clamped and for the Nastran modal transient they were determined with the SA connected to a CONM2 through RBE. The fact that the ATV s mass is only 10 5 times greater than the mass of the SA might have caused the differences in the eigenvectors (particularly in that direction). Fig. 16,18, 19 and 21 show that the general distribution for forces and moments is almost identical and that in quantitative terms the values are very close. Similar results were obtained for the transverse shear forces and for the stresses. Fig. 15 shows that the modal coordinates for the first and second modes obtained through DCAP and through the modal transient in Nastran are basically the same. This was observed for all modal coordinates, which means that the internal force and moment results should be very similar provided that the eigenvectors are the same. Fig. 16 to Fig. 21 show the differences between the values of the internal forces and moments obtained

11 Fig. 15 Modal coordinates comparison. Fig. 18 Internal moments for base element. Fig. 16 Internal forces comparison for base element. Fig. 19 Internal forces for tip element. Fig. 17 Internal forces absolute errors for base element. Fig. 20 Internal forces absolute errors for tip element.

12 Fig. 21 Internal moments for tip element. 6. CONCLUSIONS The results obtained during testing and validation of the DRP for DCAP presented in section 4, have shown that the procedures for static and dynamic data recovery work and helped establish a qualitative measure of the accuracy that can be expected from the technique. The worst results were obtained with simple 1D beam models for the reasons stated in section 4.1. It was demonstrated that, in general, better results are obtained with finer meshes, richer modal bases, smaller integration steps and that the results degrade as the simulation time increases. The results of the application of this data recovery procedure to a typical case of a real space structure, have demonstrated the worthiness and accuracy of the procedure. It was shown that it is possible to determine the internal forces and moments as well as the stresses in a flexible structure making use of the full dynamic capabilities of the DCAP software. Furthermore, this procedure and its package give the user the option to determine the forces and moments statically or dynamically in a post-processing phase, which doesn t affect DCAP computational speed. As a result, DRP can be a very useful postprocessing tool for multi-body software (DCAP) and might be used for structural stability verification and design purposes. Using the dynamic results from DCAP it is possible to investigate the forces, moments and stresses present at particularly important points of the structure. It can be also used to study the influence of control systems and environments modelled in DCAP, on flexible parts of complex space systems (like robotic manipulators, or launchers). kinematical and mechanical calculations, TOS- MCS/2002/690/ln/BD, [2] - Franco, R., Dumontel, M. L., Portigliotti S. & Venugopal, R., The Dynamics and Control Analysis Package (DCAP) - A versatile tool for satellite control, ESA Bulletin Nr. 87 August [3] - Portigliotti, S., Dumontel, M., Baldesi, G., & Sciacovelli, D., DCAP: an effective tool for modeling and simulating of coupled controlled rigid flexible structure in space environment, 6th International Conference on Dynamics and Control of Systems and Structures in Space, Riomaggiore, Italy, July [4] DCAP Study Team: DCAP Theory Manual, [5] DCAP Study Team: DCAP User Manual, [6] Bathe, K-J., Finite Element Procedures, Prentice Hall, [7] MacNeal, R. H., MSC.Nastran Theoretical manual, The MacNeal Schwendler Corporation, December [8] MSC.Nastran 2004 Quick Reference Guide. [9] MSC.Nastran 2004 Reference Manual. [10] MSC.Nastran Version 68 Basic Dynamic Analysis User s Guide. [11] MSC.Nastran 2004 DMAP programmer s guide. [12] MSC.Nastran Version 70 Advanced Dynamic Analysis User s Guide. [13] MSC.Nastran Support FAQs, Modeling Enforced Relative Motion, v2001, Solution #4846, [14] MSC.Nastran Support FAQs, A DMAP Alter Package for Enforced Motion in Dynamic Analysis, TAN #4238, [15] MSC.Nastran 2005 Release guide. [16] MSC.Nastran 2005 Quick Reference Guide. [17] Nastran Support, support.nl@mscsoftware.com. [18] Donnell, L. H., Beams, Plates, and Shells, McGraw-Hill Inc., [19] Blevins, R. D., Formulas for natural frequencies and mode shapes, Van Nostrand Reinhold Company, [20] - Deloo, P., Identification of dominant modes for S/C internal responses to shock loads (2), 22 December REFERENCES [1] - Dutilleul, B., Modeling flexible multi-body systems with DCAP, Stress recovery of the DCAP, TVC