Full report

Original page 1

NASA/TM–2017–219604 AF-Shell 1.0 User Guide Mark W. McElroy Langley Research Center, Hampton, Virginia September 2017

Original page 2

NASA STI Program. . . in Profile Since its founding, NASA has been dedicated to the advancement of aeronautics and space science. The NASA scientific and technical information (STI) program plays a key part in helping NASA maintain this important role. The NASA STI Program operates under the auspices of the Agency Chief Information Officer. It collects, organizes, provides for archiving, and disseminates NASA’s STI. The NASA STI Program provides access to the NASA Aeronautics and Space Database and its public interface, the NASA Technical Report Server, thus providing one of the largest collection of aeronautical and space science STI in the world. Results are published in both non-NASA channels and by NASA in the NASA STI Report Series, which includes the following report types: • TECHNICAL PUBLICATION. Reports of completed research or a major significant phase of research that present the results of NASA programs and include extensive data or theoretical analysis. Includes compilations of significant scientific and technical data and information deemed to be of continuing reference value. NASA counterpart of peer-reviewed formal professional papers, but having less stringent limitations on manuscript length and extent of graphic presentations. • TECHNICAL MEMORANDUM. Scientific and technical findings that are preliminary or of specialized interest, e.g., quick release reports, working papers, and bibliographies that contain minimal annotation. Does not contain extensive analysis. • CONTRACTOR REPORT. Scientific and technical findings by NASA-sponsored contractors and grantees. • CONFERENCE PUBLICATION. Collected papers from scientific and technical conferences, symposia, seminars, or other meetings sponsored or co-sponsored by NASA. • SPECIAL PUBLICATION. Scientific, technical, or historical information from NASA programs, projects, and missions, often concerned with subjects having substantial public interest. • TECHNICAL TRANSLATION. Englishlanguage translations of foreign scientific and technical material pertinent to NASA’s mission. Specialized services also include organizing and publishing research results, distributing specialized research announcements and feeds, providing information desk and personal search support, and enabling data exchange services. For more information about the NASA STI Program, see the following: • Access the NASA STI program home page at http://www.sti.nasa.gov • E-mail your question to help@sti.nasa.gov • Phone the NASA STI Information Desk at 757-864-9658 • Write to: NASA STI Information Desk Mail Stop 148 NASA Langley Research Center Hampton, VA 23681-2199

Original page 3

NASA/TM–2017–219604 AF-Shell 1.0 User Guide Mark W. McElroy Langley Research Center, Hampton, Virginia National Aeronautics and Space Administration Langley Research Center Hampton, Virginia 23681-2199 September 2017

Original page 4

The use of trademarks or names of manufacturers in this report is for accurate reporting and does not constitute an official endorsement, either expressed or implied, of such products or manufacturers by the National Aeronautics and Space Administration. Available from: NASA STI Program / Mail Stop 148 NASA Langley Research Center Hampton, VA 23681-2199 Fax: 757-864-6500

Original page 5

Abstract This document serves as a user guide for the AF-Shell 1.0 software, an efficient tool for progressive damage simulation in composite laminates. This guide contains minimal technical material and is meant solely as a guide for a new user to apply AF-Shell 1.0 to laminate damage simulation problems. 1

Original page 6

Contents 1 Introduction 2 Scope of Applicability 3 Limitations 4 Quick Start 5 User-Defined Parameters File 6 Ghost Elements 7 Contact 3 3 4 5 7 9 10 8 Example Problem: Double Cantilever Beam 10 9 Licensing and Distribution Appendices 12 15 A Obtaining Selected User Input Parameters . . . . . . . . . . . . . . . 15 B Selected Variable Definitions . . . . . . . . . . . . . . . . . . . . . . 16 C Example Problem Input Files . . . . . . . . . . . . . . . . . . . . . . 20 C.1 Example Problem User Parameter File (filename: “afshelluser.txt”) . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 20 C.2 Example Problem Abaqus Input File (filename: “dcb2.inp”) . 21 2

Original page 7

1 Introduction AF-Shell 1.0 is a tool for simulating progressive damage in laminates fabricated from uni-directional tape that is intended to offer a level of computational efficiency and ease of use not currently found in existing high mesh fidelity modeling techniques for progressive damage in composites. The increased efficiency is achieved by using finite element models comprised of a single layer of enriched shell elements. AF-Shell 1.0 may be used for static or dynamic type analyses within the Abaqus/Standard (Implicit) solver. The enrichment, based on use of the Floating Node Method (FNM) [1] and a damage algorithm based on the Virtual Crack Closure Technique [2], is such that, given a user-defined initial delamination, a damage path need not be predefined and can evolve in a model solution procedure in three dimensions throughout a laminate of varying ply orientations. The name, AF-Shell, stands for Adaptive Fidelity Shell, which refers to the adaptive mesh splitting approach that the FNM uses to split elements on demand as a damage pattern forms throughout an analysis solution. AF-Shell 1.0 is implemented as a user-defined element and external database subroutines in Abaqus/Standard. Thorough technical documentation of the model formulation can be found in several sources [3–7]. In addition to a description of the model formulation, these publications contain verification and validation cases of the model, along with some investigation into its current limitations. 2 Scope of Applicability AF-Shell 1.0 should be used to evaluate damage growth starting from an initial user-defined delamination in a flat laminate plate. The nature of loading can be general, however, large and non-linear deformation type analyses (such as stability) are not yet included in the model capabilities. The following is a list of problems that AF-Shell 1.0 may be suitable for: 1. Test coupon design: The model can be used to quickly predict damage growth behavior in composite laminate test coupons. AF-Shell 1.0 may be useful in the design of test specimens and/or the planning of test programs. 2. Damage tolerance: The model can be used to evaluate damage growth potential from an existing characterized flaw in a plate/panel type structure. 3. Skin-stringer flange pull off: Given a small user-defined “starter delamination” at a skin-stringer flange interface, the model can be used to predict damage tolerance. 4. Large scale structures: The shell formulation and high efficiency of AF-Shell 1.0 potentially allows its use in quick and cost effective simulations of large structures. While an initial delamination is still required, damage growth scenarios can be quickly evaluated at multiple locations throughout the structure without extensive model modifications or the use of a local region consisting of a high fidelity mesh and damage modeling technique. 3

Original page 8

1. Compression after impact: AF-Shell 1.0 may be useful in predicting damage initiation and growth up until a point of instability for compression after impact analyses. 6. Rapid design tool: Any of the listed uses above may utilize AF-Shell 1.0 in a rapid design type function. AF-Shell 1.0 may help early on in a design process, to guide and inform design of structures that ultimately may be subjected to testing or more expensive detailed simulations. 3 Limitations The following are limitations and considerations for the user to keep in mind while using AF-Shell 1.0. 1. Applicable only to laminates containing uni-directional fiber-reinforced-matrix composite plies. The plies may be oriented in varying directions throughout the laminate. 2. An initial delamination must be defined by the user (i.e., no damage initiation capability). 3. The initial delamination should contain a path of at least three successive “interior nodes” emanating in the crack wake from any delamination front node. For example, to satisfy this requirement, an initial delamination, square in geometry, that is not located on a free edge must have a minimum size of 4 × 4 elements. Examples of initial delaminations that are and are not acceptable are shown in Figure 1. Figure 1. Examples of initial delaminations that are and are not acceptable. 4. A maximum of one delamination (i.e., initial or otherwise) can be included at a specific location in the mesh (i.e., one delamination per element). 5. The only damage modes included are delamination and transverse matrix cracking. Furthermore, transverse matrix cracking can only occur in the model if it is associated with a delamination-changing ply interface. Additional damage modes such as fiber breaking, fiber kinking, matrix crushing, etc. are not included in the AF-Shell 1.0 simulation capabilities. 6. Matrix cracking associated with delamination-migration that traverses multiple ply blocks of differing fiber orientation (i.e., “staggered migration” [5]) 4

Original page 9

is represented in the mesh such that the model may be too flexible in these regions. 7. Care should be taken in sizing the mesh so that element edge dimensions are not less than 0.2 times the total laminate thickness. 8. Only square and rectangular elements are supported. The mesh should consist entirely of uniform square elements if possible. 9. The mesh should be aligned with the global model coordinate system. 10. Use caution if a bi-material crack tip condition exists. The model was verified to be accurate in one bi-material delamination problem [3], however, testing and investigation in this area is incomplete. 11. Progressive damage processes occurring in general layups consisting of transverse cracking and delamination-migration should be Mode II dominated for accurate transverse cracking predictions. 12. The initial delamination should be defined in a mesh located in the x-y plane (analysis of curved structures may be possible but this has not yet been verified or validated). 13. Maximum model size of 10,000 enriched shell elements and 50,000 nodes (including floating nodes). 4 Quick Start AF-Shell 1.0 must be used in conjunction with Abaqus/Standard 6.14 as a userdefined element subroutine [8]. To model damage growth in a composite structure, an Abaqus input file consisting of a shell mesh should be created with the following modifications: 1. Enrich mesh with floating nodes: The mesh can be created initially as a single layer of native S4 shell elements. The nodes in the initial layer of shells are referred to as “real nodes”. Each element is enriched by including a “floating node” in the input file at the same coordinates of each real node (i.e., the total number of nodes is doubled). The shell element definitions in the input file should be modified to include a total of 8 nodes in their definitions (i.e., append the original element definition with four floating nodes whose numbering convention follows the real nodes [8]). 2. Define the Abaqus parameters for user elements in the model using the following command: *USER ELEMENT,TYPE=U6,NODES=8,COORDINATES=3,PROPERTIES=1,VARIABLES=6 1,2,3,4,5,6 5

Original page 10

1. Assign property to element set of user elements using the following command line (in this example the element set is named “userel”): UEL PROPERTY, ELSET=userel 1 4. Populate user-defined input file, “afshelluser.txt”, with desired model parameters (see Section 5). 5. Create boundary condition at all nodes in the model to restrain degree of freedom 6 (i.e., θz). A working directory should be created containing the following three files. The working directory should be on the same drive on which Abaqus is installed (i.e., in a Windows environment, if the working directory is on drive D:, the analysis cannot be run using Abaqus that is installed on drive C: or installed on a remote server). 1. job filename.inp – Abaqus model input file (contents vary, see Section 8 for an example) 2. afshelluser.txt – text file containing user input model parameters (see Section 5 for contents) 3. nabaqus.bat – batch file (contents shown below) @echo off if NOT exist "afshelluser.txt" (ECHO "file not found (see nabaqus.bat file)") If NOT exist "afshelluser.txt" goto :exit SET CWD=%cd% "abaqus" % :exit A model is run by opening an Abaqus command prompt, navigating to the working directory, and using the modified .bat file “nabaqus” to execute a job by typing the command: >nabaqus job=job filename user=subroutine filename interactive By default, several variables, defined in Appendix B, central to the AF-Shell 1.0 code functionality are printed in the .msg file after each converged solution increment. The user may obtain detailed information from these variables which can be used to debug, plot model results (such as energy release rate along a delamination front), or gain an understanding of the model results that would otherwise be unobtainable. The user may choose to print additional information beyond the default variables. This may include information related to nodal forces and displacements, element nodal ties, or the element mass and stiffness matrices. Printing this information may be useful in certain instances, but doing so can increase both runtime and .msg file size significantly. See Section 5 for further explanation. 6

Original page 11

5 User-Defined Parameters File A text file should be included in the working directory named “afshelluser.txt”. The file includes user-defined model parameters related to material properties, damage growth parameters, layup configuration, and some model parameters unique to AF- Shell 1.0. Appendix A contains a description of how to obtain selected user-defined parameters. The syntax of the user parameter file is similar to an Abaqus input file in that keywords preceded by an “*” identify the user parameter that is included in the next line. An example user input file is shown in Appendix C.1 and is related to an example model described in Section 8. A description of each user input parameter is shown below. The units should be consistent with those of the Abaqus input file. *ELASTIC – Elastic material properties of cured lamina. Column 1 = E11 (Young’s Modulus) Column 2 = E22 (Young’s Modulus) Column 3 = ν12 (Poisson’s ratio) Column 4 = G12 (Shear Modulus) Column 5 = G13 (Shear Modulus) Column 6 = G23 (Shear Modulus) *DENSITY – Density of cured laminate. *ZK – z-coordinates of ply interfaces from the bottom up (maximum of 101 entries). *BETAK – Angle of fibers in each ply from the bottom up (maximum of 100 entries). *CONTACT – Crack surface contact modeling technique. 0 = Abaqus surfaceto-surface, 1 = z-tie, 2 = conditional z-tie (see Section 7). *NPLYTOT – Total number of plies in layup. *GIC – Mode I critical energy release rate (i.e., fracture toughness). *GIIC – Mode II critical energy release rate (i.e., fracture toughness). *GETA – Exponent parameter η used in the BK mixed-mode critical energy release rate equation [9]. *ZFRACLOC – User-defined initial delamination. Multiple rows can be used for multiple initial delaminations. For each row the columns correspond to: Column 1 = ply interface Column 2 = geometry type (1=rectangle or 2=circle, see below) 1=rectangle Columns 3 and 4 = lower and upper x-limits of rectangle Columns 5 and 6 = lower and upper y-limits of rectangle 7

Original page 12

2=circle Columns 3 and 4 = x and y coordinates of circle center Column 5 = circle radius Column 6 = 0 (N/A, set to zero) *DELADEF – Average area of elements (ideally element size is uniform). *ALPHACRIT – Critical angle between shearing direction and bounding fibers such that delmaination-migration is allowed [6] (units are degrees). Based on preliminary ◦ ◦ investigation [7], this parameter should be defined in the range of 40 -55 . *INITMUL – Multiplier for GIIc at locations on a thin insert boundary (i.e., at the boundary of a PTFE insert used to simulate a pre-existing delamination). *SPLITRAD – Number of elements ahead of crack tip that are split but tied at 4 nodes (default value is 8, minimum of 4 is recommended). *SMOOTHING – Parameters to define application of Gaussian smoothing along a delamination front for energy release rate values (GT) or for in-plane shear tie force vector angle (FSA). The values included in the examples in this guide are the default and were found to be the most accurate in previous model verification and validation work [7]. Column 1 = FSA number of smoothing passes (i.e., smoothing can be applied repeatedly to smooth already smoothed values. Set this to zero if FSA smoothing is not desired). Column 2 = FSA minimum number of nodes on a delamination front to apply smoothing (i.e., for example if this parameter is set to 16, FSA smoothing will not be performed on delamination fronts with 16 or fewer nodes). Column 3 = FSA number of nodes included in the Gaussian population on one side of a smoothed node (for example if this parameter is set equal to 1, a node that is being smoothed will include 1 node on either side along the delamination front in the Gaussian population when a smoothing factor is determined). Column 4 = GT number of smoothing passes (similar to Column 1). Column 5 = GT minimum number of nodes on a delamination front to apply smoothing (similar to column 2). Column 6 = GT number of adjacent nodes to include in the Gaussian population (similar to column 3). Column 7 = Apply GT smoothing to VCCT calculations? 1 = yes or 2 = no (recommend 2 in general use). *DEBUGPRINT – Request printing extra information in .msg file to aid with debugging. 0 = no, >0 = element number of interest (can only request information on one element at a time). *DEBUGLOC – Location in code where extra information should be printed. 0 8

Original page 13

= before analysis, 1 = start of each increment, 2 = end of each increment, 3 = element stiffness formulation. Include all desired locations, separated by a space, on one line. If line is blank, printing is suppressed. Notes or comments can be included in the user parameter file following a comma after a keyword. An example of a comment included for the keyword *GIC is shown below: *GIC, VALUE OBTAINED FROM TESTING MATERIAL SYSTEM C12K/R6376 0.33D0 6 Ghost Elements User-defined elements are unable to be plotted in the Abaqus post-processor. Post processing AF-Shell 1.0 simulation results can be done by printing information to the .msg file or, if visualization of the deformed model results is required, by using “ghost elements” superimposed over the AF-Shell 1.0 enriched elements. Ghost elements are defined using reduced integration membrane elements (Abaqus element type M3D4R) with stiffness approaching zero that are superimposed on the AF-Shell 1.0 element nodes. Different unconnected sets of ghost elements should be defined for the real nodes and the floating nodes. AF-Shell 1.0 is set up such that a ghost mesh is defined using membrane elements that have a user-defined material. The purpose of the user-defined material is so that a state variable (STV(1)) can be assigned to each ghost element, indicating the number of plies. As delaminations grow during a solution procedure and new elements are split, the state variable can be plotted in the Abaqus post-processor to indicate the delamination interface in each element. This visualization technique also illustrates the location of transverse matrix cracks. Note that if ghost elements are used, computational burden is added to the solution and the efficiency benefits offered by the Floating Node Method are not fully realized. The Abaqus input file structure for defining ghost elements is: *Element, type=M3D4R, elset=ghostel (ghost element definitions) *Orientation, name=Ori-1 1.,0.,0.,0.,1.,0. 3, 0. *Membrane Section, elset=ghostel, material=UMAT 1., *Hourglass stiffness 1 The ghost elements are assigned the user material named “UMAT”. This material 9

Original page 14

is defined as: *Material, name=UMAT *Depvar 8, *User Material, constants=9 1E-9,1E-9,1E-9,0.32,.32,.45,1E-9,1E-9, 1E-9 7 Contact Contact between delamination crack surfaces can be captured in AF-Shell 1.0 using three different techniques. The user must designate the desired approach in the user parameter file using keyword *CONTACT as described in Section 5. The three contact techniques and some comments on their use are listed below: 1. Abaqus surface-to-surface contact: The user-defines surfaces in the Abaqus input file between real and floating nodes according to typical contact modeling procedures in Abaqus. Ghost elements may also be used to define an element-based surface for contact. This option is best for problems where (i) mode-mixity throughout the model either varies or is unknown and (ii) frictional effects of the sliding crack surfaces need to be accounted for. Typical convergence difficulties related to contact modeling in Abaqus may arise when using this approach [8]. If no contact is desired, this option should be selected in the user parameter file but with the contact definition omitted from the Abaqus input file. 2. z-tie contact: The crack surfaces are tied together in the z-direction only (i.e., they can slide freely, but cannot separate). This option should only be used in cases where the (i) delaminations are Mode II dominated and (ii) friction does not need to be included. The z-tie contact option does not suffer from convergence difficulties seen in the surface-to-surface option. 3. Conditional z-tie contact: Same as z-tie contact, but the tie is removed if a real node and a floating node are trying to separate. This option should be used in cases where (i) mode-mixity throughout the model either varies or is unknown and (ii) friction does not need to be included. Contact “chattering”, where a nodal location repeatedly comes in and out of contact, is possible when using conditional z-tie contact. This behavior can lead to convergence difficulties and/or inaccurate progressive damage predictions and as a result this option is poorly suited for dynamic analyses. 8 Example Problem: Double Cantilever Beam An example AF-Shell 1.0 model is described in this section (run using Abaqus/Standard 6.14). A rudimentary model of a Double Cantilever Beam (DCB) is selected. The 10

Original page 15

example model is not based on an experiment. A summary of the specimen geometry and finite element model is shown in Figure 2. The test consists of a fiber reinforced composite laminate specimen containing a pre-existing delamination at the midplane through the width at one end. Opposing displacement controlled loads are applied normal to the specimen along the edge where the pre-existing delamination is located. Note that, in this example, the crack wake surfaces are not in contact with one another so, while the contact method is assigned to the z-tie technique, this functionality is not activated in this analysis. Complete user parameter and Abaqus input files for this example are included in Appendices C.1 and C.2, respectively. [15/0/-15] z x y δ δ B = 20.0 mm a = 25.0 mm 1.5 o 2h = 3.0 mm δ = 6.0 mm 0.75 0 2L = 100.0 mm P = reaction force -1.5 (a) Specimen configuration Prescribed displacement z • δ = -6 mm • δ = 6 mm x y Boundary condition u = v = w = θx = θy = θz = 0 (b) Finite element model overview z (mm) -15° 0° ao 15° (c) Layup detail Figure 2. Summary of DCB specimen geometry. After an initial linear elastic response, a peak force is reached and delamination growth initiates. The force-displacement (P-δ) response of the upper loading arm on the DCB is shown in Figure 3. Each peak in the sawtooth shape of the force displacement curve represents one row of nodal ties being released. If desired, the best way to minimize the sawtooth response in AF-Shell 1.0 is to refine the mesh. The deformed shape of the model at the beginning and end of the analysis is shown in Figure 4, where the contours correspond to state variable 1 (SDV1). AF-Shell 1.0 assigns SDV1 to each ghost element to represent the number of plies in that region of material. 11

Original page 16

12 10 8 6 force (N)4 2 0 0 1 2 displacement (mm) 3 4 5 6 Figure 3. Force-displacement response of upper loading arm in DCB. SDV1 1 PLY 2 PLIES 3 PLIES (a) prior to damage initiation (mesh size = 5 mm) (b) end of analysis Figure 4. Deformed shape of DCB model at the beginning and end of the analysis. 9 Licensing and Distribution The AFS software is licensed and distributed via the NASA Langley Research Center Technology Transfer Office. Interested parties should contact the Technology Transfer Office at: NASA Langley Research Center Mail Stop 151 Hampton, VA 23681-2199 Phone: (757) 864-1178 Email: LARC-DL-technologygateway@mail.nasa.gov Alternatively, the technical point of contact can be reached at: Mark McElroy mark.w.mcelroy@nasa.gov References 1. B Chen, S Pinho, N De Carvalho, P Baiz, and T Tay. A floating node method for the modelling of discontinuities in composites. Engineering Fracture Mechanics, 127:104–134, 2014. 2. R Krueger. Virtual crack closure technique: history, approach, and applications. Applied Mechanics Reviews, 57(2):109–143, 2004. 12

Original page 17

1. M McElroy. An enriched shell finite element for progressive damage simulation in composite laminates, NASA/TM 2016-219211. NASA, 2016. 4. M McElroy. Use of an enriched shell finite element to simulate delaminationmigration in a composite laminate. Composite Structures, 167:88–95, 2017. 5. M McElroy, W Jackson, R Olsson, P Hellstrom, S Tsampas, and M Pankow. Interaction of delaminations and matrix cracks in a CFRP plate, Part I: A test method for model validation (submitted). Composites Part A: Applied Science and Manufacturing, 2017. 6. M McElroy, R Gutkin, and M Pankow. Interaction of delaminations and matrix cracks in a CFRP plate, Part II: Simulation using an enriched shell finite element model (submitted). Composites Part A: Applied Science and Manufacturing, 2017. 7. M McElroy. An Enriched Shell Finite Element for Progressive Damage Simulation in Composite Laminates. PhD thesis, North Carolina State University, Raleigh, NC, 2016. 8. Dassault Systems, Abaqus 6.13 Analysis User Manual. 2013. 9. M Benzeggagh and M Kenane. Measurement of mixed-mode delamination fracture toughness of unidirectional glass/epoxy composites with mixed-mode bending apparatus. Composites Science and Technology, 56(4):439–449, 1996. 10. ASTM D3039-01 Standard test method for tensile properties of polymer matrix composite materials. In 2004 Annual Book of Standards, Volume 15.03. ASTM International, West Conshohoken, PA (USA), 2004. 11. ASTM D5379-01 Standard test method for shear properties of composite materials by the V-notched beam method. In 2004 Annual Book of Standards, Volume 15.03. ASTM International, West Conshohoken, PA (USA), 2004. 12. ASTM D5528-01 Standard test method for mode I interlaminar fracture toughness of unidirectional fiber-reinforced polymer matrix composites. In 2004 Annual Book of Standards, Volume 15.03. ASTM International, West Conshohoken, PA (USA), 2004. 13. ASTM D7905 Standard test method for determination of the mode II interlaminar fracture toughness of unidirectional fiber-reinforced polymer matrix composites. In 2014 Annual Book of ASTM Standards, Volume 15.03. ASTM International, West Conshohoken, PA (USA), 2014. 14. ASTM D6671m-04 Standard test method for mixed mode I-mode II interlaminar fracture toughness of unidirectional fiber-reinforced polymer matrix composites. In 2004 Annual Book of Standards, Volume 15.03. ASTM International, West Conshohoken, PA (USA), 2004. 13

Original page 18

1. T O’Brien, W Johnston, and G Toland. Mode II interlaminar fracture toughness and fatigue characterization of a graphite epoxy composite material, NASA/TM 2010-216838. NASA, 2010. 14

Original page 19

Appendices A Obtaining Selected User Input Parameters *ELASTIC E11, E22, and ν12: ASTM D3039 Standard Test Method for Tensile Properties of Polymer Matrix Composite Materials: Flat material specimen placed into mechanical frame, monotonic tensile load applied; force, displacement, and strain recorded [10]. G12, G23, G13: ASTM D5379 Standard Test Method for Shear Properties of Composite Materials by the V-Notched Beam Method: Rectangular beam specimen with two symmetric V-notches placed in a special shear load fixture; strain gauges at +/- 45 degree in the center of the beam measure shear response [11]. *GIC GIc: ASTM D5528 Standard Test Method for Mode I Interlaminar Fracture Toughness of Unidirectional Fiber-Reinforced Polymer Matrix Composites: Flat unidirectional laminate specimen containing a non-adhesive insert to act as a crack starter, loaded out of plane by opposing tensile forces to open and grow crack (DCB test); load and delamination length are recorded. Mode I interlaminar fracture toughness is calculated using a modified beam theory or compliance calibration method [12]. *GIIC GIIc: ASTM D7905 Standard Test Method for Determination of the Mode II Interlaminar Fracture Toughness of Unidirectional Fiber-Reinforced Polymer Matrix Composites: Rectangular unidirectional laminate specimen containing a nonadhesive insert to act as a crack starter, supported at two ends by rollers and loaded out of plane in between the supports (End Notch Flexure test). Mode II Interlaminar Fracture Toughness is obtained using the compliance calibration method [13]. *GETA η : Curve fit the the Benzeggah-Kenane equation [9] BK η c Ic IIc GIc)(GII/GT ) BK (1) G = G + (G − to three Gc vs. GII/GT data points. Two of these data points are known, i.e., pure Mode I and pure Mode II. A third must be determined experimentally (could use a Mixed-mode Bending test to obtain the experimental value [14]). *ALPHACRIT αc - Perform a biaxial-bending test as described by McElroy et al. [5]. If performing this test is not feasible, perform a numerical parametric study using AF-Shell where ◦ ◦ αc varies between 40 and 55 and choose a value for which transverse cracking is logical in terms of fiber direction and crack continuity (i.e., a predicted transverse crack should not be such that it breaks fibers). 15

Original page 20

*INITMUL fIIc - Use data from O’Brien et al. [15] or perform a similar study. The average value determined by O’Brien et al. was 1.59 for an IM7/8552 carbon-epoxy material system containing a thin Polytetrafluoroethylene insert used to simulate an initial delamination. B Selected Variable Definitions The following variables are printed to the message file (.msg) during an analysis. The data contained in these variables may be used to debug, generate plots, or gain insight to the model results. DELAMAREA – Total area of delamination at each ply interface. Each row corresponds to a ply interface. The rows are ordered by interface number from the bottom up in the laminate. Column 1 = delamination area FORMOD – Contains information on smoothed in-plane shear tie force vector angle (FSA). Each row corresponds to one node along the delamination front. The rows are sorted in nodal order along the front. Column 1 = node number Column 2 = FSA before Gaussian smoothing (degrees) Column 3 = FSA after Gaussian smoothing (degrees) Column 4 = Fx tie force component after Gaussian smoothing Column 5 = Fy tie force component after Gaussian smoothing Column 6 = Magnitude of shear tie force vector (i.e., resultant) after Gaussian smoothing FRONTFOR – A three dimensional matrix containing information on tie forces and adjacent node numbers for each delamination front node. Each row corresponds to a different tied delamination front node. The rows are sorted in nodal order along the delamination front. The 1st index in the third dimension corresponds to forces before Gaussian smoothing. The 2nd index in the third dimension corresponds to values after Gaussian smoothing. 1st index in third dimension: Column 1 = node number Column 2 = Fx tie force component before Gaussian smoothing Column 3 = Fy tie force component before Gaussian smoothing Column 4 = Fz tie force component before Gaussian smoothing Column 5 = Mx tie moment component before Gaussian smoothing Column 6 = My tie moment component before Gaussian smoothing Column 7 = adjacent node in -x direction Column 8 = adjacent node in +x direction Column 9 = adjacent node in -y direction Column 10 = adjacent node in +y direction 16

Original page 21

2nd index in third dimension: Column 1 = node number Column 2 = Fx tie force component after Gaussian smoothing Column 3 = Fy tie force component after Gaussian smoothing Column 4 = Fz tie force component before Gaussian smoothing Column 5 = Mx tie moment component before Gaussian smoothing Column 6 = My tie moment component before Gaussian smoothing Column 7 = adjacent node in -x direction Column 8 = adjacent node in +x direction Column 9 = adjacent node in -y direction Column 10 = adjacent node in +y direction FRONTINFO – Matrix containing energy release rate and delamination growth information at tied nodes along a delamination front. Each row corresponds to a different front node. The rows are sorted in nodal order along the delamination front. Column 1 = node number Column 2 = total energy release rate, GT Column 3 = critical energy release rate, Gc Column 4 = Mode I energy release rate, GI Column 5 = Mode II energy release rate, GII Column 6 = Mode II ratio, GII/GT Column 7 = number of adjacent tied nodes Column 8 = length of delamination advance, ∆a Column 9 = x-coordinate of node Column 10 = y-coordinate of node Column 11 = direction of delamination propagation (1=+x, -1=-x, 2=+y, -2=-y) Column 12 = tie shear force in propagation direction Column 13 = Fx tie force component after Gaussian smoothing Column 14 = Fy tie force component after Gaussian smoothing MIGRATION – Energy release rate information at tied nodes along a delamination front. Each row corresponds to a different node. The rows are sorted in nodal order along the delamination front. Column 1 = node number Column 2 = Mode II energy release rate calculated for delamination growth in the x direction, GSX Column 3 = Mode II energy release rate calculated for delamination growth in the y direction, GSY√ Column 4 = GSX2 + GSY 2 −1 Column 5 = tan (GSY /GSX) MIGRATION EL – Contains information for each element in the direction of delamination growth that contains a nodal tie that was released in the previous solution increment. Information in this matrix is related to evaluation of whether or not 17

Original page 22

migration occurs when this element is split as part of delamination growth. Each row corresponds to a different element. Column 1 = element number Column 2 = previous delamination ply interface (i.e., in the wake of delamination growth) Column 3 = new delamination interface Column 4 = released node number associated with delamination growth in this element Column 5 = previous angle of bounding fibers (degrees) Column 6 = new angle of bounding fibers (degrees) Column 7 = direction of delamination growth (1=+x, -1=-x, 2=+y, -2=-y) Column 8 = tie shear force angle, FSA (after Gaussian smoothing) Column 9 = difference in angle between FSA and bounding fibers, α Column 10 = did delamination-migration occur? 1 = yes, 2 = no Column 11 = energy release rate associated with transverse crack growth, Gmig Column 12 = transverse growth tendency of delamination (1 = ply above, 2 = ply below) Column 13 = index RATIOMIG determining if migration is forced in order to maintain transverse matrix crack continuity (if RATIOMIG<=1.49, a transverse matrix crack exists in an adjacent element and therefore migration may be forced to maintain crack continuity) NODEMASTER – Contains information at each node in the model concerning tie forces and relative displacements used in the VCCT calculations. Each row corresponds to a different node number. Column 1 = node number Column 2 = Fx tie force component Column 3 = Fy tie force component Column 4 = Fz tie force component Column 5 = Mx tie moment component Column 6 = My tie moment component Column 7 = adjacent node number located in the crack wake for delamination growth in the +x direction Column 8 = relative Mode II crack wake opening for delamination growth in the +x direction Column 9 = relative Mode I crack wake opening for delamination growth in the +x direction Column 10 = relative crack wake opening rotation (θy) for delamination growth in the +x direction Column 11 = adjacent node number located in the crack wake for delamination growth in the -x direction Column 12 = relative Mode II crack wake opening for delamination growth in the -x direction Column 13 = relative Mode I crack wake opening for delamination growth in the -x direction Column 14 = relative crack wake opening rotation (θy) for delamination growth 18

Original page 23

in the -x direction Column 15 = adjacent node number located in the crack wake for delamination growth in the +y direction Column 16 = relative Mode II crack wake opening for delamination growth in the +y direction Column 17 = relative Mode I crack wake opening for delamination growth in the +y direction Column 18 = relative crack wake opening rotation (θx) for delamination growth in the +y direction Column 19 = adjacent node number located in the crack wake for delamination growth in the -y direction Column 20 = relative Mode II crack wake opening for delamination growth in the -y direction Column 21 = relative Mode I crack wake opening for delamination growth in the -y direction Column 22 = relative crack wake opening rotation (θx) for delamination growth in the -y direction Column 23 = is the node tied to its corresponding floating node? 0 = no, 1 = yes, 2 = release tie in this step STATEMASTER – Designates, for all elements, split location and whether or not each real node is tied to its corresponding floating node. Each row corresponds to a different element. Column 1 = element number Column 2 = is element node 1 tied? 0 = no, 1 = yes Column 3 = is element node 2 tied? 0 = no, 1 = yes Column 4 = is element node 3 tied? 0 = no, 1 = yes Column 5 = is element node 4 tied? 0 = no, 1 = yes Column 6 = delamination ply interface (0 = no delamination) 19

Original page 24

C Example Problem Input Files C.1 Example Problem User Parameter File (filename: “afshelluser.txt”) dcb2.inp *ELASTIC 139400 10160 0.3 4600 4600 3540 *DENSITY .00000000159 *ZK -1.5 0 0.75 1.5 *BETAK 15 0 -15 *NPLYTOT 3 *CONTACT 1 *GIC 0.33D0 *GIIC 0.8D0 *GETA 2.284D0 *ZFRACLOC 2 1 75 200 -1 100 *DELADEF 6.25 *ALPHACRIT 55 *INITMUL 1.0 *SPLITRAD 8 *SMOOTHING 1 16 1 1 16 1 2 *DEBUGPRINT 1 *DEBUGLOC 0 1 20

Original page 25

C.2 Example Problem Abaqus Input File (filename: “dcb2.inp”) **Example user input file for AF-Shell 1.0 model **This input file is published in the AF-Shell 1.0 User Manual (2017) **Nodes 1-105 are "real nodes" **Nodes 106-210 are "floating nodes" **Elements 1-80 are user elements (i.e., enriched shell elements) **Elements 50001-50160 are ghost elements ** **Input file begins here: ** *Part, name=Part-1 *End Part *Assembly, name=Assembly *Instance, name=Part-1-1, part=Part-1 0, 0, 0. *Node 1,0,0,0 2,5,0,0 3,10,0,0 4,15,0,0 5,20,0,0 6,25,0,0 7,30,0,0 8,35,0,0 9,40,0,0 10,45,0,0 11,50,0,0 12,55,0,0 13,60,0,0 14,65,0,0 15,70,0,0 16,75,0,0 17,80,0,0 18,85,0,0 19,90,0,0 20,95,0,0 21,100,0,0 22,0,5,0 23,5,5,0 24,10,5,0 25,15,5,0 26,20,5,0 27,25,5,0 28,30,5,0 29,35,5,0 30,40,5,0 31,45,5,0 32,50,5,0 33,55,5,0 34,60,5,0 35,65,5,0 21

Original page 26

36,70,5,0 37,75,5,0 38,80,5,0 39,85,5,0 40,90,5,0 41,95,5,0 42,100,5,0 43,0,10,0 44,5,10,0 45,10,10,0 46,15,10,0 47,20,10,0 48,25,10,0 49,30,10,0 50,35,10,0 51,40,10,0 52,45,10,0 53,50,10,0 54,55,10,0 55,60,10,0 56,65,10,0 57,70,10,0 58,75,10,0 59,80,10,0 60,85,10,0 61,90,10,0 62,95,10,0 63,100,10,0 64,0,15,0 65,5,15,0 66,10,15,0 67,15,15,0 68,20,15,0 69,25,15,0 70,30,15,0 71,35,15,0 72,40,15,0 73,45,15,0 74,50,15,0 75,55,15,0 76,60,15,0 77,65,15,0 78,70,15,0 79,75,15,0 80,80,15,0 81,85,15,0 82,90,15,0 83,95,15,0 84,100,15,0 85,0,20,0 86,5,20,0 87,10,20,0 22

Original page 27

88,15,20,0 89,20,20,0 90,25,20,0 91,30,20,0 92,35,20,0 93,40,20,0 94,45,20,0 95,50,20,0 96,55,20,0 97,60,20,0 98,65,20,0 99,70,20,0 100,75,20,0 101,80,20,0 102,85,20,0 103,90,20,0 104,95,20,0 105,100,20,0 106,0,0,0 107,5,0,0 108,10,0,0 109,15,0,0 110,20,0,0 111,25,0,0 112,30,0,0 113,35,0,0 114,40,0,0 115,45,0,0 116,50,0,0 117,55,0,0 118,60,0,0 119,65,0,0 120,70,0,0 121,75,0,0 122,80,0,0 123,85,0,0 124,90,0,0 125,95,0,0 126,100,0,0 127,0,5,0 128,5,5,0 129,10,5,0 130,15,5,0 131,20,5,0 132,25,5,0 133,30,5,0 134,35,5,0 135,40,5,0 136,45,5,0 137,50,5,0 138,55,5,0 139,60,5,0 23

Original page 28

140,65,5,0 141,70,5,0 142,75,5,0 143,80,5,0 144,85,5,0 145,90,5,0 146,95,5,0 147,100,5,0 148,0,10,0 149,5,10,0 150,10,10,0 151,15,10,0 152,20,10,0 153,25,10,0 154,30,10,0 155,35,10,0 156,40,10,0 157,45,10,0 158,50,10,0 159,55,10,0 160,60,10,0 161,65,10,0 162,70,10,0 163,75,10,0 164,80,10,0 165,85,10,0 166,90,10,0 167,95,10,0 168,100,10,0 169,0,15,0 170,5,15,0 171,10,15,0 172,15,15,0 173,20,15,0 174,25,15,0 175,30,15,0 176,35,15,0 177,40,15,0 178,45,15,0 179,50,15,0 180,55,15,0 181,60,15,0 182,65,15,0 183,70,15,0 184,75,15,0 185,80,15,0 186,85,15,0 187,90,15,0 188,95,15,0 189,100,15,0 190,0,20,0 191,5,20,0 24

Original page 29

192,10,20,0 193,15,20,0 194,20,20,0 195,25,20,0 196,30,20,0 197,35,20,0 198,40,20,0 199,45,20,0 200,50,20,0 201,55,20,0 202,60,20,0 203,65,20,0 204,70,20,0 205,75,20,0 206,80,20,0 207,85,20,0 208,90,20,0 209,95,20,0 210,100,20,0 *USER ELEMENT,TYPE=U6,NODES=8,COORDINATES=3,PROPERTIES=1,VARIABLES=6 1,2,3,4,5,6 *Element, type=U6, elset=userel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

Original page 30

31,32,33,54,53,137,138,159,158 32,33,34,55,54,138,139,160,159 33,34,35,56,55,139,140,161,160 34,35,36,57,56,140,141,162,161 35,36,37,58,57,141,142,163,162 36,37,38,59,58,142,143,164,163 37,38,39,60,59,143,144,165,164 38,39,40,61,60,144,145,166,165 39,40,41,62,61,145,146,167,166 40,41,42,63,62,146,147,168,167 41,43,44,65,64,148,149,170,169 42,44,45,66,65,149,150,171,170 43,45,46,67,66,150,151,172,171 44,46,47,68,67,151,152,173,172 45,47,48,69,68,152,153,174,173 46,48,49,70,69,153,154,175,174 47,49,50,71,70,154,155,176,175 48,50,51,72,71,155,156,177,176 49,51,52,73,72,156,157,178,177 50,52,53,74,73,157,158,179,178 51,53,54,75,74,158,159,180,179 52,54,55,76,75,159,160,181,180 53,55,56,77,76,160,161,182,181 54,56,57,78,77,161,162,183,182 55,57,58,79,78,162,163,184,183 56,58,59,80,79,163,164,185,184 57,59,60,81,80,164,165,186,185 58,60,61,82,81,165,166,187,186 59,61,62,83,82,166,167,188,187 60,62,63,84,83,167,168,189,188 61,64,65,86,85,169,170,191,190 62,65,66,87,86,170,171,192,191 63,66,67,88,87,171,172,193,192 64,67,68,89,88,172,173,194,193 65,68,69,90,89,173,174,195,194 66,69,70,91,90,174,175,196,195 67,70,71,92,91,175,176,197,196 68,71,72,93,92,176,177,198,197 69,72,73,94,93,177,178,199,198 70,73,74,95,94,178,179,200,199 71,74,75,96,95,179,180,201,200 72,75,76,97,96,180,181,202,201 73,76,77,98,97,181,182,203,202 74,77,78,99,98,182,183,204,203 75,78,79,100,99,183,184,205,204 76,79,80,101,100,184,185,206,205 77,80,81,102,101,185,186,207,206 78,81,82,103,102,186,187,208,207 79,82,83,104,103,187,188,209,208 80,83,84,105,104,188,189,210,209 *Element, type=M3D4R, elset=ghostel 50001,1,2,23,22 26

Original page 31

50002,2,3,24,23 50003,3,4,25,24 50004,4,5,26,25 50005,5,6,27,26 50006,6,7,28,27 50007,7,8,29,28 50008,8,9,30,29 50009,9,10,31,30 50010,10,11,32,31 50011,11,12,33,32 50012,12,13,34,33 50013,13,14,35,34 50014,14,15,36,35 50015,15,16,37,36 50016,16,17,38,37 50017,17,18,39,38 50018,18,19,40,39 50019,19,20,41,40 50020,20,21,42,41 50021,22,23,44,43 50022,23,24,45,44 50023,24,25,46,45 50024,25,26,47,46 50025,26,27,48,47 50026,27,28,49,48 50027,28,29,50,49 50028,29,30,51,50 50029,30,31,52,51 50030,31,32,53,52 50031,32,33,54,53 50032,33,34,55,54 50033,34,35,56,55 50034,35,36,57,56 50035,36,37,58,57 50036,37,38,59,58 50037,38,39,60,59 50038,39,40,61,60 50039,40,41,62,61 50040,41,42,63,62 50041,43,44,65,64 50042,44,45,66,65 50043,45,46,67,66 50044,46,47,68,67 50045,47,48,69,68 50046,48,49,70,69 50047,49,50,71,70 50048,50,51,72,71 50049,51,52,73,72 50050,52,53,74,73 50051,53,54,75,74 50052,54,55,76,75 50053,55,56,77,76 27

Original page 32

50054,56,57,78,77 50055,57,58,79,78 50056,58,59,80,79 50057,59,60,81,80 50058,60,61,82,81 50059,61,62,83,82 50060,62,63,84,83 50061,64,65,86,85 50062,65,66,87,86 50063,66,67,88,87 50064,67,68,89,88 50065,68,69,90,89 50066,69,70,91,90 50067,70,71,92,91 50068,71,72,93,92 50069,72,73,94,93 50070,73,74,95,94 50071,74,75,96,95 50072,75,76,97,96 50073,76,77,98,97 50074,77,78,99,98 50075,78,79,100,99 50076,79,80,101,100 50077,80,81,102,101 50078,81,82,103,102 50079,82,83,104,103 50080,83,84,105,104 50081,106,107,128,127 50082,107,108,129,128 50083,108,109,130,129 50084,109,110,131,130 50085,110,111,132,131 50086,111,112,133,132 50087,112,113,134,133 50088,113,114,135,134 50089,114,115,136,135 50090,115,116,137,136 50091,116,117,138,137 50092,117,118,139,138 50093,118,119,140,139 50094,119,120,141,140 50095,120,121,142,141 50096,121,122,143,142 50097,122,123,144,143 50098,123,124,145,144 50099,124,125,146,145 50100,125,126,147,146 50101,127,128,149,148 50102,128,129,150,149 50103,129,130,151,150 50104,130,131,152,151 50105,131,132,153,152 28

Original page 33

50106,132,133,154,153 50107,133,134,155,154 50108,134,135,156,155 50109,135,136,157,156 50110,136,137,158,157 50111,137,138,159,158 50112,138,139,160,159 50113,139,140,161,160 50114,140,141,162,161 50115,141,142,163,162 50116,142,143,164,163 50117,143,144,165,164 50118,144,145,166,165 50119,145,146,167,166 50120,146,147,168,167 50121,148,149,170,169 50122,149,150,171,170 50123,150,151,172,171 50124,151,152,173,172 50125,152,153,174,173 50126,153,154,175,174 50127,154,155,176,175 50128,155,156,177,176 50129,156,157,178,177 50130,157,158,179,178 50131,158,159,180,179 50132,159,160,181,180 50133,160,161,182,181 50134,161,162,183,182 50135,162,163,184,183 50136,163,164,185,184 50137,164,165,186,185 50138,165,166,187,186 50139,166,167,188,187 50140,167,168,189,188 50141,169,170,191,190 50142,170,171,192,191 50143,171,172,193,192 50144,172,173,194,193 50145,173,174,195,194 50146,174,175,196,195 50147,175,176,197,196 50148,176,177,198,197 50149,177,178,199,198 50150,178,179,200,199 50151,179,180,201,200 50152,180,181,202,201 50153,181,182,203,202 50154,182,183,204,203 50155,183,184,205,204 50156,184,185,206,205 50157,185,186,207,206 29

Original page 34

50158,186,187,208,207 50159,187,188,209,208 50160,188,189,210,209 *Orientation, name=Ori-1 1.,0.,0.,0.,1.,0. 3, 0. *Membrane Section, elset=ghostel, material=UMAT 1., *Hourglass stiffness 1 *UEL PROPERTY, ELSET=userel 1 *End Instance *Nset, nset=fix,instance=Part-1-1 1,22,43,64,85,106,127,148, 169,190 *Nset, nset=loadup,instance=Part-1-1 126,147,168,189,210 *Nset, nset=loaddn,instance=Part-1-1 21,42,63,84,105 *Nset, nset=allnodes,instance=Part-1-1,generate 1,210,1 *Elset, elset=all,instance=Part-1-1,generate 1,80,1 *End Assembly *Material, name=UMAT *Depvar 8, *User Material, constants=9 .000000001,.000000001,.000000001,0.32,.32,.45,.000000001,.000000001, .000000001 *Boundary fix, 1, 6 allnodes,6,6 *Step, name=Step-1, inc=20000 *Static .01, 1., 1e-05, .01 *Boundary loadup, 3, 3, 6 loaddn, 3, 3,-6 *Restart, write, frequency=0 *Output, field *node output CF,RF,RM,RT,TF,U *element output,directions=YES LE,SDV,E *Output, history *Node Output, nset=loadup RF3, U3 *Node Output, nset=loaddn RF3, U3 *End Step 30

Original page 35

31

Original page 36

REPORT DOCUMENTATION PAGE Form Approved OMB No. 0704–0188 The public reporting burden for this collection of information is estimated to average 1 hour per response, including the time for reviewing instructions, searching existing data sources, gathering and maintaining the data needed, and completing and reviewing the collection of information. Send comments regarding this burden estimate or any other aspect of this collection of information, including suggestions for reducing this burden, to Department of Defense, Washington Headquarters Services, Directorate for Information Operations and Reports (0704-0188), 1215 Jefferson Davis Highway, Suite 1204, Arlington, VA 22202-4302. Respondents should be aware that notwithstanding any other provision of law, no person shall be subject to any penalty for failing to comply with a collection of information if it does not display a currently valid OMB control number. PLEASE DO NOT RETURN YOUR FORM TO THE ABOVE ADDRESS. 1. REPORT DATE (DD-MM-YYYY) 2. REPORT TYPE 01-09-2017 Technical Memorandum 4. TITLE AND SUBTITLE AF-Shell 1.0 User Guide 6. AUTHOR(S) McElroy, Mark W. 7. PERFORMING ORGANIZATION NAME(S) AND ADDRESS(ES) NASA Langley Research Center Hampton, Virginia 23681-2199 9. SPONSORING/MONITORING AGENCY NAME(S) AND ADDRESS(ES) National Aeronautics and Space Administration Washington, DC 20546-0001 12. DISTRIBUTION/AVAILABILITY STATEMENT Unclassified-Unlimited Subject Category 64 Availability: NASA STI Program (757) 864-9658 13. SUPPLEMENTARY NOTES An electronic version can be found at http://ntrs.nasa.gov. 14. ABSTRACT 3. DATES COVERED (From - To) 5a. CONTRACT NUMBER 5b. GRANT NUMBER 5c. PROGRAM ELEMENT NUMBER 5d. PROJECT NUMBER 5e. TASK NUMBER 5f. WORK UNIT NUMBER 432938.11.01.07.43.40.09 8. PERFORMING ORGANIZATION REPORT NUMBER L–20798 10. SPONSOR/MONITOR’S ACRONYM(S) NASA 11. SPONSOR/MONITOR’S REPORT NUMBER(S) NASA/TM–2017–219604 This document serves as a user guide for the AF-Shell 1.0 software, an efficient tool for progressive damage simulation in composite laminates. This guide contains minimal technical material and is meant solely as a guide for a new user to apply AF-Shell 1.0 to laminate damage simulation problems. 15. SUBJECT TERMS composites, delamination, shell element, progressive damage 16. SECURITY CLASSIFICATION OF: 17. LIMITATION OF ABSTRACT a. REPORT b. ABSTRACT c. THIS PAGE U U U UU 18. NUMBER 19a. NAME OF RESPONSIBLE PERSON OF STI Information Desk (help@sti.nasa.gov) PAGES 19b. TELEPHONE NUMBER (Include area code) 37 (757) 864-9658 Standard Form 298 (Rev. 8/98) Prescribed by ANSI Std. Z39.18