S5-1 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation SECTION 5 SPACE STATION TRUSS

S5-2 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation SECTION 5 SPACE STATION TRUSS

S5-3 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation SECTION 5 SPACE STATION TRUSS n Topics covered in this case study: u Introduction to Geometry u Transform Geometry u Organize the model using Groups u Mesh control u Grid points and coordinate systems u Nastran CBAR element u Multiple Subcases

S5-4 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Problem Description u The preliminary design of a Space Station truss segment is complete. The truss assembly carries a number of critical components used for navigation, communication, and heat rejection. This truss segment will be launched on the Space Shuttle and assembled in space to other truss segments. You are asked to analyze the design of the truss segment to ensure that it can survive the launch and on-orbit loading events. n Analysis Objectives u Determine stress levels in the truss members under loading. The maximum stress must be below the yield point of the truss material. CASE STUDY: SPACE STATION TRUSS

S5-5 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Getting started on the Space Station truss analysis: u For the previous case study, no geometry was used. l Nodes were directly created by entering xyz coordinates l Rod elements were created by connecting the nodes l This method works well for simple models u In general modeling situations, the structure is too complex to be modeled using the previous method. The more common method is to create or import the geometry first, then mesh the geometry to generate the finite element model. CASE STUDY: SPACE STATION TRUSS

S5-6 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation X Y Z 9 Y Z X GEOMETRY BUILDING BLOCKS IN PATRAN Point (cyan) n A point is a zero-dimensional CAD entity. It represents a location in space. n MSC.Patran creates points automatically when constructing curves, surfaces, and solids u Points are created at vertices, e.g. surface vertices (corners) It is not always necessary to construct entities starting with their points, e.g. surface from points

S5-7 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation GEOMETRY BUILDING BLOCKS IN PATRAN Curve (yellow) n A curve is a general vector function of the single parametric variable 1. It can have many types of mathematical forms: (X,Y,Z) = function ( ) n A curve has: u Two points, with one at each end A parametric coordinate ( 1 ) whose domain is from 0.0 at P1 (its origin) to 1.0 at P2 n Meshing a curve produces bar elements P2 P1 P( ) Z Y X Z X Y 5 Bar Element

S5-8 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation GEOMETRY BUILDING BLOCKS IN PATRAN Simple Surface (green) n There are two types of surface: u Simple - Green u Complex (general trimmed) - Magenta n A simple surface is a general vector function of the two parametric variables 1, 2 : (X,Y,Z) = function ( 1, 2 ) n A simple surface has: u 3 or 4 bounding edges u A parametric origin and parametric coordinates whose domains are from 0 to 1 n A simple surface with 3 visible edges has a fourth edge that is degenerate 12P2 P1 P4 P3 Z Y X Z X Y P( )

S5-9 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation MESHING A SIMPLE SURFACE n Meshing a simple surface produces 2-D elements Tria mesh Quad mesh

S5-10 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation GEOMETRY BUILDING BLOCKS IN PATRAN Complex Surface (magenta) n A complex or general trimmed surface (magenta) has more than 4 edges and can have interior cutouts u Not defined parametrically ( 1, 2 not used) u It is a trimmed parametric surface Outer boundary Inner boundaries

S5-11 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation MESHING A COMPLEX SURFACE n Meshing a complex surface produces 2-D elements Quad mesh Tria mesh

S5-12 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation P 8 P 7 P 6 P 4 P 3 P 2 P 1 P 5 P GEOMETRY BUILDING BLOCKS IN PATRAN Simple Solid (blue) n There are two types of solid: u Simple - Blue u Complex - White n Simple solid u Vector function of three parametric variables 1, 2, 3 n A simple solid has: u 4 to 6 bounding faces u Parametric origin and coordinates whose domains are from 0 to 1 n A simple solid with 4 to 5 visible faces has some degenerate faces

S5-13 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation MESHING A SIMPLE SOLID n Meshing a simple solid produces solid elements Hex mesh Wedge mesh Tet mesh

S5-14 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation GEOMETRY BUILDING BLOCKS IN PATRAN Complex Solid (white) n Complex Solid u Can have an arbitrary number of faces which define the solid boundary. It is called a boundary representation (B-rep) solid. u Complex solids can be either Patran native B-Rep or parasolid B- Rep

S5-15 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation MESHING A B-REP SOLID n Meshing a B-rep solid produces solid elements Tet mesh

S5-16 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Topological entities are subcomponents of the basic geometry entities TOPOLOGICAL ENTITIES Vertex Edge Face Solid n All topological entities can be cursor selected to perform MSC.PATRAN functions. For example u Solid 1.4 specifies face number 4 of solid 1 which is a surface u Surface 2.3 specifies edge number 3 of surface 2 which is a curve

S5-17 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation CREATING THE SPACE STATION GEOMETRY

S5-18 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a group called bulkheads CREATING A GROUP

S5-19 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Input 7 point locations XYZ CREATING POINTS

S5-20 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create 12 curves for one bulkhead CREATING CURVES

S5-21 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Make 5 copies of the bulkhead geometry X=100 X=120 TRANSFORMING THE CURVES

S5-22 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Delete unnecessary curves and points from front and rear bulkheads. FINISH CREATING THE BULKHEAD GEOMETRY

S5-23 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a new group called longerons CREATING A NEW GROUP

S5-24 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create geometry for the longerons CREATING THE LONGERON GEOMETRY

S5-25 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a new group called diagonals CREATING A NEW GROUP

S5-26 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create geometry for all diagonal members CREATING THE DIAGONAL GEOMETRY

S5-27 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n The truss geometry will next be meshed to generate nodes and elements. n There are two ways to control the element size Mesh seeds or Global edge length MESHING THE GEOMETRY

S5-28 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation CREATING A NEW GROUP Create a new group called FEM

S5-29 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Set up a mesh seed of 12 elements per curve to control the mesh density on the 4 diagonal members in the longest bay SETTING UP MESH SEEDS

S5-30 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Next mesh all the curves with a global edge length of 20 in MESH THE TRUSS GEOMETRY

S5-31 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation RESULTING MESH Coarser global mesh controlled by global edge length Finer local mesh controlled by mesh seeds

S5-32 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Equivalence the model to merge coincident nodes EQUIVALENCE THE MODEL

S5-33 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation COORDINATE SYSTEMS IN PATRAN n Coordinate systems are used in the construction and transformation of geometry

S5-34 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation COORDINATE SYSTEMS IN PATRAN (CONT.) n Coordinate systems are also used to define the direction of loads and boundary conditions

S5-35 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation COORDINATE SYSTEMS IN PATRAN (CONT.) n Coordinate systems can also be used to define the analysis coordinate system of a node

S5-36 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation CREATING COORDINATE SYSTEMS n There are three types of coordinate systems: Rectangular, Cylindrical, and Spherical n There are many ways to create coordinate systems:

S5-37 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n MSC.Nastran Coordinate systems are used to u Define locations of grid points in space u Orient each grid points displacement vector n Coordinate systems in MSC.Nastran: u Basic Coordinate System - Implicitly defined reference rectangular coordinate system (Coordinate System 0). Orientation of this system is defined by the user through specifying the components of grid point locations. u Local Coordinate Systems - User-defined coordinate systems. Each local coordinate system must be related directly or indirectly to the basic coordinate system. The six possible local coordinate systems are: l RectangularCORD1R l RectangularCORD2R l CylindricalCORD1C l CylindricalCORD2C l SphericalCORD1S l SphericalCORD2S MSC.NASTRAN COORDINATE SYSTEMS

S5-38 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n MSC.Nastran Local Coordinate Systems: u The CORD1R, CORD1C, and CORD1S entries define a local coordinate system by referencing the IDs of three existing grid points. u The CORD2R, CORD2C, and CORD2S entries define a local coordinate system by specifying the vector components of three points. u All angular coordinates are input in DEGREES. All rotational displacements associated with these coordinates are output in RADIANS. MSC.NASTRAN COORDINATE SYSTEMS (CONT.)

S5-39 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Rectangular Local Coordinate System (X, Y, Z) Point A = local coordinate system origin Point B = reference point for z axis direction Point C =reference point in the x-z plane Point P = grid point defined in local rectangular system (u x, u y, u z )= displacement components of P in local system MSC.NASTRAN RECTANGULAR COORDINATE SYSTEM

S5-40 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Cylindrical Local Coordinate System (R,, Z) Point A =local coordinate system origin Point B =reference point for z axis direction Point C =reference point in the x-z plane Point P =grid point defined in local cylindrical system (U r, U, U z ) = displacement components of P in local system MSC.NASTRAN CYLINDRICAL COORDINATE SYSTEM

S5-41 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Spherical Local Coordinate System (R,, ) Point A =local coordinate system origin Point B =reference point for z axis direction Point C =reference point in the x-z plane Point P =grid point defined in local spherical system (U r, U, U ) = displacement components of P in local system MSC.NASTRAN SPHERICAL COORDINATE SYSTEM

S5-42 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation MSC.NASTRAN COORDINATE SYSTEM ENTRIES

S5-43 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation DISPLAY OF COORDINATE SYSTEM 0 Coordinate system 0 is always displayed at the lower left-hand corner of the viewport The tick mark represents the origin of the coordinate system 0

S5-44 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation CORD1X VS. CORD2X ENTRIES n By default, coordinate systems are translated into MSC.Nastran CORD2X entries n If Coordinate Frame Coordinates in the Translation Parameters form is set to reference nodes, then CORD1X is translated where applicable

S5-45 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation NESTED COORDINATE SYSTEMS n Creating nested coordinate systems u By default, the nested relationship is lost during translation to MSC.Nastran u If nested coordinate system is desired, the Coordinate Frame Coordinates in the Translation Parameters form needs to be set to reference frame.

S5-46 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a rectangular coordinate system which will be used later to define the direction of the applied load CREATE A RECTANGULAR COORDINATE SYSTEM Point 16 Point 23 Point 17

S5-47 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Grid points are used to specify: u Structural geometry u Degrees of freedom of the structure u Locations of points at which displacements are constrained or loads are applied u Locations where output quantities are to be calculated GRID POINTS

S5-48 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Each grid point is capable of moving in six directions. These are called degrees of freedom (DOF). DOF1 = T 1 = u 1 = translation in direction 1 DOF2 = T 2 = u 2 = translation in direction 2 DOF3 = T 3 = u 3 = translation in direction 3 DOF4 = R 1 = 1 = rotation in direction 1 DOF5 = R 2 = 2 = rotation in direction 2 DOF6 = R 3 = 3 = rotation in direction DEGREES OF FREEDOM

S5-49 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n For each grid point, all six degrees of freedom must be accounted for: u Think in terms of 3D even if the problem is only 1D or 2D. u Any un-used DOF must be constrained DEGREES OF FREEDOM (cont.)

S5-50 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n The NASTRAN GRID entry is show below: FieldContents IDGrid point identification number CPIdentification number of coordinate system in which the location of the grid point is defined (integer 0 or blank; default = basic coordinate system) X1, X2, X3Location of grid point in coordinate system CP (real) CDIdentification number of coordinate system in which displacements, degrees of freedom, constraints, and solution vectors are defined at the grid point (integer 0 or blank; default = basic coordinate system). PSPermanent single-point constraints associated with grid point (any of the digits 1-6 with no embedded blanks) This method of constraining a structure is not recommended. SEIDSuperelement ID THE NASTRAN GRID ENTRY

S5-51 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Each GRID entry refers to two coordinate systems u The coordinate system in field 3 is used to locate the grid point. This is called the positional coordinate system. u The coordinate system in field 7 establishes the grid point displacement coordinate system which defines for the given grid point the directions of displacements, degrees of freedom, constraints, and solution vectors. THE NASTRAN GRID ENTRY (cont.)

S5-52 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation u The grid point displacement coordinate system is also known as the output coordinate system because all grid point results (displacements, grid point forces, etc.) are generated and output in this coordinate system. u The union of all displacement coordinate systems is called the global coordinate system. n The grid point displacement coordinate system: THE GRID POINT DISPLACEMENT COORDINATE SYSTEM

S5-53 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation GRID POINT EXAMPLE Grid points 10 and 20 are located on the aircraft fuselage as show below. The GRID entry uses coordinate system 5 to define the location of the two points and uses coordinate system 0 to define the grid point displacements. Basic coordinate system 0 GRID POINT EXAMPLE

S5-54 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Suppose we are interested in displacements and forces in the fuselage radial and tangential directions. We can accomplish this by changing field 7 of the GRID entries from coordinate system 0 to coordinate system 5. Basic coordinate system 0 GRID POINT EXAMPLE (cont.)

S5-55 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Examples of how the grid point displacement coordinate system is used CONSTRAINTS SPRINGS RIGID ELEMENTS CLEARANCE USING THE GRID POINT DISPLACEMENT COORDINATE SYSTEM

S5-56 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n There are two ways to create grid points in PATRAN: u Directly create the grid point u Mesh the geometry Equivalent to grid point in MSC.Nastran Equivalent to the displacement coordinate system in MSC.Nastran Equivalent to the positional coordinate system in MSC.Nastran CREATING A GRID POINT IN PATRAN

S5-57 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Equivalent Terminology in NASTRAN and PATRAN: NASTRAN AND PATRAN TERMINOLOGY

S5-58 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation EXERCISE Perform Workshop 5 Coordinate Systems in your exercise workbook.

S5-59 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Now back to the case study. Lets create material properties. u Aluminum 7075-T7351 plate and bar stock has been selected for the truss. u The material properties are as follows: l E = 10 x 10 6 psi = 0.3 l Tensile yield strength = 45 ksi CREATING MATERIAL PROPERTIES

S5-60 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a material named al_7075 CREATING MATERIAL PROPERTIES (cont.)

S5-61 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Input material properties CREATING MATERIAL PROPERTIES (cont.)

S5-62 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Considering load paths in the truss assembly u The truss members must carry axial and lateral loads due to the way they are loaded. Shear and bending moment will develop in the members as they are loaded laterally at locations between the truss joints as shown below. We must select an element type that is capable of resisting the shear forces and moments. P M LOAD PATH IN TRUSS

S5-63 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Following are the most commonly used one- dimensional elements in NASTRAN: u RODPin-ended rod (4 DOFs) u BARPrismatic beam (12 DOFs) u BEAMStraight beam with warping (14 DOFs) COMMONLY USED 1-D ELEMENTS

S5-64 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Guidelines on 1-D element selection: u In general, select the simplest element which gives you the correct load path. More complex elements will still do the job, but may give you a lot of unwanted output. u If only an axial load or torsional load is to be transmitted in an element, then the CROD or CONROD element is the best choice. u If shear and moment are to be transmitted in an element, then the CBAR is the easiest element to use. u Use the CBEAM element instead of the CBAR element for the following reasons: l Variable cross-section l The neutral axis and shear center are not coincident l The effect of cross-sectional warping on the torsional stiffness is significant l The mass center of gravity and shear center are not coincident l The effect of taper on the transverse shear stiffness (shear relief) is significant ELEMENT SELECTION

S5-65 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n For this problem we will use the CBAR element due to its ability to transmit shear force and bending moment. n The CBEAM element has additional capabilities which we dont need for this problem. The use of CBEAM will be demonstrated in the next section. ELEMENT SELECTION (cont.)

S5-66 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation u Connected to two grid points u Formulation derived from classical beam theory (plane sections remain plane under deformations) u Includes optional transverse shear flexibility u Neutral axis may be offset from the grid points (internally a rigid link is created) u Principal moment of inertia axis need not coincide with element axis. u Pin flag capability used to represent slotted joints, hinges, ball joints, etc. n General Features of the CBAR Element THE CBAR ELEMENT

S5-67 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n General limitations on CBAR: u Straight, prismatic member (i.e., properties do not vary along the length). u Shear center and neutral axis must coincide (therefore, not recommended for modeling channel or angle sections). u The effect of cross-sectional warping is neglected. n Displacement Components: u Six degrees of freedom at each end. n Force components: u Axial force P u Torque T u Bending moments about two perpendicular directions M 1 and M 2 u Shears in two perpendicular directions V 1 and V 2 THE CBAR ELEMENT (cont.)

S5-68 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n CBAR element entry: THE CBAR ELEMENT (cont.)

S5-69 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n CBAR element entry: THE CBAR ELEMENT (cont.)

S5-70 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n CBAR element entry: THE CBAR ELEMENT (cont.)

S5-71 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n CBAR element coordinate system u Defined by the orientation vector V u Orients input cross-sectional properties u Orients output forces and stresses u Orients pin flags x x z z THE CBAR ELEMENT (cont.)

S5-72 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.)

S5-73 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.)

S5-74 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Following are two examples of when you might define the CBAR element coordinate system orientation vector V with each of the two available options (G0 or X 1, X 2, X 3 ). If you are representing stringers on a fuselage with CBAR elements, your input will be minimized by using the G0 option to define the element coordinate system orientation vector V. Example 1 THE CBAR ELEMENT (cont.)

S5-75 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Example 2 To specify the orientation of the legs of a tripod modeled with CBAR elements as shown, it would be most efficient to use the components of a vector (X 1, X 2, X 3 ) to define the orientation vector V since the orientation of each of the legs is unique. THE CBAR ELEMENT (cont.)

S5-76 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n CBAR Offsets u The ends of the CBAR element can be offset from the Grid Points (GA, GB) by specifying the components of offset vectors W A and W B on the CBAR entry. u The offset vector is treated as a rigid link between the grid point and the end of the element. u The element coordinate system is defined with respect to the offset ends of the bar element. THE CBAR ELEMENT (cont.)

S5-77 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Thin sheet Stiffeners Grid Points n Bar Offset Example THE CBAR ELEMENT (cont.) Centroid of Stiffener Offset

S5-78 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.) n The OFFT field u OFFT is a character string code that describes how the offset and orientation vector components are to be interpreted. u By default (string input is GGG or blank), the offset vectors are measured in the displacement coordinate systems at grid points A and B and the orientation vector is measured in the displacement coordinate system of grid point A. u At user option, the offset vectors can be measured in an offset coordinate system relative to grid points A and B, and the orientation vector can be measured in the basic system as indicated in the following table:

S5-79 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.) n The OFFT field (cont.)

S5-80 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation The user specifies DOFs at either end of the bar element that are to transmit zero force or moment. The pin flags PA and PB are specified in the element coordinate system and defined in fields 2 and 3 of the optional CBAR continuation. n CBAR Pin Flags Example: Pin flag applied to rotational DOF at this end of CBAR creates a hinged joint. THE CBAR ELEMENT (cont.)

S5-81 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n CBAR Element Properties entry: THE CBAR ELEMENT (cont.)

S5-82 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n CBAR Element Properties entry (cont.) THE CBAR ELEMENT (cont.)

S5-83 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n CBAR Element Properties entry (cont.) THE CBAR ELEMENT (cont.)

S5-84 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.)

S5-85 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.)

S5-86 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Shear Factor K THE CBAR ELEMENT (cont.)

S5-87 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.)

S5-88 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Alternative CBAR Element Properties entry: THE CBAR ELEMENT (cont.)

S5-89 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.) n PBARL cross-section types

S5-90 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.) n PBARL cross-section types

S5-91 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.) n PBARL cross-section types

S5-92 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE CBAR ELEMENT (cont.) n PBARL cross-section types

S5-93 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n BAR element internal forces and moments THE CBAR ELEMENT (cont.)

S5-94 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n BAR element internal forces and moments THE CBAR ELEMENT (cont.)

S5-95 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation CBAR CBEND CBEAM Create properties for the CBAR element CREATING ELEMENT PROPERTIES

S5-96 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n For the Space Station truss segment, there are two types of cross-sections: u The longerons and bulkhead members carry large axial and bending loads and are made of heavy I-beam sections. u The diagonal members carry less loads and are made of lighter I-beam sections. CREATING ELEMENT PROPERTIES (cont.)

S5-97 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Heavy Section 6 x 6 T f = in T w = 0.25 in Light Section 6 x 6 T f = in T w = in CREATING ELEMENT PROPERTIES (cont.)

S5-98 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Post the longerons and bulkheads CREATING ELEMENT PROPERTIES (cont.)

S5-99 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a property for the longerons and bulkheads CREATING ELEMENT PROPERTIES (cont.)

S5-100 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Select the material created earlier CREATING ELEMENT PROPERTIES (cont.)

S5-101 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Enter the orientation vector CREATING ELEMENT PROPERTIES (cont.)

S5-102 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Select a section from the Beam Library CREATING ELEMENT PROPERTIES (cont.)

S5-103 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Enter dimensions for the I-beam section and type in a section name CREATING ELEMENT PROPERTIES (cont.)

S5-104 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Click Calculate/Display to compute section properties CREATING ELEMENT PROPERTIES (cont.)

S5-105 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Click OK to accept the cross-section CREATING ELEMENT PROPERTIES (cont.)

S5-106 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Click OK to accept all the physical properties CREATING ELEMENT PROPERTIES (cont.)

S5-107 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Select all curves representing longerons and bulkheads CREATING ELEMENT PROPERTIES (cont.)

S5-108 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Add to the application region box and apply CREATING ELEMENT PROPERTIES (cont.)

S5-109 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n It is important to always verify that the CBAR cross section is oriented in the correct direction. n Since a cross section from the beam library was used, PATRAN now has enough information to display the cross section in 3D space. CREATING ELEMENT PROPERTIES (cont.)

S5-110 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Display - Loads/BC/Elem. Props… CREATING ELEMENT PROPERTIES (cont.)

S5-111 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Change from 1D line display to 3D Display CREATING ELEMENT PROPERTIES (cont.)

S5-112 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Post the FEM group CREATING ELEMENT PROPERTIES (cont.)

S5-113 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation The CBAR elements are now displayed as 3D members CREATING ELEMENT PROPERTIES (cont.)

S5-114 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Zoom in to verify that the I-beams are oriented correctly CREATING ELEMENT PROPERTIES (cont.)

S5-115 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Shade the I-beams Shaded Hidden Line Wireframe CREATING ELEMENT PROPERTIES (cont.)

S5-116 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Post the diagonals CREATING ELEMENT PROPERTIES (cont.)

S5-117 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a second property set for the diagonal members CREATING ELEMENT PROPERTIES (cont.)

S5-118 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n There are two ways to define section properties in PATRAN: 1. Create a cross section using the Beam Library a.Standard shape b.Arbitrary shape 2. Compute the cross sectional properties first and enter them directly into PATRAN. n For the diagonal members, we will use Method 2 to demonstrate how to directly enter cross sectional properties. CREATING ELEMENT PROPERTIES (cont.)

S5-119 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Using equations from a handbook such as Roark, the following cross sectional properties have been calculated: Diagonals 6 x 6 T f = in T w = in A = in 2 I 1 = in 4 I 2 = in 4 J = in 4 CREATING ELEMENT PROPERTIES (cont.)

S5-120 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Select material and enter orientation vector CREATING ELEMENT PROPERTIES (cont.)

S5-121 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Enter A, I1, I2, J CREATING ELEMENT PROPERTIES (cont.)

S5-122 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Enter stress recovery points and click OK to accept properties CREATING ELEMENT PROPERTIES (cont.)

S5-123 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Select curves representing the diagonal members and apply CREATING ELEMENT PROPERTIES (cont.)

S5-124 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Since the cross-sectional properties for the diagonals were entered directly into PATRAN, PATRAN can not provide a 3D display of the I-beam cross section n However, Patran can display an equivalent rectangular section. CREATING ELEMENT PROPERTIES (cont.)

S5-125 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Post the FEM group CREATING ELEMENT PROPERTIES (cont.)

S5-126 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Another way to verify the orientation of cross sections is to display the element Y axis CREATING ELEMENT PROPERTIES (cont.)

S5-127 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n A snap shot of the NASTRAN input file for this problem shows how the connectivity entry, the property entry, and the material entry are linked together. CREATING ELEMENT PROPERTIES (cont.)

S5-128 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Boundary Conditions u The truss segment is tied down at 6 points in the Space Shuttle cargo bay during launch. Once on orbit, it is deployed and attached to neighboring truss segments. u For simplicity, we will only analyze the truss on-orbit configuration. For this configuration, assume the neighboring truss assemblies are massive enough to provide fixed boundaries for the two ends of our truss segment. LOADS AND BOUNDARY CONDITIONS

S5-129 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Applied Loads u There are a number of on-orbit loading events including Space Shuttle docking loads, assembly loads, and EVA (Extravehicular Activity) loads. For this case study, we will focus on the EVA push-off load of 200 lb produced by an astronaut while working on the Space Station. LOADS AND BOUNDARY CONDITIONS

S5-130 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a boundary condition named fixed_ends CREATE BOUNDARY CONDITIONS

S5-131 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Constrain all six degrees of freedom CREATE BOUNDARY CONDITIONS (cont.)

S5-132 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Select two ends of the truss CREATE BOUNDARY CONDITIONS (cont.)

S5-133 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Finish applying the boundary condition CREATE BOUNDARY CONDITIONS (cont.)

S5-134 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n The EVA push-off load can be applied anywhere on the truss segment by an astronaut. Lets apply the 200-lb force on a diagonal member in the longest truss bay. CREATE LOADS

S5-135 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Create a load named EVA_Load CREATE LOADS (cont.)

S5-136 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Apply a 200 lb force normal to the diagonal member using the coordinate system created earlier. CREATE LOADS (cont.)

S5-137 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Select the application region CREATE LOADS (cont.)

S5-138 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Finish creating the load CREATE LOADS (cont.)

S5-139 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation MULTIPLE SUBCASES n A structure may experience different loading scenarios. It may also be constrained differently during different phases of usage. n A good example of this is the space station. u During launch, the space station segment is attached at several hardpoints inside the shuttle cargo bay. The design driver is the severe launch vibration environment. u When in orbit, the space station segment is attached to other segments at its two ends. The launch loads are now absent. Thermal loading, EVA loads, and shuttle docking loads become more important loading events. u All these launch and on-orbit loading events can be applied using the MSC.Nastran Subcases. n Each MSC.Nastran Subcase can contain loads, boundary condition, and output requests.

S5-140 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation MULTIPLE SUBCASES (cont.) n A Subcase is created in MSC.Patran using the Load Case form as shown on the next page. n Use the Assign/prioritize form to add or remove loads and boundary conditions to the load case. n Once the load case is created, it is activated by selecting it in the Subcase Select form.

S5-141 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation CREATING THE SUBCASE

S5-142 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation SELECTING THE SUBCASE

S5-143 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation THE SUBCASE ENTRIES n A sample Nastran input file showing multiple subcases

S5-144 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Perform linear static analysis PERFORM ANALYSIS

S5-145 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Attach the.xdb file ATTACH RESULTS

S5-146 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Plot deformed shape and averaged stresses PLOT RESULTS

S5-147 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation Plot un-averaged stresses PLOT RESULTS

S5-148 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Examine the.f06 file for element stresses Minimum Combined Maximum Combined EXAMINE RESULTS

S5-149 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation n Examine the.f06 file for element forces EXAMINE RESULTS (cont.)

S5-150 NAS120, Section 5, May 2006 Copyright 2006 MSC.Software Corporation EXERCISE Perform Workshop 6 Bridge Truss in your exercise workbook.