S7-1 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation SECTION 7 AIRCRAFT WING RIB

S7-2 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation SECTION 7 AIRCRAFT WING RIB

S7-3 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation SECTION 7 AIRCRAFT WING RIB n Topics covered in this case study: u PATRAN 2D Geometry u Meshing 2D Geometry u Controlling the mesh u NASTRAN Plate and Shell Element Definitions u Loads and Constraints u Post Processing 2D analysis results

S7-4 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Wing Rib n Problem Description u We are tasked with analyzing a wing rib, which is part of the wing structure of a light aircraft. u The wing rib is attached to the front and rear spars and wing skins. u In this particular load case the rib is undergoing shear and we are going to look at the stress around the cutout lightening holes. Front Spar Rear Spar CASE STUDY: AIRCRAFT WING RIB

S7-5 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Wing Rib u We are going to simplify the analysis by assuming that the front spar loads the rib in shear and that the rear spar is effectively built in. u The loading will have been determined by assessment of the air loads and inertia loads. u The geometry is simplified by ignoring the curvature of the rib edges. CASE STUDY: AIRCRAFT WING RIB

S7-6 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation X X Fully Fixed Loading 60 lb f /in t=0.063 E = 10.0 x 10 6 lb/in 2 = 0.33 Centerline R= –T73 Aluminum R=3 R=5 CASE STUDY: AIRCRAFT WING RIB

S7-7 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Analysis Objectives u Determine stress levels in the rib skin under shear loading. The maximum stress must be below the yield stress of the rib material. u Determine the maximum vertical displacement of the rib. The aeroelastics department has specified that the maximum vertical movement of the rib should not exceed inch. CASE STUDY: AIRCRAFT WING RIB

S7-8 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Getting started on the wing rib analysis in PATRAN u Ignore the cutouts initially. u Introduce the idea of Surface Geometry Creation. u Initially we will create a basic geometric surface on which we will later create the mesh. u This type of surface is a Green surface. CASE STUDY: AIRCRAFT WING RIB

S7-9 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Simple PATRAN Surfaces (Green) u A surface is a general vector function of two parametric variables u A surface is characterized by: l A set of bounding curves A parametric origin and two parametric variables ( and ) u A surface can have the same curvature as a curve u Display lines can be turned on to visualize the interior curvature Creating Geometry

S7-10 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n A Simple Surface (Green) has 3 or 4 edges n A simple surface with 3 sides is degenerate n A simple surface can be meshed with either the Iso Mesher (Mapped) or Paver Mesher Simple Surface IsoMesh (mapped mesh) Geometry Elements Creating Geometry (cont.)

S7-11 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n A General Surface (Magenta) may have more than 4 edges and can have inner boundaries (holes) n It is also called a Trimmed Surface n General surfaces can only be meshed with the Paver Mesher n General surfaces can be optionally decomposed into simple surfaces to allow meshing with IsoMesh (Mapped) Mesher General (Trimmed) Surface Paver Mesh Geometry Elements Creating Geometry (cont.)

S7-12 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Create two curves using the xyz method First Curve: Origin 0,0,0 Vector 0,9,0 Creating Geometry (cont.)

S7-13 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Second Curve: Origin 40,0,0 Vector 0,11,0 Creating Geometry (cont.)

S7-14 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Create the surface Creating Geometry (cont.)

S7-15 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Make the bottom half of the rib by Mirroring Surface 1 Creating Geometry (cont.)

S7-16 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Surface 2 is created Creating Geometry (cont.)

S7-17 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation The Mirror reflection Plane was set up using: Coordinate System 0 Direction 2 (the y axis) Coord 0.2 The Offset was 0.0 so the Plane lies on y=0.0 We reversed the new surface so that subsequent meshing keeps consistent orientation Creating Geometry (cont.)

S7-18 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Elements Menu Create the mesh on Surface 1 and 2 MESHING THE GEOMETRY

S7-19 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Use the IsoMesh Meshing Method Elements will be Quad4 type Global Edge Length is 2 inches for the Elements in the mesh MESHING THE GEOMETRY (cont.)

S7-20 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n When meshing surfaces or solids, IsoMesh divides the surfaces or faces into groups of parallel edges called Mesh Paths n Mesh Paths are used by IsoMesh to determine the number of elements per edge for elements along a specific path. The number of elements per edge are based on the following priority: u Mesh Seeds u Adjoining meshed regions that are topologically congruent (surface 1 and 2) u Global Edge Length (set to 2 inches) MESHING THE GEOMETRY (cont.)

S7-21 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation A portion of the mesh is shown: Elements 1 to 120 are on Surface 1 Elements 121 to 240 are on Surface 2 Nodes on the common boundary must be Equivalenced MESHING THE GEOMETRY (cont.)

S7-22 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation After Equivalencing the mesh is now continuous without cracks. The redundant nodes have been deleted. MESHING THE GEOMETRY (cont.)

S7-23 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n So far we have created quad4 elements. The PATRAN quad4 element is the generic term for a family of four-noded elements which include the following: u Thin Shell Elements (will be used here) u Bending Panel Elements u 2D Solid Elements u Membrane Elements u Shear Panel Elements n The specific element type will be specified later when we create the element physical properties. MESHING THE GEOMETRY (cont.)

S7-24 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Creating Material Properties u The Designer has selected aluminum 7075-T73 sheet as the construction material. u The material properties are as follows: l E = 10 x 10 6 psi = 0.33 l Tensile Yield strength = 50 ksi l Shear Ultimate Strength = 65 ksi u The data is input using the Materials Menu as before. CREATING MATERIAL PROPERTIES

S7-25 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Creating Element Physical Properties u For this application we are going to use the Thin Shell Element type. This is a specific application within the generic PATRAN quad4 designation. u Define this specific type by selecting Thin Shell in the Element Properties Menu u Then define the physical Properties relevant to the Thin Shell: l Thickness =.063 in CREATING ELEMENT PROPERTIES

S7-26 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Property Menu Create a 2D Shell property named rib_web Link to Material Input Thickness Apply to Surfaces 1 and 2 CREATING ELEMENT PROPERTIES (cont.)

S7-27 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Question: u Why do we apply the Element Physical Properties to the Surfaces? n Answer: u The Physical Properties are then associated to the Surface – any Elements associated to the Surface via Meshing will automatically be associated to the Physical Properties u If we re-mesh the Surface the new Elements will have Physical Properties associated automatically. CREATING ELEMENT PROPERTIES (cont.)

S7-28 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Two-Dimensional Elements Overview TWO-DIMENSIONAL ELEMENTS See discussions on following pages

S7-29 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n A plate is a structural element with one small dimension and two large dimensions. u A thin plate is one in which the thickness is much less than the next larger dimension (roughly 1/15) u For linear analysis, MSC.Nastran plate elements assume classical engineering assumptions of thin plate behavior: l The deflection of the midsurface is small compared with the thickness l The midsurface remains unstrained (neutral) during bending. (This applies to lateral loads, not in-plane loads.) l The normal to the midsurface remains normal to the midsurface during bending n Two-Dimensional Elements Overview (Cont.) TWO-DIMENSIONAL ELEMENTS (cont.)

S7-30 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation u Plate and shell elements (except CQUADR and CTRIAR) have no stiffness in the normal rotational (drilling) degrees of freedom. n Two-Dimensional Elements Overview (Cont.) No stiffness in the drilling degrees of freedom TWO-DIMENSIONAL ELEMENTS (cont.) u CQUADR and CTRIAR plate elements have stiffness in the drilling degrees of freedom.

S7-31 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation New QUADR/TRIAR Element n A new QUADR/TRIAR element has been added to MSC.Nastran since version 2004 n Similar to the old QUADR/TRIAR element, it has stiffness in the drilling degree of freedom u Drilling loads are transferred correctly n It removes some of the limitations of the old QUADR/TRIAR element u Generates differential stiffness matrix u Supports layered composite u Couples the membrane and bending stiffness u Yields correct results for curved shell models u Supports heat transfer

S7-32 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation New QUADR/TRIAR Element (cont.) u Offset is allowed (shell normal should be turned off, otherwise you will get incorrect results) u Rotational mass is implemented for the drilling DOF (param,coupmass,1) u Supports SOL 200 u Supports consistent load applicationincluding edge loads (PLOAD4) u Unlike the old QUADR, the new QUADR contains all the capabilities of the QUAD4 n A companion alternate QUAD4/TRIA3 is also addedsimilar performances between the v2001 QUAD4/TRIA3 and the alternate QUAD4/TRIA3 n Can switch between different formulations n QUADR/TRIAR do not support nonlinear analysis

S7-33 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation New QUADR/TRIAR Element (cont.) n New system cell QRMETH (370) is available for selection of QUADR/TRIAR and QUAD4/TRIA3 formulations u 0selects the new QUADR/TRIAR formulation (default) u 1selects the old QUADR/TRIAR formulation u 2converts QUADR/TRIAR into QUAD4/TRIA3 using the alternate QUAD4/TRIA3 formulation u 3converts QUADR/TRIAR into QUAD4/TRIA3 using the v2001 QUAD4/TRIA3 formulation u 4selects an alternate QUAD4/TRIA3 formulation (default is the v2001 formulation) u 5converts QUAD4/TRIA3 into QUADR/TRIAR using the new QUADR/TRIAR formulation

S7-34 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation New QUADR/TRIAR Element (cont.) Applying Edge Load n The edge load option is available only for the new QUADR and TRIAR elements using the PLOAD4 entry n SORLSURF or LINE u SURFsurface load acting on the surface of the element (default) u LINEconsistent load acting on the edge of the element PLOAD4SIDEIDP1P2P3P4G1G3 or G4 CIDN1N2N3SORLLDIR

S7-35 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation New QUADR/TRIAR Element (cont.) Applying Edge Load (cont.) n Load direction is defined by either (CID, N1, N2, N3) or LDIR. Fatal message is issued if both are defined n LDIRX, Y, Z, TANG, or NORM u X,Y, Zload acting in the element x, y, or z direction u TANGload acting tangent to the edge based on element connectivity u NORMload acting normal to the edge pointing outward (default)

S7-36 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Example 1Buckling of cylinder using QUADR n Buckling analysis of cylinder simply supported at one end and subject to compressive loads at the other end n Model information Length = 20 Diameter = 20 Thickness = ,000 # load distributed to the edge using an RBE3 n Previously, QUADR cannot be used for this problem since it does not contain the differential stiffness matrix

S7-37 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Example 1Buckling of cylinder using QUADR (cont.) SOL 105 CEND DISP = ALL SPC = 1 $ SUBCASE 1 LABEL = STATIC LOAD LOAD = 1 SPCF = ALL SUBCASE 2 LABEL = EIGENVALUE CALCULATION METHOD = 1 $ BEGIN BULK FORCE $ RBE $ CQUADR CQUADR $ $ plus rest of the model ENDDATA Input File

S7-38 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Example 1Buckling of cylinder using QUADR (cont.) The eigenvalue, = yielding a buckling load of 35,029 (theoretical value = 34,225)

S7-39 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Example 2Membrane Behavior (Inplane Load) n For membrane behavior, the performances of the QUADR element are substantially better than those of the QUAD4especially for non-rectangular shape Normalized Displacements at Tip Element TypeRectangularTrapezoidalParallelogram QUAD QUADR

S7-40 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Example 3Raasch Hook with Vertical Load n Job ran with and without shell normal (SNORM) using the new QUADR. n Old QUADR converges to wrong solution without shell normal Mesh Density Theoretical Results With SNORM Without SNORM 1x x x x x

S7-41 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation u For V2001 l PARAM, K6ROT, 0. is the default for all linear solution sequences l PARAM, K6ROT, 100. is the default in nonlinear solution sequences. l PARAM, SNORM, 20., is the default u For V2004 and later l PARAM, K6ROT, 100. is the default for all solution sequences. l PARAM, SNORM, 20., is the default n Commonly used parameters for plate and shell elements TWO-DIMENSIONAL ELEMENTS

S7-42 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Element connectivity is defined on the NASTRAN CQUAD4 entry, looking at Element 1 in our rib: CQUAD4EIDPIDGRID1GRID2GRID3GRID4 THETA or MCID ZOFFS CQUAD TFLAGT1T2T3T4 CQUAD CQUAD CQUAD CQUAD CQUAD bdf file extract TWO-DIMENSIONAL ELEMENTS (cont.)

S7-43 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation FieldContents EIDElement identification number (integer>0) PIDIdentification number of a PSHELL or PCOMP property entry G1,G2,G3,G4Grid point identification numbers of connection points. (All interior angles of this element must be less than 180.) TWO-DIMENSIONAL ELEMENTS (cont.)

S7-44 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation FieldContents ThetaMaterial property orientation specification. If real or blank, specifies material property orientation angle in degrees. If integer, material x- axis orientation is along projection onto the plane of the x-axis of the specified coordinate system. TFLAGAn integer flag, signifying the meaning of Ti values. TiMembrane thickness of element at grid points G1 through G4. If TFLAG is zero or blank, then Ti are actual user specified thicknesses. If TFLAG is one, then the Ti are fractions relative to the T value of the PSHELL. The continuation entry is optional. If not supplied, then T1 through T4 is set equal to the value of T on the PSHELL data entry. Z OFFS Offset from the surface defined by the grid points to the element reference plane in the element coordinate system. TWO-DIMENSIONAL ELEMENTS (cont.)

S7-45 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Z1Z2MID PSHELLPIDMID1TMID212I/T3MID3TS/TNSM PSHELL n Element physical property is defined on the NASTRAN PSHELL entry $ Elements and Element Properties for region : rib_web PSHELL $ CQUAD CQUAD CQUAD n We will ignore the other terms for now TWO-DIMENSIONAL ELEMENTS (cont.)

S7-46 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation FieldContents PIDProperty identification number(integer >0) MID1Material identification number for membrane behavior (integer > 0 or blank) TPlate or membrane thickness MID2Material identification number for bending behavior (integer > 0 or blank, MID2 = -1 represents plane strain) Note: the default for MID2 is not to include bending stiffness. For most models, MID2 should not be blank 12I/T 3 Normalized bending inertia per unit length (real or blank, default = 1.0). The default value is correct for solid, homogeneous plates. TWO-DIMENSIONAL ELEMENTS (cont.)

S7-47 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation FieldContents MID3Material identification number for transverse shear behavior (integer > 0 or blank) TS/TTransverse shear thickness divided by membrane thickness (default = ). The default value is correct for solid, homogeneous plates. NSMNonstructural mass per unit area (real) Z1, Z2Stress recovery distances for bending (real, default Z1 = -1/2 thickness, Z2 = +1/2 thickness) MID4Material identification number to define coupling between membrane and bending deformation TWO-DIMENSIONAL ELEMENTS (cont.)

S7-48 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation $ Referenced Material Records $ Material Record : aluminum $ Description of Material : Date: 09-Oct-00 Time: 11:49:27 MAT A snap shot of the NASTRAN input file for this problem showing how the connectivity entry, the property entry, and the material entry are linked together ……… CQUAD $ Elements and Element Properties for region : rib_web PSHELL TWO-DIMENSIONAL ELEMENTS (cont.)

S7-49 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Applying Boundary Conditions and Loads u The Rear Spar is assumed fully built in u A vertical load of 60 lbs force per inch is applied at the Front Spar LOADS AND BOUNDARY CONDITIONS

S7-50 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Loads/BCs Create a boundary condition named fixed CREATE BOUNDARY CONDITION

S7-51 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation All six degrees of freedom are fixed CREATE BOUNDARY CONDITION (cont.)

S7-52 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Select the left hand side of the rib CREATE BOUNDARY CONDITION (cont.)

S7-53 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Finish creating the boundary condition CREATE BOUNDARY CONDITION (cont.)

S7-54 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n We can see visually that PATRAN has applied these constraints – but how is this written to a NASTRAN bdf file? n We do this via SPCs. n A single-point constraint (SPC) is a constraint applied to one or more components of motion at selected grid points. n There are two forms of the data input, differing only for convenience: u SPC - not supported by PATRAN u SPC1 - supported by PATRAN SINGLE POINT CONSTRAINTS

S7-55 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation $ Displacement Constraints of Load Set : fixed SPC n Grids 1, 22, 43, …… 153, 154 are selected n DOF are selected n The SPC set is given a SET ID – number 1 in this case. SINGLE POINT CONSTRAINTS (cont.)

S7-56 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation SPC1SIDCG1G2G3G4G5G6 SPC G7G8G9G10G11G12G13G n SPC1 entry format SINGLE POINT CONSTRAINTS (cont.)

S7-57 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n These constraints are selected by the SPC Case Control request n Constraints are only applied if requested n The set of constraints applied may be different for each SUBCASE n BE CAREFUL - if SPC and SPC1 entries are used, they are not applied unless specifically requested in Case Control SINGLE POINT CONSTRAINTS (cont.)

S7-58 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n SPCs are specified in the output coordinate (displacement) system of the grid point at which they are defined. Remember that the grid point output coordinate system is defined in field 7 of the GRID entry n This can be used to advantage – an example will follow in a later section n It is also a major source of error as the constraint will act in the sense of the orientation of the output coordinate system SINGLE POINT CONSTRAINTS (cont.)

S7-59 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Uses of SPCs include: u Support a structure (apply constraints) u Apply symmetric or antisymmetric boundary conditions by restraining the DOFs that must have zero values in order to satisfy symmetry or antisymmetry u Remove degrees of freedom unconnected or weakly coupled to the structure u Remove degrees of freedom not used in the structural analysis (e.g., out-of-plane DOFs for a 2-D analysis) u Apply zero or nonzero enforced displacements to grid points SINGLE POINT CONSTRAINTS (cont.)

S7-60 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Constraints can be defined as: u Permanent - defined on GRID entry (Not supported in PATRAN) u User-selected - done in Case Control with SPC=SID. Defined in the Bulk Data on SPC, SPC1, or SPCD entries u Automatic - PARAM,AUTOSPC,YES n Reaction forces at SPCd grids (termed forces of single-point constraint), may be obtained by including the Case Control request SPCFORCES=ALL SINGLE POINT CONSTRAINTS (cont.)

S7-61 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Create a Distributed Load named force Remember this is a load/unit length DISTRIBUTED LOAD

S7-62 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Input -60 lbs in the f1 direction DISTRIBUTED LOAD (cont.)

S7-63 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Select the application region DISTRIBUTED LOAD (cont.)

S7-64 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Finish creating the load DISTRIBUTED LOAD (cont.)

S7-65 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n We need to be careful with the application of the Distributed Load. u It is a running load, or load per unit length l In our case Total Load = 60 lb f /in x 22in = 1320 lb f u The direction of f1 f2 f3 is parametric, based on the orientation of the edge f2 f1 f3 y z x DISTRIBUTED LOAD (cont.)

S7-66 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n We can see visually that PATRAN has applied these loads – but how is this written to a NASTRAN BDF file? n We do this via FORCE data entries. THE FORCE ENTRY

S7-67 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation $ Distributed Loads of Load Set : force FORCE FORCE FORCE FORCE FORCE FORCE FORCE $ Distributed Loads of Load Set : force FORCE FORCE FORCE FORCE FORCE FORCE FORCE n Grids 21, 42, 63, 84, 105, etc. are selected n A value of 55.0 is applied per grid* (There are 24 grids equally spaced and a total load of 1320 lb f ) n A vector of is used n The FORCE set is given a SET ID – number 1 in this case. * Rounding causes in the translator THE FORCE ENTRY (cont.)

S7-68 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation FORCESIDGIDCIDFX1Y1Z1 FORCE n The FORCE can be applied in any Coordinate System – here we use default 0 n Beware as the Force Magnitude is multiplied by the vector resultant n FORCE entry format THE FORCE ENTRY (cont.)

S7-69 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation $ Distributed Loads of Load Set : force FORCE FORCE FORCE FORCE FORCE FORCE FORCE etc... $ Distributed Loads of Load Set : force FORCE FORCE FORCE FORCE FORCE FORCE FORCE etc... n The application of the FORCE to the grids can appear confusing as data is repeated – this is a valid way for NASTRAN to have a loading distribution on QUAD4 elements which is kinematically equivalent to a constant load Uniform 10 THE FORCE ENTRY (cont.)

S7-70 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n We have now completed the pre-processing phase of the analysis process. The next step is to send it to NASTRAN to perform matrix analysis on the model. Solver PERFORM ANALYSIS

S7-71 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Select linear static analysis PERFORM ANALYSIS (cont.)

S7-72 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Status window reports job progress PERFORM ANALYSIS (cont.)

S7-73 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n After NASTRAN completes the analysis, we are now ready to read the results back into PATRAN. Solver ACCESS ANALYSIS RESULTS

S7-74 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Read in the xdb file ACCESS ANALYSIS RESULTS (cont.)

S7-75 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Post Processing the Results u Examine the maximum vertical deflection. The allowable deflection is inch. u Examine the rib tensile stresses and shear stresses. l Must be below 50 ksi in tension (material yield strength) l Must be below 65 ksi in shear (material ultimate strength – requires a 1.5 load factor) POST PROCESS RESULTS

S7-76 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Plot the deformation Max y disp = in < in POST PROCESS RESULTS (CONT.)

S7-77 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Plot the averaged x direct stresses Max x stress = 18,900 lbs/in 2 POST PROCESS RESULTS (CONT.)

S7-78 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Plot the averaged xy stresses Max absolute xy stress = 1,930 lbs/in 2 POST PROCESS RESULTS (CONT.)

S7-79 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Plot the averaged Von- Mises stresses Max Von Mises stress = 17,100 lbs/in 2 POST PROCESS RESULTS (CONT.)

S7-80 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation POST PROCESS RESULTS (CONT.) n 2-D element stresses are computed at Z1 and Z2 positions. n By default stresses at the Z2 position are selected for display in Patran. n For this rib problem, set the position to Z1 and examine the stresses. n The Z1 results are identical to the Z2 results since there is no bending in this problem.

S7-81 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Analysis Summary: u Maximum deflection of inch is below the inch requirement. u Maximum axial stresses: l Tensile Stress = 18,900 psi at upper rear spar l Compressive Stress = -18,900 psi at lower rear spar l Margin of safety >2 u Maximum Shear Stress: l Shear Stress = 1,930 psi in center of panel in negative sense l Margin of safety >2 u Overall check Von Mises: l Max Von Mises = 17,100 psi – appears to be dominated by x direction direct stresses POST PROCESS RESULTS (CONT.)

S7-82 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Manual Check: u Maximum axial stresses at Rear Spar: l Equiv bending section I = b*d^3/12 =.063*18.0^3/12 = in^4 l Moment at Rear Spar = 1320*40 lb f in = lb f in l Stress at Rear Spar = M*y/I = 52800*9.0/ = 15,520 psi u Maximum Shear Stress: l Median Cross Sectional Area =.063*20 = 1.26 in^2 l Shear Stress = 1320/1.26 = 1047 psi POST PROCESS RESULTS (CONT.)

S7-83 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n By default, PATRAN averages the stresses at a node from neighboring elements and plots this average stress value. n By switching off the averaging option, the true maximum stresses in the quad4 elements are displayed. n We will use this to check stress gradients in the top rear spar attachment point. POST PROCESS RESULTS (CONT.)

S7-84 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Standard fringe from QuickPlot Element Averaging OFF in Fringe n The Element at the top rear spar attachment point is seeing a steep stress gradient. We would need to take care when drawing conclusions about local stress levels here. n Otherwise the gradients are very similar. POST PROCESS RESULTS (CONT.)

S7-85 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Full Rib Idealization u We now decide to do a more realistic analysis of the rib, which includes the cutouts. RIB WITH CUTOUTS

S7-86 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Geometry Menu Create the four points to define top half of rib RIB WITH CUTOUTS (cont.)

S7-87 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Create 4 Curves using the Points RIB WITH CUTOUTS (cont.)

S7-88 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Build a point at the center of the first cutout. Create a 180 deg curve using the 2D ArcAngles method RIB WITH CUTOUTS (cont.)

S7-89 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Add the other curves RIB WITH CUTOUTS (cont.)

S7-90 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Break the centerline curve 4 at the intersection of the first cutout RIB WITH CUTOUTS (cont.)

S7-91 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Curve 9 created and old curves deleted Repeat this for all the segments along the centerline RIB WITH CUTOUTS (cont.)

S7-92 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Chain all the segments around the rib half to form a single curve – curve 20 RIB WITH CUTOUTS (cont.)

S7-93 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Create a Trimmed Surface by setting curve 20 as the Outer Loop RIB WITH CUTOUTS (cont.)

S7-94 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation The Trimmed Surface is drawn in Magenta and the hatching is at an angle as we have visualization lines switched on We now mirror this surface as before RIB WITH CUTOUTS (cont.)

S7-95 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Elements Menu Create the mesh on Surface 1 and 2 RIB WITH CUTOUTS (cont.)

S7-96 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Use the Paver Meshing Method Elements will be Quad4 type Global Edge Length is 2 inches for the Elements in the mesh RIB WITH CUTOUTS (cont.)

S7-97 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Global Edge Length of 2 dominates wherever possible RIB WITH CUTOUTS (cont.)

S7-98 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Paver Mesher u Used with all surfaces l trimmed (magenta) l simple (green) u When meshing surfaces, the Paver starts at the boundary and gradually moves toward the interior n To Add More Control u Mesh seeding controls element generation along seeded curves u Paver recognizes hard points and curves added to a surface by association RIB WITH CUTOUTS (cont.)

S7-99 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Rib Cutout Model u Global Edge Length is good for areas away from stress concentrations u Mesh Density is poor around holes and in ligaments (thin regions of material) n To Add More Control u Mesh Seed around the holes, say 16 elements per 180 degrees RIB WITH CUTOUTS (cont.)

S7-100 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n To Rebuild a Mesh u Either - create the mesh again and you will be prompted to delete the old mesh u Or - Use Delete Mesh n To Change or Add Mesh Seed u You will need to delete the existing Mesh RIB WITH CUTOUTS (cont.)

S7-101 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Here we delete the mesh and Mesh Seed all 6 edges RIB WITH CUTOUTS (cont.)

S7-102 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation The mesh is improved, but the ligaments are still poor RIB WITH CUTOUTS (cont.)

S7-103 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation The edges in the ligament region are seeded RIB WITH CUTOUTS (cont.)

S7-104 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation This improves the mesh, but we wish for a more regular array of elements around the cutouts RIB WITH CUTOUTS (cont.)

S7-105 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation We go back to Geometry to create three new local coordinate systems Using View Vector is simple in this case RIB WITH CUTOUTS (cont.)

S7-106 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation We now translate the edge by 1 inch in the radial direction using a Curvilinear Reference Frame We repeat create a set of concentric curves RIB WITH CUTOUTS (cont.)

S7-107 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation The curves are now associated to their respective surfaces The association is shown by a triangular marker RIB WITH CUTOUTS (cont.)

S7-108 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation The curves are seeded and then the surfaces re-meshed RIB WITH CUTOUTS (cont.)

S7-109 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation The final mesh is accepted with: a global edge length 1.7 further concentric lines associated extra lines associated Extra Lines RIB WITH CUTOUTS (cont.)

S7-110 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n For Paver Mesher the number of elements per edge are based on the following priority: u Mesh Seeds u Adjoining meshed regions that are topologically congruent u Even number of elements along the boundary u Global edge length THE PAVER MESHER

S7-111 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Comparison of Paver and IsoMesher THE PAVER MESHER (cont.)

S7-112 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n The Rib is now completed as before u Create Material Property u Create Physical Property u Apply Loads and Boundary Conditions u Equivalence u Analyze RIB WITH CUTOUTS

S7-113 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Plot the deformation Max y disp = in > in PLOT RESULTS

S7-114 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Plot the averaged x direct stresses Max x stress = 20,300 lbs/in 2 PLOT RESULTS (cont.)

S7-115 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Plot the averaged xy stresses Max absolute xy stress = 8,710 lbs/in 2 PLOT RESULTS (cont.)

S7-116 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Plot the averaged Von Mises stress Also plot the un-averaged Von Mises stress Compare the average stress with un-averaged stress. These two values should be close to each other for a good mesh. Max Von Mises stress = 21,300 lbs/in 2 PLOT RESULTS (cont.)

S7-117 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Analysis Summary: u Maximum deflection of inch is above the inch requirement. If we include Rib Caps and Spar Attachment Flange then we would expect the deflection to be within limits. u Maximum axial stresses: l Tensile Stress = 20,300 psi at upper rear spar l Compressive Stress = -20,300 psi at lower rear spar l Margin of safety >2 u Maximum Shear Stress: l Shear Stress = 8,710 psi in center of panel in negative sense l Margin of safety >2 u Overall check Von Mises: l Max Von Mises = 21,300 psi – appears to be dominated by x direction direct stresses ANALYSIS SUMMARY

S7-118 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Manual Check: u Maximum axial stresses at Rear Spar (as before): l Equiv bending section I = b*d^3/12 =.063* 18.0^3/12 = in^4 l Moment at Rear Spar = 1320*40 lb f in = lb f in l Stress at Rear Spar = M*y/I = 52800*9.0/ = 15,520 psi u Maximum Shear Stress – reduced area l Median Cross Sectional Area =.063*12 = in^2 l Shear Stress = 1320/0.756 = 1746 psi ANALYSIS SUMMARY (cont.)

S7-119 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation We have a poorly shaped element in the mesh. By setting stress averaging off we can see the influence of that element. ANALYSIS SUMMARY (cont.)

S7-120 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation CHECKING ELEMENT DISTORTION IN MSC.PATRAN n MSC.Nastran performs a number of element distortion checks. For a complete description of element distortion checks performed by MSC.Nastran, please refer to the MSC.Nastran Linear Static Analysis Users Guide. n It is good practice to check the quality of the finite elements before running the MSC.Nastran job. n MSC.Patran has a number of element distortion checks shown on the next page.

S7-121 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation CHECKING ELEMENT DISTORTION IN MSC.PATRAN (cont.)

S7-122 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation CHECKING ELEMENT DISTORTION IN MSC.PATRAN (cont.) n Within each element type, specific element distortion tests can be made and the results are displayed in a fringe plot. n For example, verification tests for the Quad element include Aspect Ratio, Warp, Skew, and Taper.

S7-123 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation WING RIB ELEMENT DISTORTION PLOT n The quad element aspect ratio plot is shown below:

S7-124 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation EXERCISE Perform Workshop 8A Tension Coupon in your exercise workbook. Perform Workshop 8B Tension Coupon in your exercise workbook. Perform Workshop 8C Tension Coupon in your exercise workbook. Perform Workshop 8D Tension Coupon in your exercise workbook.

S7-125 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation ANALYSIS OF COMPOSITE MATERIALS n Following slides provide a brief introduction to the analysis of composites materials. n Please attend the NAS113 Analysis of Composite Materials with MSC.Nastran course for a more comprehensive treatment of composite analysis.

S7-126 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Typically a ply is a flat group of fibers imbedded in a matrix. n The matrix is usually an isotropic material that holds the fibers together. n In a ply called a tape, the fibers are unidirectional. n In a ply called a cloth, the fibers are woven at 0 and 90 degree directions. PLY DEFINITION

S7-127 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation n Fiber: u Unidirectional in tape u Direction is the 1 axis of the ply coordinate system n Matrix: u Glue that holds fibers together u Matrix direction is the 2 axis u 90 degrees to the 1 axis n Material properties are: u 2D orthotropic material in Patran u MAT8 in Nastran TAPE PLIES

S7-128 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation MAT8 BULK DATA ENTRY n Defines the ply orthotropic properties. u Elastic properties are E1, E2, NU12, G12, G1Z, G2Z. u Allowables are Xt, Xc, Yt, Yc, S. u Use STRN=1.0 if allowables are in units of strain. u F12 is for the Tsai-Wu failure theorem. u Thermal coefficients of expansion are A1 and A2. u The MAT8 TREF reference temperature is not used since it is overridden by the PCOMP TREF. u Density is RHO. u The MAT8 GE structural damping is not used since it is overridden by the PCOMP GE. n The example below is typical for a graphite/epoxy tape MAT8MIDE1E2NU12G12G1ZG2ZRHO MAT A1A2TREFXtXcYtYcS bdf file extract GEF12STRN mat8, 1, 20.+6, 2.+6, 0.35, 1.0+6, 1.0+6, 1.0+6, 1.3-4,+ +, , 4.5-6,, 1.3+5, 1.2+5, 1.1+4, 1.2+4,

S7-129 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation PATRAN 2D ORTHOTROPIC Materials: Create/ 2d Orthotropic/ Manual Input Material Name Input Properties Linear Elastic Apply Input Properties Failure Apply Note that Linear Elastic and Failure properties must be input separately with an Apply between and after

S7-130 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation COMPOSITE MATERIAL n Stack of plies n Each ply has a different direction, material, and thickness n Composite properties are calculated in the material coordinate system (Xm, Ym, Zm) n Zm is the same as the element Z axis (Ze) u Right hand rule of grid ordering, G1,G2,G3,G4 n Xm is in the direction of the 0 degree ply n Positive angles are defined by right hand rule around Zm

S7-131 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation PCOMP BULK DATA ENTRY n Defines the composite layup PCOMPPIDZ0NSMSBFTTREFGELAM PCOMP HILL0.0 MID1T1THETA1SOUT1MID2T2THETA2SOUT YES YES MID3T3THETA3SOUT3etc n Z0 is composite offset. u Use default = -(composite thickness)/2 n NSM is nonstructural mass n SB is allowable interlaminar shear stress u Put as Bonding Shear Stress in Patran 2D Orthotropic Material u Required for failure indices n FT is the ply failure theorem u Required for failure indices n TREF is reference temperature u Overrides TREFs on ply MAT8s n GE is element damping u Overrides GE on ply MAT8s n LAM is layup options n MIDi is ply material ID u MAT8 ID n Ti is ply thickness n THETAi is ply angle n SOUTi is data recovery option

S7-132 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation PCOMP BULK DATA ENTRY (cont.) n The example composite below is an 8 ply layup, symmetric about its centerline, with an equal number of plies in each of the 0, +45, 90 degree directions..bdf file extract PCOMP, 1,,, 5000., HILL, 1,.0054, 0., YES, 1,.0054, 45., YES, 1,.0054, -45., YES, 1,.0054, 90., YES, 1,.0054, -45., YES, 1,.0054, 45., YES, 1,.0054, 0., YES

S7-133 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Materials: Create/ Composite/ Laminate To create a ply, click on a ply material in Existing Materials. Repeat for each of the plies Thickness for all layers: Click on first cell in Orientation column Text Entry Mode = Overwrite Orientations: 0 45 – – Load Text Into Spreadsheet Apply PATRAN COMPOSITE

S7-134 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation CQUAD4 BULK DATA ENTRY n Defines the composite plate. n Material coordinate system can be defined one of two ways: u MCID – (integer) - ID of a user defined coordinate system whos X-axis is projected onto the element to define the elements material coordinate systems X- axis. This along with the Z-axis of the element coordinate system defines the material coordinate system. u THETA – (real) - an angle between the G1G2 vector of the element and the X-axis of the material coordinate system. The positive sense of this angle is the right hand rule direction around the elements Z-axis CQUAD4EIDPIDG1G2G3G4THETA or MCID ZOFFS CQUAD CQUAD4, 1, 1, 1, 2, 5, 4, 99 CQUAD4, 1, 1, 1, 2, 5, 4, 25.0

S7-135 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation PATRAN COMPOSITE PROPERTIES Properties: Create/ 2D/ Shell Property Set Name Option: Laminate Input Properties Click on Mat Prop Name Icon to select the material Click on coord. sys. for projection to material coord. sys. OK Select elements Apply

S7-136 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation PATRAN MATERIAL COORD. Z-AXIS Elements: Verify/ Element/ Normals Draw Normal Vectors Apply

S7-137 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation PATRAN MATERIAL COORD. X-AXIS Properties: Show Material Orientation Apply

S7-138 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation GRID GRID GRID GRID GRID GRID GRID GRID GRID $ SPC1,1,1235,1 SPC1,1,135,2,3 $ FORCE FORCE FORCE FORCE FORCE FORCE FORCE FORCE FORCE $ CORD2R, 99,, 0., 0., 0., 0., 0., 1., 0., 1., 0. ENDDATA SOL 101 CEND TITLE = Composite Workshop Chapter 2 - Sample Composite Input SPC = 1 LOAD = 1 DISP = ALL STRESS =ALL $ BEGIN BULK PARAM, POST, -1 $ PCOMP, 1,,, 5000., HILL, 1,.0054, 0., YES, 1,.0054, 45., YES, 1,.0054, -45., YES, 1,.0054, 90., YES, 1,.0054, -45., YES, 1,.0054, 45., YES, 1,.0054, 0., YES MAT8, 1, 2.+7, 2.+6,.35, 1.+6, 1.+6, 1.+6,,,, , , , , $ CQUAD CQUAD CQUAD CQUAD $ NASTRAN INPUT FILE.dat file extract n The single ply per line format on PCOMP continuation fields allows easier cutting and pasting of plies

S7-139 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation S T R E S S E S I N L A Y E R E D C O M P O S I T E E L E M E N T S ( Q U A D 4 ) ELEMENT PLY STRESSES IN FIBER AND MATRIX DIRECTIONS INTER-LAMINAR STRESSES PRINCIPAL STRESSES (ZERO SHEAR) MAX ID ID NORMAL-1 NORMAL-2 SHEAR-12 SHEAR XZ-MAT SHEAR YZ-MAT ANGLE MAJOR MINOR SHEAR E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E E+04 NASTRAN PLY STRESS OUTPUT n Printed in the f06 file if STRESS=ALL or STRAIN=ALL Case Control Commands are used..f06 file extract

S7-140 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation PATRAN PLY OUTPUT REQUEST Analysis: Analyze/ Entire Model/ Full Run Translation Parameters/ OP2 Subcases/ Create Output Requests/ Advanced/ Element Stress Ply Stresses OK Apply

S7-141 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation PATRAN PLY STRESS RESULTS

S7-142 NAS120, Section 7, May 2006 Copyright 2006 MSC.Software Corporation Perform Workshop 8E Composite Tension Coupon in your exercise workbook. Perform Workshop 16 Stiffened Plate in your exercise workbook. EXERCISE