S10-1PAT301, Section 10, October 2003 SECTION 10 ELEMENT PROPERTIES

S10-2PAT301, Section 10, October 2003

S10-3PAT301, Section 10, October 2003 ELEMENT PROPERTY DEFINITION n Element Property form is used to specify: u Element type and formulation l MSC.Nastran lumped point mass, CONM2 l ABAQUS solid element standard formulation, C3D8 u Cross-section properties l 0-D : lumped mass, mass matrix l 1-D : A, I yy, I zz, J l 2-D : thickness, plate offset, material orientation l 3-D : material, integration scheme u Region of application l Geometry l F EM l Properties associated with geometry will be re-applied to new mesh after re- meshing

S10-4PAT301, Section 10, October 2003 ELEMENT PROPERTY DEFINITION (Cont) n Element properties may vary in space as described by fields, e.g. thickness = 0.10*Y *X**2 n Property forms are specific to application code, element type, and configuration

S10-5PAT301, Section 10, October 2003 ELEMENT PROPERTY CREATION n First, if necessary select the desired analysis code in Preferences/Analysis n Select the dimensionality of the element u 0-D (Mass, Spring) u 1-D (Beam) u 2-D (Shell, 2D Solid) u 3-D (Solid) n Specify a name (maximum 31 characters) n Select element Options n Enter properties in the Input Properties form n Use Select Members list box and select menu to choose between Geometry or FEM entities Geometric entities FEM entities

S10-6PAT301, Section 10, October 2003 n Data templates are finite element solver, element type, and configuration specific n Materials may be selected by clicking the Material Prop Name icon, then selecting from the choices in Select Existing Material window PHYSICAL PROPERTY INPUT FORM

S10-7PAT301, Section 10, October 2003 PHYSICAL PROPERTY INPUT FORM (Cont.) n Brackets around a data item name denote that the specification of the item is optional, e.g. [Non-structural Mass] indicates Patran will process data without non- structural mass

S10-8PAT301, Section 10, October 2003 BEAM ELEMENT PROPERTIES n Bar/Beam elements require a vector to define the orientation of the cross-section (the local element coordinate system) u In MSC.Patran, this vector is defined using either the Patran global (X,Y,Z) or a local coordinate system n To recover bending stress, stress recovery points must be defined relative to the element coordinate system u Called C,D,E,F for MSC.Nastran u Used to determine c in the classical equation stress= Mc/I n The moments of Inertia (I1 and I2) and the torsional constant (J) are defined with respect to the local element coordinate system (J is not the polar moment of inertia) n MSC.Nastran and ABAQUS beam cross-section orientations are explained in the figure on the next page

S10-9PAT301, Section 10, October 2003 BEAM ELEMENT ORIENTATION

S10-10PAT301, Section 10, October 2003 BEAM LIBRARY n Optionally, beam sections can be created, viewed and stored in the database n A library of standard shapes is available to automatically calculate A, I11, I22, and J n Cross-section properties can be calculated for arbitrary shapes n Beam Library is available from the Input Properties form of Element Properties, or under Tools, Beam Library n Beam sections assigned to elements can be graphically viewed on each element

S10-11PAT301, Section 10, October 2003 MESHING WITH BAR ELEMENTS EXAMPLE n Construct a 64 x 64 stiffened plate n Mesh the surfaces with quad4 elements n Mesh the edges of the surfaces with Bar2 elements n Create a beam property using the tee section defined previously X Y Z

S10-12PAT301, Section 10, October 2003 BEAM PROPERTY SPECIFICATION EXAMPLE MSC.Nastran n Define a material property n Input the physical properties n Apply the physical properties to the model (i.e. Edge 2 of Surface 6) Beam [Section Name] Material Aluminum is selected Vector specifying beam (cross-section) orientation; Beam is offset –1.5 in the Patran global Y direction; Member pinned at one end (local coordinate system) Select here to use Beam Library to calculate A, I11, I22 and J. Otherwise, input A, I11, I22 and J manually.

S10-13PAT301, Section 10, October 2003 DISPLAYING BEAM SECTIONS n Beam sections and offsets can be displayed by using Display/Load/BC/Elem. Props…and choosing, for example, 3D:FullSpan+Offsets n The actual cross-section and orientation is displayed as shown u Only if the beams cross- section is defined with Beam Library n If cross-section specified with Area, I 1,1, etc. use …+Equiv. I or A

S10-14PAT301, Section 10, October 2003 n Import the following Geometry. u File/Import/Neutral. u Select four_surfs.out. u Apply. u Turn on surface labels by clicking on, then CASE STUDY: MESHING WITH QUADS AND BARS

S10-15PAT301, Section 10, October 2003 n IsoMesh the surfaces u Select the Finite Elements Applications button. u Set Action/Object/Type to Create/Mesh/Surface. u Select the IsoMesh Mesher. u Select Surface 1:4 for Surface List. u Enter 4.0 for Global Edge Length. u Apply. n Shrink the surfaces so the edges are more visible. u Click on Display in the main menu u Select Geometry… u Use Geometric Shrink slide bar to shrink the display of the surfaces slightly CASE STUDY: MESHING WITH QUADS AND BARS

S10-16PAT301, Section 10, October 2003 n The model should now appear as follows CASE STUDY: MESHING WITH QUADS AND BARS

S10-17PAT301, Section 10, October 2003 n Mesh surface edges with Bar2 Topology. u Select the Finite Elements Applications button. u Set Action/Object/Type to Create/Mesh/Curve. u Select Bar2 Topology. u Select edges Surface for Curve List. u Enter 0.1 for Global Edge Length. u Apply. CASE STUDY: MESHING WITH QUADS AND BARS

S10-18PAT301, Section 10, October 2003 n Create a material for the T shaped cross-section. u Select Material Applications button. u Set Action/Object/Method to Create/Isotropic/Manual Input. u Enter Steel for Material Name. u Click Input Properties. u Enter desired values for Elastic Modulus and Poisson ratio. u OK. u Apply. CASE STUDY: MESHING WITH QUADS AND BARS

S10-19PAT301, Section 10, October 2003 n Create the beam element properties for the Bar2 topology. u Select the Properties Applications button. u Set Action/Object/Type to Create/1D/Beam. u Enter Tee for Property Set Name. u Click Input Properties… CASE STUDY: MESHING WITH QUADS AND BARS

S10-20PAT301, Section 10, October 2003 n Enter the beam properties. u Select Steel from Mat Prop Name for Material Name. u Click the ICL Beam Library icon u Enter Tee_cs under New Section Name, and click the T button. u Enter 3 for Width and Height. u Enter 0.5 for t1 and t2. u Click on Calculate/Display. CASE STUDY: MESHING WITH QUADS AND BARS

S10-21PAT301, Section 10, October 2003 n The following window will appear. u Click OK in the Beam Library window. CASE STUDY: MESHING WITH QUADS AND BARS

S10-22PAT301, Section 10, October 2003 n Specify the cross-section bar orientation. u Under Input Properties…Enter for Bar Orientation. u Enter for Node 1. u Enter for Node 2. u OK. CASE STUDY: MESHING WITH QUADS AND BARS

S10-23PAT301, Section 10, October 2003 n Display the beam cross-section u Click on Display in the main menu, and select Load/BC/Elem. Props. u Select 3D:FullSpan+Offsets for Beam Display. u Apply. u Shade the model. CASE STUDY: MESHING WITH QUADS AND BARS

S10-24PAT301, Section 10, October 2003 n The model should now appear as follows CASE STUDY: MESHING WITH QUADS AND BARS

S10-25PAT301, Section 10, October 2003 PROPERTY SPECIFICATION USING FIELDS n Variable Thickness Plate (t = * X * Y3) n Create the field n Apply the field to the plate as input to the property thickness n Show scalar plot of the resulting thickness

S10-26PAT301, Section 10, October 2003 MASS PROPERTIES n Mass Properties application is available under Tools for 2D and 3D calculations n Can be calculated for selected groups, and can include Geometry, FEM or both n Output includes mass, volume, center of gravity, principal inertias at the center of gravity, the radii of gyration corresponding to the principal inertias at the center of gravity n A user specific coordinate frame may be used n Data can optionally be output to a text report file

S10-27PAT301, Section 10, October 2003 EXERCISE Perform Workshop 12 Cantilevered Beam Using 1D or 2D Elements, and Analysis in your exercise workbook

S10-28PAT301, Section 10, October 2003