Module 5 Beam Modeling 5 Beam Modeling They

Module 5 Beam Modeling

5. Beam Modeling • They are computationally more efficient than solids and shells and are heavily used in several industries: – Building construction – Bridges and roadways – People movers (trams, railcars, buses) – Etc. INTRODUCTION TO ANSYS 6. 0 - Part 2 • Beam elements are line elements used to create a onedimensional idealization of a 3 -D structure. Training Manual October 30, 2001 Inventory #001571 5 -2

. . . Beam Modeling Training Manual A. Beam Properties B. Beam Meshing C. Loading, Solution, Results D. Workshop INTRODUCTION TO ANSYS 6. 0 - Part 2 • In this chapter, we will present a brief introduction to beam modeling via the following topics: October 30, 2001 Inventory #001571 5 -3

Beam Modeling A. Beam Properties Training Manual • Then define the following beam properties: – Element type – Cross section – Material INTRODUCTION TO ANSYS 6. 0 - Part 2 • The first step in beam modeling, as with any analysis, is to create the geometry — usually just a framework of keypoints and lines. October 30, 2001 Inventory #001571 5 -4

Beam Modeling . . . Beam Properties Training Manual • Choose one of the following types: – BEAM 188 — 3 -D, linear (2 -node) – BEAM 189 — 3 -D, quadratic (3 -node) • ANSYS has many other beam elements, but BEAM 188 & 189 are generally recommended. – Applicable to most beam structures – Support linear as well as nonlinear analyses, including plasticity, large deformation, and nonlinear collapse – Ability to include multiple materials to simulate layered materials, composites, reinforced sections, etc. – Ability to create “user defined” section geometry – Easy to use, both in preprocessing and postprocessing phases INTRODUCTION TO ANSYS 6. 0 - Part 2 Element Type October 30, 2001 Inventory #001571 5 -5

Beam Modeling . . . Beam Properties • To completely define a BEAM 188 or 189 element, you also need to specify its cross section properties. • The Beam. Tool provides a convenient way to do this. – Preprocessor > Sections > Common Sectns. . . – Select the desired shape, then enter its dimensions. – Press the Preview button to view the shape, then OK to accept it. – If there are multiple cross sections, specify a different section ID number (and an optional name) for each. INTRODUCTION TO ANSYS 6. 0 - Part 2 Cross Section Training Manual October 30, 2001 Inventory #001571 5 -6

Beam Modeling . . . Beam Properties Training Manual A sample preview (SECPLOT) of an I-beam cross section is shown below. • In addition to the predefined cross-section shapes, ANSYS allows you to create your own, “user-defined” shape by building a 2 -D solid model. • You can save user-defined sections as well as standard sections with the desired dimensions in a section library for later use. • See Chapter 15 of the ANSYS Structural Analysis Guide for more information. INTRODUCTION TO ANSYS 6. 0 - Part 2 • October 30, 2001 Inventory #001571 5 -7

Beam Modeling . . . Beam Properties Training Manual • Both linear and nonlinear material properties are allowed. • After all beam properties are defined, the next step is to mesh the geometry with beam elements. INTRODUCTION TO ANSYS 6. 0 - Part 2 Material Properties October 30, 2001 Inventory #001571 5 -8

Beam Modeling B. Beam Meshing – Assign line attributes – Specify line divisions – Generate the mesh • The Mesh. Tool provides a convenient way to perform all three steps. INTRODUCTION TO ANSYS 6. 0 - Part 2 • Meshing the geometry (lines) with beam elements involves three main steps: Training Manual October 30, 2001 Inventory #001571 5 -9

Beam Modeling . . . Beam Meshing Training Manual • Line attributes for beam meshing consist of: – Material number – Section ID – Orientation keypoint • Determines how the cross section is oriented with respect to the beam axis. • Must be specified for all cross-section types. • A single keypoint can be assigned to multiple lines (i. e, no need to specify a separate keypoint for each line). • Each end of a line can have its own orientation keypoint, allowing the cross section to be “twisted” about the beam axis. INTRODUCTION TO ANSYS 6. 0 - Part 2 Step 1: Line Attributes October 30, 2001 Inventory #001571 5 -10

Beam Modeling . . . Beam Meshing INTRODUCTION TO ANSYS 6. 0 - Part 2 • Examples of using orientation keypoints: Training Manual October 30, 2001 Inventory #001571 5 -11

Beam Modeling . . . Beam Meshing Training Manual Pick lines Additional attributes for BEAM 188 & 189 INTRODUCTION TO ANSYS 6. 0 - Part 2 • To assign line attributes, use the “Element Attributes” section of the Mesh. Tool (or select desired lines and use the LATT command). October 30, 2001 Inventory #001571 5 -12

Beam Modeling . . . Beam Meshing Training Manual • For BEAM 188 and 189 elements, a single element spanning the entire beam length is not recommended. • Use the “Size Controls” section of the Mesh. Tool (or the LESIZE command) to specify the desired number of line divisions. INTRODUCTION TO ANSYS 6. 0 - Part 2 Step 2: Line Divisions October 30, 2001 Inventory #001571 5 -13

Beam Modeling . . . Beam Meshing • First save the database (Toolbar > SAVE_DB or SAVE command). • Then press the Mesh button in the Mesh. Tool (or issue LMESH, ALL) to generate the mesh. Pick lines INTRODUCTION TO ANSYS 6. 0 - Part 2 Step 3: Generate the Mesh Training Manual October 30, 2001 Inventory #001571 5 -14

Beam Modeling . . . Beam Meshing – Utility Menu > Plot. Ctrls > Style > Size and Shape… – Or /ESHAPE, 1 INTRODUCTION TO ANSYS 6. 0 - Part 2 • To see the cross-section shape in the element display, activate the element shape key: Training Manual October 30, 2001 Inventory #001571 5 -15

Beam Modeling . . . Beam Meshing Training Manual INTRODUCTION TO ANSYS 6. 0 - Part 2 • After beam meshing is completed, the next step is to apply loads and solve. October 30, 2001 Inventory #001571 5 -16

Beam Modeling C. Loading, Solution, Results – Displacement constraints • applied at keypoints or nodes – Forces • applied at keypoints or nodes – Pressures • load per unit length • applied on element faces – Solution > Apply > Pressures > On Beams – Or SFBEAM command – Gravity or rotational velocity • acts on entire structure INTRODUCTION TO ANSYS 6. 0 - Part 2 • Typical loading for beam models consists of: Training Manual October 30, 2001 Inventory #001571 5 -17

Beam Modeling . . . Loading, Solution, Results Training Manual – First save the database. – Then solve. (Or write the loads to a load step file and solve all load steps later. ) • Results review is the same as for other stress analyses: – View the deformed shape – Check reaction forces – Plot stresses and strains • The main advantage of BEAM 188 and 189 is that with the element shape key activated (/ESHAPE, 1), stresses can be directly viewed on the elements (similar to solids and shells). INTRODUCTION TO ANSYS 6. 0 - Part 2 • To obtain the solution: October 30, 2001 Inventory #001571 5 -18

Beam Modeling . . . Loading, Solution, Results Demo: INTRODUCTION TO ANSYS 6. 0 - Part 2 • Training Manual – Resume frame. db (contains lines, kp’s, loading, element type, material, and two cross sections) – Plot the two cross section already defined (SECPLOT, 1 & 2) – Define a third cross section using the Beam. Tool: • ID=3: Name = peak, Sub-type = box (hollow rectangle), W 1=6, W 2=6; T 1=T 2=T 3=T 4=0. 25 – Bring up Mesh. Tool, GPLOT, then assign the following line attributes: • Sloping lines: mat=1, secnum=3, orientation KP = topmost KP (#100) • Left vertical lines: mat=1, secnum=2, orientation KP = #102 • Right vertical lines: mat=1, secnum=2, orientation KP = #101 • Left & front horizontal lines: mat=1, secnum=1, orientation KP = #1 • Right & back horizontal lines: mat=1, secnum=1, orientation KP = #3 – Specify size=20 on all lines – Save, then LMESH, ALL; then EPLOT with /ESHAPE, 1 – Constrain the 4 bottom keypoints in all DOFs and apply a force of -10, 000 lb in the fy direction on keypoint #9 – Solve, then review results: deformed shape (animate), reaction forces, SX stresses (= axial + bending). Select elements with section ID=3 and replot stresses. Repeat for ID=2. October 30, 2001 Inventory #001571 5 -19

Beam Modeling D. Workshop Training Manual W 4. Building Frame Please refer to your Workshop Supplement for instructions. INTRODUCTION TO ANSYS 6. 0 - Part 2 • This workshop consists of the following problem: October 30, 2001 Inventory #001571 5 -20