plane_stress_tutorial

pdf

School

University of Rhode Island *

*We aren’t endorsed by this school

Course

466

Subject

Mechanical Engineering

Date

Dec 6, 2023

Type

pdf

Pages

Uploaded by LieutenantElementSquid28

15 Tutorial 4. Plane Stress Analysis Consider the problem of a 4” x 2” x 0.1” aluminum plate (E=10e6 psi,  =0.3) with a 1” diameter circular hole subjected to an axial stress of 100 psi. Determine the maximum axial stress associated with the stress concentration at the edge of the circular hole. Compare this solution with the design chart (ref. “ Shigley's Mechanical Engineering Design, ” 10th Edition, Budynas and Nisbett, 2015) for the case d / w =0.5 which gives  max  2.18 (200 psi) = 436 psi. UY = 0 UX = 0 Use of Symmetry Full Model

16 Finite Element solution Start => All Programs => Dassault Systems SIMULIA Abaqus => Abaqus CAE => Create Model Database With Standard/Explicit Model File => Set Working Directory => Browse to find desired directory => OK File => Save As => save plane_stress_tutorial.cae file in Work Directory Module: Sketch Sketch => Create => Approx size - 5 Add=> Point => enter coordinates (.5,0), (1,0), (1,2), (0,2), (0,.5) => select 'red X' View => Auto-Fit Add => Line => Connected Lines => select point at (.5,0) with mouse, then (1,0), (1,2), (0,2), (0,.5) => right click => Cancel Procedure => Done Add => Arc => Center/Endpoint => select point at (0,0), then (.5,0), then (0,.5) => right click => Cancel Procedure => Done Module: Part Part => Create => select 2D Planar, Deformable, Shell, Approx size - 5=> Continue Add => Sketch => select 'Sketch-1' => Done => Done Module: Property Material => Create => Name: Material-1, Mechanical, Elasticity, Elastic => set Young's modulus = 10e6, Poisson's ratio = 0.3 => OK Section => Create => Name: Section-1, Solid, Homogeneous => Continue => Material - Material-1, plane stress/strain thickness - 0.1 => OK Assign Section => select entire part by dragging mouse => Done => Section-1, Thickness: From section => OK Module: Assembly Instance => Create => Create instances from: Parts => Part-1 => Dependent (mesh on part) => OK Module: Step Step => Create => Name: Step-1, Initial, Static, General => Continue => accept default settings => OK Module: Load Load => Create => Name: Load-1, Step: Step 1, Mechanical, Pressure => Continue => select top edge => Done => set Magnitude = -100 => OK BC => Create => Name: BC-1, Step: Step-1, Mechanical, Displacement/Rotation => Continue => select bottom edge => Done => U2=0 BC => Create => Name: BC-2, Step: Step-1, Mechanical, Displacement/Rotation => Continue => select left edge => Done => U1=0 Module: Mesh Set Model: Model-1, Object => Part: Part-1

17 Seed => Edges => select full model by dragging mouse => Done => Method: By size, Bias: None, Sizing Controls, Element Size=0.1 => OK => Done Mesh => Controls => Element Shape => Tri (for triangles), Quad (for quadrilaterals), or Quad dominated (for mixed triangles and quads - mostly quads), Technique: Free > OK Mesh => Element Type => select full model by dragging mouse => Done => Element Library: Standard, Geometric Order: Linear, Family: Plane Stress => Linear/Tri (for CST), Quadratic/Tri (for LST), Linear/Quad (for 4 node quad), or Quadratic/Quad (for 8-node quad) => OK => Done (try varying element type, interpolation functions and mesh density) To refine mesh locally: Seed => Edges => Select bottom edge and arc (use Shift Key to select multiple edges) => Done => Method: By size, Bias: Single, Minimum size: .02, Maximum Size: 1, Flip Bias: Select and click on edges such that arrow points toward desired refined point => OK => Done Mesh => Part => OK to mesh the Part: Yes => Done Tools => Query => Region Mesh => Apply ( displays number of nodes and elements at bottom of screen ) Module: Job Job => Create => Name: Job-1, Model: Model-1 => Continue => Job Type: Full analysis, Run Mode: Background, Submit Time: Immediately => OK Job => Manager => Submit => Job-1 Job => Manager => Results (transfers to Visualization Module) Module: Visualization Viewport => Viewport Annotation Options => Legend => Text => Set Font => Size=14, Apply to: Legend, Title Block and State Block => OK => OK View => Graphics Options => Viewport Background = Solid=> Color => White (click on black tile to change background color) Plot => Deformed Shape Deformed Shape Options => Basic => Show superimposed undeformed plot => OK Ctrl-C to copy viewport to clipboard => Open MS Word Document => Ctrl-V to paste image Result => Options => Unselect “Average element output at nodes” => OK Result => Field Output => Name - S => Component = S22 => OK Plot => Contours => On Deformed Shape Ctrl-C to copy viewport to clipboard => Open MS Word Document => Ctrl-V to paste image Tools => Query => Probe Values => select desired Field Output (click on Field output variable icon) and select desired component (S11, S22, etc.) => OK => Probe Nodes => move cursor to desired location to view nodal results Tools => Path => Create => Node List => Continue => Add Before => select nodes along bottom edge => Done => OK Tools => XY Data => Create => Source: Path => Continue => X Distance => Plot Ctrl-C to copy viewport to clipboard => Open MS Word Document => Ctrl-V to paste image Report => Field Output => Position - Centroid => Variable – Mises, S11, S22, S12 => Apply Examine tabulated results in 'Abaqus.rpt' file.

Your preview ends here

Eager to read complete document? Join bartleby learn and gain access to the full version

Access to all documents
Unlimited textbook solutions
24/7 expert homework help

18 Typical Results (no edge bias) CST - 3 node triangle (linear interpolation) LST - 6 node triangle (quadratic interpolation) 4-node Quad (linear interpolation) 8-node Quad (quadratic interpolation)

19 Typical Results (with edge bias) CST - 3 node triangle (linear interpolation) LST - 6 node triangle (quadratic interpolation) 4-node Quad (linear interpolation 8-node Quad (Quadratic interpolation)

20 Stress Distribution along y=0 (bottom edge of mesh)

Your preview ends here

Eager to read complete document? Join bartleby learn and gain access to the full version