1 / 43

Static Analysis of Beam by Finite Element Method In Ansys Workbench version 13

Static Analysis of Beam by Finite Element Method In Ansys Workbench version 13. HORYL Petr Ostrava 2012. Contents. Open Static Structural Design Modeler (DM) – Geometry Model – input Geometry from DM, Connections, Mesh

mercer
Télécharger la présentation

Static Analysis of Beam by Finite Element Method In Ansys Workbench version 13

An Image/Link below is provided (as is) to download presentation Download Policy: Content on the Website is provided to you AS IS for your information and personal use and may not be sold / licensed / shared on other websites without getting consent from its author. Content is provided to you AS IS for your information and personal use only. Download presentation by click this link. While downloading, if for some reason you are not able to download a presentation, the publisher may have deleted the file from their server. During download, if you can't get a presentation, the file might be deleted by the publisher.

E N D

Presentation Transcript

  1. Static Analysis of Beam by Finite Element Method In Ansys Workbench version 13 HORYL Petr Ostrava 2012

  2. Contents • Open Static Structural • Design Modeler (DM) – Geometry • Model – input Geometry from DM, Connections, Mesh • Static Structural - Boundary Conditions (Force, Moment, Line Pressure, Joints) • Solution – Results (Displacement, Internal Forces, Stress…) Simply Beam

  3. Simply Beam Structure F = 3kN q= 2.5 kN/m o a = 46 M = 4 kNm A B Part1 Part3 Part2 D C 6 m 3 m 5 m a) Maximum deflection b) Course of internal forces - axial force, shearing force and bending moment c) Maximum of normal stress Cross-section of beam: D = 152 mm, d1 = 60 mm Material properties: Steel Young's modulus of elasticity E = 2.1E5 MPa, Poisson's ratio ν = 0.3 Simply Beam

  4. 1 New Project After starting the Workbench 13select the type of analysis – „Static Structural“(arrow No 1) and type new name of project (2) 2 Simply Beam

  5. 2 3 Material Properties In window „Engineering Data“ we choose „Click here to add a new material“ . Potom napíšeme jméno nového materiálu „Beam Material “ (Arrow no 1) a výběrem „Isotropic Elasticity“ (2) jsme vyzváni k zadání příslušných materiálových dat v nově se otevírající tabulce hodnot ve spodní části okna (3.). Zpět se vrátíme příkazem „Return to Project“ (4.) 4 1 Simply Beam

  6. 2 Units „mm“ Now we can select „Units“ (1). For example „Metric“ with „mm“ (2) 1 Simply Beam

  7. 1 Open Geometry => Window „Design Modeler“ For creation beam geometry you must click on row „Geometry“ (1). Name of opening window will be „Design Modeler“ Simply Beam

  8. 5 6 4 1 2 3 Geometry - Points In the next window „Geometry“ we start creation of the four point from A till D, see picture of beam. Click on „Point“ (1),in the card below left choose „Manual Input“ (2),type “Coordinates X, Y, Z” of the point (3) and click on “Generate”(4). You can “Rename”(5) Point1 to PointA. In the middle of window you can see “PointA”(6). Repeat it for PointB to PointD. Simply Beam

  9. Geometry – 4 Points All 4 Points were created. Simply Beam

  10. Geometry – Lines 1 2 3 4 5 Now we continue creation geometry namely lines. Click on „Concept“(1),in the menu top left and choose „Lines From Points“(1).Hold “Ctrl“ keyboard button and select by left mouse button “PointA”(2) and “PointC”(3). Confirm by mouse “Apply”(4) and click on “Generate”(5). We have created Part1 of our beam. Repeat it for Part1 and Part2 Simply Beam

  11. Geometry – 3 Lines => Part1 to Part3 All 3 Lines were created. PointA PointC Part1 Part2 PointD PointB Part3 Simply Beam

  12. 1 2 3 4 5 Cross section Now we select cross section of our beam. Click on „Concept“(1),in the menu top left and choose „Cross Section“(2) and “Circular Tube”(3).In the card below left, type outer “Ro“ and internal “Ri” radius(4). In main window you see cross section(5). Simply Beam

  13. 1 2 3 Cross section for our beam Click on „Line Body“(1),in the menu top left and choose „Cross Section“ and “Circular Tube”(2).Confirm it by “Generation“(3). Save Project and Exit Design Modeler. Simply Beam

  14. 1 4 2 3 Transition between Geometryand Model For the correct transition between windows „Geometry“ and „Model“must be checked „Geometry Import“. In our project window click on „Tools (1) – Options - Geometry Import (2)“ and check tick box „Line Bodies“(3). Now open window „Model“ (4). Simply Beam

  15. Creation Path in Construction Geometry 1 2 3 3 4 6 5 To plot internal forces in the beam-shaped „Shear Force - Bending Diagramm“, we must choose on beam „Path“. In Modeler window click on „Model“(1), „ConstructionGeometry“(2)and „Path“(3). Then change the „Details of Path“(4) for „Path Type“(5) on „Edge“(6). Simply Beam

  16. Creation Path in Construction Geometry - continue 1 2 3 Click on „Path“(1). Choose „Line“(2) in Selection boxes. Hold “Ctrl“ keyboard button and select by left mouse button all three lines from left to right. Click on „Apply“(3). Simply Beam

  17. Creation Path in Construction Geometry - continue 2 1 3 We get right „Path“(1) for whole beam from starting „Edge“(2) to ending „Edge“(3) Simply Beam

  18. Mesh Generation 1 2 3 4 Left mouse button click on „Mesh“(1), open „Element Size“(2) in Details of „Mesh“ and type 50mm (2). Click right mouse button again on Mesh and „Generate Mesh“(3). Zoom right end of our beam and look at Circular Tube Cross Sections(4) . Simply Beam

  19. Boundary Conditions -> JointA in PointA 1 2 3 5 6 4 Click on „Static Structural“ insert „Supports“(1) and„Remote Displacement“(2). Because joint in PointA has free only rotation around axis Z, we must change these degree of freedom in row “Rotation Z“ to „Free”(3). Click on selecting box for “Point” and select “PointA”(4) and click on “Apply”(5). Rename „Remote Displacement“ in the tree to „JointA“(6) Simply Beam

  20. Boundary Conditions -> JointA in PointA continue 2 1 Picture shows only one free degree of freedom for JointA namely “Rotation: 0,, 0,, Free”(1).Rename this row in tree to “JointA”(2). Simply Beam

  21. Boundary Conditions -> JointB in PointB 2 3 4 1 On the same way we create “JointB”(1), but here we have two Free degree of freedom : “X Component - Free”(2) and “Rotation Z - Free”(3). We renamed joint to “PointB”(4) Simply Beam

  22. Boundary Conditions -> Force, Moment and Line Pressure 3 2 1 4 Click right mouse button on “Static Structural – Insert”(1). In the next step, we will need “Force”(2), “Moment”(3) and “Line Pressure”(4). Simply Beam

  23. Boundary Conditions -> Force 2 3 1 Click right mouse button on “Static Structural“(1) „Insert“(2) and„Force”(3). Simply Beam

  24. Boundary Conditions -> Force continue 4 6 3 8 2 1 7 In the left below table „Details of „Force“(1) change in row „Define by“ to „Components“(2). Type -2084 into row „X Component“(3) e.g. FX=F*cos(alfa)= 3000*cos(46). Type -2158 into row „Y Component“(4) e.g. FX=F*sin(alfa)=3000*sin(46). Click on selecting box for “Point”(6) and select “PointD”(7) and click on “Apply”. In the middle of window you can notice red force vektor(8) Simply Beam

  25. Boundary Conditions -> Moment 2 1 Similarly as Force, specify moment to „PointC“(1) as „Z Component“(2) -4E6 N.mm. In the middle of window you can notice sense of bending moment M, drawn in red (1) Simply Beam

  26. Boundary Conditions -> Line Pressure 2 1 3 4 5 Similarly as previous boundary conditions specify „Line Pressure“ on „Part2“(1). You must select box „Line“(2) from selection boxes. Into table „Details of „Line Pressure“(3) type -2,5 N/mm in row„Y Component“(4) and click on „Apply“(5). Simply Beam

  27. Boundary Conditions -> Line Pressure continue 1 2 In the middle of window you can notice red „Line Pressure“(1) with Y Component -2,5 N/mm(2). Simply Beam

  28. All Boundary Conditions in one picture 1 If you click on „Static Structural“ you can see all Boundary Conditions with their values(1). Simply Beam

  29. Solution 1 3 2 Now befor Solution we must prepare results which we need for our example analysis. It could be „Deformation“(1), „Beam Results“(2) for getting internal forces or „Beam Tool“(3) for stress results. Simply Beam

  30. Solution 1 2 3 As you can see, we select: „Total Deformation“, „Axial Force“, „Total Shear Force“, „Total Bending Moment“(1) and „Directional Shear-Moment Diagram (VY-MZ-UY)“(2). Befor selecting row „Directional Shear-Moment Diagram (VY-MZ-UY)“(2) in table „Details of …“, we must select in row „Path“ the same name for our beam also „Path“(3). Simply Beam

  31. Solution – Beam Tool and Force Reaction 1 2 3 4 We can add also: „Beam Tool“(1) with three possibility of resulting stress. „Direct Stress“, „Minimum Combined Stress“ and „ Maximum Combined Stress“(2). Important are also reaction forces. Click on „Probe“(3) and „Force Reaction“(4). Simply Beam

  32. Solution – Force Reaction continue 1 2 3 After clicking on „Probe“ and „Force Reaction“ select in table „Details of „Force Reaction“(1) row „Boundary Condition - JointA“(2). After that you can see small green table in the place of JointA „Force Reaction“(3). Do the same proces for JointB. Simply Beam

  33. Solution - Solve 1 Start computing proces with clicking on „Solve“(1) Simply Beam

  34. Results – Total Deformation 1 2 3 Details on exercises Simply Beam

  35. Results – Total Deformation Simply Beam

  36. Results – Axial Force Simply Beam

  37. Results – Shear Force Simply Beam

  38. Results – Bending Moment Simply Beam

  39. Results – Axial Sress Simply Beam

  40. Results – Maximum Combined Sress Simply Beam

  41. Results – Shear-Moment-Diagram Simply Beam

  42. Results – Force Reaction in JointA Simply Beam

  43. Results – Force Reaction in JointB Simply Beam

More Related