Element Topologies: Beams vs. Shells vs. Solids And Linear vs. Quadratic

1. Element Topologies: Beams vs. Shells vs. Solids And Linear vs. Quadratic

2. The Big Assumption… Calculate the area of a circle... • Divide a complex problem into a number of simple ones • Solve these simple problems, add them all up and get the answer to a complex problem • Perfect use of a computer (billions of similar numerical operations)

3. uy Y ux [ k ]e { u }e = { f }e X element level Finite Element Discretisation • A “Finite Element” is equivalent to one of these “simple” sub-problems • The process of splitting-up a structural component into finite elements is called “discretisation”

4. The Finite Element… • Finite Elements have simple geometric shapes, e.g. lines, triangles, rectangles, cubes • The points at the corners are called Node or Grid points • Nodes connect the elements together

5. F = 1000 N A = 20mm2E = 210000 N/mm2 L = 50 mm A = 50mm2E = 210000 N/mm2 L = 50 mm “Real Life…” • A spigot in need of analysis…

6. The “Numerical” Approximation… • The spigot can be represented in many ways, here we use “beam” finite elements… Node 3 L = 50 mm A = 20mm2E = 210000 N/mm2 Element 2 Node 2 L = 50 mm A = 50mm2E = 210000 N/mm2 Element 1 Node 1

7. A “Real” Finite Element Mesh • The geometry has been divided into finite elements • The elements are “assembled” to give the global stiffness matrix • Loading and supports are applied • The overall matrix solution is solved to give the displacement at each node • The solution size can vary from tens to multi-millions of nodes • The solution time can vary from seconds to multi-weeks

8. Types of Finite Elements • The choice of the element type is dependent on the structure to be analyzed • In geometric terms, “Line”, “Surface” or “Volume” elements are available • In finite element terms, these correspond to, “Beam”, “Shell” or “Solid” elements…

9. Beam/Bar Element Analysis Examples Frames Trusses Pantograph Useful in representing stiffeners on shells

10. Beam Element Analysis Examples • A detailed model of this bridge would take hundreds of thousands of shell or solid elements

11. Shell Element Analysis Examples Thin plane or curvedmetal sheets Thin shells, thin walled pressure vessels Aircraft components Automotive parts

12. Shell Element Analysis Examples Courtesy of Adtranz

13. Solid Element Analysis Examples Thick plates and consoles Thick walled pressure vessels Cast iron parts and fittings

14. Solid Element Analysis Examples Courtesy of Volvo Car

15. Damper Concentrated Mass Gap (element 12) (Point-Point-Contact) Spring Rigid / Interpolation Examples of “Special“ Element 除了gap以外，其餘並無對應的real element，應視為一種傳力的“方式’

16. A Real Life Example... The International Space Station

17. Beam/Bar Model Analysis of Solar Array Truss

18. Shell Model Analysis of crew compartment module

19. Solid Model Analysis of lifting lug

20. Y X Z qy v u qx w qz Degrees of Freedom • The displacement at a node generally consists of translational and/or rotational behaviour. Each of these displacement components are termed degrees of freedom • In a structural analysis, each node typically has a maximum of 6 degrees of freedom: • u, v, w translations corresponding to displacements in the x, y, z axis directions respectively • qx, qy, qzrotations corresponding to rotations aboutthe x, y, z axes respectively • Different element types have different degrees of freedom, for example: • Solid elements have 3 DOF’s (u,v,w translation) • Shell elements have 6 DOF’s (u,v,w and qx,qy,qzrotations) • Example: A bar/rod element having only (u,v) degrees of freedom will not be able to carry a torque • Example: A solid brick element having only (u,v,w) degrees of freedom will not be able to carry a torque

21. Element Type Comparison

22. Element Selection: Some Overall Issues • Consider a rectangular beam frame: • Beams are 100 mm wide, 200 mm high, 5mm thick • Overall length is 2m • Total width is 1m • Centerline of the cross bars are located 550 mm from each end • The beams are welded together, but the weld fillets are to be neglected due to their small size • The structure carries a load of 2000 kg evenly distributed over the two cross bars • Investigate the maximum overall deflection and maximum stress • Element aspect ratios greater than 5 are not permitted • What are the differences in time and effort when carrying out a beam, shell and solid analysis of the same structure…

23. Beam Model Element size 100 mm

24. ShellModel Element size 33 mm

25. Solid Model Element size 25 mm

26. Comparing The Three Analyses BeamShellSolid Number of nodes 60 9072 66015 Number of elements 60 3024 33003 DOF 336 44640 196317 Disk usage for solving 1 MB 195 MB 124 MB Memory usage for solving 16 MB 21 MB 1530 MB Modelling time 20 min 30 min 60 min Solving time 2 sec 70 sec 2000 sec Postprocessing time 15 min 2 min 1 min Total time 35 min 33 min 94 min Maximum deflection 0.0984 mm 0.143 mm 0.135 mm

27. Comparing The Three Analysis • Beam Model • Minimal modelling effort, accurate calculation results • Lowest solution cost • Does not calculate beam cross section deformation (which happens in this case) • Postprocessing somewhat awkward and time consuming, could present errors • Shell Model • Higher modelling effort, good calculation results • Average solution cost • Must have control of what is “top“ and “bottom“ of elements • Solid Model • Highest modelling effort, good calculation results • Highest solution cost • Does not give any significant additional results compared to shell model

28. The Element Library

29. Patran groups elements by their geometric shape: 0D: Point mass, damping 1D: Bar, beam elements (whether 2D or 3D formulations) 2D: 2D continuum elements and 3D shell elements 3D: 3D continuum elements Element types can also be divided into four basic categories: Beam elements such as trusses, rods and bars Shell Elements, such as plates, shells, shells of revolution Continuumelements such as 3D solids, plane stress, plane strain and axisymmetric (without 4,5,6 d.o.f.) Special Elements such as point mass, gaps, pipe bend, shear panel, semi-infinite Point Elements Element Library Categories

30. Element Library Categories • Further element options include: • Reduced integration • Assumed strain • Constant dilatation • “Herrmann” formulation MSC.MARC supports an extensive element library that can be used to simulate a variety of “real world” structure

31. Element Type Numbering • Elements are mostly defined by a numbering scheme • Volume B contains all the details for each elements • Mentat uses the element number to make selection (e.g. 7) • Patran uses element description to make the selection (e.g. “solid”)

32. yelem xelem zelem Beam Elements

33. Euler-Bernoulli Beams 2D: 3 DOF @ nodes: Ux, Uy, qz 3D: 6 DOF @ nodes: Ux, Uy, Uz, qx, qy, qz Evaluates shear and moments Takes no account of transverse sheardeformation Also known as “thin” beams (standard) Bending moments may vary linearly over this element Timoshenko Beams 2D: 3 DOF @ nodes: Ux, Uy, qz 3D: 6 DOF @ nodes: Ux, Uy, Uz, qx, qy, qz Evaluates shear and moments Allows for transverse shear deformation effects Also known as “thick” beams (general) Bending moments are constant over this element Beam Elements Truss, Spar, Rod Elements • 2D: 2 DOF @ nodes: Ux, Uy • 3D: 3 DOF @ nodes: Ux, Uy, Uz • Specifically for axial-only members All these elements support geometric and material nonlinearity

34. Beam Elements: Properties • Beam elements show up on the screen as lines with no visible cross section • Beam elements have no geometrical attributes other than length • All cross sectional characteristics must be given as element properties: • Cross sectional Area (A) - transfers axial forces • Moments of Inertia (Ixx/Iyy) - transfers bending and shear • Torsional Moment of Inertia (J) - transfers torsional forces • A vector to define the orientation of the cross section (the local element coordinate system)In Patran, this vector is defined in either its global (X,Y,Z) or a local coordinate system…

35. < 0 1 1 > Beam Elements: Properties X Ixx J XZ Plane Izz Node2 Z Node 1 Y Z Y X Global CS

36. Bar and Beam elements are numerically integrated along their axial direction using Gaussian integration For Beam elements, the stress strain law is integrated through the cross section using Simpson’s rule Takes account of the variation of bending through the depth Stresses and strains are evaluated at each integration point through the thickness This allows an accurate calculation if nonlinear material behaviour is present In elastic beam elements, only the total axial force and moments are computed at the integration points Beam Elements: Integration

37. Beam Elements: Choice • The choice of beam is dependent on whether the analysis is 2D or 3D; whether it is an open or closed section; whether it is a thick or a thin beam; whether nonlinear behaviour is required • Beam element types 76-79 are the recommended beams for fully nonlinear analysis • Marc does not currently have an arbitrary solid cross section beam element for use in nonlinear analyses (they are mostly thin-walled, open/closed section). In this case, it is necessary to build up the solid section using the beam branching capability • For an elastic, geometrically nonlinear analysis then 52 or 98 would be recommended and easiest to use

38. 2D Solid Continuum Elements

39. “Cut-down” versions of 3D solid continuum elements – using assumptions for specific geometries Elements in this suite includes: Plane Strain Generalized Plane Strain Plane Stress Axisymmetric Come with 3, 4 nodes for low order (“linear”) elements Come with 6 and 8 nodes for higher order (“quadratic”) elements Corresponding heat transfer elements “Herrmann” formulation elements are also part of this suite and will be discussed later 2D Solid Continuum

40. 2D Solid Continuum • Plane Stress • 2 DOF @ nodes: Ux, Uy • Out-of-plane stresses assumed zero • Results include sx, sy, txy, (ex, ey, ez, gxy) • Definition of thickness is required • Flat panels subject to in-plane loads • Plane Strain • 2 DOF @ nodes: Ux, Uy • Out-of-plane strains assumed constant or zero • Results include sx, sy, sz, txy, (ex, ey, gxy) • Definition of thickness is required • Slice of car’s door rubber seal Plane Stress Plane Strain

41. 2D Solid Continuum This CAD model… • Axisymmetric Elements • 2 DOF @ nodes: Ux, Uy (Ur) • Results include sx, sr, sq, txr, (ex, er, eq, gxr) • Axisymmetric structures with axisymmetric loadings • Definition of thickness is not required – a 1 radian segment is assumed • Results are given for a 1-radian segment therefore • Global X-axis is the assumed axis of symmetry • Global Y-axis is the assumed radial direction Could have this CAE model

42. Shell Elements

43. Elements in this suite includes: Thin shell Thick Shell Membrane Shear Panel Axisymmetric Shell Results typically based on a plane stress assumption and include sx, sy, txy, (ex, ey, ez, gxy) Come with 3, 4 nodes for low order (“linear”) elements Come with 6 and 8 nodes for higher order (“quadratic”) elements Corresponding heat transfer elements Shell Elements show up on the screen as 2D entities with a thickness of zero (viewed from the edge) The thickness is given as a property of the element Shell Elements

44. Shell Elements Thin Shells: • 6 DOF @ nodes: Ux, Uy, Uz, qx, qy, qz • Definition of thickness is required • In-plane/out-of-plane loadings in planar and curved surfaces • Ignores out-of-plane normal stress • Ignores out-of-plane transverse shear stresses(Normal’s remain normal) • Thickness very small (<5%) compared to typical surface

45. Shell Elements Thick Shells: • 6 DOF @ nodes: Ux, Uy, Uz, qx, qy, qz • Definition of thickness is required • In-plane/out-of-plane loadings in planar and curved surfaces • Ignores out-of-plane normal stress • Considers out-of-plane transverse shear stresses (plane sections remain plane) • Thickness small (>5%, but <10%, ) compared to typical surface dimensions

46. Shell Elements Shear Panel: • 3 DOF @ nodes: Ux, Uy, Uz • In-plane loadings only in planar and curved surfaces • A shear panel is an idealised model of an elastic sheet • If there are stiffeners present, the panel resists the shearing forces and the stiffeners resist normal and bending forces • Restricted to linear materials • Large displacement effects are neglected • Evaluates only shear stress at all four nodal points Membranes: • 3 DOF @ nodes: Ux, Uy, Uz • In-plane loadings only in planar and curved surfaces • Very thin structures unable to sustain bending - very unstable. • This element is usually used with the LARGE DISP parameter, in which case the tensile initial stress stiffness increases the rigidity of the element • All constitutive models can be used with this element. • Tension space structure covering

47. Shell Elements Axisymmetric Shells: • 3 DOF @ nodes: Ux, Uy, qz • In-plane loadings only • Suitable for large displacements and large membrane strains • One-point Gaussian integration is used for the mass and pressure determination • All constitutive models can be used with this element

48. t Shell Element Characteristics • The stress distribution through the thickness of a shell is needed • The thickness of a shell is divided into “layers” • At each layer the in-plane stresses are evaluated using (typically) a 2x2 Gauss rule • A through-thickness integration of these layer stresses gives the bending response of the shell (Simpsons or Gauss rule) • Typically top, middle, and bottom layer stresses are calculated and reported • This numerical integration allows any material behavior at each layer; for example • Yelding of a nonlinear elastic-plastic shell can be followed through the section from a fully elastic to a fully plastic section • Similarly composite failure can be simulated • The number (density) of integration points through the thickness can vary according to user specification: • 1 layer: Linear materials • 7 layers: Most nonlinear problems • 11 layers: Extremely nonlinear response – such as elastic-plastic dynamic problems • Composite shells have one stress recovery point in each laminate layer

49. The layer number convention is such that layer 1 lies on the side of the positive normal to the shell, and the last layer is on the side of the negative normal Reference: MSC.Marc, Volume B, Element Library. Chapter 1, Shell Layer Convention n Top 4 3 3 n 1 2 Z Y 1 Bottom 2 X Shell Element Characteristics Z1 is bottom layer in Nastran And top layer in Marc

50. Results: Shell Elements • The stresses reported for shell elements are oriented in local element axes by default (can be modified in post-processing) • As part of creating a contour plot of shell element results the user must select which layer is of interest (typically ”top”, ”bottom” or ”middle”) • Shown are the stresses in the Y-direction. They should be tensile on the positive z-side and compressive on the negative z-side of the model