line

| Aspect ratio | Percent error in displacement v at point A | | ------------ | ----------------------------------------- | | 2 | -5 | | 4 | -10 | | 6 | -25 | | 24 | -55 |

Figure 7–1 (b) Inaccuracy of solution as a function of the aspect ratio (numbers in parentheses correspond to the cases listed in Table 7–1) Table 7–1 Comparison of results for various aspect ratios

Case	Aspect Ratio	Number of Nodes	Number of Elements	Vertical Displacement, v (in.)		Percent Error in Displacement at A
				Point A	Point B
1	1.1	84	60	-1.093	-0.346	5.2
2	1.5	85	64	-1.078	-0.339	6.4
3	3.6	77	60	-1.014	-0.328	11.9
4	6.0	81	64	-0.886	-0.280	23.0
5	24.0	85	64	-0.500	-0.158	56.0
Exact solution [2]				-1.152	-0.360

Therefore, rollers are used at nodes along both the vertical and horizontal planes of symmetry. As previously indicated in Chapter 3, in vibration and buckling problems, symmetry must be used with caution since symmetry in geometry does not imply symmetry in all vibration or buckling modes.  (a）Large aspect ratio 

text_image

h₁ h₂ h₂ >> h₁

(b）Approaching a triangular shape 

text_image

β α α >> β

(c)）Very large and very small corner angles 

natural_image

Simple geometric triangle diagram with three vertices and connecting edges (no text or labels)

(d）Triangular quadrilateral Figure 7–2 Elements with poor shapes 

text_image

12 in. 10 lb/in. 6 24 36 42 48 54 60 66 5 4 3 2 1 7 19 31 37 43 49 55 61 48 in. 96 in. Axis of symmetry

Figure 7–3 Use of symmetry applied to a soil mass subjected to foundation loading (number of nodes ¼ 66, number of elements ¼ 50) (2.54 cm ¼ 1 in., 4.445 N ¼ 1 lb) # Natural Subdivisions at Discontinuities Figure 7–6 illustrates various natural subdivisions for finite element discretization. For instance, nodes are required at locations of concentrated loads or discontinuity in loads, as shown in Figure 7–6(a) and (b). Nodal lines are defined by abrupt changes of plate thickness, as in Figure 7–6(c), and by abrupt changes of material properties, as in Figure 7–6(d) and (e). Other natural subdivisions occur at re-entrant corners, as in Figure 7–6(f ), and along holes in members, as in Figure 7–5. 

text_image

Axes of symmetry 4 in. 4 in. 4 in. 2 in. 1.5 in. 200 lb/in. 3 in.

(a) Plane stress uniaxially loaded member with fillet 

text_image

5 0.75" 1 1.5 in. 0.5" 4 in. 78 1 in. 76

(b) Enlarged finite element model of the cross-hatched quarter of the member (number of nodes = 78,number of elements = 60) (2.54 cm = 1 in.) Figure 7–4 Use of symmetry applied to a uniaxially loaded member with a fillet # Sizing of Elements and the h and p Methods of Refinement For structural problems, to obtain displacements, rotations, stresses, and strains, many computer programs include two basic solution methods. (These same methods apply to nonstructural problems as well.) These are called the h method and the p method. These methods are then used to revise or refine a finite element mesh to improve the results in the next refined analysis. The goal of the analyst is to refine the mesh to obtain the necessary accuracy by using only as many degrees of freedom as necessary. The final objective of this so called adaptive refinement is to obtain equal distribution of an error indicator over all elements. The discretization depends on the geometry of the structure, the loading pattern, and the boundary conditions. For instance, regions of stress concentration or high stress gradient due to fillets, holes, or re-entrant corners require a finer mesh near those regions, as indicated in Figures 7–4, 7–5, and 7–6(f). We will briefly describe the h and p methods of refinement and provide references for those interested in more in-depth understanding of these methods. h Method of Refinement In the h method of refinement, we use the particular element based on the shape functions for that element (for example, linear functions for the bar, quadratic for the beam, bilinear for the CST). We then start with a baseline mesh to provide a baseline solution for error estimation and to provide guidance for 

text_image

y x

(a) Plate with hole under plane stress 

text_image

Axis of symmetry Axis of symmetry

(b) Finite element model of one-quarter of the plate Figure 7–5 Problem reduction using axes of symmetry applied to a plate with a hole subjected to tensile force mesh revision. We then add elements of the same kind to refine or make smaller elements in the model. Sometimes a uniform refinement is done where the original element size (Figure 7–7a) is perhaps divided in two in both directions as shown in Figure 7–7b. More often, the refinement is a nonuniform h refinement as shown in Figure 7–7c (perhaps even a local refinement used to capture some physical phenomenon, such as a shock wave or a thin boundary layer in fluids) [19]. The mesh refinement is continued until the results from one mesh compare closely to those of the previously refined mesh. It is also possible that part of the mesh can be enlarged instead of refined. For instance, in regions where the stresses do not change or change slowly, larger  Figure 7–6 Natural subdivisions at discontinuities elements may be quite acceptable. The h-type mesh refinement strategy had its beginnings in [20–23]. Many commercial computer codes, such as [12], are based on the h refinement. p Method of Refinement In the p method of refinement [24–28], the polynomial p is increased from perhaps quadratic to a higher-order polynomial based on the degree of accuracy specified by the user. In the p method of refinement, the p method adjusts the order of the polynomial or the p level to better fit the conditions of the problem, such as the boundary conditions, the loading, and the geometry changes. A problem is solved at a given p level, and then the order of the polynomial is normally increased while the element geometry remains the same and the problem is solved again. The results of the iterations are compared to some set of convergence criteria specified by the user. Higher-order polynomials normally yield better solutions. This iteration process is done automatically within the computer program. Therefore, the user does not 

text_image

P P

(a) Original mesh 

text_image

P P

(b) A uniformly refined mesh 

text_image

P P

(c) A possible nonuniform h refinement 

text_image

P P

(d) A possible uniform p refinement Figure 7–7 Examples of h and p refinement 

text_image

Pro/MECHANICA(R) 2000i2 Displacement Mag Deformed Original Model Max Disp +7.4182E-04 Scale 1.6176E+03 Load: LoadSet 1 "window3" - Design_2_MPA - Design_2_MPA

Figure 7–7 ðContinuedÞ need to manually change the size of elements by creating a finer mesh, as must be done in the h method. (The h refinement can be automated using a remeshing algorithm within the finite element software.) Depending on the problem, a coarse mesh will often yield acceptable results. An extensive discussion of error indicators and estimates is given in the literature [19]. The p refinement may consist of adding degrees of freedom to existing nodes, adding nodes on existing boundaries between elements, and/or adding internal degrees of freedom. A uniform p refinement (same refinement performed on all elements) is shown in Figure 7–7d. One of the more common commercial computer programs, Pro/MECHANICA [29], uses the p method exclusively. A typical discretized finite element model of a pulley using Pro/MECHANICA is shown in Figure 7–7e. # Transition Triangles Figure 7–4 illustrates the use of triangular elements for transitions from smaller quadrilaterals to larger quadrilaterals. This transition is necessary because for simple CST elements, intermediate nodes along element edges are inconsistent with the energy formulation of the CST equations. If intermediate nodes were used, no assurance of compatibility would be possible, and resulting holes could occur in the deformed model. Using higher-order elements, such as the linear-strain triangle described in Chapter 8, allows us to use intermediate nodes along element edges and maintain compatibility. # Concentrated or Point Loads and Infinite Stress Concentrated or point loads can be applied to nodes of an element provided the element supports the degree of freedom associated with the load. For instance, truss elements and two- and three-dimensional elements support only translational degrees of freedom, and therefore concentrated nodal moments cannot be applied to these elements; only concentrated forces can be applied. However, we should realize that physically concentrated forces are usually an idealization and mathematical convenience that represent a distributed load of high intensity acting over a small area. According to classical linear theories of elasticity for beams, plates, and solid bodies [2, 16, 17], at a point loaded by a concentrated normal force there is finite displacement and stress in a beam, finite displacement but infinite stress in a plate, and both infinite displacement and stress in a two- or three-dimensional solid body. These results are the consequences of the differing assumptions about the stress fields in standard linear theories of beams, plates, and solid elastic bodies. A truly concentrated force would cause material under the load to yield, and linear elastic theories do not predict yielding. In a finite element analysis, when a concentrated force is applied to a node of a finite element model, infinite displacement and stress are never computed. A concentrated force on a plane stress or strain model has a number of equivalent distributed loadings, which would not be expected to produce infinite displacements or infinite stresses. Infinite displacements and stresses can be approached only as the mesh around the load is highly refined. The best we can hope for is that we can highly refine the mesh in the vicinity of the concentrated load as shown in Figure 7–6(a), with the understanding that the deformations and stresses will be approximate around the load, or that these stresses near the concentrated force are not the object of study, while stresses near another point away from the force, such as B in Figure 7–6(f ), are of concern. The preceding remarks about concentrated forces apply to concentrated reactions as well. Finally, another way to model with a concentrated force is to use additional elements and a single concentrated load as shown in Figures 7–6(h). The shape of the distribution used to simulate a distributed load can be controlled by the relative stiffness of the elements above the loading plane to the actual structure by changing the modulus of elasticity of these elements. This method spreads the concentrated load over a number of elements of the actual structure. Infinite stress based on elasticity solutions may also exist for special geometries and loadings, such as the re-entrant corner shown in Figure 7–6(f). The stress is predicted to be infinite at the re-entrant corner. Hence, the finite element method based on linear elastic material models will never yield convergence (no matter how many times you refine the mesh) to a correct stress level at the re-entrant corner [18]. We must either change the sharp re-entrant corner to one with a radius or use a theory that accounts for plastic or yielding behavior in the material. # Infinite Medium Figure 7–3 shows a typical model used to represent an infinite medium (a soil mass subjected to a foundation load). The guideline for the finite element model is that enough material must be included such that the displacements at nodes and stresses within the elements become negligibly small at locations far from the foundation load. Just how much of the medium should be modeled can be determined by a trialand-error procedure in which the horizontal and vertical distances from the load are varied and the resulting effects on the displacements and stresses are observed. Alternatively, the experiences of other investigators working on similar problems may prove helpful. For a homogeneous soil mass, experience has shown that the influence of the footing becomes insignificant if the horizontal distance of the model is taken as approximately four to six times the width of the footing and the vertical distance is taken as approximately four to ten times the width of the footing [4–6]. Also, the use of infinite elements is described in Reference [13]. After choosing the horizontal and vertical dimensions of the model, we must idealize the boundary conditions. Usually, the horizontal displacement becomes negligible far from the load, and we restrain the horizontal movement of all the nodal points on that boundary (the right-side boundary in Figure 7–3). Hence, rollers are used to restrain the horizontal motion along the right side. The bottom boundary can be completely fixed, as is modeled in Figure 7–3 by using pin supports at each nodal point along the bottom edge. Alternatively, the bottom can be constrained only against vertical movement. The choice depends on the soil conditions at the bottom of the model. Usually, complete fixity is assumed if the lower boundary is taken as bedrock. In Figure 7–3, the left-side vertical boundary is taken to be directly under the center of the load because symmetry has been assumed. As we said before when discussing symmetry, all nodal points along the line of symmetry are restrained against horizontal displacement. Finally, Reference [11] is recommended for additional discussion regarding guidelines in modeling with different element types, such as beams, plane stress/plane strain, and three-dimensional solids. # Connecting (Mixing) Different Kinds of Elements Sometimes it becomes necessary in a model to mix different kinds of elements, such as beams and plane elements, such as CSTs. The problem with mixing these elements is that they have different degrees of freedom at each node. The beam allows for transverse displacement and rotation at each node, while the plane element only has inplane displacements at each node. The beam can resist a concentrated moment at a node, whereas a plane element (CST) cannot. Therefore, if a beam element is connected to a plane element at a single node as shown in Figure 7–8(a), the result will be a hinge connection at A. This means only a force can be transmitted through the 

text_image

Plane elements B A Beams P


text_image

B A Beams P Plane elements

(b) Figure 7–8 Connecting beam element to plane elements (a) No moment is transferred, (b) moment is transferred node between the two kinds of elements. This also creates a mechanism, as shown by the stiffness matrix being singular. This problem can be corrected by extending the beam into the plane element by adding one or more beam elements, shown as AB, for one beam element in Figure 7–8(b). Moment can now be transferred through the beam to the plane element. This extension assures that translational degrees of freedom of beam and plane element are connected at nodes A and B. Nodal rotations are associated with only the beam element, AB. The calculated stresses in the plane element will not normally be accurate near node A. For more examples of connecting different kinds of elements see Figures 1–5, 11–10, 12–10 and 16–31. These figures show examples of beam and plate elements connected together (Figures 1–5, 12–10, and 16–31) and solid (brick) elements connected to plates (Figure 11–10). # Checking the Model The discretized finite element model should be checked carefully before results are computed. Ideally, a model should be checked by an analyst not involved in the preparation of the model, who is then more likely to be objective. Preprocessors with their detailed graphical display capabilities (Figure 7–9) now make it comparatively easy to find errors, particularly the more obvious ones involved with a misplaced node or missing element or a misplaced load or boundary support. Preprocessors include such niceties as color, shrink plots, rotated views, sectioning, exploded views, and removal of hidden lines to aid in error detection. Most commercial codes also include warnings regarding overly distorted element shapes and checking for sufficient supports. However, the user must still select the proper element types, place supports and forces in proper locations, use consistent units, etc., to obtain a successful analysis. # Checking the Results and Typical Postprocessor Results The results should be checked for consistency by making sure that intended support nodes have zero displacement, as required. If symmetry exists, then stresses and displacements should exhibit this symmetry. Computed results from the finite element program should be compared with results from other available techniques, even if