Lateral Analysis

Part 1: Right Way, Wrong Way with Software

The increasing ease of performing a Lateral Analysis of a structure is becoming a double-edged sword: there are many benefits, but it can also be quite dangerous. A fair share of presentations and articles from seasoned engineers warn about colleagues losing a sense of the real behavior of structures, or that engineers today simply do not know how to design structures without a computer.

To rationalize such comments, one may remember that the engineering curriculum remains similar to the education that engineers received 10, 20, or even 30 years ago. Many engineering programs focus on statics, dynamics, and material properties courses. So what explains this current perspective that today’s engineers are not as grounded as their predecessors in their understanding of structural engineering design? One explanation is rooted in the thought that structural engineers are overly reliant on software programs and that software processes are replacing engineering judgment.

Software programs should make better engineers, not worse. They are tools and should be treated as such. Each program has unique and varying abilities to create a representation of the real structure, some with more features and options than others. However, it is better to view all structural engineering software programs as incredible graphic user interfaces, able to solve complex sets of equations and run predefined formulae. It should not be assumed that software programs can understand the complexity of the structures and the loads that need to be applied, or be able to devise and create unique solutions.

These tools provide the ability to solve problems very efficiently and iterate design options until the best possible alternative is developed, provided the problem has been accurately identified. Accurately defining the problem is the main issue. Also, the isolated manner in which engineers work leads to few people thoroughly examining the design problem to ensure it has been defined accurately. Individuals are then left to complete the work with no one watching, in an ever-increasing budget-constrained, schedule-cramped environment. This is an opportunity for the shortcomings of using software to take root. The May 2016 issue of STRUCTURE magazine included an article on the use of the Finite Element Method (FEM) for masonry, and perhaps future articles will feature the specific uses of other materials with FEM. This article, however, is on the broader topic of lateral analysis, and the right way and wrong way to use FEM software programs. Therefore, this piece does not include material-specific recommendations; instead, it discusses lateral load generation, element (beam, column, wall) properties, diaphragm properties, loads on diaphragms, element connection to diaphragms, types of lateral analysis, and methods for quality assurance of the lateral analysis.

Brief Review of FEM Basics

The FEM is the process of simplifying a real life structure, generally a continuum with infinite degrees of freedom, to a finite number of elements with unique material properties.

The FEM is broken up into three steps:

  1. Modeling: Pre-processing step where a user defines elements of the model, element connectivity, support conditions, and forces to represent various loading conditions.
  2. Analysis: Processing step that requires little input from the user – users establish a few important parameters and then allow the software to solve vast sets of equations based on modeling.
  3. Validation and Design: Post-processing, the step of interpreting and verifying the results of the analysis and then designing elements based on parameters determined by the material codes one uses.

Part 1 of this article examines the first and most important step for FEM, model generation.


In defining a model, users establish one-dimensional line elements (straight or curved) with two end nodes, and/or two-dimensional plate elements (square, rectangular, or triangular planar shape) with nodes at each corner of the element. In the process of defining the elements and end nodes, some nodes need to be identified as supports. Others remain as free nodes able to translate in three dimensional (X, Y, and Z) degrees of freedom (DOF), and rotate about the three axes (RX, RY, & RZ).

Support nodes generally have translational and/or rotational DOFs fixed. Remember that, for the actual condition the model represents, most support conditions are less than the idealized fixed condition. In nearly all cases, it would be more accurate to specify the support as a resistance over a potential displaced distance; in other words, a spring support. This is true for both translational and rotational degrees of freedom. Small differences in these support conditions may have a significant impact on the lateral resistance of the assigned members.

Not that all foundations should be spring supported, but their true behavior should be considered, especially when a building has dissimilar lateral resisting elements such as moment frames and walls where lateral load distribution may be greatly affected by soil stiffness. However, when dealing with similar resisting elements, such as a building with equally sized and uniformly distributed braced frames, fixed supports or spring supports may have little effect on the outcome of the analysis. Here, a column’s foundation can be modeled as a pinned support (free rotational DOF) since rotational stiffness may have less impact compared to vertical and horizontal translational stiffness.

Modeling Line and Plate Elements

Section properties and member elasticity for line and plate elements need to be defined. Many of the software programs are based on a linear elastic analysis, which is sufficient for members that remain elastic under static loads such as dead load, live load, snow load, and even idealized wind loads on a model. However, additional material properties must be considered when an inelastic response is expected, such as for concrete elements that respond in a non-linear manner when the concrete cracks under tensile stress and engages reinforcement. Inelastic response is also expected for members designed to resist seismic dynamic loading with a response modification factor that is, in part, based on an inelastic response.

This inelastic behavior of concrete is accounted for by reducing the stiffness with an element reduction factor. It is very important to realize that software tools do not make this modification automatically, and require user input through several iterations of modeling and analysis (loads to the member change as stiffness changes and may require further member modification).

Many software programs allow the users to define the geometric boundaries of entire slab elements or wall panels and discretize those large geometries into smaller finite elements by a process called meshing. Sometimes meshing is a manual process, and other times programs offer automatic meshing. To a certain extent, the finer the mesh (smaller the elements), the better the finite element method can approximate the result. There is a point of diminishing return in which finer meshes only result in a small percentage change in the results. It should be noted that finer meshes also produce significantly increased processing times for the finite element analysis. Having a mesh with nodes closer together than the thickness of the element (this is especially relevant with concrete materials) is unnecessary in most cases, as it would be unreasonable to have differential movement between nodes spaced that close together.

With respect to the elements of the finite element model, the last critical piece of information is connectivity. This can be simply defined as pinned (translational movement is shared between elements that share the same node) or fixed (translations and rotational degrees of freedom are maintained between the elements that share the node). Similar to the nodal degrees of freedom, it is important to note that idealized connections between members are more accurately represented by elastic springs. Some deformation can occur between the two elements at a joint otherwise considered as rigid, just as some rotational stiffness occurs for most connections specified as pinned. Just as with nodes, not all joints need to be connected with springs, but consider the implication for each element end to deform independently compared to the idealized condition and model accordingly. For example, it would be challenging to have a forty-inch-deep steel beam with thirteen rows of bolts act as a truly pinned end condition.

Another option for one-dimensional members in most software programs is the ability to shorten members using rigid offsets, based on the dimension of the member into which it is framing. This allows a user to create a model that reflects the actual joint size and should be considered since all members have a physical dimension (width and depth). Users define members using centerline modeling, but then the program recognizes the member lengths to be the elastic portion between rigid links. This creates a stiffer model, wherein the elastic portion of the element is shorter and reactions are at the face of the joint.

When building a finite element model, one can over-restrain members to nodes. For example, if there are two-line elements that share a common node, they are connected, and one can choose each members’ connectivity at the node. If the rotational restraint for each member is released, one will likely receive a warning of a local instability. A node needs to be elastically attached to one member or the other. However, to avoid the error, engineers fix both axes (not one or the other), possibly resulting in an over-connected model. Often, at the end of a steel beam, only the strong-axis moment is designed as a moment-resisting connection. The modeled weak-axis moment rigidity participates in the models’ resistance to lateral loads. Although in most situations this may be relatively small, it can make a difference in load distribution. In certain models where large sections have modeled weak axis moment conditions, it may “collect” relatively large loads that need to be addressed.

Another element restraint that is often overlooked and used in a nonconservative manner for the purpose of eliminating instability warnings is torsional restraint (or rotational stiffness along the member length). This may not be an issue for sections such as concrete or closed steel sections (HSS), but open steel sections do not resist torsion well. This is an example of how a simple error in modeling may result in the collection of loads that are not being checked during design.

Modeling Diaphragms

A very important criterion of lateral loading for buildings is the types of diaphragms that are defined. With nodes, line element columns and beams, and plate element walls, many programs offer the ability to define a diaphragm constraint instead of requiring plate element slabs to be modeled. Both rigid and non-rigid diaphragm types are idealized to simplify analysis. Rigid diaphragms fix the translation of all nodes of a similar elevation relative to one another, while non-rigid diaphragms allow free horizontal translation of one node relative to another.

Is this idealized modeling necessary? In fact, this approach of trying to capture the true diaphragm behavior is even named semi-rigid diaphragm modeling. Geometric irregularities, lateral resisting elements with different materials and different types (walls and frames), or diaphragms with relatively large openings, should be defined as semi-rigid. Semi-rigid diaphragms complicate the stiffness of the finite element model by requiring many plate element slabs be defined, which again leads to increased time in analysis. Not every diaphragm needs to be semi-rigid. For example, diaphragms with similar and regular vertical lateral resistance elements and diaphragms with uniform and consistent slabs with few slab penetrations can likely be considered rigid.

When it comes to diaphragm action, caution must be used when there is a step in the diaphragm. Not only does diaphragm behavior require a vertical element (short wall, braces) to transfer load, but the diaphragm chords (generally at edges or extreme stress locations) must be adequate locally or transition from one diaphragm level to another. Rigid diaphragms should not be specified to include isolated diaphragms supported at multiple levels. Elements should be modeled that transition diaphragm forces as load transitions from one diaphragm level to the other.

Consider the element properties of semi-rigid diaphragms similar to other modeled elements. Settings for in-plane axial and shear stiffness, and out-of-plane shear and bending stiffness, need to take into account either the elastic or potentially inelastic behavior of semi-rigid diaphragm elements.

Modeling Element Stiffness

All of these options for nodes, one and two-dimensional members, and diaphragms changes the lateral load distribution. The more strength and stiffness that is represented by an area of the model, the more the lateral load is distributed to that area. It is important in the modeling phase to define actual properties. Far too often, users take shortcuts such as defining idealized support conditions, not defining section modification factors because it takes too much time, or defining material properties that are arbitrarily low in an effort to be conservative. Not only are each of these and other modeling shortcuts incorrect, but they lead to inaccurate lateral load distribution. This results in some areas being assigned too much load (regions with too much stiffness) and other areas being assigned too little load, leading to unconservative designs (regions with too little stiffness).

We all would like to think of ourselves as being progressive in our industry by using FEA software. Much more progress should be made. It would be wrong to blindly use software tools without fully understanding them, and also wrong to not fully utilize the tools. As author C.S. Lewis states,

We all want progress. But progress means getting nearer to the place where you want to be. And if you have taken a wrong turning, then to go forward does not get you any nearer. If you are on the wrong road, progress means doing an about-turn and walking back to the right road; in that case the man who turns back soonest is the most progressive man.

If you find yourself on the wrong path, reconsider your approach to modeling with FEA software. The next article (Part 2) discusses completing the modeling step by offering suggestions regarding applying loads to the model, comments on analyzing the model and when to review the results, and finally a discussion regarding the design of members.▪

About the author  ⁄ Samuel M. Rubenzer, P.E., S.E.

Samuel M. Rubenzer is the founder of FORSE Consulting and assists with designs on a variety of projects and building types. He has also been the structural engineering consultant to Structural Masonry Coalitions in several states. He can be reached at

Comments posted to STRUCTURE website do not constitute endorsement by NCSEA, CASE, SEI, C3 Ink, or the Editorial Board.

No Comments

Leave a Comment

Download this article