# FEA gap elements: choosing the right stiffness.

FEA Gap Elements: Choosing the Right Stiffness

While many structural problems can be formulated in terms of a single continuous domain, there is a large class of problems that involve contact surfaces and friction. Perhaps the most common of these is the bolted joint, but there are numerous other examples, such as electrical contacts sliding past each other, a pin bearing against the side of a hole in a plate, bolt threads bearing against the inner threads of a threaded hole, or any two surfaces in contact. To address such contact problems, many developers of finite element analysis software have included gap elements, more precisely called interface elements, in their element libraries.

Useful Features

Gap elements simulate contact between two surfaces by generating restoring (contact) forces when the two surfaces approach each other and by removing the contact forces when the two surfaces move away from each other. This means that gap elements have two stiffness values associated with them, a finite value (usually quite large) when the surfaces are in contact and zero (or nearly zero) when the surfaces are not in contact (see Figure 1). For this reason, gap elements are frequently called bilinear elements.

Another useful feature of gap elements is their ability to simulate sliding with friction. When subjected to a shearing force, gap elements generate a counteracting friction force. When the shearing force exceeds the maximum friction force that the gap elements can generate, then the gap elements let the contact surfaces slip past each other. The maximum friction force is governed by the user-defined coefficient of friction and the contact force.

The user-defined stiffness of gap elements is a key parameter. If a finite element model includes gap elements that are defined with a stiffness that is too small, then the displacements calculated with that model will be incorrect. If the gap elements are defined with a stiffness value that is too large, then the model may not yield a solution at all. Instead, it may fall prey to a phenomenon called bouncing. Bouncing simply means that the gap elements change their status (open/closed/open) with each iteration of the solution process. Therefore, the stiffness of gap elements must be chosen with some care.

Rule of Thumb

The developers of the Ansys finite element analysis program recommend a stiffness for gap elements that is one or two orders of magnitude greater than the stiffness of adjacent elements. This is a convenient rule of thumb, but it is important that we understand the basis for the recommendation, particularly if we are using the elements for the first time. To this end, we demonstrate the use of gap elements with an example. Consider the one-dimensional problem illustrated in Figure 2. The system consists of two short columns stacked end to end subjected to a compressive load. Our objectives is to calculate the displacement of the upper column. Clearly, this simple problem can be solved in seconds, either analytically or numerically. In fact, we could readily obtain a finite element solution without resorting to the use of gap elements. But since our purpose is to illustrate their use, we will solve the problem using the finite element model shown in Figure 3.

The finite element model consists of two spar elements, a gap element, and four nodes. The top spar element connects nodes 1 and 2. The lower spar element connects nodes 3 and 4. The single gap element connects nodes 2 and 3 and simulates the interface between the two columns. To maintain the simplicity of the example, each spar element is defined with a unit stiffness and the gap element is defined with a stiffness that is n times that of one spar element. Also, the model is subjected to a unit compressive load.

With the three-element model shown in Figure 3 we will calculate accurate displacements for the nodes attached to the lower spar element, but the displacements calculated for the nodes of the upper spar element will include an error. That error is due to the finite stiffness of the gap element and equals the amount of deflection experienced by the gap element. We must remember that the stiffness of the gap element is a mathematical fabrication. If the value of that stiffness is too small, then the two spar elements will appear to penetrate each other. We could make the gap element arbitrarily stiff, but as we've already mentioned, that could cause bouncing. Therefore, since we are forced to accept some error, it is useful for us to determine the magnitude of that error.

Figure 4 shows a plot of the fractional error in the displacement calculated for node 2. According to the figure, if the stiffness of the gap element is 100 times (two orders of magnitude) greater than the stiffness of one spar element, then the deflection of the gap element (the error) is one percent of the deflection of one spar. In other words, the displacement calculated for node 2 includes a one percent error. If we make the gap element only 10 times (one order of magnitude) greater than the stiffness of one spar, then the displacement calculated for node 2 has a 10 percent error. This is probably more than we could tolerate in a real problem. In fact, in some instances an error of only one percent may be intolerable. Therefore, we must choose the stiffness of gap elements carefully, rather than blindly following a rule of thumb. And we must base that choice on the relative importance of the displacement solution at the contact surfaces.

Examining the Pitfalls of Gap Elements

We have already mentioned that overly stiff gap elements may prevent us from obtaining a solution entirely, by causing bouncing. But there is another more insidious danger associated with overly stiff gap elements. One feature of the gap elements that are included in the Ansys element library is the user-specified option to include a small stiffness in the event that two contact surfaces open. The purpose of this small stiffness is to prevent portions of a finite element model from breaking free, a condition that results in a fatal error message and a premature (though graceful) exit from the program. That small stiffness is calculated as one-millionth of the contact stiffness of the gap elements. But if we define a gap element with an unnecessarily large contact stiffness, then even one-millionth of that contact stiffness can be a substantial value and can cause the model to calculate positive normal stresses for what should be the free surfaces of an open interface. Clearly, this is a condition that must be avoided.

The stiffness of the solid elements in a finite element model, on either side of an interface, can be approximated as (AE/L), where A is the cross-sectional area of the element, E is the modulus of elasticity, and L is the length of the element in the direction perpendicular to the contact surfaces. One way of selecting a stiffness for the gap elements is to simply do the (AE/L) calculation by hand and use a multiple of the resulting value, e.g., 100 times greater. However, this process can become tedious during the course of an analysis conducted with a parametric finite element model, i.e., a model that is defined entirely in terms of variables for the purpose of conducting parametric studies. With such a model, the stiffness value has to be checked with each parameter change because the element sizes may change appreciably. The element sizes also change considerably during a convergence study. Therefore, doing the calculations by hand is less than desirable.

The Ansys Parametric Design Language (APDL) provides a means for conveniently automating the way we define the stiffness of gap elements in parametric finite element models. With APDL, we can have the program do the (AE/L) calculation for us before each run. All that is required is to define a characteristics element length, width, and depth as functions of the appropriate model dimensions and mesh parameters. We illustrate this with a second example.

Figure 5 illustrates the problem of a cube being pushed into a plate. The dimensions of the plate and cube are shown as variables, parameters in Ansys terminology. The parameters within the parentheses indicate the number of mesh divisions for the respective dimensions. APDL lets us define all the variables with simple assignment statements, not unlike the assignment statements that we would use in a Fortran program, as follows: a = 0.09 b = 0.11 c = 0.15 d = 0.05 e = 0.25 f = 0.25

In addition, APDL lets us perform algebraic operations on the parameters. Therefore, we can easily definite the necessary characteristic element lengths as follows: ela = a/nda elb = b/ndb elc = c/ndc

Further, if we denote the elastic modulus as Ex, we can use APDL to calculate the characteristics stiffness of the solid elements as follows: ksol = ((ela*elb)/elc)*Ex

At this point we define another parameter, fact, as the number by which we multiply the characteristics stiffness of the solid elements to arrive at the stiffness value for the gap elements, and we calculate the gap element stiffness: fact = (a number of our choice) kgap = ksol*fact

With this simple method we have automated the calculation of the stiffness of the gap elements and eliminated one possible way of introducing modeling mistakes that could cause errors and unwanted expense.

Gap elements exist because they provide a useful way of simulating contact between objects. But the correct use of gap elements - indeed, the correct use of finite element analysis software - is something that requires considerable care.

PHOTO : Figure 1. Gap elements generate a restoring force only when the gap is closed. The magnitude of the restoring force depends on the stiffness and the interference.

PHOTO : Figure 2. An example problem of two columns stacked end to end and subjected to a compressive load is used to demonstrate the effect of the gap stiffness on a finite element solution.

PHOTO : Figure 3. The finite element model used to solve the example problem consists of two spar elements of unit stiffness and a single gap element with stiffness n times that of one spar.

PHOTO : Figure 4. The displacement error caused by a closed gap element can be controlled by carefully defining the gap element's stiffness. However, gap elements that are too stiff may prevent the solution from coverging.

PHOTO : Figure 5. The Ansys Parametric Design Language makes it possible to define the stiffness in terms of the other variables in the finite element model. Therefore, changes in the mesh size are automatically reflected in the gap stiffness.
COPYRIGHT 1991 American Society of Mechanical Engineers
No portion of this article can be reproduced without the express written permission from the copyright holder.