you are here:   / News & Insights / Engineering Advantage Blog / How to Model Foundation Supports

Engineering Advantage

How to Model Foundation Supports

Foundation Soil Structure Interaction under Seismic Loading | FEA Consulting
June 26, 2015 By: Peter Barrett

Whether you are analyzing a tall building, a concrete dam or an electronics cabinet, often one of the most critical finite element modeling decisions is how to simulate the foundation support. The underlying structure support (concrete, rock, soil etc.) and analysis accuracy requirements will dictate the best foundation modeling assumptions. This blog summarizes some of my recommendations from 30 years of modeling foundation supports.

Finite element analyses are often performed under the assumption that the base support is a rigid fixed boundary condition. Take an electronics cabinet that is bolted to a 3 foot thick concrete basement floor, or a building foundation system that extends to solid bedrock. For these cases, a fixed support is a reasonable assumption for most loading conditions. Since a fixed support is easy to implement, I recommend starting with the fixed support in most models, even if a more accurate flexible foundation stiffness needs to be accounted for, since it provides a benchmark for comparison purposes.

If temperature loads need to be accounted for, fixing all the base nodes in all directions will result in large unrealistic stresses since thermal expansion at the boundary is restricted artificially. A frictionless vertical support coupled with local lateral constraints can be used to eliminate this over-constraint. Lateral constraints should be positioned to prevent rigid body motion while allowing for thermal growth. I suggest that the added supports are defined to take into account the anticipated shear load transfer mechanism. Lateral supports at discrete bolt supports, pile locations, shear walls etc. coupled with the vertical constraint on all nodes on the bottom of the foundation would be an example of this type of boundary condition.  Weak springs can also be placed between the lateral support points and ground as necessary if over-constraint still occurs.

If the stiffness of the foundation is similar to that of the structure or a non-uniform support is present, then the frictionless support assumption needs to be replaced with a more explicit model of the foundation. The simplest method is an elastic foundation support. In many finite element programs, the elastic foundation can be prescribed as a force/length/unit area (See ANSYS Surface Effect Elements for example). The advantage of these elements over individual springs is that they automatically adjust the spring support stiffness for a variable size mesh.

When overturning loads are present due to wind or seismic conditions, it may be necessary to simulate the possibility of uplift and/or lateral sliding. If either of these conditions are present, then frictional contact elements are typically used to capture the uplift and sliding behavior. For complex structures which require a nonlinear transient analysis, simplifying the superstructure model to a beam-mass equivalent model can save significant computational time. Modeling of the underlying foundation is best served with a mesh of continuum and/or shell elements on either side of the contact interface, coupled with an elastic foundation to approximate the underlying soil. Figure 1 above illustrates a soil-structure interaction (SSI) response using contact interface elements where significant uplift and sliding response is captured.

For lateral soil supports where the foundation is buried in relatively soft soil, accurate modeling of the nonlinear SSI might be required under seismic loading. One method for simulating this foundation support is to utilize interface elements such as ANSYS's INTER195.  This element was originally developed to model gaskets, but can be adapted to model lateral soil constraints, since it has the capability to simulate a series of unique loading and unloading curves. A thermal load can be added to create an initial back pressure, such that the side wall is initially in a state of compression.  Unique loading and unloading stiffness curves are used to simulate the reduced stiffness where the earth pressure disappears as the foundation moves away from the existing soil.  Figure 2 illustrates an example soil pressure vs. displacement input response where the vertical axis represents the equivalent pressure imposed from the soil onto the wall and the positive horizontal axis represents the relative normal compressive displacement between the wall and the soil.  In this example, soil crushing occurs at a factored pressure coefficient = 3.0 (a flat curve after this point) and a reversal of displacement due to unloading is illustrated to occur (near vertical unloading slope) when the relative lateral displacement reaches 3 inches.

Figure 2 - Example Side Wall Pressure vs. Deflection using Interface Elements

However one decides to model their foundation supports, I recommend a sequential analysis approach, starting with the fixed support and adding complexity as needed, while referencing the simplified models along the way for validation and sanity check purposes. A check against actual test data is always helpful, when possible.

How do you model foundation supports?  I would love to hear from others about their approaches.