Boundary conditions are the stage at which many engineers make incorrect assumptions. They are one of the least understood topics for FEA beginners, and even experienced engineers can have difficulty defining them properly. This Book Byte explains what boundary conditions are, the role they play, the types of constraints and loads, and a strategy to define, test and validate them.
Why boundary conditions deserve attention
Boundary conditions have a major impact on the results of an analysis. A small mistake in their definition can make the difference between a correct and an incorrect simulation. To define them properly, you need to follow a strategy that lets you test and validate them.
What is a boundary condition?
Practically speaking, a boundary condition is the setting of a physical state on a portion of a model. The boundary can be a point, an edge or a surface, and the boundary condition is a known value of a displacement or a loading.
To properly understand boundary conditions, it is absolutely necessary to relate them to reality.
Why do we need boundary conditions?
Without boundary conditions, there would be an infinite number of solutions to the system of equations the solver has to compute. Specific boundary conditions allow the solver to generate a unique solution.
What role do boundary conditions play?
The role of boundary conditions in the simulation process includes:
- Fixing the value of displacements in a specific region of the model
- Applying representative loads in a specific region of the model
- Replacing a part that is not modeled, to simplify the model
The different types of boundary conditions
There are three types of boundary conditions:
- Constraints: remove an equation from the stiffness matrix.
- Loadings: represent an input to the FEA (force, moment, pressure, gravity, acceleration, velocity, temperature, and so on). They do not add stiffness to the FEM.
- Contact: defines the interactions between components of a model.
Using boundary conditions to constrain a model
Practically speaking, boundary conditions are applied to the FEM by imposing constraints on certain degrees of freedom. These boundary conditions must be representative of the physical conditions of the modeled part.
Such constraints are imposed using single-point constraints (SPCs) on up to six degrees of freedom to ground the model. In addition, FEA software offers the capability of creating linear constraint relationships between several degrees of freedom, using multi-point constraints (MPCs).
Modeling errors that can produce mechanisms
- Unintentionally omitted constraints
- Discontinuities in the structure (nodes disconnected by meshing)
- Improperly defined rigid body elements or MPCs
- Incompatible degrees of freedom between elements
- 1D truss elements used to resist bending loads (the truss element has only axial stiffness)
- A pinned-pinned 1D beam element with all three rotations released at both ends
- A 2D shell element without bending properties (membrane)
- Too large a stiffness variation between adjacent elements
- Improperly defined material properties
Constraint types
The degrees of freedom describe how a model is free to move. In mechanical analysis, there are six degrees of freedom: three translations and three rotations. By removing some degrees of freedom with a boundary condition, the model is constrained in one position. Constraints can be applied at one or several nodes of the model.
| Constraint | Degrees of freedom removed |
|---|---|
| Fixed constraint | 3 translations and 3 rotations |
| Support constraint | 3 translations and 2 rotations |
| Pinned constraint | 3 translations |
| Roller constraint | 2 translations and 2 rotations |
Loadings and constraints may be ineffective
For the element degrees of freedom, a fundamental rule must be considered: a boundary condition cannot load or constrain a degree of freedom that is not supported by the elements to which it is applied. The solver ignores these loadings or constraints.
Not all degrees of freedom are necessarily active at a node. The degrees of freedom available at a node depend on the type of element it belongs to:
| Element type | TX | TY | TZ | RX | RY | RZ |
|---|---|---|---|---|---|---|
| 1D truss | Yes | No | No | Yes | No | No |
| 1D beam | Yes | Yes | Yes | Yes | Yes | Yes |
| 2D membrane | Yes | Yes | Yes | No | No | No |
| 2D plate | Yes | Yes | Yes | Yes | Yes | No |
| 3D solid | Yes | Yes | Yes | No | No | No |
Properly defining boundary conditions
First rule: boundary conditions are never perfect
Defining the right boundary conditions will be one of the most complex problems you have to solve. There will always be discrepancies compared to reality. The boundary conditions you define only need to simulate the structure well enough to achieve your goal.
Don't be afraid to experiment: with boundary conditions, it is not uncommon for your first assumptions to be incorrect.
What you need to determine
To apply the proper boundary conditions, you need to determine:
- The locations where the displacements will be fixed
- Which degrees of freedom will be fixed
- The locations where the loads will be applied
- Which loads will be applied
The seven questions to answer to define boundary conditions successfully
- Where are your structure's supports in real life?
- What are the degrees of freedom of your structure in reality?
- If you apply a certain set of boundary conditions, do you allow or restrict the degrees of freedom that exist in the physical system you are modeling?
- Where are the loads applied to the structure?
- What types of loads are applied to your structure in the real world?
- Can you remove some parts of your modeled structure, replace them with boundary conditions, and still produce a realistic representation?
- Does your structure exhibit contact between some parts?
A strategy for defining boundary conditions
The first step is to guess the boundary conditions and test your hypothesis by running the FEA. The more you refine your FEA skills, the more accurate your first guesses will be. Don't worry if you make mistakes in the beginning: when checking the results, you may realize that the boundary conditions were not right, so change them. The rest of the process is iterative:
- Consider how the structure is supported and loaded in reality.
- Guess the boundary conditions.
- Apply them in your model.
- Run the model.
- Examine the results.
- Do the results line up with reality? If not, modify the boundary conditions and run again.
- If they do, can you improve the results to bring them closer to reality? If yes, modify the boundary conditions and run again. If not, you have determined the boundary conditions.
Over-stiffening and under-stiffening
The two main reasons why boundary conditions may not be realistic are over-stiffening and under-stiffening of the model:
- Over-stiffening: the model is stiffer than the real structure. The model deforms less than the real structure would.
- Under-stiffening: the model is less stiff than the real structure. The model deforms too much compared to the real structure.
The types of loading
| Loading type | Definition | Application region |
|---|---|---|
| Enforced displacement | Direction and magnitude are defined by entering the components of a vector. | Vector defined at one or several nodes |
| Concentrated forces and moments | Direction and magnitude are defined by entering the components of a vector. | Vector defined at one or several nodes |
| Distributed load on a line element | Applied to 1D truss or beam elements | 1D elements |
| Pressure load | Applied to a surface in terms of three or four nodes, to a 2D shell element, or as a general-purpose pressure load on a 2D element or the surface of a solid element | Surfaces and faces |
| Gravity | Gravity vector. The forces applied to the structure are based on the mass distribution in the model. | Inertia load applied to the entire model; no application region is required |
| Velocity | Translational and rotational velocities across the structure. The forces are based on the mass distribution in the model. | Vector defined at one or several nodes |
| Acceleration | Translational and rotational accelerations across the structure. The forces are based on the mass distribution in the model. | Vector defined at one or several nodes |
| Thermal load | Thermal field across the structure | Scalar value defined at one or several nodes |
Go further
This Book Byte is taken from Chapter 11 of Practical Finite Element Analysis for Mechanical Engineers by Dominique Madier. The topic is covered in depth, with worked examples, in the on-demand course Practical Basic FEA.
See the Practical Basic FEA course Take the free FEA diagnostic