top of page
  • SimulaX

Understanding loads, boundary conditions and time-steps

Updated: Aug 6, 2023

In this blog post, we will explore the relationship between loads, boundary conditions in the form of stiffness matrix, convergence, time-steps, and how they all connect. By using easily understandable examples, we will clarify the connections between these concepts. In just a short 5-minute read, you will gain a better general understanding of these phenomena and their practical applications in real life.


  1. Loads and boundary conditions

    1. External forces and displacement

    2. Boundary conditions

  2. Time steps

    1. What are steps and increments?

    2. How does the software calculate these?

    3. Solution convergence criteria

Loads and boundary conditions

In the context of FEM, "loads" refer to external forces and external displacements meanwhile, boundary conditions are constraints and supports. The stiffness of a component is determined by its material properties, while the behavior and response of the structure under various conditions are influenced by the applied loads and boundary conditions. Loads and BC's are essential in FEM as they provide a way to incorporate real-world constraints and behavior into the analysis. What are key benefits of using them?

  • Realistic representation: Loads, BC's help capture the physical behavior of a structure or system. By specifying them appropriately, you can simulate how the structure interacts with its surroundings or how it responds to external forces and constraints. This allows for a more realistic representation of the problem under consideration.

  • Constraints and supports: Boundary conditions enable the modeling of various types of constraints and supports. For example, you can define fixed supports, rollers, or prescribed displacements at certain boundaries to represent how the structure is connected or constrained in reality. By incorporating these conditions, you can accurately predict the response and behavior of the structure under different loading conditions.

It is critical to apply the correct boundary conditions as restricting motion in a direction in which the body is actually free to move or expand, will yield false results compared to reality. Wrongly applied loads can also be catastrophic if the deformation is displacement driven in reality but force load is applied in the simulation. Keep it in mind, that loads are simulation type specific: thermal loads are not available in a structural simulation and vice versa (unless they are coupled of course).

Below you can see the representation of a boundary condition and applied loads. The beam is fixed in all direction at the left end, meanwhile force is applied to the right end, causing the beam to deflect.

Loads and boundary conditions
Left: Applied boundary conditions; Right: Resulting displacement of the beam

The easiest way to think about loads and BC's is by using the basic FEM equation: {F}=[K]{x}. Once the movement of one node into one direction is restricted, that value becomes zero in the {x} matrix and therefore, the corresponding values in the stiffness matrix [K] cancel out. On the other side of the equation, the force {F} is not calculated on that node in that direction since displacement is restricted and reaction forces would be zero.

The basis of the problem is a 1D beam element with 2 nodes and 3 DOF's at each end.

1D beam element degree of freedom
1D beam element with 2 nodes and 2x3 DOF

Below, you can see the representation of the above described schematic in the form of actual equations. Note, that this [K] is the element stiffness matrix and the simulation transforms it into the global one where all the nodes are connected.

The previously presented small {F}=[K]{x} equation can be expanded into it's full form that describes the behavior of the 1D beam element.

2D beam element stiffness matrix

The single values of the matrix [EI/L] are not derived here as that's not the focus of this post and can be found in every FEM academic book. However, important to note that these are calculated using Euler-Bernoulli beam theory in combination with the shape functions of the beam element. Given that Euler-Bernoulli beam theory is applicable solely to small deformations, it is logical to conclude that this method will only hold true within the context of linear analysis.

Euler-Bernoulli beam equation
Moment (M) and transverse force (V) equations formulated using Euler-Bernoulli method

In beams, axial stress is absent unless an axial load is applied to its ends (axial direction: u1 and u2). In most cases, there is little justification for exerting such a load, and the primary stresses occur in compression and tension due to bending as a result of transverse loads. These stresses vary throughout the beam's cross-section, reaching a minimum at the neutral axis and a maximum at the outer fibers of the beam.

Stress representation in a beam section
Section of a beam in bending with transverse forces and moments

Therefore, the full matrix reduces to the following where only transverse displacement and rotation is present:

2D beam reduced stiffness matrix

Now that the general formulation of the matrix has been established, the boundary conditions and loads can be applied to the stiffness matrix. The left side of the beam is fixed (imagine that it's built into a wall), meanwhile a transverse point load (P) is applied to the right side.

2D beam boundary conditions

In order to achieve equilibrium in the beam, forces must counterbalance each other, therefore V=P=F2y. Moment (M) can be calculated by M=P*x. Since transverse displacement and rotation is zero on the left side, these can be cancelled out and the equation reduces to:

2D beam stiffness matrix with applied boundary conditions

It is a 2-by-2 matrix with 2 unknowns: v2 and θ2 which we can easily solve for!

After understanding the working principle of FEM and familiarizing yourself with the concept, you might wonder about the various types of loads and boundary conditions involved in FEM.

External forces and displacements: These are forces, pressures, or displacements applied to the structure from the outside.

  • Point loads: Concentrated forces or displacements applied at specific locations at single points.

Point load
  • Distributed loads: Forces or pressure applied over an area or along a line. The distribution of the load can be constant, linearly varying or dependent on an equation.

Distributed load
  • Surface loads: Forces or pressure applied over the entire surface of the structure.

Surface loads
  • Thermal loads: Applied temperature at certain nodes, surfaces, volume of the assembly or body. The applied temperature can cause heat transfer or thermal expansion/contraction in a structure. Heat transfer can only happen through elements with shared nodes.

Thermal loads
  • Inertial forces: Forces resulting from the acceleration or deceleration of mass. It is relevant in case of quickly moving structure, drop or impact simulation, crash tests.

Inertial forces

Boundary conditions: These represent the constraints or fixed conditions applied to the structure, which restrict its movement or behavior.

  • Displacement constrains: Restricting the movement or displacements of specific points or regions into specific directions!

Displacement constraint
  • Support conditions: Fixing certain points, surfaces to prevent any movement. Fixed support indicates no movement in any direction on the applied surface. (Fixed support was used in the above examples at the left side of the beam)

Support conditions
  • Symmetry conditions: This can be applied to reduce the size of the model if possible. This boundary condition can only be applied when the problem is symmetric and the pattern is repetitive, meaning that 1/2 or 1/4 etc. of the body is modelled and symmetry boundary condition is applied. This way, the software calculates results taking the effects of the rest of the model into account as if those were present too. The advantage of the boundary condition is that modelling 1/4 of the model will reduce the time and computational power to 1/4.

Symmetry conditions

The goal of the described relationship between loads and stiffness matrix is to provide the reader a simple explanation for the working principle. By using appropriate boundary conditions, you can limit the analysis to the region of interest and exclude unnecessary areas. This reduces the size of the problem and, consequently, the computational effort required for the analysis. This is of course one of the simplest explanations possible, and loads can actually make life really difficult as well by accounting for contacts between bodies in the model or applying a sudden large force that will severely deform the body. In these cases we can't talk about a linear approach anymore but a non-linear one in necessary and the presented stiffness matrix explanation does not hold true anymore.

Significant large loads can give rise to additional challenges. Achieving convergence, which refers to finding a solution, becomes more difficult during non-linear analysis and time steps, increments play a crucial role in such cases. In the following, you can read about these phenomenon and their link to applied loads!

Time steps

In order to understand steps and increments, it is crucial to understand convergence in simulations. Convergence is achieved when the basic {F}=[K]{x } equation is satisfied, but when is it satisfied? External forces are applied to bodies in the software, and the body reacts to those forces with displacements (the nodes move w.r.t each other). Next, the stiffness matrix is evaluated (is it stiff enough to support the applied load?) based on that, reaction forces (internal forces) are calculated. Convergence is reached when the internal forces and external (applied) forces are in equilibrium (equal) or with other words, when the difference (residual forces) is zero.

Convergence criteria

Convergence, time-steps, increments and loads are closely related. Each of the load is applied in a separate time-step which is then broken down to increments to achieve convergence. How is this all done?

Steps and convergence
Relationship of loads, steps, increments and convergence

What are steps?

Step refers to the number of applied loads in the simulation. As many steps can be applied as needed depending on the loads and boundary conditions. Sequence of loads can also be applied and the number of steps would be equal to the number of applied individual loads.

What are increments?

Imagine that 10 [kN] force is applied to the body in 1 step. How would it react if it had to be solved right away with 1 increment? The simulation would not be able to cope with the sudden applied load, elements would distort due to the sudden large deformation and an error message would appear. Therefore, the software breaks down the applied load to small "steps" so called increments. Increments can be imagined as the sub-version of steps and each step can contain several hundreds and thousands of increments if needed. The number of increments in 1 step is independent of the number of increments in the next one. The solver will always try to use the least amount of increments and its only a question of how successful that is. Since the load has been broken down to small portions, it is now a lot easier for the software to find that equilibrium in each of the nodes in each of the increments slowly.

What are iterations?

Within each increment, the software compares the external and internal forces (Residual force) and it iterates until equilibrium is obtained.

What are attempts?

When the iteration is not successful, the software applies a cutback and decreases the increment size to a smaller one and tries again. The more often it tries the more attempts are counted. Once the limit is reached, the simulation terminates.

This description provides any individual a representation of what happens but

How does the software actually calculate all these?

time increments in FEM

Engineers must specify the length of the step and the extremes of increments (initial, min and max values). Lets say we want to simulate 1 [s] with initial=0.01 [s], min=0.001 [s] and max=0.1 [s] increments.

What it really means is that simulation will start out with 0.01 [s] since that's the initial value (here the number of increments would be 1/0.01=100). If the software finds equilibrium then this value can be increased up to 0.1 [s] (as that was our max value). In this best scenario, the simulation would be solved in only 10 increments compared to the initial 100. Now we just described what happens when convergence is found and the max values can be used, but lets look at the more common scenario when things don't converge.

When there is a sudden change in the simulation (stress concentration, sudden contact, material reaches nonlinear values) the force equilibrium can't be found easily. What happens then? When there is no equilibrium between the forces, the software uses an equation (based on the force difference and stiffness) to predict the next increment that might be suitable for convergence. Based on the prediction, the software tries to break down the applied load to smaller increments (this is when the minimum set value comes into the picture).

steps increments convergence relationship

Increment size can be decreased to as small as the min value (the smaller the value the smaller portion of the load is applied at once so the higher the chance is for convergence, but the longer it takes because more increments are generated). The software then calculates the corresponding internal forces and compares them to external ones to search for equilibrium. In principle, it does that as long as equilibrium is not found. It happens that the minimum value is reached and equilibrium is not found: that's when we say the simulation is not converging!

Solution convergence criteria:

In FEM, the convergence criteria typically involve comparing certain quantities between consecutive iterations of the solution process. These quantities can include the displacements, stresses, strains, or other relevant variables of interest. The convergence criteria aim to assess whether the solution has converged to a stable and consistent result, indicating that further iterations will not significantly change the solution. In reality, it would be nearly impossible or an infinite number of iterations would be needed to obtain perfect equality. Therefore, the convergence criteria are usually defined by setting tolerance values, which determine the acceptable level of deviation between consecutive iterations. If the solution satisfies these tolerance values, the analysis is considered converged.

Tolerance values are set by the engineer. The smaller the value is, the longer it takes to find equilibrium in each elements. On the contrary, the larger value is set, convergence is found faster but the result will be less precise. It is difficult to estimate a correct value but 10e-6 is a reasonably common relative tolerance.

Convergence issues are common in FEM software and in order to find the problematic area in the simulation, one must understand the connection between all these phenomenon. Boundary conditions will reduce the size of the stiffness matrix and hence the problem if applied correctly, but a wrongly applied BC can over-constrain the model and will also terminate the simulation. Small loads will converge in seconds but large deformations require non-linear solver and smaller increments. Hence, more power and time to find a solution.

This topic is as complex as it gets and this post was just an introduction to the topic of loads, boundary conditions and time-steps!

Recent Posts

See All


bottom of page