Explicit Dynamics and Ansys: Part I

November 12, 2020

What is the Explicit Method?

In the last 15 years, Ansys has gone from offering a single explicit dynamics workflow, using Mechanical APDL with a third-party solver and postprocessor, to offering several unique and versatile solutions. These days Ansys customers can leverage two distinct solvers and multiple pre and post processors in various combinations in order to best meet their needs. However, before a user can determine the right explicit solution for themselves, they must first understand what the term “explicit dynamics” means and what sort of problems that methodology is meant to tackle.

Implicit vs. Explicit Methods in FEA

Traditionally, finite element analysis of a transient structural system is carried out using an implicit solutions method; this approach involves two key principles:

  1. The assembly of the mass, stiffness, and damping matrices to describe the inherent factors relating to the motion of the structure.
  2. The approximated solution an ordinary differential equation describing that motion:

CaptureFor those inclined to stare blankly at the first sign of math, this equation of motion essentially shows that any external force acting on an object will result in displacement (u vector), velocity (v vector) and acceleration (a vector) of that object. The magnitude of that motion will be inversely related to the stiffness in the system (K matrix), the amount of damping (C matrix), and the mass of the system (M matrix). You can think of these matrices as how springy or elastic the material in use is, how much kinetic energy loss occurs due to heat or sound, and how much resistance to a change in velocity exists respectively. Things get further complicated by the fact that displacement, velocity, and acceleration are all interrelated in a way that makes these equations very difficult to solve directly.

The other significant concept here is the use of matrices to define behavior of a complex system. Since FEA in general involves a component or assembly of components that are broken down into many nodes with many more connections to adjacent nodes, the equations of motion for each node starts to get complicated very quickly. Matrices are a way to describe these complex systems in an organized way that allows a solver to take advantage of certain operations possible in linear algebra.

Consider this 1-dimensional system of springs and nodes. Note that we are only considering the elastic (displacement-related) portion of the motion equations and not inertial (acceleration) or damping (velocity):

The total force acting on, and displacement of each node is going to be related to the relative displacement of the adjacent node or nodes and the stiffness of the springs connecting them. Using a stiffness matrix, we can describe the behavior of the entire system mathematically:

CaptureThis might look somewhat familiar if you look at the first part of that motion-equation we looked at earlier. In this case, we’re looking at the global stiffness matrix of a simple system as opposed to the matrix of a single node or object. The stiffness between nodes in a finite element model can be thought of as being very similar to the springs’ stiffness in our simple system, and the mass of the system and damping properties can be thought of very similarly to the stiffness in terms of matrix assembly.

So, where are we going with all this? Well, FEA software uses a linear algebraic approach to simplify these matrices before attempting to solve the full equations of motion of the system. In fact, much of the CPU time consumed during the solve process is taken up by this matrix “decomposition” as it is known. Additionally, because the full transient equations of motion can’t easily be solved directly from one point in time to the next, a set of values known as Newmark’s Parameters are used to approximate an incremental change of displacement, velocity, and acceleration between time-steps. The most common method of leveraging these parameters is known as the Newton-Raphson iteration, and involves an iterative approach to solving for the force on any node in the system.

It works like this: the starting position, velocity, and acceleration of the system are known, so the matrices at this state act as our starting point. For the first time increment, a set of matrices modified using the Newmark’s Parameters are formulated and a test force is applied at each node. This test force will result in a new set of positions, velocities, and accelerations at each nodal location. This newly calculated equilibrium state will also result in a new set of calculated forces at each node, and this calculated force can then be compared to the test force. Usually the first iteration will not result in values that fall within a range resulting in an acceptable residual value, so the matrices will be further modified from this first attempt and the process will repeat. This same process repeats until the test force and the calculated force are close enough to be considered converged.

Picture2That, in a nutshell, is how the implicit transient method works. In contrast, explicit dynamics takes a different approach to solving motion equations altogether. Instead of using a test force value and incrementally adjusting the system matrices until that test force value matches the resultant equilibrium forces, the explicit approach involves simply integrating the acceleration and velocity terms in the equations over a short period. This results in equations that are defined in terms of displacement alone, meaning they can be solved without the need for convergence toward a solution! Not only that, but this approach also bypasses the need for matrix assembly and decomposition as well, meaning no need for the solver to spend all that time building and simplifying a matrix.


By getting rid of these two often onerous steps, the explicit method allows users to tackle highly complex and nonlinear problems that would otherwise be very difficult to converge (and in many cases it can do so much, much faster). In fact, the Explicit method can be used for some very sophisticated analyses, such as simulating breakage (elements being deleted from the simulation) based on a limit strain value, because the solution at a timestep does not need to converge based on the state of the system at a previous step.

You might be thinking, “Great! Clearly the explicit method is superior. Why wouldn’t we use that approach for everything?” Well, here is the rub: explicit study requires that the analysis be both time-dependent (or transient), and that a minimum time step size be used. The explicit dynamic EOMs are probably not worth showing in their entirety, but one particular term is the issue here:

That innocuous-looking little term might look familiar if you know the equation for the natural frequency of an oscillator:

CaptureThe significance here is that if the timestep of the explicit analysis, identified here as Δt_i, is longer than the shortest period corresponding to the natural frequencies of the system divided by pi, the motion equation becomes unstable and can’t be solved.


The natural frequencies of the system are sensitive to numerous factors, most significant here are that this period for the natural frequency will decrease with:

  1. Increasing material stiffness
  2. Decreasing material density or decreasing mass
  3. Decreasing size of the SMALLEST element in the entire model

Therefore, the stiffer, more massive, and smaller that smallest element in the model is, the shorter our timestep needs to be to get a solution. And these timesteps can be a tiny fraction of a millionth of a second in many cases! Therefore, even though the Explicit method is a more direct way of solving the equations involved, depending on the problem involved, it might still be more efficient to approach with an implicit solver because of the numerous timesteps necessary for an explicit solution.

Here’s the Bottom Line

The Implicit approach is still a robust and reliable method for solving FEA problems, and usually is the more time and effort-friendly approach for static cases or those that don’t involve much nonlinearity. However, whenever a simulation involves very rapid changes to the state of the model, involves large amounts of deformation or material nonlinearity, or deletion of elements based on material failure, the explicit method excels.

CaptureHigh/Hyper-Velocity Impact and Material FailureCaptureFoam and other Highly Non-linear Material



Explicit dynamics can also be very useful for simulating snap-through behavior, metal forming operations, and any number of other events that might otherwise be impossible with the implicit approach. In part 2, we will explore the Ansys Explicit Dynamics portfolio and discuss how each software stacks up against the others in some key areas.

Previous Article
Acoustic Analysis in Ansys Mechanical
Acoustic Analysis in Ansys Mechanical

In the minds of many engineers, Ansys Mechanical can be used solely to address the behavior of solids. Howe...

Next Article
Explicit Dynamics and Ansys: Part II
Explicit Dynamics and Ansys: Part II

Which Explicit Tool is Right for Me? In my Explicit Dynamics and Ansys: Part I blog post, I discussed the f...

Get help from FEA & structural experts

Learn More