Differences between ABAQUS Standard & ABAQUS Explicit

Figure 1: Procedure types in Abaqus

2. What is Abaqus Implicit (Standard) Solver?

When we talk about “Abaqus Implicit solver”, we’re usually referring to the Abaqus/Standard solver. This solver uses an implicit time integration scheme. The implicit time integration scheme is used for static or slow-moving systems. It calculates the system’s response at each time step using information from current and previous steps, solving for unknowns like displacement or velocity simultaneously, which is great for taking on a variety of challenges! It can tackle both linear and nonlinear problems and is well-equipped for static analysis, dynamic simulations, and even certain cases of heat transfer and mass transport. The goal of the solver is to find an equilibrium solution for each time step by using some nifty iterative methods.

In Abaqus, an equilibrium solution is the state where internal forces (stresses) balance external forces (applied loads), indicating stability without further movement. For equilibrium:

1. Force equilibrium: Total external forces must equal internal forces.
2. Moment equilibrium: The sum of all moments around any point or axis must be zero.

Abaqus checks for equilibrium by solving for displacements and stresses, which is crucial in static analyses focusing on the final deformed shape and stress distribution.

Abaqus/Standard comes with a range of implicit analysis procedures, each crafted for different kinds of problems. Here’s an overview of the key Abaqus implicit steps, organized by the type of analysis and procedure:

2.1. Static, General Step

The Static General procedure in Abaqus/Standard is widely used for static analysis of structures, ideal for gradual loads or boundary conditions until equilibrium is reached. It helps analyze structural deformation, stress distribution, and static loads in both linear and nonlinear systems.

When setting up a static general procedure, the Edit Step dialog box displays three tabs—Basic, Incrementation, and Other (fig 2)—allowing you to customize settings like the time period, maximum increments, increment size, load variation, and geometric nonlinearity. We explore these options to tailor the procedure!

Figure 2: Static, general procedure

You can easily set up important settings like “Nlgeom” and “stabilization” using the Basic tabbed page. Let’s walk through it step by step!

1. Choose your Nlgeom option:

   – If you select “Off,” you’ll be running a geometrically linear analysis for this step.

   – If you’d like ABAQUS/Standard to factor in geometric nonlinearity, select “On.” Just remember, once you turn Nlgeom on, it stays active for all the next steps!

2. If you’re expecting any local instabilities (local instabilities refer to situations where a structure or a component experiences sudden, uncontrolled deformations in a localized region.) like surface wrinkling or local buckling, go ahead and toggle on Use “Stabilization” (fig.3). This feature helps ABAQUS/Standard stabilize those tricky areas by applying damping throughout the model.
3. If you have turned on Use Stabilization, click the arrow of the combo box to choose a method for defining the damping factor (fig 3):

   – You can opt for the dissipated energy fraction, which allows ABAQUS/Standard to calculate the damping factor based on a fraction you provide. Just enter the value in the adjacent field.

Figure 3: Apply stabilization

4. If you’re conducting an adiabatic stress analysis (Adiabatic stress analysis studies stress and temperature changes in a material or structure under conditions without heat exchange between the system and its surroundings.), don’t forget to toggle on Include Adiabatic Heating Effects (fig 4). This is only relevant for isotropic metal plasticity materials that have a Mises yield surface.

Figure 4: apply adiabatic heating

Nex in the Incrementation tab to easily configure your increment size and the maximum number of increments. Here’s a guide to help you through the process:

1. Automatic Type:

   – If you prefer some flexibility, select Automatic. This lets ABAQUS/Standard decide on the best increment sizes for efficiency (fig 5).

Figure 5: Choose Automatic type

   – In the “Maximum number of increments” field, you can set an upper limit for how many increments are allowed in this step. Just keep in mind that if this limit is exceeded, the analysis will stop before ABAQUS/Standard finds the complete solution.

   – Initial: Enter your starting time increment here.

   – Minimum: Enter the smallest time increment you’d like to allow.

   – Maximum: Set your upper limit for the time increment here.

2 – Fixed Type:

   – Want full control? Go for Fixed! This option lets you set a constant increment size that will be used throughout the step (fig 6).

Figure 6: Apply Fixed incrementation type

Figure 7: Equation Solver Method

3. Handle Severe Discontinuities:

   Click the arrow next to the “Convert severe discontinuity iterations” field and choose how to approach severe discontinuities during your analysis (fig 8):

   – Off: Start a new iteration if any severe discontinuities pop up.

   – On: Let ABAQUS estimate residual forces related to these discontinuities, checking if equilibrium tolerances are being met. This might allow for convergence in some cases.

   – Propagate from the previous step: Use a value from the last general analysis step.

Figure 8: Handle Severe Discontinuities

4. Extrapolate Previous State:

 Click the arrow next to the “Extrapolation of the previous state at the start of each increment” field and select a method. The method determines how Abaqus predicts the starting point (initial guess) for the solution in the current increment based on the results from the previous increment. A good initial guess can significantly speed up convergence in nonlinear problems (fig 9).

   – Linear: Abaqus extrapolates the displacement and stress states linearly from the previous increment to predict the initial conditions for the current increment. This is typically more efficient and helps accelerate convergence, especially when the system is behaving smoothly.

   – Parabolic: Use a quadratic extrapolation based on the last two increments.

   – None: Skip the extrapolation altogether.

Figure 9: Extrapolate Previous State

2.2. Dynamic Implicit Abaqus

“Dynamic Implicit Abaqus” describes a time integration method in ABAQUS/Standard for dynamic problems. It computes next time step values using current and previous values, allowing for larger time steps than explicit integration. However, it requires solving nonlinear equations at each step, making it suitable for structural problems where stability and time step control are crucial.

When you’re setting up a “dynamic, implicit” procedure in ABAQUS, you’ll see three tabs in the step editor: Basic, Incrementation, and Other. These tabs let you adjust important settings like the time period, increment size, and solver preferences for your analysis.

Basic Tab Settings (fig 10):

The Basic tab settings are all like the ones in the “Static, General” step. But let’s see its applications.

       1. Application:

• Transient fidelity specifically relates to how accurately the dynamic implicit Abaqus solver can capture a system’s time-dependent behavior, especially under dynamic loading conditions, such as impacts, vibrations, or other transient effects. It reflects how well the solver can model the time evolution of quantities such as displacement, velocity, acceleration, and stresses during a dynamic event.
• Moderate dissipation involves adding a controlled amount of artificial damping to the system. This helps to remove high-frequency oscillations or numerical noise that can arise in dynamic problems, particularly those with rapid loading or unstable modes of vibration.
• Quasi-static in Implicit Dynamic in Abaqus refers to using a dynamic solver to handle time-dependent nonlinear behavior but neglecting inertial effects. Thus, the problem is effectively treated as a slow-static problem while still benefiting from the robustness of implicit integration and the ability to model complex nonlinearities.

2. For adiabatic stress analysis (only for isotropic metal plasticity with a Mises yield surface), toggle Include adiabatic heating effects.

Figure 10: Dynamic Implicit basic tab settings

Incrementation Tab Settings are also like the ones in the “Static, General” step. In this step, optionally, you can toggle on Suppress half-step residual calculation to speed up the solution.

Figure 11: Incrementation Tab Settings

Figure 12: Other Tab Settings

By following these steps, you can ensure your dynamic analysis is set up to meet your specific needs, whether you’re focusing on accuracy, computational efficiency, or both.

3. What is the Abaqus Explicit Solver (Dynamic and Dynamic, Temp-Disp, Explicit)

In Abaqus, explicit solvers are used for dynamic events like impact, crash, or fluid-structure interactions, where large deformations and high strain rates occur. Dynamic, Explicit, and Temp-Disp Explicit refer to different analysis procedures, with the main difference being the inclusion of thermal effects in Dynamic and Temp-Disp, which is essential for heat transfer scenarios. Both share the same solver settings. Here are the main settings for explicit solvers in Abaqus:

3.1. Abaqus Dynamic Explicit

An Abaqus dynamic Explicit step is a type of analysis step used to simulate highly dynamic, transient problems involving large deformations, high strain rates, or complex contact interactions. Unlike implicit methods, explicit methods directly solve the equations of motion and are well-suited for problems involving impacts, crashes, explosions, or other fast-changing events. Let’s explore the configuration options available in the Edit Step dialog box for setting up a Dynamic, Explicit procedure in Abaqus! Here’s a guide to help you navigate the different tabs and make the most of your settings:

Basic Tab: Like the general statics, this Tab is designed to solve problems (Fig 13).

Figure 13: Basic settings for dynamic Explicit Abaqus

Incrementation Tab:

Like other solvers, the incrementation tab is divided into two types: fix and automatic.

Automatic incrementation is essential when simulating problems with complex contact interactions (e.g., impacts or collisions), where large changes in forces and velocities occur rapidly (fig 14).

• A stable increment estimator is used to automatically determine the maximum stable time increment for each analysis step. This time increment is critical because it controls the rate at which the solution progresses through time. The increment must be small enough to satisfy stability criteria, particularly for problems involving high-speed events, large deformations, or complex interactions.
• Abaqus provides several methods to improve the selection of time increments during explicit dynamic analysis. The goal is to achieve a balance between computational efficiency and accuracy while maintaining the stability of the solution. To use this feature you must enable the “improved Dt method”.
• You can define a maximum time increment for the analysis. This is useful to control how finely the time steps are taken. Smaller time increments may improve accuracy but increase computational cost.

Figure 14: Automatic incrementation in Abaqus Explicit

The fixed type in the explicit solver is like the fixed type in general implicit so that you could see in the static, General section.

Figure 15: fixed type in dynamic, Explicit

Mass Scaling Tab:

Mass scaling is often used to artificially speed up the simulation by scaling the mass matrix. This is particularly useful when you are simulating a very long or complex dynamic process but want to make the simulation more computationally efficient (fig 16).

1. Mass Scaling:

1. • Mass scaling can be used to increase the mass of certain elements in the model, which effectively reduces the time steps needed for stable results.
   • You can specify the scaling factor, the regions of the model to apply mass scaling, and the magnitude of the scaling.

Figure 16: mass scaleing

Note: While mass scaling can make simulations more computationally efficient, it should be used with care, as it can alter the physical behavior of the system, especially if applied in a non-physical manner (e.g., scaling mass in regions that experience little motion).

Other Tab:

This tab has an advanced option that can affect the behavior and performance of the simulation.

1. Bulk Viscosity(fig 17):

1. • Bulk viscosity helps control high-frequency oscillations in the results that may arise in explicit dynamics simulations. It applies a damping force proportional to the rate of change of the velocity field.
   • You can configure the bulk viscosity parameter to smooth out high-frequency noise in the solution, particularly in simulations with shock waves or high deformation rates.

Figure 17: other tab for Dynamic, Explicit

5. Abaqus implicit and Explicit Solvers | Abaqus standard vs implicit!

First, I have to say that there are no differences between Standard and Implicit. In fact, these are two names for one solver. The main discussion is about Abaqus Implicit and Explicit solvers.

These solvers are based on two approaches in FEM analysis, namely implicit (for Abaqus/Standard) and explicit. The distinction between the two different numerical approaches makes it possible to understand which solver to use.

Read More: Debugging of ABAQUS errors

In the case of the implicit method, equilibrium is enforced between externally applied load and internally generated reaction forces at every solution step (Newton Raphson method).
In the case of the explicit method, there is no enforcement of equilibrium. But this does not mean that explicit is not accurate. You can minimize its deviation from equilibrium to almost zero by increasing the number of solution steps, i.e. reducing the time step size.
We can list the main differences below:

Implicit is unconditionally stable.
Implicit schema is incremental as well as iterative. However, explicit schema is only incremental (Abaqus Increment).
In terms of cost per Increment, it is costly for implicit and cheaper for explicit. Disk space and memory usage are typically much smaller than that for implicit. The explicit method shows great cost savings over the implicit method as the model size increases:

Therefore, Abaqus/Standard(or implicit) must iterate to determine the solution to a nonlinear problem but Abaqus/Explicit determines the solution without iterating by explicitly advancing the kinematic state from the previous increment. Read More: Abaqus Quasi Static Analysis

[learn_press_recent_courses]

6. Explicit or Standard, Which one should I use?

For many analyses, it is clear whether Abaqus Explicit or Standard should be used. For example, Abaqus/Standard is more efficient for solving smooth nonlinear problems; on the other hand, Abaqus/Explicit is the clear choice for high-speed dynamic analyses such as crash analysis or drop test. There are, however, certain problems that can be simulated well with either program.

Typically, these are problems that usually Standard can solve but may have difficulty converging because of contact or material complexities, resulting in a large number of iterations. For example, in problems where very complex contact conditions or very large deformations are present. Such analyses are expensive in Standard because each iteration requires solving a large set of linear equations.

Until now, we have tried to explain ‘Abaqus Standard and Explicit’ thoroughly so that you can choose the right solver for your needs. Here, you can find Abaqus Examples for training and understand the concept of these solvers and how to use each one properly.

additionally, It would be useful to see Abaqus Documentation to understand how it would be hard to start an Abaqus simulation without any Abaqus tutorial. Also, please share your views with the CAE Assistant experts in the comment section. We really appreciate your feedback, as it helps us improve our tutorials and fulfill all your CAE needs without requiring additional tutorials.

Abaqus CAE is a powerful software tool used for both pre-processing and post-processing in finite element analysis, essential for modeling, analyzing, and visualizing complex mechanical systems.

⭐⭐⭐Free Abaqus Course | ⏰10 hours Video  👩‍🎓+1000 Students   ♾️ Lifetime Access ✅ Module by Module Training                                  ✅ Standard/Explicit Analyses Tutorial ✅ Subroutines (UMAT) Training                    …           ✅ Python Scripting Lesson & Examples …………………………                 …………………….. ……………   ………………………………….Start Free Abaqus Course

You can have the PDF of this post by clicking on CAE Assistant- Abaqus implicit or Abaqus explicit

Thank you for being with us in this article. In order to always provide you with up-to-date and engaging content, we need to be familiar with your educational and professional experiences so that we can offer articles and lessons that are most useful to you.