Abaqus Standard vs Explicit Explained: Pick the Right One

Which one should you use: Abaqus Standard or Abaqus Explicit? If you’ve run into this question while working in Abaqus, you’re definitely not alone.

Abaqus gives you two powerful solvers for finite element analysis—Standard (Implicit) and Explicit. But when you’re dealing with complex simulations, knowing which one to use isn’t always obvious.

Think of it this way:
The Abaqus Standard solver works like a cautious planner. It checks that everything balances—loads, reactions, deformations—before moving to the next step. This makes it perfect for static problems or slower nonlinear simulations.

In contrast, the Abaqus Explicit solver is built for speed. It skips the heavy balancing act at every step and pushes the simulation forward quickly. That’s why it shines in dynamic events like impacts, crashes, or sudden contact.

This blog breaks down the core in the Abaqus Standard vs Explicit debate. You’ll learn:

• How each solver approaches the problem

• The types of scenarios each one is best suited for

• Which solver saves you time (and when)

By the end, you’ll have a clear understanding of which Abaqus solver to choose—and why it matters.

6 hours of professional, in-depth, yet beginner-friendly tutorials, with hands-on workshops to help you apply what you learn. The Abaqus for beginners package is all you need to start mastering Abaqus and become a skilled FEA analyst.

Lesson 1: ABAQUS/CAE Introduction Lesson 2: Finite Element Method Introduction Lesson 3: Different elements introduction in ABAQUS Lesson 4: Types of analysis Lesson 5: Some consideration in EXPLICIT Analysis Lesson 6: buckle and frequency analysis Lesson 7: Heat transfer and Coupled temperature-displacement analysis Lesson 8: Simulation of composite material in Abaqus

1. What Are Implicit and Explicit Methods?

Before we compare Abaqus Standard vs Explicit, it’s useful to understand what implicit and explicit actually mean in simulation terms.

These terms refer to how the solver handles time and motion—specifically, how it steps forward through a simulation.

Implicit Method (Used in Abaqus Standard)

In an implicit method, the solver checks balance at every time step. It solves a system of equations to make sure forces and displacements are in equilibrium. This often involves iterative methods like Newton-Raphson, especially in nonlinear problems.

It’s more stable and allows larger time steps—but takes more computational effort per step.

Want to learn how Newton-Raphson works in detail? Check out this simple breakdown.

Explicit Method (Used in Abaqus Explicit)

An explicit method doesn’t solve equations for balance at every step. Instead, it calculates accelerations directly from the applied forces and updates the motion step by step.

It’s fast and efficient for very short time steps—especially useful in high-speed or complex contact problems.

2. What is Abaqus Standard (Implicit) Solver?

Abaqus Standard, also known as the implicit solver, is designed for simulations where the system needs to find equilibrium at each step.

This solver uses an implicit time integration method, meaning it solves a set of equations that balance forces, displacements, and constraints. It typically uses Newton-Raphson iteration to converge on the solution—especially for nonlinear problems.

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.

When Should You Use Abaqus Standard?

Use Abaqus Standard when your simulation involves:

• Static problems (e.g. structural loading, thermal steady-state)

• Quasi-static nonlinear problems (e.g. contact or plasticity under slow loading)

• Abaqus dynamic implicit simulations (e.g. vibration, fatigue, or stability)

• Coupled field problems (e.g. thermal-mechanical analysis)

It’s especially powerful for accurate long-term behavior in structures, where equilibrium matters more than speed.

Strengths of Abaqus Standard

• Unconditionally stable: You can use larger time increments without worrying about numerical instability.

• Ideal for equilibrium-based problems: Great for slow or static loads where final balance is key.

• Excellent for nonlinear behavior: Handles large deformations, plasticity, contact, and creep with precision.

• Supports advanced analysis types: Like buckling, frequency extraction, and thermal-mechanical coupling.

Limitations of Abaqus Standard

• Computationally intensive: Solving equilibrium iteratively takes time, especially for nonlinear problems.

• Can struggle with severe contact: Too many contact interactions can slow convergence.

• Less efficient in high-speed dynamics: For crash-like simulations, this solver is often too slow or unstable.

If your problem is more about accuracy and balance over time, and not sudden impacts, Abaqus Standard (or Abaqus Implicit) is the better choice.

Think of it as a solver that prioritizes control and stability, even if it means taking a little longer to get there.

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 1)—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 1: 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.2). 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 2):

   – 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 2: 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 3). This is only relevant for isotropic metal plasticity materials that have a Mises yield surface.

Figure 3: apply adiabatic heating

Next 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 4).

Figure 4: 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 5).

Figure 5: Apply Fixed incrementation type

Figure 6: 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 7):

   – 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 7: 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 8).

   – 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 8: Extrapolate Previous State

2.2. Abaqus Dynamic Implicit

“Abaqus Dynamic Implicit” 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 9):

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 9: 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 10: Incrementation Tab Settings

Figure 11: 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?

Abaqus Explicit is built for fast, high-energy events—the kinds where things crash, explode, or deform in milliseconds.

It uses an explicit time integration method, which means it doesn’t solve complex equations at every time step. Instead, it calculates the motion directly based on known values of forces and accelerations.

This makes it incredibly fast for very short time steps—perfect for events that happen quickly and involve lots of contact or failure.

When Should You Use Abaqus Explicit?

Use Abaqus Explicit when your simulation involves:

• High-speed dynamics (e.g. impact, crash, drop tests)

• Abaqus dynamic explicit scenarios (e.g. blast, penetration, metal forming)

• Severe contact and large deformation (e.g. airbags, crushing, cutting)

• Material failure or erosion (e.g. fracture, element deletion)

• Short-duration events (e.g. milliseconds)

It’s also useful when the Abaqus implicit method fails to converge—like in cases with complicated contact interactions.

Strengths of Abaqus Explicit

• No need to solve equations per step: Each time step is direct and fast.

• Excellent for complex contact: Easily handles parts that slide, collide, or separate suddenly.

• Great for failure and large deformation: Simulates materials breaking, tearing, or flowing.

• Supports mass scaling: You can speed up simulations without losing accuracy—if done right.

• Stable for short time steps: Perfect for fast events.

Limitations of Abaqus Explicit

• Conditionally stable: Requires very small time steps to remain accurate and stable.

• Not efficient for slow simulations: Overkill for long, slow processes like creep or static loading.

• Time-consuming for long durations: Even if each step is fast, thousands of tiny steps can take a while.

If your simulation is all about speed, impact, and complexity, go with Abaqus Explicit. It’s built for chaos—fast-moving events with contact, breakage, or violent motion.

Think of it as a solver that trades calculation effort for speed, moving fast step by step without solving the whole system each time.

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 12).

Figure 12: 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 13).

• 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 13: 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 14: 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 15).

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 15: 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 16):

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 16: other tab for Dynamic, Explicit

4. Abaqus Standard vs Explicit: A Side-by-Side Comparison

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.

Now that you understand what Abaqus Standard (Implicit) and Abaqus Explicit solvers do individually, let’s put them head to head.

When choosing between them, it all comes down to your simulation’s needs: speed, accuracy, contact complexity, stability, or long duration.

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.

Here’s a simple breakdown of how they compare in key areas:

Now, let’s get into some details to better understand the Abaqus Standard VS Explicit:

• Dynamic Effects each solver has;
• how each solver handle contact;
• and special features for each solver.

4.1. Dynamic Effects: Motion, Forces, and Stability

How your simulation handles motion and inertia can completely change the results. Here’s how Abaqus Standard and Abaqus Explicit approach dynamic effects:

Abaqus Standard (Implicit)

By default, Abaqus Standard solves for static equilibrium—where all forces balance out, and nothing accelerates. You can also run Abaqus dynamic implicit simulations to include inertia and damping. But if you’re running a purely static analysis:

• Every part must be fully constrained (connected to the ground in all directions).

• Rigid body motion isn’t allowed—it will cause the solution to fail.

• You can’t rely on inertia to help reach equilibrium.

• If your system needs to “settle” (e.g., through vibrations or internal energy release), you’ll need to artificially help it—like applying damping.

In short: if your system doesn’t naturally reach static equilibrium, the implicit solver won’t solve it unless you guide it.

Abaqus Explicit

Abaqus Explicit always solves for dynamic equilibrium, based on Newton’s second law:
Force = Mass × Acceleration.

That means:

• Vibrations and oscillations are expected, even in what feels like a static problem.

• Time is real—how fast you apply loads matters.

• You can’t just ignore dynamic effects; they’re always there.

• If you don’t want dynamic effects to influence results (e.g., you’re simulating a slow press), you need to apply the load very slowly.

Mass scaling is often used here. You can artificially increase the mass of the system to take larger time steps and speed up the simulation. But be careful—too much scaling can introduce nonphysical results by adding unwanted inertia.

4.2. Contact Handling: Why Explicit Often Wins

If you’ve ever worked with contact in simulations, you know it’s one of the trickiest parts. Fortunately, both Abaqus Standard and Abaqus Explicit support a wide range of contact definitions—but how they handle it under the hood is very different.

Abaqus Standard (Implicit)

While Abaqus implicit solvers offer robust contact options, there’s a catch:

• Changes in contact are highly non-linear.

• The implicit solver must iterate many times to reach convergence when contact changes.

• This makes contact problems slow and computationally expensive, especially when objects repeatedly touch, separate, or slide.

For simple or slowly-evolving contact, Abaqus Standard can work just fine. But as complexity grows—multiple parts, moving contacts, or large deformations—it starts to struggle.

Abaqus Explicit

Abaqus Explicit naturally excels at complex contact problems, and here’s why:

• It doesn’t require iterative convergence.

• It uses small time increments by default, which lets it track contact changes more smoothly.

• As a result, problems involving impact, sliding, or separation become easier to solve—even if they look chaotic.

Bottom line: If your simulation has challenging or highly dynamic contact, Abaqus Explicit will usually perform better, faster, and with fewer headaches.

4.3. Solver-Specific Features: What You Only Get in One

Even though Abaqus Standard and Abaqus Explicit cover a lot of the same ground, there are still some powerful features that are only available—or much more developed—in one solver. Knowing these can help you avoid wasting time trying to do something a solver simply can’t do.

Features Unique to Abaqus Standard (Implicit)

Abaqus Standard shines when it comes to advanced structural and non-structural analysis types:

• Frequency analysis – Great for vibration and modal studies.

• Buckling analysis – Detect stability issues under compressive loads.

• Thermal-stress coupling – Full interaction between heat and structural deformation.

• X-FEM (Extended Finite Element Method) – Used for crack modeling without needing to remesh.

• Higher-order elements – Allow more accurate stress distribution in curved geometries.

• Acoustic analysis – For sound-related simulations.

• Pressure penetration – Useful for simulating effects like bolt preloading or pressurization in contact zones.

These capabilities make Abaqus Standard the go-to solver for simulations involving steady-state behavior, precision stress analysis, or linear and low-speed nonlinear problems.

Features Unique to Abaqus Explicit

Abaqus Explicit is your tool of choice when the physics gets extreme:

• CEL (Coupled Eulerian-Lagrangian) – Ideal for simulations involving fluids and solids interacting (like metal cutting or fluid sloshing).

• SPH (Smoothed Particle Hydrodynamics) – Mesh-free method for large deformations or fluid fragmentation.

• DEM (Discrete Element Method) – Used for simulating granular materials like powders or rocks.

• Element deletion – Enables progressive material failure and erosion.

• High-speed forming and impact – Naturally handled with stable time stepping.

These features make Abaqus dynamic explicit simulations perfect for crashes, explosions, fragmentation, and other high-energy events.

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

Choosing between Abaqus Standard and Abaqus Explicit isn’t always as simple as “static vs. dynamic.” In fact, both solvers can often handle the same problems—but with different levels of efficiency, accuracy, or stability.

Here’s the key: it’s not just about what kind of simulation you’re doing, but how the system behaves and what challenges your model includes.

The table below will be your guide:

Solver Selection Guide

Final Thoughts

Sometimes, Abaqus Explicit is used even for quasi-static problems—especially when Abaqus Standard struggles with convergence due to high nonlinearity or complex contact. You can slow down the load application or use mass scaling to mimic a quasi-static response with Explicit, making it a practical workaround.

On the other hand, if your simulation is long, smooth, and doesn’t involve violent motion or deformation, Abaqus Standard will almost always be faster and more accurate.

Pro tip: Don’t hesitate to try both solvers on a small version of your model. Run test cases, compare results, and see which solver gets you closer to your goals with less pain.

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.

⭐⭐⭐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.