Speeding Up Quasi-static Analysis in Abaqus/Explicit

quasi static abaqus

Part 1: Increasing Load Rates

Quasi-static analysis in Abaqus/explicit and its related methods to increase solving speed, like load rate scaling or mass scaling, are fully described in this post. Follow me to start speeding up our CAE analysis step by step.

We previously discussed differences between Abaqus/Standard and Abaqus/explicit in the article:
Abaqus/Standard or Abaqus/Explicit?

In addition, you can see this Q&A to have a sense of how we decide whether an analysis is quasi-static (static) or not:
How can I know if my simulation is quasi-static or not?

Quasi static problems are one of those that usually would be solved with Abaqus/Standard but may have difficulty converging because of contact or material complexities, resulting in a large number of iterations. Challenging nonlinear quasi-static problems often involve:

* Very complex contact conditions, which Abaqus/Standard may fail to converge due to contact issues.

** Very large deformations that can lead to severe mesh distortion.

For example, typically, in metal forming analysis, we face such difficulties:

quasi static

Example: Simulation of tearing in a deep drawing process
It is really hard to model such a problem with Abaqus/Standard.

quasi static ⭐⭐⭐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

…………………………                 …………………………….. ……………   …………………………….

Abaqus/Explicit in Quasi-static Analysis Problems

Abaqus/Explicit is more efficient for modeling highly nonlinear static (quasi-static analysis) problems. This is especially true for three-dimensional problems involving contact and very large deformations like metal forming.

Application of Abaqus/Explicit to model quasi-static events requires special consideration. It is computationally impractical to model the process in its natural time period. Literally, millions of time increments would be required. Therefore, we artificially increase the speed of the process in the simulation to obtain an economical solution.

Two approaches to obtaining economical quasi-static analysis solutions with Abaqus/Explicit are:

1. Increased load rates

We can artificially reduce the time scale of the process by increasing the loading rate. Increased load rates reduce the time scale of the simulation, so fewer increments are needed to complete the job.

Increasing load rates by a factor of f, increases the analysis speed by a factor of f.

2. Mass scaling

It increases the size of the stable time increment, so fewer increments are needed to complete the job. Artificially increasing the material density (mass scaling) by a factor of f2 increases the analysis speed by a factor of f.

In this article, our focus is on the increased load rates approach. Mass scaling will be discussed in detail later.

To reduce the number of increments required in an Abaqus/Explicit analysis, we can speed up the simulation compared to the time of the actual process—that is, we can artificially reduce the time period of the event or, equally, increase the rate of loading. This will introduce possible errors. If the loading rate is increased too much, the increased inertia forces will change the predicted response. In an extreme case, the problem will exhibit a wave propagation response. The only way to avoid this error is to choose a load rate that is not too large.

How to find out if a load rate is appropriate or not?

1) Running several simulations with different load rates

  1. Run a series of simulations in the order from the fastest load rate to the slowest. As you know, the analysis time is greater for slower load rates.
  2. Examine the results (deformed shapes, stresses, strains and energies) to get an understanding of the effects of varying the model when changing the load rate Abaqus:

»Excessive tool speeds in sheet metal forming tend to promote unrealistic localized stretching.

»Excessive tool speeds in bulk forming simulations cause jetting (hydrodynamic-type response).

load rate abaqus»Excessive loading rates can cause highly localized deformation near the applied load.

»Excessive loading rates in a quasi-static collapse analysis can result in a steep initial slope of the load versus displacement curve due to increased (non-structural) resistance to initial deformation. Sometimes, localized buckling may occur near the applied load.

2) Using natural frequency to check the load rate

The dominant response of a quasi-static analysis will be the first structural mode. Therefore, we use the frequency of this mode to estimate the proper load rate Abaqus:

  1. Estimate the first natural frequency (f) of the model. In simple models, we may find this frequency by available analytical relations. For models that are more complex, first, run a Frequency analysis in Abaqus.
  2. Calculate the corresponding time period (T) using the first natural frequency of the model:


  1. Run the Explicit analysis (step time=T) and estimate the global deflection (D) in the impact direction of the model during this time (T).
  2. Calculate the impact velocity (V):


  1. A general recommendation is to limit the impact velocity to less than 1% of the wave speed of the material. Typical wave speed in metals is 5000 m/sec.

Example (Door Beam Intrusion Test)

To illustrate the problem of determining the proper loading rate, consider the deformation of a side intrusion beam in a car door. The actual test is quasi-static.

mass scalingWe model the test as the circular beam (length of l, diameter of d and thickness of t) is fixed at each end, and a rigid cylinder (diameter of D) deforms the beam.

mass scaling abaqusHere, we check the velocity of 20 m/s and 400 m/s for a cylinder to see which one can be applicable to our problem.

quasi static analysis

  • The frequency of the first mode is approximately 250 Hz: f=250
  • This rate corresponds to a period of 4 milliseconds: T=1/250=0.004 s
  • Using a velocity of 20 m/sec, the analysis shows cylinder will be pushed into the beam 0.1 m in 4 milliseconds: D=0.1 m
  • The impact velocity is:

V=D/T= 0.08/0.004= 20 m/s

  • Recalling the wave speed in metals is about 5000 m/sec, so the impact velocity 25 m/sec is about 0.5% of the wave speed (less than 1%).

If we check the velocity of 400 m/s it will result in about 4% of wave speed (unacceptable).


i. As the speed of the process is increased, a state of static equilibrium evolves into a state of dynamic equilibrium and inertia forces become more dominant. We should try to model the process in the shortest time period (largest load rate Abaqus) in which inertia forces are still insignificant.

ii. Some aspects of the problem other than inertia forces—for example, material behavior—may also be rate-dependent. In this case, the actual time period of the event being modeled cannot be changed. The mass scaling approach gets attractive in such problems.

Using Smooth Step amplitude curve

We could obtain a more accurate quasi-static solution by applying loads gradually.

By default, Abaqus/Explicit loads are applied immediately and remain constant throughout the step. Instantaneous loading may induce the propagation of a stress wave through the model, producing undesired results. For instance, constant velocity boundary conditions result in a sudden impact load onto a deformable body.

We can ramp up (or down) the loading gradually from (to) zero by defining a smooth step amplitude in Abaqus:

quasi static abaqus Defining Smooth Step Amplitude 2 | quasi static abaqus

It would be useful to see Abaqus Documentation to understand how it would be hard to start an Abaqus simulation without any Abaqus tutorial. If you want to get complete information about load rate scaling and mass scaling methods, watch the below demo video of the Abaqus course for beginners package:

Quiz Time!

1. Abaqus/standard is not appropriate for metal forming simulation at all. (True/False)

2. Stretching is one of the bulk metal forming processes in which Abaqus/explicit is more efficient to simulate. (True/False)

3. We artificially increase the time scale of the process by increasing the loading rate. (True/False)

4. Jetting is a hydrodynamic-type response when tool speed in bulk forming simulations is excessive happens. (True/False)

5. Mass scaling by a factor of f decreases the computational cost by a factor of √f. (True/False)

6. Increasing load rate by a factor of f decreases the computational cost by a factor of f. (True/False)

7. By default, Abaqus/Explicit apply loads gradually throughout the step.

quasi static ⭐⭐⭐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

…………………………                 …………………….. ……………………   …………………………….

Practice Time!

Try to model intrusion tests based on the information provided about geometry, material, etc. First, conduct a Frequency analysis to find the basic frequency (first mode) of the beam (with given BC). Then, run three Dynamic, Explicit analyses (as shown in the poster of the article) and compare results.

(function(d,u,ac){var s=d.createElement(‘script’);s.type=’text/javascript’;s.src=’’;s.async=true;s.dataset.user=u;s.dataset.campaign=ac;d.getElementsByTagName(‘head’)[0].appendChild(s);})(document,147270,’cmpslimbu2jp4ovk04hk’);

✅ Subscribed students +80,000
✅ Upcoming courses +300
✅ Tutorial hours +300
✅ Tutorial packages +100

2 thoughts on “Speeding Up Quasi-static Analysis in Abaqus/Explicit

  1. Avatar of Margy Jacobo Margy Jacobo says:

    finest post

  2. Avatar of facebook facebook says:

    Some genuinely prize articles on this site, saved to favorites . Kerrill Bondie Bearce

Leave a Reply