Blog

Speeding Up Quasi-static Analysis in Abaqus/Explicit (1)

Part 1: Increasing Load Rates

We previously discussed differences of 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 an analysis is quasi-static (static) or not:
How can I know my simulation is quasi-static or not?

Quasi-static problems are one of those 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 may Abaqus/Standard, may fail to converge due to contact issues.

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

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

Tearing in Deep drawing

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

Abaqus/Explicit in Qausi-static Problems

Abaqus/Explicit is more efficient for modeling highly nonlinear static (quasi-static) 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 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 and 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 and 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 increased load rates approach. Mass scaling will discuss 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 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 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 for the effects of varying the model when changing load rate:

»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).

Jetting in metal forming»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 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:

  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:

T=1/f

  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):

V=D/T

  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.

Door beam intrusion TestWe 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.

Here we check velocity of 20 m/s and 400 m/s for cylinder to see which one can be applicable for our problem.

Door beam intrusion Model Results

  • 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).

Limitations

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) 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. Mass scaling approach get 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 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 ramping up (or down) the loading gradually from (to) zero by defining a smooth step amplitude in Abaqus:

Defining Smooth Step Amplitude 2

Quiz Time!

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

2. Stretching is one of 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.

Practice Time!

Try to model intrusion test based on the information provided about geometry, material, etc. First, conduct a Frequency analysis to find 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.


One thought on “Speeding Up Quasi-static Analysis in Abaqus/Explicit (1)

  1. Margy Jacobo says:

    finest post

Leave a Reply