**Increasing load rate in an Abaqus quasi static analysis**

A lot of Abaqus users face a common problem: their analyses, especially the **quasi static analysis**, take a really long time to finish. This can be quite annoying. Fortunately, there are two methods to speed up these Abaqus quasi static analysis: one is using “Abaqus mass scaling,” and the other is increasing the “**Abaqus load rate**.” In this post, we’ll concentrate on the latter method, which involves making your analyses faster by adjusting the load rate. We’ll also guide you on how to determine which load rate is suitable for your quasi static analysis in Abaqus.

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:

*Example: Simulation of tearing in a deep drawing process*

*It is really hard to model such a problem with Abaqus/Standard.*

Stay with us, The **CAE Assistant group**, which always trying to be your complete assistant in CAE challenges. 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 analysis in Abaqus/Explicit 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.

If you would like to know more about Abaqus/Standard and Abaqus/Explicit, we’ve already covered the differences between them in this article titled,Abaqus/Standard or Abaqus/Explicit? |

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

**1. Increasing Abaqus Load Rates**

We can artificially reduce the time scale of the process by increasing Abaqus 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 **f ^{2}**ย increases the analysis speed by a factor of

**f**.

In this article, our focus is on **increasing Abaqus load rates**.

To reduce the number of require increments in an quasi static analysis in Abaqus/Explicit, we can speed up the simulation compared to the time of the actual processโthat 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.

**Finding out Abaqus load rate is appropriate or not**

As discussed, there are two options to reduce the computational cost of quasi-static analysis: mass scaling and increasing the load rate in Abaqus. When utilizing the Abaqus mass scaling feature, the system’s mass is multiplied by a factor. While it can reduce computational costs, high mass scaling coefficients may significantly affect results. Moreover, increasing the load rate in Abaqus can lead to a dynamic response rather than the quasi-static Abaqus solution. Therefore, both techniques must be used with care. Various criteria have been provided to check if quasi-static analysis in Abaqus is performed with sufficient accuracy.

**1) Running several simulations with different load rates**

- 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 Abaqus load rates.
- 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:

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

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

**ยป**Excessive loading rates can cause highly localized deformation near the applied load.

**ยป**Excessive loading rates in an Abaqus 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 Abaqus 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:

- 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. - Calculate the corresponding time period (
**T**) using the first natural frequency of the model:

**T=1/f**

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

**V=D/T**

- 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**.

### 3) Comparison of kinetic and internal energies in quasi-static analysis

To ensure quasi-static behavior, especially when increasing the load rate or defining a mass scaling factor in an explicit step within Abaqus, you can compare kinetic and internal energies. This helps verify that the mass scaling factor and the load rate in Abaqus are sufficiently small. For those interested in the practical implementation of this approach, it is discussed in the following section.

In quasi-static analysis, it is crucial to keep the kinetic energy of deformable bodies below a critical percentage of the total internal energy. The Abaqus documentation recommends maintaining this critical range between 5 and 10 percent. We will now explain how to check this criterion in your simulation.

When defining a dynamic explicit step in Abaqus, the energy for the entire system is automatically extracted in the form of history outputs. To examine this process, create a dynamic explicit step in the ‘Step’ module and then click on the ‘History Output Manager’ icon. As shown in the next figure, Abaqus automatically generates a history output for the explicit step.

You can edit the created history output and deselect unnecessary results. For example, as illustrated in the next figure, we have unchecked all energy components except ALLIE and ALLKE. They represent the total internal energy and kinetic energy, respectively.

Note that the kinetic energy chosen in the ‘Edit History Output Request’ window includes the energy for the rigid bodies. However, if your model has rigid bodies with assigned mass, you must subtract the kinetic energy for rigid bodies from the total kinetic energy. To achieve this, start by creating a set that includes all rigid bodies with mass. To do so, navigate to the ‘Step’ module, click on ‘Tools’, then select ‘Set’, and finally, click on ‘Create’. Choose ‘Geometry’ for the type and click ‘Continue’. The procedure is illustrated in the following figure.

Now, choose the rigid bodies in the model and click ‘Done’. Next, click on the ‘History Output Manager’ icon, and copy the existing history output, as illustrated in the next figure. Finally, click ‘OK’ to generate the history output.

Next, in the โHistory Output Managerโ window, select the second history output and click ‘Edit’. As shown in the next figure, choose ‘Set’ from the ‘Domain’ combo box, then select the set that includes rigid bodies (e.g., Set-6 in the figure). Uncheck ALLIE since it is not needed, and click ‘OK’ to proceed. Abaqus will now extract the kinetic energy for rigid bodies.

Now, assume that you have submitted the job, and it is completed. You want to check the solution to determine whether the load rate in Abaqus is sufficiently small to access a quasi-static solution or not. To do so, go to the visualization module, click on the ‘Create XY Data’ icon, and then ensure that the ‘ODB history output’ is chosen. Finally, click ‘Continue’. The procedure is presented in the following figure.

Afterward, select the internal and kinetic energies, as shown in the following figure, and click on ‘Save as’. Note that if you have no rigid body in your model, you only need to choose the total internal and kinetic energies. Otherwise, the kinetic energy for the rigid body must also be selected.

In the displayed window, choose ‘As is’ and click ‘OK’. If you have rigid bodies with assigned mass in your model, click on the ‘Create XY Data’ icon, and then select ‘Operate on XY data’. Click ‘Continue’ to proceed.

Now, select the total kinetic energy and click ‘Add to expression’. Then, click on the minus sign and choose the kinetic energy for the rigid bodies. Once more, click ‘Add to expression’ and then click ‘Save as’. The procedure is illustrated in the following figure.

Choose a name for your data and save it. Note that the saved data is the total kinetic energy minus the energy of rigid bodies. Click the ‘XY Data Manager’ icon, and select both the operated data and the total internal energy. If your model has no rigid bodies with assigned mass, choose the total kinetic energy instead of the operated data. Finally, click ‘Plot’.

Now you have plotted the internal and kinetic energies, as shown in the following figure. So, you can compare their ratio to determine if the load rate in Abaqus is sufficiently small to indicate a quasi-static solution or not.

Moreover, you can click on the ‘Create XY Data’ icon and select ‘Operate on XY Data’. Next, divide the kinetic energy by the total internal energy to check if the ratio is below 10 percent. If the ratio exceeds the critical value, you can either decrease the mass scaling factor or adjust the load rate in Abaqus.

**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. This test falls into the category of Abaqus quasi-static analysis

We model the test as the circular beam (length of * l*, diameter of

*and thickness of*

**d***) is fixed at each end, and a rigid cylinder (diameter of*

**t***) deforms the beam.*

**D**Here, 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.

- 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 Abaqus) in which inertia forces are still insignificant.

**ii.** Some aspects of the problem other than inertia forcesโfor example, material behaviorโmay 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 Abaqus 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 an Abaqus quasi-static solution:

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

In this post, we completely covered speeding up quasi-static analysis in Abaqus by increasing the load rate. You can now choose the appropriate Abaqus load rate and examine it using the methods we discussed, such as ‘Running several simulations’ and ‘Using natural frequency.’ Additionally, by studying the example provided, you can gain a deeper understanding of Abaqus quasi static problems.

**It’s your turn** to dive into the article and join our quiz! Don’t forget to check out the ‘Practice Time‘ section; you’re supposed to conduct the intrusion test. Please share your experiences, questions, or any comments you might have with us, The CAE Assistant, your assistant in CAE challenges.”

**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 Abaqus 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 โ**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. (True/False)

**Practice Time!**

Try to model intrusion tests, one of the Abaqus quasi static problems. you can model 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.

You can have the PDF of this Post by clicking on speeding up quasi static analysis in Abaqus

โ Subscribed students | +80,000 |

โ Upcoming courses | +300 |

โ Tutorial hours | +300 |

โ Tutorial packages | +100 |

#### What is a quasi-static analysis?

**The quasi-static**** analysis is a way to study how things behave when they are slowly loaded or changed over time.** It is a simplified approach that assumes that the thing being studied remains in balance at each stage of the analysis. This means that the effects of inertia, or how fast the thing is accelerating, are ignored.

#### What is quasi-static analysis with Abaqus explicit?

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.

#### How to reduce analysis time in Abaqus?

**Increasing Abaqus Load Rates:**

Artificially reduce the time scale of the process by increasing the Abaqus loading rate.

**Mass scaling:**

Increases the size of the stable time increment, reducing the number of increments needed to complete the job.

After looking into a handful of the blog posts on your site, I really appreciate your way of writing a blog. I bookmarked it to my bookmark webpage list and will be checking back in the near future. Take a look at my web site too and tell me how you feel. Maddalena Benedetto Brownley