Advanced Tutorial: Crash Test of FSAE Impact Attenuator

This article provides a step-by-step tutorial for a dynamic simulation of an FSAE Impact Attenuator.

displacement impact attenuator — Figure 1: Visualization of the displacement on the Impact Attenuator

Overview

This tutorial teaches how to:

Set up and run a dynamic simulation.
Assign boundary conditions, material, and other properties to the simulation.
Mesh with SimScale’s Standard meshing algorithm.

You are following the typical SimScale workflow:

Prepare the CAD model for the simulation.
Set up the simulation.
Create the mesh.
Run the simulation and analyze the results.

Attention!

This tutorial performs simulation with the Dynamic analysis type which is only accessible to users with a Professional plan and those who are already on the Community plan. New Community users or those recently downgraded to the Community plan will no longer be able to perform this tutorial. See our pricing page to request additional features.

1. Prepare the CAD Model and Select the Analysis Type

To start with the tutorial, please click on the button below. This will create a copy of the tutorial project in your Workbench.

Import tutorial into Workbench

The following picture demonstrates what should be visible after importing the tutorial project.

imported cad in workbench — Figure 2: Imported CAD model of the Impact Attenuator in the SimScale Workbench

This is the standard Formula SAE Impact Attenuator (IA). The job of the impact attenuator is to reduce the maximum acceleration of the driver during an impact to ensure driver safety. The IA is attached to a steel tube frame, with a lead block that represents the mass of a moving car. Finally, the concrete block is a rigid structure that is the worst-case scenario for an impact.

geometry parts overview explanation — Figure 3: CAD model showing the lead block, steel tubing, impact attenuator, and a concrete block

1.1. Create the Simulation

Start by clicking on the new geometry, and then on the ‘Create Simulation‘ button.

create simulation workbench — Figure 4: Creating a new simulation with the impact attenuator geometry

Hitting the Create Simulation button leads to several CFD and FEA options. Select ‘Dynamic‘ as the type of analysis.

dynamic analysis fsae impact attenuator library — Figure 5: Choose **‘Dynamic’** from the analysis type widget options.

2. Set Up the Simulation

2.1. Contacts

SimScale will automatically set any faces that perfectly touch within the geometry as Contacts, but sometimes assignments are needed for faces that SimScale won’t automatically pick up. For this tutorial, two additional Contacts are needed. To add a bonded contact, click the plus next to Contacts in the simulation tree and select ‘Bonded‘ under Manual contact creation.

add bonded contact under manual contact creation — Figure 6: Creating a new bonded contact

The first additional contact is between the faces of the steel tubing and the adjacent face on the plate. The tubing faces will be assigned as the Master assignment, while the steel plate will be the Slave assignment.

Figure 7: Displaying the master (in blue) and slave assignments (in pink) for the first additional bonded contact

Select all four external faces from the Tubing as Master assignments
Hide the Mass volume by clicking on the ‘eye’ icon
After hiding the Mass volume, you can select the top Steel plate face as the Slave assignment

With a similar workflow, the Tubing volume will be bonded to the Mass. This time, you can define all of the Tubing walls as Slave assignments. By hiding the Steel plate and Impact attenuator volumes, the bottom face of the Mass volume can be defined as the Master assignment:

Figure 8: Displaying the master and slave assignments of the third bonded contact

It is important to be careful when assigning slave and master assignments. SimScale will not allow you to have multiple slave assignments on the same face. As shown above, the tubing faces were the master assignment in Bonded 2, but the slave assignment in Bonded 3.

After creating the bonded contacts, you need to set a Physical contact between the front faces of the IA and the impact block. This physical contact will allow the set of faces to interact with each other when the impact occurs.

creating a physical contact within simscale — Figure 9: Creating a new physical contact

In this definition, the top face of the concrete Block will be the Master assignment, whereas the bottom faces of the Impact attenuator will be the slave assignments.

physical contact master assignment boundary — Figure 10: Displaying the master and slave assignments of the physical contact

For the Slave faces, pick all of the bottom faces of the Impact Attenuator—there should be 17 faces in total.

2.2. Materials

The SimScale platform comes with many default materials. To add new materials, click on the ‘+’ icon next to the Materials in the simulation tree:

Start by selecting ‘Steel’ for the steel plate and tubing from the Material list.

material list steel — Figure 12: The materials library comes with several pre-defined materials

By default, the material behavior for steel is Linear elastic. For this simulation, please adjust the material behavior setting to ‘Elasto-plastic’. You will be prompted to define the stress-strain curve of the material by clicking on the table definition icon.

elasto-plastic material definition simscale — Figure 13: The table input icon, indicated by the arrow, allows the definition of a stress-strain curve

The stress-strain curve definition for steel can be found in the first sheet from this spreadsheet (named Steel – Tubing & Steel plate). Therefore, make sure to download the first sheet as a .csv file, and upload it to SimScale using the import box shown below.

importing stress strain curve via csv file — Figure 14: It is possible to type in the table values, or directly import a stress-strain curve via a .CSV file

Finally, please assign this material to the ‘Tubing‘ and ‘Steel plate‘ by selecting them from the geometry tree at the right of the Workbench.

assigning materials to steel plate and tubing — Figure 15: Assigning steel as the material for the *Tubing* and *Steel plate*

Create a new material, this time selecting ‘Rubber‘ from the Material list—this one will be used for the Impact Attenuator volume. Some changes will be performed on the default rubber settings:

The new material behavior will be ‘Elasto-plastic’
The Young’s modulus will be changed to ‘9e6’ \(Pa\) due to the stress-strain data that will be defined (see more notes on Young’s modulus calculation on this documentation page).
Find the stress-strain curve for the rubber material in the second sheet from this spreadsheet (named Plastic – Impact Attenuator). Again, downloading the data as a CSV file and uploading it to SimScale is the best way to proceed.
Finally, assign the rubber material to the ‘Impact attenuator’.

rubber properties elasto-plastic — Figure 16: Assigning rubber as the material for the IA

Changing the material behavior to plastic allows the material to hold its deformation once a force is no longer applied. With the elastic behavior, the material will return to its original shape. The elastic behavior is suitable for small deformation simulations, but for larger deformations the plastic material behavior is essential.

The next material from the list will be ‘Lead‘. Please assign it to the ‘Mass’ volume.

assignment lead material properties mass — Figure 17: Assigning Lead as the material for the **‘Mass’** volume, keeping the default settings

Repeat the same process, now with ‘Concrete‘ as the material, assigning it to the ‘Block’ volume with default settings.

2.3. Initial Conditions

For time-dependent simulations such as dynamic analyses, the initial conditions are very important, as they define the initial state of the system. In this tutorial, all volumes except for the concrete block will receive a velocity initialization:

velocity initialization dynamic impact analysis — Figure 18: With a velocity initialization, you can control the velocity of the object immediately before the impact.

Click on the ‘+’ icon next to the Subdomains, under (U) Velocity.
Apply a velocity of ‘-7’ \(m/s\) in the Y direction.
Assign this velocity to the ‘Steel plate, Impact attenuator, Tubing, and Mass’ volumes.

2.4. Boundary Conditions

Up next, you can define constraints and loads via boundary conditions. In this tutorial, the base of the concrete block will be fully constrained with a Fixed support boundary condition:

add fixed support boundary condition — Figure 19: Adding a fixed support boundary condition

Rotate your model and click on the face on the bottom of the concrete block to fix it. This configuration will ensure that the base of the block doesn’t move during the collision.

constraint dynamic simulation bottom concrete block — Figure 20: Assigning a fixed support condition to the bottom of the concrete block. With this configuration, the bottom face is completely constrained.

2.5. Simulation Control

To better capture the impact, some simulation control settings will be changed. Adjust the Simulation interval to ‘0.05’ seconds, and the Maximum runtime to ‘30000’ seconds. To capture the impact more precisely, the Maximum time step length will be defined via a table:

simulation control panel — Figure 21: Editing the simulation control settings

With the settings below, the simulation will have timesteps of:

0.005 seconds from t = 0 until t = 0.01 s
0.002 seconds from t = 0.01 until t = 0.03 s
0.001 seconds from t = 0.03 until t = 0.05 s

time step table — Figure 22: By lowering the step size during the impact, you can capture the impact and vibrations more precisely.

2.6. Result Control

Within Result control, the user can define additional monitors/outputs for the simulation run. Please create a Point data within the Result control tab. The first point will monitor the ‘Acceleration’ on the top of the lead volume:

creating a new point data result control — Figure 23: By clicking on the **‘+’** button next to *Geometry primitives*, you can define the coordinates of the point of interest.

The first point will maintain coordinates 0 for X and Z. The coordinate in Y will be changed to ‘0.235’ meters. When saving the point definition, it will be assigned to the Point data 1 result control.

point coordinate for a result control — Figure 24: The platform provides a visual representation of the point coordinate. The first point is placed on the top of the lead volume.

Create a second point data result control, this time selecting ‘Displacement’ for the field. The coordinates for the second point will remain default (0, 0, 0):

3. Mesh

The standard mesh will be used with an Automatic sizing and Fineness of ‘3’:

standard mesh fineness definition dynamic — Figure 26: With a small fineness, regions far away from the impact area will be captured more coarsely

Before generating the mesh, some region refinements will be added to the impact regions, to better capture the collision.

To create a new refinement mesh, click on the ‘+’ button next to Refinements. From the window that comes up, select a ‘Region refinement’:

new refinement region meshing — Figure 27: Adding a new refinement region

In the configuration window, you can adjust the Maximum edge length of the cells inside the region of interest. For the first refinement, a maximum edge length of ‘0.02’ meters will be applied to a cartesian box:

creating a new region refinement for a mesh — Figure 28: Selecting a cartesian box for a new refinement region

The first region refinement will be applied to two cartesian boxes. The coordinates of the first one are below:

moving region dimensions refinement — Figure 29: Dimensions of the cartesian box for the moving region

After saving the first coordinates, add another cartesian box, this time for the impact region:

impact region dimensions refinement — Figure 30: Dimensions of the cartesian box for the concrete region where the collision will occur

After saving the coordinates of the second box, make sure that both are assigned to the first region refinement.

first region refinement definition complete — Figure 31: Final configuration of the first region refinement setting

Finally, create another region refinement, this time with a Maximum edge length of ‘0.01’ meters, assigned to the cartesian box below:

impact attenuator dimensions refinement — Figure 32: Dimensions of the cartesian box for the impact attenuator

After assigning the second region refinement to the impact attenuator cartesian box, open the Mesh tab and ‘Generate’ a new mesh.

generating a new standard mesh dynamic simulation — Figure 33: After setting up the necessary refinements, you can **‘Generate’** a new mesh

4. Start the Simulation

To create a new simulation run, please click on the ‘+’ button next to the Simulation Runs.

starting a new simulation run in simscale — Figure 34: Simulation setup tree before starting the simulation

5. Post-Processing

Once the simulation run is finished, you can post-process the impact analysis results. To access the online post-processor you can use one of two methods:

accessing the online post-processor simscale — Figure 35: The post-processor is accessible by clicking on **‘Solution Fields’** or **‘Post-process results’.**

5.1 Visualize the Stress

You can notice that the default visualization state shows the Von Mises Stress contour over the geometry. Nonetheless, we can improve the visualization by tweaking the upper legend bound:

tweaking stress plot online post-processor simscale — Figure 36: Tweaking the post-processor legend for a better stress visualization

Initially, adjust the upper legend bound to ‘1e8’ Pascals. Furthermore, you can also right-click on the legend bar to set a ‘Continuous scale’:

legend bar contextual menu online post-processor simscale — Figure 37: Contextual menu for the legend bar. Use the continuous scale option for a smooth transition between contours.

Finally, to better inspect the stress in the interior of the attenuator, we can create a cutting plane. On the top Filters ribbon, click on the ‘Cutting Plane’ icon and adjust its Orientation to ‘X’:

creating cutting plane online post-processor simscale — Figure 38: Creating a new *Cutting Plane* using the filters ribbon

Now you can rotate and zoom the viewer to inspect the stress distribution on any cutting plane of interest.

5.2 Deformation

You might have noticed that the default visualization also included a Displacement filter. This filter allows us to see the movement and deformations in the parts. If it is not added already, please go ahead and add the ‘Displacement’ field from the top ribbon.

deformation evaluation in simscale — Figure 39: The displacement filter allows the user to see how the updated location of the parts for each time step.

After making sure that the Displacement filter is created, change the Coloring from the Cutting Plane 1 and Parts Color to ‘Displacement magnitude’. By using the Steps bar on the right-hand side panel, you can go through the various timesteps that were saved from the simulation.

displacement visualization impact analysis — Figure 40: When going through the various timesteps, the displacement and quantities are automatically updated in the viewer

We find that the point of maximum compression is at step 0.036 \(s\), and we can appreciate the displacement distribution, especially on the impact attenuator part.

5.3 Impact Test Animation

The whole deformation process can be better visualized by creating an Animation filter. Adjust the Coloring of all components back to ‘Von Mises Stress’ and set the animation to play to observe the physics of the collision:

visualization impact analysis animation — Figure 41: The animation filter will smoothly play all saved states, allowing the user to see how the collision occurs.

Once an animation is created, it is possible to output a recording by using the Record capture feature:

Find below a gif version of the animation, created with the Record feature.

gif recording of an animation in simscale — Animation 1: Animation for the crash test process of the impact attenuator, with coloring according to the developed stresses

The deformations and stress evolution of the parts can be appreciated in context thanks to the animation. Regions colored in yellow and red show the development of higher stress values.

Analyze your results with the SimScale post-processor. Have a look at our post-processing guide to learn how to use the post-processor.

Congratulations! You finished the tutorial!

Have a look at the finished project

Note

If you have questions or suggestions, please reach out either via the forum or contact us directly.

Last updated: December 4th, 2023

Did this article solve your issue?

How can we do better?

We appreciate and value your feedback.