Learning Forum

[StudentJack]

Hi,

I am trying to simulate a steel bumper crash against a concrete wall at both 1.1m/s and 13.89m/s and find out how much energy is being absorbed. The mass of a vehicle is about 1511kg. The car bumper is expected to crumple on impact, however, it doesnt seem to crumple as well. I believe it has got to do with the engineering data of steel but I am not sure which properties have.

1) Should i still be using explicit dynamics?

   if using explicit dynamics, am i suppose to just use explicit materials only?

2) It seem like the steel bumper does not crumple even at 100m/s even though I have turned on material erosion. Is there something I am doing wrong?

3) What material properties for steel should i have in my engineering data

My ultimate goal is just to study the amount of energy it can absorb. May i know how to go about doing it as well?

[peteroznewman]

Hi Jack,

The material you have for the bumper is Structural Steel with only Linear Elastic properties. That is why the bumper is just bouncing off the block without crumpling. I thought the Erosion would have removed some elements that exceeded a strain value of 1.5. I don't know why that didn't happen, but you should change material as explained below. Which 3 faces is the point mass scoped to?

In order for a steel bumper to crumple, it needs a material property called Plasticity. Open Engineering Data and you can see a list of Plasticity models. The simplest one is Bilinear Isotropic Hardening. When you drag and drop that on Structural Steel, there are two values needed. Enter the Yield Strength in the correct units.  Use 0 for the Tangent Modulus. This works well for loading in Static Structural and should also work in Explicit Dynamics.

Explicit Dynamics is good for crash simulations.  In that solver, there is a material model called Equation Of State (EOS).  Click on Engineering Data Sources, Click on the Explicit Materials, scroll down to STEEL 1006 and click the yellow + sign to add that material to your model.

In Workbench, Refresh the model. In Mechanical, click on the solid body that is the bumper and assign STEEL 1006 to the body.

In the Analysis Settings, in the Output Controls, change the Result Number of Points from 20 to 200. Now solve the model. You should see some crumpling.  If it stops for an Energy Error, increase the Maximum Energy Error number.