## LS Dyna

#### Solving Explicit Simulation of Safety Barrier

• luis.serra5
Subscriber
Hi! I am currently doing my thesis and my project is about a crash test between a car and road safety barrier. I need to use the model ilustrated in the next image.
After start solving the numerical model, my project gets an error ("Solver Error -Energy Error too large") and it stops at the middle of the process. Besides that, the time of simulation is huge (300 hrs).
Can you help solving this issues (Error and Computational time)?

I did some simplifications to my model:
- I Removed round faces and some holes of some bodys;
- I put springs to model the bolts;
- I am using surface bodies in all bodies, except the car.

• peteroznewman
Subscriber

The maximum time step in Explicit Dynamics is calculated using the minimum characteristic length of all the elements in the mesh. In the Mesh Details, request the Mesh Metric of Characteristic Length (it is the last item on the list so scroll to the bottom of the list).  Look at the statistics on this metric. If the average element length is 100 mm and the minimum length is 1 mm, it is the 1 mm element that sets the maximum time step. Look at where the 1 mm element is. Simplify the geometry so that it can mesh with a larger element. If you can remesh so the smallest Characteristic length is 10 mm, then the 300 hours will be reduced to 30 hours.  If you can get the minimum length to 100 mm, the solution time might reduce to 3 hours.

Under Analysis Settings, you can type in a larger Maximum Energy Error to keep the simulation running. After it finishes, you can plot the Energy Error and evaluate whether the simulation is acceptable.

• luis.serra5
Subscriber
Thank you for your reply. I was doing that and my minimum length is about 0.80 mm, as you could see in the following image. The problematic geometry is the barrier. How can I fix that without compromise the accuracy of the simulation? Is there another option to solve the energy error issue besides changing the Maximum Energy Error?

Regards.

• luis.serra5
Subscriber
I tried to do those changes in my model but it didn't work well...My time of simulation is always increasing and it doesn´t fix in a specific value. Can I send you my model?
• peteroznewman
Subscriber
I expect you can get a good representation of the shape of the safety barrier using 10 mm edge lengths on the quad elements.

The minimum characteristic length at the begining of the model will get smaller as the element deforms.
Explicit Dynamics uses Erosion to remove highly distorted elements from the simulation to keep the time step from getting a lot shorter. What are your Erosion Control settings?

In Workbench, use File, Archive to create a .wbpz file.
Put that file in a file sharing location such as Google Drive, Jumpshare or Dropbox.
Copy the link and paste it into your reply along with the version of ANSYS you are using.
Then anyone can get a copy of that file.
• luis.serra5
Subscriber
I didn´t turn on any of the erosion control settings. I used the specifications of the Low Velocity analysis type.
I changed the car geometry: removed the wheels and the axles and I designed its body as a shell body, in order to have only shell elements in the model. It went very well because I had low simulation times (100 hrs) when compared to the previous model. Thank you for your suggestions!

I have another doubt: Is it possible to specify the mass center of the car without change the geometry? I introduced a point mass but I have to set it to rigid and when I do that, I can´t specify another constraints like displacements.