November 21, 2019 at 10:35 am
November 23, 2019 at 4:34 pmpeteroznewmanSubscriber
RMB on the Solution branch and Open Solver Files Directory. In the Windows Explorer that opens, find Solve.out and open that with Notepad. In there you will see the following.
Checking model setup.....Please wait
ERROR! Number of elements exceeded for Academic Teaching version - elements limited to 32000.
The number of nodes or elements must be < 32000 for the solver to run. Your mesh has 46,400 elements.
There are several things wrong with this model.
1) You should convert this thin-walled solid to a midsurface model using SpaceClaim. Then you will have shell elements with an assigned thickness covering surfaces that represent the car and the pole instead of solid bodies. Once you mesh with shell elements, you will easily stay below the Student license limit.
2) You should move the car (or pole) until they are tangent (touching). The reason is that explicit dynamics must use very small time steps dictated by the smallest element in the model. You have about a 0.14 m gap between the car and the pole. At the velocity used of 11 m/s, it will take about 0.0125 seconds until impact. That is a lot of cycles to be waiting for the interesting part.
3) You have correctly assigned an initial velocity to the car. Don't also assign a velocity boundary condition to the whole car. That turns the car into a rigid body. Similarly, don't apply displacement boundary conditions to the car. Once it is a surface model, you can pick a circular edge of a wheel well and create a remote displacement to set Y=0. Repeat four times so each wheel is independent.
November 30, 2019 at 11:39 amHayatiSubscriber
Okey. Noted. Thank you very much.
November 30, 2019 at 11:42 ampeteroznewmanSubscriber
Please mark this DIscussion as Solved by clicking the Is Solution link.
- You must be logged in to reply to this topic.
Boost Ansys Fluent Simulations with AWS
Computational Fluid Dynamics (CFD) helps engineers design products in which the flow of fluid components is a significant challenge. These different use cases often require large complex models to solve on a traditional workstation. Click here to join this event to learn how to leverage Ansys Fluids on the cloud, thanks to Ansys Gateway powered by AWS.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- explicit dynamics
- Explicit dynamics ERRORS
- turning simulation
- getting zero maximum and minimum stress value in explicit analysis
- How to figure out impact force in Explicit Dynamic Analysis
- Running an explicit dynamics simulation on a composite plate
- How do get Full values instead of just minimum and maximum ?
- Monte Carlo Simulation
- Euler Domain Restricting Simulation
- Which analysis to use for dynamic and quasi-static compression of auxetic structures?
© 2023 Copyright ANSYS, Inc. All rights reserved.