October 30, 2018 at 5:18 amrupaknayakSubscriber
Dear sir i am doing the simulation of orthogonal turning in explicit dynamics.
the problem i am facing is "the simulation completion time goes on increasing continously from (30 hrs to around 130 hrs). finally i get the message of energy error too large. plzz help me to sort out this problem.
i am attaching the wbpz file of my simulation plz take look and advice what changes i need to make.
October 30, 2018 at 1:19 pmrupaknayakSubscriberI request the moderators to plzz reply .
October 31, 2018 at 4:29 amrupaknayakSubscriber
peteroznewman sir plzz reply.
October 31, 2018 at 11:52 ampeteroznewmanSubscriber
Sorry rupaknayak, but I can't run your model now as I am using my license and big computer to do my own work and your problem doesn't fit in the Student license that runs on a second computer I have available.
I opened your archive and see you have not assigned Initial Conditions to the tool at 2 m/s but you have the tool with that velocity as a boundary condition with a Step input. Please add a Velocity Initial Condition to the Tool. This may have nothing to do with why you get the energy error too large, but it is a mistake. I also see you have applied zero displacements in y and z to all the faces of the tool and applied an x velocity to all the faces of the tool. This effectively makes the tool a rigid body. Try picking just the top face of the tool and letting the tool have some deformation as well as the workpiece.
Change the Maximum Energy Error to 10 and request Output at a higher number of points than 80, like 200 points and rerun to see how far the simulation goes and then post details on the deformation at the last output time and we will see how far it got. You can plot the Energy Error to see when it exceeded 0.1.
Explicit Dynamics is inherently a time consuming task. You have a clean mesh to avoid one small element that can slow down the whole model. The only way to get a solution in less time is to find a computer with more cores and a fast clock. If all you want is an illustrative video, increasing the density of the material by a factor of 1000 will speed up the simulation time, but change the physics. I sometimes do that to show a concept when I don't need quantitative data.
November 1, 2018 at 3:44 pmSandeep MedikondaAnsys Employee
To add to what Peter says above. In explicit dynamics simulations, only mass and momentum conservations are enforced and program monitors for the total energy balance have to be monitored by the user, i.e.,
Please see this section of the help that explains this error in detail.
The energy error is just a warning message. It does not mean that the results are completely wrong. The error message just stops the calculation in Explicit Dynamics and let user examine the results before running the calculation further.
Usually, you would need to pay attention to the energy balance if there is a spike in the energy history curve under Solution -> Solution Information -> Energy Conservation.
If the energy error gradually increases, usually the results are OK. If the energy error goes up very quickly in very few cycles, you need to examine the results and the model setup very carefully since it usually indicates the problems with the model setup or the solutions. There could also be problems in the result due to eroded elements, element sizes not small enough and other similar symptoms.
Now, If you think the energy balance looks ok and just want to get the problem to run you can Disable the energy balance check by setting the Reference Energy Cycle to the same number as Maximum Number of Cycles (default 1E+7) in Step Controls. This disables the energy error check in Explicit Dynamics and Autodyn Component systems. The program will still calculate the energy and the energy error but it won’t interrupt the solving process when the energy error exceeds the specified value.
Best Practices on the Student Community
November 19, 2018 at 2:39 pmrupaknayakSubscriber
Can you please tell me that what is the PDE the autodyn solver solves in Ansys Explicit dynamics and displays the result ???
November 20, 2018 at 4:24 amrupaknayakSubscriber
Sandeep medikonda sir plzz answer ??
What i know is only mass and momentum conservation are monitered in explicit dynamics. then how are we able to calculate the temperature (user defined through worksheet) generated ???
November 21, 2018 at 7:02 pmrupaknayakSubscriberSir plzz reply .....
February 24, 2019 at 7:15 pmSandeep MedikondaAnsys Employee
Sorry about the delay. If you post in a discussion which is marked as solved I don't get notified until I explicitly open it like I did today (please take a moment to review the Guidelines). Please open a new discussion for any new questions, this discussion will be marked to be closed.
We are still solving the equations of motion, Temperature is being accounted as an additional degree of freedom using the Co-efficients of Thermal Expansion (CTEs) for that material in the Constitutive Relations.
- 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.