June 26, 2018 at 5:14 amvelu.annaduraiSubscriber
Can anyone help me to resolve the below issue.
I am facing Convergence issues with Solid185 elements.
i have tried to solve using time steps 5,5,20.but still facing issues.
June 26, 2018 at 12:08 pmpeteroznewmanSubscriber
I assume you have frictional contact in this model.
Did you insert a Contact Tool into the Connections branch of the Outline? Please do that and reply with an attachment for the Initial Contact Results.
Also, take a screen snapshot of the Solution folder Force Convergence Plot. Does it converge on the initial substep and later fail to converge, or does it fail to converge on the very first substep? That is important to know.
Have you turned on the Newton Raphson Force Residual Plots under the Solution Information folder. Those are very useful to show where the convergence problem is.
Finally, you can adjust the Contact Stiffness to help convergence. Sandeep's post provided a link to a good article on convergence issues.
June 27, 2018 at 3:24 am
June 27, 2018 at 10:10 ampeteroznewmanSubscriber
I can see that the solver is trying to apply the entire load in the first substep (Time = 1). We can see that it cut the substep in half 3 times or a factor of 8.
Under Analysis Settings, Step Controls, change the Auto Time Stepping from Program Controlled to On the for Initial Substeps, type 10. That means it will apply 1/10th of the load during the first substep. You can see that in the last bisection, that it almost converged with 8 substeps or 1/8th the load. With 10 substeps, it should converge, but if it doesn't you can type 20 for the Initial Substeps. You can leave Minimum Substeps to 1. The Maximum Substeps must be larger than the Initial and I generally use 100 for that.
June 28, 2018 at 8:35 amAshish KhemkaAnsys Employee
As indicated above by Peter, try increasing the substeps - which will apply the load more gradually. On as safe side try increasing equilibrium iterations - neqit,100. Default is 25/26.
July 3, 2018 at 8:02 am
July 3, 2018 at 11:39 ampeteroznewmanSubscriber
Click on Static Structural and insert a Command object. In the text window that opens, type NEQIT,100 as akhemka suggested. If you used Initial Substeps of 10, change that to 20.
Click on the Solution Information folder and in the details window, type 6 for the Number of Newton Raphson Force Residual Plots. Then click Solve. A plot will be created for the last 6 attempts to converge. The location of the maximum value on those plots shows you where the solver has the largest residual force, which may be larger than the convergence criterion. The corrective action can be to use smaller element size in the area of maximum N-R Force Residual. Sandeep's post provided a link to a good article on convergence issues.
July 3, 2018 at 11:42 amvelu.annaduraiSubscriber
Thanks a lot for your advice which is really awesome.
- 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.
- Solver Pivot Warning in Beam Element Model
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- What is the difference between bonded contact region and fixed joint
- User manual
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- material damping and modal analysis
- Colors and Mesh Display
© 2023 Copyright ANSYS, Inc. All rights reserved.