March 22, 2021 at 10:44 ambouzasoscarSubscriberHello everybody!nI'm trying to implement a probabilistic nonlinear structural analysis (using optisLang) so I need to define my desired inputs and outputs as parameters (I'm using Mechanical, not APDL).nI have two time steps. During first time step, self-weight loads are applied, then, in the second time step, forces required by the standards are applied. Probabilistic analysis is going to compare if the solution converge (pass) or not (fail), in order to do it I am trying to compare the last converged time step with 2 (pass if the last converged time step is equals to two, fail if the last converged time step is lower than two).nBut I have a problem. I need to parameterize the last time step in solution output, but Ansys always takes the last time step equals to two, it doesn't care if the solution converge or not.nIs there a way to parameterize the last converged time step?nThanks in advance.n
April 23, 2021 at 3:27 pmMike RifeAnsys EmployeeSo first point is that WB Mechanical is still using MAPDL as the solver. Which is good as MAPDL writes the unconverged results to the result file but as sub-step number 999999 of the load step. A post processing command object can be used to *get the number of the last sub-step and if equal to 999999 then set some parameter to say one, otherwise set it to zero. If a post processing command object parameter is named with a leading my_ that parameter gets pulled into the command object list of parameters in the Mechanical UI. And these can be flagged as WB parameters.nPlease see the MAPDL Help, Command Guide on the following commands: ncnv, finish, /post1, set, *get, *ifnNCNV is used in a environment (where loads are defined) command object. Set the value to 2 to continue processing the input file if the solution fails (due to non-convergence). When the solve fails the command will then skip ahead in the input file to the next FINISH command.nThen the post-processing command object will:nFinishnEnter the post processornRead in the last set of resultsn*get the current sub-step numbern*if/*else/*endif construct to set a my_ parameter value based on the current sub-step number.nHave fun.nMiken
April 27, 2021 at 3:52 pmbouzasoscarSubscriberThank you so much, Mike! It works perfectly.nHave fun.n?scarn
- You must be logged in to reply to this topic.
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.
- Saving & sharing of Working project files in .wbpz format
- An Unknown error occurred during solution. Check the Solver Output…..
- Understanding Force Convergence Solution Output
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- How to calculate the residual stress on a coating by Vickers indentation?
- whether have the difference between using contact and target bodies
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.