

January 23, 2021 at 4:29 pm

January 24, 2021 at 2:22 ampeteroznewmanSubscriberArraynBEAM161 was available in ANSYS 18.2 and the Help says, This element is used in explicit dynamic analyses onlyYou will use BEAM188 in ANSYS 2020 R2 in a Transient analysis. This element will be used by default.nCowperSymonds Strength is only in Explicit Dynamics. It is for defining yield strength of isotropic strain hardening, strain rate dependent materials.nIf you are not solving an impact event, you don't need a ratedependent material. If your transient is low speed, you can use RateIndependent plasticity. You have found Bilinear Kinematic Hardening. The paper mentioned Bilinear Isotropic Hardening, which is also available.nYou can use either of these, and neither have a failure criterion. You judge if failure has occurred by plotting Total Equivalent Strain in postprocessing. You have a strain failure threshold of 0.2 which you will compare with Total Equivalent Strain. The simulation will go way past 0.2 if the load takes it there. Use a small Maximum Time Step so you can find a value in the tabular output of Total Equivalent Strain close to 0.2 to know the time when failure occurred.nTurn on large deflection for your analysis setting in the Transient Structural analysis.n

January 24, 2021 at 5:29 pmMickMackSubscriberI am developing structural models of modular buildings so i can work toward progressive collapse analysis, which will replicate sudden removal of columns or entire modules.nnFrom your comments i have now had a cursory look at what may be involved in explicit dynamics from the following websites and the ANSYS helppage nExplicit Dynamics Analysis Guide;nhttps://blogs.rand.com/randsim/2020/11/explicitdynamicsandansysparti.htmlnnFrom reading the information i would consider that i should be using an transient explicit analysis as the removal of the column/or module from the structure will be a sudden change and cause large non linear effects. I have Ansys Academic Research will i be able to use the explicit dynamic analysis (using AUTODYN) based on this license shown below. Do you agree with this?nnI have also included the details of the FE model i am trying to replicate, below, to provide a full picture of what the previous researcher did. Based on this is explicit dynamic analysis the most similar analysis i can use to recreate the LSDYNA analysis?.nI hope i have articulated the above sufficiently well.nnThanks,nMichaelnn

January 24, 2021 at 7:21 pmpeteroznewmanSubscribernHi Michael,nYes, it looks like you have Explicit Dynamics using the Autodyn solver. That is similar to the LSDYNA solver, which you do not have.nYou can use Transient Structural to evaluate if the load is exceeding the strength of the structure.nExplicit Dynamics is good if you want to evaluate the collapse of the structure.n

January 24, 2021 at 11:58 pmMickMackSubscriberWhile i am not expecting the model to fail i may induce failure to study the response. There could certainly be significant buckling as the structure develops catenary actionnnHow can i 'evaluate the load is exceeding the strength of the structure' in transient? Or will it be evident simply by the analysis not converging and the GUI showing a collapse?.There will be most likely several models. Is it best to keep as much of the analysis in transient using NewtonRaphson Method for the models that don't significantly deform and then use the explicit method for the models with larger deformation? nWill i have issues then comparing the results i wonder if i use outputs from two different solvers?.Thanks,nMichaeln

January 25, 2021 at 2:56 pmpeteroznewmanSubscribernHi Michael,nSolid elements in explicit dynamics solutions contain a lot of high frequency noise, so you need to apply filters to the data to plot smooth curves for stress. Transient structural solutions don't have this problem, so yes, it can be difficult to compare results between the two solvers. My experience with Explicit Dynamics has been with solid and shell elements. I haven't had a model with beams in it before, which might behave better.nMost of the time, when the analysis does not converge, that is due to a numerical problem that an improvement in the model will fix, then the analysis can get further than the point at which it stopped with an error.nSome of the time, the analysis does not converge due to physical limits having been reached in the solution, such as a complete plastic hinge causing excessive deformation. This is a true indication of structural failure.nYou may have your own definitions of failure, like a displacement limit. The solver might continue past the displacement limit you have, and you can use solution trackers to plot that displacement as the solver runs so that you can interrupt the solution once it goes past your defined failure limit.n

January 25, 2021 at 3:56 pmMickMackSubscriberThank you for the comprehensive response, i will consider this in detailn

 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.
Ansys Blog
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

5290

3311

2471

1308

1016
© 2023 Copyright ANSYS, Inc. All rights reserved.