

November 2, 2022 at 5:15 pmnds88Subscriber
As the title mentions, I ran a simple model to test the stated process for creating a stable explicit time step as proposed by the Ansys Learning video. So in the model, all I did was create a simple 2x2x2mm Linear Hex of Structural Steel. Following the video for wave speed in a solid element, c = 5856.36 m/s . The characteristic length of this single undeformed element is described in the Explicit Analysis Guide as "The volume of the element divided by the square of the longest diagonal of the zone and scaled by (sqrt2)/3." Doing the math on that, the longest diagonal is the body diagonal of the cube, 3.464mm, and the characteristic length is then 0.3143mm. The mesh output plot, if set to "Characteristic Length (AutoDyn)" reads 0.54433mm. What is the discrepency here? If I run any model using this as my only element size (set to hard to fix its size), then program controlled gives me a time step increment in the post output. If I work back this time step by the CFL condition, the plotted characteristic length from Mesh Diagnostic does not actually give that time step. Also, the Analysis Setting of "Characteristic Dimension: Diagonal" (or any option) does not appear to change that mesh value. I understand that there may be more factors influencing the time step, such as contact, but the guidance for using CFL seems to not work either way. It seems like the best approach to getting a stable time step is to let ANSYS program control it, then take that number and reduce it as needed. I'm almost positive I have done the math right and checked units, but no matter how I try to work it, ANSYS usually gives around half of the CFL value as the initial program controlled time step.

November 3, 2022 at 1:39 amMike RifeAnsys Employee
Hi @nds88
Which version of the help are you referencing? It looks like the scale factor has had a few different typos! It is supposed to be 3/sqrt(2). It is correct in the 2022R2 Help.
Mike

November 3, 2022 at 3:20 pmnds88Subscriber
Hi Mike, this came from 2021R1. It looks like sqrt(2/3) will create the right value though according to the mesh diagnostic (whoops this may have been a typo on my end). Regardless of that, If I set a model to have no contacts, one linear hex, use a time safety factor of 1, add a simple displacement to the element and solve, then time increment in POST still does not equal t = (1)*L/c . Am I missing another factor or is CFL just a starting point to work from?


November 3, 2022 at 3:46 pmMike RifeAnsys Employee
Hi @nds88
Watch out as there is a default scale factor of 0.9 to the time step and not 1 as the equation you are showing has.
Mike

November 3, 2022 at 5:05 pm


 You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from lifesaving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
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.
 How to calculate the residual stress on a coating by Vickers indentation?
 An Unknown error occurred during solution. Check the Solver Output…..
 Saving & sharing of Working project files in .wbpz format
 Solver Pivot Warning in Beam Element Model
 Understanding Force Convergence Solution Output
 Colors and Mesh Display
 whether have the difference between using contact and target bodies
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 Massive amount of memory (RAM) required for solve
 What is the difference between bonded contact region and fixed joint

1970

1726

935

708

391
© 2022 Copyright ANSYS, Inc. All rights reserved.