Tagged: 15, materials, mechanical, plasticity, structuralmechanics


January 25, 2023 at 7:34 amFAQParticipant
Question: What is the difference in plasticity definition for bilinear vs. multilinear models? Is the bilinear stressstrain definition based on total strain or plastic strain? What does the multilinear stressstrain input require plastic strain? Answer: Please note that the definition of multilinear vs. bilinear stressstrain curves in Engineering Data are different. When we define bilinear stressstrain curves, we define the tangent modulus “E_T” based on total strain. It is the slope of stress (“sigma”) vs. total strain (“epsilon_total”) curve after yielding. We do this because the input is simple from the user’s standpoint. If we take E_T as the tangent modulus of stress vs. total strain, we have the following relationship for plastic strain (“epsilon_plastic”): delta(sigma) = E_T * delta(epsilon_total) delta(sigma) = E_T * (delta(epsilon_elastic) + delta(epsilon_plastic)) delta(sigma) = E_T * (delta(sigma)/E + delta(epsilon_plastic)) delta(sigma) * (1 – E_T/E) = E_T * delta(epsilon_plastic) delta(sigma) = E*E_T / (E – E_T) * delta(epsilon_plastic) and you will see here that “C” is the slope of stress vs. plastic strain, but it is not the input tangent modulus “E_T”. Instead, “C” is equal to “E*E_T/(E E_T)”. For multilinear stressstrain curves, in Engineering Data, however, we define stress vs. plastic strain. This is because, if you define stress vs. total strain, the stressstrain data contains elastic information that must be consistent with the elastic modulus (i.e., yield point defined by (sigma_y, epsilon_y) must line on the elastic modulus slope). There are some cases where users have temperaturedependent data for E and nuxy that are different than the temperaturedependent stressstrain data, and when the solver does the interpolation, E(T_i) may not match with (sigma(T_i), epsilon(T_i)) – we would have a problem since we would end up with two different yield points, and it’s not clear which to use. To prevent this type of inconsistent definition, we only define stress vs. plastic strain in Engineering Data. If you have true stress vs. total strain, in Excel, simply add another column for elastic strain calculations, which would be your current stress divided by elastic modulus. Then, subtract your column of elastic strain from total strain to get plastic strain, which would be used for input into Engineering Data. A common mistake is to determine the elastic strain at yield and subtract this constant value from the total strain, but this is not correct; after initial yield, as long as there is strain hardening, your stress will increase, which implies that elastic strains increase as well.

Introducing Ansys Electronics Desktop on Ansys Cloud
The Watch & Learn video article provides an overview of cloud computing from Electronics Desktop and details the product licenses and subscriptions to ANSYS Cloud Service that are...
How to Create a Reflector for a Center HighMounted Stop Lamp (CHMSL)
This video article demonstrates how to create a reflector for a center highmounted stop lamp. Optical Part design in Ansys SPEOS enables the design and validation of multiple...
Introducing the GEKO Turbulence Model in Ansys Fluent
The GEKO (GEneralized KOmega) turbulence model offers a flexible, robust, generalpurpose approach to RANS turbulence modeling. Introducing 2 videos: Part 1 provides background information on the model and a...
Postprocessing on Ansys EnSight
This video demonstrates exporting data from Fluent in EnSight Case Gold format, and it reviews the basic postprocessing capabilities of EnSight.
 Question: What is the difference between PLNSOL, EPPL, EQV and PLNSOL,NL,EPEQ?
 Guidelines of modeling a gasket.
 ANSYS Mechanical: Delamination Analysis using Contact Debonding
 How to use layered section to simulate composites and post process the results in ANSYS Mechanical
 ANSYS ACCS: Simulation of a Composite Rib Using ANSYS Composite Cure Simulation Tool
 What are Isochronous stressstrain curves? How can they be used in ANSYS for modeling creep?
 Why is the unit of the elastic foundation stiffness N/m^3?
 Hyperelastic Simulations
 For the stresslife fatigue method, how are the Goodman and Gerber mean stress theories used to modify the calculated stress amplitude in the Workbench Fatigue Module?
 How do I enter major Poisson’s ratio in ANSYS Mechanical?
© 2024 Copyright ANSYS, Inc. All rights reserved.