

September 29, 2020 at 10:36 amSoniSubscriberHello Everyone,nI am trying to simulate a dogbone tensile test in Ansys Workbench. I am trying to match the Stress Strain curve output by Ansys with a StressStrain curve I calculate manually. i.e. Find out the force along a particular crosssection then divide it by the area of the crosssection. Further, I calculate the strain by selecting two nodes at random and then divide the difference in the deformation by the original distance between them. I think we should be able to obtain the same curve using both the methods. However, I am unable to get the same curve. Please could someone help? Can someone elebaorate on the theory used bx Ansys to calculate the equivalent stress and strain?nI would be thankful for any inputnnwarm regards,nPratikn

September 29, 2020 at 12:01 pmpeteroznewmanSubscriberThe stressstrain material curve is an input to an ANSYS model.nWith that input, ANSYS can compute a stiffness matrix for a shape, compute the unknown deformations that provide a force balance equilibrium, convert the deformations to strains, then use the stressstrain curve to compute stresses.nThere are six components of stress in a 3D solid model. For ductile materials, it is helpful to compute the von Mises Equivalent Stress from those components to compare with the Yield Strength measured in a tensile testing machine. That allows the engineer to decide if the loading generates a peak equivalent stress that is above the yield strength, and therefore, the design is unable to support that load without yielding.n

September 30, 2020 at 7:31 amSoniSubscriberThank you for the response . Yes, I understand that the stressstrain curve is an input to the ANSYS model, however, after running the simulation, you can determine the forces along a crosssection and divide it by the area to obtain stress. Similarly, from first principles, the strain can be obtained by choosing two nodes at random and dividing their change in length with the initial distance between them. If we plot stress vs strain thus obtained, shouldn't we obtain the same stressstrain curve that we have input? For me the curves do not match. My question is, am I calculating the stress and strain to simplistically ? Are there some more factors in ANSYS calculations that I don't know about?.

September 30, 2020 at 11:55 ampeteroznewmanSubscribernIt is best to discuss this with a specific material model because there are different inputs to ANSYS.nFor example, the StressStrain data input to the Multilinear Kinematic Hardening Plasticity material model is in terms of True Stress and True Strain.nANSYS plots True Stress on a stress plot.nWhen you divide a force by an original area, you are calculating Engineering Stress, so you would have to convert that to True Stress to compare with the input curve.nIf you are talking about the linear elastic portion of the stressstrain curve, then there is no significant difference between the two.nYou said that you would choose two nodes at random. It would be better to choose two nodes along the axial direction of the dog bone sample.nHere is a link to the equations to convert Engineering Stress and Strain to True Stress and Strain.nhttps://forum.ansys.com/discussion/472/multilinearkinematicplasticitycreatedfromastressstraingraphn

September 30, 2020 at 11:57 ampeteroznewmanSubscriberP.S. I'm glad you understand the stressstrain curve is an input to ANSYS. Some members have posted questions on the forum that implied that they did not know that and expected the software to behave like a tensile testing machine and tell them the stressstrain curve!n

October 1, 2020 at 7:09 amSoniSubscriberThank you, that clarifies quite a few things. nThe material model I am using is Multilinear Isotropic Hardening Plasticity. nThis is an Excel Plot of the curves that I have plot. The orange curve is the engineering stressstrain curve and as you say, Ansys plots the true stressstrain, I calculated it and that turns out to be the grey curve. This grey curve, although matches with the given data from material curve, it does so only up to a certain point. The red curve is directly obtained by plotting the stressstrain given by Ansys and it matches better than the grey curve. Considering that both calculations are performed by ANSYS, shouldn't they be almost similar?nThe above data is with large deflections 'on'nI also found something else that is quite interesting, after turning off large deflections, and using the forces thus obtained, the curve seems to match quite well. And in this case, it matches directly, there seems to be no need to calculate true stressstrain. This is a photonIn this case, the orange curve is very close to the given material data, but the grey curve (calculated true stressstrain values) are further up. Please could you elaborate what is going on.nI have also chosen the nodes such that they are along the Yaxisn

October 1, 2020 at 4:57 pmpeteroznewmanSubscribernThe equations that convert Engineering StressStrain to True StressStrain are only valid up to the point where necking begins. After necking begins, the equations no longer work. nYou must have Large Deflection On to model Plasticity.nWatch this video for further understanding.nn

October 1, 2020 at 7:51 pmSoniSubscriberThank youn

 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
 whether have the difference between using contact and target bodies
 Colors and Mesh Display
 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

1862

1677

917

670

351
© 2022 Copyright ANSYS, Inc. All rights reserved.