General Mechanical

General Mechanical

Fundamental Calculations of equivalent stress and strain in ANSYS Workbench

    • Soni
      Subscriber
      Hello Everyone,nI am trying to simulate a dog-bone tensile test in Ansys Workbench. I am trying to match the Stress Strain curve output by Ansys with a Stress-Strain curve I calculate manually. i.e. Find out the force along a particular cross-section then divide it by the area of the cross-section. 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
    • peteroznewman
      Subscriber
      The stress-strain 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 stress-strain 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
    • Soni
      Subscriber
      Thank you for the response . Yes, I understand that the stress-strain curve is an input to the ANSYS model, however, after running the simulation, you can determine the forces along a cross-section 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 stress-strain 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?.
    • peteroznewman
      Subscriber
      nIt is best to discuss this with a specific material model because there are different inputs to ANSYS.nFor example, the Stress-Strain 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 stress-strain 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/multilinear-kinematic-plasticity-created-from-a-stress-strain-graphn
    • peteroznewman
      Subscriber
      P.S. I'm glad you understand the stress-strain 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 stress-strain curve!n
    • Soni
      Subscriber
      Thank 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 stress-strain curve and as you say, Ansys plots the true stress-strain, 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 stress-strain 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 stress-strain. This is a photonIn this case, the orange curve is very close to the given material data, but the grey curve (calculated true stress-strain values) are further up. Please could you elaborate what is going on.nI have also chosen the nodes such that they are along the Y-axisn
    • peteroznewman
      Subscriber
      nThe equations that convert Engineering Stress-Strain to True Stress-Strain 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
    • Soni
      Subscriber
      Thank youn
Viewing 7 reply threads
  • You must be logged in to reply to this topic.