August 22, 2018 at 9:16 pmFilipSubscriber
Hi, i spent days to get full stress-strain hysteresis loop but i still do not have the solution. I have chosen nonlinear characteristics on a steel honeycomb element loaded with opposite sine forces with increasing amplitude during time. Since i have to calculate the energy dissipating characteristics i need to plot the total stress strain hysteresis loop. So far i get the results only with positive values (see screenshots). I have tried with even simpler model of a steel stick but the problem stays the same. Can someone suggest a solution? Tnx
August 22, 2018 at 10:16 pmSandeep MedikondaAnsys Employee
Filip, Is the problem when you plot or do you not see any negative stresses being generated in the tabular data at any point? If it is the later then you have different boundary conditions in your model right? Could those be affecting the overall stresses that are being reported?
August 23, 2018 at 7:16 amFilipSubscriber
I do not see negative value for the equivalent total stress in the table too although the boundary conditions allow that kind of displacements. I plot total stress vs total strain, also tried in a node on one site of the surface but the problem stays the same...
August 23, 2018 at 11:34 amSandeep MedikondaAnsys Employee
But this is how equivalent stress is defined. It will be a single positive value.
August 23, 2018 at 2:40 pmpeteroznewmanSubscriber
Sandeep is correct, equivalent stress is always positive.
What I have done in the past to study fatigue issues is to plot two values, Max Principal Stress and Min Principal Stress. The first plots the peak tensile stresses, the second plots the peak compressive stresses. If you have those two results probing a vertex or coordinate point, you will get the full positive and negative values of stress.
Another important point is the material model. You don't show us the properties of the material you are using. Please make a screen snapshot of the Engineering Data for that material. If you only have Elasticity and no Plasticity defined, there will be no energy dissipation. If you have defined Plasticity, what kind of plasticity, because Isotropic plasticity is not appropriate for evaluating stress cycles since the yield surface will expand. Kinematic plasticity is better because the yield surface translates and when the stress is reversed, the yield surface is closer and plastic strain occurs sooner. The best model is Chaboche Kinematic Hardening.
All this talk of plasticity assumes your displacements take the material past yield. If not, then the linear elastic material model is sufficient. The stress range, when below yield, can be plotted against the Stress-Life fatigue curve for the material to evaluate cycles to failure.
August 24, 2018 at 2:02 pmFilipSubscriber
Sandeep, i totally agree and i understood your point.
Peteroznewman, i have defined nonlinear structural steel with bilinear isotropic hardening but i assume that at least the loop have to follow the rule of the material, so later on i will play with the type of nonlinear material. The goal is to get the Strain vs Stress plot of the whole model as in the attached photos.
This is the input material model
this is what i get when i plot the max principal stress, max principal stress and total strain.
August 24, 2018 at 5:07 pmpeteroznewmanSubscriber
Thanks for the images. I see a problem with the mesh. Solid elements that fill a thin member and experience bending must have three or more elements through the thickness to properly capture the variation in stress through the thickness. See this post and the one below it for an example.
August 24, 2018 at 9:46 pmFilipSubscriber
I tried your suggestion but nothing happened. I started again with the simplest form of exercise, a steel cube loaded with + and - displacements. The goal as i said before is to get the stress vs strain hysteresis loop. The material characteristics, meshing, boundary conditions and some of the results are shown on the photos.
i do get the strain energy from the plot but i need the full stress strain loop.
What should i exactly plot in order to get what i need?
Best regards, Filip
August 25, 2018 at 2:03 ampeteroznewmanSubscriber
That's great that you made a special cube model to study the material properties! I've been doing that myself. There is an improvement you can make. Delete the Fixed Support and replace it with a zero Z displacement support, then supplement that with a zero Y displacement support on the face normal to the Y axis, and a zero X displacement support on the face normal to the X axis. Now when you apply a displacement on the face opposite the zero Z face, the cube is free to expand and contract due to the Poisson's Ratio.
You can't get the plot you want inside ANSYS. You have to do some manual labor to get it to come out the way you want. The example I show below is for this material. I made the modulus ten times more flexible so the slopes are not so steep on the plots.
I then applied the following displacement time history to the face on cube that is 112.4 mm long.
I requested the Normal Stress, the Elastic Strain and the Equivalent Plastic Strain, shown below.
Notice that the last plot, Equivalent Plastic Strain, doesn't look like the others. That is because equivalent results are always positive, but to make your plot, we need signed plastic strain. Maybe one of the ANSYS members who knows more than me will tell us the result to use, but I just manually flip the plastic strain to the opposite side by multiplying the hump that should go down by -1. Then I get a signed plastic strain.
Add this to the elastic strain to get a signed Total Strain. Now you can plot the Stress vs signed Total Strain.
You can show your appreciation by clicking Like below the posts that are helpful.
August 25, 2018 at 1:50 pm
December 4, 2022 at 6:32 amMLS MLSSubscriber
I'm trying to correlate experimental low cycle fatigue data with simulation but the stress-strain loop that i obtain is different from the experimental data even if i succes to fit the chaboche parameters using ansys.
Above is the fit.
I tried with a single cube (1mm x 1mm x 1mm) in order to get the stress and the strain using a sine function as load with a displacement magnitude of 0.01mm and R = -1 but the stress and strain are completely off.
Can anyone help please with the FEM model ?
- You must be logged in to reply to this topic.
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.
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.
- Saving & sharing of Working project files in .wbpz format
- Understanding Force Convergence Solution Output
- An Unknown error occurred during solution. Check the Solver Output…..
- Solver Pivot Warning in Beam Element Model
- Colors and Mesh Display
- whether have the difference between using contact and target bodies
- How to calculate the residual stress on a coating by Vickers indentation?
- What is the difference between bonded contact region and fixed joint
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- User manual
© 2023 Copyright ANSYS, Inc. All rights reserved.