March 31, 2020 at 1:20 pmAutonewbieSubscriber
I am converting engineering stress strain to true stress strain. I got a material spec as below:
Yield Stress = 25 MPa, Yield Strain = 2.1% but E = 3100 MPa.
Does E is initial modulus as Yield Stress/ Yield Strain not equal to 3100 MPa?
So Plastic Strain should be started after Yield Stress = 25 MPa, right?
March 31, 2020 at 4:58 pmWenlongAnsys Employee
For materials like metal, yield strain is usually defined as 0.2% shifting, and it is possible that the stress-strain curve is not linear before the yield strain and Yield stress/E not equal yield strain. Your E should be the initial modulus.
Please refer to https://en.wikipedia.org/wiki/Yield_(engineering) for more details.
April 1, 2020 at 1:26 am
April 1, 2020 at 2:28 pmWenlongAnsys Employee
Before yielding, the elastic strain value is calculated by stress/initial modulus. At the yielding point, the plastic strain is 0. Note the difference between plastic strain and yielding strain. So the first point you should input for the multilinear isotropic hardening model is plastic strain = 0, stress = 25MPa.
April 2, 2020 at 1:26 amAutonewbieSubscriber
I understand the plastic strain starts at 0. I am not sure the yielding point....
If I use 25MPa, the modulus is not equal to initial modulus.
Another issue is the yield at break is 4% at 31MPa, I guess it is too close to the strain at yield. The calculated True Stress is lesser than the true stress at previous point which is not allowed in MISO...
April 2, 2020 at 2:14 pmWenlongAnsys Employee
1. I understand 25MPa/3100MPa ~= 0.008, which is not equal to 2.1%, I would contact the manufacturer and find out how that yield strain is defined. Or, if better, get the stress vs. strain curve.
2. Right. Multilinear hardening does not allow a less than 0 tangent modulus, so you cannot model the softening behavior using the hardening model. In static structural analysis, it is not common to model the softening behavior of metal as it is hard to converge.
April 4, 2020 at 1:22 amAutonewbieSubscriberHi Wenlong
I have the yield stress and strain in the material spec as well as stress strain data provided by supplier.
The yield stress and strain is not measured at 0.2% offset. It is plastic material.
My concern is whether the elastic strain is set, always, at 0.2%?
April 4, 2020 at 7:42 amAutonewbieSubscriber
I have another question that if the stress in the model exceeds the max true stress/ strain in MISO, would it cause the simulation unconverged?
April 4, 2020 at 2:51 pmAutonewbieSubscriber
I attached the data below for better discussion. I tried to use MISO and take the data up to max point as the following points after max stress show lower true stress. It is mainly due to the strain is very small. I have other case where the break point is 50% strain and true stress is much higher.
However, this way does not work. It does not converge... so I change to use BISO and use the tangent modulus at YS given instead of at the elastic limit from the chart. Any thoughts?
Yield Stress = 25 MPa
Yield Strain = 2.1%
E = 3100 MPa.
April 5, 2020 at 7:20 pmpeteroznewmanSubscriber
Read this discussion to help understand how to use Multilinear Hardening Plasticity.
- Discard the Yield Strain of 2.1% that the manufacturer provided. It is meaningless here.
- I drew an orange line for E=3,100 MPa. Look at how it is wrong. That is not the initial slope.
- I drew a green line through the linear portion of the curve to estimate the initial slope.
- It looks like the linear portion ends at 10 MPa, so that is the Yield Strength.
- From the plot, the strain at 10 MPa is about 0.002 so the Initial Modulus is 10,000/.002 = 5,000 MPa not 3,100 MPa.
- Make the Young's Modulus 5000 MPa.
The first row in the multilinear kinematic hardening plasticity column will look like this:
April 6, 2020 at 7:22 pmWenlongAnsys Employee
"The slope of the stress-strain curve is assumed to be zero beyond the last user-defined stress-strain data point." according to the manual.
- How to access Ansys Online Help Document
- How to show full resolution image
- How to use Google to search within Ansys Student Community
April 7, 2020 at 3:34 pmAutonewbieSubscriber
I used BISO instead of MISO for better convergence issue... I draw two lines below... at this case, yield strength is approximately 28MPa...
I wonder if I assess for plastic deformation, I should use the yield strain following the bilinear chart below, which is 0.6%? And plastic strain calculated in ANSYS would be where the total strain exceeds 0.6%?
Lastly, when the part show largely plastic strain, it does not mean that the whole beam will not return to its original position, is that right?
April 7, 2020 at 3:54 pmAutonewbieSubscriber
Based on the bilinear above and assume 1% yield strain, I run a simulation and hope to see how the plastic deformation looks like...
The beam tip is being pushed by large displacement and released at last step... I notice some plastic deformation but not as severe as I expect although the area exceeds yield (>1%) seems to be very large area...
I was expecting if the root shows largely plastic deformation, the beam will not be returning back to original position...any idea? Thanks
April 7, 2020 at 9:35 pm
April 8, 2020 at 12:38 amAutonewbieSubscriber
Hi, it is true scale.
April 8, 2020 at 1:33 ampeteroznewmanSubscriber
How are you "releasing" the tip after using a Displacement to move it to the left?
If you had a Displacement of 10 mm in Step 1, and the Displacement in Step 2 is 0 mm, that is not releasing the tip, that is forcing the tip back to 0.
In order to release the tip after using a Displacement to move it 10 mm to the left in Step 1, you have to Deactivate the Displacement boundary condition in Step 2.
April 8, 2020 at 1:42 amAutonewbieSubscriber
I think I know the problem. I set it to 0 at step 2. It works now!
- 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 life-saving 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.
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.
- What is the difference between bonded contact region and fixed joint
- Massive amount of memory (RAM) required for solve
© 2022 Copyright ANSYS, Inc. All rights reserved.