Hello,
When uni-axial tensile test is performed, the stress-strain data obtained from test represents an average property of the specimen. Strain localizes in the necking area after necking occurs. In stress-strain data, local strain after necking is not accurately captured. The local strain after necking is a lot higher.
So question arises when doing FEA for cases where large local strain occurs at the area of interest. For example, in wiping-die bending, and hemming, the strain is localized along the bending line and strain magnitude is normally beyond what is obtained from test data.
So, now I have force-elongation data from the tension test. If I want to simulate those large local strains after necking in tension test ,
1) what material model is appropriate in Ansys?
I am asking this because multi-linear hardening models is valid until necking, since after necking this model assumes constant stress for strain beyond last strain data point.
Bi-linear hardening model goes along the tangent modulus after necking, this is not the correct representation of what happens on reality.
2) How can I get the stress-strain data, which can used as input in Ansys?
Thank you.
It is not possible to obtain the true stress-strain data after necking with the standard tensile test. There are analytical models, like the published by Bridgman, which shows ways to solve this question.
You need to measure the section area and the radius of the necking just after the maximum engineering stress at some points before the final fracture. Bridgman model uses these data to predict the stress-strain behavior after necking, but it works fine only for some specific materials.
Jose Calaf-Chica, Thanks for your explanation.
I want to simulate bending/hemming of aluminum sheets. Tensile tests were done to get stress-strain data for the materials. As I mentioned in my question, there are large localized strain in bending/hemming process. The magnitude typically goes well beyond necking strain. Goal of the simulation is to get the strain after bending/hemming. So, now if I use the stress-strain curve obtained from tension test as material input in Ansys, the stress-strain curve would certainly misrepresent the material behavior after necking.
In addition, I don't have the possibility of measuring the section area and the radius of the necking just after the maximum engineering stress.
How can I get the strain in simulation in this case?
You could simulate the tensile test performed experimentally with a FEM software. The strain hardening data could be introduced in your FEM software as follows:
1. The true stress - plastic strain data until the maximum engineering stress would be obtained from the experimental tensile test.
2. You could introduce a linear strain hardening with a specific plastic modulus "Ep" just after the maximum engineering stress. The value of this Ep would be obtained with iterative FEM simulations of the tensile test, until reach the most accurate match between the load-elongation result of the simulated tensile test and the experimental tensile test.
In this simulation it is important to introduce a critical section area in the geometry of the tensile specimen. For example, if your tensile specimen has a diameter of 12.50mm in the gage length, you have to introduce a small reduction of this diameter in the mid-length of this gage length of, for example, 12.49mm. This is important to motivate the necking at this critical location during the simulation.
Jose Calaf-Chica If I understood correctly, Ep you suggested is tangent modulus of the material. Does that mean the local strain after necking can be estimated using bi-linear isotropic hardening model once Ep is figured out?
What if I estimate the stress-strain relationship after necking using power law, which is obtained by curve fitting to the experimental data?
- Badges
- Science topic