Tensile Test Modeling in LS-Dyna

[DynaUser]

I'm trying to model a simple tensile test for a Polypropylene material in LS-Dyna.

1. Converted the Engg Stress-Strain data from tensile test and converted into plastic strain - true stress.
2. Used Mat_24 in Dyna- (Defined yield value and hardening curve)
3. Meshed the specimen as per test specifications. Constrained at one end and pulled at a very slow rate on the other end.
4. Extracted Secforce (at necking area) and also SPC force from constrained end in LS-dyna (obviously these two data matches)
6. Engg stress = Force /Ao & Engg strain = /\L/L. and cross
plotted the data
7. Compared the LS-dyna Engg S-S to actual Test.
8. The Results DON'T MATCH. {Especially after Yielding}

I did this for plastic material and also for high-strength steel. The simulation vs test seems to match very good for HSS, but very bad for plastic especially after yielding. Refining the mesh for plastic
(element size down to 0.5 and taking care of timestep) is not helping. However, if I just take 1-element (for plastic material), then my input matches output. In other words Test vs simulation results match.

Is this approach right? Why are not the results matching for plastic material when I have the compete specimen?
Thanks for any inputs

[Jorgen]

Hello DynaUser,

Very interesting question. First, your approach seems fine.

If I understand you right, you have a problem in that the full simulation of the test specimen using the calibrated material model did not match the experimental data, but that a 1-element simulation does match.

I think I know what is going on. You are using a material model that was developed for metals, and hence work well for metals, but that does not capture the large-strain multiaxial deformation behavior of polymers such as polypropylene. That is, even though Mat_24 can be calibrated to the uniaxial data, it does not provide accurate predictions of more general deformation states (which is what is going on the test specimen).

This is a well known problem that occurs when metal plasticity models are applied to plastics: you can often get good calibrations, but the model predictions are not good for general multiaxial deformation states.

The solution in this case is to use a more accurate material model that is specifically developed for polymers.

- Jorgen

[DynaUser]

Dr. Jorgen

Thanks for the insights. I have seen LSTC recommending MAT_24 for plastic modeling. Is it because of lack of good material model for modeling plastics.

Moreover, the way I'm looking at is, my input data into model (derived from tensile test) is matching the simulation output data when I simply use 1-Element. This means my input is matching output. (which essentially means the 1-element is following the Stress-strain curve defined through MAT_24 card). However when I have the compete specimen model, my input is not matching output. Is this because of large strains in lateral directions as mentioned in your reply?

Thanks-

[Jorgen]

It is common to use MAT_24 for plastic modeling. The main reason for this is that it is a simple to use model. It is quite clear, however, that this model is not an accurate, general purpose model for plastic modeling. There are other models that are much more accurate and applicable in general situations. These more advanced models, have the disadvantage of currently not being built-into the software but are only available through external subroutines.

The difference that you noticed between 1-element and true geometry modeling using multiple elements is a nice example illustrating the "danger" of calibrating a material model (such as MAT_24) to a small set of experimental data and then expecting that just because you were able to get a good calibration fit, that the calibrated model is accurate in more general deformation modes. As you noticed, that is not always the case.

It is important to perform both calibration and validation of the material model in order to built confidence and check the accuracy of the model predictions.

Jorgen