Hi, I am experiencing similar problems with PLA plastic. I am used to work with large deformation problems, but I think it cannot be applied to this kind of problem since the range of deformation is too small and the non-linear response of the material will be negligible (I do not know if this is also your case). 

I think the best way is to model a non-linear behaviour in small deformations, but I am still working on it. Maybe somebody by any chance could shed some light onto the problem?

Cheers

The non linearity comes from mainly the damage when you are dealing with the 45° test specimen.It's not plasticity for my point of view but only damage. Using damage model like ONERA damage model could answer you question . 

Hi Kangyeong,

With the test data from your material, you can always input the behaviour after the yiels stress. So, instead of specifying plastic yield as

*PLASTIC

1000., 0.

you could say

*PLASTIC

1000., 0.

1.0, 0.001

which is in effect degrading the properties to near zero after a post-yield strain of 0.001 mm/mm. The post-yield stress and strain values would depend on your material of course but also need to be set keeping convergence issues in mind.

If you can use shell-based geometry, you can use the Hashin composite failure criteria available within Abaqus. If these options are not satisfactory, you can of course go with a user-defined material routine, in which case you can go with a maximum principal stress failure crtierion, which is well suited to brittle materials.

In Abaqus, Typically composites are modeled as linear elastic materials. You can use HILL yield surface for plasticity definition for specific cases but it's always suggested to go with UMAT (for Abaqus/Standard) or VUMAT (for Abaqus/Explicit) to define your own material model. 

If you want to use HILL yield surface, please refer the following section in Abaqus documentation for details

23.2.6 Anisotropic yield/creep

Thanks & Regards,

Ranjith.

If you are investigating the failure/ultimate load of the structure you will need to implement a progressive failure algorithm that include a degradation model. The failure criteria mentioned above only identify failure. What you need is to establish how failure at matrix and fibre level affect degrades the stiffness (and strength) of the panel. I am not aware if ANSYS or ABAQUS currently have progressive failure algorithms ready to go. What I do know is that you can code them yourself in ANSYS using APDL. For more detailed information check E.J. Barbero Finite Element Analysis of Composite materials. 

Hi,

Incorporating Material Nonlinearity will always be a cyclic process of Analysing for forces in members, finding the stresses, modifying the Young's modulus based on stress values in Tension, additionally checking for buckling for compression, then repeating the analysis with modified youngs modulus and so on.... The correction due to deformation will be a geometric non-linear analysis. In Purely plastic stage, Youngs modulus reduces to 0 ( Zero) . This does not mean that the Entire structure will collapse. Only those members, where the stresses exceed the yeild value loose the stifness ( AE/L or 12EI/L^3...etc ) in the strictural stiffness matrix. This may lead to a local failure of the structure. If the members are made of different materials, the yield criterion will be different.

Composite Material Construction. In My opinion, convert the Sections to equivalent sections for based on relative Values of A,I, E,K,G, etc. in the calculation of Element stiffness matrix.

Hi,

1) Epoxy (except for toughened epoxy) is usually quite brittle. Cracking in these materials (matrix cracking) will dominate their behavior in tension. Even though on a global level this could lead to a non-linear response, on a material level very little non-linearity is observed in case of tensile loading. However, in case of a shear loading, you could see some significant non-linear behavior. This non-linearity is due to a combination of gradual increase of micro-crack density and plastic flow. It is really not easy to distinguish between these two and cyclic testing is needed to find out which part of the non-linearity is due to damage and which part is due to plasticity.  Since plasticity will not affect the elasticity response (elastic modulus will not change) and damage degrades the modulus (elastic response), it is often assumed that the non-linearity is purely due to damage (micro-cracks), which in most cases makes the analysis result conservative.

2) In abaqus you have the option to use the HASHIN model, which allows for damage initiation and progressive damage propagation. However this model is only implemented for shell elements. If your problem can be solved under plane-stress assumptions, then this model could give you good results. I would advice you to obtain experimental test results for the material system you are using. Usually you need 5 individual material tests:

Use these test results to calibrate the HASHIN model in abaqus. Preferably you want to verify the calibration by simulating a simple material test with a mixed-layup. If the results of the verification is positive in terms of comparison of the load-displacement between the test and analysis, you can carry on with more complex geometries and laminates. 

If, for what ever reason,  you need solid elements, then you can expand the 2D HASHIN model to a 3D model in a UMAT. I believe ABAQUS has an example about writing a 3D HASHIN UMAT. 

I hope this helps. If you need more, please also include the type of analysis you are considering (impact, buckling, etc.) and the solver type (explicit/implicit)