Radioss 2022.1 - Composite tensile failure not matching

Sanjay Dinker_21074
Sanjay Dinker_21074 Altair Community Member
edited July 2023 in Community Q&A

Hello, 

Currently, I am using Radioss 2022.1 solver for creating composite material model.

We did some coupon level tests on our composite materials.
We have the test data for the tension test (ASTM D3039).

Now I am in the process of making the material model in Radioss 2022.1.

I followed the following procedure,

  1. Post processed the test data to obtain the true stress vs true strain curves.
  2. Calculated the elastic work and the plastic work.
  3. Plotted the graph between plastic work and true stress.
  4. Later used this expression to estimate the b and n parameters.
    1. I estimated these parameters based on the equations specified in CH4-RADIOSS-COMPOSITES-MATERIAL-PARAMETERS-16APR-2019.pdf
  5. Later I specified these values in the MAT25_COMPSH for tension and compression. 
  6. I defined my failure card based on Hashin failure criteria. 
    1. My maximum tensile failure is set to be 361 MPa. Obtained from true stress vs true strain curve.
  7. When I simulate my model, in the .out file -> It is showing that the failure is due to S11 = 361 MPa for a particular element. (element id 97)
    1. However, when I look into the curve using hypergraph or with hyperview, the failure is way lower to 280 MPa.

I am not sure what is happening. I have uploaded my .hm model as well. 

Could you let me know, what I am missing or if I have made a mistake in my modelling approach.
Additionally, if you need more information from me or have any questions, please do not hesitate to reach out to me.

Thanks and regards,
Sanjay Dinker

 

 

Tagged:

Answers

  • Mathis
    Mathis
    Altair Employee
    edited July 2023

    Hi Sanjay,

    I had a deep look into your model and your results. 

    I think there is nothing wrong in your models neither in Radioss results themselves. It is in fact a post-processing topic and also a topic of where the rupture is occuring. 

    The post-processing topic:
    Your model is with Ishell=12, so fully integrated elements with 4 Gauss points in each "integration layer". When you have a message of failure from Hashin, it means that one of the Gauss point has reached the limit of 361MPa that you set but not necessary the 3 other Gauss points. In term of post-processing when you plot stresses in your element (either in HV or HG), Radioss is giving you the average stress over the 4 Gauss points. That's why you have a failure in 1 Gauss point when you actually see a stress lower than your limit Hashin. 

    But you will probably tell me : "well here my values are far below what I expect. Moreover, it is a tensile test, the values should be close to each other in each Gauss points". It is where the second topic comes. 

    The rupture location topic:
    Your rupture occurs at elements connected to a rigid body. As a consequence, the 2 Gauss points that are close to the rigid body are seeing a stress that is much lower than the stress of the 2 other Gauss points. So the average of the stress in the element is relatively small before the rupture of the element. 

     

    How to check that Radioss is doing things correctly? 
    When I switch to reduce integration scheme with Ishell=24 (for instance), there is now only 1 integration scheme, so no question of average. Hence, I have a stress level that fits the expectation:

    image

     

    I hope this answers your question.

    Regards,

    Mathis. 

     

Categories