COMPOSITE FAILURE

Scap97
Scap97 Altair Community Member
edited October 2020 in Community Q&A

Hi,

I create a Material Law Type 25 (Orthotrophic Shell) and then create a Property law type 11 (Sandwich Shell). My Sandwich shell is made by 5 layer of the same material and I create it in property. 

I used Tsai-Wu failure model and I add all the 'Yield Stress in direction 1-2 an 12'; while for 'Total element failure criteria' I choose '0' option. 

How can I understand if my laminate will brake or not during the impact? I have to choose some particular control card?

 

Another question:

In post-processing  to show the Von Mises stress I choose two different control cards:

- ANIM_ELTYPE_RESTYPE

-ANIM_SHELL_TENS_RESTYPE

With first control card I obtain a stress of about 50 MPa while with the second one I obtained a stress of about 500 MPa.

How can I understand which is the correct one?

 

Thank you for the help!!

Tagged:

Answers

  • Simon Križnik
    Simon Križnik Altair Community Member
    edited December 2019

    Hi,

     

    to asses if the component will break you need to define failure parameters on law 25 or add failure model. The yield stress parameters only relate to the start of plasticity, not rupture. See the attached document and links for more details:

     

    https://insider.altairhyperworks.com/accuracy-matters/
    https://insider.altairhyperworks.com/composites-rupture/

     

    With Composite stress, you look for stress in each ply (ANIM_SHELL_TENS_RESTYPE). The other stress is homogenized one over the entire laminate (ANIM_ELTYPE_RESTYPE). In composites, it's important to understand stress in each ply. With /ANIM/SHELL/TENS/STRESS/ALL and /ANIM/SHELL/TENS/STRAIN/ALL keywords we can output the stress and strain for all plies in the composite material.

    <?xml version="1.0" encoding="UTF-8"?>1.PNG

    In case failure cards for the composite are provided (like /FAIL/LAD_DAMA, which describes the Ladeveze failure model for delamination (interlaminar fracture) you can input /ANIM/SHELL/IPLY/MAXDA, /ANIM/SHELL/IPLY/DAM keywords in the engine file for extracting damage parameters.

     

    Unable to find an attachment - read this blog

  • pohan
    pohan Altair Community Member
    edited December 2019

    Hi. Try /PROP/TYPE51.

  • Scap97
    Scap97 Altair Community Member
    edited December 2019

    Hi, thanks for replying me!

    I tried using Failure Criteria (Chang) but I obtain only error #44 (abnormal error).

     

    I tried adding on Material description the TOTAL TENSILE FAILURE dir 1 and 2 to show me if some layer or element failed (using control card ANIM_SHELL_TENS_STRESS_ALL and ANIM_SHELL_TENS_STRAIN_ALL )...am I wrong?

     

    Thanks for the help

     

  • Simon Križnik
    Simon Križnik Altair Community Member
    edited December 2019

    Glad to help.

     

    Error ID 44 is a general error and can be due to many modeling issues. Share the model for debugging if possible. 

     

    With total tensile failure defined, the element will be deleted when the specified strain is reached. To output damage evolution use /ANIM/SHELL/DAMA which generates animation files containing a damage value for each layer of a shell element. The damage value is the maximum of damage over time of all failure criteria associated with the material.

     

    You may also find this presentation useful (especially p18-19):

    https://altairuniversity.com/wp-content/uploads/2012/11/Presentazione_Dolci2.pdf

Categories