Problem: Plastic strain results do not match with the Von Mises stress results.

Altair Forum User
Altair Forum User
Altair Employee
edited October 2020 in Community Q&A

Hi all,

 

I'm getting very low plastic strain results in my simulations. the Von mises stress (422 MPa) clearly passes the yield point (355 MPa), however plastic strain only reaches a value of 0,008. This Von mises value approaches the UTS value of 455 MPa, the strain at uts is defined as 0,09. Can someone please explain to me how i can solve this, or explain why this is happening?

 

materiaal_Definitie.JPG.1f7a4f035a9bbb5c3c0d61601260ac3f.JPG

<?xml version="1.0" encoding="UTF-8"?>1871648011_VonMises.thumb.jpg.f55da6f263efe4327e83817706c407da.jpg

 

<?xml version="1.0" encoding="UTF-8"?>Plastische_rek.jpg

Unable to find an attachment - read this blog

Tagged:

Answers

  • Andy_20955
    Andy_20955 New Altair Community Member
    edited May 2019

    Hi,

    With LAW2, Iflag=1 the UTS and strain at UTS are engineering strain values.    But the output by Radioss is true stress and strain.  If you look in the Radioss starter you can see the Iflag=0, a, b, n values that are calculated using your input. 

      

     JOHNSON COOK MODEL :      YIELD STRESS  . . . . . . . . . . . . .=  355.0000000000          ULTIMATE STRESS (UTS) . . . . . . . . .=  470.0000000000          STRAIN AT UTS (Ag). . . . . . . . . . .= 9.0000000000000E-02      YIELD COEFFICIENT A . . . . . . . . . .=  355.0000000000          YIELD COEFFICIENT B . . . . . . . . . .=  312.9879880695          YIELD COEFFICIENT N . . . . . . . . . .= 0.2806664576242          EPS-MAX . . . . . . . . . . . . . . . .= 0.2100000000000          SIG-MAX . . . . . . . . . . . . . . . .= 1.0000000000000E+30      ISO-KINEMATIC HARDENING FACTOR. . . . .=  0.000000000000

     

    You can input the a, b, n value into the equation in the comments of LAW2.  image.png  Note this equation is true stress as a function of plastic strain and I have left off the temperature and strain rate terms.

     

    Or the pre-processor HyperCrash lets you plot a material when you use a, b, n in LAW2.

     

    screenshot.699.png

     

    Note that this is a plot of True stress versus true strain (not plastic strain). 

     

    Please check if your output makes better sense using these stress strain plots. 

     

    It is good that you are thinking about the results with respect to your material input to see if they make sense.  Not everyone does this but they should!

     

    Thanks,

    Andy

     

  • Altair Forum User
    Altair Forum User
    Altair Employee
    edited May 2019

    Hi Andy,

    Thank you for you're response and insight.

     

    So it could be that the plastic strain of 0,008 is realistic. When I calculate the stress with the JC formula, I get a true stress value of 435 MPa at a plastic strain of 0,008. Which could match the true stress strain plot. 

    Could you tell me how the Plastic strain is calculated for post processing purposes?

     

    Thanks,

    Cedric

Categories