ASME Section VIII Division 2 - Protecion Against Local Failure

[antoniol]

I perform calculations according to 5.3.3 Elastic-plastic analysis - Local strain limit. According to Step 2, the equivalent stress should be calculated according to equation (5.1.). Equation 5.1 is a simplified version of von Mises (for principal stresses), which is calculated using only principal stresses. If I calculate a 3D model with results in x, y and z directions and shear stresses, should I still use this equation 5.1 as a user-defined variable in abaqus? Or should I use the von Mises equation, which also includes shear stresses? in case of my calculation using eq. 5.1. it is impossible to convert equation 5.6

 

[IdanPV]

Check out the following discussions that may help you:

Questions Regarding ASME VIII-2 Part 5 - ASME (mechanical) Code Issues

Hello All, Few questions regarding the use of non-linear FEA and ASME VIII-2 Part 5. 1. Is there any mesh setings requirments for the elastic-plastic method? I know that for the elastic analysis, you must have enough elements through the thickness in order to get an accurate SCLs. But, what...

www.eng-tips.com

How to calculate Strain limit in elastic plastic analysis-local strain limit (ASME VIII Div 2) - Boiler and Pressure Vessel engineering

Hi Everyone Can anyone guide me how to calculate how to calculate local strain limit Ɛpeq in equation 5.7 in Elastic plastic local strain limit in ASME VIII div 2. Regards Senthil ramajayam

www.eng-tips.com

How to calculate Strain limit in elastic plastic analysis-local strain limit (ASME VIII Div 2) - Boiler and Pressure Vessel engineering

Hi Everyone Can anyone guide me how to calculate how to calculate local strain limit Ɛpeq in equation 5.7 in Elastic plastic local strain limit in ASME VIII div 2. Regards Senthil ramajayam

www.eng-tips.com

Local failure assessment of nozzle junctions - weld sharp edges - Finite Element Analysis (FEA) engineering

Hi, i need to analyze the nozzle junction of a pressure vessel (designed by ASME XIII div. 1) according to appendix 46 (following the steps of div. 2 part 5). i am using an elastic plastic model. i´ve searched a lot of threads of this subject but none of them answers my particular inquiry...

www.eng-tips.com

Check also this Linkedin post:

Idan Raz on LinkedIn: #solidworks #designbyanalysis #asme #fea #pressurevessels

ASME VIII-2 - Protection Against Local Failure When conducting finite element analysis in accordance with ASME Section VIII Division 2, it is imperative for…

www.linkedin.com

 

[TGS4]

If you are using Abaqus, then skip user-defined variables, and just directly use the Ductile Damage Material Property and the DMICRT variable. And whether the von Mises invariant is calculated using the principal stress approach, or the normal and shear stresses, you will get the exact same answer.

See this paper.

Or am I completely not understanding your question?

 

[antoniol]

If you are using Abaqus, then skip user-defined variables, and just directly use the Ductile Damage Material Property and the DMICRT variable. And whether the von Mises invariant is calculated using the principal stress approach, or the normal and shear stresses, you will get the exact same answer.

See this paper.

Or am I completely not understanding your question?

Thank you for your reply.
I read a paper about using Ductile Damage Material property, but in my case it is not possible (there is a need to include forming strain based on the material and fabrication method).
For this reason, I want to use user-defined variables.
In my case there is a problem with equation 5.1 (the equivalent stress). In some specific areas I got really small results (I believe this is due to the fact that shear forces are acting in these areas).
Because of this small values of eqvalent stress when I tried to calculte limiting triaxial strain using eq. (5.6) I got the error: over or underflow in exp math operation.
I checked that when I use MISES equation that also includes shear stresses no such problem appears. That's where my question comes from if I can use the von Mises invariant calculated using the normal and shear stresses

 

[TGS4]

Don't forget that the equation 5.1 references the principal stresses - so the calculation of von Mises stress will, by definition, be the same whether you use the component stress (and shear stress) formulation or the principal stresses.

Nevertheless, in a situation where you have perfect triaxial tension, the von Mises stress is identically zero, which leads to a potential divide-by-zero result in Equation 5.6. That should be captured, not as an error, but as a situation where X/0 = infinity, and therefore e^-infinity=0, so the limiting triaxial strain is zero.

 

[IdanPV]

Why don't you extract the 3 principal stress and the equivalent stress directly from the FEA software and use them to calculate determine the limiting stress using eq. (5.6)?

I build an excel spreadsheet for that and it works pretty good.

 

[antoniol]

Thank you TGS4 and IdanPV. I found the solution of my problem.