Abaqus VS Patran/Nastran for Tsai Wu

[ben38360]

Hello everyone,

I'm currently doing a finite element analysis of a composite plate (45/0/0/-45/90/-45/0/0/45) under tensile load.

I'm using 2 softwares to calculate the F.I. according Tsai Wu theory.

Patran/Nastran gives me : FI (90deg ply) = 0.65, FI (45deg ply)=0.25 and FI(0deg ply) = -0.1

SAMCEF and hand calculations gives me the same results.

However, when I run the analysis in Abaqus, I have some problems.
All the stresses (S11,S12,S22) in each ply are the same as Patran or Samcef but the Tsai Wu failure indices are different.

FI (90deg ply) = 0.65, FI (45deg ply)=0.35 and FI(0deg ply) = 0.21

I have checked the allowable stresses but it's ok. In addition to that, failure indices according the max stress theory match the results coming from Patran.

Moreover, if I perform hand calculations with the stresses given by Abaqus and the tsai wu equation given in Abaqus documentation, I get the Patran results. But Abaqus viewer plots the wrong indices...

I have heard about the fact that Abaqus does not manage the negative failure indices...

Does anyone of you could help me to overcome this problem???


Thank you

 

[loki3000]

http://www.eng-tips.com/viewthread.cfm?qid=289576&page=3

here is something similar

 

[ben38360]

Hi,

Thank you but I'm already able to plot the tsai wu failure indices. My question is about the fact I don't get the good failure indices even if I have the good stresses in the laminate.

 

[RPstress]

The failure indexes really should tie up. It sounds as though there's a problem with Abaqus and Tsai-Wu, but that seems very unlikely. These sort of post-processing activities should be realtively simple to implement and be subject only to 'finger trouble' types of errors in coding.

You say that you've heard that 'Abaqus does not manage the negative failure indices.' It really shouldn't matter. A negative Tsai-Wu FI is certainly possible. For what it's worth the closest I can get is 90° ply 0.62, 45° ply 0.26 and 0° plies -0.016 for that layup in carbon under tension. That's at ply centrelines. It's possible that Abaqus and whatever that bit of Patran is are using ply extremeties vs. centrelines to recover stresses, but then the stresses should show a difference.

There can be problems with failure indexes and conversion to RFs, where Tsai-Wu needs a conversion using a quadratic equation, which some people don't implement for some reason. However, that shouldn't affect the FI. Because this sort of work is dependent only on the stresses in a ply it shouldn't be dependent on the actual FE analysis methods; it should work with Abaqus explicit and implicit. (Different analysis techniques will cetainly make a difference to the stresses, but not the derivation of something as crude as FIs from those stresses. If your stresses aren't different then neither should your FIs be.)

Try to understand possible limits for the FIs in Abaqus. If you can isolate an apparent problem that is general and not specific to one loading and material/layup combination, then you'll have a problem that you can take to their help service. For instance, try to isolate the behaviour with simpler loading such as some even simpler layups with unidirectional loading.

 

[ben38360]

Thank you for your answer. I will try to do so.

 

[MorAero]

Hello everyone,

I'd like to obtain the FI values of a SOLID model using Patran/Nastran 2010. Also if I active the 'Material Status=Failure' of my model using isotropic or orthotropic material I can't obtain my results. Any reference to the criteria I choose is in the .bdf file.
Does anyone of you can help me?
...Thank you!

 

[RPstress]

MorAero: you need red flag your current post and start a new thread with a new title (maybe along the lines of 'failure indexes for solid anisotropic elements in Nastran' or similar). I have to say I'm not at all sure how to get this, other than by post-processing the element stresses/strains in a spreadsheet. Composite 3D elements in Nastran are used relatively rarely in my experience, and mostly for sandwich. There aren't that many true 3D failure criteria for laminates, if that is what you have.

 

[Hansmeister]

One possibility for not having the Failure Index's match is that Tsai-Wu requires an interaction term. On some programs that can be set by the user, and in other cases it is internally fixed.

In many cases, the interaction term is set at -.5, but can also be 0 or +.5

The software documentation should tell you what value is in use.

 

[zgzomb]

Also ensure your Abaqus element type matches the Nastran integration order, it must be equivalent to the CQUAD/CTRIA Nastran Mindlin to get equivalent results.

It's wise to test mesh resolution sensitivity before bouncing between solvers. A too-coarse mesh can result in hourglassing even under your uniaxial load.

The two post processors must also be set and used consistently with regards to nodal averaging for lots of things including failure indices.

Large strain theory should be turned off in Abaqus as well.