Truss and Beam element axial loading - stress difference

[MOZER8]

Hello All,

I have a problem. I made a very simple simulation to test the 1D element performances. One has been built with beam elements, other has been built with truss elements. All other properties are the same. Both are under tensile loading, nlgeam is on since the material is nonlinear. (Cross-sections are also same - for beam 3mmx30mm rectangle, for truss 90mm^2 cross-section was defined.) However stress results are different. After I checked the results, hand calculation is supporting the beam element results. Am I missing something in truss elements? You can check the model and see the results. Normally, I would expect are 34MPa from both elements. Thank you for your help.

 

[FEA way]

For linear elastic material stresses are the same. This indicates that there’s a difference in performance of truss and beam elements when hyperelastic material is used and strains are large. In the documentation about truss elements it says that for large strain analyses cross-sectional area of truss is updated assuming incompressible material regardless of its actual definition.

 

[MOZER8]

That explains it. Is it possible to turn off cross-section update during the analysis. Because I have force - strain data, and I converted it into stress-strain assuming the cross-section is constant during the analysis.

 

[FEA way]

No, unless you turn NLGEOM off. Cross-section update is standard procedure in analyses of 1D elements with geometric nonlinearity.

 

[MOZER8]

I had another idea: I set the poisson's ratio to zero in order to prevent cross-section shrinkage? However results are still not logical. Any idea?

 

[FEA way]

If you want to keep NLGEOM on and hyperelastic material then try lowering applied force. With smaller load strains will be lower and the effect of this cross-section update should reduce.

 

[MOZER8]

This one is just a dummy model to test element behavior. I won't be able to lower the force since the force is applied from a accelerated mass (you can check my previous post about ball catch analysis with a net). Beside from that, since the material is nonlinear, lowering force will not give linearly proportional results.

What I want to understand is: How does abaqus calculates cross-section change? Does poisson's ratio play a role in this calculation? If it does would that be possible to minimize this effect?

 

[FEA way]

When strains are large Abaqus uses simplified formulation for truss elements assuming that they are made of incompressible material (Poisson’s ratio of 0.5 and thus no change in volume). You can find this formulation in the Theory Guide chapter „Truss elements” (topic „Virtual work contribution”). So basically when the truss elements extends its cross-section is updated in such way that the volume is the same as before extention.

 

[MOZER8]

FEA way, thank you for your reply. I missed the part about truss element that their cross-sections are calculated with the assumption of they are incompressible.

 

[MOZER8]

I found the solution in updating the stress-strain table in hyperelastic material properties. By doing so, stress values will neglect the cross-section updating effect. It require some hand calculations which can be achieved by excel easly.