Turns out they used a formula from Autodesk Inventor Nastran documentation to answer a question about their equivalent strain.
This is straight from SW manual:
But I’ve also found this interesting explanation from LS-DYNA:
Especially see the last part.
Is that test from some known source. Could you share the reference to do some testing?
INP format please.
A similar test (but with plasticity) is described here: https://us.v-cdn.net/6038102/uploads/attachments/4d977d34dbbac250cfd5f6a4e2961990/equivalent_plastic_vs_tensor_plastic_strain.pdf
Sorry no reference. This is a random model that I calculated using Code Aster and Prepomax for comparison. Except for the von Mises strain, the results are practical identical. The pmx file is attached.
02.pmx (3.1 MB)
Edit
for info, code asters INVa_2 = Prepomax (2/3*Tostrain.Mises) =
=
Input deck exported from this file: 02.inp (167.6 KB)
@Gunnar Thanks
@FEAnalyst Thanks
This two formulas are the same and lead to the same result. Although the compact form in terms of Principal Strains is much clean and fast. Note all those strains are True Strains.
My result:
ESTRN = 0.0714
ANSYS_FORMULA(0_5) = 0.0714
Deviation with ANSYS result is 3%.
This seems to introduce a new definition in which only the plastic Strain is used.
Yeah, it’s more like an alternative to PEEQ - calculated differently, without time integration, so they explain how to distinguish these two measures.
I’ve found a plug-in for Abaqus that uses the SolidWorks formula for equivalent strain: GitHub - costerwi/plugin-equivalent-strain: Abaqus CAE plugin to calculate Solidworks equivalent strain for each frame from the currently displayed odb
This is the result using Gunnar’s model:
Hello FEA,
Referencing ABAQUS in this example could lead to error. If I understood you correctly , ABAQUS standard output for strains in Plasticity are Logarithmic (Hencky,True) strain which allows the direct usage of strain components in the formulas above. Ccx Standard output for Plasticity is Lagrange (Green) Strain and as exposed requires a previous transformation.
Regards
Abaqus provides multiple strain outputs for most cases. The plug-in uses NE (nominal/engineering strain), but of course it could be also modified.
Sorry, but I think you accidentally mixed up both approaches as replacement for Ln in your formula:
If I also remove the multiplier “2x” Tostrain.Prin…, we seem to be very close to Abaqus’ solution (sorry that i missed it, but where comes “2x” Tostrain from?)
I suspect the small discrepancies arise from slightly different results for the calculated strains between Abaqus and Calculix. But to verify this, the exact values from Abaqus are needed.
Hi,
I applied FEA optional formula for LN() . I didn’t undestood yours well.
The sqrt comes from converting Lagrangian to True before operating.
Lagrange Strain in terms of Stretch:
E(Lagrange)=1/2(lambda^2-1) —> Lambda=sqrt(2*E(Lagrange)+1 )
Logarithmic (True) Strain in terms of Stretch :
e(True)=Ln(Lambda )
We substitute Lambda in terms o f E
e(True) =Ln(sqrt(2*E(Lagr ange) +1))
Each Strain component in the equation is transformed as
e(True) =Log(sqrt(2*E(Lagrange)+1),exp (1))
exp(1) =Euler number
By the way, if someone has ever ask himself about the comment on the manual pag 277:
(-0.5 being the smallest possible Lagrange strain) here you have the answer.
The radicand (2*E(Lagrange) +1) would become negative.
Regarding that Plug-in for ABAQUS extracted from Solidworks it doesn’t make sense to me. If it plugs engineering strains into the formula as FEA said , it is because you are supposedly in the elastic regime. (CalculiX also delivers engineering strain in Linear elastic with NLGEOM=OFF). If that’s the case, assuming Poisson Ratio=0.5 (it is implicit in the formula) is not right and the assumptions behind the formula are not fulfilled.
Note ANSYS changes Poisson ratio and “approriate” Strain values (Strain Measure) depending on the material behaviour.
Enginieering Strains + material Poisson ratio for Elastic Regime
Logaritmic + Poisson=0.5 for Plasticity. (The elastic part of a Plastic material analisys is solved using an hiperelastic material in calculix too)
The plug-in is open-source so I can always modify it to use e.g. logarithmic instead of nominal strains. Or change the formula.
Regarding that 3% deviation compared to ANSYS. Note that we start from Lagrangian Strains value at the node —> Compute the equivalent Logarithmic —–> Plug them into the formula. ANSYS and the others are probably converting Lagrange to Logarithmic before,at the integration points, and averaging to the nodes is done later .
Thanks, but my comparison of the Abaqus and prepomax results was incorrect. As already noted, my conversion done in prepomax was:
instead of
Nevertheless, I would still be interested in the Abaqus results, but only the exact values for the one node where ESTRAN=7.275e-2
Sure, more precisely, it’s ESTRN: 0.072747:
Also, logarithmic strain, if needed:
