To my shame, I didn’t pay much attention to this value before, but I’ve noticed that the result of the von Mises equivalent strain is relatively large compared to the other principal strain values and doesn’t match the result from the formula below: this should yield 2.30E-4 for the selected node, but as you can see, prepomax/ccx reports 3.45E-4 (it is a simple rod subjected to tensile stress).
Ansys 2.65E-4 (btw, very close to Prin_Max in ccx)
SolidWorks 2.30E-4
Diana 2.35E-4
Code Aster 2.30E-4
Prepomax 3.45E-4
Dlubal RFEM 2.65E-4
I would find it less surprising if the equivalent Mises strain were of a similar order of magnitude to the dominant principal strain - just as the equivalent stress of a tensile specimen relates to the principal normal stress.
But as I’ve now learned, there is no right or wrong answer here. However, for comparability reasons, I would also prefer a similar order of magnitude for Prepomax. Especially when switching to open source, comparability is a major topic.
*Note: of course, all results are calculated using the stress components from Calculix!
@FEAnalyst I have also checked in different versions of the Ansys theory manuals and agree with you so the formula you posted must be the correct one and the formula in the Ansys PowerPoint must be wrong.
@Gunnar I can’t really imagine how both formulas should be identical because extracting the divisor from the fraction in the square root will leave the 6 factor for the shear strain compared to APDL formula where the shear strain factor is 3/2.
If I compress a cube with a uniaxial strain state (only one strain component is different from 0), I would expect the equivalent strain value to be = the unique component different from zero = unique Principal Strain different from zero.
The only formula that fullfill that when you cancel all the components except 1 is the ANSYS formula.
I have done it compressing 0.1 mm single element cube of 1mmx1mmx1mm and zero poisson ratio with nonlinear analisys (Lagrange Strain)
Result is ezz = -0.095, Principal Strain e3= -0.095 and ANSYS formula is 0.095 all consistent.
Yeah, strain measures in CalculiX differ depending on the material model:
As basic measure of strain in CalculiX the Lagrangian strain tensor E is used for elastic
media, the deviatoric elastic left Cauchy-Green tensor for incremental plasticity, the logarithmic (or Hencky) strain for some other plasticity models as deformation plasticity and Johnson-Cook hardening and linear strains where appropriate, i.e. for small deformations combined with small rotations.
E [TOSTRAIN (real),TOSTRAII (imaginary)]: strain. This is the total Lagrangian strain for (hyper)elastic materials and incremental plasticity and the total Eulerian strain for deformation plasticity.
To clarify, deformation plasticity is the Ramberg-Osgood model (*DEFORMATION PLASTICITY) while incremental plasticity is the regular plasticity model (*PLASTIC), but it can use either multiplicative decomposition (if Nlgeom is enabled) or additive decomposition (if Nlgeom is disabled).
One important thing I repeat to myself when talking about Strains (Although I tend to forget it) is first, be sure to know which measure the book or author is using.
Note the difference in the shear component letter in the formulas:
I guess the main difference in the implementations is whether they use Poisson’s ratio or not then. Quite often this output is not available at all (only equivalent plastic strain is provided) and has to be computed from the existing outputs (using custom maps or plots) or the user needs to check e.g. max principal stress instead.
FLAC3D uses:
where e_ij is the deviatoric part of the strain tensor.
I need to fix something in my previous comment. I’m not ANSYS user and I got confused. Need to go deeper to see why there is such an agreement between the formula and principal Strain.
This is from AI after many refinement request for clarification:
In ANSYS, when one enable Large Deflection (NLGEOM, ON), there is a clear distinction between the internal computation and the reported output:
Internal Computation: The solver uses formulations based on the Green-Lagrange strain tensor (or Almansi strain measures) to solve the equilibrium equations and handle large rotations and displacements.
Reported Results (Output): By default, the post-processor converts those internal values and displays Logarithmic Strains (True Strains) for the von Mises equivalent strain.
Therefore, the ANSYS formula assumes Logarithmic (True) strains because that is the specific value you will see plotted on your screen in ANSYS when you request an “Equivalent Strain” result.
That can also be an additional source of discrepancy between the formulas. If I use the ANSYS formula pluging the Calculix Strains it shouldn’t work. Calculix reported strains in Nonlinear are Lagrangian not logarithmic.
but I don’t understand the equality between the Ansys formulation and the last 2 formula which you have posted, so I will ask if could come up with a little clue which could help my understanding
I don’t use ANSYS either so I can only check its docs:
For elements which have large strain capability, stresses (output as S) are true (Cauchy) stresses in the rotated element coordinate system (the element coordinate system follows the material as it rotates). Strains (output as EPEL, EPPL, etc.) are the logarithmic or Hencky strains, also in the rotated element coordinate system.
In Abaqus, the following strain measures are used in these special cases:
analyses without Nlgeom - infinitesimal strain measure
analyses with Nlgeom and finite strain elements - logarithmic strain by default, E is not available
small-strain shells and beams in Abaqus/Standard - Green’s strain (variable E) by default
hyperelastic materials - logarithmic strain
Otherwise, the strain measure can be selected in most cases:
By default, the strain output in Abaqus/Standard is the “integrated” total strain (output variable E). For large-strain shells, membranes, and solid elements in Abaqus/Standard two other measures of total strain can be requested: logarithmic strain (output variable LE) and nominal strain (output variable NE).
Logarithmic strain (output variable LE) is the default strain output in Abaqus/Explicit; nominal strain (output variable NE) can be requested as well. The “integrated” total strain is not available in Abaqus/Explicit.
