# Geometrical Nonlinearity in Abaqus

In Abaqus, there is an option NLGEOM to turn on the geometrical nonlinearity. But I'm not clear what it does specifically. Because it also works with UMAT written for small strain formulation, i.e. using infinitesimal strain and return Cauchy stress. For NLGEOM, does it take in Green-Lagrange strain and convert the Cauchy stress to PK2 stress in the internal forces calculation?

• You might find more satisfying answers by asking on the Abaqus-specific forums, rather than here. Sep 12 at 14:26

NLGEOM tells abaqus to use an expression for strain that will equal zero when the body undergoes large rigid body translations or rotations. The exact definition of this strain depends on both the material model and the element type you select. Some material models and element types are suitable only for small-strain (but large rotation) deformations and for these, it is my understanding the the Green-Lagrange strain tensor is used to compute the stress (internal forces) and is also displayed if you select "E" as an output variable.

I have not verified this but it is my understanding that for elements supporting large-strain, essentially the log strain is input to a UMAT and for small-strain elements, Green-Lagrange strains are passed in.

• I have verified by printing the values that for NLGEOM, the input strains (STRAN and DSTRAN) are logarithmic (Hencky) strains. The output is always Cauchy stress as claimed in the theory manual. Therefore, to use a Umat for small displacement for large strain analysis using the Total Lagrangian approach, which at the end uses GL strain and PK2 stress, a conversion procedure is needed. This procedure can be found in Calculix theory manual.
– kstn
Sep 17 at 12:00
• What element type did you use in your tests? I'm curious as to whether element type affects the behavior of the UMAT but don't have a good way to test this myself. As an aside, GL strain and PK2 stress are certainly one way to implement a Lagrangian formulation. But other conjugate stress and strain pairings are equally valid and may be computationally more convenient. Sep 17 at 12:40
• plane strain element, CPE4
– kstn
Sep 17 at 13:06
• Well, CPE4 is a large strain element so what you see in the UMAT is expected. I guess a more relevant question is what kind of material model both requires a UMAT and also where GL strain would be the most useful strain measure? As you say, you can convert to GL strain but why do you need to do this for your particular material model? Sep 17 at 13:23
• I disagree. CPE4 can well be used for small strain analysis. It just provides shape functions and derivatives. The intention is to use the same UMAT for both small strain and large strain analysis. Practically it does not make sense since the value interpretation is very important. Technical-wise, this shouldn't be an isssue.
– kstn
Sep 18 at 7:40