Use with caution: *Elastic with Nonlinear Geometry in Abaqus-What you should know

I’ve seen many Abaqus users attempt to use a linear elastic material model with the nonlinear geometry option. It might be acceptable when the strain is not very large (<5%, according to the SIMULIA QA article). I understand that there are situations where only elastic material parameters are available. However, if you use *Elastic in a geometrically nonlinear analysis, it can lead to the following issues

*Disclaimer: I'm not trying to say that using *Elastic with NLGEOM=Yes option is wrong. It is useful in many cases. But you should know what it means and its limitation.

1) Unphysical Residual Strain

Yes, it sounds strange—how can there be a residual strain if the material is elastic? It can happen numerically. When you use *Elastic with NLGEOM=YES, Abaqus applies an incremental formulation, meaning stress and strain are updated incrementally while considering the material orientation in each time increment.

Let’s assume there is an element where sinusoidal strain-rate loading is applied. If the time increment is relatively large, the integration of the strain rate over one loading cycle may not sum to zero, resulting in a numerical residual stress. You can refer to QA00000008902 and QA00000009383 for more details.

This becomes problematic, for example, when modeling a foldable display. Fig. 2 shows a simplified foldable display using a linear elastic material. After one loading cycle, the residual strain is 0.017—a value that is definitely not negligible.

The residual strain (or stress) issue can also occur in small strain cases. Fig. 3 shows one element test with cyclic shear loading. (Example from Abaqus 2025 documentation-Release notes). You can see that the residual stress increases, and gets worse as the loading cycle increases. Also it gets worse for large time increment case.

2) Severe Element Distortion or Non-Convergence

Fig. 4 shows a cube under tension with a large strain of 300%, using a linear elastic material. The model runs fine up to about 200% strain, but then it becomes unstable and the elements distort severely, ultimately leading to an aborted analysis. Abaqus/Explicit was used for this example, but the phenomenon is similar in Abaqus/Standard (although in Standard, you typically see non-convergence rather than severe distortion).

What causes the issue? As mentioned in the first point, when you use *Elastic with NLGEOM=YES, Abaqus updates stress and strain incrementally, taking into account material orientation in each time step. Although this incremental approach might sound reasonable, there is a critical drawback: it is not necessarily thermodynamically consistent (in terms of energy conservation, entropy, etc.).

A key result in continuum mechanics states that stress must be expressed in a specific form to satisfy the second law of thermodynamics for elastic materials:

where σ is the stress, F is the deformation gradient tensor, θ0 is the reference temperature, J is the Jacobian, and ψ is the Helmholtz free energy (which can be considered internal or strain energy in the isothermal case). As complicated as it looks, it essentially says we need a strain energy potential to ensure thermodynamic consistency. This is why hyperelastic material models are required for large strains.

The approach used with *Elastic and NLGEOM=YES is a type of hypo-elastic model—an incremental method for elastic materials that does not use a strain energy potential. While you can define a hypo-elastic material in Abaqus, the documentation clearly states that it is valid only for small-strain.

The Solution

As discussed, hyperelastic material models are thermodynamically consistent and use a total formulation, where stress is derived directly from the current configuration rather than incrementally. Revisiting the foldable display example, running the same model with a hyperelastic material shows negligible strain remaining after one loading cycle (Fig. 4). Likewise, the cube model runs to completion without element distortion, as shown in Fig. 6.

Usage in Abaqus

Now we know hyperelastic material models solve these issues. But what if you only have elastic properties (Elastic modulus and Poisson’s ratio)? How do we convert these to hyperelastic parameters?

There are two options:

• Hencky Hyperelastic Model (from Abaqus 2024 Hot Fix 2) A new model intended to extend linear elastic properties to large strains using a hyperelastic formulation. You simply provide the elastic modulus and Poisson’s ratio:

*Hyperelastic, HENCKY
<Elastic modulus>, <Poisson ratio>        

• Neo-Hookean Model You can convert elastic parameters to equivalent Neo-Hookean parameters using:

See QA00000009360 for similar conversion formulas for other hyperelastic models.