Specifying stress-strain data for nonlinear materials

You can specify the measure of stress-strain data for nonlinear materials as either engineering or true.

When writing out the solver input file, the software converts the stress-strain data to the format required by the solver for the type of analysis to be performed. When Simcenter Nastran or Simcenter Samcef is the solver, the software additionally takes into account the type of solution and the setting of the Type of Nonlinearity option. The units of Young’s modulus should be consistent with the input stress-strain data.

In the Materials dialog boxes, on the Mechanical page, the Stress-Strain Related Properties group includes the Stress-Strain Input Data Type option, with these available types:

• Engineering Stress-Strain (default)

• Engineering-Plastic Strain

• True Stress-Log Strain

• True Stress-Plastic Strain

• Undefined

When they are migrated from earlier versions of this software, materials that contain stress-strain property data will be set to the Undefined option automatically.

Conversion details

Solver	Solution type	Type of Nonlinearity (TYPE)	Converts to	Corresponding solver syntax
NastranSimcenter 3D Multiphysics	SOL 601,106	NLELASTPLASTIC	There is no conversion. Stress-strain data is written to the input file as specified in the material data.	MATS1, NLELASTMATS1, PLASTIC
PLSTRN	Not supported.A fatal error is reported.	N/A
SOL 106	NLELASTPLASTIC	Engineering Stress-Strain	MATS1, NLELASTMATS1, PLASTIC
PLSTRN	Engineering Stress-StrainTYPE is changed to PLASTIC	MATS1, PLSTRN
SOL 401 (Simcenter Nastran)SOL 402 (Simcenter Nastran)Multi-Step Nonlinear (Multiphysics)	NLELAST	Not supported.A fatal error is reported.	N/A
PLASTIC	Engineering Stress-Strain	MATS1, PLASTIC
PLSTRN	Engineering Stress-Plastic StrainNote: For SOL 402, the conversion is based on the value for the Type of Nonlinearity option.	MATS1, PLSTRN
Abaqus	All	N/A	True Stress-Plastic Strain	*PLASTIC keyword
ANSYS	All	N/A	True Stress-Log Strain	Depends on the Material plasticity model (stress-strain option) that is selected in the Solution dialog box. TB, MELAS (default)TB, MISOTB, KINH
LS-DYNA	All	N/A	True Stress-Plastic Strain	*MAT_PIECEWISE_LINEAR_PLASTICITY keyword (constant temperature only)
Simcenter Samcef	Nonlinear	PLASTIC	Samcef Biot, Cauchy, or Kirchoff laws.See Understanding stress-strain yield stress input for Samcef	.MAT BIOT/CAUCHY/KIRC

For example, if you enter engineering strain for an ANSYS solution, the software performs the conversion from engineering strain to true strain as follows.

Type	Conversion
Engineering strain → log (true) strain
Engineering stress → true stress

where:

• εT = engineering total strain

• εe = engineering elastic strain

• εp = engineering plastic strain

• S = engineering stress

• v = Poisson’s ratio

• σ = true stress

• εl = log (true) strain

• E = Young’s modulus

Setting Stress-Strain Input Data Type to Undefined

When Stress-Strain Input Data Type is set to Undefined, the software writes out the stress-strain data directly as specified in the material data and does not perform a conversion.

Note:

For SOL 402, the solver writes the stress-strain data to the input file with no conversion of measure (except for potential conversion from total strain to plastic strain or vice versa). Therefore, we recommend that you do not use the Undefined option for SOL 402.

When you import SOL 402 input files from releases that did not have the STRMEAS field on the MATS1 bulk entry, the hardening curves are imported as Undefined. In the solver, stress-strain curves without the STRMEAS field on the MATS1 bulk entry, and stress-strain curves with the Undefined option, are considered to be in engineering measure. For large strain analysis, these stress-strain curves are converted to true measure.

Where do I find it?

Application	Pre/Post
Prerequisite	Simcenter Nastran, MSC Nastran, Simcenter 3D Multiphysics, Simcenter Samcef, Abaqus, ANSYS, or LS-DYNA as the selected solver
Command Finder	Manage Materials
Location in dialog box	Create Material →Mechanical page→Stress-Strain Related Properties group

How do I

Define a material with stress-strain data

Model temperature-dependent stress-strain behavior of materials

Quick links

Command reference

Pre/Post video examples

Bulk Entry Descriptions

Simcenter 3D tutorials

Browse Simcenter 3D help by product area

Specifying stress-strain data for nonlinear materials, Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });