Tools › Structures › Materials › FEA Stress-Strain Input

FEA Stress-Strain Input

Turns handbook material properties (E, Ec, ν, Ftu, Fty, Fcy, the Ramberg-Osgood exponents nt and nc and the elongation) into the nonlinear material input of the finite-element packages: a multi-point stress-strain table in the measure each one expects (engineering or true stress, total or plastic strain), a bilinear yield and tangent-modulus pair, or the Ramberg-Osgood parameters. Nastran (MSC, Simcenter, Femap, Inventor Nastran, OptiStruct), Ansys Mechanical APDL and Workbench, Abaqus and CalculiX, LS-DYNA, Radioss, SolidWorks Simulation, COMSOL and Code_Aster are covered. Enter the properties or load a saved MIL-HDBK-5J material; when the package takes one curve for tension and compression the two are averaged. The result is the card text ready to download or copy, the point table in every measure, and a chart of the engineering, true and FEA curves overlaid.

  • Ramberg-Osgood curve from E, Fty, n and the ultimate point; n fitted through the ultimate point when not entered

  • Each package's own input: total or plastic strain, engineering or true measure, bilinear or multi-point, with the first-point and extrapolation rules it applies

  • Tension and compression averaged where the package takes one curve; written as two branches for Nastran NLELAST

  • Nastran MATS1 / MATEP / TABLES1, Ansys TB,BISO / BKIN / PLASTIC, Workbench tables, Abaqus *PLASTIC and *DEFORMATION PLASTICITY, LS-DYNA MAT_003 / MAT_024, Radioss LAW36, SolidWorks, COMSOL, Code_Aster, CSV

  • Download or copy the file; chart of the engineering, true and FEA curves

FEA Stress-Strain Input

Unit System: /

Material Properties (optional fields may be blank: Ec = E, nc = nt, nt fitted, no density)

Sign in












Output









What each FEA package expects, and how the curve is built | Method page
×

What Each Package Expects

FEA Stress-Strain Input: What Each Package Expects, and How the Curve Is Built

Purpose

A handbook gives a material as a few numbers: the moduli E and Ec, Poisson's ratio ν, the strengths Ftu, Fty and Fcy, the Ramberg-Osgood exponents nt and nc and the elongation e. A finite-element program wants the whole stress-strain curve, and every program wants it in its own form: a table against total strain or against plastic strain, in engineering or in true (logarithmic) measure, a yield stress with a tangent modulus, or the Ramberg-Osgood parameters in its own notation. Getting the form wrong is the commonest error in a nonlinear material definition: a total-strain table read as plastic strain, an engineering curve in a large-strain run, a first point that is not at yield. This tool builds the curve once and writes it the way the chosen package reads it.

What Each Package Expects

The rules below were read from the vendors' reference pages (saved with the tool's sources). Every elastic-plastic model in this list is a von Mises plasticity with a single curve for tension and compression; only Nastran's NLELAST takes two branches.

Package and optionStrain columnStress and strain measureFirst pointBeyond the last point
Nastran MATS1 PLASTIC + TABLES1, TYPSTRN 0 (MSC SOL 106 and 400, Simcenter, Femap, Inventor Nastran, OptiStruct)total strainengineering in a small-strain run; true stress and logarithmic strain with PARAM,LGDISP(0, 0), then the initial yield LIMIT1 at LIMIT1/E: the first segment's slope must equal E of MAT1linear with the last slope
Nastran MATS1 PLASTIC + TABLES1, TYPSTRN 1 (Simcenter SOL 401, 402, 601; OptiStruct)plastic straintrue for a large-strain runyield stress at zero plastic strainlinear with the last slope
Nastran MATS1 bilinear (LIMIT1, H)—eitherLIMIT1 is the yield; H is the work-hardening slope, stress against plastic strain, H = E Et/(E − Et)—
Nastran MATS1 NLELAST + TABLES1total strain, both quadrantsengineering (small strain)the table passes through the origin; compression branch at negative strainlinear with the last slope
MSC Nastran SOL 400 MATEP + TABLES1 (TYPE 2)plastic straintrue stress, logarithmic strainyield at zero plastic strainlinear with the last slope
Ansys TB,BISO and TB,BKIN—true with NLGEOM,ONC1 yield stress, C2 tangent modulus of the stress–total-strain line—
Ansys TB,PLASTIC,,,,MISO and KINHplastic straintrue with NLGEOM,ONyield at zero plastic strain; every segment slope between 0 and Econstant (perfectly plastic)
Ansys TB,MISO (archived command)total straintrue with NLGEOM,ONthe yield point at strain yield/EX, so its slope is EX; the origin itself is not enteredconstant
Ansys Workbench, Multilinear Isotropic or Kinematic Hardeningplastic straintrue with Large Deflection onzero plastic strain at the yield stressconstant
Ansys Workbench, Bilinear Isotropic or Kinematic Hardening—true with Large Deflection onYield Strength and Tangent Modulus of the total-strain line—
Abaqus *PLASTIC (also CalculiX and PrePoMax)logarithmic plastic straintrue stressthe first row's plastic strain must be zeroconstant
Abaqus *DEFORMATION PLASTICITY——E, ν, σ0, n, α with Eε = σ + α (|σ|/σ0)n−1 σ—
LS-DYNA *MAT_024 with LCSSeffective plastic straineffective (true) stressyield at zero plastic strain; SIGY and ETAN are ignored when LCSS is givenlinear with the last slope
LS-DYNA *MAT_024 and *MAT_003 bilinear—trueSIGY and ETAN, the tangent modulus of the true stress–true strain line (plastic modulus E ETAN/(E − ETAN))—
Radioss /MAT/LAW36plastic straintruethe first point of each yield function at zero plastic strainlinear with the last slope
SolidWorks Simulation, plasticity von Mises curvetotal strainengineering (small strain) or Cauchy stress and logarithmic strain (Large strain option)the yield pointlinear through the last two points
SolidWorks bilinear—eitherSIGYLD and ETAN (the solver refuses ETAN above E or below about E/100); RK = 1 isotropic, 0 kinematic—
COMSOL Plasticity, hardening functionequivalent plastic strainlogarithmic with large plastic strainσh(εpe) = σys − σys0 must be zero at zero plastic strainthe interpolation function's extrapolation setting
COMSOL linear isotropic hardening—eitherσys0 and ETiso, the tangent modulus of the total-strain line—
Code_Aster VMIS_ISOT_TRACtotal strainengineering (PETIT) or logarithmic (GDEF_LOG)the yield stress at strain σy/E, slope E; later slopes lowerPROL_DROITE (LINEAIRE written)
Code_Aster VMIS_ISOT_LINE—eitherSY and D_SIGM_EPSI, the tangent modulus—

Two distinctions run through the table. Total or plastic strain: a plastic-strain table is not the total-strain table shifted sideways; the plastic strain of every point is its total strain minus its own elastic strain σ/E, which grows along the curve. Engineering or true: a small-strain solution (Nastran SOL 106 without LGDISP, Ansys without NLGEOM, SolidWorks small strain, Code_Aster PETIT) takes the engineering curve as tested; a large-strain solution works in Cauchy (true) stress and logarithmic strain and must be given the curve converted. Abaqus, LS-DYNA, Radioss and MATEP take true values only.

The Source Curve

The curve is Ramberg and Osgood's three-parameter relation with the 0.2 % offset yield, the form MIL-HDBK-5 uses: ε = σ/E + 0.002 (σ/Fy)n. It is engineering stress against engineering strain, valid to the ultimate stress; the elongation e is the engineering strain at the ultimate point and ends the curve. When no exponent is entered, n is fitted so that the curve passes through the ultimate point, n = ln[(e − Ftu/E)/0.002] / ln(Ftu/Fty), the construction Cozzone used for his shape factor. A handbook n usually gives a plastic strain at Ftu smaller than the elongation (the specimen necks after the uniform elongation), in which case the curve reaches Ftu first and the tool adds a flat (perfectly plastic) point at the elongation, or ends at Ftu when the Curve End input says so. When the handbook n is small enough that the curve reaches the elongation below Ftu, the table ends at the elongation and the page says so.

Tension and compression. Von Mises plasticity has one yield surface: the program cannot take a tension curve and a compression curve. When a compression yield is entered the tool averages the two sets, Eb = (E + Ec)/2, Fyb = (Fty + Fcy)/2, nb = (nt + nc)/2, and writes the Ramberg-Osgood curve of the averaged properties; the ultimate point stays the tensile one, since compression has no ultimate. The Curve Basis input can force the tension or the compression curve instead. Figure 1 draws the three curves so the compromise is visible. Nastran's NLELAST, a nonlinear elastic law that unloads along the loading curve, takes the table in both quadrants and is written with the compression branch from the compression properties and the tension branch from the tension properties, no averaging; the generic CSV lists both curves.

Building the Table

Initial yield. A Ramberg-Osgood curve has no sharp yield; the plastic strain is small but not zero at every stress. Every package needs a first point with zero plastic strain, and a Nastran total-strain table needs its first segment to have the slope E exactly. The tool takes the initial yield σ0 as the stress at a plastic strain εp0 = 0.01 % (the usual proportional-limit definition, adjustable), treats the material as linear below it and drops that offset from the plastic strains above it: εpl = 0.002 (σ/Fy)n − εp0, total strain σ/E + εpl. The table then starts at (σ0/E, σ0) with zero plastic strain and differs from the exact curve by 0.01 % strain. Starting the table at the 0.2 % offset yield instead, as is sometimes done, drops the knee of the curve between 0.01 % and 0.2 % plastic strain and overstates the stiffness there.

Point spacing. The plastic strains of the points are spaced geometrically from εp0 to the plastic strain at the end of the curve, so the points are dense around the knee, where a piecewise-linear interpolation would otherwise cut the corner, and sparse along the nearly straight hardening part. Twenty points keep the interpolated curve within a fraction of a percent of the Ramberg-Osgood curve in stress; Ansys accepts up to a hundred per temperature.

True values. Up to the ultimate point the deformation is uniform and the conversions are exact: σtrue = σ (1 + ε) and εtrue = ln(1 + ε). A large-strain program decomposes the logarithmic strain as σtrue/E + εpl,true, so the plastic strain written is εpl,true = ln(1 + ε) − σtrue/E. Near yield that expression is slightly negative, by about 1.5 (σ/E)2, because ln(1 + ε) falls below ε while σ(1 + ε)/E rises above σ/E; the value at the first point (under 0.01 % strain) is subtracted from every point so the first has zero plastic strain and the sequence never decreases, and the true total strain of the table is rebuilt as σtrue/E + εpl,true so that the two columns agree with the program's own decomposition.

Bilinear. The yield is the 0.2 % offset yield Fyb at the strain Fyb/Eb; the tangent line runs from there to the ultimate point, (e, Ftu) in engineering measure or (ln(1 + e), Ftu(1 + e)) in true measure, unless a tangent modulus is entered. Programs differ in which slope they call the hardening input: Ansys, LS-DYNA, SolidWorks, COMSOL and Code_Aster take the tangent modulus Et of the stress–total-strain line; Nastran's H is the plastic modulus, the slope of stress against plastic strain, H = E Et/(E − Et), and the two agree only when Et is much smaller than E. Abaqus has no bilinear keyword; two *PLASTIC rows, the yield at zero plastic strain and the ultimate at its plastic strain, do the same.

Ramberg-Osgood parameters. Abaqus's deformation plasticity writes the same curve as Eε = σ + α (|σ|/σ0)n−1 σ. With σ0 = Fyb the yield offset is α = 0.002 Eb/Fyb, because 0.002 E (σ/Fy)n = [0.002 E/Fy] (σ/Fy)n−1 σ. It is a total-strain (deformation) theory meant for monotonic loading in fracture-mechanics problems and does not unload elastically.

Units

A finite-element model has no units of its own: the stress, length, force and time units must be consistent, and the density goes in as mass per volume in the same system. The Output Units input selects the set: psi with inches, lbf and seconds (density in lbf·s2/in4, the weight density in lb/in3 divided by g = 386.09 in/s2); ksi with inches and kips; MPa with millimetres, newtons and tonnes (density in t/mm3, the kg/m3 value times 10−12); or Pa with metres, newtons and kilograms. The file header records the choice.

Limits

The curve is monotonic and rate-independent, at the temperature of the entered properties (a saved material brings its temperature-adjusted values). Nothing is written beyond the ultimate point: the post-necking part of a true stress–strain curve, which a crash or forming model needs, must come from a test with a necking correction (Bridgman) or from an extrapolation law (Swift, Voce, Hockett-Sherby), not from handbook allowables. Kinematic and mixed hardening options are written with the same curve; the hardening rule itself is a modelling choice for reversed loading. Strain-rate, temperature-dependent and anisotropic (Hill) definitions are not produced.



References

Ramberg, W., and Osgood, W. R. (1943). Description of Stress-Strain Curves by Three Parameters. NACA Technical Note 902, National Bureau of Standards, Washington, D.C.

U.S. Department of Defense (2003). Metallic Materials and Elements for Aerospace Vehicle Structures. MIL-HDBK-5J, 31 January 2003.

Hill, H. N. (1944). Determination of Stress-Strain Relations from "Offset" Yield Strength Values. NACA Technical Note 927, Aluminum Company of America, New Kensington, PA.

Dowling, N. E. (2013). Mechanical Behavior of Materials: Engineering Methods for Deformation, Fracture, and Fatigue, 4th ed. Pearson, Boston.

MSC Software (2021). MSC Nastran Quick Reference Guide. MSC Software Corporation, Newport Beach, CA.

Siemens Digital Industries Software (2022). Simcenter Nastran Quick Reference Guide. Siemens, Plano, TX.

Altair Engineering (2024). OptiStruct Reference Guide: MATS1 Bulk Data Entry. Altair Engineering, Troy, MI.

Altair Engineering (2024). Radioss Reference Guide: /MAT/LAW36 (PLAS_TAB). Altair Engineering, Troy, MI.

Autodesk (2022). Inventor Nastran Reference: MATS1 (Material Stress Dependence). Autodesk, San Rafael, CA.

Ansys, Inc. (2024). Mechanical APDL Material Reference: Rate-Independent Plasticity. Ansys, Inc., Canonsburg, PA.

Dassault Systèmes (2017). Abaqus Keywords Reference Guide: *PLASTIC and *DEFORMATION PLASTICITY. Dassault Systèmes Simulia Corp., Providence, RI.

Dhondt, G. (2023). CalculiX CrunchiX User's Manual, Version 2.21. Munich.

Livermore Software Technology (2024). LS-DYNA Keyword User's Manual, Volume II: Material Models. Ansys, Inc., Livermore, CA.

Dassault Systèmes SolidWorks (2021). SOLIDWORKS Simulation Help: Defining Stress-Strain Curves; Plasticity von Mises Model. Dassault Systèmes SolidWorks Corp., Waltham, MA.

COMSOL (2022). Structural Mechanics Module User's Guide, Version 6.1: Plasticity. COMSOL AB, Stockholm.

Électricité de France (2023). Code_Aster Reference Manual R5.03.02: Elastoplastic Behaviour Laws of von Mises with Isotropic Hardening. EDF R&D, Paris.

DISCLAIMER: The methods and calculation on aNOWysis.com are provided as means to educate the reader. There is no warranty, expessed or implied, as to the relevance or accuracy of the methods or calculations. All calculations should be checked by a qualified analyst for appropriateness and accuracy. We will not be held liable for any damages, injuries or deaths caused by using methods or calculations from this site.