Finite Element Modeling of Deformation Behavior of Steel Specimens under 

Various Loading Scenarios

Dilip Banerjee1,a*, Mark Iadicola1,b, Adam Creuziger1,c, and Timothy Foecke1,d

1Material Measurement Laboratory, NIST, 100 Bureau Dr, Gaithersburg, MD 20899, USA

aDilip.Banerjee@nist.gov, bMark.Iadicola@nist.gov, aAdam.Creuziger@nist.gov,

aTimothy.Foecke@nist.gov

Keywords: uniaxial and biaxial tensile tests, finite element modeling, steel, cruciform

Abstract. Lightweighting materials (e.g., advanced high strength steels, aluminum alloys etc.) are 

increasingly being used by automotive companies as sheet metal components. However, accurate 

material models are needed for wider adoption. These constitutive material data are often developed 

by applying biaxial strain paths with cross-shaped (cruciform) specimens. Optimizing the design of 

specimens is a major goal in which finite element (FE) analysis can play a major role. However, 

verification of FE models is necessary. Calibrating models against uniaxial tensile tests is a logical 

first step. In the present study, reliable stress-strain data up to failure are developed by using digital 

image correlation (DIC) technique for strain measurement and X-ray techniques and/or force data 

for stress measurement. Such data are used to model the deformation behavior in uniaxial and 

biaxial tensile specimens. Model predictions of strains and displacements are compared with 

experimental data. The role of imperfections on necking behavior in FE modeling results of uniaxial 

tests is discussed. Computed results of deformation, strain profile, and von Mises plastic strain agree 

with measured values along critical paths in the cruciform specimens. Such a calibrated FE model 

can be used to obtain an optimum cruciform specimen design.

1. Introduction

Automotive companies are actively interested in the increased use of advanced lightweighting 

materials such as advanced high strength steels (AHSS), aluminum alloys etc. as sheet metal 

components. However, accurate material models are needed before these materials can be widely 

used. These material models are often developed using linear strain paths using cross-shaped biaxial 

specimens (i.e., cruciform) [1, 2, 3]. But successful cruciform mechanical testing is dependent on 

the specimen design itself. In the past, a wide variety of designs have been used [4, 5, 6, 7]. The 

specimen design should meet certain goals: (a) Both strain uniformity and eventual failure in the 

biaxially loaded gauge area, (b) reduction of stress concentration outside of the gauge area, (c) 

minimization of shear strains in the gauge area, and (d) similar behavior during repeat tests. A 

prudent approach for obtaining optimum specimen design is to combine FE simulation with 

optimization software such that the above objectives are achieved. But the first step is to calibrate 

the FE model against precise experimental measurements. These measurements were obtained using 

the state of the art mechanical testing facility at the National Institute of Standards and Technology 

(NIST) Center for Automotive Lightweighting (NCAL) [8]. In this paper, the verification of FE 

models against experimental measurements is discussed for both uniaxial and biaxial tensile tests. 

Additionally, plastic deformation behavior in the specimens is discussed. Note that uncertainties 

associated with the measurement of displacement and strain are reported in ref [9].

2. Uniaxial Tensile Tests

2.1 Uniaxial Tensile Test Experiments. Uniaxial test specimens were made of two different steels: 

(a) 9.525 mm (0.375 in) thick hot-rolled low carbon steel (hereinafter called “thick specimen”) and 

(b) 3.038 mm (0.1196 in) thick cold-rolled AISI 1008 steel (hereinafter called “thin specimen”). 

This thin specimen steel has much lower yield and ultimate tensile strength than the thick specimen
steel. Uniaxial tests were conducted both to verify the FE model and to generate stress-strain data 

for uniaxial and biaxial tensile tests. Uniaxial tensile tests were performed for both steels in the 

rolling direction of the sheet. These tests were performed using the X-axis of the cruciform 

machine and the DIC system [8]. The gauge section as designed has a nominally parallel length of 

101.6 mm and width of 19.05 mm with radii of 50.8 mm to the 28.58 mm wide end-tabs. The same 

planar geometry was used for both thicknesses of material. Since the biaxial test and model will 

achieve strains beyond the uniform strain of a 

standard tensile test, it was necessary to 

approximate the true-stress/true-strain 

relationship at strains beyond uniform 

deformation. The true axial strain was 

calculated as the average strain across the 

width for each point in time in the axial 

direction at the eventual location of failure. 

The true stress was calculated as the applied 

force divided by the current cross-sectional 

area at the same location and time. The 

resulting stress strain curves are shown in 

Fig. 1. The uniaxial test for the thin material 

used a constant displacement rate, which resulted in an undesirable increase in strain rate from 

approximately 8x10-5s

-1

before initial localization (maximum force) to 2x10-3s

-1

as the sample 

approached failure. In the thick material uniaxial test the displacement rate was reduced twice 

during the test (at approximately 0.26 and 0.49 true strain) to keep the average strain rate 

near 9x10-4s

-1

. Following the tensile tests, history-dependent axial displacement values at locations 

in the end-tabs approximately 82 mm away from the central point were extracted for subsequent use 

in the FE simulation as boundary conditions (BC). The displacement values were interpolated from 

the DIC field data at the FE nodal coordinate values nearest to X=±82 mm along the axial direction. 

The force-displacement curve for the thick specimen is shown in Fig. 2. Displacement and 

strain data corresponding to the four loading points (A, B, C, and D) in Fig. 2 were extracted for 

comparison with FE results. Such axial 

displacement vs. x-coordinate data as measured 

by the DIC system were output along three 

specimen lines (i.e., along centerline, along 

lines ± 4.63 mm away from centerline) in the 

axial direction. Only centerline data are used in 

this study.

2.2 FE Simulation of Uniaxial Tensile Tests. 

A 3D finite element model of the thick uniaxial 

specimen was developed using ABAQUS1

software [10]. Constitutive material model data 

were obtained from experimental stress-strain 

 

1

Certain commercial software or materials are identified to describe a procedure or concept adequately. Such 

identification is not intended to imply recommendation, endorsement, or implication by NIST that the software or 

materials are necessarily the best available for the purpose.

Fig. 1. True stress – true strain data obtained in 

uniaxial tensile tests.

0

100

200

300

400

500

600

700

800

900

0 0.5 1 1.5

True stress, MPa

True strain

9.525 mm (0.375 in) (thick) specimen

3.175 mm (0.125 in) (thin) specimen

0

20

40

60

80

100

0 10 20 30

Force, kN

Displacement, mm

Comparison points

Fig. 2. Force-displacement curves for the thick 

specimen. 

A B C

D

a

b
data in uniaxial tension tests (Fig. 1). Isotropic hardening is assumed in this study. Young’s 

modulus of 210 GPa and Poisson ratio of 0.3 were assumed for both materials. A 1/2 symmetry FE 

model was developed by taking advantage of the mirror 

symmetry in the specimen shape and loading. The solid 

model was developed using mapped meshing, and 3D linear 

hexahedral elements (C3D8R) were used. Fig. 3 shows a 

typical FE mesh. In order to introduce instability in the 

simulation, geometric imperfections were introduced. This 

was accomplished by physically displacing nodes at the 

edge by a small fraction of the grid spacing (see Fig. 3).

Note that all the nodes through the depth at this edge

location were displaced by the same amount. This is similar 

to the concept of creating a notch to initiate instability. 

ABAQUS simulations showed that the ultimate failure 

occurred near the vicinity of this imperfection but not at the 

exact point of imperfection. Experiments on the thick 

specimens showed the formation of Lüders bands (typically 

encountered in low carbon steels). The eventual necking and failure occurred near the locations 

where Lüders bands initiated. Therefore, it was necessary to capture this behavior in the FE 

simulation by introducing imperfections near the regions where the Lüders bands were seen.

Figure 4 shows both the measured and computed axial displacements along the centerline of the 

specimen for points corresponding D in Fig. 2. Good agreement was seen except for the point near 

the necking region. This is because there is a slight difference between the model predicted location

of necking and that obtained in the experiment. Additionally, the model seems to predict a sharper 

localization than that seen in the experimental results. Figure 5 shows the comparison between the 

measured von Mises equivalent strain and computed von Mises plastic strain plots. Again, the 

agreement is good in terms of the overall shape and maximum values. However, ABAQUS values 

slightly under-predict the strains away from the maximum localization point. This is 

understandable, as ABAQUS plots do not include the elastic component of the strain (which is quite 

small compared to the plastic component of the strain). Figure 6 shows measured and computed 

contour plots of von Mises equivalent strain on the surface of the specimen. The overall strain 

profile along the specimen length as computed by ABAQUS agrees well with measured values.

Node 

shift

-0.2

0

0.2

0.4

0.6

0.8

1

1.2

1.4

-100 -50 0 50 100 von Mises equivalent strain

Distance along specimen length, mm

Experiment

ABAQUS

-15

-10

-5

0

5

10

15

-100 -50 0 50 100 Longitudinal displacement, mm

Distance along specimen length, mm

Centerline (D)

Experiment

ABAQUS

Fig. 4. Measured and computed longitudinal 

displacements along the specimen length 

corresponding to the point D in Fig. 2.

Fig. 5. von Mises equivalent strain and ABAQUS 

computed von Mises plastic strain along the 

specimen length corresponding to point D in Fig. 2.

Fig. 3. Finite element mesh and a 

schematic showing node shift used 

to introduce instability in FE 

simulation.
3. Biaxial Tensile Tests

3.1 Cruciform Specimen Design. Cruciform geometries for in-plane biaxial tests are advantageous 

because (a) the region of interest is far away from locations where BCs are applied and (b) varying 

strain ratios can be applied along the arms of the specimen. In most of the specimen designs, failure 

occurred outside the central gauge section of interest and at strains well below traditional forming 

limit strains, due to a combination of various factors such as stress and deformation concentrations 

at corners or near slits in the arms [11]. In some designs, the central gauge section is thinned down 

to achieve higher strain and possibly failure in the middle of the gauge section. In this study, the 

specimen design follows that of ref. [7], with the initial specimen being enlarged in all three 

directions to a thickness of 0.953 mm. The present specimen design for the thick specimen is 

described in ref [9]. Cruciform samples were machined by water-jet with the X-axis aligned with 

the rolling direction of the sheet. A similar geometry was used for the thin specimen, except that it 

had a designed thickness of 0.749 mm (0.0295 in) in the thinned down region in the center and that 

the fillet radius at the peripheral region of the central pocket was 0.397 mm (0.016 in). 

3.2 Biaxial Tensile Tests. Biaxial loading was applied using four hydraulic actuators, which are 

controlled in orthogonal pairs [11]. Each of these actuators has 500 kN load capacity and has a ±50 

mm displacement range from a reference distance of 640 mm between grip faces on the X or Y-axis. 

Details of the loading and in situ DIC data acquisition are described in [11]. In the present study, the 

biaxial tests were conducted using displacement control. Fig. 7 shows force-displacement curves. 

The 3D displacement of top surface about the center of the cruciform specimen was measured with 

a stereo DIC system. Surface strains are calculated from the measured displacement fields. 

Measured, history-dependent average U and V values at locations approximately 25 mm away from 

the central point were extracted for subsequent use in FE simulation (see Fig. 8). Since cruciform

specimens tend to concentrate strain in the corners between the arms leading to premature failure, it 

is important for FE model to be able to capture the mechanical behavior in these corners. 

Accordingly, measured displacement and strain data were extracted along a diagonal line that 

bisects the region between the central pocket and the reentrant radius at the meeting point of the X 

and Y arms (see "Path" in Fig. 8). These data are compared to FE data corresponding to loading 

points shown in Fig. 7. Results are shown here for only the maximum force point in Fig. 7.

3.3 FE Modeling. A 3D FE model of the cruciform specimens was developed using ABAQUS 

software [10]. See section 2.2 for details on material data. A 1/8th symmetry model was developed 

DIC Measurements

ABAQUS computed plot

Fig. 6. Contour plots of measured von Mises equivalent strain and ABAQUS computed 

von Mises plastic strain along the specimen length corresponding to point D in Fig. 2.
by using the mirror symmetry in the specimen shape and loading. FE model included both regular

(C3D8) and reduced integration brick (C3D8R) elements. In addition to symmetry conditions, axial 

displacement boundary conditions were applied on each arm (Fig. 8). Simulated results were 

extracted for all points labeled in Fig. 7 along the path shown in Fig. 8 and compared with DIC data. 

Only data corresponding to the maximum force point are discussed below for the thin specimen. 

3.4 Results and Discussion. Fig. 9 shows both 

experimental and computed U displacement fields. There 

are four equivalent paths for which experimental data 

have been measured. However, because of the symmetry 

used in the model, only one plot is available for the FE

model. Two sets of ABAQUS results are shown (one 

each for C3D8R and C3D8 element). Fig. 9 shows that 

the model predicts the displacement field correctly. Fig. 

10 shows plots of normal strains in the Z direction. The 

measured thickness strains were calculated assuming 

volume conservation, using ezz = -(exx+eyy). ABAQUS 

simulations with C3D8 elements are in better agreement 

with experimental results. However, the modeled peak 

ezz for C3D8 element exceeds those seen in experimental data. It is also noticed that the model 

predicts a slightly narrower width of the ezz profile than that in the experimental results. The 

measured von Mises equivalent strain plot is shown in Fig. 11. This plot is compared with the von 

Mises equivalent plastic strain (PEEQ) in ABAQUS. This comparison is justified since elastic strain

is very small. Fig. 11 shows the largest value at the reentrant radius of about 0.38 and around 0.084 

in the central region. Uniform equivalent strain is seen in the central pocket, which is also seen in 

the ABAQUS results in Fig. 12. The ABAQUS results show a value of 0.16 in the central pocket 

and a value of 0.3 at the outer edge of the reentrant corner. The model shows a slight decrease in 

strain along the diagonal from the reentrant radius to the peripheral region of the central pocket, 

where a value of about of 0.24 is obtained. Although the model does not show as thick a band of 

PEEQ of 0.3 along the diagonal from the reentrant radius to the peripheral region of the central 

pocket (as seen in experimental result in Fig. 11), it is intuitive that the failure initiation will 

probably start at the strain concentration at the base of the fillet from the thicker region into the 

thinner region. In fact, the experiment showed that the failure initiated at both the top left and 

Displacement boundary 

condition

Path

0

15

30

45

60

75

0

5

10

15

20

25

0 2 4 6

Force, kN

Displacement, mm

thin material

comparison points

"thick material"

Fig. 8. A portion of the FE mesh of the thin 

cruciform specimen along with locations for axial 

displacement boundary conditions. Also shown is 

the path on which the FEA results are extracted 

for comparison with experimental measurements. Fig. 7. Force-displacement curves for X-axis from 

cruciform specimens.

-0.2

0

0.2

0.4

0.6

0.8

1

0 10 20 30

U displacement, mm

Distance along path, mm

U-expt-1

U-expt-4

U-expt-3

U-expt-2

ABAQUS-U-C3D8R

ABAQUS-U-C3D8

a

Fig. 9. U displacement along path in 

Fig.8: U-expt-1 etc. (measured); 

ABAQUS-U-C3D8 etc. (computed).
bottom right of the pocket area at the base of the fillet radius, and these cracks propagated from the 

periphery to the center of the pocket.

4. Summary

FE analyses of uniaxial and biaxial tensile tests were conducted using ABAQUS software. The 

numerical model uses constitutive material data obtained in uniaxial tests. The model employed 

history-dependent displacement BC data that were obtained from in situ DIC measurements.

Overall, the numerical model showed reasonable agreement with experimental measurements. The 

model predicted the necking correctly in uniaxial specimen. Biaxial straining were seen in the 

central region of interest in cruciform, as desired. The model predicts the path along which the 

eventual failure was seen in the experiment. This model can be used for specimen optimization. 

5. References

[1] T. Foecke et al., A method for direct measurement of multiaxial stress-strain curves in sheet 

metal, Metall.Mater Trans. 38A (2007) 306–313.

[2] M.A. Iadicola, T. Foecke, S.W. Banovic, Experimental observations of evolving yield loci in 

biaxially strained AA 5754-O, Int. J. Plasticity. 24(2008) 2084–2101.

[3] W. Mü̈ller, K. Pöhlandt, New experiments for determining yield loci of sheet metal, J. Mater. 

Process. Tech. 60 (1996) 643–648.

[4] C.C. Tasan et al., In-Plane biaxial loading of sheet metal until fracture, Society for Experimental 

Mechanics (SEM), Orlando, FL, 2008.

[5] E. Hoferlin et al., The design of a biaxial tensile test and its use for the validation of 

crystallographic yield loci, Model. Simul. Mater. Sc. 8 (2000) 423–433.

[6] T. Kuwabara, A. Bael, E. Iizuka, Measurement and analysis of yield locus and work hardening 

characteristics of steel sheets with different r-values, Acta Mater. 50 (2002) 3717–3729.

[7] F. Abu-Farha, L.G. Hector, M. Khraisheh, Cruciform-shaped specimens for elevated 

temperature biaxial testing of lightweight materials, JOM 61 (2009) 48–56.

[8] NIST Center for Automotive Lightweighting, http://www.nist.gov/lightweighting/.

[9] D. Banerjee, M. Iadicola, A. Creuziger, T. Foecke, An Experimental and Numerical Study of 

Deformation Behavior of Steels in Biaxial Tensile Tests, to be published in TMS 2015 

Conference Proceedings, Warrendale, PA.

[10] ABAQUS 12.2 software. Dassault Systemes. http://www.3ds.com/.

[11] M.A. Iadicola, A.A. Creuziger, T. Foecke, Advanced biaxial cruciform testing at the NIST 

Center for Automotive Lightweighting, SEM , 2013.

Fig. 10. Z normal strains: ezz-expt-1 etc.

(measured); ABAQUS-le11-C3D8R (ABAQUS).

Fig. 11. Measured von Mises 

strain.

-0.16

-0.14

-0.12

-0.1

-0.08

-0.06

-0.04

-0.02

0

0 10 20 30

Normal strain, zz

Distance along path, mm

ezz-expt-1

ezz-expt-2

ezz-expt-3

ezz-expt-4

ABAQUS-le33-C3D8

ABAQUS-le33-C3D8R

Fig. 12. ABAQUS computed von 

Mises equivalent plastic strain

using C3D8 elements.