Evaluation of LS-DYNA Concrete

Material Model 159

Publication No. FHWA-HRT-05-063 May 2007

Research, Development, and Technology

Turner-Fairbank Highway Research Center

6300 Georgetown Pike

McLean, VA 22101-2296
Foreword 

This report documents the evaluation of a concrete material model that has been implemented 

into the dynamic finite element code, LS-DYNA, beginning with version 971. This material 

model is in keyword format as MAT_CSCM for Continuous Surface Cap Model. This model 

was developed to predict the dynamic performance—both elastic deformation and failure—of 

concrete used in safety structures when involved in a collision with a motor vehicle. An example 

of a roadside safety structure is a concrete safety barrier that divides opposing lanes of traffic on 

a roadway. Default input parameters for concrete are stored in the model and can be accessed for 

use. This material model only replicates the concrete aggregate. Appropriate reinforcement bars 

or rods must be included in the structure model separately. 

This report is the second of two that completely documents this material model. This report 

documents the testing performed to review the model’s performance and accuracy of results. The 

first report is Users Manual for LS-DYNA Concrete Material Model 159, which documents the 

theoretical basis and required input format, and includes limited hypothetical problems for the 

user. 

This report will be of interest to research engineers who are associated with the evaluation and 

crashworthy performance of roadside safety structures, particularly engineers responsible for 

predicting the crash response of such structures when using the finite element code, LS-DYNA. 

 Michael Trentacoste 

 Director, Office of Safety R&D 

Notice 

This document is disseminated under the sponsorship of the Department of Transportation in the 

interest of information exchange. The United States Government assumes no liability for the use 

of the information contained in this document. This report does not constitute a standard, 

specification, or regulation. 

The United States Government does not endorse products or manufacturers. Trademarks or 

manufacturers’ names appear in this report only because they are considered essential to the 

objective of the document. 

Quality Assurance Statement 

The Federal Highway Administration (FHWA) provides high-quality information to serve 

Government, industry, and the public in a manner that promotes public understanding. Standards 

and policies are used to ensure and maximize the quality, objectivity, utility, and integrity of its 

information. FHWA periodically reviews quality issues and adjusts its programs and processes to 

ensure continuous quality improvement. 
1. Report No. 

FHWA-HRT-05-063 

2. Government Accession No. 3. Recipient's Catalog No. 

5. Report Date 

May 2007 

4. Title and Subtitle 

Evaluation of LS-DYNA Concrete Material Model 159 6. Performing Organization Code 

7. Author(s) 

Yvonne D. Murray 

Akram Abu-Odeh and Roger Bligh

8. Performing Organization Report No. 

9. Performing Organization Name and Address 10. Work Unit No. (TRAIS) 

APTEK, Inc. 

1257 Lake Plaza Dr. Suite 100 

Colorado Springs, CO 80906 

 

Texas Transportation Institute 

Texas A&M University System 

3135 TAMU 

 College Station, TX 77843 

11. Contract or Grant No. 

DTFH61-98-C-00075 

13. Type of Report and Period Covered 

Final Report 

September 27, 2001 through 

December 26, 2004

12. Sponsoring Agency Name and Address 

Volpe National Transportation Systems Center 

55 Broadway, Kendall Square 

Cambridge, MA 02142-1093 

Federal Highway Administration 

6300 Georgetown Pike 

McLean, VA 22101-2296 

14. Sponsoring Agency Code 

15. Supplementary Notes 

The Contracting Officer’s Technical Representative (COTR) for this project is Martin Hargrave, Office of 

Safety Research and Development, HRDS-04, Turner-Fairbank Highway Research Center. 

16. Abstract 

An elastoplastic damage model with rate effects was developed for concrete and implemented into LSDYNA, a commercially available finite element code. This manual documents the evaluation of the 

concrete material model, including the selection of the concrete model input parameters. The model is 

evaluated through correlations with test data: drop tower impact of 1⁄3-scale beams (plain and reinforced), 

bogie vehicle impact of full-scale reinforced beams, pendulum impact of bridge rails, and quasi-static 

loading of a safety-shaped barrier. Although the model was developed and evaluated for roadside safety 

applications, it should also be applicable to many dynamic problems. 

The companion manual to this report is Users Manual for LS-DYNA Concrete Material Model 159, 

FHWA-HRT-05-062.

17. Key Words 

concrete, LS-DYNA, material model, reinforced beam, New 

Jersey barrier, bridge rail, pendulum, bogie vehicle

18. Distribution Statement 

No restrictions. This document is 

available through the National 

Technical Information Service, 

Springfield, VA 22161. 

19. Security Classif. (of this report) 

Unclassified 

20. Security Classif. (of this page) 

Unclassified 

21. No. of Pages 

206 

22. Price 

N/A 

Form DOT F 1700.7 (8-72) Reproduction of completed page authorized 
ii

SI* (MODERN METRIC) CONVERSION FACTORS 

APPROXIMATE CONVERSIONS TO SI UNITS

Symbol When You Know Multiply By To Find Symbol 

LENGTH 

in inches 25.4 millimeters mm 

ft feet 0.305 meters m 

yd yards 0.914 meters m 

mi miles 1.61 kilometers km 

AREA 

in2 square inches 645.2 square millimeters mm2

ft2 square feet 0.093 square meters m2

yd2 square yard 0.836 square meters m2

ac acres 0.405 hectares ha

mi2 square miles 2.59 square kilometers km2

VOLUME 

fl oz fluid ounces 29.57 milliliters mL 

gal gallons 3.785 liters L 

ft3 cubic feet 0.028 cubic meters m3 

yd3 cubic yards 0.765 cubic meters m3 

NOTE: volumes greater than 1000 L shall be shown in m3

MASS 

oz ounces 28.35 grams g

lb pounds 0.454 kilograms kg

T short tons (2000 lb) 0.907 megagrams (or "metric ton") Mg (or "t") 

TEMPERATURE (exact degrees) o

F Fahrenheit 5 (F-32)/9 Celsius oC 

or (F-32)/1.8 

ILLUMINATION 

fc foot-candles 10.76 lux lx

fl foot-Lamberts 3.426 candela/m2 cd/m2

FORCE and PRESSURE or STRESS 

lbf poundforce 4.45 newtons N 

lbf/in2 poundforce per square inch 6.89 kilopascals kPa 

APPROXIMATE CONVERSIONS FROM SI UNITS 

Symbol When You Know Multiply By To Find Symbol 

LENGTH

mm millimeters 0.039 inches in 

m meters 3.28 feet ft 

m meters 1.09 yards yd 

km kilometers 0.621 miles mi 

AREA mm2

 square millimeters 0.0016 square inches in2 

m2 square meters 10.764 square feet ft2 

m2 square meters 1.195 square yards yd2 

ha hectares 2.47 acres ac

km2 square kilometers 0.386 square miles mi2 

VOLUME 

mL milliliters 0.034 fluid ounces fl oz 

L liters 0.264 gallons gal 

m3 cubic meters 35.314 cubic feet ft3 

m3 cubic meters 1.307 cubic yards yd3 

MASS 

g grams 0.035 ounces oz

kg kilograms 2.202 pounds lb

Mg (or "t") megagrams (or "metric ton") 1.103 short tons (2000 lb) T 

TEMPERATURE (exact degrees) o

C Celsius 1.8C+32 Fahrenheit oF 

ILLUMINATION 

lx lux 0.0929 foot-candles fc 

cd/m2 candela/m2 0.2919 foot-Lamberts fl

FORCE and PRESSURE or STRESS 

N newtons 0.225 poundforce lbf 

kPa kilopascals 0.145 poundforce per square inch lbf/in2

*SI is the symbol for th International System of Units. Approp e riate rounding should be made to comply with Section 4 of ASTM E380. 

(Revised March 2003)
iii

TABLE OF CONTENTS

CHAPTER 1. INTRODUCTION ..................................................................1 

MODEL THEORY........................................................................................................ 1 

MODEL INPUT............................................................................................................ 2 

LIMITATIONS OF MATERIAL PROPERTY DATA..................................................... 2 

EVALUATION PROCESS........................................................................................... 3 

EVALUATION CALCULATIONS ................................................................................ 3 

CHAPTER 2. SINGLE ELEMENT SIMULATIONS ....................................5 

UNIAXIAL AND TRIAXIAL STRESS .......................................................................... 5 

VOLUME EXPANSION ............................................................................................... 7 

CYCLIC LOADING...................................................................................................... 7 

PRESSURE VERSUS VOLUMETRIC STRAIN .......................................................... 7 

RATE EFFECTS.......................................................................................................... 9 

KINEMATIC HARDENING ........................................................................................ 11 

CHAPTER 3. SINGLE MATERIAL CYLINDER SIMULATIONS..............13 

CYLINDER GEOMETRY AND LOADING CONDITIONS ......................................... 13 

CYLINDER TENSION RESPONSE........................................................................... 14 

CYLINDER COMPRESSION RESPONSE................................................................ 15 

Damage Modes Observed in Tests..................................................................... 15 

Fixed End Conditions .......................................................................................... 15 

Capped End Conditions ...................................................................................... 17 

Contact Surface Type .......................................................................................... 22 

CHAPTER 4. REGULATION OF SOFTENING FORMULATION.............29 

SINGLE ELEMENTS IN TENSION AND COMPRESSION....................................... 29 

CYLINDERS IN TENSION AND COMPRESSION.................................................... 32 

Details of Each Cylinder Mesh............................................................................ 32 

Demonstration of Mesh Size Sensitivity ............................................................ 33 

Description of Regulatory Technique ................................................................ 37 

Evaluation of Regulatory Technique .................................................................. 37 

Effect of Additional Mesh Refinement on Cylinder Response......................... 40 

SUMMARY REGARDING REGULATION................................................................. 43 

CHAPTER 5. SIZE EFFECT.....................................................................45 

CHAPTER 6. BEAM DROP TOWER IMPACT SIMULATIONS...............51 

TEST DATA .............................................................................................................. 51 

LS-DYNA SIMULATIONS ......................................................................................... 53 

Plain Beams.......................................................................................................... 53 
iv

Reinforced Beams................................................................................................ 56 

SUMMARY FOR DROP TOWER SIMULATIONS .................................................... 64 

CHAPTER 7. BEAM BOGIE VEHICLE IMPACT SIMULATIONS............65 

TEST DATA .............................................................................................................. 65 

LS-DYNA CORRELATIONS ..................................................................................... 67 

High Velocity Impact............................................................................................ 67 

Intermediate Velocity Impact............................................................................... 69 

Low Velocity Impact............................................................................................. 73 

Displacement Histories ....................................................................................... 76 

Strain Histories..................................................................................................... 77 

SUMMARY FOR IMPACT SIMULATIONS ............................................................... 79 

CHAPTER 8. TEXAS T4 BRIDGE RAIL ..................................................81 

USER INTRODUCTION ............................................................................................ 81 

OVERVIEW ............................................................................................................... 82 

PENDULUM TESTING.............................................................................................. 82 

TEST RESULTS........................................................................................................ 83 

SIMULATION METHODOLOGY............................................................................... 88 

PENDULUM MODEL CALIBRATION....................................................................... 88 

FINITE ELEMENT MODEL OF T4 BRIDGE RAIL.................................................... 94 

Overview of T4 Parapet/Deck Model................................................................... 95 

Meshing ................................................................................................................ 98 

Sectional Properties ............................................................................................ 99 

Constraints and Boundary Conditions ............................................................ 100 

Material Definitions............................................................................................ 104 

ANALYSES OF T4 BRIDGE RAIL.......................................................................... 105 

Baseline Parameters.......................................................................................... 105 

Baseline Analysis............................................................................................... 108 

Parametric Analyses.......................................................................................... 108 

Modified System Analyses................................................................................ 115 

Full System Analysis: Four-Bolt Design .......................................................... 117 

Full System Analysis: Three-Bolt Design ........................................................ 120 

SUMMARY FOR BRIDGE RAIL ANALYSES......................................................... 125 

CHAPTER 9. ANALYSES OF SAFETY-SHAPED BARRIER................127 

FINITE ELEMENT MODEL ..................................................................................... 129 

USER EVALUATION RESULTS............................................................................. 132 

DEVELOPER BASELINE CALCULATIONS .......................................................... 133 

DEVELOPER APPLIED FORCE CALCULATIONS ............................................... 139 

SUMMARY FOR SAFETY-SHAPED BARRIER CALCULATIONS........................ 141 

CHAPTER 10. SUMMARY AND RECOMMENDATIONS......................143 

DEVELOPER COMMENTS..................................................................................... 143 

USER COMMENTS................................................................................................. 144 
v

APPENDIX A. USER CODE VERIFICATION ........................................147 

INTRODUCTION ..................................................................................................... 147 

CASE 1. SINGLE ELEMENT SIMULATIONS......................................................... 147 

CASE 2. CYLINDER RUNS .................................................................................... 151 

CASE 3. PLAIN CONCRETE BEAM ...................................................................... 154 

CASE 4. REINFORCED CONCRETE BEAM ......................................................... 158 

CASE 5. BOGIE IMPACT TESTS........................................................................... 162 

APPENDIX B. DEVELOPER SUPPORT OF THE TEXAS T4 BRIDGE 

RAIL ANALYSES................................................................................................... 167 

INTRODUCTION ..................................................................................................... 167 

BRIDGE RAIL DATA .............................................................................................. 168 

PARAMETRIC STUDIES ........................................................................................ 169 

Fixed Parapet Computational Results.............................................................. 170 

Full Deck Computational Results ..................................................................... 178 

DECK TO PARAPET CONNECTION ..................................................................... 185 

SUMMARY OF BRIDGE RAIL CALCULATIONS................................................... 187 

REFERENCES.........................................................................................189 
vi

List of Figures 

Figure 1. The default behavior of the concrete model in uniaxial tensile stress and pure shear 

stress is linear to the peak, followed by brittle softening........................................................ 6 

Figure 2. Strength and ductility increase with confining pressure in these triaxial compression 

simulations .............................................................................................................................. 6 

Figure 3. The concrete model simulates volume expansion in uniaxial compressive stress, in 

agreement with typical test data (strains and stress positive in compression)........................ 8 

Figure 4. The modulus of concrete degrades with strength, as demonstrated by this cyclic 

loading simulation................................................................................................................... 8 

Figure 5. The difference in pressure at a given volumetric strain for these isotropic compression 

and uniaxial strain simulations is due to shear enhanced compaction.................................... 9 

Figure 6. The increase in strength with strain rate is significant in tension at a strain rate of 100 

per second. ............................................................................................................................ 10 

Figure 7. The increase in strength with strain rate in pure shear stress is similar to that modeled 

in uniaxial tensile stress. ....................................................................................................... 10 

Figure 8. The increase in strength with strain rate in uniaxial compression stress is less 

pronounced than in uniaxial tensile stress or pure shear stress............................................. 11 

Figure 9. Application of kinematic hardening simulates prepeak nonlinearity accompanied by 

plastic volume expansion...................................................................................................... 12 

Figure 10. Realistic damage modes are simulated in concrete cylinders loaded in tension and 

compression .......................................................................................................................... 13 

Figure 11. Two bands of damage initiate symmetrically about the axial midplane, then one band 

of damage rapidly dominates................................................................................................ 14 

Figure 12. Damage modes observed in cylinder compression tests as a function of end 

conditions. Source: CRC Press. ........................................................................................... 15 

Figure 13. The damage mode calculated for compression cylinders with fixed ends agrees with 

the X-shaped damage bands observed in tests...................................................................... 16 

Figure 14. Concrete cylinder tested as part of the bogie vehicle impact test series. .................... 17 

Figure 15. A diagonal band of damage is calculated with frictional end constraints if both end 

caps are allowed to rotate and slide (no end cap constraints)............................................... 18 

Figure 16. A diagonal band of damage is calculated with frictional end constraints if one end 

cap is allowed to rotate and slide relative to the other (bottom cap constrained from 

rotating and sliding) .............................................................................................................. 19 

Figure 17. A double diagonal band of damage is initially calculated if both end caps are 

prevented from rotating and sliding (bottom and top caps constrained from rotating and 

sliding). ................................................................................................................................. 20 

Figure 18. A double diagonal band of damage is initially calculated if one end cap is free to 

rotate (bottom cap restrained from rotating and sliding, top cap restrained from sliding). .. 20 

Figure 19. A single diagonal band of damage initiates, but is not retained, if the cylinder is overconstrained (bottom and top caps restrained from sliding)................................................... 21 

Figure 20. Diagonal damage bands are calculated using the 

*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE option, although the diagonal 

band location varies with scale factor................................................................................... 23 

Figure 21. Differences in initial slope are primarily due to differing amounts of contact surface 

penetration between the concrete cylinder and end caps...................................................... 23 
vii

Figure 22. End cap versus concrete displacement with penetration (SFS = 1). ........................... 24 

Figure 23. End cap versus concrete displacement with little penetration (SFS = 10). ................. 24 

Figure 24. The relative displacement between the ends of the concrete cylinder depends on the 

amount of interface penetration present................................................................................ 26 

Figure 25. The stress-displacement histories are in reasonable agreement if the relative 

displacement of the cylinder is used. .................................................................................... 27 

Figure 26. Early time tensile damage occurs in some compressive cylinder calculations in the 

vicinity of the contact surface interface................................................................................ 27 

Figure 27. The fracture energy, which is the area under the softening portion of the stressdisplacement curve, is independent of element size in the direct pull simulations (not 

shifted). ................................................................................................................................. 30 

Figure 28. The fracture energy, which is the area under the softening portion of the stressdisplacement curve, is independent of element size in the direct pull simulations (shifted to 

displacement at peak stress).................................................................................................. 30 

Figure 29. Although the fracture energy is constant, the softening curves vary slightly with 

element size in the unconfined compression simulations (not shifted). ............................... 31 

Figure 30. Although the fracture energy is constant, the softening curves vary slightly with 

element size in the unconfined compression simulations (shifted to displacement at peak 

stress). ................................................................................................................................... 31 

Figure 31. Refinement of each mesh used in sensitivity analyses................................................ 33 

Figure 32. The stress-displacement curves calculated in direct pull with an unregulated 

softening formulation do not converge as the mesh is refined. ............................................ 34 

Figure 33. The damage mode calculated in direct pull with an unregulated softening 

formulation is damage within a single band of elements...................................................... 35 

Figure 34. The stress-displacement curves calculated in unconfined compression with an 

unregulated softening formulation are similar for the basic and refined meshes 

(fixed ends). .......................................................................................................................... 36 

Figure 35. The damage mode calculated in unconfined compression with an unregulated 

softening formulation is a double diagonal (in the basic and refined meshes with 

fixed end conditions)............................................................................................................. 36 

Figure 36. The stress-displacement curves calculated in direct pull with a regulated softening 

formulation converge as the mesh is refined. ....................................................................... 37 

Figure 37. The damage modes calculated in direct pull with a regulated softening formulation 

are in agreement for the basic and refined mesh simulations. .............................................. 38 

Figure 38. The stress-displacement curves calculated in unconfined compression with a 

regulated softening formulation nearly converge as the mesh is refined (fixed ends). ........ 39 

Figure 39. The X-shaped damage mode calculated in unconfined compression with a regulated 

softening formulation is similar for the basic and refined mesh simulations (fixed ends). .. 39 

Figure 40. A crisp X-shaped band of damage is calculated for the very refined mesh, with or 

without regulation of the softening response........................................................................ 41 

Figure 41. The stress-displacement curves calculated in unconfined compression without a 

regulated softening formulation become more brittle as the mesh is refined (fixed ends)... 42 

Figure 42. The stress-displacement curves calculated in unconfined compression with a 

regulated softening formulation become more ductile as the mesh is refined (fixed ends). 42 

Figure 43. Schematic of the size effect, as suggested by Bazant and Planas.(9) ........................... 45 

Figure 44. Refinement of the concrete beam mesh used in the size effect analyses. ................... 46 
viii

Figure 45. The damage simulated in the full-scale beam is more severe than that simulated 

in the 1⁄3-scale beam, which is consistent with the size effect............................................... 47 

Figure 46. The stress-deflection behavior of the full-scale beam is softer than that of the 

1⁄3-scale beam, which is consistent with the size effect......................................................... 48 

Figure 47. Without regulation of the softening formulation, the damage simulated in the fullscale and 1⁄3-scale beams is nearly the same, which is inconsistent with the size effect....... 49 

Figure 48. Without regulation of the softening formulation, the stress versus relative deflection 

curves of the full and 1⁄3-scale beams are nearly identical, which is inconsistent with the 

size effect .............................................................................................................................. 49 

Figure 49. Sketch of four-point bend tests, showing dimensions in millimeters.(10) .................... 52 

Figure 50. Six of the eight plain concrete specimens initially failed with two major cracks 

in the impact regime.............................................................................................................. 53 

Figure 51. Two of the eight plain concrete specimens initially failed with one major crack 

in the impact regime.............................................................................................................. 54 

Figure 52. All plain concrete specimens impact the bottom of the test fixture. ........................... 54 

Figure 53. Four of the eight plain concrete specimens ultimately break into five pieces............. 54 

Figure 54. The plain concrete beam initially breaks into three large pieces in all baseline 

calculations performed (shown at 12 msec for impact at 5.8 m/sec (19.0 ft/sec)). ............. 55 

Figure 55. The plain concrete beam ultimately breaks into five pieces in three of four 

calculations performed (shown at 26 msec for impact at 5.8 m/sec (19.0 ft/sec)). .............. 55 

Figure 56. The plain concrete beam ultimately broke into four pieces in one of four calculations 

performed (shown at 26 msec for impact at 5.0 m/sec (16.4 ft/sec)).................................... 55 

Figure 57. This preliminary calculation demonstrates the formation of one primary crack......... 56 

Figure 58. The over-reinforced concrete beam has localized tensile cracks and concrete 

crushing in the impactor regime (test 15 conducted at 5 m/sec (16.4 ft/sec)). ..................... 57 

Figure 59. The damage mode of the over-reinforced concrete beam at peak deflection is 

localized tensile cracks and concrete crushing in the impactor regime (shown at 16 msec 

for impact at 5 m/sec (16.4 ft/sec)). ...................................................................................... 57 

Figure 60. The simulated damage fringes for impact at 10.6 m/sec (34.8 ft/sec) are less 

extensive than those simulated at 5.0 m/sec (16.4 ft/sec)..................................................... 58 

Figure 61. The measured displacement histories are accurately simulated by LS-DYNA 

concrete material model MAT 159. ...................................................................................... 59 

Figure 62. The processed velocity histories drift once the impactor separates from the beam 

during rebound at about 17 msec.......................................................................................... 60 

Figure 63. The damage mode measured for half of the under-reinforced beam specimens is 

two major cracks beneath the impactor points, without rebar breakage............................... 61 

Figure 64. The damage mode simulated for all under-reinforced beam specimens is two major 

cracks beneath the impactor points, with additional damage toward the ends of the beam. 61 

Figure 65. About half of the under-reinforced beam specimens exhibited cracks originating 

on the top of the specimen, and located halfway between the impactor points and ends of 

the beam................................................................................................................................ 61 

Figure 66. Good displacement history and peak deflection comparisons of LS-DYNA drop 

tower impact simulations with test data for plain and reinforced concrete beams. .............. 64 

Figure 67. Schematic of bogie vehicle impacting reinforced concrete beam. .............................. 65 

Figure 68. The beam rests on greased supports and reacts against two load frames.................... 66 
ix

Figure 69. The beam tested at an impact velocity of 33.1 km/h (20.5 mi/h) exhibits inclined 

shear cracks, localized crushing, and bond failure. .............................................................. 68 

Figure 70. Inclined shear cracks, localized crushing, and bond failure are simulated in the 

calculation conducted at 33 km/h (20.5 mi/h). ..................................................................... 69 

Figure 71. The beam tested at an impact velocity of 15.9 km/h (9.9 mi/h) exhibits inclined 

shear cracks, localized crushing, and bond failure. .............................................................. 70 

Figure 72. Damage dominates one side of the beam impacted at 15.9 km/h (9.9 mi/h). ............. 70 

Figure 73. Tensile damage, inclined shear damage, and bond failure are simulated in the 

calculation conducted at 15.9 km/h (9.9 mi/h) with erosion set to 10 percent strain. .......... 71 

Figure 74. The beam breaks into two major pieces and does not rebound when impacted at 

18 km/h (11.2 mi/h). ............................................................................................................. 72 

Figure 75. This damage modeled at 15.9 km/h (9.9 mi/h) with erosion set to 1 percent strain is 

more extensive than when erosion is set to 10 percent strain............................................... 73 

Figure 76. Cracks form on the tensile face of the beam impacted at 8.6 km/h (5.3 mi/h) and 

propagate toward the compression face................................................................................ 74 

Figure 77. The beam rebounds when impacted at 8.6 km/h (5.3 mi/h), pushing the bogie vehicle 

backward............................................................................................................................... 75 

Figure 78. The simulation of the beam impacted at 8.6 km/h (5.3 mi/h) exhibits substantial 

damage, but retains its integrity and rebounds...................................................................... 75 

Figure 79. The displacement histories from the LS-DYNA bogie vehicle impact simulations 

compare well with the test data............................................................................................. 76 

Figure 80. The calculations conducted at 8.6 km/h (5.3 mi/h) correlate best with the test data 

if the supports are modeled................................................................................................... 77 

Figure 81. Strain histories measured on the compressive face of each beam peak around 0.23 

percent strain......................................................................................................................... 78 

Figure 82. The strain histories from the LS-DYNA bogie vehicle impact simulations vary with 

impact velocity...................................................................................................................... 78 

Figure 83. Details of T4 rail with four-bolt anchorage and 254-mm- (10-inch-) wide parapet. .. 84 

Figure 84. Details of T4 rail with three-bolt anchorage and 317.5-mm- (12.5-inch-) wide 

parapet................................................................................................................................... 85 

Figure 85. Parapet before test P3. ................................................................................................. 86 

Figure 86. Parapet before test P5. ................................................................................................. 86 

Figure 87. Parapet damage after test P3........................................................................................ 87 

Figure 88. Parapet damage after test P4........................................................................................ 87 

Figure 89. Parapet damage after test P5, side. .............................................................................. 89 

Figure 90. Parapet damage after test P5, rear. .............................................................................. 89 

Figure 91. Parapet damage after test P7........................................................................................ 90 

Figure 92. Original pendulum model............................................................................................ 91 

Figure 93. Modified pendulum model. ......................................................................................... 91 

Figure 94. Comparison of the SBP model to rigid pole calibration test....................................... 92 

Figure 95. Force-time histories for benchmark tests and spring models. ..................................... 93 

Figure 96. Force-displacement relationships for benchmark tests and SBP2 model.................... 94 

Figure 97. Model of T4 bridge rail specimen with four-bolt anchorage and 254-mm- 

(10-inch-) wide parapet......................................................................................................... 95 

Figure 98. Model of T4 bridge rail specimen with three-bolt anchorage and 317.5-mm- 

(12.5-inch-) wide parapet...................................................................................................... 96 
x

Figure 99. Closeup view of steel rail system with four-bolt anchorage. ...................................... 96 

Figure 100. Steel reinforcement and anchor bolts for T4 bridge rail specimen with four-bolt 

anchorage and 254-mm- (10-inch-) wide parapet................................................................. 97 

Figure 101. Steel reinforcement and anchor bolts for T4 bridge rail specimen with three-bolt 

anchorage and 317.5-mm- (12.5-inch-) wide parapet........................................................... 97 

Figure 102. Right end view of parapet-only model for four-bolt design and three-bolt design... 98 

Figure 103. Original parapet mesh used for merging nodes with steel reinforcement............... 100 

Figure 104. Revised parapet mesh with steel reinforcement. ..................................................... 101 

Figure 105. Linear mesh biasing along the height of parapet and width of deck....................... 101 

Figure 106. Bell curve mesh biasing along length of parapet and uniform meshing along 

length of deck...................................................................................................................... 102 

Figure 107. Boundary conditions used for the full system model with deck and for the 

parapet-only model. ............................................................................................................ 102 

Figure 108. Anchor bolt constraint to base plate. ....................................................................... 103 

Figure 109. Contacts definitions for the T4 bridge rail model. .................................................. 104 

Figure 110. Damage fringe for baseline simulation of T4 with four-bolt anchorage and 

254-mm- (10-inch-) wide parapet....................................................................................... 108 

Figure 111. Element erosion profile (simulation case02, ERODE =1) on traffic side. .............. 109 

Figure 112. Element erosion profile (simulation case02, ERODE =1) ...................................... 109 

Figure 113. Damage fringes for simulation case02 (ERODE =1).............................................. 110 

Figure 114. Parapet failure with fracture energies at 20 percent of baseline values. ................. 111 

Figure 115. Energy-time histories for pendulum impact of T4 bridge rail with fracture 

energies at 20 percent of baseline values............................................................................ 112 

Figure 116. Parapet failure with fracture energies at 50 percent of baseline values. ................. 112 

Figure 117. Parapet failure with fracture energies at 27.5 percent of baseline values. .............. 113 

Figure 118. Energy-time histories for pendulum impact of T4 bridge rail with fracture 

energies at 27.5 percent of baseline values......................................................................... 114 

Figure 119. Enhanced anchor bolt-to-base plate connection model........................................... 115 

Figure 120. Fracture profile of modified T4 system at 0.080 seconds. ...................................... 116 

Figure 121. Fracture profile of modified T4 system at 0.115 seconds. ...................................... 116 

Figure 122. Fracture profile of modified T4 system at 0.250 seconds. ...................................... 117 

Figure 123. Profile of damaged T4 bridge rail system with four-bolt anchorage after 

pendulum impact................................................................................................................. 118 

Figure 124. Fracture profile for T4 bridge rail with four-bolt anchorage for parapet and eroded 

elements................................................................................................................................118 

Figure 125. Pendulum bogie accelerations for impact of T4 bridge rail with four-bolt anchorage 

and 254-mm- (10-inch-) wide parapet ................................................................................ 119 

Figure 126. Pendulum bogie velocities for impact of T4 bridge rail with four-bolt anchorage and 

254-mm- (10-inch-) wide parapet....................................................................................... 120 

Figure 127. Profile of T4 bridge rail system with three-bolt anchorage after pendulum 

impact.................................................................................................................................. 121 

Figure 128. Damage to 317.5-mm- (12.5-inch-) wide parapet after pendulum impact showing 

element erosion. .................................................................................................................. 122 

Figure 129. Damage to 317.5-mm- (12.5-inch-) wide parapet after pendulum impact showing 

damage fringes.................................................................................................................... 122 
xi

Figure 130. Pendulum bogie accelerations for impact of T4 bridge rail with three-bolt 

anchorage and 317.5-mm- (12.5-inch-) wide parapet......................................................... 124 

Figure 131. Pendulum bogie velocities for impact of T4 bridge rail with three-bolt anchorage 

and 317.5-mm- (12.5-inch-) wide parapet. ......................................................................... 124 

Figure 132. Test setup for static load tests on safety-shaped barriers. ....................................... 127 

Figure 133. Failure mode at end of the safety-shaped barrier. ................................................... 128 

Figure 134. Measured load versus displacement for the safety-shaped barrier.......................... 128 

Figure 135. Cross section of the Florida safety-shaped barrier with New Jersey profile.(8)....... 130 

Figure 136. Cross section of Florida barrier model concrete mesh and reinforcement layout... 131 

Figure 137. Isometric view of steel reinforcement in Florida barrier model.............................. 131 

Figure 138. Model of quasi-static load test setup. ...................................................................... 132 

Figure 139. Fracture profile of Florida safety-shaped barrier..................................................... 133 

Figure 140. A damage concentration is simulated in the parapet due to application of the 

steel/timber spreader plate that is not observed in the post-test parapet............................. 134 

Figure 141. The damage concentration is relieved if the timber is realistically modeled as an 

elastoplastic damaging material.......................................................................................... 135 

Figure 142. A realistic damage and erosion pattern is simulated if the timber remains in 

contact with the parapet (ERODE = 1.05).......................................................................... 136 

Figure 143. The primary erosion agrees with the measured crack pattern if the timber remains 

in contact with the parapet (ERODE = 1.0)........................................................................ 137 

Figure 144. The primary erosion agrees with the measured crack pattern if the timber remains 

in contact with the parapet (ERODE = 1.0)........................................................................ 138 

Figure 145. The calculated force versus deflection history is in reasonable agreement with the 

measured curve for the first 12 mm (0.5 inches) of deflection........................................... 139 

Figure 146. The computed damage mode is similar to that measured if the load is applied via 

concentrated nodal point forces (at 11- to 12-mm (0.43- to 0.5-inch) deflection). ............ 140 

Figure 147. The computed force versus displacement unloads, when the load is applied via 

concentrated nodal point forces (ERODE = 1.05).............................................................. 140 

Figure 148. Single element under compressive loading, developer. .......................................... 148 

Figure 149. Single element under compressive loading, user. ................................................... 148 

Figure 150. Single element under tensile loading, developer..................................................... 149 

Figure 151. Single element under tensile loading, user.............................................................. 149 

Figure 152. Single element under pure shear loading, developer............................................... 150 

Figure 153. Single element under pure shear loading, user........................................................ 150 

Figure 154. Concrete cylinder model with inclined cross section.............................................. 151 

Figure 155. Damage fringe t = 13.498 msec............................................................................... 152 

Figure 156. Damage fringe t = 13.598 msec............................................................................... 152 

Figure 157. Damage fringe at t = 40 msec.................................................................................. 153 

Figure 158. Cross-sectional force (developer)............................................................................ 153 

Figure 159. Cross-sectional force (user)..................................................................................... 154 

Figure 160. Plain concrete damage fringe at 1 msec (developer)............................................... 155 

Figure 161. Plain concrete damage fringe at 4 msec (developer)............................................... 155 

Figure 162. Plain concrete damage fringe at 20 msec (developer)............................................. 155 

Figure 163. Plain concrete damage fringe at 30 msec (developer)............................................. 155 

Figure 164. Plain concrete damage fringe t =1 msec (user Linux)............................................. 156 

Figure 165. Plain concrete damage fringe t = 4 msec (user Linux)............................................ 156 
xii

Figure 166. Plain concrete damage fringe t = 20 msec (user Linux).......................................... 156 

Figure 167. Plain concrete damage fringe t = 30 msec (user Linux).......................................... 156 

Figure 168. Plain concrete damage fringe t = 1 msec (user Windows). ..................................... 157 

Figure 169. Plain concrete damage fringe t = 4 msec (user Windows). ..................................... 157 

Figure 170. Plain concrete damage fringe t = 20 msec (user Windows). ................................... 157 

Figure 171. Plain concrete damage fringe t = 30 msec (user Windows). ................................... 157 

Figure 172. Reinforced concrete damage fringe t = 1 msec (developer).................................... 159 

Figure 173 Reinforced concrete damage fringe t = 4 msec (developer)..................................... 159 

Figure 174. Reinforced concrete damage fringe t = 16 msec (developer).................................. 159 

Figure 175. Reinforced concrete damage fringe t = 20 msec (developer).................................. 159 

Figure 176. Reinforced concrete damage fringe t = 1 msec (user Linux). ................................. 160 

Figure 177. Reinforced concrete damage fringe t = 4 msec (user Linux). ................................. 160 

Figure 178. Reinforced concrete damage fringe t = 16 msec (user Linux). ............................... 160 

Figure 179. Reinforced concrete damage fringe t = 20 msec (user Linux). ............................... 160 

Figure 180. Displacement of node 49,072 in millimeters (developer). ...................................... 161 

Figure 181. Displacement of node 49,072 in millimeters (user Linux)...................................... 161 

Figure 182. Bogie damage, t = 4 msec (developer). ................................................................... 163 

Figure 183. Bogie damage t = 8 msec (developer). .................................................................... 163 

Figure 184. Bogie damage, t = 48 msec (developer). ................................................................. 163 

Figure 185. Bogie damage, t = 80 msec (developer). ................................................................. 163 

Figure 186. Damage fringes t = 4 msec (user Windows). .......................................................... 164 

Figure 187. Damage fringe t = 8 msec (user Windows)............................................................. 164 

Figure 188. Damage fringe t = 48 msec (user Windows)........................................................... 164 

Figure 189. Damage fringe t = 80 msec (user Windows)........................................................... 164 

Figure 190. Damage, t = 4 msec (user Linux). ........................................................................... 165 

Figure 191. Damage, t = 8 msec (user Linux). ........................................................................... 165 

Figure 192. Damage, t = 48 msec (user Linux). ......................................................................... 165 

Figure 193. Damage t = 80 msec (user Linux). .......................................................................... 165 

Figure 194. Finite element model of the pendulum, rail, and fixed end of parapet.................... 169 

Figure 195. Damage fringes calculated with baseline properties for a fixed end parapet.......... 170 

Figure 196. The deformed configuration and damage of the Texas T4 bridge rail (four-bolt 

design) from impact with the simplified pendulum model (without a crushable nose) at 

25 percent maximum available kinetic energy is similar to that observed during the tests.172 

Figure 197. Stiffening the spring increases the maximum deceleration and decreases the time 

at which the maximum deceleration occurs........................................................................ 176 

Figure 198. Good comparison of measured and calculated acceleration histories for the 

reduced fixed parapet mesh (spring stiffened using 80 percent deflection scale factor). ... 177 

Figure 199. Addition of the deck model improves correlations with the test data (spring 

stiffened using 80 percent deflection scale factor). ............................................................ 178 

Figure 200. All calculations run with baseline or slightly reduced properties (repow = 0.5 

and Gfs / Gft = 0.5) produce rail deflections within two standard deviations of the measured 

results .................................................................................................................................. 181 

Figure 201. Deflection and damage calculated with baseline properties using a stiffened 

spring (80 percent displacement scale factor)..................................................................... 182 

Figure 202. Closeup of damage calculated with baseline properties using a stiffened spring 

(80 percent displacement scale factor)................................................................................ 182 
xiii

Figure 203. Deflection and damage calculated with slightly reduced properties using a 

stiffened spring (80 percent displacement scale factor)...................................................... 183 

Figure 204. Closeup of damage calculated with slightly reduced properties using a stiffened 

spring (80 percent displacement scale factor)..................................................................... 183 

Figure 205. Larger rail deflections are calculated at 9,835 mm/sec (large dots) compared with 

9,556 mm/sec (solid and large dashed lines). ..................................................................... 185 

Figure 206. The tensile damage at the base of the parapet is eliminated if a flexible joint is 

modeled (80 percent displacement scale factor with baseline properties).......................... 186 
xiv

List of Tables 

Table 1. Over-reinforced beam test matrix................................................................................... 51 

Table 2. Under-reinforced beam test matrix................................................................................. 51 

Table 3. Plain concrete beam test matrix...................................................................................... 52 

Table 4. Primary crack analysis of test 15 conducted at 5 m/sec (16.4 ft/sec). ............................ 58 

Table 5. Comparison of measured and computed deflections for the over-reinforced beams. .... 59 

Table 6. Crack analysis for one under-reinforced beam tested with an impactor mass 

of 31.75 kg (70 lb). ............................................................................................................... 62 

Table 7. Comparison of measured and computed deflections for the under-reinforced beams. .. 62 

Table 8. Short input format for parapet concrete material model............................................... 106 

Table 9. Short input format for bridge deck concrete material model........................................ 106 

Table 10. Long input format for parapet concrete material model............................................. 107 

Table 11. Long input format for bridge deck concrete material model. ..................................... 107 

Table 12. Force comparison between tests and simulation for T4 rail system with four-bolt 

anchorage. ........................................................................................................................... 119 

Table 13. Force comparison between tests and simulation for T4 rail system with three-bolt 

anchorage. ........................................................................................................................... 123 

Table 14. Rail deflection and pendulum crush in the Texas T4 bridge rail tests........................ 168 

Table 15. Rail deflection as a function of maximum kinetic energy available........................... 172 

Table 16. Rail deflection, pendulum crush, and crush energy as a function of spring stiffness 

and concrete properties for the fixed end parapet model.................................................... 175 

Table 17. Rail deflection, pendulum crush, and crush energy as a function of spring stiffness 

and concrete properties for the full deck model.................................................................. 179 

Table 18. Rail deflection, pendulum crush, and crush energy for calculations conducted with 

increased impact velocity (9,835 mm/sec) for the full deck model.................................... 184 
xv

Acronyms and Abbreviations 

CEB Comite Euro-International Du Beton 

COTR Contracting Officer’s Technical Representative 

CSCM continuous surface cap model 

FHWA Federal Highway Administration 

FIP Fédération Internationale de la Précontrainte 

FOIL Federal Outdoor Impact Laboratory 

LSTC Livermore Software Technology Corporation 

NCAC National Crash Analysis Center 

NCHRP National Cooperative Highway Research Program 

SBP spring-based pendulum 

SGI Silicon Graphics, Inc. 

1 

CHAPTER 1. INTRODUCTION 

Three million human injuries and 42,000 premature deaths occur annually as a result of motor 

vehicle crashes.(1) To help reduce the toll of this problem, the Federal Highway Administration 

(FHWA) has set a strategic goal to improve the safety of our Nation’s roadways. One way this is 

being accomplished is by expanding the use of the LS-DYNA finite element code to replicate 

three-dimensional motor vehicle crashes into roadside safety structures.(2) The objective is to 

protect the vehicle occupants from serious injury by making the structures more crashworthy. 

Roadside safety structures include bridge rails, barriers, and guardrails. One important bridge, 

barrier, and guardrail material is concrete (with reinforcement). 

The roadside safety community supplements measured crash test data with LS-DYNA 

simulations performed on the computer. The accuracy of the simulations depends, in part, on the 

material models formulated to simulate the behavior of the roadside structures and vehicle 

materials. A comprehensive concrete material model was developed, implemented in the 

LS-DYNA finite element code, and evaluated for simulating the deformation and damage to 

reinforced concrete structures from dynamic impact. For ease of use, default material properties 

for standard concrete are incorporated into the model as a function of concrete compressive 

strength and maximum aggregate size. Correlations with drop tower, bogie vehicle, and 

pendulum impact tests are used to evaluate the model and finalize the default material properties. 

The calculations of chapters 1 through 7, chapter 9, and appendix B of this evaluation report 

were conducted and documented by the developer of the concrete material model, referred to 

here as the “developer.” The calculations of chapter 8, chapter 9, and appendix A were 

conducted and documented by a potential end user of the concrete material model, referred to 

here as the “user.” Conclusions and recommendations from both the developer and user are 

discussed in chapter 10. 

MODEL THEORY 

The concrete model was primarily developed to simulate the deformation and failure of concrete 

in roadside safety structures impacted by vehicles. Examples are bridge rails and safety barriers. 

The concrete model is commonly referred to as a smooth or continuous surface cap model. 

Hence, model 159 is implemented in keyword format as MAT_CSCM for Continuous Surface 

Cap Model. A smooth and continuous intersection is formulated between the failure surface and 

hardening cap. The main features of the model are: 

• Isotropic constitutive equations. 

• Three stress invariant yield surface with translation for prepeak hardening. 

• A hardening cap that expands and contracts. 

• Damage-based softening with erosion and modulus reduction.

• Rate effects for increasing strength in high-strain rate applications. 

General discussions of these types of formulations are given in references by Murray, Lewis, and 

Schwer.(3,4,5) Thorough details of the concrete model theory, a user’s guide, and example input 
2 

are documented in the companion manual to this report titled FHWA HRT 05-062 Users Manual 

for LS-DYNA Concrete Model 159.(6) 

Concrete structures typically contain steel reinforcement. Steel reinforcement exhibits rate 

effects, and yields in a ductile manner until it breaks at an ultimate strain greater than about 20 

percent. The reinforcement model plays an important role in modeling reinforced concrete 

behavior. Our approach is to explicitly model the reinforcement (beam elements) separately from 

the concrete (hex elements) using an elastoplastic material model with yielding, hardening, rate 

effects, and plastic strain-based failure (such as MAT_PIECEWISE_LINEAR_PLASTICITY). 

MODEL INPUT 

There are two methods for setting up the model input. The traditional method is to supply all 

material parameters, such as moduli, strengths, hardening, softening, and rate effects parameters 

(MAT_CSCM). A more convenient method is to request default parameters 

(MAT_CSCM_CONCRETE). Default parameters are provided for the concrete model based on 

three input specifications: the unconfined compression strength (grade), the aggregate size, and 

the units. The parameters are fit to data for unconfined compression strengths between about 20 

and 58 megapascals (MPa) (2,901 and 8,412 pounds per square inch (lbf/inch2)), and aggregate 

sizes between 8 millimeters (mm) (0.3 inches) and 32 mm (1.26 inches). The unconfined 

compression strength affects all aspects of the fit, including stiffness, three-dimensional yield 

strength, hardening, and damage-based softening. The aggregate size affects only the softening 

behavior of the damage formulation. 

The suite of material properties was primarily obtained through use of the Comite EuroInternational Du Beton-Fédération Internationale de la Précontrainte Model (CEB-FIP) Code,(7)

supplemented through correlations with the drop tower, bogie vehicle, and pendulum impact 

tests. This code is a synthesis of research findings and contains a thorough section on concrete 

classification and constitutive relations. Various material properties, such as compressive and 

tensile strengths, stiffness, and tensile fracture energy, are reported as a function of grade and 

aggregate size. A thorough discussion of the model input parameters is documented in the 

concrete model user’s manual.(6) 

LIMITATIONS OF MATERIAL PROPERTY DATA 

Limitations of published laboratory test data for setting the default material properties include: 

• No direct measurements of the softening behavior (fracture energy) in pure shear stress. 

The fracture energy is an area under the stress-displacement curve (from peak stress to 

zero stress). 

• Limited information on rate effects for stress states other than uniaxial tensile stress and 

uniaxial compression stress. This includes the effect of rate on fracture energy as well as 

strength. 
3 

Our methodology is to estimate the missing material property values through LS-DYNA 

correlations with static and impact data provided by the user. Hence the LS-DYNA simulations 

discussed in this document serves not only to evaluate the material model but also to set default 

material property values. 

EVALUATION PROCESS 

Calculations were compared with a wide variety of test data to evaluate the performance of the 

concrete material model and the accuracy of the default material parameters. The evaluation of 

the concrete model proceeded in two steps. The first step was to evaluate the model as a userdefined material, which the developer accomplished. This means that the model was hooked up 

to the LS-DYNA code (version 970) as material model #42 via an interface. The developer 

retained access to the concrete model source code in order to enhance the formulation and adjust 

the default parameters during the evaluation process. 

Once the evaluation was near completion and all default parameters were tentatively selected, the 

concrete model was forwarded to Livermore Software Technology Corporation (LSTC) for 

permanent implementation into the LS-DYNA code. LSTC and the developer implemented the 

model into a beta 971 version of LS-DYNA as material model 159. 

The second step was to evaluate the concrete model as material model 159 in the LS-DYNA 

code. Both the developer and the user accomplished this step. One objective was to check the 

permanent implementation to make sure that material model 159 produced the same results as 

the user-defined material. Adjustments in the LSTC implementation were made until agreement 

was achieved. A second objective was to make sure that the model produced the same or similar 

results on different computer platforms. Generally, results agree by platform until erosion occurs, 

at which time they diverge slightly (see appendix A). A third objective was to allow a potential 

end user access to the model for independent evaluation. Calculations performed by the 

developer were conducted using LS-DYNA beta version 971 (revisions 1432 and 2582) on a PC 

using Microsoft® (MS) Windows® XP. Calculations performed by the user were conducted using 

LS-DYNA beta version 971 with MS-Windows (release 1612 single precision) and LinuxTM 

Intel 32 bit architecture (release 1708 single precision). Minor adjustments in the model theory 

and default parameters were finalized with LSTC before documenting this effort. Results and 

conclusions from both the developer and user are included at the end of this document. 

EVALUATION CALCULATIONS 

Evaluation of the model requires two general types of test data: basic material property data of 

plain concrete for determining input parameters to the model and impact tests of reinforced 

concrete for evaluation of the model formulation. Most of the tests simulated are intended to 

produce failure conditions in the concrete that replicate the failure conditions in roadside safety 

applications. Evaluation simulations performed are: 

• Single element simulations to check the implementation of the model via examination of 

the stress versus displacement behavior. 
4 

• Single material simulations (cylinders in tension and compression) to check simulation of 

the damage modes and to check convergence of the model with mesh refinement. 

Computed damage modes are compared with measured damage modes discussed in the 

general literature. 

• Drop tower impact simulations of plain and reinforced concrete beams. Computed results 

are compared with test data on 1⁄3-scale beams in dynamic four-point bending. The test 

data were specifically generated for use on this project. 

• Bogie vehicle impact simulations of full-scale reinforced concrete beams in dynamic 

four-point bending. Computed results are compared with test data specifically generated 

for this project. 

• Pendulum impact simulations of the Texas T4 bridge rail parapet and deck section with 

two base-plate configurations (test 3-11 of National Cooperative Highway Research 

Program (NCHRP) Report 350). Computed results are compared with test data generated 

by the user on a separately funded project.(8)

• Quasi-static simulations of a New Jersey profile concrete safety-shaped barrier. 

Computed results are compared with test data generated by the user on a separately 

funded project.(9)

All calculations discussed in this report were performed with knowledge of the test results. This 

is because correlations with test results were used to set various default parameters and to help 

refine the model. Future calculations performed by roadside safety analysts will assess the 

predictive capability and provide a more thorough evaluation and validation of the concrete 

material model. Analysts include those at FHWA, National Highway Traffic Safety 

Administration, National Crash Analysis Center (NCAC), and FHWA-organized Centers of 

Excellence for Finite Element Crash Analysis. Accurate predictions, in which the analyst is 

unaware of the measured results before the simulation, build more confidence in a model than 

accurate correlations. 
5 

CHAPTER 2. SINGLE ELEMENT SIMULATIONS 

Single element simulations were performed with LS-DYNA to verify the implementation of the 

concrete model and to display the basic stress-strain behavior of the model. All simulations were 

conducted with cubic hex elements, 38.1 mm (1.5 inches) in each dimension. Unless otherwise 

specified, approximate default material properties are used for 28 MPa (4,061 lbf/inch2) concrete 

with 19 mm (0.75 inches) maximum aggregate size. Stresses and strains are plotted positive in 

tension unless otherwise noted. 

UNIAXIAL AND TRIAXIAL STRESS 

Typical behavior of the concrete model in uniaxial and triaxial stress is shown in Figures 1 and 2. 

In uniaxial tensile stress and pure shear stress, the stress-displacement behavior is modeled linear 

to peak, followed by brittle softening. Although not shown, the behavior of the model in biaxial 

and triaxial tensile stress is nearly identical to that shown for uniaxial tensile stress, with the 

same peak strength and softening response. 

In uniaxial compressive stress, the stress-displacement behavior is also modeled linear to peak 

followed by gradual softening to near zero strength. The unconfined compressive strength is 

approximately 10 times the unconfined tensile strength, in agreement with typical test data for 

concrete. The fracture energy shown in unconfined compression is approximately 100 times 

greater than the fracture energy in unconfined tension. The energy is the area under the softening 

portion of the stress versus displacement curve. The developer recommends values between 50 

and 100 for the compression to tension fracture energy ratio. A value of 100 was ultimately 

selected at the end of the program as the default value. 

The concrete elements also soften when confined at moderate pressure, although they exhibit a 

residual strength (plateau) rather than softening to zero. Triaxial compression refers to tests or 

simulations in which the lateral confining pressure is held constant around the specimen 

(element) while the axial compression load is quasi-statically increased. The concrete strength 

increases with confining pressure in the simulations, in qualitative agreement with typical test 

data. 
6 

cm = 0.39 inch 

Figure 1. The default behavior of the concrete model in uniaxial tensile stress and pure shear 

stress is linear to the peak, followed by brittle softening. 

cm = 0.39 inch 

Figure 2. Strength and ductility increase with confining pressure in these triaxial 

compression simulations.

Stress (MPa)
7 

VOLUME EXPANSION 

Standard concrete exhibits volume expansion under compressive loading at low confining 

pressures less than about 100 MPa (14,504 lbf/inch2

). This volume expansion is called dilation 

and is calculated in the concrete model by the plasticity formulation. The volumetric behavior of 

the model is shown in Figure 3 for uniaxial compressive stress for 35 MPa (5,076 lbf/inch2) 

concrete. The volume initially compacts during the elastic phase, because Poisson’s ratio is less 

than 0.5. Volume expansion commences at peak strength and continues throughout the combined 

plasticity-softening phase. The effective Poisson’s ratio during dilation may exceed 0.5 

CYCLIC LOADING 

As concrete softens, its stiffness also degrades. Stiffness degradation is shown in Figure 4 for 

uniaxial stress with cycling from tension to compression, and then back to tension for 45 MPa 

(6,527 lbf/inch2

) concrete. The unloading occurs along a different slope (degraded modulus), 

then the initial loading slope (undamaged modulus). In addition, when the state of stress 

transitions from tension to compression, the undamaged modulus is recovered (recovered 

modulus). This is the default option obtained with recov = 0. If recov = 1, the modulus remains 

fully degraded when transitioning from tension to compression. If recov is set between 0 and 1, 

the modulus remains partially degraded. 

PRESSURE VERSUS VOLUMETRIC STRAIN 

Concrete hardens due to pore compaction. Consider the pressure versus volumetric strain 

behavior of the model shown in Figure 5. One simulation was conducted for isotropic 

compression (also called hydrostatic compression), the other for uniaxial strain. Note that the 

pressure versus volumetric strain curves differ. This is because the amount of compaction 

depends upon the amount of shear stress present. Less pressure is required to compact concrete 

to a given volumetric strain when shear stress is present (the uniaxial strain simulation), than 

when shear stress is not present (the isotropic compression simulation). This behavior is known 

as shear enhanced compaction. It occurs in concrete and most geological materials. Slight shear 

enhanced compaction at low confining pressures is expected in roadside safety applications. 
8 

psi = 145.05 MPa 

Figure 3. The concrete model simulates volume expansion in uniaxial compressive stress, in 

agreement with typical test data (strains and stress positive in compression). 

psi = 145.05 MPa 

Figure 4. The modulus of concrete degrades with strength, as demonstrated 

by this cyclic loading simulation. 

Undamaged Modulus 

Degraded Modulus 

Recovered Modulus 
9 

psi = 145.05 MPa 

Figure 5. The difference in pressure at a given volumetric strain for these isotropic compression 

and uniaxial strain simulations is due to shear enhanced compaction. 

RATE EFFECTS 

The strength of concrete increases with increasing strain rate. For roadside safety applications, 

strain rates in the 1 to 10 per second (sec) range will produce peak strength increases of about 35 

to 50 percent in compression and 150 to 300 percent in tension. The initial elastic modulus does 

not change significantly with strain rate.

 Rate effects are computationally demonstrated in Figures 6–8 for simulations conducted in 

uniaxial tensile stress, pure shear stress, and uniaxial compression stress. The simulations were 

conducted at a high-strain rate of 100/sec. Note that the increase in strength in tension and shear 

is much greater than that in compression. Also note that the softening response depends on the 

value of repow. A value of repow = 0 minimizes the fracture energy. A value of repow = 1 

increases the fracture energy in proportion to the increase in strength, and is the default value. 
10 

psi = 145.05 MPa, mm = 0.039 inch

Figure 6. The increase in strength with strain rate is significant in tension at a strain rate of 100 

per second.

psi = 145.05 MPa, mm = 0.039 inch

Figure 7. The increase in strength with strain rate in pure shear stress is similar to that modeled 

in uniaxial tensile stress. 
11 

psi = 145.05 MPa, mm = 0.039 inch 

Figure 8. The increase in strength with strain rate in uniaxial compression stress is less 

pronounced than in uniaxial tensile stress or pure shear stress. 

KINEMATIC HARDENING 

One optional variation on the behavior previously shown in Figure 2 is the addition of prepeak 

nonlinearity simulated with the kinematic hardening formulation. Such behavior is shown in 

Figure 9 for uniaxial stress in compression. Dilation initiates when hardening initiates, just prior 

to peak strength. Prepeak nonlinearity is more pronounced in compression than in tension or 

shear. This formulation is optional and not default because it is not essential to good performance 

of the model. The developer has found that accurate modeling of the damage fracture energies 

and rate effects are the key behaviors needed for good correlations with most dynamic roadside 

safety test data. 
12 

psi = 145.05 MPa

Figure 9. Application of kinematic hardening simulates prepeak nonlinearity accompanied by 

plastic volume expansion. 
13 

CHAPTER 3. SINGLE MATERIAL CYLINDER SIMULATIONS 

Simulations of plain concrete allow us to evaluate the behavior of the concrete model without the 

complicating effects of the steel reinforcement. One such set of simulations performed were 

quasi-static loading of plain concrete cylinders in tension and compression. These simulations 

demonstrate that the concrete model simulates the basic damage modes observed in tests. These 

are splitting of the cylinder in tension, and diagonal failure in compression, as shown in Figure 

10. 

Figure 10. Realistic damage modes are simulated in concrete cylinders loaded in tension 

and compression. 

CYLINDER GEOMETRY AND LOADING CONDITIONS 

The cylinder analyzed is 304.8 mm (12 inches) long and 152.4 mm (6 inches) in diameter. 

Loading conditions are direct pull (uniaxial tensile stress) and unconfined compression (uniaxial 

compression stress). These are achieved by applying a uniform constant velocity to the nodes at 

one end of the cylinder (tension) or to the end caps (compression). Velocity is used to represent 

displacement control, rather than pressure or force conditions, in order to model softening 

following peak strength. Steel end caps, with slight friction between the cap and cylinder, are 

modeled in compression in order to simulate the diagonal failure observed in compression tests 

conducted as part of the bogie vehicle impact tests. Idealized end conditions in compression 

(applied nodal velocities without lateral constraint or friction) produce wedge-type failure, rather 

than diagonal failure. Laterally constrained ends produce two diagonal bands of damage (damage 

in an X-shape), as discussed in subsequent paragraphs. 
14 

The fringes shown in all deformed configuration plots of this paper range from 0 to 1 and 

indicate the level of damage calculated by the concrete model. A fringe value of 0 indicates no 

damage, so concrete strength and stiffness are those originally specified as input values. A fringe 

value of 1 indicates maximum damage, in which the concrete strength and stiffness are reduced 

to zero. Elements ERODE (are removed from the calculation and figure) when damage exceeds 

0.99 and the maximum principal strain exceeds a user-specified value (typically between 0 and 

0.10). An example fringe scale is given in Figure 10, which relates damage level to color. 

Alternatively, for those with difficulty distinguishing color, lighter fringes indicate higher levels 

of damage. Commentary is added to figures, where needed, to identify fringes of high damage. 

CYLINDER TENSION RESPONSE 

One boundary condition is analyzed for direct pull of the cylinders. The boundary condition is no 

lateral constraint on the ends of the cylinder so the cylinder is free to expand or contract laterally 

along its entire length. This idealized condition produces a realistic damage mode (breaking of 

the cylinder along one band of elements), as shown in Figure 11. 

Figure 11. Two bands of damage initiate symmetrically about the axial midplane, then one band 

of damage rapidly dominates. 

Initially, at very low damage levels, two bands of damage form, as shown at 13.598 milliseconds 

(msec). These bands are symmetrically located relative to the axial midplane of the cylinder. 

The location of the damage bands is thought to be dependent upon wave propagation within the 

cylinder, because the applied nodal velocities and damage bands are symmetric about the 

midplane. However, following initial formation, one of these bands becomes more dominant 

than the other band. Such asymmetric behavior probably results from numerical roundoff during 

brittle softening. This calculation demonstrates that a realistic damage mode is simulated by the 

concrete model in tension. 
15 

CYLINDER COMPRESSION RESPONSE 

Damage Modes Observed in Tests 

The damage mode observed in cylinder compression tests depends upon the end conditions of 

the test, as schematically shown in Figure 12. These figures are reproduced from a text by Bazant 

and Planas.(9) Cylinders with fixed ends exhibit two diagonal bands of damage. Cylinders with 

one fixed end and one sliding end (with negligible friction) exhibit a single diagonal band of 

damage. Small cylinders tested with two sliding ends with negligible friction (well lubricated 

platens or brushes) may split axially. Supposedly, these end conditions do not resist axial 

splitting. In practice, an axial split is difficult to achieve during testing. 

Figure 12. Damage modes observed in cylinder compression tests as a function of 

end conditions. Source: CRC Press.(9)

Fixed End Conditions 

Cylinders with fixed ends (laterally constrained ends) were analyzed at three different mesh 

refinements, and all produced two diagonal bands of damage, consistent with schematic test 

results shown in Figure 12. Damage fringes from one refined mesh simulation are shown in 

Figure 13 at various simulation times and rotations. Note that the X-shaped damage bands appear 

as O-shaped bands when the cylinder is rotated 90 degrees along its axis. The calculation was 

run for 1.5 sec, during which time the 304.8-mm (12-inch) cylinder was compressed 3.81 mm 

(0.15 inches). Some views show damage on a slice through the midplane of the cylinder. Other 

views show damage on the outside of the cylinder. 
16 

Figure 13. The damage mode calculated for compression cylinders with fixed ends agrees with 

the X-shaped damage bands observed in tests. 
17 

Capped End Conditions 

Cylinders with steel end caps were also analyzed to determine the effect of frictional lateral end 

constraint on cylinder response. These calculations were performed because it is standard 

practice to cap cylinders during testing. Capping provides some lateral constraint. An example 

test cylinder, for the 46 MPa (6,672 lbf/inch2) concrete used in the beams impacted by bogie 

vehicles, is shown Figure 14. Each idealized end cap is 165.1 mm (6.5 inches) in diameter (12.7 

mm (0.5 inches) larger than the cylinders) and 12.7 mm (0.5 inches) in height. A contact surface 

is modeled between each end cap and the concrete cylinder using frictional coefficients ranging 

from 0.1 to 0.3. The contact surface type selected was 

*CONTACT_CONSTRAINT_NODES_TO_SURFACE using the soft contact option. The 

cylinder was loaded in compression by applying a constant axial velocity to the layer of nodes 

along the top of the top end cap. The bottom end cap was restrained from axial motion along the 

bottom layer of end cap nodes. A few sample calculations were performed to determine that 

compressing from one end of the capped cylinder gives approximately the same results as 

compressing from both ends. 

Figure 14. Concrete cylinder tested as part of the bogie vehicle impact test series. 

Five variations in boundary conditions were considered. They are: 

1. No nodal constraints on the end caps to prevent them from sliding or rotating. 

2. Constrain the bottom end cap from rotating and sliding. 

3. Constrain the bottom and top end caps from rotating and sliding. 

4. Constrain the bottom end cap from rotating and sliding and the top end cap from sliding. 

5. Constrain the bottom and top end caps from sliding (rotation allowed). 

Damage fringes from these five calculations are given in Figures 15–19. They indicate that the 

calculated damage mode depends on how the boundary conditions are modeled. 
18 

The first calculation without nodal constraints gives a distinct band of diagonal damage, as 

shown in Figure 15. However, further observation indicates that the capped cylinder is rotating 

about its longitudinal axis. To the eye, the rotation of the top cap is in sync with the rotation of 

the bottom cap (no relative rotation between the top and bottom caps). The top cap also slides 

laterally relative to the bottom cap. 

The second calculation was conducted by laterally constraining some nodes of the bottom cap to 

prevent the bottom cap from rotating. This constraint also prevents the bottom end cap from 

sliding laterally. No nodal constraints were applied to the top cap, so it is free to slide and rotate 

relative to the bottom cap. Results of this calculation are shown in Figure 16. This calculation 

also gives a distinct band of diagonal damage. The diagonal band of damage forms prior to 

noticeable sliding of the top cap. Relative sliding of the top and bottom caps becomes apparent 

as the calculation progresses, as shown. Rotation of the top cap relative to the bottom cap is not 

apparent. These end constraints produce damage similar to that shown in Figure 12 for one 

frictionless end, because the frictionless end if free to slide relative to the fixed end. 

 

 

Figure 15. A diagonal band of damage is calculated with frictional end constraints if both end 

caps are allowed to rotate and slide (no end cap constraints). 

 
19 

 

Figure 16. A diagonal band of damage is calculated with frictional end constraints if one end cap 

is allowed to rotate and slide relative to the other (bottom cap constrained from rotating 

 and sliding). 

The third calculation was conducted by preventing both the bottom and top end caps from 

rotating and sliding. This means that there is no relative rotation or relative sliding. This was 

accomplished by laterally constraining a few select nodes on each cap. Results of this calculation 

are shown in Figure 17. The damage mode calculated is initially two diagonal bands of damage, 

similar to the fixed end condition results. The difference between this calculation and the fixed 

end calculation is that this calculation allows for frictionally restricted lateral expansion at the 

cylinder ends, whereas the fixed end calculation allows no lateral expansion at the cylinder ends. 
20 

 

Figure 17. A double diagonal band of damage is initially calculated if both end caps are 

prevented from rotating and sliding (bottom and top caps constrained from rotating and sliding). 

The fourth calculation was conducted by constraining the bottom cap from rotating and sliding 

laterally and the top cap from sliding laterally. The top cap is free to rotate relative to the bottom 

cap. Damage fringes from this calculation are shown in Figure 18. Again, two diagonal bands of 

damage form initially. Although the bands of damage are evident on an axial slice through the 

midplane, they are less distinct when viewed from the outside of the cylinder. 

 

 

Figure 18. A double diagonal band of damage is initially calculated if one end cap is free to 

rotate (bottom cap restrained from rotating and sliding, top cap restrained from sliding). 
21 

The fifth calculation was conducted by constraining the bottom and top caps from sliding relative 

to one another, while allowing them to rotate. Initially, two diagonal bands of damage form, with 

one more prominent than the other, as shown in Figure 19. 

The calculations just discussed indicate that one diagonal band of damage forms if the end caps 

are allowed to slide relative to one another, whether or not relative rotation of the end caps 

occurs. Otherwise, double bands of damage form initially, followed by severe bulging and 

damage towards the cylinder midheight. These calculations demonstrate that the concrete model 

accurately predicts a diagonal damage mode when the end conditions are modeled appropriately. 

They also indicate that slight variations in the boundary conditions affect the damage mode 

predicted. 

The end caps calculations just discussed were all conducted with a 0.3 coefficient of friction 

(static and dynamic). Additional calculations conducted with a 0.1 coefficient of friction give 

similar results. Calculations conducted with a 0.01 coefficient of friction are discussed in the 

next section that reviews free or frictionless end conditions. 

 

Figure 19. A single diagonal band of damage initiates, but is not retained, if the cylinder is overconstrained (bottom and top caps restrained from sliding). 
22 

Contact Surface Type 

Use of additional contact surface types is discussed here to make users aware of issues 

surrounding the use of contact surfaces. Many of the previously discussed calculations with end 

caps were conducted with the *CONTACT_CONSTRAINT_NODES_TO_SURFACE interface. 

The CONSTRAINT option doesn’t allow separation between the concrete cylinder and end caps. 

A few calculations were also conducted with the *CONTACT_NODES_TO_SURFACE and 

*CONTACT_SURFACE_TO_SURFACE interfaces. These options allow separation between 

the concrete cylinder and end caps. 

The reason the *CONTACT_CONSTRAINT_NODES_TO_SURFACE interface was used in 

many calculations is because it did not result in any penetration between the concrete cylinder 

and end caps. Hence the axial displacement histories of the nodes on the end of the cylinder are 

the same as those on the caps. This makes post-processing easy, because the displacement 

history is readily calculated by scaling time by the applied nodal velocity. On the other hand, 

with most other contact surfaces and options selected, some penetration occurred between the 

cylinder and end caps, at least initially. 

Consider two calculations conducted with the *CONTACT_SURFACE_TO_SURFACE 

interface. SURFACE_TO_SURFACE interfaces commonly are used because it is easier to call 

out a surface than to list all the nodes that define the surface. This particular interface also allows 

the concrete to separate from the end caps, as needed. Boundary conditions are one bottom end 

cap that is constrained from rotation and sliding, and a top end cap that is free to rotate and slide. 

In one calculation, default scale factors with a value of 1 were used for the slave and master 

surfaces (SFS = 1). In the other calculation, the slave surface scale factor was increased from 1 to 

10 (SFS = 10). The diagonal damage band calculated with either of these scale factors (Figure 

20) is the similar to that calculated with the *CONTACT_CONSTRAINT interface (previously 

shown as Figure 16). 

Although the damage modes are similar, the stress-histories calculated with the SURFACE_ 

TO_SURFACE interface are different than that calculated with the CONSTRAINT option 

(Figure 21). One reason these stress-histories are different is because the end cap penetrates the 

concrete with the SURFACE_TO_SURFACE interface, but not with the CONSTRAINT 

interface, as shown in Figures 22 and 23. Nodes 1 and 8001 give the displacement histories at 

each end of the concrete cylinder. Nodes 9001 and 9501 give the displacement histories of the 

steel cap at the interface with the concrete cylinder. Nodes 18001 and 18501 give the 

displacement histories of the cap on the top and bottom free surfaces. The difference between the 

concrete displacements and end cap displacements is the amount of penetration present. 

Therefore, at a given time, the axial strain in the cylinder with penetration is less than that 

without penetration. The result is that the initial slopes of the stress histories are different, as 

previously shown in Figure 21. End cap penetration also occurs when the concrete material 

model is replaced with an elastic material model (Mat 1) of equivalent modulus (not shown). 

 
23 

Figure 20. Diagonal damage bands are calculated using the 

*CONTACT_AUTOMATIC_SURFACE_TO_SURFACE option, although the diagonal band 

location varies with scale factor. 

psi = 145.05 MPa 

Figure 21. Differences in initial slope are primarily due to differing amounts of contact surface 

penetration between the concrete cylinder and end caps. 
24 

mm = 0.039 inch

Figure 22. End cap versus concrete displacement with penetration (SFS = 1). 

 mm = 0.039 inch 

Figure 23. End cap versus concrete displacement with little penetration (SFS = 10). 
25 

Stress versus displacement is obtained from a cross plot of the concrete stress history with the 

concrete displacement history. One must take special care in extracting the correct displacement 

history. If penetration occurs, use of the end cap displacement histories would overestimate the 

compression of the concrete. The result is that the concrete elastic modulus would appear to be 

lower than the user-supplied input value. This is easily corrected by using nodal displacement 

histories at the ends of the concrete cylinder, rather than on the end caps, as shown in Figure 24. 

The relative displacement plotted is the difference between the nodal displacements at the ends 

of the concrete cylinder. Note that at any given time, the relative displacement calculated with 

the SURFACE_TO_SURFACE interface with SFS = 1 is less than that calculated with the 

CONSTRAINT interface. 

The corresponding stress versus displacement histories are shown in Figure 25. Note that with 

use of the correct concrete displacement history, two of the calculations are in good agreement. 

The exception is the calculation conducted with SFS = 10. The reason it is different is due to the 

presence of early time tensile damage, as discussed in the following paragraph. 

Different options are available to relieve penetration. One is the soft constraint option. This 

option is recommended for use when the materials on each side of the interface have different 

stiffness, like steel and concrete. This option relieves some, but not all, of the penetration. 

Another option is to increase the scale factor of the concrete (slave) surface by a factor of 10. 

This option successfully prevents penetration of the end caps into the concrete (Figure 23). As 

desired, a diagonal damage band forms. The only concern is that slight tensile damage initiates 

near the contact surface very early in time at 20 msec, before the time of peak strength at 400 to 

500 msec, as shown in Figure 26. This tensile damage is triggered by axial extension of the 

concrete in the vicinity of the contact surface. Such tensile damage has also been observed in 

some, but not all, of the calculations conducted with the *CONTACT_CONSTRAINT option. 

The early-time tensile damage lowers the stiffness of the concrete relative to that observed in 

calculations without early-time tensile damage, as previously shown in Figure 25. 

In summary, the contact surface parameters and interface type affect damage initiation in these 

cylinder compression calculations. This effect appears to be due to the presence of early time 

tensile damage in the vicinity of the contact surface. In some calculations, this early time damage 

results in an accumulation of damage near one end of the cylinder. In other calculations, single 

and double bands of damage form, as desired. When creating stress-displacement curves, the 

displacement at the ends of the cylinder should be used to get the right modulus, if penetration 

between the end caps and concrete cylinder occurs. 
26 

mm = 0.039 inch

Figure 24. The relative displacement between the ends of the concrete cylinder depends on the 

amount of interface penetration present. 
27 

psi = 145.05 MPa, mm = 0.039 inch 

Figure 25. The stress-displacement histories are in reasonable agreement if the relative 

displacement of the cylinder is used. 

 

Figure 26. Early time tensile damage occurs in some compressive cylinder calculations in the 

vicinity of the contact surface interface. 

29 

CHAPTER 4. REGULATION OF SOFTENING FORMULATION 

One desirable attribute of the finite element method is convergence of the solution with 

reasonable mesh refinement. However, finite element solutions are known to have difficulty 

converging if the materials being modeled contain softening formulations. With softening 

formulations, there is a tendency for the greatest amount of damage to accumulate in the smallest 

elements. This is the result of modeling smaller fracture energy in the smaller elements. To 

overcome this tendency, a regulatory method was implemented to promote convergence by 

eliminating element-to-element variation in fracture energy. Refer to this report’s companion 

Users Manual for a theoretical discussion of the regulatory technique implemented.(6) This 

chapter demonstrates convergence of results using the regulatory technique implemented for 

both single element and single material simulations. 

SINGLE ELEMENTS IN TENSION AND COMPRESSION 

Calculations were performed with single elements as a first step in evaluating mesh objectivity of 

the softening response. Calculations were performed for four cube sizes: 12.7 mm (0.5 inches), 

38.1 mm (1.5 inches), 76.2 mm (3 inches), and 152.4 mm (6 inches) on each side. Each cube is 

modeled with quarter symmetry using nodal boundary conditions. Two loading conditions are 

analyzed. These are direct pull (uniaxial tensile stress) and unconfined compression (uniaxial 

compression stress). In each case, a uniform constant velocity is applied to the four nodes at one 

end of the element, while the four nodes at the other end are restrained from axial motion (lateral 

motion is not restrained). The velocity is 2.54 millimeters per second (mm/sec) (0.1 inch per 

second (inch/sec)) and is held constant for the duration of the simulations. 

Stress-displacement curves for the direct pull simulations are shown in Figures 27 and 28. All 

elements exhibit linear elastic behavior to peak strength, followed by softening. The strength is 

independent of element size, although the displacement at peak strength increases with 

increasing element size. If stress-strain rather than stress-displacement were plotted (not shown), 

then all elements would peak at the same strain level (as expected). 

Shifted stress-displacement results are shown in Figures 27 and 28. The curves are shifted by 

subtracting the displacement at peak stress from the displacement history. With such 

manipulation, the peak stress of each curve is plotted at a shifted displacement of 0. Plotted in 

this manner, the softening portion is identical for each curve, as desired. Hence the fracture 

energy (area under the softening portion of the stress-displacement curve) is constant from one 

element to another. These simulations demonstrate that the element-based softening theory is 

accurate and implemented without any coding errors. 

Stress-displacement results for the unconfined compression simulations are shown in Figures 29 

and 30. Once shifted, the softening portions of the four stress-displacement curves are close to, 

but not exactly equal to, each other. Careful checking of these results indicates that all four 

curves have the same fracture energy, but not the same shape. Note that all four curves have a 

point of agreement around 0.25 mm (0.01 inches) of displacement. For displacements less than 
30 

0.25 mm (0.01 inches), the smaller elements soften more rapidly than the larger elements. For 

displacements greater than 0.25 mm (0.01 inches), the smaller elements soften less rapidly than 

the larger elements. The overall result is consistent fracture energy from element to element. 

psi = 145.05 MPa, mm = 0.039 inch

Figure 27. The fracture energy, which is the area under the softening portion of the stressdisplacement curve, is independent of element size in the direct pull simulations (not shifted). 

psi = 145.05 MPa, mm = 0.039 inch 

Figure 28. The fracture energy, which is the area under the softening portion of the stressdisplacement curve, is independent of element size in the direct pull simulations (shifted to 

displacement at peak stress). 
31 

psi = 145.05 MPa, mm = 0.039 inch

Figure 29. Although the fracture energy is constant, the softening curves vary slightly with 

element size in the unconfined compression simulations (not shifted). 

psi = 145.05 MPa, mm = 0.039 inch

Figure 30. Although the fracture energy is constant, the softening curves vary slightly with 

element size in the unconfined compression simulations (shifted to displacement at peak stress). 
32 

These results indicate that in compression, the regulatory method allows small differences in 

softening behavior to occur as a function of element size. However, the author suggests that the 

regulation is adequate despite these small differences. Figure 29 and 30 show that the largest 

and smallest elements vary in size by a factor of 12. This variation in element size is much larger 

than that typically meshed by most analysts. Within a region of interest, a factor of 2 variations 

in element size is typical. The 38.1-mm (1.5-inch) and 76.2-mm (3-inch) elements in Figures 29 

and 30 vary in size by a factor of 2, and their difference in softening response is minimal. 

CYLINDERS IN TENSION AND COMPRESSION 

The objective of this chapter is to demonstrate mesh size sensitivity, and its regulation, for direct 

pull and unconfined compression of a concrete cylinder. This chapter begins with a description 

of each mesh used in the calculations, followed by results of calculations performed without 

regulation of the softening formulation. In general, these calculations do not converge to a 

unique solution and therefore demonstrate mesh size sensitivity, which is undesirable. This 

demonstration is followed by a theoretical discussion of softening formulations, with and without 

regulation. The chapter then discusses the results of calculations performed with regulation. The 

direct pull simulations demonstrate convergence to a unique solution with reasonable mesh 

refinement. The unconfined compression calculations tend toward convergence, but do not 

actually converge. Finally, conclusions are drawn concerning application of the technique 

implemented for regulating convergence of material models containing softening formulations. 

Details of Each Cylinder Mesh 

The specimen analyzed is a concrete cylinder that is 304.8 mm (12 inches) long and 152.4 mm (6 

inches) in diameter. This simple structure is being analyzed because it isolates one softening 

material model of interest, without interaction with other materials or complications from 

detailed boundary conditions or contact surfaces. 

Cylinders of two mesh refinements are analyzed, as shown in Figure 31. The basic mesh contains 

768 solid elements. This mesh refinement is intended to be typical of what most users would 

generate to simulate a cylinder test. The more refined mesh contains 2,592 solid elements. This 

mesh is more refined than what most users would generate. In addition, one single element and a 

two element mesh are analyzed. The single element is 304.8 mm (12 inches) long and 135.1 mm 

(5.32 inches) along each edge of the square cross section, in such manner that the volume of the 

single element is equal to the volume of the cylinder. Each element of the two element mesh is 

152.4 mm (6 inches) long, with a 135.1 mm (5.32 inches) by 135.1 mm (5.32 inches) 

cross section. 

Two loading conditions are analyzed. These are direct pull (uniaxial tensile stress) and 

unconfined compression (uniaxial compression stress). In each case, a uniform constant velocity 

is applied to the nodes at both ends of the cylinder. The velocity is 1.27 mm/sec. It is held 

constant for the 40 msec duration of the direct pull simulations and for the 1,500 msec duration 

of the unconfined compression simulations. 
33 

One boundary condition is analyzed for direct pull of the cylinders. The boundary condition is no 

lateral constraint on the ends of the cylinder so that the cylinder is free to expand or contract 

laterally along its entire length. This idealized condition produces a realistic damage mode 

(breaking of the cylinder along one band of elements). 

One boundary condition is analyzed for the unconfined compression cylinder. The boundary 

condition is a fixed end condition (no lateral motion of the nodes along the top and bottom of the 

cylinder). This condition produces a realistic double diagonal-type damage mode often seen in 

tests. 

 

Figure 31. Refinement of each mesh used in sensitivity analyses. 

Demonstration of Mesh Size Sensitivity 

Direct Pull without Regulation. Stress-displacement curves and damage fringes for the direct 

pull simulations without regulation are given in Figures 32 and 33. The stress history for the 

single and double elements is output directly from LS-POST. The stress history for the cylinders 

is obtained from the cross-sectional force history that is output from LS-POST. The cross section 

is located at the axial midplane of the cylinder. The stress is calculated by dividing the force 

history by the initial cross-sectional area of the cylinder (which is 719.2 millimeters square 

(mm2

) (28.3 inches square (inches2)). Each displacement history is output by LS-POST at the end 

nodes. 
34 

Figure 32 demonstrates that the softening response becomes more and more brittle as the mesh is 

refined. In particular, the stress-displacement behavior for the basic mesh does not converge to 

that of the refined mesh. This situation is undesirable. The damage modes for the basic mesh and 

refined mesh (see Figure 33) are similar, although they appear to be different at first glance. 

Damage is localized into a single row of elements that soften as they stretch. The row of 

elements is at one end of the refined mesh, but more toward the center of the basic mesh. 

Parametric studies (not shown) indicate that the row of elements that damages is sensitive to the 

rate of loading. The rate of loading affects the uniformity of the stress distribution along the 

length of the cylinder. The rate of loading used in these calculations (quasi-static at 1.27 mm/sec 

(0.05 inch/sec) is slow enough that the stress distribution is uniform at peak strength to within 

about .001 of 1 percent. With a top-to-bottom uniform mesh, loading, and stress distribution, 

fracture is likely to occur anywhere along the length of the cylinder, and not necessarily at the 

center of the cylinder. However, the addition of friction at each end of the cylinder would 

probably push damage more toward the center of the cylinder. 

For the single element mesh, the damage mode is softening of the entire element. For the double 

element mesh, very slight damage initiates simultaneously in both elements. But then damage in 

one of the two elements rapidly dominates, resulting in the softening and stretching of that one 

element, while the other remains effectively undamaged. 

All direct pull calculations were conducted with the user-defined material model for concrete 

linked to version 970, using softening parameters of A = 0.2467 and B = 0.1 in tension (P < 0) 

and A = 1.058 and B = 100 in compression (P > 0). These parameters are more fully described in 

the next section. 

psi = 145.05 MPa, mm = 0.039 inch

Figure 32. The stress-displacement curves calculated in direct pull with an unregulated softening 

formulation do not converge as the mesh is refined. 
35 

Figure 33. The damage mode calculated in direct pull with an unregulated softening formulation 

is damage within a single band of elements. 

Unconfined Compression without Regulation. Stress-displacement curves and damage fringes 

for these fixed end unconfined compression simulations without regulation are given in Figures 

34 and 35. The softening response tends to become more brittle as the mesh is refined. However, 

lack of convergence is not nearly as pronounced as previously demonstrated in Figure 32 for the 

direct pull simulations. In fact, the stress-displacement behavior for the basic mesh resembles 

that of the refined mesh. The author of this report considers the agreement between the basic and 

refined mesh curves as acceptable. 

In addition, note that the single element does not damage. With fixed end conditions, the single 

element simulates uniaxial strain response, not uniaxial stress response. Therefore, this 

simulation displays hardening behavior (pushes the cap out without triggering damage) that is 

typically seen in tests of concrete under uniaxial strain conditions. The single element with fixed 

ends is a very poor representation of a cylinder with fixed ends. 

As seen in Figure 35, the damage mode for the basic mesh and refined mesh is similar. Damage 

is primarily localized into two diagonals, forming an X-shape. This damage is in agreement with 

the double diagonal damage mode commonly observed in compression tests with fixed ends. For 

the double element mesh, both elements damage almost simultaneously and equally. 
36 

psi = 145.05 MPa, mm = 0.039 inch 

Figure 34. The stress-displacement curves calculated in unconfined compression with an 

unregulated softening formulation are similar for the basic and refined meshes (fixed ends). 

 Figure 35. The damage mode calculated in unconfined compression with an unregulated 

softening formulation is a double diagonal (in the basic and refined meshes with 

fixed end conditions). 
37 

Description of Regulatory Technique 

Softening is a reduction in strength with continued straining once a damage threshold is reached. 

Softening is modeled via a damage formulation. Without the damage formulation, most material 

models predict perfectly plastic behavior for laboratory test simulations like direct pull and 

unconfined compression. Such behavior is not realistic for materials like concrete, rock, soil, 

composites, and wood. 

Softening is modeled with two parameters. Without regulation of mesh size dependency, these 

parameters are A and B, and are independent of element size. With regulation, these parameters 

are B and Gf rather than A and B. When the damage threshold is attained, the concrete material 

model internally solves for the value of A based upon the initial element size, the initial damage 

threshold, the fracture energy Gf, and a user-specified input value for B. 

Evaluation of Regulatory Technique 

Direct Pull with Regulation. Stress-displacement curves and damage fringes for the direct pull 

simulations with regulation are given in Figures 36 and 37. Although the softening response 

becomes more brittle as the mesh is refined, convergence is attained for the basic and refined 

meshes, as desired. In addition, the damage modes for the basic mesh and refined mesh are also 

in agreement: both calculate fracture along a single band of elements. 

psi = 145.05 MPa, mm = 0.039 inch

Figure 36. The stress-displacement curves calculated in direct pull with a regulated softening 

formulation converge as the mesh is refined. 
38 

 

Figure 37. The damage modes calculated in direct pull with a regulated softening formulation are 

in agreement for the basic and refined mesh simulations. 

All direct pull calculations were conducted with the user-defined material model for concrete 

linked to version 970, using softening parameters of Gf = 0.098 megapascal-millimeters (MPamm) (0.56 pounds per inch (lb/inch)) and B = 0.1 in tension (P < 0) with Gf = 9.81 MPa-mm (56 

lb/inch) and B = 100 in compression (P > 0). 

Unconfined Compression with Regulation. Stress-displacement curves and damage fringes for 

these fixed end unconfined compression simulations with regulation are given in Figures 38 and 

39. The stress-displacement behavior for the refined mesh is nearly in agreement with that of the 

basic mesh, although the refined mesh is slightly more ductile. Greater ductility with mesh 

refinement is opposite the trend observed for the direct pull simulations. 

The damage mode for the basic and refined meshes (see Figure 39) is similar. Damage is roughly 

localized into two diagonals, forming an X-shape. However, the damage is less diffuse (more 

localized), forming a sharper X, for the refined mesh than it is for the basic mesh. This situation 

suggests that a correlation may exist between diffusivity and softening response: the more 

diffuse the damage, the more brittle the softening behavior. These results also suggest that 

additional mesh refinement is needed to attain complete convergence. 
39 

psi = 145.05 MPa, mm = 0.039 inch

Figure 38. The stress-displacement curves calculated in unconfined compression with a regulated 

softening formulation nearly converge as the mesh is refined (fixed ends). 

 

Figure 39. The X-shaped damage mode calculated in unconfined compression with a regulated 

softening formulation is similar for the basic and refined mesh simulations (fixed ends). 
40 

The argument could be made, however, that the basic and refined mesh simulations conducted 

without regulation (Figures 34 and 35) are in just as good agreement as those conducted with 

regulation (Figures 38 and 39). Hence, these simulations are inconclusive with regard to whether 

the proposed regulation scheme is necessary for the compressive response mode. 

Note also that regulation has an opposite effect on the softening response in tension than it does 

in compression. In tension, regulation increases brittleness as the mesh is refined, at least until 

convergence is attained. In compression, regulation decreases brittleness (increases ductility) as 

the mesh is refined, hopefully until convergence is attained. Hence, if an analysis is conducted 

with a mesh that is too crude, there may be a tendency to underpredict tensile damage and 

overpredict compressive damage. 

All unconfined compression calculations were conducted with concrete material model 159 in 

LS-DYNA version 971, using softening parameters of Gf = 0.098 MPa-mm (0.56 lb per inch 

(lb/inch)) and B = 0.1 in tension (P < 0) with Gf = 9.81 MPa-mm (56 lb/inch) and B = 100 in 

compression 

(P > 0). 

Effect of Additional Mesh Refinement on Cylinder Response 

A very refined mesh with 6,144 elements was created to further evaluate mesh size objectivity of 

the cylinder in compression. Refinement of this mesh is shown in Figure 40. Damage modes 

calculated with and without regulation are also shown in Figure 40. The calculations were 

conducted with fixed end conditions. Both calculations exhibit two diagonal bands of damage, 

forming an X. In the regulated calculation, these bands form simultaneously and about equally. 

In the unregulated calculation, one band forms prior to the other and exhibits greater damage. 

This X damage mode is the same as that previously calculated with less mesh refinement (768 

and 2,592 elements), except now the damage is more localized so that the bands are more 

distinct. 

Stress-displacement histories are shown in Figure 41 for all calculations without regulation and 

in Figure 42 for all calculations with regulation. Without regulation, the history calculated with 

the very refined mesh is more brittle than those calculated with less mesh refinement. With 

regulation, the history calculated with the very refined mesh is slightly more ductile than those 

calculated with less mesh refinement. Agreement is reasonable, but not exact. 
41 

 

Figure 40. A crisp X-shaped band of damage is calculated for the very refined mesh, with or 

without regulation of the softening response. 
42 

psi = 145.05 MPa, mm = 0.039 inch

Figure 41. The stress-displacement curves calculated in unconfined compression without a 

regulated softening formulation become more brittle as the mesh is refined (fixed ends). 

psi = 145.05 MPa, mm = 0.039 inch

Figure 42. The stress-displacement curves calculated in unconfined compression with a regulated 

softening formulation become more ductile as the mesh is refined (fixed ends). 
43 

SUMMARY REGARDING REGULATION 

The direct pull calculations demonstrate that the technique implemented for regulating mesh size 

sensitivity achieves convergence of the solution with reasonable mesh refinement, as proposed. 

The direct pull calculations exercise the brittle damage mode only; therefore, this conclusion 

applies to the brittle damage mode only, and not the ductile damage mode. 

The unconfined compression calculations support the application of the proposed regulation 

technique for the ductile damage mode, but do not indicate that it is absolutely necessary. 

Convergence is reasonable, but not exact. The fixed end calculations produce a double diagonal 

(X-shaped) damage mode that becomes more localized (less diffuse) with mesh refinement. This 

damage mode is similar to that seen in cylinder tests. 

All calculations were performed for a single material without the use of contact surfaces or 

detailed boundary conditions. The appropriate element size to obtain convergence in more 

detailed applications may be problem dependent. 

Finally, as previously noted, regulation in tension increases brittleness, whereas regulation in 

compression decreases brittleness (as the mesh is refined), until convergence is attained. Hence, 

if an analysis is conducted with a mesh that is too crude, there will be a tendency to underpredict 

tensile damage and overpredict compressive damage. 

45 

CHAPTER 5. SIZE EFFECT 

Numerous articles in the literature, particularly those by Bazant, suggest that larger structures are 

softer than smaller structures.(9) This observation is schematically demonstrated in Figure 43. In 

general, a larger structure will be more brittle and have lower strength than a smaller, scaleddown structure. The larger structure will experience more damage than the smaller structure. The 

size effect is examined computationally by analyzing reinforced beams in four-point bending. 

Figure 43. Schematic of the size effect, as suggested by Bazant and Planas.(9)

The effect of size on computed response was analyzed for two geometrically similar beams: one 

at full scale and the other at 1⁄3-scale. The full-scale beam is 4,572 mm (180 inches) long, with a 

cross section 457.2 mm (18 inches) deep and 342.9 mm (13.5 inches) wide. Two #3 longitudinal 

rebars are modeled on the tension side using beam elements with nodes common to the concrete 

hex elements. The rebars are located 228.6 mm (9 inches) apart and 276.2 mm (10.9 inches) deep 

(from the compression face of the beam). The concrete and rebar dimensions are reduced 

correspondingly in the 1⁄3-scale beam. 

The beams are loaded in four-point bending, using nodal velocities to apply the load. The nodal 

velocity is 3,810 mm/sec (150 inches/sec) in the full-scale beam and 1,270 mm/sec (50 

inches/sec) in the 1⁄3-scale beam. These velocities are intended to be slow enough to produce 

quasi-static conditions in the beam (no wave propagation effects). Pinned supports are modeled 

using nodal constraints. No contact surfaces are modeled. The concrete material was modeled 

with rate effects properties turned off. The steel reinforcement is modeled with elastic material 

properties. 

The mesh of the concrete beam is shown in Figure 44. The full-scale and 1⁄3-scale beams are 

geometrically similar and are meshed with the same number of elements. The elements differ in 

length by a factor of 3. Only one mesh is shown, because the full-scale and 1⁄3-scale mesh 

refinements are identical. 
46 

 

Figure 44. Refinement of the concrete beam mesh used in the size effect analyses. 

Damage fringes and stress versus relative displacement curves, calculated with regulation of the 

softening formulation, are shown in Figures 45 and 46. The larger beam experiences 

substantially more damage, and softens with more brittleness, than the smaller beam. This result 

is consistent with the size effect. The nominal stress is the vertical reaction force divided by the 

beam cross-sectional area. The relative deflection is the midpoint beam deflection (u) divided by 

the beam depth (D). 
47 

Figure 45. The damage simulated in the full-scale beam is more severe than that simulated in the 

1⁄3-scale beam, which is consistent with the size effect. 
48 

psi = 145.05 MPa

Figure 46. The stress-deflection behavior of the full-scale beam is softer than that of the 1⁄3-scale 

beam, which is consistent with the size effect. 

It is interesting that the size effect is calculated when the softening response is regulated, but not 

when it is unregulated. Without regulation, the full and 1⁄3-scale beams exhibit the same amount 

of damage, as shown in Figure 47. In addition, the stress versus relative deflection behaviors are 

nearly the same. This similarity is because the strain distributions in the full and 1⁄3-scale beams 

are identical in the elastic regime and quite similar in the damage regime. The unregulated 

softening formulation keeps the softening stress versus strain consistent, regardless of size. 

Hence, damage is nearly equivalent because strain is nearly equivalent. But equivalent damage is 

not consistent with the size effect. 

On the other hand, the regulated softening formulation keeps the softening stress versus 

displacement (crack opening) consistent. Displacements in the full-scale beam are 3 times as 

large as those in the 1⁄3-scale beam. Hence, damage is more pronounced in the full-scale beam (as 

shown in Figure 48). 

One-third Scale 

Full Scale 
49 

Figure 47. Without regulation of the softening formulation, the damage simulated in the 

full-scale and 1⁄3-scale beams is nearly the same, which is inconsistent with the size effect. 

psi = 145.05 MPa

Figure 48. Without regulation of the softening formulation, the stress versus relative deflection 

curves of the full and 1⁄3-scale beams are nearly identical, which is inconsistent with the 

 size effect.

51 

CHAPTER 6. BEAM DROP TOWER IMPACT SIMULATIONS 

TEST DATA 

Forty-seven dynamic drop tower tests were conducted on 1⁄3-scale beams. Drop tower tests allow 

for dynamic testing of simple concrete structures in a controlled, well-documented environment. 

Scaling was necessary to perform the tests in the indoor drop tower facility. The beams are 

approximate scale models of typical bridge rails or posts. All testing procedures, tests results, 

and data reduction are documented in Oldani.(10) Figures of the test results and testing apparatus, 

shown in this section, are reproduced from that reference.

Three sets of beams were tested in dynamic, four-point bending: over-reinforced, 

under-reinforced, and plain concrete beams. Test matrices are given in Table 1–3. Calibration 

tests were conducted to determine the target impact kinetic energy at which the over-reinforced 

beams failed. Beam failure consisted of cracks running completely through the beam thickness, 

without pulverizing the beam. This target kinetic energy was held approximately constant 

throughout all tests while four combinations of impactor mass and velocity were tested. For all 

three types of tests, an increase in the impactor mass (with a corresponding reduction in impactor 

velocity) resulted in an increase in the beam deflection with deeper and wider cracks. The steel 

reinforcement did not break in any of the tests. 

Table 1. Over-reinforced beam test matrix. 

Mass Target Velocity Target Impact Energy No. of Tests kg (lb) m/sec (ft/sec) J (ft-lb)

4 14.5 (32) 10.8 (35.4) 850 (627) 

6 31.8 (70.1) 7.3 (24) 850 (627) 

6 47.9 (105.6) 6.0 (19.7) 850 (627) 

8 63.9 (140.9) 5.2 (17.1) 850 (627) 

Table 2. Under-reinforced beam test matrix. 

Mass Target Velocity Target Impact Energy No. of Tests kg (lb) m/sec (ft/sec) J (ft-lb)

2 14.5 (32) 10.6 (34.8) 822 (606) 

2 31.8 (70.1) 7.1 (23.3) 803 (592) 

2 47.9 (105.6) 5.8 (19) 778 (574) 

2 63.9 (140.9) 5.0 (16.4) 754 (556) 
52 

Table 3. Plain concrete beam test matrix. 

Mass Target Velocity Target Impact Energy No. of Tests kg (lb) m/sec (ft/sec) J (ft-lb)

2 14.5 (32) 10.6 (34.8) 822 (606) 

2 31.8 (70.1) 7.1 (23.3) 803 (592) 

2 47.9 (105.6) 5.8 (19) 778 (574) 

2 63.9 (140.9) 5.0 (16.4) 754 (556) 

The beams tested in these drop tower tests are intended to be approximate scale models of the 

beams tested in the bogie impact tests discussed in the next section. The 1,524-mm- (5-ft-) long 

beams are impacted by two steel 32-mm (0.10-ft) diameter cylinders spaced 203 mm (0.67 ft) 

apart, as schematically shown in Figure 49. The beams are supported on each end with 32-mm 

(0.10-ft) diameter cylinders. Tie-down straps are also placed around each beam at each end to 

prevent the beam from bouncing off the supports. 

mm = 0.039 inch

Figure 49. Sketch of four-point bend tests, showing dimensions in millimeters.(10)

The cross section of the beam is 152.4 mm (6 inches) wide and 114.3 mm (4.5 inches) deep in 

the loading direction. Two bars of longitudinal reinforcement are located 76.2 mm (3 inches) 

apart and 92.08 mm (3.63 inches) deep from the loading face. No shear reinforcement is 

included. For the over-reinforced beams, the reinforcements are 9.525 mm (0.375 inches) in 

diameter (size #3 rebar). For the under-reinforced beams, the reinforcements are 3.2 mm (0.13 

inches) in diameter (smooth cold-rolled steel rods). 

To provide basic material property data for the analyses, the quasi-static compressive strength of 

the concrete was measured via cylinder compression tests. The nominal compressive concrete 

strength averages about 28 MPa (4,061 lbf/inch2

). The quasi-static tensile strength was measured 

using splitting tensile tests. The nominal tensile strength ranges from 1.82 to 2.7 MPa (264 to 

392 lbf/inch2). The stress-displacement behavior of the rebar was also measured. The initial yield 
53 

strength of the steel reinforcement averages about 457 MPa (66,282 lbf/inch2), with an ultimate 

stress of about 614 MPa (89,053 lbf/inch2

). 

LS-DYNA SIMULATIONS 

All baseline calculations were conducted with default material properties for 28 MPa (4,061 

lbf/inch2) concrete with a 10-mm (0.39-inches) aggregate. The concrete is modeled with 170 hex 

elements along the length of the beam and 17 by 14 elements through the cross section. The 

reinforcement is modeled with beam elements with common nodes with the concrete hex 

elements. The steel impact and support cylinders are modeled with hex elements. 

In some calculations, the tie-down straps are modeled with truss elements to prevent the concrete 

beam from bouncing off of the steel supports. The majority of calculations were conducted 

during development of the concrete model while it was interfaced with LS-DYNA as a 

user-defined material. A few calculations were performed with the final version of concrete 

material model as MAT 159. 

Plain Beams 

Multi-element simulations of the plain concrete beams were analyzed to ensure that the concrete 

model accurately predicts the damage mode observed in the tests, without the complicating 

effects of the steel reinforcement. A total of eight tests were conducted on plain beams, with two 

tests for each of the four combinations of mass and velocity. Six of the eight specimens initially 

failed with two major cracks beneath the impactor points, as shown in Figure 50. This initial 

failure mode occurred for all four combinations of mass and velocity tested. The remaining two 

specimens initially failed with one major crack beneath one impactor point, as shown in Figure 

51. This initial failure mode occurred for one test conducted at 5 m/sec, (16.4 ft/sec) and another 

conducted at 5.8 m/sec (19.02 ft/sec). The beams do not rebound. They eventually hit the bottom 

of the test fixture. The final failure mode is breakage into three to five pieces, as shown in 

Figures 52 and 53. Four specimens broke into five pieces, three specimens broke into four 

pieces, and one specimen broke into three pieces. It is not clear to the developer whether the 

additional breakage occurs prior to, or because of, impact with the bottom of the text fixture. 

Figure 50. Six of the eight plain concrete specimens initially failed with two major cracks in the 

impact regime. 
54 

Figure 51. Two of the eight plain concrete specimens initially failed with one major crack in the 

impact regime. 

Figure 52. All plain concrete specimens impact the bottom of the test fixture. 

Figure 53. Four of the eight plain concrete specimens ultimately break into five pieces. 
55 

Four baseline calculations were conducted, one at each of the four mass-velocity combinations. 

The initial damage mode simulated in all four calculations is the formation of two major cracks 

on the tensile face of the beam. These cracks propagate toward the impactor points on the 

compressive face of the beam, ultimately splitting the beam into three distinct sections. The 

deformed configuration with damage fringes from one simulation is shown in Figure 54. The 

beam does not rebound. Additional breakage occurs as the calculations progress, as shown in 

Figures 55 and 56. In three of the four calculations, the beam broke into five pieces. In the other 

calculation, conducted at 5 m/sec (16.4 ft/sec), the beam broke into four pieces. Any additional 

damage that may have occurred due to impact with the bottom of the test fixture was not 

simulated, because the bottom of the test fixture was not modeled. 

Figure 54. The plain concrete beam initially breaks into three large pieces in all baseline 

calculations performed (shown at 12 msec for impact at 

5.8 m/sec (19.0 ft/sec)). 

 

Figure 55. The plain concrete beam ultimately breaks into five pieces in three of four 

calculations performed (shown at 26 msec for impact at 5.8 m/sec (19.0 ft/sec)). 

Figure 56. The plain concrete beam ultimately broke into four pieces in one of four calculations 

performed (shown at 26 msec for impact at 5.0 m/sec (16.4 ft/sec)). 

Overall, there is good agreement between the computed and measured damage mode. The 

damage mode simulated is the primary damage model measured in the tests, i.e., the initial 

formation of two cracks beneath the impactor points, followed by additional breakage into five 

pieces. No accelerometer measurements were made for comparison with computed deflection 

histories. 
56 

Occasionally, in preliminary calculations conducted during model development and parameter 

selection, the damage mode simulated was the initial formation of one crack beneath one 

impactor point. One preliminary result, which was conducted before completing the model and 

selecting default properties, is shown in Figure 57. This damage mode does not occur using the 

final default properties implemented for 28 MPa (4,061 lbf/inch2) concrete with 10-mm (0.4-

inch) aggregate, but may be possible to obtain with user-specified properties. 

Figure 57. This preliminary calculation demonstrates the formation of one primary crack. 

Reinforced Beams 

Multi-element simulations of the over-reinforced and under-reinforced beams were also 

performed with LS-DYNA. Over-reinforced beams are statically designed to have the concrete 

crush before the steel reinforcement yields. Under-reinforced beams are statically designed to 

have the steel reinforcement yield before the concrete crushes. Over-reinforced beams are more 

brittle than under-reinforced beams; thus, each type of beam exhibits different response modes. 

The combined concrete and reinforcement models used in the analyses accurately simulate the 

different response modes. 

Over-reinforced beam behavior is shown in Figure 58 for the post-test beam and in Figure 59 for 

the LS-DYNA simulation. Upon impact, in both the test and simulation, multiple cracks 

primarily initiate on the tensile face of the beam and propagate towards the compressive face. A 

listing of the primary cracks noted in the post-test specimen is given in Figure 59. Impact 

damage (crushing) is also visible beneath each impactor. The beam rebounds following peak 

deflection. 
57 

Figure 58. The over-reinforced concrete beam has localized tensile cracks and concrete crushing 

in the impactor regime (test 15 conducted at 5 m/sec (16.4 ft/sec)). 

Figure 59. The damage mode of the over-reinforced concrete beam at peak deflection is localized 

tensile cracks and concrete crushing in the impactor regime (shown at 16 msec for impact at 5 

m/sec (16.4 ft/sec)). 
58 

Table 4. Primary crack analysis of test 15 conducted at 5 m/sec (16.4 ft/sec). 

Crack 

# 

Position x 

(mm) 

Depth Front 

(mm) 

Depth 

Front 

percent 

Depth back 

(mm) 

Depth 

Back 

percent 

Opening 

Top/Bottom

1 460.375 9.525 8.333 12.700 11.111 Bottom 

2 673.100 114.300 100.000 114.300 100.000 Bottom 

3 763.588 101.600 88.889 101.600 88.889 Bottom 

4 835.025 114.300 100.000 114.300 100.000 Bottom 

5 855.663 95.250 83.333 114.300 100.000 Bottom 

6 949.325 95.250 83.333 88.900 77.778 Bottom 

7 1009.650 34.925 30.556 88.900 77.778 Bottom 

8 1168.400 63.500 55.556 50.800 44.444 Top 

One measured trend is that the cracks become deeper and wider with an increase in impactor 

mass, or correspondingly with a decrease in impactor velocity. This trend is evident in the 

calculations, as shown in Figure 60. This figure shows the damage from the calculation 

conducted at the highest impact velocity of 10.6 m/sec (34.8 ft/sec). Note that fewer damage 

fringes are present in the impact regime at 10.6 m/sec (34.8 ft/sec) than previously shown in 

Figure 59 at 5.0 m/sec (16.4 ft/sec). 

Figure 60. The simulated damage fringes for impact at 10.6 m/sec (34.8 ft/sec) are less extensive 

than those simulated at 5.0 m/sec (16.4 ft/sec). 

In three sets of the over-reinforced beam tests, an accelerometer attached to the impactor 

measures acceleration that is integrated to produce velocity and displacement histories. The 

measured displacement histories are shown in Figure 61. Peak deflections attained from 

integration of the accelerometer readings agree with those attained from the videos to within 

about 5 percent accuracy. Peak deflections attained from the videos are given in Table 5. They 

indicate that as the impactor mass increases, the measured beam deflection increases. This trend 

is accurately simulated by the concrete material model. All four calculations are shown in Figure 

61 for comparison with the test data. Good agreement is noted until just past peak deflection. 
59 

mm = 0.039 inch 

Figure 61. The measured displacement histories are accurately simulated by LS-DYNA concrete 

material model MAT 159. 

Table 5. Comparison of measured and computed deflections for the over-reinforced beams. 

Specimen 

Mass Velocity Measured Displacement Range

Calculated 

Displacement 

kg (lb) m/sec (ft/sec) mm (inches) mm (inches) 

14.5 (32) 10.8 (35.4) 16 (0.63) 18 (0.71) 

31.75 (70) 7.3 (24.0) 19–25 (0.75–0.98) 24 (0.94) 

47.86 (105.5) 6.0 (19.7) 22–27 (0.87–1.06) 28 (1.10) 

63.93 (141) 5.2 (17.1) 26–33 (1.02–1.3) 30 (1.18) 

 

The measured and computed results previously shown in Figure 61 are not plotted past 20 msec, 

even though the accelerometer gage measurements continued to record past 20 msec. This 

happens because the deflection histories obtained from integrating the accelerometer readings 

begin to differ from the behavior shown in the videos once peak deflection is attained. This 

difference is attributed to a loss in the accelerometer’s accuracy. Once peak deflection is 

attained, the impactor (upon which the accelerometer rests) separates from the beam. This 

separation greatly reduces the high amplitude, short duration acceleration experienced by the 

piezoelectric shock gage. Consequently, the gage is subjected only to the constant acceleration of 

gravity. The sensitivity of the gage is poor under constant acceleration conditions, and its 

response is a slow exponential decay according to the time constant of the gage. Such decay is 

shown in Figure 62. Here, the velocities histories are obtained by integrating the accelerometer 
60 

records. This decay is not present in the computed velocity histories. These computed histories 

were obtained from preliminary calculations conducted during the model’s development, before 

the default material properties were selected. This discussion indicates having redundant 

measurements (the videos) serves as a good check on accelerometer measurements. 

m/sec = 3.28 ft/sec 

Figure 62. The processed velocity histories drift once the impactor separates from the beam 

during rebound at about 17 msec. 

Under-reinforced beam behavior is shown in Figure 63 for one post-test beam specimen and in 

Figure 64 for the corresponding LS-DYNA simulation. In both the test and simulation, two 

major cracks initiate on the tensile face of the beam and propagate toward the compressive face, 

essentially splitting the concrete into three sections. Impact damage (crushing) is also visible 

beneath each impactor. Little rebound occurs, although the reinforcement does not break. The 

behavior shown is for the test and simulation conducted at 5.2 m/sec, (17.1 ft/sec) but it is typical 

of most test specimens and calculations. 

Half of the test specimens also exhibited smaller but visible cracks originating on the top of the 

beam. These cracks are located approximately halfway between each impactor and each end of 

the beam, as shown in Figure 65 and listed in Table 6. The computed behavior previously shown 

in Figure 64 exhibits damage fringes, also originating on the top the beam, which are consistent 

with this behavior. 
61 

Figure 63. The damage mode measured for half of the under-reinforced beam specimens is two 

major cracks beneath the impactor points, without rebar breakage. 

Figure 64. The damage mode simulated for all under-reinforced beam specimens is two major 

cracks beneath the impactor points, with additional damage toward the ends of the beam. 

Figure 65. About half of the under-reinforced beam specimens exhibited cracks originating on 

the top of the specimen, and located halfway between the impactor points and ends of the beam.
62 

Table 6. Crack analysis for one under-reinforced beam tested with an impactor mass 

of 31.75 kg (70 lb). 

Crack Position x Depth Front Depth Back 

# mm (inches) mm (inches) 

Depth 

Front 

(%) mm (inches) 

Depth 

Back 

(%) 

Opening 

Top/ 

Bottom 

1 349.250 (13.75) 114.300 (4.5) 100.000 114.300 (4.5) 100.000 T 

2 660.400 (26) 114.300 (4.5) 100.000 114.300 (4.5) 100.000 B 

3 863.600 (34) 114.300 (4.5) 100.000 114.300 (4.5) 100.000 B 

4 1,168.400 (46) 114.300 (4.5) 100.000 114.300 (4.5) 100.000 T 

No accelerometer measurements were made for the under-reinforced beams, so deflection 

histories are not available for plotting. However, peak deflections were extracted from the 

videos, as listed in Table 7. Two sets of deflections are listed. One, labeled “mid,” gives the peak 

deflection measured at the horizontal midpoint of the beam. The other, labeled “max,” gives the 

maximum deflection measured, which is not necessarily located at the midpoint of the beam. 

Although the beam is symmetric in design, the deformation doesn’t remain symmetric once 

damage initiates. Also, the velocities listed are those used in the calculations, which differ by up 

to 7 percent from the actual velocities attained in the tests. 

Table 7. Comparison of measured and computed deflections for the under-reinforced beams. 

Specimen Tests Calculations 

Mass Velocity Mid Max Mid Max 

kg (lb) (m/sec) (ft/sec) mm (inches) mm (inches) mm (inches) mm (inches) 

81 (3.2) 88 (3.5) 14.5 (32) 10.8 (35.4) 106 (4.2) 113 (4.4) 98 (3.9) 98 (3.9) 

136 (5.4) 146 (5.7) 31.75 (70) 7.3 (24) 144 (5.7) 150 (5.9) 132 (5.2) 132 (5.2) 

184 (7.2) 200 (7.9) 47.86 (106) 6.0 (19.7) 200 (7.9) >230 (>9.1) 154 (6.1) 154 (6.1) 

229 – >230 – 63.93 (141) 5.2 – 222 – >230 – 167 – 167 –

 

The computed deflections underestimate the measured deflections for the calculations conducted 

at the two lowest impact velocities of 5.2 and 6.0 m/sec (17.1 and 19.7 ft/sec). Parametric studies 

were conducted to determine what changes in boundary conditions, concrete properties, or rod 

reinforcement properties would improve the correlations. Changes in boundary conditions 

(strapped ends, free ends, nodal constraints on ends) and concrete properties (27 MPa to 31 MPa 

(3,916 to 4,496 lbf/inch2

) concrete) changed the peak deflection by less than 4 percent. However, 

changes in the steel rod properties proved significant. For example, removing rate effects from 

the rod model increased the peak deflections by nearly 50 percent. Changing the material model 

from MAT_PIECEWISE_LINEAR_PLASTICITY to MAT_PLASTIC_KINEMATIC reduced 

deflections by about 5 percent. Changing the rod yield strength from 476 MPa to 620 MPa 

(69,038 to 89,923 lbf/inch2

) reduced the deflections by about 20 percent. Hence, the controlling 

issue is the rod material model and its parameters. 
63 

In addition, the smooth rods used in the tests are not ribbed like rebar and slide relative to the 

concrete. During the calibration tests, the rods slipped and did not yield. Therefore, vise grips 

were clamped at both ends of the exposed rods to prevent them from pulling into the concrete 

specimen, although some slippage still occurred during the tests. This slippage is not modeled in 

the finite element model. The rods in the under-reinforced specimens are modeled identical to 

those in the over-reinforced specimens, with common nodes between the concrete hex elements 

and steel beam elements. This method models a stronger bond between the concrete and 

reinforcement than occurs during the tests. Additional efforts to model slippage might include 

separating the steel beam nodes from the concrete hex nodes, then coupling the steel to the 

concrete via the *CONSTRAINED_LAGRANGE_IN_SOLID command with frictionless 

sliding. 

No additional efforts were made to improve correlations for the under-reinforced beams because 

this type of effort would focus on the smooth rod model and not the concrete model, which is the 

focus of this effort. The use of smooth rods in place of rebar was necessary due to scaling of the 

test structure. Rebar, rather than smooth rods, is used in full-scale roadside safety structures; 

therefore, continued efforts to improve the rod model are beyond the scope of this effort. 

The peak deflections measured in the under-reinforced beam tests are about five times greater 

than those measured in the over-reinforced beam tests. Such differences in deflection are 

accurately simulated by the concrete and reinforcement models, as shown Figure 66 for the tests 

and simulations conducted at 7.3 m/sec (24 ft/sec). In this figure, one average displacement 

history (solid line) for the over-reinforced beams is compared with the corresponding LS-DYNA 

simulation (dashed line). The range in peak deflections extracted from the under-reinforced beam 

videos is also compared with the corresponding LS-DYNA simulation. 
64 

mm = 0.039 inch 

Figure 66. Good displacement history and peak deflection comparisons of LS-DYNA drop tower 

impact simulations with test data for plain and reinforced concrete beams. 

SUMMARY FOR DROP TOWER SIMULATIONS 

Dynamic impact testing of over-reinforced, under-reinforced, and plain concrete beams indicates 

that each type of beam experiences a distinct deflection history and damage mode. The concrete 

model simulates, with reasonable accuracy, these deflection histories and damage modes. Like 

the test data, the model predicts that the under-reinforced beams deflect roughly five to nine 

times more than the over-reinforced beams, with no rebound of the plain beams. In addition, an 

increase in the impactor mass results in an increased beam deflection for both sets of reinforced 

beams. The over-reinforced beams experience multiple but fine tensile cracks that propagate 

through the beam thickness, while preserving the continuity of the beam. On the other hand, the 

under-reinforced and plain specimens primarily failed with two large, wide cracks beneath the 

impactor points, which disrupt the continuity of the beam. 
65 

CHAPTER 7. BEAM BOGIE VEHICLE IMPACT SIMULATIONS 

TEST DATA 

Three dynamic bogie vehicle impact tests were conducted on full-scale beams as part of this 

project. The reinforced concrete beams were simply supported and designed with longitudinal 

tensile reinforcement only. The bogie was setup with an impact head to produce four-point 

bending, as schematically shown in Figure 67. The test setup is similar to a concrete bridge rail 

impact, yet significantly simplified in order to isolate the concrete behavior. All tests were 

conducted with a 2,186.9 kilograms (kg) (0.05 lb) vehicle at speeds of 8.6, 15.9, and 33.km/h 

(5.3, 9.9, and 21 mi/h)). Observed damage consisted of flexural type cracks with beam rebound 

at low impact speed to inclined shear cracks and beam breakage (no rebound) at high impact 

speed. All testing procedures, tests results, and data reduction are documented in Bielenberg.(11) 

Figures of the test results and testing apparatus, shown in this section, are also reproduced from 

that reference.

 

mm = 0.039 inch 

 

Figure 67. Schematic of bogie vehicle impacting reinforced concrete beam. 

The beam is 4,887 mm (192.4 inches) long with a rectangular cross section that is 203 mm (8 

inches) wide and 343 mm (13.5 inches) deep. The distance from the beam compression face to 

the single row of rebar is 279 mm (11 inches). The steel reinforcement is two No. 6 rebars (19-

mm (0.75-inch) diameter). 

Load Frame Load Frame 

304.8 

mm

4267.2

Vimpact

1828.8 mm

343 mm 

1828.8 mm 609.6 

mm

304.8 

mm 

4267.2 mm 
66 

The bogie head is fitted with two impact cylinders made of 76-mm (3-inch) diameter round bar 

stock. The beam reacts against two load frames, located near the ends of the beam, which are 

also fitted with 76-mm (3-inch) diameter round bar stock. The beam rests on two intermediate 

supports, placed between each impact cylinder and load frame. The beams are greased to reduce 

friction between the beam and support shelf, as shown in Figure 68. 

Test instrumentation included videos, high-speed film, gages, and post-test photographs. Videos 

of each test were taken from overhead and from the side. These videos were used to determine 

deflection histories in two of the three tests. High-speed film was also used to record the event 

and to generate high-resolution photographs for documentation. The concrete beams were 

instrumented with strain gages on the compressive face of the beam. Strain gages were also 

placed on the rebar, but were under-ranged and yielded little information. The load frames were 

instrumented with strain gages on the angled tube of each frame, as shown in Figure 68. The 

bogie was instrumented with an accelerometer near its center of mass. The accelerometer failed 

to trigger in one test and yielded different force history results than the load frame gages in the 

other two tests. Therefore, the accelerometer data were considered unusable by those who 

conducted the tests. 

Figure 68. The beam rests on greased supports and reacts against two load frames. 

To provide basic material property data for the analyses, the static compressive strength of the 

concrete was measured via cylinder compression tests. The nominal 40-day concrete 

compressive strength was 46 MPa (6,672 lbf/inch2) at the time tests were conducted. The tensile 

strength was not measured. The static yield and ultimate strength of the No. 6 Grade 60 rebar 
67 

was also measured in tension. The average initial yield strength was 462 MPa (67,007 lbf/inch2), 

and the ultimate strength was 721 MPa (104,572 lbf/inch2

). 

LS-DYNA CORRELATIONS 

All baseline calculations were conducted with default material properties for 46 MPa (6,672 

lbf/inch2) concrete with 19-mm (0.75-inch) aggregate. Unless otherwise stated, erosion was set 

to occur at 10 percent maximum principal strain. The concrete is modeled with 192 hex elements 

along the length of the beam, and 15 by 9 elements through the cross section. The reinforcement 

is modeled with beam elements with common nodes with the concrete hex elements. The steel 

impact and load frame cylinders are modeled with hex elements. In the calculations conducted at 

8.6 km/h (5.3 mi/h), the supports that the beam rests on are modeled as rigid planes, with low 

friction between the beam and planes. Unless otherwise stated, the final calculations reported 

here were conducted with concrete material model MAT 159 implemented into LS-DYNA beta 

version 971 revision 2582. 

High Velocity Impact 

Two deformed configurations for the high velocity impact test conducted at 33.1 km/h (20.5 

mi/h) are shown in Figure 69. Localized crushing from the cylinder heads occurs following 

impact on the compression face of the beam. Four diagonal shear cracks are visible in the 

photograph at 8 msec. The beam has broken into four or five major fragments by 48 msec, 

including a large trapezoidal-shaped block that forms along two of the inclined shear cracks. 

Bond failure along the steel reinforcement also is evident. 
68 

 

Figure 69. The beam tested at an impact velocity of 33.1 km/h (20.5 mi/h) exhibits inclined shear 

cracks, localized crushing, and bond failure. 

Three deformed configurations for the high velocity impact simulation conducted at 33.1 km/h 

(20.5 mi/h ) with baseline properties are shown in Figure 70. The deformed configuration of the 

high velocity simulation is localized crushing from the impact cylinders, inclined shear cracks 

originating on the compression face of the beam, plus peeling away of the concrete cover from 

the reinforcement on the tensile face of the beam (bond failure). The beam breaks into three 

major pieces. This damage is similar to that previously shown in Figure 69 for the corresponding 

test. Additional bond failure occurs in the simulation along the tensile face of the trapezoidal 

block that is not evident in the test. However, such centrally located bond failure is evident in the 

test conducted at 15.9 km/h (9.9 mi/h). 

 
69 

Figure 70. Inclined shear cracks, localized crushing, and bond failure are simulated in the 

calculation conducted at 33 km/h (20.5 mi/h). 

Intermediate Velocity Impact 

Two deformed configurations for the intermediate velocity impact test conducted at 15.9 km/h 

(9.9 mi/h) are shown in Figures 71 and 72. The failure mode is predominantly inclined shear 

cracking and bond failure along the tensile reinforcement, with localized crushing beneath the 

impact cylinders. The failure dominates the right side of the beam. Here, one large shear crack 

forms at about 42 msec on the compression face and propagates at-angle toward the 

reinforcement on the tensile side. The crack then propagates along the tensile reinforcement, 

resulting in bond failure. Smaller shear cracks also form on the left side of the beam. The beam 

and bogie do not rebound. 
70 

Figure 71. The beam tested at an impact velocity of 15.9 km/h (9.9 mi/h) exhibits inclined shear 

cracks, localized crushing, and bond failure. 

Figure 72. Damage dominates one side of the beam impacted at 15.9 km/h (9.9 mi/h). 

Three deformed configurations for the intermediate velocity impact simulation, conducted at 

15.9 km/h (9.9 mi/h) with baseline properties, are shown in Figure 73. The deformed 
71 

configurations exhibit slight localized damage from the impact cylinders, early time tensile 

damage, inclined shear damage, plus bond failure between the concrete and tensile 

reinforcement. Initially, tensile damage fringes and inclined shear fringes form in the vicinity of 

the impact cylinders (in the constant moment region), as shown at 8 msec. Additional inclined 

shear damage fringes form outside the constant moment region, as shown at 104 msec. 

Substantial bond failure is also evident at this time. The damage is similar to but less severe than 

that previously shown in Figure 71 for the corresponding test. One main difference between the 

simulation and test is that the beam rebounds at 104 msec in the simulation, but it did not 

rebound in the test. The second difference is that the damage is fairly symmetric from side to 

side in the simulation, but dominates one side of the beam in the test. The cause of the 

asymmetry in the test is not known. 

 

Figure 73. Tensile damage, inclined shear damage, and bond failure are simulated in the 

calculation conducted at 15.9 km/h (9.9 mi/h) with erosion set to 10 percent strain. 

One parametric study was conducted to determine the effect of impact velocity on the computed 

response. The impact velocity in the calculation just discussed was increased from 15.9 km/h 

(9.9 mi/h) to 18 km/h (11.2 mi/h). At 18 km/h (11.2 mi/h), fracture occurs through the thickness 

of the beam, along with substantial bond failure, as shown in Figure 74. The beam breaks into 

two major pieces. The beam and bogie do not rebound. The damage is qualitatively similar to 

that measured in the test, although less bond failure is evident. This study suggests that 15.9 

km/h (9.9 mi/h) is close to the impact velocity at which the bogie just breaks through the beam 

without rebound. 
72 

 

Figure 74. The beam breaks into two major pieces and does not rebound when 

impacted at 18 km/h (11.2 mi/h). 

Another parametric study was conducted to determine the effect of erosion on the computed 

response. In the baseline calculation previously discussed, erosion is set to occur at 10 percent 

maximum principal strain. Two additional calculations were conducted with erosion set to 5 

percent and 1 percent maximum principal strain. The strain value at which erosion occurs is an 

option set by the user. Erosion can only occur after damage exceeds 99 percent. 

Damage fringes for the calculation conducted with erosion set to 5 percent strain are similar to 

those calculated at 10 percent strain (not shown). The peak deflection attained before rebound is 

211 mm (8.3 inches), in agreement with that calculated at 10 percent strain. Damage fringes for 

the calculation conducted with erosion at 1 percent strain are shown in Figure 75. In this case, 

the erosion is more extensive than that calculated at 5 percent and 10 percent strain and breaks 

the beam into five major pieces. No rebound of the beam occurs. This computational comparison 

indicates that the erosion strain value affects the computed response, and lower erosion values 

tend to make the simulation more flexible. The developer has typically used 10 percent strain 

based on past experience. Numerous calculations throughout this report also use 5 percent strain. 
73 

 

 

Figure 75. This damage modeled at 15.9 km/h (9.9 mi/h) with erosion set to 1 percent strain is 

more extensive than when erosion is set to 10 percent strain. 

Low Velocity Impact 

Three deformed configurations for the low velocity impact test conducted at 8.6 km/h (5.3 mi/h) 

are shown in Figures 76 and 77. Slight damage occurs beneath each impact cylinder upon 

contact. Cracks form on the tensile face and propagate toward the compression face. The cracks 

are most dominant in the impact (constant moment) region and extend about two-thirds of the 

way through the beam before the beam rebounds. Smaller cracks are observed outside the 

constant moment region. The beam reaches a maximum deflection of about 70 mm (2.8 inches) 

at 60 msec, then it rebounds, pushing the bogie vehicle backwards. Additional cracking occurs 

following rebound during reverse bending. 
74 

The deformed configuration of the low velocity test is similar to that of the 1⁄3-scale tests of overreinforced concrete beams shown in the previous section. This similarity is because the drop 

tower test beams are approximate scaled versions of the bogie vehicle test beams. These beams 

exhibit substantial cracking, but retain their integrity and rebound. 

. 

Figure 76. Cracks form on the tensile face of the beam impacted at 8.6 km/h (5.3 mi/h) 

and propagate toward the compression face. 

Two deformed configurations for low velocity impact simulation conducted at 8.6 km/h 

(5.3 mi/h) with baseline properties are shown in Figure 78. Damage fringes form on the tensile 

face and are most dominate in the impact region. They extend about three-quarters of the way 

through the beam before the beam rebounds at about 64 msec. The peak deflection is 69 mm (2.7 

inches), which agrees with measurements in the tests. Substantial additional damage occurs 

during reverse bending following rebound. 
75 

Figure 77. The beam rebounds when impacted at 8.6 km/h (5.3 mi/h), pushing the 

bogie vehicle backward. 

 

Figure 78. The simulation of the beam impacted at 8.6 km/h (5.3 mi/h) exhibits 

substantial damage, but retains its integrity and rebounds. 
76 

Displacement Histories 

Displacement history comparisons are shown in Figure 79 for the low and high velocity tests and 

simulations. Solid lines represent the data; dashed lines represent the simulations. Histories for 

both the beam and bogie vehicle are given at low velocity, because the vehicle separates from the 

beam upon rebound. The simulations accurately calculate the displacement histories through 

rebound. Some discrepancy exists following rebound at low velocity, in which the simulated 

beam and vehicle rebound more significantly than during the test. A displacement history is not 

shown for the intermediate velocity test because the overhead camera did not function. 

 mm = 0.039 inch 

Figure 79. The displacement histories from the LS-DYNA bogie vehicle impact 

simulations compare well with the test data. 

One parametric study was conducted to determine the effect of modeling the four supports (load 

frame and intermediate) on the computed displacement history. Little effect is noted at high 

impact velocity. However, at low impact velocity, inclusion of the supports affects the rebound 

displacement history, as shown in Figure 80. Without modeling the supports, the beam impacted 

at 8.6 km/h (5.3 mi/h) rebounds, but to a greater extent than that measured in the tests. Better 

agreement with the tests is obtained if the supports are modeled. This agreement was 

accomplished by modeling the four supports as rigid planes. Dynamic relaxation was used to 

achieve contact between the beam and supports before impact. The computational a coefficient 
77 

of friction of 0.3. Gravity was applied to the beam. Results previously shown in Figures 78 and 

79 were conducted with the supports modeled. 

mm = 0.039 inch 

Figure 80. The calculations conducted at 8.6 km/h (5.3 mi/h) correlate best 

with the test data if the supports are modeled. 

Strain Histories 

Strain histories were measured on the concrete compressive face midway along the length of the 

beam. One gage was placed 32 mm (1.26 inches) above the centerline, the other 32 mm (1.26 

inches) below the centerline. Approximate peak values are 0.0025 and 0.0027 for test 2 at 33.1 

km/h (20.6 mi/h), 0.0021 and 0.0023 for test 1 at 15.9 km/h (9.9 mi/h), and 0.0023 for test 3 at 

8.6 km/h (5.3 mi/h). The three strain histories measured below the centerline are shown in Figure 

81. The strain histories measured above and below the centerline are similar (not shown). The 

peak strain attained is similar in each test and is approximately 0.23 percent. 

Strain histories calculated on the compressive face of the beam, just below the centerline, are 

shown in Figure 82. Histories calculated above and below the centerline are similar; therefore, 

only one history is shown. Unlike the measured histories, the calculated histories attain different 

peaks in each simulation. The peak strain is lowest for the high velocity impact simulation 

conducted at 33.1 km/h (20.6 mi/h). It is low because the beam breaks centrally into a large 

trapezoidal piece, and the compressive face of this piece bends less than during pure bending. 
78 

km/h = 0.621 mi/h 

Figure 81. Strain histories measured on the compressive face of each 

beam peak around 0.23 percent strain. 

km/h = 0.621 mi/h 

Figure 82. The strain histories from the LS-DYNA bogie vehicle 

impact simulations vary with impact velocity. 
79 

The peak strain attained for the low velocity simulation conducted at 8.6 km/h (5.3 mi/h) is 

approximately 0.21 percent, which is about twice that attained at high impact velocity. This 

beam retains its integrity during bending and then rebounds; thus, larger bending strains are 

calculated than at high impact velocity. The peak strain attained is similar to that measured at 

low impact velocity. However, the calculated strains go into tension at about 230 msec, while the 

measured strains remain compressive at about 0.058 percent for the duration of the recording to 

468 msec. It is unclear why the measurements remain compressive once the test beam rebounds 

and goes into reverse flexure at about 200 msec. 

The peak strain attained for the intermediate velocity simulations conducted at 15.9 km/h (9.9 

mi/h) is approximately 0.38 percent. In this simulation, the bending calculated between the two 

impact cylinder locations is significant, while little bending occurs between each impact cylinder 

and edge of the beam. The strains become tensile once the beam rebounds. 

These comparisons demonstrate how difficult it is to correlate strain measurements, even when 

good correlations are obtained for deformed configurations and deflections. The difficulty lies in 

the fact that strain histories are local behaviors that can vary significantly from position to 

position along the beam. 

SUMMARY FOR IMPACT SIMULATIONS 

The response of the three beams tested depends on the impact velocity. The computational model 

accurately simulates the substantially different displacement histories and damage modes 

measured between high (33.1 km/h (20.6 mi/h) and low (8.6 km/h (5.3 mi/h)) velocity impact. At 

high velocity impact, damage is dominated by inclined shear cracks, and the beam breaks into 

several large pieces without rebounding. At low velocity impact, tensile cracks form, but the 

beam retains its integrity and rebounds. 

At intermediate velocity (15 km/h (9.3 mi/h)), a combination of bending and shear was observed 

in the test. The beam ultimately failed on one side without rebounding due to large tensile and 

shear cracks. The simulation exhibited a more symmetric behavior with a combination of 

bending and shear cracks, but ultimately rebounded. However, the computed damage becomes 

similar to the measured damage, without rebound, if the impact velocity is increased from 15.9 

km/h (9.9 mi/h) to 18 km/h (11.2 mi/h). This suggests that the 15.9 km/h (9.9 mi/h) impact 

velocity tested is close to the velocity needed to transition from rebound to breakthrough. An 

additional parametric study indicates that reducing erosion strain from 5 percent to 1 percent also 

improves correlations by transitioning the simulation results from rebound to breakthrough. 

81 

CHAPTER 8. TEXAS T4 BRIDGE RAIL 

USER INTRODUCTION 

This chapter, parts of chapter 9, and appendix A present findings related to the evaluation of the 

concrete material model by a potential end user of the model. The evaluation consisted of a 

series of verification calculations and validation analyses using the LS-DYNA implementation of 

the concrete material model (MAT type 159 or MAT_CSCM). The user obtained a beta binaries 

release of LS-DYNA version 971 for the following platforms: Silicon Graphics, Inc. (SGI) 

IRIX® (version 971 release 1490 double precision ), MS-Windows (version 971 release 1612 

single precision), and Linux Intel 32 bit architecture (version 971 release 1708 single precision). 

Because LS-DYNA version 971 is a beta release, several releases of these binaries were added 

during the project period. The research team used the Linux Intel 32 bit architecture (version 971 

release 1708 single precision) release to maintain consistency and avoid potential software 

glitches associated with beta releases that occurred subsequent to the project’s initiation. 

The work plan followed in the model evaluation process consisted of two tasks. First, 

calculations were performed to establish that the executable of LS-DYNA obtained by the user 

gave the same results as the executable used by the developer. This was accomplished by 

reproducing five developer evaluation calculations using developer-supplied input files. The 

calculations included three concrete impact simulations that correlate with bogie impact tests of 

reinforced concrete beams, and two drop-tower simulations that correlate with drop-tower tests. 

Results of these calculations are given in appendix A. 

Second, the concrete material model was used in the impact analysis of a roadside safety 

structure in which some concrete failure was observed. The structure selected for analysis was 

the Texas T4 bridge rail. After the initial evaluation of the concrete material model, the roadside 

safety structure model was used in a parametric study to evaluate model sensitivity to variations 

in key material parameters. Results of calculations conducted by the user are given in this 

chapter . Additional support calculations conducted by the developer are given in appendix B. 

The user wanted to more fully evaluate the concrete material model in other roadside safety 

structures. Considerable test data exist for various bridge rail parapets, bridge decks supporting 

metal rails, and portable concrete barriers in which varying degrees of concrete damage and/or 

failure occurred. However, the resources allocated for the evaluation and validation effort were 

not sufficient to support additional model development and analyses. A model of a safety-shape 

bridge rail with New Jersey profile was developed under this research effort. Data available for 

this bridge rail included quasi-static load tests to failure and two full-scale vehicular crash tests. 

Although some preliminary calculations were performed on this model, project resources were 

depleted before the structure could be fully analyzed by the user. Preliminary calculations 

performed by both the user and developer are discussed in chapter 9. 
82 

OVERVIEW 

This task involved modeling and analyzing a roadside safety structure made of concrete and 

using the results to help define the applicability of the concrete material model to the analysis 

and design of concrete roadside safety structures. The structure selected for analysis was the 

Texas Type T4 bridge rail. 

Two different design variations of the T4 rail were evaluated through dynamic pendulum testing 

under a previous research study.(12) Using these tests for evaluation of the concrete model has 

several benefits. First, the tests provide an opportunity to assess the concrete model in a roadside 

safety application. Second, use of the pendulum bogie makes the tests more controlled and 

eliminates the variability associated with full-scale vehicles. Third, two specimens were tested 

for each design variation, which provides some information about system variability. Finally, the 

two design variations demonstrated different levels of damage and, therefore, provide the ability 

to assess sensitivity of the concrete model to small design changes under similar loading 

conditions. 

PENDULUM TESTING 

The T4 railing consists of a 381-mm- (15-inch-) tall metal rail anchored to the top of a 457.2-

mm- (18-inch-) tall concrete parapet wall, providing an overall rail height of 838.2 mm (33 

inches). The metal rail consists of a short section of an elliptically shaped steel tube welded atop 

a post fabricated from steel plate. The steel post is welded to a steel base plate that is anchored to 

the concrete parapet. 

In one design variation, the width of the steel-reinforced concrete parapet is 254 mm (10-inch), 

and the steel rail is attached to the parapet using four 22.2-mm- (0.087-inch-) diameter anchors. 

In the second variation, the width of the concrete parapet is 317.5 mm (12.5 inches), and the steel 

rail is attached to the parapet using three 22.2-mm- (0.087-inch-) diameter anchors. Vertical 

reinforcement in the parapets consisted of #5 V bars spaced 266.7 mm (10.5 inches) apart. 

Longitudinal reinforcement in the parapets consisted of two #5 bars equally spaced at the top of 

each parapet and within the V bars. 

Detailed drawings of the bridge rail specimens are shown in Figures 83 and 84 for the 

254-mm- (10-inch-) and 317.5-mm- (12.5-inch-) wide parapet designs, respectively. A 

photograph of a test specimen with a 254-mm- (10-inch-) wide parapet is shown in Figure 85; a 

photograph of the test installation with a 317.5-mm- (12.5-inch-) wide parapet is shown in 

Figure 86. 

To simulate the actual connection of the rail system to a bridge, each parapet was constructed on 

top of a 203.2-mm- (8-inch-) thick steel-reinforced concrete bridge deck that was cantilevered 

off a concrete beam a distance of 736.5 mm (29 inches). Transverse reinforcement in the deck 

cantilevers consisted of two layers of #5 bars located 152.4 mm (6 inches) apart. Longitudinal 

reinforcement in the top layer of each deck consisted of #4 bars located 228.6 mm (9 inches) 

apart. Longitudinal reinforcement in the bottom layer of the deck cantilevers consisted of two #5 

bars located near the field side edge spaced approximately 76.2 mm (3 inches) apart with the 
83 

next adjacent bar located 304.8 mm (12 inches) away. Average concrete compressive strengths 

for the decks and parapets were determined on the day of testing to be: 

• 35.50 MPa (5,149 lbf/inch2

) for the decks for all tests. 

• 30.44 MPa (4,415 lbf/inch2

) for the parapets for all tests. 

TEST RESULTS 

Testing was conducted with a gravitational pendulum equipped with a crushable nose assembly. 

The pendulum bogie was built in accordance with the specifications of the Federal Outdoor 

Impact Laboratory’s (FOIL) pendulum. The crushable nose assembly is the FOIL 10-stage 

honeycomb nose that uses expendable aluminum honeycomb material of differing densities in a 

sliding frame structure. Frontal crush stiffness of the staged nose assembly is calibrated to 

represent the frontal crush stiffness of a small passenger car. The pendulum body was 

instrumented with an accelerometer. The mass of the instrumented pendulum bogie was 838 kg 

(1,848 lb), and it was raised to a height sufficient to achieve an impact speed of 9,835 mm/sec, 

(387.2 inches/sec), which is 35.4 km/h (22 mi/h)). The nose of the pendulum bogie contacted the 

elliptical tube on the steel rail portion of the system. The impact loads were transferred to the 

concrete parapet and deck through the steel rail. 

For each design variation of the T4 bridge rail, two identical specimens were constructed and 

tested. For the design variation with the 254-mm- (10 inch-) wide parapet, the test designations 

were P3 and P4. For the design variation with the 317.5-mm- (12.5-inch-) wide parapet, the test 

designations were P5 and P7. 

The observed failure mode in tests P3 and P4 was punching shear failure of the field side of the 

concrete parapet due to load applied through the anchor bolts and base plate. In each test, the 

impact forces caused the concrete to fracture and spall off the field side of the parapet. In 

addition, cracks in the top of the concrete parapet radiated outward from the outside anchor bolts 

of the base plate and pieces of concrete were pushed out on the field side of the parapet. Damage 

to the test specimen with a 254-mm- (10 inch-) wide parapet after test P3 is shown in Figure 87. 

Post-test damage from test P4 is shown in Figure 88. 
.

mm = 0.039 inch 

Figure 83. Details of T4 rail with four-bolt anchorage and 254-mm- (10-inch-) wide parape

84 
.

mm = 0.039 inch 

Figure 84. Details of T4 rail with three-bolt anchorage and 317.5-mm- (12.5-inch-) wide parap

85 
86 

Figure 85. Parapet before test P3.

Figure 86. Parapet before test P5. 
87 

Figure 87. Parapet damage after test P3. 

Figure 88. Parapet damage after test P4. 
88 

In test P5, a T4 rail with three-bolt anchorage design and a 317.5-mm- (12.5-inch-) wide parapet 

was evaluated. The pendulum impact caused no visible damage to the concrete parapet or deck. 

Damage to the test specimen with a 317.5-mm- (12.5-inch-) wide parapet after test P5 is shown 

in Figures 89 and 90. The same parapet was tested again (test P6) with different staging of the 

pendulum nose assembly. The impact caused small cracks to be formed in the concrete parapet. 

The cracks radiated out at an angle from the anchor bolts on the top of the parapet and continued 

at an angle down the field side of the parapet into the bridge deck. 

The second test specimen with 317.5-mm- (12.5-inch-) wide parapet was evaluated in test P7. 

The impact conditions and pendulum configuration were the same as those used in tests P3, P4, 

and P5. The impact forces imparted by the pendulum caused the formation of thin hairline cracks 

in the top of the concrete parapet that radiated out from the anchor bolts of the base plate and 

down the field side of the parapet into the bridge deck. Post-test damage from test P7 is shown in 

Figure 91. 

SIMULATION METHODOLOGY 

The methodology followed to model the bridge parapets, simulate pendulum impacts, and 

evaluate the concrete material model consisted of the following steps: 

1. Modify, optimize, and calibrate the crushable nose pendulum model. 

2. Construct finite element model of the two variants of the T4 rail system. 

3. Incorporate the new concrete material model for concrete parts (e.g., parapet and bridge 

deck). 

4. Identify critical parameters of the model and investigate the performance of the model 

through finite element analysis. 

5. Compare results with test data and identify any further investigation needed. 

PENDULUM MODEL CALIBRATION 

To simulate the test conditions described here, it is critical to have an accurate representation of 

the impacting device. A model of the FOIL pendulum with crushable honeycomb nose assembly 

was obtained from NCAC. The internal honeycomb cartridges and spacers comprising the nose 

of the pendulum (see Figure 92) were replaced with a single nonlinear spring as shown in Figure 

93. The external honeycomb cartridge on the leading edge of the nose assembly was maintained 

in the model. However, its density was increased to account for mass of the removed cartridges. 

Previous experience with the original model with honeycomb nose required runtimes of around 8 

central processing unit hours on a mainframe computer to complete a calibration run with the 

pendulum impacting a rigid pole. The modified pendulum model requires only 15 minutes on a 

personal computer for a similar problem. The spring-based pendulum (SBP) model was 

calibrated using a test of the pendulum impacting a rigid pole. The stiffness values of the 

nonlinear spring were iteratively adjusted until the force-time history obtained from the SBP 

model closely matched data measured in the rigid pole test.(13)
89 

Figure 89. Parapet damage after test P5, side. 

Figure 90. Parapet damage after test P5, rear. 
90 

 Figure 91. Parapet damage after test P7. 
91 

[

Figure 92. Original pendulum model. 

Figure 93. Modified pendulum model. 
92 

As shown in Figure 94, the SBP model’s force-time history closely matches the rigid pole 

pendulum calibration test. This calibrated model was used in initial simulations of both 

variations of the T4 bridge rail system. As the research progressed, it was observed that the 

impact forces imparted by the pendulum model did not correspond to those measured in the 

pendulum tests. Comparison of the T4 bridge rail test data with the original pendulum calibration 

test data indicated that the initial segments of the pendulum nose used in the T4 bridge rail tests 

were stiffer than those used in the original rigid pole calibration tests. Whereas the pendulum 

response in tests P3, P4, P5, and P7 appeared reasonably consistent, the response measured in the 

calibration tests differed. 

kN = 225 lbf 

 

Figure 94. Comparison of the SBP model to rigid pole calibration test. 

Aluminum honeycomb is known to be a variable material. While crush characteristics of the 

honeycomb used in the rigid pole calibration were quantified through separate axial compression 

tests, no such tests were performed prior to the T4 bridge rail tests. It is speculated that the crush 

properties of the honeycomb material used to construct the crushable nose assembly in the 1997 

rigid pole calibration tests differed from those of the honeycomb materials used in the 2002 

pendulum tests of the T4 bridge rail specimens. Any change in pendulum stiffness would affect 

the force-time history response and, hence, the energy applied to the barrier. 

Because proper load application is critical to evaluating barrier damage and the concrete material 

model, a recalibration exercise was undertaken. Test P5 on the T4 bridge rail alternative with 

three-bolt anchorage and 317.5-mm- (12.5-inch-) wide parapet was used for recalibrating the 

nonlinear spring representing the honeycomb cartridges. This test was selected because no 

damage to the parapet was observed after the test. However, the rail system did undergo some 

A 

B 

B 

A 
93 

elastic deformation and rebound during the test. Thus, the calibration process involved applying 

a prescribed displacement to the elliptical steel rail. The displacements that were prescribed on 

the rail were obtained from the test using high-speed film analysis measurements. By explicitly 

accounting for the displacement of the rail, the pendulum response can be uniquely obtained. 

As with the original calibration, the recalibration process involved iteratively adjusting the 

stiffness values of the nonlinear spring model until the resulting force-time history closely 

matched data measured in the test P5. The recalibrated pendulum model was labeled SBP2. As 

shown in Figure 95, the pendulum configuration used in the rigid pole test has a different forcetime history than the pendulum used in the test of the almost rigid T4 rail with 317.5-mm- (12.5-

inch-) wide parapet (test P5). The good correlation achieved between the recalibrated pendulum 

model (SBP2) and the pendulum configuration used in test P5 can also be observed in Figure 95. 

Figure 96 presents the force-deflection relationships obtained from both simulation and testing of 

both the rigid pole and T4 bridge rail with 317.5-mm- (12.5-inch-) wide parapet (test P5). As 

shown in this figure, the crushable nose used in test P5 is indeed stiffer than that used in the 

original rigid pole pendulum calibration test. It can also be observed from Figure 96 that the 

recalibrated pendulum model provides reasonable correlation with the pendulum used in test P5. 

The pendulum model follows the same stiffness trend, and the difference in energy between 

simulation and test is less than 1.0 percent. 

kN = 225 lbf 

Figure 95. Force-time histories for benchmark tests and spring models. 

A 
94 

kN = 225 lbf 

Figure 96. Force-displacement relationships for benchmark tests and SBP2 model. 

FINITE ELEMENT MODEL OF T4 BRIDGE RAIL 

Finite element analysts typically follow certain procedures before and after running the 

numerical solver to help maintain quality control and achieve efficient analysis. The solver used 

for this study was LS-DYNA. LS-DYNA is an explicit-implicit, multiphysics, nonlinear finite 

element solver. The pre-processor used for this study was HyperMesh®. The post-processor used 

was LS-POST. The following steps were followed in analyzing the application of the new 

concrete material model in the T4 bridge rail system: 

1. Geometrical modeling of the structure’s components. This step includes defining the 

spatial topology of the model. 

2. Meshing the model. In this step, the spatial topology of each model component is 

discretized into thousands of small elements (i.e. finite elements). 

3. Defining sectional properties. This step includes establishing the thickness of shell 

elements, the cross-sectional properties of beam elements, and prescribing an element 

formulation for all element types. 

4. Prescribing boundary conditions, contacts, initial velocity, and other constraints needed 

for accurately representing the physics of the impact. 

5. Incorporating material models for all parts including concrete components. 

6. Conducting the analysis. 

7. Post-process results and comparing these results to test data. 

Various steps of this process were systematically repeated to evaluate sensitivity of the model’s 

response to changes in certain modeling and material parameters. 
95 

Overview of T4 Parapet/Deck Model 

The finite element representation of the T4 bridge rail specimens consists of the following 

components: 

• Concrete parapet and deck. 

• Steel reinforcement and anchor bolts. 

• Steel elliptical rail, post, and base plate. 

Figures 97 and 98 show the model components for the four-bolt and three-bolt parapet designs, 

respectively. The concrete parapet and bridge deck were modeled using solid elements, as were 

the steel base plate and the plates comprising the steel post. Shell elements were used to model 

the elliptical steel rail. Beam elements were used to model the anchor bolts and steel 

reinforcement inside the parapet and bridge deck. 

Figure 99 shows a closeup view of the steel portion of the bridge rail model, including the 

elliptical rail, post, base plate, and anchor bolts. Figures 100 and 101 show the steel 

reinforcement and anchor bolts incorporated into the four-bolt and three-bolt parapet models, 

respectively. All vertical and longitudinal steel were explicitly modeled. 

Figure 97. Model of T4 bridge rail specimen with four-bolt anchorage 

and 254-mm- (10-inch-) wide parapet. 
96 

Figure 98. Model of T4 bridge rail specimen with three-bolt anchorage 

and 317.5-mm- (12.5-inch-) wide parapet. 

Figure 99. Closeup view of steel rail system with four-bolt anchorage. 

. 
97 

Figure 100. Steel reinforcement and anchor bolts for T4 bridge rail specimen 

with four-bolt anchorage and 254-mm- (10-inch-) wide parapet. 

Figure 101. Steel reinforcement and anchor bolts for T4 bridge rail specimen 

with three-bolt anchorage and 317.5-mm- (12.5-inch-) wide parapet. 
98 

Figure 102. Right end view of parapet-only model for four-bolt design and three-bolt design. 

The investigations included evaluating model sensitivity to variations in material parameters and 

making any needed changes to the default values coded into the material model subroutine. To 

facilitate this effort and reduce the computational time required to perform numerous parametric 

runs, the parapet models were extracted from the bridge rail system models as shown in Figure 

102. The bottom edge of the parapet in these subsystem models was constrained against 

movement. Although this artificially increased the stiffness of the parapet to some degree, it 

provided a more computationally efficient means of evaluating the effect of model changes on 

parapet response. After converging on a reasonable set of parameters, the full system models 

(including bridge deck) were simulated and the results compared to measured and observed test 

data. 

Meshing 

As indicated previously, the concrete parts were meshed with solid elements, the steel base plate 

and post were meshed with solid elements, the tubular rail element was meshed using shell 

elements, and the steel reinforcement and anchor bolts were meshed using beam elements. The 

meshes for these components were kept fixed during this study except for the mesh of the 

concrete parapet. 
99 

The original mesh of the parapet was constructed to enforce matching between nodes of concrete 

and those of the steel reinforcement. This construction enables coincident nodes to be merged, 

thus ensuring connectivity between the concrete and steel components. This parapet mesh is 

depicted in Figure 103. Together, the concrete parapet and deck models had a total of 115,000 

elements. The requirement of matching nodes led to elements with poor aspect ratios and the 

creation of unnecessarily small element sizes (e.g., 7 mm (0.276 inch) and 5.6 mm (0.22 inch)), 

which has a significant effect on time step control. 

To mitigate this problem, a different connection scheme was utilized between the parapet and the 

steel reinforcement, which permits a more regular, uniform mesh to be used throughout the 

parapet. Use of coupling (*CONSTRAINED_LAGRANGE_IN_SOLID) permits the concrete 

mesh to be assigned without consideration of the location of steel reinforcement. Details of this 

connection scheme are explained in the Constraints and Boundary Conditions section of this 

report. 

A uniform mesh of 25.4-mm (1-inch) solid elements was used in some preliminary calculations. 

However, an alternate meshing strategy with a biasing scheme was ultimately used in the 

evaluation to provide desired refinement in critical areas of the model without significantly 

affecting the overall size and run time of the model. A two-dimensional biasing scheme was 

incorporated into the model of the concrete parapet. Along the parapet height, the elements were 

linearly biased from approximately 20 mm (0.79 inch) at the bottom of the parapet to 13 mm 

(0.51 inch) at the top of the parapet using a linear biasing function in HyperMesh. A bell curve 

biasing was used along the length of the parapet with element sizes ranging from approximately 

36 mm (1.42 inches) at the ends of the parapet to 16 mm (0.63 inch) in the middle of the parapet. 

The meshing across the width of the parapet was kept semi-uniform with an element size of 16 

mm (0.63 inch). Thus, the largest solid element in the parapet was 16 mm (0.63 inch) by 20 mm 

(0.79 inch) by 36 mm (1.42 inches); the smallest was approximately 14-mm by (0.55 inches) by 

13 mm (0.51 inch) by 16 mm (0.63 inch). A cross section of the revised parapet mesh is shown 

in Figure 104. 

The bridge deck was meshed uniformly along its length using an element size of 25.4 mm 

(1 inch). A linear biasing technique was used across the width of the deck (i.e., along the impact 

direction), with larger elements used at the front deck and smaller elements used at the back of 

the deck where it ties into the parapet. The biased meshing scheme used for the parapet and deck 

system, which consists of approximately 76,000 elements, is shown in Figures 105 and 106. 

Sectional Properties 

The thickness for the shell elements comprising the elliptical steel rail and the cross-sectional 

properties of the beam elements used to model the steel reinforcement and anchor bolts were 

assigned according to the details and specifications of the Texas Type T4 bridge rail system. 

Fully integrated elements (type 16) were used for the steel rail, and the Hughes-Liu beam 

element with cross section integration (type 1) was used for the steel reinforcement and anchor 

bolts. The concrete brick elements were type 1 (underintegrated) with stiffness form of hourglass 

control (type 5) specified. 
100 

Constraints and Boundary Conditions 

For cases in which the bridge deck was included in the analysis, the constraints were imposed on 

the front side of the deck and beam, the bottom of the beam, and the ends of the transverse steel 

reinforcement in the deck as shown in Figure 107. In the simulations conducted with the parapetonly subsystem, the bottom of the parapet and the lowermost points of the vertical reinforcement 

were constrained (i.e., fixed) in all degrees of freedom. Figure 107 also shows an illustration of 

the boundary condition setup for this case. 

Boundary conditions were also imposed on some of the nodes of the rigid pendulum body to 

constrain the motion of the pendulum body in both the vertical and the lateral directions (both of 

which are perpendicular to the impact direction). Motion of the pendulum in these two directions 

is limited by the cables attaching the pendulum to its support towers. Note that the pendulum 

follows a circular arc. Thus, the linear motion prescribed is an approximation, which is accurate 

within a small displacement setting as is the case with the T4 bridge rail. 

A constraint was used to represent the interaction between the anchor bolts, steel reinforcement, 

and the surrounding concrete continuum. The steel reinforcement and anchor bolts are coupled 

(rather than merged) to the surrounding concrete continuum. This coupling was achieved using 

the *CONSTRAINED_LAGRANGE_IN_SOLID feature in LS-DYNA. In this constraint, the 

steel reinforcement and anchor bolts are treated as slave material that is coupled with a master 

material comprised of the deck and parapet concrete. Using this methodology, the slave part(s) 

can be placed anywhere inside the master continuum part without any special mesh 

accommodation. 

Figure 103. Original parapet mesh used for merging nodes with steel reinforcement. 
101 

Figure 104. Revised parapet mesh with steel reinforcement. 

Figure 105. Linear mesh biasing along the height of parapet and width of deck. 
102 

Figure 106. Bell curve mesh biasing along length of parapet and 

uniform meshing along length of deck. 

. 

Figure 107. Boundary conditions used for the full system model 

with deck and for the parapet-only model. 
103 

To verify the proper functionality of this method, an example of a reinforced concrete beam 

modeled with merged nodes as supplied by the developer was modified and rerun using the 

coupling methodology. The response and damage obtained for the two runs was very close. 

The anchor bolts are also constrained to the steel base plate via node merging. Each bolt is 

merged to one node on the upper surface and one node on the lower surface of the base plate. 

This constraint is illustrated in Figure 108. 

Figure 108. Anchor bolt constraint to base plate. 

Three contacts were defined within the bridge parapet model to account for interactions between 

various components: one between the lower surface of the base plate and the top of the parapet, 

one between the lower surface of the parapet and the deck, and one for interaction among the 

steel reinforcement bars. Note that the bridge rail test specimens were constructed using two 

different concrete pours: one of the deck and one for the parapet. The contact definition between 

the parapet and deck represents the construction joint that exists between these two components. 

This contact definition was not used when the parapet-only model was being analyzed. 

It is also noteworthy that the pendulum model has its own internal contact definition as well as 

an additional contact definition between the front cartridge of the crushable nose and the tubular 

steel rail section. All of these contact definitions are depicted in Figure 109. 
104 

Figure 109. Contacts definitions for the T4 bridge rail model. 

Material Definitions 

Material models are essential to accurately studying the performance of any system. This 

research focuses specifically on the newly developed concrete material model; however, other 

material models (e.g., steel) also had to be implemented to achieve appropriate system response. 

All steel reinforcement was modeled using an elastoplastic material model that incorporates a 

strain rate effect on yield strength. The anchor bolts were modeled using elastic steel definition 

due to their size (19.05-mm- (0.75-inch-) diameter), material composition (high strength steel), 

and the behavior observed in the full-scale pendulum tests. It was analytically verified through 

careful monitoring of bolt stresses that none of the anchor bolts reached yield stress at any time 

during simulation. The tubular rail, the base plate, and the steel posts were modeled using an 

elastoplastic material model definition. 

The parapet and deck were both modeled using the new concrete material model developed by 

APTEK. In the beta version of LS-DYNA 971, it is designated as material type 159. The model 

name is *MAT_CSCM_CONCRETE or *MAT_CSCM. The “_CONCRETE” suffix indicates a 

short input format that utilizes hard-coded default values for numerous variables; the other name 

indicates a long input format for which the user must supply values for all the required input 

parameters. Input parameters are not listed here because they are explained in the companion 

Users Manual for the material model. However, some salient parameters studied in this research 

are discussed. These parameters are (as excerpted from the Users Manual): 
105 

ERODE Elements erode when damage exceeds 0.99 and the maximum principal strain 

exceeds 1 − ERODE. For erosion that is independent of strain, set ERODE equal 

to 1.0. Erosion does not occur if ERODE is less than 1.0. 

f 'C Unconfined compression strength. If left blank, default is 30 MPa (4,351 

lbf/inch2). 

 Dagg Maximum aggregate size. If left blank, default is 19 mm (0.75 inches). 

 Gfc Fracture energy in uniaxial compression. 

 Gft Fracture energy in uniaxial tension. 

 Gfs Fracture energy in pure shear. 

repow Power that increases fracture energy with rate effects. 

The element erosion parameter (ERODE) is part of both input formats. The compression strength 

of concrete (f 'C) and the maximum aggregate size (Dagg) are required as part of the short input 

format. The fracture energy related parameters (Gfc ,Gft , Gfs, repow) are part of the long input 

format. The short input format will work with default model parameters based on the 

user-supplied compression strength of concrete (f 'C) and the maximum aggregate size (Dagg); 

the long format requires the user to explicitly define all the model parameters. 

For the T4 bridge rail analysis, the concrete had a maximum aggregate size of 25.4 mm (1 inch). 

The concrete used for the bridge deck had an average compressive strength of 35.5 MPa (5,149 

lbf/inch2

) on the day of testing. The parapet concrete had an average compressive strength of 

30.44 MPa (4,415 lbf/inch2

). 

In this study, the short input format was used to generate and list the full set of parameters in the 

LS-DYNA output file. These parameters were then used in the long input format, and selected 

parameters were varied as part of the performance/sensitivity study. 

ANALYSES OF T4 BRIDGE RAIL 

Numerous analyses were conducted using the models of the T4 bridge rail variants as part of the 

evaluation of the concrete material model. Only the significant analyses are reported here. 

Baseline Parameters 

All dimensional parameters are based on the following units: 

• Megagram for mass. 

• Second for time. 

• Millimeter for length. 

• Newton for force. 

• Megapascal for stress or pressure. 

• Millijoules for energy. 
106 

This corresponds to the UNITS field being set to “2” in the third line of the short input format. 

For the T4 parapet model, which had an average compressive strength of 30.44 MPa (4,415 

lbf/inch2) and a maximum aggregate size of 25.4 mm (1 inch), the short input is shown in t

Table 8. For the bridge deck, which had an average compressive strength of 35.5 MPa (5,149 

lbf/inch2

) and a maximum aggregate size of 25.4 mm (1 inch), the short input is shown in Table 

9. 

Table 8. Short input format for parapet concrete material model. 

*MAT_CSCM_CONCRETE 

$ mid Ro nplot incre irate erode recover iretract

159 2.32-09 0 0.00E+00 1 1.1 1.00E+01 0

$ 

$ PreD 

0 

$ 

$ f'c Dagg Units 

30.44 25.4 2 

Table 9. Short input format for bridge deck concrete material model. 

*MAT_CSCM_CONCRETE 

$ mid ro nplot incre irate erode recover iretract

159 2.32-09 0 0.00E+00 1 1.1 1.00E+01 0

$ 

$ PreD 

0 

$ 

$ f'c Dagg Units 

35.52 25.4 2 

Values for the parameters comprising the long input format of the concrete model were obtained 

from the d3hsp (ASCII output) file of LS-DYNA. However, when these values were obtained, it 

was noticed that the printed output did not correspond to the format provided in the draft manual. 

This identification mismatch affected the parameters K, G (modulus), alpha, theta, lambda, and 

beta of all three surfaces (triaxial compression, torsion, and triaxial extension as well as R and 

X0. These format errors were communicated to the developer, and corrections were made for 

later releases of LS-DYNA 971 to make the manual consistent with the output routine. 

To avoid any confusion or possible modeling errors, the long format input parameters for the 

concrete material models used in the analyses of the T4 bridge rail alternatives were submitted to 

the developer for a correctness check. The long input format parameters for the parapet and deck 

concrete are shown in Table 10 and Table 11, respectively. The values shown in these tables are 

herein referred to as the “baseline values.” Changes to the material model were made with 

reference to these baseline values. The parameters that were varied as part of the material model 

evaluation are shown as shaded. Note that these baseline values are not the default values 
107 

currently implemented in LS-DYNA version 971. They are preliminary values that were later 

adjusted based on results of all calculations presented within this evaluation report. 

Table 10. Long input format for parapet concrete material model. 

*MAT_CSCM_TITLE 

Parapet concrete f'c =4415 psi 

MID RO NPLOT INCRE IRATE ERODE RECOV IRETRC 

14 2.32E-09 1 0 1 1.1 10 0

PreD 

0 

G K α θ λ β NH CH

11520 12610 14.56 0.2979 10.51 0.01929 

α1 θθ1 λ1 β1 α2 θ2 λ2 β2

0.7473 0.001139 0.17 0.07014 0.66 0.001374 0.16 0.07014

R X0 W D1 D2 

5 90.74 0.05 2.50E-04 3.49E-07 

B Gfc D Gfs Gft pwrc pwrt pmod 

100 9.487 0.1 9.49E-02 9.49E-02 5 1 0 

η0χ Nc η0τ Nt overc overt Srate repow 

1.01E-04 0.78 6.22E-05 0.48 21.63 21.63 1 1

Table 11. Long input format for bridge deck concrete material model. 

*MAT_CSCM_TITLE 

concrete for the deck f'c=5152 psi 

MID RO NPLOT INCRE IRATE ERODE RECOV IRETRC 

15 2.32E-09 1 0 1 1.1 1 0

PreD 

0 

G K α θ λ β NH CH

12120 13280 15.16 0.3143 10.51 0.01929 

α1 θ1 λ1 β1 α2 θ2 λ2 β2

0.7473 9.95E-04 0.17 0.0646 0.66 0.001201 0.16 0.0646

R X0 W D1 D2 

5 93.31 0.05 2.50E-04 3.49E-07 

B Gfc D Gfs Gft pwrc pwrt pmod 

100 10.57 0.1 1.06E-01 1.06E-01 5 1 0

η0χ Nc η0τ Nt overc overt Srate repow 

1.13E-04 0.78 6.71E-05 0.48 24.02 24.02 1 1
108 

Baseline Analysis 

A dynamic pendulum impact into the T4 bridge rail with four-bolt anchorage and 254-mm- 

(10-inch-) wide parapet was simulated using the aforementioned baseline values for the concrete 

material model and the initial SBP pendulum model. As shown in Figure 110, the damage fringe 

obtained from the simulation approximates that observed during the testing (see Figure 88). The 

damage fringes depict the damage of each element on a scale from 0 to 1 where the value 0 

indicates no damage and the value 1 indicates total damage (i.e., the element is not capable of 

carrying load). However, unlike the tests, no material failure (i.e., element erosion) was observed 

in this simulation. 

Figure 110. Damage fringe for baseline simulation of T4 

with four-bolt anchorage and 254-mm- (10-inch-) wide parapet. 

Parametric Analyses 

Given that the baseline values did not provide the desired failure response, a sensitivity study 

was conducted to investigate system sensitivity to selected parameters. Another analysis 

(case02) was conducted for which erosion was enabled independent of strain (i.e., ERODE equal 

to 1.0). The other variables were unchanged from their baseline values. 

As shown in Figures 111 and 112, elements were eroded from both the parapet and the deck. 

With ERODE set to 1.0, the elements eroded based on a set damage threshold (i.e., above 0.99) 

without consideration of strain. Damage fringes for this simulation case are shown in Figure 113. 
109 

Figure 111. Element erosion profile (simulation case02, ERODE =1) on traffic side. 

Figure 112. Element erosion profile (simulation case02, ERODE =1) 

on field side. 
110 

Figure 113. Damage fringes for simulation case02 (ERODE =1). 

Elements eroded on the field side of the parapet (see Figure 112) propagated in a pattern similar 

to that observed in the test. However, element erosion on the traffic face of the parapet and the 

tension (top) face of the bridge deck (see Figure 111) does not replicate test results. Recall that 

no visible damage or cracks were observed on either of these faces after tests P3 or P4. This 

result indicates that element erosion should not be used independent of a maximum principal 

strain criterion. 

 

Another simulation was conducted with the value of the ERODE parameter set to 1.05. Although 

the pattern of the damage fringes was generally consistent with that observed in the pendulum 

tests, no element erosion/failure occurred, which makes the results similar to those from the 

baseline simulation with ERODE = 1.1. 

The focus then shifted toward studying the effect of the fracture energies (Gfc, Gfs, and Gft) on the 

damage profile and erosion of elements. Initially, very low values of the fracture energies (20 

percent of the original baseline values) were used. As might be expected, this change resulted in 

extensive element erosion and very weak parapet response as shown in Figure 114. 

It was noticed during this simulation that the energy balance of the model changed during the 

analysis. More specifically, the total energy of the system increased. The change was attributed 

to an inappropriate increase in total internal energy of the system. Further investigation revealed 
111 

that this unrealistic increase in energy, shown in Figure 115, was traceable to the concrete 

material. Beginning at about 0.05 s, the total energy increases 2.5 times its original value. The 

changes in the internal energy of the concrete material correspond to this change in the total 

system energy and appear to be related to the damage calculations. As damage of the concrete 

components increases (as indicated by the damage fringes and contours), the total system energy 

increases. 

Similar behavior was present in the baseline simulation as well. However, this behavior was not 

as readily detectable because the percentage of increase in energy is related to the damage 

induced in the concrete. This behavior was disclosed to the developer during the early stages of 

model validation, and a fix was incorporated into later releases of LS-DYNA version 971. 

Continuing with the parametric evaluation, the values of fracture energies were next increased to 

50 percent of the baseline values. As shown in Figure 116, the associated fracture profile 

radiated out from the outer anchor bolts on the top of the parapet but did not extend to the field 

side of the parapet. 

A process of bisection of fracture energy values was followed until a set of values that produced 

a similar fracture profile to that observed in the test was identified. With the fracture energy 

values set at 27.5 percent of their baseline values, the simulation resulted in a damage pattern and 

fracture profile similar to those observed in the test. The fracture profile shown in Figure 117 

indicates that a piece of concrete similar in shape and size to those that fractured in tests P3 and 

P4 would fracture and possibly spall off. Additionally, the model captures the deflection and 

rotation of the anchor bolts inside the parapet wall similar to that observed in the tests. 

Figure 114. Parapet failure with fracture energies at 20 percent of baseline values. 
112 

Joule = 0.73756 ft-lb

Figure 115. Energy-time histories for pendulum impact of T4 bridge rail 

with fracture energies at 20 percent of baseline values. 

Figure 116. Parapet failure with fracture energies at 50 percent of baseline values. 
113 

Figure 117. Parapet failure with fracture energies at 27.5 percent of baseline values. 

The energy-time histories associated with this run are shown in Figure 118. As previously 

discussed, an increase in the total system energy can be observed to coincide with a significant 

increase in the internal energy of the system at about 0.05 sec. The extent to which the 

calculations are affected by this behavior is not known. The developer indicated that the problem 

was confined to a reporting issue and does not affect the simulation outcome. A fix was 

incorporated into later releases of LS-DYNA version 971. 

Realizing that fracture energies set at 27.5 percent of the baseline values could not be physically 

justified, two other aspects of the model were further investigated. First, in consultation with the 

developer, the stiffness of the crushable nose of the pendulum impactor was studied to see 

whether the impact energy absorbed by the pendulum and transferred to the barrier agreed with 

test data. The second aspect investigated was an enhancement of the anchor bolt connection 

between the base plate and concrete parapet. 

Comparison of data from the rigid pole calibration tests and the T4 bridge rail impacts showed a 

discrepancy in the stiffness of the nose assembly. Additional checks on the properties of the 

aluminum honeycomb material commonly used in the crushable nose assembly of the pendulum 

bogie indicated that the material stiffness can vary considerably (e.g., 10 percent to 20 percent) 

among different batches. Because the properties of the honeycomb used in the pendulum testing 

of the T4 bridge rail were not directly measured, a new stiffness curve for the pendulum spring 

(SBP2) was developed based on test P05 as previously described. The net result is a stiffer 

pendulum nose that correlates with the honeycomb material used in the actual pendulum tests of 

the T4 bridge rail systems. 

Upon consultation with the developer, it was suggested that a set of fracture energy values at 80 

percent of the baseline values is a reasonable lower bound for concrete having a maximum 

aggregate size consistent with that used in the T4 bridge rail installations. Consequently, the 

modified SBP2 pendulum model was used in an impact analysis of the T4 parapet system with 

four-bolt anchorage and 254-mm- (10-inch-) wide parapet using 80 percent of the baseline 
114 

fracture energy values. However, this configuration did not result in a significant change to the 

damage profile compared with the parapet impacted by the lower stiffness pendulum (SBP). 

Next, further study was devoted to the connection between the base plate and anchor bolts. 

Initially, nodes on the anchor bolts were merged to corresponding nodes on the base plate. This 

merging constrained the base plate from rotation, a behavior that was observed in the high-speed 

video of the pendulum tests. The interaction between the base plate and anchor bolts was 

subsequently enhanced by removing the merged nodes connection and adding washers on the top 

surface of the base plate to constrain upward vertical motion of the base plate. The washers were 

tied to the anchor bolts. A *CONSTRAINED_NODE_SET was added between nodes of the 

anchor bolts and the closest base plate nodes to constrain motion in the horizontal plane of the 

base plate. 

Joule = 0.73756 ft-lb 

Figure 118. Energy-time histories for pendulum impact of T4 bridge rail 

with fracture energies at 27.5 percent of baseline values. 

This configuration gives the base plate more freedom to rotate when subjected to an applied 

moment due to rail impact based on the material properties of the bolts and washers. The vertical 

downward constraint on the base plate was handled by contact with the top surface of the 

concrete parapet. This modeling change was considered to more accurately represent the 

behavior of the actual connection without significantly affecting computer processing time. The 

enhanced connection model between the base plate and anchor bolts is depicted in Figure 119. 
115 

Figure 119. Enhanced anchor bolt-to-base plate connection model. 

Modified System Analyses 

An LS-DYNA model was constructed using the SBP2 pendulum model, the lower end of the 

recommended fracture energy values (80 percent of baseline values), and the enhanced base 

plate-to-anchor bolt connection. The parapet-only model of the T4 parapet system with four-bolt 

anchorage and 254-mm- (10-inch-) wide parapet (discussed previously) was used in the 

simulation to reduce computational time. 

Figures 120–122 show sequential views of the simulation at different times. Although the 

general pattern was similar, the fracture damage profile was more extensive than that observed in 

the pendulum tests (tests P3 and P4). This result was expected in part due to the use of the 

parapet-only model, which is less flexible than the more detailed model configuration that 

incorporates the bridge deck. It is noteworthy that the rail-post-base plate assembly rigidly 

rotated and subsequently rebounded as observed in the actual pendulum tests. 
116 

Figure 120. Fracture profile of modified T4 system at 0.080 seconds. 

Figure 121. Fracture profile of modified T4 system at 0.115 seconds. 
117 

Figure 122. Fracture profile of modified T4 system at 0.250 seconds. 

Full System Analysis: Four-Bolt Design 

The parameters used in the analysis of the parapet-only simulation of the modified T4 parapet 

system with four-bolt anchorage and 254-mm- (10-inch-) wide parapet were incorporated into 

the full system model that included the bridge deck. As before, the SBP2 pendulum model was 

used as the impactor. 

A profile of the damaged bridge rail system after impact is shown in Figure 123. The fracture 

profile of the parapet is shown in Figure 124 with the steel components of the parapet removed 

for better visualization. Due to the inherent flexibility of the bridge deck, the fracture profile of 

the concrete parapet was less severe than that for the parapet-only model and was similar to that 

observed in the pendulum tests. Element erosion radiated from the outer anchor bolts and 

extended to the back edge of the parapet and down the field side of the parapet wall. 
118 

Figure 123. Profile of damaged T4 bridge rail system with 

four-bolt anchorage after pendulum impact. 

Figure 124. Fracture profile for T4 bridge rail with four-bolt anchorage 

for parapet and eroded elements. 
119 

As shown in Table 12, the peak impact force in the simulation of the T4 bridge rail system with 

four-bolt anchorage compares favorably with those measured in the corresponding pendulum 

tests. Acceleration-time histories for the tests and simulation, filtered at 180 Hertz (Hz), are 

compared in Figure 125. The simulation data tracks the test data reasonably well up to the time 

of peak acceleration. After this time, the rebound portion of the pendulum simulation data 

deviates from the tests. However, this rebound phase does not have direct bearing on the 

evaluation of the concrete material model or roadside safety structure. 

Table 12. Force comparison between tests and simulation 

for T4 rail system with four-bolt anchorage. 

Description Maximum Peak Impact Force 

kilonewtons (kN) (kips) 

Test P3 145.0 (32.6) 

Test P4 129.0 (29.0) 

Four-Bolt Simulation 130.3 (29.3) 

Figure 125. Pendulum bogie accelerations for impact of T4 bridge rail 

with four-bolt anchorage and 254-mm- (10-inch-) wide parapet. 

The peak impact force for test P3 is approximately 10 percent greater than the peak impact force 

for test P4 and the simulation. Because the test specimens and impact conditions are nominally 

similar, this difference is attributed to normal material and test variation. The acceleration pulse 

indicated during the rebound phase of test P3 is attributed to pitching and “bucking” of the 

suspended pendulum mass. 

C 
120 

Figure 126 presents the velocity-time histories for the pendulum tests and simulation. Because 

these data are based on integration of the acceleration data, they are expected to be smoother and 

correlate better. Note that the negative portions of the velocity curves represent rebound of the 

pendulum. The simulation data tracks the data from test P4 up to the rebound phase of the impact 

(velocity < 0). The data for test P3 deviates from test P4 and the simulation before rebound. 

m/sec = 3.28 ft/sec

Figure 126. Pendulum bogie velocities for impact of T4 bridge rail 

with four-bolt anchorage and 254-mm- (10-inch-) wide parapet. 

Overall correlation between the simulation and test data is considered to be good. The simulation 

matches particularly well with test P4. Thus, researchers decided to proceed to simulation of the 

T4 bridge rail system with three-bolt anchorage and 317.5-mm- (12.5-inch-) wide parapet to 

further evaluate the concrete material model. When tested, this design variation had a different 

level of damage than the system with four-bolt anchorage and 254-mm- (10-inch-) wide parapet, 

thus providing an opportunity to assess the sensitivity of the concrete model to small design 

changes under similar impact loading conditions. 

Full System Analysis: Three-Bolt Design 

The same parameters used in the simulation of the T4 bridge rail with four-bolt anchorage and 

254-mm- (10-inch-) wide parapet were incorporated into the full system model of the T4 bridge 

rail with three-bolt anchorage and 317.5-mm- (12.5-inch-) wide parapet. As discussed 

previously, the full system model incorporates the bridge deck. The modified SBP2 pendulum 

model was used as the impactor. 
121 

Figure 127 shows the calculated response of the parapet-deck system after being impacted by the 

pendulum. No element erosion occurred in the analysis. The rail/parapet assembly rebounded 

after a small deflection. Recall that no visible damage was observed after test P5, and only small 

hairline cracks were found after test P7. Figures 128 and 129 show the damage fringes from the 

simulation. The fringe pattern is similar to the cracking pattern observed in test P7, which 

indicates that under a more severe impact, the concrete would fail in a pattern similar to that 

initiated in test P7. 

Figure 127. Profile of T4 bridge rail system with three-bolt anchorage after pendulum impact. 
122 

Figure 128. Damage to 317.5-mm- (12.5-inch-) wide parapet after pendulum impact showing 

element erosion. 

Figure 129. Damage to 317.5-mm- (12.5-inch-) wide parapet after pendulum impact showing 

damage fringes. 
123 

The maximum impact force calculated in the simulation compares very favorably with those 

measured in the test P5 as shown in Table 13. A considerable difference exists between the peak 

force measured in test P5 and test P7. These tests were conducted on the same day on two 

different test specimens under nominally similar impact conditions. Beyond test variability, the 

cause of the difference in peak force is not known. 

Table 13. Force comparison between tests and simulation for T4 rail system with three-bolt 

anchorage. 

Description Maximum Peak 

Measured Force kN 

(kips) 

Test P5 133.9 (30.1) 

Test P7 176.7 (39.7)

Three-Bolt Simulation 134.8 (30.3) 

Acceleration-time histories for the pendulum tests and simulation of the T4 rail system with 

three-bolt anchorage and 317.5-mm- (12.5-inch-) wide parapet are compared in Figure 130. The 

simulation data tracks the test data reasonably well during both the loading and unloading (i.e., 

rebound) phases of the impact. Recall that data from test P5 was used for the recalibration of the 

pendulum model. Test P7 is an independent test of a similar installation under similar impact 

conditions. Figure 43 shows that the peak acceleration for test P7 exceeds that for test P5 and the 

simulation. 

Velocity-time histories for the pendulum tests and simulation are presented in Figure 131. The 

simulation data tracks the test data reasonably well during both the loading and unloading (i.e., 

rebound) phases of the impact. 
124 

Figure 130. Pendulum bogie accelerations for impact of T4 bridge rail with three-bolt anchorage 

and 317.5-mm- (12.5-inch-) wide parapet. 

m/sec = 3.28 ft/sec

Figure 131. Pendulum bogie velocities for impact of T4 bridge rail with three-bolt anchorage and 

317.5-mm- (12.5-inch-) wide parapet. 
125 

Overall correlation between the simulation and test data is considered to be good. The simulation 

matches particularly well with test P5 in terms of damage, peak force, and acceleration-time 

history. 

SUMMARY FOR BRIDGE RAIL ANALYSES 

The analyses of the T4 bridge rail alternatives provided a good benchmark for evaluating the 

application of the new concrete material model in roadside safety applications. Use of the 

pendulum bogie provided more controlled tests and eliminated many variables associated with 

the comparison of simulation to full-scale vehicle crash tests. Two specimens were tested for 

each design variation, providing some information regarding system variability. Furthermore, the 

two design variations demonstrated different levels of damage to the concrete parapet, which 

provided an opportunity to assess the sensitivity of the concrete model to small design changes 

under similar loading conditions. 

After calibration of the material model parameters and enhancement of the base plate connection 

model, simulations of the two bridge rail alternatives were able to capture the general pattern and 

severity of concrete damage observed in pendulum tests of both the 254-mm- (10-inch-) and 

317.5-mm- (12.5-inch-) wide parapets. As mentioned previously, the user desired to more fully 

evaluate the concrete material model in other roadside safety structures. A model of a 

safety-shape bridge rail with New Jersey profile was developed for this purpose. Although some 

preliminary calculations were performed on this model, project resources were depleted before 

the structure could be fully analyzed. More details of this bridge rail model, available test data, 

and discussions of preliminary calculations are presented in the next chapter. 

127 

CHAPTER 9. ANALYSES OF SAFETY-SHAPED BARRIER 

The user conducted static and dynamic tests on a Florida safety-shape barrier with New Jersey 

profile.(8) The tests were conducted prior to, and separate from, this effort. Test data available 

for this barrier include quasi-static load tests to failure at both the end and middle of the parapet. 

The initial test case selected for evaluating the barrier model was a quasi-static load test to failure 

on the end of the parapet section (TTI test 421323-S1). Test S1 was performed on the upstream 

end of the test installation and was intended to represent loading at the barrier ends or at an 

interior bridge expansion joint. 

The test setup is shown in Figure 132. The load was applied using a hydraulic cylinder with an 

inline load cell. The hydraulic cylinder was attached to a fabricated steel frame that was bolted to 

the concrete deck structure. A steel wide flange beam stiffened with welded gussets was clamped 

to the face of the parapet to distribute the applied load over a distance of 1,219 mm (48 inches) A 

tapered wood block was placed between the back flange of the beam and the sloped face of the 

concrete parapet to permit horizontal application of the load. The steel beam was mounted to the 

parapet with the top edges of the flanges flush with the top surface of the parapet. The hydraulic 

cylinder applied the load to the middle of the steel beam. Displacement of the barrier was 

measured using a string pot. 

Figure 132. Test setup for static load tests on safety-shaped barriers. 
128 

The maximum load attained in test S1 was 156 kN (35.1 kips). The resulting failure mode and 

force-deflection curve are shown in Figures 133 and 134. The load capacity calculated from a 

yield line analysis was 185 kN (41.6 kips). Subsequent destructive inspection of the test 

installation showed the last stirrup was spaced approximately 152 mm (6 inches) from the end of 

the parapet wall rather than 50.8 mm (2 inches) and likely contributed to the lower than expected 

fracture load. 

Figure 133. Failure mode at end of the safety-shaped barrier. 

Figure 134. Measured load versus displacement for the safety-shaped barrier. 
129 

FINITE ELEMENT MODEL 

A finite element model of a steel-reinforced concrete safety-shape bridge rail with New Jersey 

profile was developed by the user. The model conformed to details and specifications of a rail 

that was once a standard of the Florida Department of Transportation (FDOT) (FDOT Sheet 

Index No. I-799). The 813-mm- (32-inch-) tall barrier is 152 mm (6 inches) at the top and 382 

mm (15 inches) at its base. The barrier was cast atop a 178-mm- (7-inch-) thick reinforced 

concrete bridge deck cantilevered off of a concrete beam. The concrete used in the bridge rail 

parapet had a maximum aggregate size of 25.4 mm (1 inch) and an average compressive strength 

of 24.9 MPa (3,611 lbf/inch2

). The bridge deck concrete had a maximum aggregate size of 25.4 

mm (1 inch) and an average compressive strength of 27.1 MPa (3,931 lbf/inch2

). Dimensions of 

the barrier system and steel reinforcement details are shown in Figure 135. 

A modeling approach similar to that used for the Texas T4 bridge rail was followed for the New 

Jersey safety-shape rail system. The concrete parapet and bridge deck were modeled using solid 

elements. Beam elements were used to model the steel reinforcement inside the parapet and 

bridge deck. The element formulation used for the steel reinforcement was the Hughes-Liu beam 

element with cross section integration (type 1). The concrete brick elements were type 1 

(underintegrated) with stiffness form of hourglass control (type 5) specified. The short input 

format for the new concrete material model was used to generate the values for the parameters 

required in the long input format, and these established the baseline input values for the Florida 

safety-shaped barrier model.(8) The steel reinforcement was coupled to the surrounding concrete 

using the *CONSTRAINED_LAGRANGE_IN_SOLID feature in LS-DYNA. Figure 136 shows 

the meshing for the parapet and the deck and the layout of steel reinforcement in both. Figure 

137 shows the overall steel reinforcement layout in the model. 

The steel reinforcement in the parapet model was revised to reflect the actual construction details 

of the stirrups, which were 152.4 mm (6 inches) from the end. A simple surrogate impactor was 

modeled to represent the hydraulic cylinder. The wood block was modeled to account for any 

compliance associated with the load transfer to the parapet. Figure 138 illustrates the load 

application setup with respect to the bridge rail model. 

The impactor was forced to follow a displacement-time curve that simulated the quasi-static 

loading condition. The long duration of the test is problematic to reproduce in an explicit 

analysis procedure. Therefore, the solution must take into account effects. In the analysis, the 

duration of the simulation was 0.150 sec, which is a fraction of the actual test duration. 
130 

mm = 0.039 inch 

Figure 135. Cross section of the Florida safety-shaped barrier with New Jersey profile.(8)
131 

Figure 136. Cross section of Florida barrier model concrete mesh and reinforcement layout. 

Figure 137. Isometric view of steel reinforcement in Florida barrier model. 
132 

Figure 138. Model of quasi-static load test setup. 

USER EVALUATION RESULTS 

As shown in Figure 139, simulation results using the preliminary baseline concrete material 

properties indicate fracture damage (i.e., element erosion) along the cold construction joint 

between the parapet and the deck, at the transition between the toe of the barrier and parapet 

wall, and on the edge of the parapet wall just below the impactor. Additional analyses were 

conducted using 80 percent and 27.5 percent of the baseline fracture energies without significant 

change in the fracture profile. 

Due to time and resource constraints, the user could not perform additional investigation of this 

barrier system. The user suggested that the following actions should be undertaken: changing the 

contact definition at the cold construction joint between the parapet and the deck, adjusting the 

impactor interaction with the parapet, and studying the sensitivity of the system to the rate effect 

parameters in the concrete model. The developer followed up on some of these suggestions, and 

evaluations of these activities are provided in the following section. 
133 

Figure 139. Fracture profile of Florida safety-shaped barrier. 

DEVELOPER BASELINE CALCULATIONS 

The developer began the calculations using the mesh setup by the user, as previously shown in 

Figure 138, but made a few adjustments. All concrete material properties were adjusted to 

default properties, except the shear fracture energy was set to Gfs = 1⁄2 Gf t instead of Gfs = Gf t. 

This reduced fracture energy was used in shear because it proved appropriate in some of the 

bridge rail analyses discussed in appendix B. Unless otherwise specified, each calculation was 

conducted with erosion occurring at 99 percent damage with a maximum principal strain of 5 

percent (ERODE = 1.05). A joint exists between the deck and parapet that is much weaker than 

solid concrete. This joint interface was adjusted from 

*CONTACT_TIED_NODES_TO_SURFACE to *CONTACT_NODES_TO_SURFACE, to 

allow separation in tension. 

Rate effects were turned from on to off in the concrete model. Turning rate effects off allowed 

the quasi-static simulations to run at a higher rate than the quasi-static test. Performing this step 

is typical and necessary. The turnaround time of the calculations would be extremely long (days) 

if the calculations were run at the same slow rate as the tests. 

As previously mentioned, the quasi-static load was generated using lateral displacements applied 

directly to all nodes of the steel spreader plate (modeled as rigid shell elements connected to the 

timber hex elements). The applied displacements increase linearly from 0 to 38.1 mm (0 to 1.5 

inches) over 150 msec, as setup by the user. This increase is slow enough to eliminate wave 

propagation effects. 
134 

Damage fringes at about 70 msec are shown in Figure 140. At this time, the parapet has 

displaced laterally about 16 mm (0.63 inches). Three regions of high damage are noted. First, 

parapet damage extends from the front at midlevel to the back at deck level, similar to that 

observed in the post-test photograph. A large inclined shear crack also extends from midlevel 

upward to the top of the parapet. Finally, concentrated damage is also noted where the lower 

edge of the timber contacts the parapet. This concentrated damage is not observed in the post-test 

photograph. 

Close examination of the computed results indicates that the timber is not remaining in complete 

contact with the parapet, also shown in Figure 140. The contact is concentrated at the bottom of 

the timber spreader, resulting in a stress concentration in the concrete at the point of this contact. 

This concentration may not be realistic. The developer thinks that complete contact likely 

occurred during the tests due to the presence of the clamps, or slight deformation of the timber, 

as previously shown in Figure 133. The timber is modeled as elastic using material model 1 with 

a modulus of 247 MPa (35,824 lbf/inch2

). 

Figure 140. A damage concentration is simulated in the parapet due to application of the 

steel/timber spreader plate that is not observed in the post-test parapet. 

Therefore, a second calculation was performed with the timber modeled as a plastically 

deformable, damageable material using wood model 143. Properties selected are defaults for 

saturated Grade 1 pine at room temperature. The modulus in the loading direction is 247 MPa 

(35,824 lbf/inch2

), which is the same as that used in the elastic timber model of the previous 

calculation. Damage fringes are shown in Figure 141 at 16.5 mm (0.65 inches) and 38.1 mm (1.5 

inches) of lateral deflection. Switching the timber model from elastic to elastoplastic with 

damage relieves the stress concentration previously calculated at the lower edge of the spreader 

beam. However, a gap between the beam and parapet is still noted, and late-time unexpected 

damage occurs near the base of the parapet that is not evident in the test. In addition, the peak 
135 

force attained in the calculation is 282 kN (63.4 kips), which is 81 percent higher than the 156 

kN (35.1) measured during the test. 

mm = 0.039 inch

 

Figure 141. The damage concentration is relieved if the timber is realistically modeled as an 

elastoplastic damaging material. 

Finally, two additional calculations were conducted in an attempt to retain contact between 

spreader beam and parapet and to reduce the computed peak force. Figure 142 is an example of 

how the finite element model was enhanced to include a single rigid element representing the 

load application face of the hydraulic ram. The quasi-static load is generated using a lateral 

displacement history applied directly to the nodes of the ram element, rather than the steel 

spreader beam. A contact surface (CONTACT_NODES_TO_SURFACE) separates the ram 

element from the spreader beam elements that allows for separation but not penetration. In this 

way, the spreader beam can rotate slightly relative to the ram element and retain contact with the 

parapet during displacement. 
136 

mm = 0.039 inch

Figure 142. A realistic damage and erosion pattern is simulated if the timber remains in contact 

with the parapet (ERODE = 1.05). 

Damage fringes for one calculation are shown in Figure 142 at 20 mm (0.8 inches) of lateral 

deflection. Rate effects were also removed from the steel reinforcement. This calculation was 

conducted with erosion occurring at 99 percent damage with a maximum principal strain of 5 

percent, like all previously discussed calculations (ERODE = 1.05). The pattern of erosion and 

damage is consistent with that observed in the test, as previously shown in Figure 133. The peak 

force attained in this calculation is 183 kN (41.1 kips) at 31 mm (1.2 inches) deflection, which is 

consistent with the 185 kN (41.6 kips) force the user expected to measure, but is 17 percent 

higher than the force actually measured. 

Damage fringes for the second calculation are shown in Figure 143 at 10 mm and in Figure 144 

at 20 mm (0.8 inches) of lateral deflection. This calculation was conducted with erosion 

occurring at 99 percent damage, regardless of maximum principal strain value (ERODE = 1.0). 

The peak force is measured at approximately 10 mm (0.4 inches) of deflection. The final 

measurement before loss of strength is made at approximately 20 mm (0.8 inches) of deflection. 

Two views are shown—with and without the visible mesh—to better view the erosion. In this 

case, the damage pattern is less diffuse, and the erosion pattern is much more prominent, than 

calculated with ERODE = 1.05. 

Again, the calculated erosion and damage pattern in the parapet is consistent with the post-test 

cracking pattern previously shown in Figure 133. However, additional erosion occurs in the deck 

that is not visible in post-test photo. The developer thinks erosion occurs because the deck 
137 

section modeled is not nearly as long as the actual test section, due to the need to retain a 

reasonable run time with a reasonable number of elements. Hence, the cantilever-type bending of 

the short deck produces tensile stresses in the concrete that are higher than those that would be 

produced in a longer deck. 

The peak force attained in this calculation is 181 kN (40.1 kips) at 31 mm (1.2 inches), which is 

within 16 percent of the measured value. The calculated force versus deflection history is shown 

in Figure 145. It is in good agreement with that previously shown in Figure 134 for the first 

12 mm (0.5 inches) of deflection. However, the peak force continues to increase beyond 12 mm 

(0.5 inches) to a higher force, and with more ductile behavior, than measured. The computed 

force remains fairly constant (or increases slightly) with increasing deflection beyond 31 mm 

(1.2 inches), while the measured force decreases in magnitude. It is not clear, at least to the 

developer, why the measured force drops down to near 0 even though the steel reinforcement 

remains intact. 

mm = 0.039 inch

 

Figure 143. The primary erosion agrees with the measured crack pattern if the timber remains in 

contact with the parapet (ERODE = 1.0). 
138 

mm = 0.039 inch

 

Figure 144. The primary erosion agrees with the measured crack pattern if the timber remains in 

contact with the parapet (ERODE = 1.0). 
139 

mm = 0.039 inch, kN = 225 lbf

Figure 145. The calculated force versus deflection history is in reasonable agreement with the 

measured curve for the first 12 mm (0.5 inches) of deflection. 

DEVELOPER APPLIED FORCE CALCULATIONS 

One alternative method of simulating the barrier test is to simplify the geometric model and 

loading conditions. Simplified loading conditions are often used as a first step in performing a 

finite element analysis and are quite often sufficient. The timber remains in contact with the 

parapet during the test; thus, the timber applies lateral force to the parapet over the entire contact 

region. Therefore, concentrated lateral forces are directly applied to the nodes of the parapet over 

the timber-to-parapet contact region. The total load applied increases nonlinearly from 0 to 156 

kN (0 to 35.1 kips) in 40 msec, remains at 156 kN (35.1 kips) until 50 msec, then drops to 18 kN 

(4.0 kips) by 260 msec. The steel/timber spreader plate is completely removed from the finite 

element model. 

Damage fringes are shown in Figure 146 for two calculations conducted with different erosion 

values. One force-displacement history is shown in Figure 147. The damage simulated extends 

from the front at midlevel to the back at deck level. Inclined shear damage lines are also present. 

The computed damage is similar to the damage observed in the post-test photograph. It is also 

similar to that calculated and previously shown in Figure 144 where the timber remains in 

contact with the parapet. As desired, concentrated damage in the loading regime is not simulated. 

Nor is unexpected damage near the base of the parapet. 

 
140 

Figure 146. The computed damage mode is similar to that measured if the load is applied via 

concentrated nodal point forces (at 11- to 12-mm (0.43- to 0.5-inch) deflection). 

mm = 0.039 inch, kN = 225 lbf

 

Figure 147. The computed force versus displacement unloads, when the load is applied via 

concentrated nodal point forces (ERODE = 1.05). 
141 

Approximately 11 mm (0.43 inches) to 12 mm (0.5 inches) of parapet displacement are 

computed at the center of the loading region when the applied load is 156 kN (35.1 kips), in good 

agreement with the measured displacement previously shown in Figure 134. However, once the 

applied force begins to drop at 50 msec, the barrier displacement begins to decrease, which is not 

realistic. The drawback of this calculation is that the force history is applied and its magnitude is 

assumed equal to that measured (the timing of the application is not available). 

SUMMARY FOR SAFETY-SHAPED BARRIER CALCULATIONS 

The application of the load in the static test of the safety-shaped barrier proved critical to 

accurate modeling of the damage mode. The simplest calculation conducted using concentrated 

nodal forces applied directly to the parapet provides good correlations with the measured damage 

mode and with the force versus displacement history to peak strength. However, the drawback of 

this calculation is that the applied force history is assumed, not predicted. 

The best correlations are obtained when the timber plate is free to adjust orientation in order to 

maintain good contact between the timber and concrete. This situation was accomplished by 

representing the load application face of the hydraulic ram as a single rigid element, with 

flexibility between this element and the timber/spreader plate. If the timber is restrained from 

adjusting orientation, then a gap forms between the timber and concrete, which produces 

undesirable damage concentrations in the concrete. The main difference between this calculation 

and the measured results is that the computed force attained agrees with the pretest estimated 

value of 185 kN (41.6 kips), but is higher than the measured value of 156 kN (35.1 kips). 

All safety-shaped barrier calculations conducted focused on applying the load correctly, setting 

the proper contact surface conditions at the joint between the parapet and deck, and in turning off 

rate effects to better simulate quasi-static behavior. No parametric studies were conducted related 

to the concrete model or its properties. All calculations used default properties for the concrete 

except for setting Gfs = 1⁄2Gft. This reduced shear modulus was used because the Texas T4 bridge 

rail simulations indicate that a reduced shear modulus may be appropriate. Ultimately, a 

reasonable damage mode was predicted using these reduced properties and appropriate load and 

boundary conditions. 

This series of calculations demonstrates that well-defined load and boundary conditions are 

essential when analyzing tests for material model evaluation. Otherwise, a good portion of the 

effort may be spent refining the load and boundary conditions, rather than evaluating the material 

model. However, tests such as the safety-shaped barrier just analyzed often are conducted for 

purposes other than material model evaluation. Financial and time constraints require that 

published and available test data are used. The analyst must be prepared to critically review all 

aspects of the geometric and material models being used in the simulation and not just inspect 

the particular material model under evaluation. 

143 

CHAPTER 10. SUMMARY AND RECOMMENDATIONS 

DEVELOPER COMMENTS 

A material model for concrete was developed and implemented into the LS-DYNA finite 

element code. Also implemented was a suite of default material properties as a function of 

concrete compressive strength and maximum aggregate size. The model and default properties 

were evaluated for use in roadside safety applications through correlations with test data. Some 

of the test data—including those related to drop tower and bogie vehicle impact into reinforced 

concrete beams—as generated specifically for this effort. Some of the test data was generated 

prior to this effort but made available for this study, including pendulum impact into bridge rails 

and quasi-static loading of a safety-shaped barrier. 

Analyses of these tests indicate that in most cases, damage modes and deflection histories were 

accurately simulated using default material properties. In a few cases, alternative properties were 

suggested to simulate additional damage. The properties that seemed to be most critical are the 

fracture energies (Gft in tension, Gfs in shear, Gfc in compression), the rate effect on fracture 

energy (repow), and the maximum principal strain at which erosion occurs (ERODE). In general, 

the developer recommends using default properties of Gfs = Gft with Gfc = 100 Gft with repow = 

1. The fracture energy in tension was obtained from values listed in the CEB. If more shear or 

compression based damage is desired, then use of Gfs = 1⁄2 Gft or Gfc = 50 Gf are reasonable 

reductions. If more overall damage is desired, then repow = 0.5 is a reasonable reduction. 

Reductions below these values are not recommended. 

Erode is a control parameter. If a value is not specified (ERODE = 0.0), then erosion will not 

occur. The recommendation is to specify erosion between 5 and 10 percent maximum principal 

strain (1.05 ≤ ERODE ≤ 1.10). By taking this step, severe damage is able to accumulate and be 

maintained before erosion occurs. In numerous calculations, erosion set to 5 and 10 percent 

strain gave similar results. Erosion at 1 percent strain was evaluated but typically simulates a 

structural response that is more flexible than at 5 to 10 percent strain and may be more flexible 

than measured. Once an element erodes, then a 25- to 38-mm (1- to 1.5-inch) gap forms (the 

dimension of the element eroded). This type of gap is much larger than a hairline crack. Thus, it 

is reasonable to delay erosion for lightly cracked structures, particularly if the structures are 

cycling between tension and compression (opening and closing cracks). 

During the computational review of the concrete material model, the user recommended the 

following changes: 

• Adjust fracture energies to 80 percent of the preliminary values used by the user. This 

change was made, and any reference to default values within this report refers to the 

updated fracture energies. These updated fracture energies are those documented in the 

companion to this report’s Users Manual and are in agreement with those tabulated in the 

CEB. The updated fracture energies are, however, 80 percent less than those predicted by 

the formula given in the CEB. An inconsistency appears to exist between the tabulated 
144 

values and formula documented in CEB for aggregate sizes greater than 19 mm (0.75 

inches). 

• Correction to an unrealistic increase in the concrete internal energy. This correction was 

made to the material model energy term. 

• Correction to some reporting problems associated with the long input format of the 

concrete material model. These corrections were made. The companion to this report 

Users Manual and material model printout routines reflect these changes. 

USER COMMENTS 

Numerical analyses were conducted using the newly developed LS-DYNA concrete material 

model. The analyses showed very good potential for useful application of the model in analyses 

of steel-reinforced concrete roadside safety structures. The T4 bridge rail study is a good 

example of this potential. The analyses of the T4 bridge rail alternatives provided a good 

benchmark for evaluating the strengths, sensitivity, and usability of the new concrete material 

model. Use of the pendulum tests provided more controlled impact conditions and eliminated 

many variables associated with the comparison of simulation to full-scale vehicle crash tests. 

Two specimens were tested for each design variation, providing some information regarding 

system variability. Furthermore, the two design variations demonstrated different levels of 

damage to the concrete parapet, which provided an opportunity to assess the sensitivity of the 

concrete model to small design changes under similar loading conditions. 

After adjusting the fracture energies to 80 percent of their preliminary baseline values, good 

overall correlation was achieved between the T4 bridge rail simulations and pendulum test data 

for both design alternatives investigated. The simulation matches reasonably well with respect to 

the damage profile, concrete fracture (i.e., element erosion in simulation), peak impact force, and 

acceleration-time history of the pendulum impactor. 

After calibrating the fracture energies, the simulation of the T4 bridge rail system with three-bolt 

anchorage and 254-mm- (10-inch-) wide parapet captured the punching shear failure of the 

concrete underneath the steel base plate and post. As in the pendulum tests, the concrete failure 

radiated out from the anchor bolts across the top surface of the concrete parapet and extended 

down the back side of the parapet wall. When the same material properties were used in a 

subsequent simulation of the T4 bridge rail with four-bolt anchorage and 317.5-mm- (12.5-inch-) 

wide parapet, the results again correlated with the test data. No concrete fracture was observed, 

and the damage fringes matched the pattern of hairline cracks observed in one of the test 

specimens. 

The user recommended that the default fracture energies be adjusted to levels found to provide 

damage correlation between simulations and tests. The developer followed this recommendation, 

which is available in subsequent releases of LS-DYNA 971. Results of the parametric analyses 

also indicate that element erosion should be used in conjunction with a maximum principal strain 

failure criterion (i.e., the ERODE parameter should be set greater than 1.0). The current default 

setting (ERODE = 1.1) accomplishes this recommendation. 
145 

The model is stable and has a reasonable time step. Some problems were identified with the 

energy balance associated with use of the concrete material model. As damage accumulates in 

the concrete structures, an artificial or nonphysical increase in internal energy appears to causes 

the total energy of the system to increase dramatically. This glitch was reported to the developer, 

and a fix was implemented in subsequent releases of LS-DYNA 971. 

Some reporting problems related to the long input format of the concrete material model were 

also identified. The parameter listing generated by the output routines does not correspond to the 

written documentation of the model. Details of this problem were reported to the developer, and 

corrections were made in subsequent releases of LS-DYNA 971. 

The short input format is recommended for a first cut analysis and to generate the long input 

format values. However, the user is encouraged to perform experiments to determine values that 

best fit his or her concrete data. 

All analyses reported herein were conducted using a single processor on a Linux platform 

because releases for other hardware and multiple processors were not available or were unstable. 

However, a few analyses were conducted using different platforms and multiple processors as 

some of the beta binaries became available during the course of the project. The analyses 

conducted on different platforms showed some differences in the number of eroding elements in 

the simulations involving concrete fracture. However, the differences are not considered to be 

significant or indicative of a flaw in the material model. Moreover, the eroding pattern was the 

same across all calculations for a given case. Note that erosion takes place when the damage 

value associated with a particular element exceeds a prescribed threshold (if desired by the user). 

The numerical analysis has established that different hardware platforms, roundoff errors, and 

number of processors have an influence on results consistency. This influence was observed in 

other research efforts where a sudden collapse, element erosion, and any other discontinuity 

phenomenon were numerically analyzed. Therefore, the researchers believe that these differences 

for the cases studied are not attributed to the material model but rather to other factors. 

Although the results of the evaluation of the concrete material model are encouraging, resource 

limitations precluded a more indepth evaluation of the model. Further study is recommended to 

more fully quantify the applications and limitations of the material model. The investigation of 

the New Jersey safety-shape bridge rail is incomplete due to lack of time and resources. Further 

investigation of the quasi-static load tests would be helpful. Additionally, an analysis of the 

pickup truck impact into this barrier and/or a portable concrete barrier is recommended. 

147 

CHAPTER 11. APPENDIX A. USER CODE VERIFICATION 

INTRODUCTION 

This task involved repeating the finite element calculations previously performed by the 

developer using input files supplied by the developer, and comparing the results of these 

calculations. Five models were supplied to the user by the developer. The models included a 

single element model (three load cases), concrete cylinder under tension, plain (unreinforced) 

concrete beam under impact loading, over-reinforced concrete beam under impact loading, and 

reinforced concrete beam under impact loading by surrogate vehicle. 

All the input files incorporate the new material (MAT type 159 or MAT_CSCM) to be released 

in LS-DYNA version 971. The user obtained a beta binaries release of LS-DYNA version 971 

for the following platforms/operating systems: SGI IRIX (version 971 release 1490 double 

precision ), MS-Windows (version 971 release 1612 single precision), and Linux Intel 32 bit 

architecture (version 971 release 1708 single precision). The SGI IRIX binary crashed with a 

floating point exception error during the initialization phase of reading an input file. The 

researchers believe the crash occurred because the SGI binary beta release (1490) might not be 

as “bug free” as the other binaries. 

CASE 1. SINGLE ELEMENT SIMULATIONS 

In this case, a single solid element was used to verify the basic behavior of the material model. 

There are three loading conditions for this case. The first load case was compression of the 

element as shown in Figures 148 and 149. The second load case was application of a tensile load 

to the element as shown in Figures 150 and 151. The last load case was a shear load applied on 

the element as shown in Figures 152 and 153. For each of these load conditions, the user 

calculations precisely matched the developer’s calculations as Figures 148–153 indicate. 

 
148 

psi = 145.05 MPa

Figure 148. Single element under compressive loading, developer. 

psi = 145.05 MPa

Figure 149. Single element under compressive loading, user. 
149 

psi = 145.05 MPa

Figure 150. Single element under tensile loading, developer. 

psi = 145.05 MPa

Figure 151. Single element under tensile loading, user. 
150 

psi = 145.05 MPa

Figure 152. Single element under pure shear loading, developer. 

psi = 145.05 MPa

Figure 153. Single element under pure shear loading, user. 
151 

CASE 2. CYLINDER RUNS 

This case consists of a plain unreinforced concrete cylinder subject to tensile loading. The 

tension loading was simulated by pulling both ends of the cylinder at a constant velocity. An 

inclined cross section was defined in the model to track force versus time, as shown in Figure 

154 below. 

Figure 154. Concrete cylinder model with inclined cross section. 

Fringes of the damage to the materials were plotted at various times during the analysis. The 

damage parameter plotted is the maximum of brittle and ductile damage calculated by the 

material model. It is noteworthy that damage is a normalized entity from 0 (no damage) to 1.0 

(complete damage). 

Figures 155–157 show these damage fringe plots at key times. Figures 158 and 159 show the 

cross-sectional force versus time measured on the inclined plane from the developer calculation 

and the user calculation, respectively. The user calculations matched the developer’s calculations 

in terms of both damage fringes and cross-sectional force for this model. Two binaries were used 

for this calculation; however, only the Windows results are presented because there was no 

significant difference between the computed results. 
152 

 

Figure 155. Damage fringe t = 13.498 msec. 

Figure 156. Damage fringe t = 13.598 msec. 
153 

Figure 157. Damage fringe at t = 40 msec. 

psi = 145.05 MPa

 

Figure 158. Cross-sectional force (developer). 
154 

psi = 145.05 MPa

Figure 159. Cross-sectional force (user). 

CASE 3. PLAIN CONCRETE BEAM 

In this case, an unreinforced concrete beam was modeled using the CSCM concrete model. 

Unlike previous cases, this model incorporates element erosion and contact definitions. The 

element erodes based on a set damage threshold above 0.99. Contacts were defined to represent 

surface interaction between parts (beam, impact parts, support parts, etc.). 

Damage fringes were plotted at simulation times (t) of 1, 4, 20, and 30 msec. Figures 160–163 

show the respective damage fringe plots obtained from the developer calculations for these 

simulation times. Figures 164–167 show the corresponding damage fringes plots from the user’s 

calculations using the Linux binary. Similarly, Figures 168–171 show the respective damage 

fringe plots from the user’s calculations using the Windows binary for the aforementioned 

simulation times. 

At 1 msec of simulation time, the beam was already experiencing damage as shown in Figure 

160 (developer), Figure 164 (user Linux), and Figure 168 (user Windows). The damage fringe 

from all three calculations looks very similar. Some elements were already eroded at t = 4 msec 

as shown in Figure 161 (developer), Figure 165 (user Linux), and Figure 169 (user Windows). 

Although the number of eroded elements is different among the three calculations, the fracture 

pattern is considered to be bounded within expected behavior of concrete. This same degree of 

variation in cracking patterns is observed among identical laboratory tests. 
155 

Figure 160. Plain concrete damage fringe at 1 msec (developer). 

Figure 161. Plain concrete damage fringe at 4 msec (developer). 

Figure 162. Plain concrete damage fringe at 20 msec (developer). 

Figure 163. Plain concrete damage fringe at 30 msec (developer). 
156 

Figure 164. Plain concrete damage fringe t =1 msec (user Linux). 

Figure 165. Plain concrete damage fringe t = 4 msec (user Linux). 

Figure 166. Plain concrete damage fringe t = 20 msec (user Linux). 

Figure 167. Plain concrete damage fringe t = 30 msec (user Linux). 
157 

 

Figure 168. Plain concrete damage fringe t = 1 msec (user Windows). 

Figure 169. Plain concrete damage fringe t = 4 msec (user Windows). 

 

Figure 170. Plain concrete damage fringe t = 20 msec (user Windows). 

 

Figure 171. Plain concrete damage fringe t = 30 msec (user Windows). 
158 

CASE 4. REINFORCED CONCRETE BEAM 

In this case, an over-reinforced concrete beam was modeled using the CSCM concrete model. 

The setup is similar to the model used in case 3 with the exception that beam elements are added 

to model the steel reinforcement inside the concrete beam. Both Windows and Linux binaries 

were used for conducting calculations with this model. Due to their similarity to one another, 

only one set of results (from the Linux binary) is presented in this report. Figures 172–175 show 

the damage fringes plots obtained from the developer calculations at simulation times 

corresponding to 1, 4, 16, and 20 msec, respectively. Figures 176–179 show damage fringe plots 

from the user Linux’s calculations using the same simulation times. Figures 180 and 181 show 

the displacement history plot of a node on the impacting heads using the developer and user 

calculations, respectively. 

Due to the over-reinforced nature of the beam, element erosion did not initiate in this analysis 

case. Close correlation was obtained between the user and the developer calculations for both the 

damage fringes and the displacement history of the impactor node. The minor variations that 

exist are well within the anticipated range of behavior. 
159 

Figure 172. Reinforced concrete damage fringe t = 1 msec (developer). 

 

Figure 173 Reinforced concrete damage fringe t = 4 msec (developer). 

Figure 174. Reinforced concrete damage fringe t = 16 msec (developer). 

Figure 175. Reinforced concrete damage fringe t = 20 msec (developer). 
160 

Figure 176. Reinforced concrete damage fringe t = 1 msec (user Linux). 

Figure 177. Reinforced concrete damage fringe t = 4 msec (user Linux). 

Figure 178. Reinforced concrete damage fringe t = 16 msec (user Linux). 

Figure 179. Reinforced concrete damage fringe t = 20 msec (user Linux). 
161 

mm = 0.039 inch

Figure 180. Displacement of node 49,072 in millimeters (developer). 

mm = 0.039 inch

Figure 181. Displacement of node 49,072 in millimeters (user Linux). 
162 

CASE 5. BOGIE IMPACT TESTS 

In the final case, another steel-reinforced concrete beam was modeled using the CSCM concrete 

model. The loading condition represents a bogie vehicle impacting the reinforced beam at a 

speed of 33 km/h (20.5 mi/h). Figures 182–185 show the damage fringes plots from developer 

calculations at simulation times of 4, 8, 48, and 80 msec, respectively. Figures 186–189 show 

damage fringes plots from user Windows binary calculations at these same simulation times. 

Figures 190–193 show the corresponding damage fringes plots from user Linux binary 

calculations. 

As for the beam analyzed in case 3, the damage fringes for the impacted beam in the user 

calculations developed similarly to those obtained from the developer calculations, and the 

subsequent element erosion pattern representing the cracking and failure of the beam shows 

differences for each calculation. However, the element erosion/fracture patterns are bounded 

within the same physical regions of the beam and the differences are considered to be within 

normal variability and range of behavior expected of a concrete member of this type. 
163 

 

Figure 182. Bogie damage, t = 4 msec (developer). 

Figure 183. Bogie damage t = 8 msec (developer). 

Figure 184. Bogie damage, t = 48 msec (developer). 

 

Figure 185. Bogie damage, t = 80 msec (developer). 
164 

Figure 186. Damage fringes t = 4 msec (user Windows). 

Figure 187. Damage fringe t = 8 msec (user Windows). 

 Figure 188. Damage fringe t = 48 msec (user Windows). 

 Figure 189. Damage fringe t = 80 msec (user Windows). 
165 

Figure 190. Damage, t = 4 msec (user Linux). 

Figure 191. Damage, t = 8 msec (user Linux). 

 Figure 192. Damage, t = 48 msec (user Linux). 

 Figure 193. Damage t = 80 msec (user Linux). 

167 

APPENDIX B. DEVELOPER SUPPORT OF THE TEXAS T4 BRIDGE 

RAIL ANALYSES 

INTRODUCTION 

This appendix discusses the calculations performed by the developer in support of the evaluation 

of the Texas T4 bridge rail conducted by the user. These calculations examine bridge rail 

response and deflection as a tradeoff between the concrete material properties and the spring 

material properties. They were conducted after the user explored the use of reduced fracture 

energies for concrete, but before recalibration of the spring model and adjustment of the anchor 

bolt model. They should be considered preliminary calculations, not the final result. They are 

included here to show how the calculations evolved from being overly stiff to reasonable, and to 

show the thought process involved in the effort. 

Pertinent conclusions drawn from these calculations are: 

• Approximately 85 to 90 percent of the available kinetic energy is absorbed by the 

pendulum spring and honeycomb. Therefore, a 10 percent change in pendulum energy 

absorption results in a 100 percent change in concrete energy absorption. This suggests 

that accurate models of the pendulum spring and honeycomb are needed to get accurate 

delivery of energy to the bridge rail. 

• Data-to-data comparisons indicate that the honeycomb in tests P3 through P7 is slightly 

stiffer than that in the calibration tests; therefore recalibration of the spring model was 

warranted. The developer’s approximate technique was to scale up the stiffness of the 

existing spring model, as discussed in this appendix, to correlate measured and computed 

spring/honeycomb compressions. The user’s more thorough technique was to develop a 

new spring model through correlations with test P5, as discussed in chapter 8. The 

developers data-to-data comparisons for the pendulum stiffness are not included in this 

report (but are available upon request), because the focus of this report is the concrete 

model, and not the spring/honeycomb model. 

• With use of the developer’s scaled spring model, calculated deflections correlate well 

with test P4 with 51 mm (2 inches) of rail deflection if default concrete material 

properties are used (repow = 1.0 and Gfs / Gft = 1.0). Calculated deflections correlate best 

with test P5 with 117 mm (4.6 inches) of rail deflection if slightly reduced fracture 

energies are used (repow = 0.5 and Gfs / Gft = 0.5). 

Unless otherwise specified, these calculations were performed with: 

• The original SBP spring model before recalibration with test P5. Scaling of the original 

SBP model is used to stiffen the spring in numerous calculations. 
168 

• The original anchor bolt model with nodes merged to the base plate. 

• Concrete fracture energies that are approximately 80 percent of the preliminary properties 

originally tabulated by the user. These 80 percent values are the default fracture energies 

currently implemented in LS-DYNA (at the time this report was written). They are 

referred to as the developer’s baseline properties. 

BRIDGE RAIL DATA 

The user conducted five pendulum impact tests on the Texas Department of Transportation T4 

Bridge Rail.(12) The pendulum contains a crushable nose with 10 stages of replaceable aluminum 

honeycomb cartridges. Two bridge rail designs were tested: one four-bolt design and one 

three-bolt design. The pendulum is 838 kg (1,847 lbs) and impacts the rail at a nominal velocity 

of 9,835 mm/sec (22 mi/h). The four-bolt rail experienced punching shear failure in two tests 

(designated P3 and P4). The three-bolt rail did not fail, although hairline cracks were visible in 

one of two tests (P5 and P7). A third three-bolt rail test was conducted using the previously 

tested, but undamaged rail (P6). Again, this rail did not fail, but hairline cracks were visible. Rail 

deflections and pendulum crush are listed in Table 14 for all five tests. 

Table 14. Rail deflection and pendulum crush in the Texas T4 bridge rail tests. 

Test No. Design Rail Deflection Honeycomb 

Crush 

Damage 

P3 four-bolt 117 mm 

(4.6 inch) 

417 mm 

(16.4 inch) 

Punching shear 

failure 

P4 four-bolt 51 mm 

(2.0 inch) 

414 mm 

(16.3 inch) 

Punching shear 

failure 

P5 three-bolt 15 mm 

(0.6 inch) 

439 mm 

(17.3 inch) 

None 

P6 three-bolt 33 mm 

(1.3 inch) 

295 mm 

(11.6 inch) 

Cracks 

P7 three-bolt 30 mm 

(1.2 inch) 

439 mm 

(17.3 inch) 

Cracks 

 

The honeycomb crush listed in Table 14 is for nine stages of the honeycomb, as reported in 

Buth.(12) It does not include the first stage, which is the 76-mm (3-inch) stage that impacts the 

bridge rail. In all tests, the first stage crushes nearly completely; thus, the developer suggests 

adding an additional 70 to 76 mm (2.8 to 3 inches) to the crush listed in Table 1 to get the total 

crush of all 10 honeycomb stages. 

The measured deflections vary by a factor of 2.3 for the four-bolt design. The average rail 

deflection measured in tests P3 and P4 is 81.5 mm (3.21 inches), and the standard deviation is 

43.1 mm (1.7 inches). Assuming a normal distribution, approximately 68 percent of all test 

results are expected to lie within 1 standard deviation of the mean, 95 percent within 2 standard 

deviations, and 99 percent within 3 standard deviations. Therefore 68 percent of all test results 
169 

are expected to lie between 38 and 125 mm (1.5 and 5 inches), 95 percent of all test results are 

expected to lie between 0 and 168 mm (0 and 6.1 inches) , and 99 percent of all test results are 

expected to lie between 0 and 211 mm (0 and 8.31 inches). 

PARAMETRIC STUDIES 

At the beginning of the computational effort discussed in this appendix, initial calculations 

conducted by the user correlated well with the measured deflections and damage modes of the 

three-bolt design, but not those of the four-bolt design. The four-bolt design calculations were 

stiff (less deflection and damage) relative to the test data. Therefore, the user reduced the mesh 

size (fewer elements) in order to improve the run time for parametric studies. This task was 

accomplished by removing the entire deck and fixing the nodes at the bottom of the parapet. 

The developer performed a series of parametric studies to help understand and improve the 

correlations for the four-bolt design. Studies were conducted using both the original mesh with 

the full deck and the reduced mesh with the fixed parapet. The baseline impact velocity used was 

that measured in test P3, which is 9,555.6 mm/sec (376 inches/sec), 34.4 km/h (21.375 mi/h). 

The three-bolt design was not analyzed by the developer. 

Parametric studies were conducted to examine three possible sources of excess stiffness: 

• The concrete material properties. 

• The steel reinforcement material properties. 

• The pendulum spring material properties. 

A spring element with a nonlinear force-deflection curve is used to represent nine crushable 

stages of the honeycomb. Hex elements and a honeycomb material model are used to represent 

the first stage of honeycomb that impacts the rail. The reduced finite element mesh is shown in 

Figure 194. 

Figure 194. Finite element model of the pendulum, rail, and fixed end of parapet. 
170 

The studies indicate that adjustments in the steel reinforcement properties have little effect on the 

computed response. On the other hand, adjustments in both the concrete model properties and 

pendulum spring properties have significant effects on the computed response. The tradeoffs 

between adjustments in the properties of the concrete versus pendulum spring are discussed by 

the developer in the following sections. 

Fixed Parapet Computational Results 

Damage from the baseline property calculation is shown in Figure 195. Baseline properties are 

approximately those for 30.44 MPa (4,415 lbf/inch2

) concrete with 24 mm (0.94 inches) 

maximum aggregate size. Most parametric studies examine response for variations in fracture 

energy; thus, fracture energy values are reported throughout this chapter. The baseline fracture 

energies are Gft = 0.074 N-mm with Gfs = Gf t and Gfc = 100 Gf t. Although the damage mode is 

similar to that observed in the tests, the damage is less severe. Rail deflection is approximately 

10 mm (0.4 inches), which is substantially less than the 51 mm (2 inches) and 117 mm (4.6 

inches) measured in the tests. 

Figure 195. Damage fringes calculated with baseline properties for a fixed end parapet. 

Modified Concrete Property Studies. The first parametric studies were conducted on the 

concrete material properties. These calculations indicate that an overall reduction in concrete 

properties, for example, those of concrete in the 22 to 24 MPa (3,191 to 3,481 lbf/inch2

) range, 

would produce the measured deflection. However, 22 to 24 MPa (3,191 to 3,481 lbf/inch2) is a 

much lower strength concrete than the 30.4 MPa (4,415 lbf/inch2

) used in the test. It is doubtful 

that the concrete used in the test structure could somehow be as low as 22 to 24 MPa (3,191 to 

3,481 lbf/inch2

) when the reported value is 30.4 MPa (4,415 lbf/inch2). 

For example, as a lower bound case, the four-bolt calculation was run with approximate 

properties for 20 MPa (2,901 lbf/inch2

) concrete with 8 mm (0.3 inches) aggregate (Gft = Gfs = 
171 

0.041 N-mm and Gfc = 2.03). Recall that fracture energy and stiffness decrease with a reduction 

in concrete compressive strength. Fracture energy also decreases with a reduction in aggregate 

size. With these weak and brittle properties, the rail breaks through the concrete, with no rebound 

of the pendulum. Additional calculations were performed with 26 MPa (3,771 lbf/inch2) 

concrete with fracture energies for 8 mm (0.3 inches) (Gft = 0.049 N-mm) and 24 mm (0.94 

inches) (Gft = 0.066 N-mm) aggregate. Although damage was more extensive than calculated 

with the baseline properties, the calculated deflections of 27 mm (1.06 inches) and 14 mm (0.6 

inches) are still less than measured. Also note that a 35 percent increase in tensile fracture energy 

due to aggregate size results in a computed decrease in deflection of nearly 50 percent (from 27 

mm (1.06 inches) to 14 mm (0.6 inches)). 

Energy Absorption Studies. The next parametric studies examined the amount of energy needed 

to deflect the rail 51 to 117 mm (2 to 4.6 inches) using 30.4 MPa (4,415 lbf/inch2) concrete. The 

mass and impact velocity of the pendulum set the maximum amount of energy available to be 

absorbed by the pendulum and target rail. Crushing of the pendulum honeycomb and spring 

absorbs energy. As more energy is absorbed during pendulum crush, less energy is imparted to 

the rail target. Less rail energy results in less rail deflection. 

The objective of these studies was to determine if it were possible to achieve the measured 

deflections using 30.44 MPa (4,415 lbf/inch2

) concrete if no energy were absorbed by the 

pendulum crush. These bounding calculations maximize the energy imparted to the rail by 

eliminating the energy absorbed by pendulum crush. These calculations allowed the author to 

determine the relationship between the energy absorbed by the rail and its subsequent damage 

and deflection. The boundary calculation also provided a rough estimate of the energy needed to 

computationally damage and deflect the structure in a manner consistent with that observed in 

the tests. 

All energy absorption studies were conducted using a noncrushable pendulum model and the 

fixed end parapet model. The original finite element model of the pendulum was simplified by 

removing the moveable crushable nose of the pendulum (spring and honeycomb) and replacing it 

with elastic steel. The simplified pendulum has the dimensions of the first stage of honeycomb. 

The mass of the simplified pendulum is equal to that of the original pendulum (838 kg (1,847.5 

lb)). Little or no internal energy is absorbed by the simplified pendulum model. 

Computed rail deflections as a function of kinetic energy level are given in Table 15. Six 

calculations were performed at six different pendulum impact velocities, which correspond to six 

different pendulum initial kinetic energy levels. The kinetic energy levels are listed as a 

percentage of the maximum kinetic energy available from impact with an 838 kg (1,847.5 lb) 

pendulum at a velocity of 9,555.6 mm/sec. 
172 

Table 15. Rail deflection as a function of maximum kinetic energy available. 

Kinetic Energy (%) Rail Deflection 

10 26 mm (1.02 inches) 

15 42 mm (1.7 inches) 

20 60 mm (2.4 inches) 

25 95 mm (3.7 inches) 

30 >163 mm (6.42 inches) 

100 No rebound 

 

Approximately 20 to 25 percent of the available kinetic energy is needed to deflect the rail 

between 51 and 117 mm (2 and 4.61 inches) (the measured values). At 30 percent kinetic energy, 

no rebound occurred by 100 msec (the duration of the calculation). Therefore, the deflection is 

probably infinite rather than 163 mm (6.42 inches). The deformed configuration of the structure 

for the 25 percent kinetic energy case is shown in Figure 196. 

Figure 196. The deformed configuration and damage of the Texas T4 bridge rail (four-bolt 

design) from impact with the simplified pendulum model (without a crushable nose) at 25 

percent maximum available kinetic energy is similar to that observed during the tests. 

The significance of these calculations is that the majority of available kinetic energy is absorbed 

by crush of the pendulum and not by internal energy of the structure. Small changes in the 

amount of energy absorbed by pendulum crush result in large changes in the energy absorbed by 

the structure. For example, an 11 percent change in energy absorbed by the pendulum (from 90 
173 

to 80 percent) results in a 100 percent change in energy absorbed by the structure (from 10 to 20 

percent). This level of change can make the difference between the structure appearing to be too 

stiff and the structure deflecting in the appropriate range. Therefore, accurate modeling of the 

crush and energy absorption of the pendulum spring and honeycomb is needed in order to get 

accurate delivery of energy to the target structure. 

Review of the theoretical honeycomb cartridge configurations discussed in reference 12 confirms 

that most of the available kinetic energy is expected to be absorbed by crush of the pendulum, as 

is being calculated. The available kinetic energy is approximately 38,200 kN-mm, based on the 

pendulum mass and impact velocity. If the theoretical potential energy of crush is calculated, 

based on the total crush force of each honeycomb cartridge times the thickness of each cartridge, 

a total of 49,500 kN-mm is estimated. However, honeycomb typically crushes to about 75 

percent strain, then stiffens dramatically, so the estimated crush energy is about equal to the 

available kinetic energy. 

Fracture Energy Studies. Additional concrete material property studies were conducted with the 

noncrushable pendulum model. Unlike the previously discussed studies, which examined 

different strengths of concrete, these studies examine only 30.4 MPa (4,415 lbf/inch2) concrete 

with possible modifications in baseline fracture energies. 

Four calculations were conducted with 10 percent of available impact energy. In the first 

calculation, the fracture energy was reduced from the baseline value of Gft = 0.072 N-mm to a 

low end value of Gft = 0.040 N-mm. Rail deflection increased from 26 mm (1.02 inches) to about 

35 mm (1.38 inches). In the other three calculations, the rate effect on the fracture energy was 

adjusted via the repow input parameter. This parameter scales the fracture energy in proportion 

to the theoretical increase in strength with strain rate, as discussed in the companion to this report 

Users Manual. The additional three calculations were conducted with the following parameters: 

• repow = 0 and Gft = 0.072 N-mm. 

• repow = 0 and Gft = 0.040 N-mm. 

• repow = 0 and Gft = 0.072 N-mm and Gfs = 0.5Gft. 

By default, repow = 1. With this value, if the rate effects formulation increases the strength by a 

factor of 3, the rate effects formulation will also increase the fracture energy by a factor of 3. If 

repow = 0, no increase in fracture energy is calculated; the input value is used independent of the 

strain rate. 

Calculated deflections are 36 mm (1.42 inches), 68 mm (2.68 inches), and 40 mm (1.57 inches), 

respectively. The first additional calculation indicates that removing the rate effect from the 

baseline fracture energy moderately increases deflection from 26 mm (1.02 inches) to 36 mm 

(1.42 inches), similar to the effect of reducing Gft from 0.072 to 0.040 N-mm. Reducing both 

repow and Gft has a combined effect and moves the rail deflection into the desired range. The 

third addition calculation indicates that reducing Gfs from one to one-half of Gft also has a small 

but noticeable effect on rail deflection. 

These studies indicate that it is possible to achieve the measured deflection of 51 mm (2 inches) 

to 117 mm (4.61 inches) at 10 percent of available impact energy if the tensile fracture 
174 

energies—static and dynamic—are reduced below the current default baseline values. However, 

the values needed are not necessarily realistic. For example, the fracture energy Gft = 0.072 

N-mm is the approximate default fracture energy for 30.44 MPa (4,415 lbf/inch2) concrete with 

24-mm (0.94-inch) aggregate. The fracture energy Gft = 0.040 N-mm is the approximate default 

for 20 MPa (2,901 lbf/inch2) concrete with 8-mm (0.31-inch) aggregate. The default value for 

30.44 MPa (4,415 lbf/inch2) concrete with 8-mm (0.31-inch) aggregate is Gft = 0.054 N-mm. 

These values agree with CEB tabulated values. Hence, use of Gft = 0.040 N-mm for 30.44 MPa 

(4,415 lbf/inch2) concrete is unusually brittle and outside the range of expected values. 

In general, the developer recommends a rate effect on fracture energy equivalent to repow = 1, as 

do many experienced analysts. However, some analysts suggest no rate effect. Thus, it may be 

reasonable to allow repow to drop below a value of 1. In addition, although the fracture energy in 

tension is well documented, the fracture energy in shear is not well documented. It therefore 

seems reasonable to allow the fracture energy in shear to drop below the tensile baseline value as 

well. 

Modified Spring Stiffness. It was previously concluded that the energy absorbed by crush of the 

spring and honeycomb models has a significant effect on computed response. Therefore, a series 

of parametric studies was conducted with an increase in spring stiffness. The spring is defined by 

a tabulated force versus deflection curve. The increase in stiffness is accomplished by scaling the 

tabulated deflection listing by a scale factor. The smaller the deflection scale factor, the larger 

the spring stiffness. For example, a scale factor on deflection of 80 percent results in an increase 

in spring stiffness of 125 percent (the reciprocal of 0.8). 

Results from the baseline calculation, plus 10 additional calculations, are given in Table 16. 

Results are reported as a function of the scale factor applied to the spring deflection, as well as 

the input values used for repow and the ratio Gfs/Gft (with Gft = 0.074 N-mm). Results reported 

are approximate crush energy (absorbed by spring and honeycomb), rail deflection, and 

pendulum crush (of the spring plus honeycomb). The majority of the studies were conducted 

with the 60 percent deflection scale factor because, at the time, it was not known that only 9 of 

the 10 honeycomb stages were included in the documented crush measurements. Therefore, most 

calculations were conducted to achieve a computed crush of about 417 mm (16.4 inches), the 

documented value. 
175 

Table 16. Rail deflection, pendulum crush, and crush energy as a function of spring stiffness and 

concrete properties for the fixed end parapet model. 

Spring 

Deflection 

Factor (%) 

Stiffness 

Factor 

Repow Gfs / Gft Crush 

Energy 

(%) 

Rail 

Deflection 

(mm) 

Pendulum 

Crush 

(mm) 

50 2.00 1 – 79 65 363 

60 1.00 1 1 87 41 427 

60 1.67 1 1⁄2 82 65 414 

60 1.67 1⁄2 1 84 57 418 

60 1.67 1⁄2 1⁄2 76 129 411 

60 1.67 0 1 76 ∞ 424 

60 1.67 0 1⁄2 68 ∞ 374 

70 1.43 1⁄2 1⁄2 83 76 451 

80 1.25 1⁄2 1⁄2 89 47 513 

100 1.00 0 1⁄2 95 39 568 

100 1.00 1⁄2 1⁄2 97 18 586 

100 1.00 1 1 98 10 592 

mm = 0.039 inch 

 

 

One significant point is that as the spring stiffness increases (the applied deflection scale factor 

decreases), the energy absorbed by the pendulum spring and honeycomb decreases. This is the 

desired trend because it increases the amount of energy delivered to the structure, which 

increases rail deflection. In general, pendulum crush energy absorption in the 79 to 89 percent 

range produces computed rail deflections in agreement with measured deflections. 

Stiffening of the spring also affects the calculated acceleration history. Calculated acceleration 

histories are given Figure 197. The calculated histories are plotted for the baseline calculation, as 

well as three stiffened spring calculations. The calculated trend observed is that as spring 

stiffness increases, the maximum deceleration increases, and the time to maximum deceleration 

decreases. In addition, as rail deflection increases, the “tail” on the initial triangular-shaped pulse 

also increases. In other words, the deceleration does not drop down to 0 as rapidly as it does with 

minimal rail deflection. 
176 

mm/sec = 0.039 inch/sec

Figure 197. Stiffening the spring increases the maximum deceleration and decreases the time at 

which the maximum deceleration occurs. 

As an additional sensitivity study, one calculation was conducted at 9,835 m/sec (32,267 ft/sec) 

(35.4 km/h) (22 mi/h, the nominal impact velocity) rather than 9,556 m/sec (31,352 ft/sec) (34.45 

km/h) (21.4 mi/h), the measured impact velocity). The calculation was conducted with a 60 

percent scale factor on spring deflection (1.67 on spring stiffness), using baseline properties. The 

calculated deflection is 52 mm (2.05 inches) at 35.41 km/h (22 mi/h) compared with 41 mm (1.7 

inches) at 34.45 km/h (21.4 mi/h). This is an increase in rail deflection of 27 percent for an 

increase in velocity of 2.9 percent. 

The best correlation between the measured and calculated spring compression occurs for the 

80 percent deflection scale factor case (1.25 on spring stiffness). Recall that the measured 

pendulum crush (all 10 stages) is just below 500 mm (19.7 inches). The computed compression 

of 513 mm (20.2 inches) is in reasonable agreement with this value. In addition, the 47 mm (1.9 
177 

inches) of deflection is also in reasonable agreement with the 51 mm (2 inches) of measured 

deflection reported for test P4. Figure 198 shows that the computed acceleration history is in 

good agreement with the P3 and P4 test histories throughout most of the measured response. This 

calculation was conducted with reduced properties (Gfs/Gft = 0.5 and repow = 0.5). 

mm = 0.039 inch

Figure 198. Good comparison of measured and calculated acceleration histories for the reduced 

fixed parapet mesh (spring stiffened using 80 percent deflection scale factor). 
178 

Full Deck Computational Results 

The bridge rail tested is mounted on top of a parapet, which is attached to a deck. All previously 

discussed calculations were conducted with the parapet fixed at the bottom edge, without 

inclusion of the deck. This was done to increase the runtime of the calculations so that 

parametric studies could be performed with reasonable turnaround time (overnight). Calculations 

discussed in this section were conducted with the deck modeled. 

Comparisons With and Without Deck. To start, one calculation was conducted with the full 

deck mesh using baseline properties and original spring stiffness. The calculated rail deflection is 

28 mm (1.1 inches) and the calculated spring compression is 578 mm (25.8 inches). This 

deflection is 280 percent larger than the 10 mm (0.4 inches) calculated with the fixed end 

condition previously reported in Table 16 using baseline properties and the original spring 

stiffness. Both models (full or reduced meshes) underpredict the measured deflections of 51 mm 

(2 inches) and 117 mm (4.6 inches). 

The acceleration history for a second calculation conducted with the deck explicitly modeled is 

shown in Figure 199. The computed acceleration history is compared with both the P3 and P4 

test data and with the corresponding calculation conducted with the fixed parapet end condition. 

The calculations were conducted with reduced properties (Gfs/Gft = 0.5 and repow = 0.5) and 

with the spring stiffened with the 80 percent scale factor. 

mm = 0.039 inch

 

Figure 199. Addition of the deck model improves correlations with the test data (spring stiffened 

using 80 percent deflection scale factor). 
179 

With the deck modeled, the calculated rail deflection is 87 mm (3.4 inches) and the calculated 

pendulum crush is 484 mm (19.1 inches). Without the deck modeled, the calculated rail 

deflection is 47 mm (1.9 inches) and the calculated pendulum crush is 513 mm (20.2 inches). 

Both calculations compare well with the measured P3 and P4 test results (51- and 117-mm (2- 

and 4.61-inch) deflection and 500-mm (19.7-inch) crush). However, the calculated accelerometer 

history with the deck modeled is in better agreement with the late time accelerometer 

measurements than that calculated with the fixed end condition. Hence, inclusion of the deck 

adds flexibility to the rail structure and improves correlation with the measured accelerometer 

records. 

Note that the stiffness of the adjusted spring model is based on scaling the stiffness of the 

original nonlinear spring model. Additional adjustments to the spring might improve correlations 

if the spring is made more stiff at low deflection (below about 200-mm (7.87-inch) compression) 

and made less stiff at high deflection (above about 400-mm (15.7-inch) compression). Refer 

back to Figure 197 for the original spring stiffness modeled. This type of adjustment is discussed 

in subsequent sections. 

Spring Stiffness Parameter Studies. Eleven calculations were run with the full deck mesh, as 

listed in Table 17. All were conducted at 9,555.6 mm/sec (21.375 mi/h). Three calculations were 

conducted with original spring stiffness (100 percent spring deflection scale factor), as provided 

by the user. The remainder of the calculations was calculated with a stiffened spring, using a 60 

to 90 percent scale factor on the spring deflection. 

Table 17. Rail deflection, pendulum crush, and crush energy as a function of spring stiffness and 

concrete properties for the full deck model. 

Spring 

Deflection 

Factor (%) 

Stiffness 

Factor 

Repow Gfs / Gft Crush 

Energy 

(%) 

Rail 

Deflection 

(mm) 

Pendulum 

Crush 

(mm) 

60 1.67 1 1 76 75 413 

65 1.54 1⁄2 1⁄2 74 ∞ 423 

70 1.43 1 1 83 56 461 

75 1.33 1⁄2 1⁄2 79 ∞ 464 

80 1.25 1⁄2 1⁄2 89 87 484 

80 1.25 1 1 86 44 499 

90 1.11 1⁄2 1⁄2 85 57 530 

90 1.11 1 1 90 33 541 

100 1.00 0 1⁄2 83 ∞ 550 

100 1.00 1⁄2 1⁄2 88 45 568 

100 1.00 1 1 91 28 578 

mm = 0.039 inch

Calculations conducted with a spring deflection scale factor of 80 percent are in best agreement 

with the measured pendulum crush of approximately 500 mm (19.7 inches). One of the two 

calculations was run with original baseline properties and the 80 percent scale factor on the 

spring deflection. The calculated rail deflection is 44 mm (1.73 inches) and the calculated spring 

compression is 499 mm (19.6 inches). These computed values compare well with measured 
180 

values of 51 mm (2 inches) of rail deflection and 500 mm (19.7 inches) of pendulum crush for 

test P4. The other calculation was run with reduced properties (Gfs/Gft = 0.5 and repow = 0.5) and 

the 80 percent scale factor on the spring deflection. The calculated rail deflection is 87 mm (3.43 

inches) and the calculated spring compression is 484 mm (19.1 inches). These computed values 

compare well with the average measured deflection and the 500 mm (19.7 inches) of pendulum 

crush for test P3. Hence, the baseline properties model the stiffer response associated with test 

P4, while the reduced properties (Gfs/Gft = 0.5 and repow = 0.5) model the more flexible response 

associated with the average of test P3 and test P4. 

Calculations conducted with original spring stiffness do not correlate as well with the test data as 

do the calculations with increased spring stiffness (80 percent scale factor on deflection). Using 

baseline properties, the computed rail deflection of 28 mm (1.1 inches) is lower than those 

measured in tests P3 and P4 (51 mm (2 inches) and 111 mm (4.4 inches), respectively). The 

computed pendulum crush is higher than measured (500 mm (19.7 inches) in both tests). Using 

reduced properties, the calculated rail deflection varies from 45 mm (1.8 inches) to infinity. The 

45 mm (1.78 inches) of rail deflection is in agreement with the stiffer measured value (51 mm (2 

inches)) of test P4. Property adjustments also could be made to obtain agreement with test P3 

(112 mm (4.41 inches) of rail deflection). However, the calculated pendulum crush is still larger 

than the measured value. Hence, use of reduced concrete properties with original spring stiffness 

does not correlate well with all test measurements. 

Results from Table 17 are plotted in Figure 200, along with the range in measured data. By 

examining the computed results in Table 17 and Figure 200, it is apparent that only one 

calculated rail deflection lies outside the three standard deviations range. This is the calculation 

conducted with repow reduced to 0 (which means that fracture energy is independent of rate 

effects) and Gfs / Gft = 0.5. Although not shown in Table 17, the observed trends indicate that all 

calculations, regardless of spring deflection scale factor, would produce infinite deflection with 

repow = 0 and Gfs / Gft = 0.5. This suggests that repow = 0 with Gfs / Gft = 0.5 are not appropriate 

input parameter values. The response modeled is too brittle, at least for this example problem. 

Only one calculated rail deflection lies outside the one standard deviation range, although it lies 

within the two standard deviations range. This is the calculation conducted with baseline 

properties and original spring stiffness. The calculated deflection of 28 mm (1.1 inches) is 26 

percent lower than the one standard deviation value of 38 mm (1.5 inches). This suggests that 

baseline properties are on the stiff side if original spring stiffness is assumed, but they are 

adequate if reduced spring stiffness is assumed. 

Damage fringes for two of the stiffened spring calculations (80 percent scale factor on 

deflection) are shown in Figures 201–204. The damage calculated with reduced properties 

(Gfs/Gft = 0.5 and repow = 0.5) is more severe than that calculated with baseline properties. Both 

results are similar to the post-test damage previously shown in chapter 8 for tests P3 and P4. 

Following this computational effort, data-to-data comparisons were made between the 

accelerometer records of bridge rail tests P3 through P7 with those of the rigid pole calibration 

tests. Comparisons were made for acceleration versus time, force versus deflection, energy 

absorbed versus deflection, and derived spring stiffness versus deflection. These comparisons 

indicated that the honeycomb in the calibration tests was less stiff than that in the bridge rail 
181 

tests; therefore, stiffening of the spring was warranted. Ultimately, a new stiffened spring model 

was setup by the user. 

mm = 0.039 inch

 

Figure 200. All calculations run with baseline or slightly reduced properties (repow = 0.5 and 

Gfs / Gft = 0.5) produce rail deflections within two standard deviations of the measured results. 
182 

 

Figure 201. Deflection and damage calculated with baseline properties using a stiffened spring 

(80 percent displacement scale factor). 

Figure 202. Closeup of damage calculated with baseline properties using a stiffened spring (80 

percent displacement scale factor). 
183 

 

 

Figure 203. Deflection and damage calculated with slightly reduced properties using a stiffened 

spring (80 percent displacement scale factor). 

Figure 204. Closeup of damage calculated with slightly reduced properties using a stiffened 

spring (80 percent displacement scale factor). 
184 

Impact Velocity Parameter Study. Additional full deck mesh calculations were conducted at 

9,835 mm/sec (35.41 km/h) (22 mi/h), the nominal impact velocity) rather than 9,555.6 mm/sec 

(34.4 km/h (21.4 mi/h), the measured impact velocity), as shown in Table 18 and plotted in 

Figure 205. This is an increase of roughly 1 km/h (0.62 mi/h). In general, the increase in velocity 

has a much stronger effect on the deflections computed with reduced properties than on the 

deflections produced with baseline properties. For the calculation with baseline spring and 

concrete properties, the deflection is 33 mm (1.3 inches) at 35.4 km/h (22 mi/h) 9,835 mm/sec 

compared with 28 mm (1.1 inches) at 9,555.6 mm/sec. This is an increase in rail deflection of 18 

percent for an increase in velocity of 2.9 percent and an increase in kinetic energy of 5.9 percent. 

The 33-mm (1.3-inch) computed rail deflection is close to the 38-mm (1.5-inch) deflection 

associated with 1 standard deviation. 

Table 18. Rail deflection, pendulum crush, and crush energy for calculations conducted with 

increased impact velocity (9,835 mm/sec) for the full deck model. 

Spring 

Deflection 

Factor (%) 

Stiffness 

Factor 

Repow Gfs / Gft Crush 

Energy 

(%) 

Rail 

Deflection 

(mm) 

Pendulum 

Crush 

(mm) 

60 1.67 1 1 78 95 412 

70 1.43 1⁄2 1⁄2 78 ∞ 451 

80 1.25 1 1 89 54 510 

85 1.18 1⁄2 1⁄2 83 107 510 

90 1.11 1⁄2 1⁄2 86 216 544 

100 1.00 1⁄2 1⁄2 91 62 574 

100 1.00 1 1 96 33 589 

mm = 0.039 inch
185 

 mm = 0.039 inch

Figure 205. Larger rail deflections are calculated at 9,835 mm/sec (large dots) compared with 

9,556 mm/sec (solid and large dashed lines). 

DECK TO PARAPET CONNECTION 

One final study examined how the joint is modeled between the deck and parapet. In the test 

structure, the concrete in the deck is poured separately from the concrete in the parapet. Thus, a 

joint exists between the deck and parapet. In all calculations previously discussed, this joint is 

not modeled. Instead, a tied interface firmly connects the parapet to the deck 

(CONTACT_TIED_NODES_TO_SURFACE). The developer’s experience is that this type of 

interface is more suitable for a deck and parapet that are poured at one time (without a joint), but 

it is much too strong for a joint. Therefore, two additional calculations were conducted with the 

joint explicitly modeled. This was accomplished by using an interface that allows concrete 

separation but not penetration (CONTACT_NODES_TO_SURFACE). The parapet will not 

disconnect from the deck because it is secured by steel reinforcement. 

The two calculations were conducted with baseline and reduced properties, using the spring 

stiffened with the 80 percent scale factor. With baseline properties, the effect of modeling the 

joint is to increase the calculated deflection 9 percent from 44 mm (1.7 inches) to 48 mm (1.9 
186 

inches). The calculated pendulum crush is 502 mm (19.8 inches). Damage fringes are shown in 

Figure 206. The effect of including the joint is to eliminate damage at the base of the parapet 

where it connects to the deck. With reduced properties, inclusion of the joint increases the 

calculated rail deflection from 87 mm (3.4 inches) to infinity. The rail breaks completely through 

the concrete. Maximum separation between the deck and parapet is approximately 0.36 mm 

(0.01 inches), which is not visible to the eye. 

The developer suggests that the calculations performed with the joint modeled are a better 

representation of the test structure than the calculations performed without the joint modeled. 

Both are bounding calculations. With a tied interface, the effect is to model no joint at all, as if 

the deck and parapet were one piece of continuously poured concrete. This calculation provides 

an upper bound on joint stiffness. With a separable interface, the effect is to model a joint with 

no tensile strength, as if there were no bonding of the paste from the parapet with that from the 

deck. This provides a lower bound on joint stiffness. In reality, slight bonding and tensile 

strength probably exist (but are much less than those of solid concrete). The developer’s 

recommendation is to model joints with an interface that allows for separation but not 

penetration. More sophisticated approaches might include adding tensile strength to the contact 

surface or predamage to the concrete. 

 

Figure 206. The tensile damage at the base of the parapet is eliminated if a flexible joint is 

modeled (80 percent displacement scale factor with baseline properties). 
187 

SUMMARY OF BRIDGE RAIL CALCULATIONS 

All calculations conducted with the full deck mesh produce rail deflections that lie within two 

standard deviations of the measured rail deflections using either baseline (repow = 1.0 and Gfs /

Gft = 1.0) or slightly reduced (repow = 0.5 and Gfs / Gft = 0.5) material properties for concrete. 

This is true regardless of whether the pendulum model is run with original spring stiffness or 

increased spring stiffness. However, the developer suggests that these calculations are overly 

stiff because the joint between the deck and parapet was not modeled. 

Data-to-data comparisons (not shown) indicate that the pendulum crushing stiffness in the bridge 

rail tests is greater than that in the original calibration tests. Therefore, use of a stiffened spring 

model is warranted. The spring stiffened with an 80 percent deflection scale factor (1.25 stiffness 

factor) produces spring/honeycomb compressions in agreement with those in the tests. Therefore, 

the spring with 80 percent deflection scale was chosen as the appropriate spring stiffness. All full 

deck mesh calculations conducted with the stiffened spring (80 percent scale factor on 

displacement) produce rail deflections that lie within one standard deviation of the measured rail 

deflections using either baseline or slightly reduced material properties for concrete, whether or 

not the joint is modeled. 

Without modeling the joint, the baseline properties tend to produce a response on the stiff side of 

the measured deflections, whereas the slightly reduced properties tend to produce a response 

closer to the mean measured deflection. Extremely reduced properties (repow = 0 and Gfs / Gft = 

0.5) produce infinite deflections, and therefore are not recommended for use. 

With the joint modeled, more flexibility is added to the structure. The baseline properties 

produce a response close to that of test P4. The slightly reduced properties allow the bridge rail 

to break through the concrete parapet. The developer‘s recommendation is to leave the baseline 

properties modeled as currently implemented, but to make each user aware that slightly reduced 

properties (repow = 0.5 and Gfs / Gft = 0.5) are an option that could be examined parametrically. 

189 

CHAPTER 12. REFERENCES 

1. Hargrave, M.W. and D. Smith, “Using the Computer and DYNA3D to Save Lives,” Public 

Roads Magazine, January/February 2001. 

2. Livermore Software Technology Corporation (LSTC), LS-DYNA Keyword Users Manual 

(Nonlinear Dynamic Analyses of Structures in Three Dimensions), Version 960, Volume 1, 

2001. 

3. Murray, Y.D., “Modeling Rate Effects in Rock and Concrete,” Proceedings of the 8th

International Symposium on Interaction of the Effects of Munitions with Structures, Volume 

IA, Defense Special Weapons Agency, April 1997. 

4. Murray, Y.D. and B.A. Lewis, Numerical Simulation of Damage in Concrete, APTEK 

technical report to the Defense Nuclear Agency, Contract No. DNA001-91-C-0075, Report 

No. DNA-TR-94-190, November 1995. 

5. Schwer, L.E. and Y.D. Murray, “A Three-Invariant Smooth Cap Model with Mixed 

Hardening,” International Journal for Numerical and Analytical Methods in Geomechanics, 

Vol. 18, pp. 657–688, 1994 

6. Murray, Y.D., “Users Manual for LS-DYNA Concrete Material Model 159,” Report No. 

FHWA-HRT-05-062, Federal Highway Administration, 2007. 

7. CEB-FIP Model Code 1990, Comité Euro-International du Béton, Thomas Telford House, 

1993. 

8. D.C. Alberson, W.F. Williams, W.L. Menges, and R.R. Haug. Testing and Evaluation of the 

Florida Jersey Safety Shaped Bridge Rail, Research Report 9-8132-1. Texas Transportation 

Institute, College Station, TX, February 2004. 

9. Bazant, Z.P. and J. Planas, Fracture and Size Effect in Concrete and Other Quasi-brittle 

Materials, CRC Press, ISBN 0-8493-8284-X, 1998. 

10. Oldani, E., F. Orengo, C.A. Plaxico, and M.H. Ray, Drop Tower Testing of Concrete Beams,

Worcester Polytechnic Institute Report submitted to APTEK, Inc., July 2003. 

11. Bielenberg, B.W., R.K. Faller, J.D. Reid, J.C. Holloway, J.R. Rohde, and D.L. Sicking, 

“Impact Analysis of Three Reinforced Concrete Beam Specimens,” Midwest Roadside 

Safety Facility, University of Nebraska, Report #TRP-03-130-03, submitted to APTEK, 

Inc., March 2003. 

12. Buth, E., NCHRP 350 Pendulum Test and Transition Connection Project, Letter Report for 

Project 408930, Texas Transportation Institute, College Station, TX, August 2002. 
190 

13. Zimmer, R.A. and A.G. Arnold, Calibration of the TTI 820 KG Pendulum, Texas 

Transportation Institute Report 270687, College Station, TX, June 1997. 
HRDS-04/05-07(1M)E

Recycled

Recyclable