This tutorial demonstrates how to simulate an uniaxial tensile test using a
standardized specimen with a defined cross-sectional area which is stretched until
fracture.
The tensile test is a standardized method of material testing to determine the yield
strength, tensile strength, elongation at break and other material parameters. It is
one of the quasi-static, destructive test methods. Figure 1.
In this lesson you will learn to:
Step1: Load the Radioss (Block) interface and load initial solver
deck
Step 2: Define material
Step 3: Define property
Step 4: Create rigid body
Step 5: Create boundary conditions
Step 6: Create imposed velocity
Step 7: Create output (time history / anim)
Step 8: Create Engine setup and export the model
Step 9: Run the model using Compute Console
Step 10: Post-process with
HyperView and HyperGraph
Model Description
UNITS: Length (mm), Time (ms),
Mass (kg), Force (kN) and Stress (GPa)
Simulation time D01 [0 –
40.]
At the right side, a constant
velocity is applied = 1 mm/ms on -X direction.
Tensile test object dimensions
= 12 x 200 with a uniform thickness = 1.7 mm
Johnson-Cook elastic plastic material /MAT/PLAS_JOHNS (Aluminum
6063 T7).
Material
Value
Initial density, [Rho_I]
2.7e-6Kg/mm3
Young's modulus, [E]
60.4 GPa
Poisson's ratio, [nu]
0.33
Yield stress, [SIGMA_Y]
0.09026 GPa
Ultimate tensile stress, [UTS]
0.175 GPa
Engineering strain at UTS, [E_UTS]
0.24
Failure plastic strain, [EPS_max]
0.75
Prerequisites
To run this simulation, you will need access to a licensed version of Radioss. You will need an internet connection to watch the
video tutorials and download the files.
Model Files
Before you begin, copy the file(s) used in this tutorial to your
working directory.
