Document

YU/DME Yeditepe University
Department of Mechanical Engineering
1
ME 266
SOLID MECHANICS LABORATORY
VIRTUAL HARDNESS TEST TUTORIAL
˘ lu.
This document was Prepared by Rıza Bayog
1
Problem Description
One of the most popular hardness tests is Rockwell B whose configuration is
shown in Fig. 1. In this test, an indenter is pressed onto the surface of the
specimen, to which a hardness number is assigned, based on the indentation
depth. The minor and major loads applied in this test are 10 kgf and 100 kgf,
respectively. The diameter of the ball indenter is 1/16 in (r = 0.8 mm).
Figure 1: Test configuration for Rockwell B testing.
The purpose of this tutorial is to show you how to perform a Rockwell B
hardness test in ADINA. Please make it habit to follow the procedures shown
here step by step. Remember that ADINA System does not require to select
any unit system. For example, if your geometry entities are in mm, and force
is in Newton, software will automatically know that your pressure unit will
be in MPa. This problem can be solved with the 900 nodes version of the
ADINA System.
1 PROBLEM DESCRIPTION
1.1
2
Model Control Data
Now, let’s adjust some control parameters in this part.
Problem heading: Choose Control =⇒ Heading, enter the heading “ADINA Hardness Test Tutorial” and click OK.
Master degrees of freedom: Choose Control =⇒ Degrees of Freedom, uncheck
the X-Translation, X-Rotation, Y-Rotation and Z-Rotation buttons and click
OK. (We perform this step because the two-dimensional solid elements that
we will use only provide stiffness for the y-translation and z-translation degrees of freedom.)
Choose Control =⇒ Time Function, adjust the parameters as indicated in
the below figure.
Choose Control =⇒ Time step, adjust the parameters as indicated in the
below figure.
1 PROBLEM DESCRIPTION
1.2
3
Analysis Assumptions
Choose =⇒ Analysis Assumptions =⇒ Kinematics and select Large Displacement and Large Strains.
1.3
Test Geometry (Solid Modeling)
Due to axisymmetry about the z-axis, our model is constructed as a 2 − D
problem. Therefore, only right side beyond the symmetry axis is modeled.
Here is a diagram showing the key geometry points used in defining this
model:
, enter the following inforTo define points, click the Define Points icon
mation into the X2, X3 columns of the table (you can leave the X1 column
blank), then click OK.
Points
1
2
3
4
5
6
X2
0
10
10
0
0.8
0
X3
0
0
10
10
10.8
10.8
Arc line: Click the Define Lines icon
, add line 1, set the Type to Arc,
set P1 to 4, P2 to 5, Center to 6 and click Save.
, add surface 1, make sure that
Surface: Click the Define Surfaces icon
the Type is set to Vertex, then use points 4, 3, 2, 1.
The graphics windows should look something like this.
2 MATERIAL PROPERTIES
2
4
Material Properties
In this tutorial, we will assume that our specimen is steel, and define material
properties given in the below table.
Material Properties
Young’s Modulus (MPa)
Yield Stress (MPa)
Strain Hardening Modulus
Poisson’s Ratio
experiment
200000
220
1700
0.3
Click the Manage Materials icon
, and click the Plastic Blinear button,
then click add. In the Define Blinear Elastic-Plastic Material dialog box, add
material 1, set the Young’s Modulus to 2E5, the Poisson’s ratio to 0.3, initial
yield stress to 220, strain hardening modulus to 1700, and click OK. Click
Close to close the Manage Material Definitions dialog box.
3
3.1
Loads and Boundary Conditions
Defining and Applying Boundary Conditions
We need only one boundary condition (B.C.) for specimen fixation (we don’t
need to use symmetry boundary conditions in this problem due to the fact
that ADINA accepts z-axis as the axisymmetry axis, and automatically takes
cares everything.
, and click the Define... button. In the Define
Click the Apply Fixity icon
Fixity dialog box, add fixity name ZT, check the Z-Translation button and
click Save. In the Apply Fixity dialog box, set the “Apply to” field to Lines.
Set the fixity for line 4 to ZT.
3.2
Defining and Applying Loads
, define and apply -1 mm displacement in the
Click the Apply Load icon
z direction to line 1, (y = 0).
4
Defining and Applying Contact
Contact Group: Click the define Contact Groups icon
1 and click OK.
, add contact group
Contact surfaces: Click the Define Contact Surfaces icon
, set the Line
number to 1 and save. Then, add contact surface number 2, set the Line
Number to 2 and click OK to close the dialog box.
Contact pair: Click the Define Contact Pairs icon
, add contact pair
number 1, set the Target Surface to 1, the Contactor Surface to 2 and click
OK.
5 MESH GENERATION
5
5.1
5
Mesh Generation
Specimen Mesh
Element group: Click the Define Element Groups icon
, add group number 1, set the Type to 2−D Solid, set the Element Subtype to Axisymmetric,
and click OK.
Subdivision data: In this mesh, we will apply mesh densities for each line in
the model.
Choose Meshing=⇒Mesh Density=⇒Line, and adjust the Number of Divisions and Length Ratio of Element Edges according to the Fig. 2.
Figure 2: Mesh densities for each model edges.
Element generation: Click the Mesh Surfaces icon
, enter 1 in the first
row of the Surface ] table, change Nodes per Element to 8 and click OK.
5.2
Target Surface Mesh
Click the Mesh Rigid Contact Surface icon
menu
in the define Contact Groups
, set the Contact Surface to 1 and click OK. Click the Show Seg-
ments Normal icon
and Show Contact Surfaces icon
. Finally, the
6 POST-PROCESSING
6
complete FE model should look similar to the Fig. 3.
Figure 3: Complete finite element model.
Generating the ADINA data file, running ADINA, loading the
porthole file:
First click the Save icon
, and save the database to file hardness tutorial. To generate the ADINA data file and run ADINA, click the Data
, set the file name to hardness tutorial, make sure that
File/Solution icon
the Run Solution button is checked and click Save.
6
Post-processing
When ADINA is finished, close all open dialog boxes. Choose Post-Processing
from the Program Module drop-down, list and discard all changes. Click the
, and open porthole file hardness tutorial. Now, you are ready
Open icon
for post processing.
Here, the report deliverables to be included in virtual part of your hardness
test report will be mentioned.
6.1
Strain Contour Plot
Obtain a contour plot of the plastic strain over the entire domain.
6.2
Contact Force Displacement Graph
Obtain the variation of contact force in the z-direction at the contact interface
as a function of displacement applied (in the z-direction).