
Department of Engineering 


The ABAQUS FAQ
5. ABAQUS  Materials
Read the relevant section in Chapter 6 : Analysis Procedures (User's manual Vol. I). This gives
an overview about the analysis and has more information about the
material properties.
Read also the following sections in Chapter 17 : Materials Introduction of
the ABAQUS User's manual.
 Section 17.1.1  Material Library : Overview
 Section 17.1.2  Material Data Definition
 Section 17.1.3  Combining Material Properties
Section 17.1.3 lists the material model combination tables. Several models
are available to define the mechanical behaviour (elastic, plastic).
Some material options require the presence of other material options. Some
exclude the use of the other material options. For example *DEFORMATION
PLASTICITY completely defines the material's mechanical behaviour and should
not be used with *ELASTIC.
Once you have all the relevant keywords to define the material properties
consult the keyword Manual for
each of the keywords. This will explain what data is required for each of
the keyword.
Referring to Section 17.1.3 of the ABAQUS User's manual you will require
the heat transfer properties as well as the electrical properties. These are listed below :
 Heat Transfer properties
 *CONDUCTIVITY
 *LATENT HEAT
 *SPECIFIC HEAT
 *HEAT GENERATION
 Electrical properties
 *DIELECTRIC
 *ELECTRICAL CONDUCTIVITY
 *JOULE HEAT FRACTION
 *PIEZOELECTRIC
This forms the complete set of properties. If Piezoelectric elements are not
used then *PIEZOELECTRIC and *DIELECTRIC properties will not be required.
If only the steady state heat transfer response is of interest then *SPECIFIC HEAT properties are not required. Similarly if there are no phase changes involved
then *LATENT HEAT is not required.
*JOULE HEAT FRACTION is used to specify the fraction of electrical energy that
will be released as heat.
Example problem 5.2.1  thermalelectrical modelling of an automotive fuse illustrates the thermalelectrical analysis.
ABAQUS allows for redundant material properties to be specified. It will simply
ignore the material properties not required for the current analysis.
Typical example of material properties :
*MATERIAL, NAME=ZINC
*CONDUCTIVITY
0.1121, 20.0
0.1103, 100.0
*ELECTRICAL CONDUCTIVITY
16.75E3, 20.0
12.92E3, 100.0
*JOULE HEAT FRACTION
1.0
*DENSITY
7.14E6
*SPECIFIC HEAT
389.0
Referring to Section 17.1.3 of the ABAQUS User's manual you will require
the heat transfer properties as well as the mechanical properties. These are listed below :
 Mechanical properties
 *ELASTIC
 Additional properties which may be required : example plastic
 Heat Transfer properties
 *CONDUCTIVITY
 *LATENT HEAT
 *SPECIFIC HEAT
 *HEAT GENERATION
Referring to Section 9.1.3 of the ABAQUS User's manual you will require the electrical properties.
These are listed below :
 Electrical properties
 *DIELECTRIC
 *ELECTRICAL CONDUCTIVITY
 *JOULE HEAT FRACTION
 *PIEZOELECTRIC
Use the concrete model available with rebar to model the reinforcements.
Section 1.1.5 of the ABAQUS Example's manual gives an example of the collapse analysis of a concrete slab subjected to a central point load.
The data file for that example is collapse example.
The complete set of ABAQUS input files can be obtained by using the following
command :
abaqus fetch j=collapseconcslab*
*CONCRETE
3000., 0. abs. value of compressive stress, abs. value of plastic strain.
5500., 0.0015 " "
*FAILURE RATIOS
1.16, 0.0836
This is used to define the shape of the failure surface (see section 11.5.1
of the ABAQUS USER's manual Vol. II).
The first parameter is the ratio of the ultimate biaxial compression stress, to the uniaxial compressive stress. Default is 1.16.
The second parameter is the absolute value of the ratio of
uniaxial tensile stress at failure to the uniaxial compressive
stress at failure. Default is 0.09.
Tension Stiffening
*TENSION STIFFENING
1., 0.
0., 2.E3
First parameter is the fraction of remaining stress to stress at cracking.
The second parameter is the absolute value of the direct strain minus
the direct strain at cracking.
This defines the retained tensile stress normal to the crack as a function
of the deformation
in the direction of the normal to the crack.
Shear Retention
*SHEAR RETENTION
Not used for this example.
Reinforcement modelling
*REBAR is used to model the reinforcement.
*REBAR,ELEMENT=SHELL,MATERIAL=SLABMT,GEOMETRY=ISOPARAMETRIC,NAME=YY
SLAB, 0.014875, 1., 0.435, 4
*REBAR,ELEMENT=SHELL,MATERIAL=SLABMT,GEOMETRY=ISOPARAMETRIC,NAME=XX
SLAB, 0.014875, 1., 0.435, 1
Here SLAB is the element name or name of the element set that
contains these rebars. The geometry is ISOPARAMETRIC. Other choice is
SKEW. ELEMENT can be BEAM, SHELL, AXISHELL or CONTINUUM type.
The following are the other parameters specified :
 crosssectional area of the rebar.
 spacing of the rebars in the plane of the shell
 position of the rebar. Distance from the reference surface. Here
the midsurface is the reference surface and the minus sign indicates
that the distance is measured in the opposite direction to the direction
of positive normal. The positive normal is defined by the right hand rule
as the nodes are considered in an anticlockwise sequence.
 edge number to which rebars are similar.
Alternate Method o modelling REBAR Reinforcements
Alternatively REBAR can be modelled as follows :
*NODE
....
....
**END NODES FOR REBAR BEAM ELEMENTS
501, 0.0, 0.15, 0.02
541, 1.5, 0.15, 0.02
601, 0.0, 0.15, 0.07
641, 1.5, 0.15, 0.07
701, 0.0, 0.60, 0.02
741, 1.5, 0.60, 0.02
801, 0.0, 0.60, 0.07
841, 1.5, 0.60, 0.07
....
....
**GENERATE INTERMEDIATE NODES
*NGEN, NSET=BAR10TF
701, 741, 2
*NGEN, NSET=BAR10TB
801, 841, 2
...
...
**GENERATE THE BEAM ELEMENTS
*ELEMENT, TYPE=B31
701, 701, 703
801, 801, 803
*ELGEN, ELSET=BAR10TF
701, 20, 2, 1, 1, 1, 1
*ELGEN, ELSET=BAR10TB
801, 20, 2, 1, 1, 1, 1
...
...
**DEFINE THE MATERIAL PROPERTIES
*MATERIAL, NAME=BAR8
**
** 8 mm dia bar
**
*ELASTIC, TYPE=ISO
197.E6, 0.3
*PLASTIC
354.E3, 0.
364.E3, 0.0018
**
**DEFINE THE SECTION PROPERTIES
...
...
*BEAM SECTION, SECTION=CIRC, MATERIAL=BAR10, ELSET=BAR10TF
0.005
*BEAM SECTION, SECTION=CIRC, MATERIAL=BAR10, ELSET=BAR10TB
0.005
...
**DEFINE AN ELEMENT SET WHICH CONTAINS
**THE ELEMENTS THROUGH WHICH THE REBAR
**ELEMENTS PASSES.
....
*ELSET, ELSET=TOP, GENERATE
5, 80, 5
**
**
*EMBEDDED ELEMENT,HOST ELSET=TOP
BAR10TF,BAR10TB
**
See section 11.2.11 of the users' manual (Vol. II). See also section 23.4.7 of
the users' manual (Vol. III), keyword section.
For example :
*DEFORMATION PLASTICITY
1.E3, 0.3, 2., 3, 0.396
Here the data line contains the Young's modulus, Poissons ratio, Yield stress,
Exponent, Yield offset respectively. If it is necessary to define the dependence
of these parameters on temperature then the 6th parameter will be the temperature.
Then repeat the dataline for different temperatures as required.
L  metres
Stress  kPa
Density  KN/m^3
Unit weight of water  Kg/m^3
Using Pascals for stress resulted in convergence problems.