B2000++ Materials
This part describes the materials models of B2000+++ and how to define material properties with the material command of MDL. Currently the following materials are supported:
User defined materials (requires userwritten material code).
Solid Mechanics Materials
This part describes the materials models of B2000+++ and how to define material properties with the material command of MDL.
Material type 
Description 

Linear elastic and isotropic material models for stress analysis. 

Linear elastic and orthotropic material models for stress analysis. 

Laminates and equivalentstiffnesslayer material models for stress analysis. 

Viscoelastic linear materials models for stress analysis. 

Linear and nonlinear material models for heat analysis. 

Userdefined material. 
Linear elastic materials models are supported by all stress elements (rod/cable, beam, 2D, shell, and 3D elements). Isotropic, orthotropic, and anisotropic material properties can be specified.
Linear Elastic Isotropic Material
Linear elastic isotropic materials are supported by all stress elements (rod/cable, beam, 2D, shell, and 3D elements).
MDL Material Specification
material id type isotropic
E <float>
[nu <float>]
[alpha <float>]
[failure ... end]
[density <float>]
end
MDL Parameters
E <float>
Specifies the modulus of elasticity
E
.nu <float>
Specifies Poisson’s ratio
nu
. Default is 0.alpha <float>
Specifies the thermal expansion coefficient. Default is 0.
failure ... end
Specifies a Solid Mechanics Failure Criteria criterion (optional).
density <float>
Specifies the material density. Default is 0.
Linear Elastic Orthotropic Material
Linear elastic orthotropic material models are supported by all 2D, shell, and 3D stress elements). Depending on the element, not all material constants need to be specified.
MDL Material Specification
material id type orthotropic
[planestrain]
E1 <float> E2 <float> E3 <float>
nu12 <float> nu13 <float> nu23 <float>
g12 <float> g13 <float> g23 <float>
[alpha11 <float> alpha22 <float> alpha33 <float> alpha12 <float> alpha13 <float> alpha23 <float>]
[failure ... end]
[density <float>]
end
MDL Parameters
E1 <float> E2 <float> E3 <float>
Specifies the moduli of elasticity in the material directions 1, 2, and 3. All 3 constants are required.
planestrain
Specifies planestrain elasticity. For 2D elements, default is planestress. Is ignored by non2D elements (shell elements are always planestress, and 3D elements are neither planestrain nor planestress).
nu12 <float> nu13 <float> nu23 <float>
Specifies Poisson’s ratio relating the different material directions. Shell elements and 2D elements make use of
nu13
andnu23
for the planestress and planestrain (2D elements only) conditions, respectively. All 3 constants are required.g12 <float> g13 <float> g23 <float>
Specifies the shear modulus. 2D elements will ignore
g13
andg23
. All 3 constants are required.alpha11 <float> alpha22 <float> alpha33 <float> alpha12 <float> alpha13 <float> alpha23 <float>
Specifies the thermal expansion coefficients. Default is 0. 2D elements will ignore
alpha33alpha13alpha23
.
failure ... end
Specifies a Solid Mechanics Failure Criteria (optional).
density <float>
Specifies the material density
density
. Default is 0.
Example:
material 1 type orthotropic
e1 124000.0
e2 9000.0
nu12 0.3
g12 5100.0
g13 5100.0
g23 5000.0
density 1.53e3
end
Orthotropic strainstress relation
The strainstress (compliance) relation of a linear elastic orthotropic 3D material is defined as follows:
The strainstress (compliance) relation of a linear elastic orthotropic 2D material is defined as follows:
Linear Elastic ortho25 Material
The “ortho25” (twoandahalf dimensions) material is applied to laminates, where the shear in the element normal direction has to be taken into account.
MDL Material Specification
material id type ortho25
e1 <float> e2 <float>
nu12 <float> nu13 <float> nu23 <float>
g12 <float> g13 <float> g23 <float>
[alpha11 <float> alpha22 <float>]
[failure ... end]
[density <float>]
end
mid 6 # m1
type ortho25
e1 1.473000e+05 e2 1.180000e+04
p1 3.000000e01
g1 6.000000e+03 g2 3770 g3 6000
MDL Parameters
E1 <float> E2 <float>
Specifies the moduli of elasticity in the material directions 1 and 2. Required.
nu12 <float>
Specifies Poisson’s ratio inplane. Required.
g12 <float> g13 <float> g23 <float>
Specifies the shear moduli. All 3 constants are required.
alpha11 <float> alpha22 <float>
Specifies the thermal expansion coefficients. Optional.
failure ... end
Specifies a Solid Mechanics Failure Criteria (optional).
density <float>
Specifies the material density
density
. Default is 0.
Example
Laminate material definition from verification case psc5.
material 1
type ortho25
e1 1.473000e+05 e2 1.180000e+04
p1 3.000000e01
g1 6.000000e+03 g2 3770 g3 6000
end
Hyperelastic materials models are provided with B2000++ Pro and are supported by 2D and 3D elements.
Linear Elastic Anisotropic Material
Linear elastic anisotropic material models are supported by all shell and 3D stress elements.
MDL Material Specification
material id type anisotropic
[planestrain]
c1111c1122c1133c1112c1113c1123
c2222c2233c2212c2213c2223
c3333c3312c3313c3323
c1212c1213c1223
c1313c1323
c2323
[alpha11 <float> alpha22 <float> alpha33 <float> alpha12 <float> alpha13 <float> alpha23 <float>]
[failure ... end]
[density <float>]
end
MDL Parameters
planestrain
Specifies planestrain elasticity. For 2D elements, default is planestress. Is ignored by non2D elements (shell elements are always planestress, and 3D elements are neither planestrain nor planestress).
cijkl <float>
Specifies an entry in the constitutive matrix. Default is 0 for all entries.
alpha11 <float> alpha22 <float> alpha33 <float> alpha12 <float> alpha13 <float> alpha23 <float>
Specifies the thermal expansion coefficients. Default is 0. 2D elements will ignore
alpha33alpha13alpha23
.
failure ... end
Specifies a Solid Mechanics Failure Criteria criterion (optional).
density <float>
Specifies the material density
density
. Default is 0.
Laminates
Laminates are supported by shell elements and by hexahedral and prismatic 3D elements.
MDL Material Specification
material id type laminate
t al id
t al id
...
end
The plies of the laminate are arranged in the element thickness
direction from the bottom surface to the top surface, with the first
ply located at the bottom and the last ply located at the top. Each
ply must specify the ply thickness t
, the angle of rotation al
(in degrees), and the material identifier id
of the layer. The
angle of rotation is specified around the element surface, according
to the righthand rule (see figure below).
Note
See additional information in the Special Topics Section Laminates.
ABD Material
The ABD material model is a linear equivalentstiffnesslayer material model for shell analysis with the plane stress assumption. It allows to directly specify the A,B,D matrices from classical laminate theory. It is supported by all shell elements.
MDL Material Specification
material id type abd
membrane_matrix [ <C1111> <C1122> <C1112> <C2222> <C2212> <C1212> ]
bending_matrix [ <C1111> <C1122> <C111>2 C2222> <C2212> C1212> ]
coupling_matrix [ <C111>1 <C1122> <C1112> <C2222> <C2212> <C1212> ]
transverse_shear_matrix [ <C1313> <C2313> <C2323> ]
membrane_alpha [<A11> <A22> <A12>]
bending_alpha [<A11> <A22> <A12>]
mass <float>
end
membrane_matrix [ <C1111> <C1122> <C1112> <C2222> <C2212> <C1212> ]
Specifies the components
Cijkl
of the upper part of the symmetric 3x3 matrix of the membrane shell section stiffness. It corresponds to the Amatrix of classical laminate theory.
bending_matrix[ <C1111> <C1122> <C111>2 C2222> <C2212> C1212> ]
Specifies the upper part of the symmetric 3x3 matrix of the bending shell section stiffness. It corresponds to the Dmatrix of classical laminate theory.
coupling_matrix[ <C111>1 <C1122> <C1112> <C2222> <C2212> <C1212> ]
Specifies the upper part of the symmetric 3x3 membranebending coupling matrix. It corresponds to the Bmatrix of classical laminate theory.
transverse_shear_matrix [ <C1313> <C2313> <C2323> ]
Specifies the upper part of the symmetric 2x2 matrix containing the transverseshear shell section stiffnesses. It is required by sheardeformable shell elements such as the MITC elements. This matrix must incorporate the shear correction factor. For example, with isotropic materials, the two diagonal elements would have a value of \(\frac{5}{6}\frac{Et}{2(1+\nu)}\) where \(t\) is the shell thickness, \(E\) the modulus of elasticity, and \(\nu\) Poisson’s ratio.
membrane_alpha [<A11> <A22> <A12>]
Specifies the thermal expansion coefficients for the membrane components of the strain tensor.
bending_alpha [<A11> <A22> <A12>]
Specifies the thermal expansion coefficients for the bending components of the strain tensor.
mass <float>
Specifies the mass per unit area.
All shell elements are assumed to have a thickness of 1 and an eccentricity of 0, regardless of what is specified otherwise. Hence, the matrices are not scaled by a thickness, instead, they are utilized as is specified.
The material law is as follows:
where \(\Delta T\) is the difference between the interpolated temperature to the reference temperature (see the MDL temperatures command). It is evaluated at the shell midsurface (it is the average of the values at the bottom and top shell surface).
The inlayer strains and stresses are not calculated and are not
written to the database. Instead, the shell section strains, expressed
in the material reference frame, are stored in the
STRAIN_SHELL_MATERIAL
dataset, with the
components aligned with the ABD material matrix. The shell section
stresses, also expressed in the material reference frame, are stored
in the STRESS_SHELL_MATERIAL
dataset Field.
PSHELL Material
The PSHELL material model is a linear equivalentstiffnesslayer material model for shell analysis with the plane stress assumption. It is supported by all shell elements. Its purpose is to provide compatibility with FE models that were created for Nastran.
MDL Material Specification
material id type pshell
[membrane_mid mid]
[bending_mid mid]
[tranverse_shear_mid mid]
[coupling_mid mid]
[bending_scale_factor f]
[shear_correction_factorvf]
[thickness t]
[non_structural_mass m]
end
The MITC elements are ReissnerMindlin shell elements and as such require a nonzero but finite transverseshear stiffness. The B2000++ implementation of PSHELL ensures this: If no material id for the transverse shear is given, transverseshear stiffness will be derived from the membrane material. If no membrane material is specified, transverseshear stiffness will be derived from the bending material.
According to Nastran conventions, the transverse shear stiffness is
extracted as follows according to the type of material: For isotropic
materials, g
is used. For orthotropic materials, g13
and g23
are used. For anisotropic materials, the submatrix
[[C1111,C1122],[C1122,C2222]]
is used.
If no thickness is specified for the PSHELL material, a thickness for the shell element must be specified. The thickness is used to scale the membrane matrix and the transverse shear stiffnesses by \(t\) and the bending matrix by \(\frac{t^{3}}{12}\). The coupling matrix is not scaled.
To account for nonhomogeneous materials, the bending_scale_factor
(default 1) can be modified.
The shear_correction_factor
(default 5/6) should not be set to zero.
MooneyRivlin Material Model
The nonlinear hyperelastic MooneyRivlin material model is suited for finite strain analysis of rubberlike isotropic materials. The elastic potential includes a hydrostatic work term. This material model is supported by 2D and 3D elements.
MDL Material Specification
material id type mooney_rivlin
c1 <float>
[c2 <float>]
kappa <float>
[alpha <float>]
[failure ... end]
[density <float>]
end
MDL Parameters
c1c2 <float>
Specifies the MooneyRivlin material constants. If
c2
is not specified, it will be assumed 0, in which case a NeoHookean material is described.kappa <float>
Specifies the bulk modulus.
alpha <float>
Specifies the thermal expansion coefficient. Default is 0.
failure ... end
Specifies a Solid Mechanics Failure Criteria criterion (optional).
density <float>
Specifies the material density. Default is 0.
Alternatively, the elastic modulus e and Poisson’s ratio nu may be specified instead of the MooneyRivlin coefficients c1, c2, and kappa. In this case, the MooneyRivlin material constants will be calculated from e and nu.
Generalised BlatzKo Material Model
The nonlinear hyperelastic generalized BlatzKo material model is suited for finite strain analysis of foamrubber materials. The elastic potential includes a hydrostatic work term. This material model is supported by 3D elements.
MDL Material Specification
material id type blatz_ko
g <float>
nu <float>
[f <float>]
[alpha <float>]
[failure ... end]
[density <float>]
end
MDL Parameters
g <float>
Specifies the shear modulus.
nu <float>
Specifies Poisson’s ratio.
f <float>
Specifies the volumefraction of voids in the foamrubber material. Default is 0.5.
alpha <float>
Specifies the thermal expansion coefficient. Default is 0.
failure
Specifies a Solid Mechanics Failure Criteria criterion (optional).
density <float>
Specifies the material density. Default is 0.
Alternatively, the elastic modulus e may be specified instead of the shear modulus g.
Viscoelastic Isotropic Material
The viscoelastic material models is an elastic isotropic material with dynamic material damping properties according to the Generalized Maxwell Model (GMM):
Viscoelastic material models are supported by shell and 3D elements and assume small strains.
MDL Material Specification
material id type viscoelastic_isotropic
e <float>
nu <float>
g <float>
relative_moduli flist
relaxation_times flist
[volumetric yesno]
[instantaneous_elasticity yesno]
[alpha <float>]
[density <float>]
end
MDL Parameters
e <float>
Specifies the modulus of elasticity.
nu <float>
Specifies Poisson’s ratio. Default is 0.
relative_moduli flist
Specifies the values of the relative moduli of the GMM elements. The number of values must be identical to those in
relaxation_times
.relaxation_times flist
Specifies the relaxation times for the GMM elements. The number of values must be identical to those in
relative_moduli
.volumetric yesno
Specifies if the components refer to volumetric tensor or not. Default is
yes
. Ifno
is specified, the volumetricdeviatoric split is performed, and the viscous damping is performed only on the deviatoric components.instantaneous_elasticity yesno
Specifies if the relaxation function assumes instantaneous elasticity. Default is
yes
(creep). Ifno
is specified, viscous damping is performed.alpha <float>
Specifies the thermal expansion coefficient. Default is 0.
failure ... end
Specifies a Solid Mechanics Failure Criteria criterion (optional).
density <float>
Specifies the material density. Default is 0.
Viscoelastic Orthotropic Material
The viscoelastic orthotropic material model is an elastic orthotropic material with dynamic material damping properties according to the Generalized Maxwell Model (GMM) (see Schematic representation of Maxwell model) and it is supported by shell and 3D elements and assumes small strains.
MDL Material Specification
material id type viscoelastic_orthotropic
e1e2e3 <float>
nu12nu13nu23 <float>
g12g13g23 <float>
relative_moduli_ij flist
relaxation_times_ij flist
[volumetric yesno]
[instantaneous_elasticity yesno]
[alpha11alpha22alpha33alpha12alpha13alpha23 <float>]
[density <float>]
end
MDL Parameters
e1e2e3 <float>
Specifies the modulus of elasticity in the material directions. If
e
is specifiednu12nu13nu23 <float>
Specifies Poisson’s ratio relating the different material directions. Shell elements make use of
nu13
andnu23
for the planestress condition.g12g13g23 <float>
Specifies the shear modulus.
relative_moduli_ij flist
Specifies the values of the relative moduli of the GMM elements in the material direction ij (11, 22, 33, 12, 13, 23). The number of values must be identical to those in
relaxation_times
.relaxation_times_ij flist
Specifies the relaxation times for the GMM elements in the material direction ij (11, 22, 33, 12, 13, 23). The number of values must be identical to those in
relative_moduli_ij
.volumetric yesno
Specifies if the components refer to volumetric tensor or not. Default is
yes
. Ifno
is specified, the volumetricdeviatoric split is performed, and the viscous damping is performed only on the deviatoric components.instantaneous_elasticity yesno
Specifies if the relaxation function assumes instantaneous elasticity. Default is
yes
(creep). Ifno
is specified, viscous damping is performed.alpha11alpha22alpha33alpha12alpha13alpha23 <float>
Specifies the thermal expansion coefficients. Default is 0.
failure ... end
Specifies a Solid Mechanics Failure Criteria criterion (optional).
density <float>
Specifies the material density. Default is 0.
Theoretical Background
The convolution integral of the constitutive equation of a generalized Maxwell element for a linear initial material and infinitesimal (‘small’) strain is
and the normalized relaxation functions are defined as
\(\tau_{i}\) is the relaxation time and \(\gamma_{i}\) the relative modulus of the i^{th} out of \(N\) Maxwell elements.
This model is sometimes extended with an additive split of the strain as
a deviatoric and a volumetric strain with a different constitutive
equation for each part of the strain (option volumetric no
). This is
justified for nearly incompressible materials like some polymeric
materials where the bulk response is only elastic and the deviatoric
response is viscoelastic. The material model assumes ‘small’ strains,
which is justified for metallic or composite materials.
The relaxation function as reported above assumes instantaneous
elasticity. If not (parameter instantaneous_elasticity
set to
no
), then the relaxation function g is defined as:
Staverman and Schwarz [Staverman52] gave the expression of the free energy for a generalized Maxwell element in one dimension. Piero and Deseri [Piero96] generalized this expression to threedimensional linear viscoelasticity. The free energy \(F\) of the generalized Maxwell element is
Using the thermodynamic equation
\(T_{0}\) is the constant temperature and \(\Theta\) the entropy production. By differentiating with respect to the time we obtain the rate of dissipated energy \(D = {T_{0}\Theta}\)
Solid Mechanics Failure Criteria
Failure indices are evaluated on a per element base whenever the element material refers to on of the failure criteria described in this section.
Maximum Principal Stress Failure Criterion
With the maximum pricipal stress \(\sigma_i\) failure criterion failure is said to occur if
The maximum principal stress failure criterion (Rankine) is intended for brittle materials. In plane stress Failure will occur if
MDL Failure Criterion Specification within Material Block
failure max_principal_stress
t <float>
c <float>
s <float>
filter max_of_element
fi_min <float>
end
MDL Failure Criterion Parameters
t <float>
Specifies the maximum tensile yield stress, that is, the maximum value of the largest of the 3 principal stresses.
c <float>
Specifies the maximum compressive yield stress, that is, the minimum value of the smallest of the 3 principal stresses.
s <float>
Specifies the maximum shear stress.
filter max_of_element
Specifies that for each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index. This option significantly reduces gradient storage requirements and is recommended for use with large meshes with layered materials, where the total amount gradient data can be very large.
fi_min <float>
Specifies the minimum failure index which is required to store the evaluated failure criterion in the database (B2000++). Default is 0.0, which means that storage is always performed. A value of 0.25 means that storage is performed only when the failure index is greater than or equal to 25%.
In addition to the FAILURE_INDEX
dataset, the values of the
failure criterion evaluated at the element integration points are stored
in the FC_MAX_PRINCIPAL_STRESS
dataset. For each element
integration point, the maximum failure index, the corresponding
marginofsafety, the number of the failure mode (“component”) are
stored, and the failure indices for the tensile, compressive, and shear
stresses are stored. The convention is such that a failure mode of 1
corresponds to the tensile stress, a failure mode of 2 corresponds to
the compressive stress, and a failure mode of 3 to the shear stress.
Example
material 1 type isotropic
# Aluminium 2024T3
e 72400. # [MPa]
nu 0.33
density 2.8e9 # [t/mm^3]
alpha 22.8e6 # [1/K]
failure max_principal_stress
t 138.0 # [MPa]
c 138.0 # [MPa]
s 138.0 # [MPa]
end
end
Maximum Stress Failure Criterion
A linear criterion based on tension, compression and shear stress. Failure occurs when
MDL Failure Criterion Specification within Material Block
failure max_stress
t <float> (t1 <float> t2 <float> t3 <float>)
c <float> (c1 <float> c2 <float> c3 <float>)
s <float> (s12 <float> s23 <float> s13 <float>)
filter max_of_element
fi_min <float>
end
MDL Failure Criterion Parameters
t <float> (t1 <float> t2 <float> t3 <float>)
Specifies the value of the tension failure stresses.
t1
is defined in the material direction 1,t2
in the material direction 2, andt3
in the material direction 3. Except for planestress conditions, wheret3
can be omitted, all parameters must be specified and positive. Specification oft
impliest1 t2 t3 t
.c <float> (c1 <float> c2 <float> c3 <float>)
Specifies the value of the compressive failure stresses.
c1
is defined in the material direction 1,c2
in the material direction 2, andc3
in the material direction 3. Except for planestress conditions, wherec3
can be omitted, all parameters must be specified and positive. Specification ofc
impliesc1 c2 c3 c
.s <float> (s12 <float> s23 <float> s13 <float>
Specifies the value of the shear failure stresses. Except for planestress conditions, where
s23
ands13
can be omitted, all parameters must be specified and positive. Specification ofs
impliess12 s23 s13 s
.filter max_of_element
Specifies that for each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index. This option significantly reduces gradient storage requirements and is recommended for use with large meshes with layered materials, where the total amount gradient data can be very large.
fi_min <float>
Specifies the minimum failure index which is required to store the evaluated failure criterion in the database (B2000++). Default is 0.0, which means that storage is always performed. A value of 0.25 means that storage is performed only when the failure index is greater than or equal to 25%.
In addition to the FAILURE_INDEX
dataset, the values of the
failure criterion evaluated at the element integration points are
stored in the FC_MAX_STRESS
dataset. For each element integration
point, the maximum failure index, the corresponding marginofsafety,
and the number of the failure mode (“component”) are stored. Note that
the components of the stress tensor must be arranged in the sequence
[Sxx, Syy, Szz, Sxy, Syz, Sxz]
and that a failure mode of 1 corresponds to the first stress component, a failure mode of 2 corresponds to the second stress component, etc.
Example:
material 1 type isotropic
# Aluminium 2024T3
e 72400. # [MPa]
nu 0.33
density 2.8e9 # [t/mm^3]
alpha 22.8e6 # [1/K]
failure max_stress
t 138.0 # [MPa]
c 138.0 # [MPa]
s 138.0 # [MPa]
end
end
Maximum Principal Strain Failure Criterion
With the maximum pricipal strain \(\epsilon_i\) failure criterion failure is said to occur if
MDL Failure Criterion Specification within Material Block
failure max_principal_strain
t <float>
c <float>
s <float>
filter max_of_element
fi_min <float>
end
MDL Failure Criterion Parameters
t
Specifies the maximum tensile strain, that is, the maximum value of the largest of the 3 principal strains.
c <float>
Specifies the maximum compressive strain, that is, the minimum value of the smallest of the 3 principal strains.
s <float>
Specifies the maximum shear strain.
filter max_of_element
Specifies that for each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index. This option significantly reduces gradient storage requirements and is recommended for use with large meshes with layered materials, where the total amount gradient data can be very large.
fi_min <float>
Specifies the minimum failure index which is required tostore the evaluated failure criterion in the database. The default is 0.0, which means that storage is always performed. A value of 0.25 means that storage is performed only when the failure index is greater than or equal to 25%.
In addition to the FAILURE_INDEX
dataset, the values of the
failure criterion evaluated at the element integration points are stored
in the FC_MAX_PRINCIPAL_STRAIN
dataset. For each element
integration point, the maximum failure index, the corresponding
marginofsafety, the number of the failure mode (“component”) are
stored, and the failure indices for the tensile, compressive, and shear
strains are stored. The convention is such that a failure mode of 1
corresponds to the tensile strain, a failure mode of 2 corresponds to
the compressive strain, and a failure mode of 3 to the shear strain.
Example:
material 1 type isotropic
# Aluminium 2024T3
E 72400. # [MPa]
nu 0.33
density 2.8e9 # [t/mm^3]
alpha 22.8e6 # [1/K]
failure max_principal_strain
t +4500.e6
c 3000.e6
s +5000.e6
filter max_of_element
end
end
Maximum Strain Failure Criterion
A linear criterion based on tension, compression and shear strain. Failure occurs when
MDL Failure Criterion Specification within Material Block
failure max_principal_strain
tt1t2t3 <float>
cc1c2c3 <float>
ss12s23s13 <float>
filter max_of_element
fi_min <float>
end
MDL Failure Criterion Parameters
tt1t2t3 <float>
Specifies the value of the tension failure strains.
t1
is defined in the material direction 1,t2
in the material direction 2, andt3
in the material direction 3. Except for planestrain conditions, wheret3
can be omitted, all parameters must be specified and positive. Specification oft
impliest1=t2=t3=t
.cc1c2c3 <float>
Specifies the value of the compressive failure strains.
c1
is defined in the material direction 1,c2
in the material direction 2, andc3
in the material direction 3. Except for planestrain conditions, wherec3
can be omitted, all parameters must be specified and positive. Specification ofc
impliesc1=c2=c3=c
.ss12s23s13 <float>
Specifies the value of the shear failure strains. Except for planestrain conditions, where
s23
ands13
can be omitted, all parameters must be specified and positive. Specification ofs
impliess12=s23=s13=s
. The shear strengths should be given as true strains (not as engineering strains, that is, not multiplied by 2).filter max_of_element
Specifies that for each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index. This option significantly reduces gradient storage requirements and is recommended for use with large meshes with layered materials, where the total amount gradient data can be very large.
fi_min <float>
Specifies the minimum failure index which is required tostore the evaluated failure criterion in the database. The default is 0.0, which means that storage is always performed. A value of 0.25 means that storage is performed only when the failure index is greater than or equal to 25%.
In addition to the FAILURE_INDEX
dataset, the values of the
failure criterion evaluated at the element integration points are
stored in the FC_MAX_STRAIN
dataset. For each element integration
point, the maximum failure index, the corresponding marginofsafety,
and the number of the failure mode (“component”) are stored.
Von Mises Failure Criterion
Specifies the von Mises failure criterion for the current material.
MDL Failure Criterion Specification within Material Block
failure von_mises
r <float>
filter max_of_element
fi_min <float>
end
MDL Failure Criterion Parameters
r <float>
Specifies the von Mises equivalent stress strength value for the (isotropic) strength for tension, compressive, and shear. This parameter is required and must be positive. Setting``r`` to 1.0 will produce the von Mise sequivalent stress instead.
filter max_of_element
Specifies that for each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index. This option significantly reduces gradient storage requirements and is recommended for use with large meshes with layered materials, where the total amount gradient data can be very large.
fi_min <float>
Specifies the minimum failure index which is required to store the evaluated failure criterion in the database. The default is 0.0, which means that storage is always performed. A value of 0.25 means that storage is performed only when the failure index is greater than or equal to 25%.
In addition to the FAILURE_INDEX
dataset, the values of the
failure criterion evaluated at the element integration points are
stored in the FC_VON_MISES
dataset. For each element integration
point, the maximum failure index and the corresponding
marginofsafety are stored.
TsaiWu Failure Criterion
Specifies the TsaiWu failure criterion for the current material.
MDL Failure Criterion Specification within Material Block
failure tsai_wu
tt1t2t3 <float>
cc1c2c3 <float>
ss12s23s13 <float>
f12i <float>
f13i <float>
filter max_of_element
fi_min <float>
end
MDL Failure Criterion Parameters
tt1t2t3 <float>
Specifies the value of the tension failure stresses.
t1
is defined in the material direction 1,t2
in the material direction 2, andt3
in the material direction 3. Except for planestress conditions, wheret3
can be omitted, all parameters must be specified and positive. Specification oft
impliest1=t2=t3=t
.cc1c2c3 <float>
Specifies the value of the compressive failure stresses.
c1
is defined in the material direction 1,c2
in the material direction 2, andc3
in the material direction 3. Except for planestress conditions, wherec3
can be omitted, all parameters must be specified and positive. Specification ofc
impliesc1=c2=c3=c
.ss12s23s13 <float>
Specifies the value of the shear failure stresses. Except for planestress conditions, where
s23
ands13
can be omitted, all parameters must be specified and positive. Specification ofs
impliess12=s23=s13=s
.f12if23i <float>
Specifies the TsaiWu interaction coefficients (in the range of [1, 1)].
filter max_of_element
Specifies that for each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index. This option significantly reduces gradient storage requirements and is recommended for use with large meshes with layered materials, where the total amount gradient data can be very large.
fi_min <float>
Specifies the minimum failure index which is required to store the evaluated failure criterion in the database. The default is 0.0, which means that storage is always performed. A value of 0.25 means that storage is performed only when the failure index is greater than or equal to 25%.
In addition to the FAILURE_INDEX
dataset, the values of the
failure criterion evaluated at the element integration points are
stored in the FC_TSAI_WU
dataset. For each element integration
point, the maximum failure index and the corresponding
marginofsafety are stored.
Hashin Failure Criterion
Specifies the [Hashin80] failure criterion for the current material. This failure criterion is intended for transversely isotropic materials. For a consistent response when \(\sigma_{11}\) is almost zero, the shear stresses \(\tau_{12}\) and \(\tau_{23}\) are not used to detect fiber tensile failure, that is, \({fi1+} = \frac{\sigma_{11}}{t1}\).
MDL Failure Criterion Specification within Material Block
failure max_principal_stress
t <float>
c <float>
s <float>
filter max_of_element
fi_min <float>
end
MDL Failure Criterion Parameters
inplane yesno
If set to yes, assume a plane stress state and use the plane stress failure criterion rather than the 3D failure criterion which is the default.
t1 <float>
The axial tensile failure stress.
c1 <float>
The axial compressive failure stress.
t2 <float>
The transverse tensile failure stress.
c2 <float>
The transverse compressive failure stress.
s12 <float>
The axial shear failure stress.
s23 <float>
The transverse shear failure stress. If not available from material data, it can be obtained, assuming pure compressive and an angle of 53 degrees for the fracture surface, using equation 68: \({s23} = 0.378*{c2}\), see [Larc04].
filter max_of_element
Specifies that for each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index. This option significantly reduces gradient storage requirements and is recommended for use with large meshes with layered materials, where the total amount gradient data can be very large.
fi_min <float>
Specifies the minimum failure index which is required to store the evaluated failure criterion in the database. The default is 0.0, which means that storage is always performed. A value of 0.25 means that storage is performed only when the failure index is greater than or equal to 25%.
In addition to the FAILURE_INDEX
dataset, the values of the
failure criterion evaluated at the element integration points are
stored in the FC_HASHIN
dataset. For each element integration
point, the maximum failure index, the corresponding marginofsafety,
and the number of the failure mode (“component”) are stored: 1 means
fiber tensile, 2 fiber compressive, 3 matrix tensile, and 4 means
matrix compressive.
Example:
material 1 type orthotropic
# T300/1034C graphite/epoxy, units in [MPa]
e1 146.86e+03
e2 11.376e+03
e3 11.376e+03
nu12 0.3
nu13 0.3
nu23 0.3
g1 6.186e+03
g2 6.186e+03
g3 6.186e+03
failure hashin
t1 1730.0
t2 66.5
c1 1379.0
c2 268.2
s12 133.763
s23 101.4
end
end
LaRC04 Failure Criterion
Specifies the LaRC04 failure criterion for the current material. It is implemented as a plane stress failure criterion according to Maimi et.al [mcmd06], rather than according to the original LaRC04 description [Larc04], which describes a 3D failure criterion.
MDL Failure Criterion Specification within Material Block
failure larc04
parameters
end
MDL Failure Criterion Parameters
t1t2 <float>
Specifies the values of the inplane tensile strengths. Both parameters must be specified and must be positive.
c1 <float>
Specifies the value of the inplane compressible strength in xdirection. Must be specified and must be positive.
s12 <float>
Specifies the value of the inplane shear strength. Must be specified and must be positive.
g12g2p <float>
Specifies the values of the fracture toughness parameters.
g12
must be specified whileg2p
may be omitted. All specified values must be positive.filter max_of_element
Specifies that for each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index. This option significantly reduces gradient storage requirements and is recommended for use with large meshes with layered materials, where the total amount gradient data can be very large.
fi_min <float>
Specifies the minimum failure index which is required to store the evaluated failure criterion in the database. The default is 0.0, which means that storage is always performed. A value of 0.25 means that storage is performed only when the failure index is greater than or equal to 25%.
In addition to the FAILURE_INDEX
Field, the values of the failure
criterion evaluated at the element integration points are stored in
the FC_LARC04 dataset. For each element integration point, the maximum
failure index, the corresponding marginofsafety, and the number of
the failure mode (“component”) are stored: 1 means fiber tensile, 2
fiber compressive, 3 matrix tensile, and 4 means matrix compressive.
Example
material 1 type orthotropic
# T300/1034C graphite/epoxy, units in [MPa]
e1 146.86e+03
e2 11.376e+03
e3 11.376e+03
nu12 0.3
nu13 0.3
nu23 0.3
g1 6.186e+03
g2 6.186e+03
g3 6.186e+03
failure larc04
t1 1730.0
t2 66.5
c1 1379.0
c2 268.2
s12 133.763
g2p 0.23
g12 0.46
fi_min 0.5
filter max_of_element
end
end
PostProcessing of Failure Criteria
Failure criteria are computed by one of the B2000++ solvers or with Simples and they can be extracted from the model database and visualized with baspl++ or with the B2000++ data browser or with Simples scripts.
baspl++ Examples
The first example script file:fi.py displays the maximum failure index per element:
if len(sys.argv) != 2:
print 'usage: baspl++ fi.py database'
sys.exit(1)
m = Model(sys.argv[1])
p = NPart(m)
p.edge.show = True
p.elements.extract = 1
f = Field(m, 'FAILURE_INDEX', case_index=0, cycle_index=1)
p.contour.colmap.min = 0
p.contour.colmap.max = 1
p.contour.field = f
The next examplescript file:fi.py displays the failure index per element at each element integration point.
if len(sys.argv) != 2:
print 'usage: baspl++ fi_ip.py database'
sys.exit(1)
m = Model(sys.argv[1])
p = NPart(m)
p.edge.show = True
p.face.show = False
p.elements.extract = 1
f = Field(m, 'FAILURE_INDEX', case_index=0, cycle_index=1)
p.sampling.compname = 'fi'
p.sampling.colmap.min = 0
p.sampling.colmap.max = 1
p.sampling.field = f
Heat Flow Materials
The material type heat
is used to specify linear and nonlinear
material parameters for heat conduction, heat convection, and heat
radiation elements. For heat conduction, isotropic and orthotropic
materials are supported. Depending whether heat conduction elements or
heat convection and heat radiation ‘overlay’ elements reference the
material, different parameters may need to be specified.
MDL Specification
material id type heat
kk1k2k3 ...
[specific_heat ...]
[density <float>]
h_c ...
diffuse_reflectivity <float>
emissivity <float>
stefan_boltzmann_constant <float>
radiation_reference_temperature <float>
end
Heat Conduction Parameters
kk1k2k3 ...
Specifies the conductivity coefficient in material directions 1, 2 and 3. If
k
is specified, this meansk1=k2=k3=k
.The conductivity can be specified as a constant, as a set of support points for a linear or cubicspline interpolation, or as a Python expression.
kk1k2k3 <float> kk1k2k3 interpolated linearcubic flist kk1k2k3 function f
For the interpolation, the temperatures and corresponding conductivity coefficients must be specified with a list. Example:
k interpolated cubic [100.0 8.95 173.15 8.95 273.15 11.5 1623.15 46. 3623.15 51. 5623.15 51. ]
If the conductivity is specified as a Python expression, that expression must be specified as a string, where t is the temperature:
k function '0.3 * t**2'
c_p ...
Defines the specific heat (required for nonstationary analysis). The specific heat can be specified as a constant, as a set of support points for a linear or cubicspline interpolation, or as a Python expression.
c_p <float> c_p interpolated linearcubic flist c_p function f
density <float>
Specifies the value of the density of the material (required for nonstationary analysis).
Heat Convection Parameters
h_c ...
Specifies the convection coefficient. The convection coefficient can be specified as a constant, as a set of support points for a linear or cubicspline interpolation, or as a Python expression.
h_c <float> h_c interpolated linearcubic flist h_c function f
Heat Radiation Parameters
diffuse_reflectivity <float>
Specifies the fraction of incident radiation reflected by the radiating surfaces (in the range of 0.0 to 1.0). The reflection is supposed to be diffuse. Default value is 0.0, i.e. all incoming radiation is absorbed.
emissivity <float>
Specifies the ratio of the energy radiated by the material to the energy radiated by a black body at the same temperature in the range of 0.0 to 1.0. Default value is 0.0, i.e the material does not radiate.
stefan_boltzmann_constant <float>
Specifies the StefanBoltzmann constant, must be given according to the units used. Default is 5.6704e8 for use with S.I. units.
radiation_reference_temperature <float>
Specifies the reference temperature for radiation into the void. Default is 0.0.
Example
material 1 type heat
k 10.0
c_p 1000.0
radiation_reference_temperature 300.
density 1000.
emissivity 0.83
stefan_boltzmann_constant 5.67e8
end
User Defined Materials
Parameters for userspecific material implementations can be specified in dictionary as follows:
material id type=user materialname
key k type IFS <values>
key k type IFS <values>
end
where materialname is the name of the material implementation under which it is registered. At the beginning of an analysis, the shared library containing the material implementation is located and dynamically loaded, and the material object is instantiated and initialized.
The material parameters are given in keytypevalue form, where k must
not be longer than 63 characters. type
defines the type of
<values>
: I
is a list of`` <int>`` enclosed in []
, F
a
list of <float>
enclosed in``[]``, and S
a character string.
Gradients
Large FE models, nonlinear analysis, or analysis with layered materials produce very large amounts of gradient data stored in sample point fields. In such situations the amount of data produced can be reduced:
In the material definition, specify a failure criterion and set the option
filter max_of_element
For each element, gradient data (of any kind) is stored only for the integration point with the maximum failure index.
In the material definition, failure criterion and set the option
fi_min <float>
Gradient data is stored only for integration points having a failure index greater than or equal to
fi_min
.In the MDL case specification, use the
gradients
to control at which load increments gradient data is written to the database.
In the following example, the amount of gradient data written to the database is drastically reduced:
material 1 type orthotropic
# T300/1034C graphite/epoxy, units in [MPa]
e1 146.86e+03
e2 11.376e+03
e3 11.376e+03
nu12 0.3
nu13 0.3
nu23 0.3
g1 6.186e+03
g2 6.186e+03
g3 6.186e+03
failure hashin
t1 1730.0
t2 66.5
c1 1379.0
c2 268.2
s12 133.763
s23 101.4
filter max_of_element # take only the integration point with maximum fi
fi_min 0.5 # and only if fi >= 0.5
end
end
case 1
ebc 1
analysis nonlinear
gradients 1 # only at the end of the nonlinear analysis
end
Stresses and Strains
Stresses, strains, and any failure criteria computed by B2000++ and stored in the database, are computed at the integration points (“Gauss” points). Stress and strain tensors (see figure below)
are stored as vectors similar (but not equal!) to the Voight notation:
Tensors (stored as vectors), such as stresses and strains are expressed in the branch global coordinate system. Specifically,
Strains and stresses originating from linear analysis are “engineering” strains and stresses.
Strains originating from nonlinear analysis are GreenLagrange strains.
Stresses originating from nonlinear analysis are Cauchy stresses.
For the twodimensional elements, stresses and strains that are stored in the database are expanded to 3D. For planestress analysis, the transversal strain \(\epsilon_{33}\) is computed, and for planestrain analysis, the transversal stress (\(\sigma_{33}\) is computed.
The prismatic and the hexahedral elements support laminate materials (in
similar fashion as the shell elements do). In case of laminate
materials, the integration scheme is applied to each layer separately.
This may result in a large number of integration points per element. For
instance, for a hexahedral element HE27.S.TL
using the default
integration rule GAUSS3X3X3
and a laminate consisting of 10 layers,
the number of integration points is 270. When the number of layers is
greater than 3 or 4, the integration rule GAUSS3X3X1
(9 integration
points per layer instead of 27) can be used instead. See also
Integration Schemes.