Materials

The different material types provided by OptiStruct are: isotropic, orthotropic, and anisotropic materials. The material property definition cards are used to define the properties for each of the materials used in a structural model.

The MAT1 Bulk Data Entry is used to define the properties for isotropic elastic materials. It can be referenced by any of the structural elements and can also be referenced by any property card.

The MAT2 entry is used to define the properties for anisotropic materials. It applies only to triangular or quadrilateral membrane and bending elements, and can only be referenced by PSHELL, PCOMP, and PCOMPG property cards. This material type specifies the relationship between the in-plane stresses and strains. The angle between the material coordinate system and the element coordinate system is specified on the connection cards.

The MAT3 entry is used to define the material properties for axisymmetric and plane-strain elements. It can be referenced by CTRIAX6 elements and can also be referenced by any PAXI property card which is in turn referenced on CTAXI or CQAXI elements. Similarly, it can be referenced by the PPLANE property which is referenced by plane-strain CQPSTN and CTPSTN elements.

The MAT4 entry is used to define the isotropic thermal material properties. It can be referenced by any of the structural elements, and can also be referenced by any property card.

The MAT5 entry is used to define the anisotropic thermal material properties. It can be referenced by any of the structural elements and can also be referenced by any property card.

The MAT8 card is used to define the properties for planar orthotropic elastic materials in two dimensions. Individual plys of a layered composite lay-up typically possess such orthotropic properties. Since layered composite laminates are modeled using shell elements, MAT8 property data can only be referenced by PSHELL, PCOMP, and PCOMPG property cards.

The MAT9 Bulk Data Entry can be used to define the properties for anisotropic elastic materials for three dimensional solid elements. The general an-isotropic stress-strain relationship linking the six independent stress components of the stress tensor at a point and the six independent strain components of the tensor at the point contain 21 independent constants in the elasticity matrix. These values are supplied using the MAT9 Bulk Data card. The MAT9 Bulk Data card is used with the CHEXA, CPENTA, CPYRA, and CTETRA solid elements, and can only be referenced on the PSOLID property card. The optional coordinate system in which MAT9 data are specified is supplied via the PSOLID Bulk Data Entry.

The MAT10 Bulk Data Entry is used to define material properties for fluid elements in coupled fluid-structural (acoustic) analysis. It may only be referenced on PSOLID entries with FCTN=PFLUID.

Biot (poroelastic) material is defined using MATPE1 entry.

Temperature dependent material properties are defined using MATT1, MATT2, MATT8, and MATT9. All four have the same characteristics as described above. The temperature dependency of each property is defined through TABLEM1, TABLEM2, TABLEM3, or TABLEM4 table entries.

Composite Laminates are defined using the PCOMP, PCOMPP and PCOMPG properties. They are not material types; each ply in the laminate lay-up can reference a different material.

Elasto-plastic material properties are defined using MATS1. The nonlinear material characteristics may need the table input TABLES1. MATS1 is defined as an extension to a MAT1 with the same MID. MATS1 is applicable to all nonlinear solutions.

Hyperelastic material properties are defined using MATHE. Various Hyperelastic material models are available, such are Ogden, Arruda-Boyce, and so on.

Viscoelastic material properties are defined using MATVE or MATFVE, if frequency-dependency is required.

Creep material properties are defined using MATVP.

Cohesive Zone Modeling can be defined using MCOHE or MCOHED entries.

Cast Iron Plasticity material can be defined using MCIRON Bulk Data Entry.

User-defined structural material properties are available using MATUSR. .dll or .so libraries can be referenced via the LOADLIB entry. For more information, refer to User-Defined Structural Material in the User Guide.

User-defined thermal material properties are available using MATUSHT. .dll or .so libraries can be referenced via the LOADLIB entry.

Material models can also be defined using Multiscale Designer and used via the MATMDS entry.

For explicit dynamic subcases (with Radioss integration), more nonlinear material laws are available. As a general rule, material definitions that are only applicable in explicit dynamic analysis are defined on extensions to a MAT1 material that defines the basic elastic properties. The extensions are grouped with the base entry by sharing the same MID. The MATXyx extensions available are listed below. If a law requires material curves, TABLES1 entries are used.

Table 1. Implicit Analysis
Material Property	Nonlinearity	Time-dependency	Temperature-dependency	Frequency-dependency	Material Card
Isotropic	-	-	-	-	MAT1
	-	-	-	Yes	MAT1 + MATF1
	-	-	Yes	-	MAT1 + MATT1
	Elasto-plasticity	-	-	-	MAT1 + MATS1
	Elasto-plasticity	-	Yes	-	MAT1 + MATS1 (referencing TABLEST)
	Hyperelasticity	-	-	-	MATHE
	Viscoelasticity	-	-	-	MAT1 + MATVE
	Viscoelasticity	-	-	Yes	MAT1 + MATFVE
	Viscoelasticity, Hyperelasticity	-	-	-	MATHE + MATVE
	Creep	-	-	-	MAT1 + MATVP
	Creep, Elasto-plasticity	-	-	-	MAT1 + MATVP + MATS1
	Creep	-	Yes	-	MAT1 + MATVP + MATTVP
Anisotropic	-	-	-	-	MAT9 (solid elements) MAT2 (shell elements)
	-	-	-	Yes	MAT9 + MATF9 (solid elements) MAT2 + MATF2 (shell elements)
	-	-	Yes	-	MAT9 + MATT9 (solid elements) MAT2 + MATT2 (shell elements)
	Viscoelasticity	-	-	-	MAT9 + MATVE
	Viscoelasticity	-	-	Yes	MAT9 + MATFVE
Orthotropic	-	-	-	-	MAT9OR (solid elements) MAT8 (shell elements) MAT3 (axisymmetric and plane strain elements)
	-	-	-	Yes	MAT8 + MATF8 (shell elements) MAT3 + MATF3 (axisymmetric and plane strain elements)
	-	-	Yes	-	MAT9OR + MATT9OR (solid elements) MAT8 + MATT8 (shell elements) MAT3 + MATT3 (axisymmetric and plane strain elements)
Fluid	-	-	-	-	MAT10
Fluid	-	-	-	Yes	MAT10 + MATF10
Thermal	-	-	-	-	MAT4 (Isotropic) MAT5 (Anisotropic)
Thermal	Yes (Temperature)	-	Yes	-	MAT4 + MATT4 (Isotropic)
Gasket	-	-	Yes	-	MGASK
Fatigue	-	-	-	-	MATFAT
Biot (Poroelasticity)	-	-	-	-	MATPE1
User-Defined Structural Material Subroutines	Yes	Yes	Yes	-	MATUSR (Fortran and C for subroutines)
User-Defined Thermal Material Subroutines	Yes (Temperature)	Yes	Yes	-	MATUSHT (Fortran and C for subroutines)
Multiscale Designer-based Material	Yes	-	-	-	MATMDS (using Altair Multiscale Designer).
Failure Criteria	-	-	-	-	Criteria and Allowables on MATF Criteria/Allowables can also be defined on MAT1, MAT2, MAT8, PCOMP, PCOMPP, PCOMPG

Table 2. Explicit Dynamic Analysis
Material Property	Nonlinearity	Time-dependency	Temperature-dependency	Frequency-dependency	Material Card
Isotropic	-	-	-	-	MAT1
	Elasto-plasticity	-	-	-	MAT1 + MATS1
	Hyperelasticity	-	-	-	MATHE
	Viscoelasticity	-	-	-	MAT1 + MATVE
	Viscoelasticity, Hyperelasticity	-	-	-	MATHE + MATVE
Anisotropic	-	-	-	-	MAT2 (shell elements)
Anisotropic	Viscoelasticity	-	-	-	MAT9 + MATVE
Orthotropic	-	-	-	-	MAT8 (shell elements)

For explicit dynamic subcases (with Radioss integration), more nonlinear material laws are available. As a general rule, material definitions that are only applicable in explicit dynamic analysis are defined on extensions to a MAT1 material that defines the basic elastic properties. The extensions are grouped with the base entry by sharing the same MID. The MATXyz extensions available are listed below. If a law requires material curves, TABLES1 entries are used.

Explicit Dynamic Analysis (Radioss Integration via ANALYSIS=EXPDYN)

Material Card: Description
MATX0: Void material
MATX02: Johnson-Cook elastic-plastic material
MATX13: Rigid material
MATX21: Rock-Concrete material
MATX25: Composite shell material, TSAI-WU and CRASURV formulations
MATX27: Brittle elastic-plastic material
MATX28: Honeycomb material
MATX33: Visco-elastic foam material
MATX36: Piece-wise linear elastic-plastic material
MATX42: Ogden-Mooney and Rivlin material
MATX43: Hill orthotropic material
MATX44: Cowper-Symonds elastic-plastic material
MATX60: Piece-wise nonlinear elastic-plastic material
MATX62: Hyper-visco-elastic material
MATX65: Tabulated strain-rate dependent elastic-plastic material
MATX68: Honeycomb material
MATX70: Tabulated visco-elastic foam material
MATX82: Ogden material

User-Defined Structural Material

The MATUSR Bulk Data Entry, in combination with the LOADLIB I/O Option Entry, allows for the definition of structural material through user-defined external functions.

The external functions may be written in Fortran or C. The resulting libraries and files should be accessible by OptiStruct regardless of the coding language, provided that consistent function prototyping is respected, and adequate compiling and linking options are used.

Write External Functions

The OptiStruct installation provides an example file with subroutines for Fortran (umat.F) with proper subroutine definition, arguments, and compilation directives. This file can be used as a starting point to write your own subroutines. This file is located at $ALTAIR_HOME/hwsolvers/demos/optistruct.

Two Fortran subroutines are required to define user material in OptiStruct. First, a Nonlinear subroutine for the nonlinear solution, and another subroutine for the linear solution. Both subroutines are mandatory, and the same argument order should be followed as:

Nonlinear subroutine:

subroutine usermaterial(idu, stress, strain, dstrain, stater,
 state, nstate, drot, props, nprops, 
 temp, dtemp, ieuid, kinc, dt, t_step,
 t_total, cdev, cbulk)

integer idu, nstate, nprops, kinc, ieuid
double precision stress(6),stater(*),state(*),
     $     cdev(6,6),cbulk, drot(3,3), temp, dtemp, dt, 
     $     t_step, t_total,
     $     strain(6), dstrain(6), props(nprops)

Linear subroutine:

subroutine smatusr(idu, nprop, prop, smat)
integer idu, nprop
double precision prop(nprop), smat(*)

Note: It is important that both subroutines be named “usermaterial” and “smatusr”, respectively.

Subroutine Arguments

The following table briefly describes the arguments which are passed among OptiStruct and the external subroutines. OptiStruct calls these two subroutines for every integration point of every element in the model. Therefore, the values listed below are calculated at each integration point.

Argument	Type	Input / Output	Description
`idu`	integer	Input	This is defined via the `USUBID` parameter on the MATUSR Bulk Data Entry. This argument can be used to define and choose between different types of materials within the same user subroutine. optional use
`stress`	double (table)	Input/Output	This is the Stress tensor. The initial stress is considered to be input and the stress, tensor calculated during the nonlinear solution are output from the user subroutine to OptiStruct.
`strain`	double (table)	Input	Strain tensor. The initial strain is considered to be input.
`dstrain`	double (table)	Input	Incremental strain table. The incremental strain is input from OptiStruct to the user subroutine.
`stater`	double (table)	Input/Output	Table of State variables at the previous increment. State variables are variables that can be requested as output in the H3D file. Any variable (for example, plastic strain, equivalent plastic strain, and so on) calculated within the solution process in the subroutine can be output by defining it as a state variable.
`state`	double (table)	Input/Output	Table of State variables at the current increment. See `stater` for more information.
`nstate`	integer	Input/Output	Number of State Variables that the user requires in the subroutine. See `stater` for more information.
`props`	double (table)	Input	This table contains all the user-defined material property information from the `PROPERTY` continuation line of the MATUSR entry.
`nprops`	Integer	Input	This is the total number of material properties defined on the `PROPERTY` continuation line of the MATUSR entry.
`temp`	double	Input	This is the temperature at the previous converged increment.
`dtemp`	double	Input	This is the temperature increment.
`ieuid`	integer	Input	Element ID. This subroutine is called for every integration point for every element.
`kinc`	integer	Input	Current increment.
`dt`	double	Input	Current Time increment
`t_step`	double	Input	Subcase time.
`t_total`	double	Input	Total time (if CNTNLSUB is used)
`cdev`	double (table)	Output	Deviatoric material modulus matrix. These are calculated during the solution and are output to OptiStruct to form the stiffness matrix.
`cbulk`	double (table)	Output	Bulk material modulus Matrix. These are calculated during the solution and are output to OptiStruct to form the stiffness matrix.
`smat`	Double (table)	Output	Material modulus matrix. These are calculated during the solution and are output to OptiStruct to form the stiffness matrix.

Build External Libraries for User-defined Materials

Allows building shared libraries on Windows or Linux.

Refer to Build External Libraries for more information.

User-Defined Thermal Material

The MATUSHT Bulk Data Entry, in combination with the LOADLIB I/O Option Entry, allows for the definition of thermal material through user-defined external functions.

Write External Functions

The OptiStruct installation provides an example file with subroutines for Fortran (userlmat.F) with proper subroutine definition, arguments, and compilation directives. This file can be used as a starting point to write your own subroutines. It is located at $ALTAIR_HOME/hwsolvers/demos/optistruct.

Subroutine:

subroutine usrmatht(idu, matID, ieuid, Stater, State,
 nState, drot, rmat, nprops, etempmat, 
 dtemp, kinc, dt, t_step, hgen, smat)

integer*8 i, idu, matID, ieuid, nState, nprops, kinc
      double precision Stater(nState), State(nState)
      double precision drot(3,3), rmat(nprops)
      double precision etempmat, dtemp, dt, t_step
      double precision hgen, smat(*)

Subroutine Arguments

The following table briefly describes the arguments which are passed among OptiStruct and the external subroutines. OptiStruct calls these subroutines for every integration point of every element in the model. Therefore, the values listed below are calculated at each integration point.

Argument	Type	Input / Output	Description
`idu`	integer	Input	This is defined via the `USUBID` parameter on the MATUSHT Bulk Data Entry. This argument can be used to define and choose between different types of materials within the same user subroutine. optional use
`matID`	Integer	Input	Material ID.
`ieuid`	integer	Input	Element ID. This subroutine is called for every integration point for every element.
`drot(3,3)`	Double (table)	Input	Transformation matrix.
`props`	double (table)	Input	This table contains all the user-defined thermal material property information from the `PROPERTY` continuation line of the MATUSHT entry.
`nprops`	Integer	Input	This is the total number of thermal material properties defined on the `PROPERTY` continuation line of the MATUSHT entry.
`temp`	double	Input	This is the temperature at the end of the current increment.
`dtemp`	double	Input	This is the temperature increment of the current increment.
`kinc`	integer	Input	Current nonlinear increment.
`dt`	double	Input	Current time step increment
`t_step`	double	Input	Current subcase time of the current time step.
`Stater`	double (table)	Input/Output	Table of State variables at the last converged time-step. They are constant between iterations of the same time step. State variables are variables that can be requested as output in the H3D file. Any variable calculated within the solution process in the subroutine can be output by defining it as a state variable.
`State`	double (table)	Input/Output	Table of State variables at the current time-step. They are updated and passed between iterations of the same time-step. See `Stater` for more information.
`nState`	integer	Input/Output	Number of State Variables that the user requires in the subroutine. See `Stater` for more information.
`hgen`	double (table)	Output	Generated heat at the integration point.
`smat`	Double (table)	Output	Material matrix. These are calculated during the solution and are output to OptiStruct. Format for smat matrix is provided below. `smat(1): KXX Thermal Conductivity smat(2): KXY Thermal Conductivity smat(3): KXZ Thermal Conductivity smat(4): KYY Thermal Conductivity smat(5): KYZ Thermal Conductivity smat(6): KZZ Thermal Conductivity smat(7): CP Heat Capacity per unit mass smat(8): RHO Density smat(9): Free Convection Heat Transfer Coefficient (Unused).`

Build External Libraries for User-defined Materials

You can build shared libraries on Windows or Linux.

Refer to Build External Libraries for more information.

Cast Iron Plasticity

Cast iron material model is used to describe the yield behavior of grey cast iron, in which tension and compression behavior are different.

In this material model, rate form is used for strain evolution and the strain rate is decomposed into two parts (elastic and plastic parts) in an additive way.(1)

\dot{ε} = {\dot{ε}}^{e} + {\dot{ε}}^{p}

The yielding criteria is defined as:(2)

f \leq 0

Where,

$f = {\begin{matrix} \frac{2}{3} q \cos θ + p - σ_{t} p > - \frac{σ_{c}}{3} \\ q - σ_{c} p \leq - \frac{σ_{c}}{3} \end{matrix}$
$q = \sqrt{3 J_{2}} = \sqrt{\frac{3}{2} S : S}$
$p = \frac{σ_{x x} + σ_{y y} + σ_{z z}}{3}$
$S$ is the tensor form of deviatoric stress.
$S = [\begin{matrix} S_{x x} & S_{x y} & S_{x z} \\ S_{y x} & S_{y y} & S_{y z} \\ S_{z x} & S_{z y} & S_{z z} \end{matrix}]$
$\cos (3 θ) = {(\frac{r}{q})}^{3}$
$r = (\frac{9}{2} S \cdot S : S)$

In the principal stress space, the yield function is:

The flow rule is expressed as:(3)

{\begin{matrix} \frac{{(p - g)}^{2}}{a^{2}} + q^{2} = 9 g^{2} p > - \frac{σ_{c}}{3} \\ q = 3 g p \leq - \frac{σ_{c}}{3} \end{matrix}

Hardening Rule

In this material model, only isotropic hardening is considered. The yield strength is increasing as the equivalent plastic strain grows. It is noted that as tension and the compression have different flow rules, the equivalent plastic strain is different for tension and compression. Hence, the tensile yield strength and the compressive yield strength are looked up from the tensile and the compressive table separately.

The compressive equivalent plastic strain is expressed as:(4)

e_{n}^{p l c} = e_{n - 1}^{p l c} + {\dot{e}}^{p l c}

(5)

{\dot{e}}^{p l c} = \sqrt{\frac{2}{3} S ({\dot{ε}}^{p}) : S ({\dot{ε}}^{p})}

Where, $S ({\dot{ε}}^{p})$ is the tensor of deviatoric part of plastic strain rate.

The tensile equivalent plastic strain is:(6)

e_{n}^{p l t} = e_{n - 1}^{p l t} + {\dot{e}}^{p l t}

(7)

{\dot{e}}^{p l c} = \frac{1}{σ_{t n}} (p {\dot{ε}}_{v o l}^{p} + q {\dot{e}}^{p l c})

Where, ${\dot{ε}}_{v o l}^{p} = {\dot{ε}}_{x x}^{p} + {\dot{ε}}_{y y}^{p} + {\dot{ε}}_{z z}^{p}$ .

In the above expressions, the subscript index $n$ implies the physical quantity is at time $t = n$ , and $n - 1$ means the physical quantity is at the last converged time $t = n - 1$ .

Input

Cast iron plasticity material data can be specified by using the MCIRON Bulk Data Entry which has the same identification number as an existing MAT1 Bulk Data Entry. The Tensile and Compressive stress-strain curves can be defined using the TABLE_T and TABLE_C fields on the MCIRON entry.

Cast iron material via MCIRON is supported for Small and Large Displacement Nonlinear Static Analysis. It is supported for CHEXA, CTETRA, CPENTA, and CPYRA elements (both first and second order).

In addition to regular result output, additional results from this material model are output if STRAIN(PLASTIC) I/O Option is specified. These results include, 6 plastic strain components, equivalent compressive plastic strain, equivalent tensile plastic strain, nodal results, and integration results are also available.

Multiscale Modeling

OptiStruct (OS) and Multiscale Designer (MDS) can be combined to perform multiscaling analysis on structural components utilizing both linear and nonlinear materials.

Heterogeneous materials such as composites, soil, solid foams, and polycrystals consist of one or more distinguishable constituents that have different mechanical properties. ³ For example, it is known that fiber-reinforced composite materials have a stiffer and stronger phase known as the reinforcement and, a less stiff and weaker phase known as the matrix. The governing equations are well understood in one of the scales, either the micro-scale or the macro-scale. While general constitutive equations are applicable to solids under deformation in the macro-scale, continuum models are required in the micro-scale. In order to bridge the gap between the two scales, you need to consider models at different scales simultaneously. This can be achieved by multiscaling techniques.

Classical laminate theory can predict the overall properties of heterogeneous laminates; whereas, homogenization theory provides information on the individual phase properties and phase geometries. Knowledge of individual phases is important to characterize material damage and failure. Hence, multiscaling techniques open unique opportunities for modeling by focusing the material behavior on different levels of physical laws.

An overall flowchart for integration between the two softwares is provided in Figure 5. Multiscale Designer has four pre-processing steps which are used to create material subroutines. These subroutines characterize the micro-scale material behavior in the linear and nonlinear domain. Later they are integrated with OptiStruct through the MATUSR material card for structural analysis.

The four pre-processing steps in Multiscale Designer are:

Unit cell geometry and mesh definition
Linear material characterization
Reduced-order homogenization
Nonlinear material characterization

Note: Detailed information on the four pre-processing steps is explained in the Multiscale Designer User Manual. ¹ Users are expected to understand material characterization in Multiscale Designer.

Single-scale Model

The basic steps required to construct a single-scale material model.

Cast iron plasticity is interesting to study because it has different yielding and hardening behavior when subjected to tensile and compressive loads. The first two sections explain the input data required from the Multiscale Designer (MDS). The next two sections explain the procedure to integrate the material in OptiStruct (OS) and perform structural analysis.

Linear Material Characterization

The material model type is selected as a single scale material characterization. Multiscale Designer allows material characterization for:

isotropic
trans-isotopic
orthotropic
anisotropic material

Here a homogeneous material with the properties of cast iron is utilized for characterization in the linear regime. The input elastic properties/parameters and values of the material are:

Linear elastic parameter properties and values of cast iron ²

Tensile Young’s modulus (GPa), $E_{t}$: 95.5
Compressive Young’s modulus (GPa), $E_{c}$: 95.5
Poisson's ratio, $ν$: 0.26

Nonlinear Material Characterization

Various constitutive laws are available in Multiscale Designer, such as rate-independent plasticity, visco-elasticity, damage laws. Here isotropic damage – 3-piecewise Linear Evolution is used to simulate the nonlinear behavior of the material. The damage model formulation within Multiscale Designer follows the continuum damage mechanics framework. The elastic stiffness matrix is degraded by using a damage state variable which is a function of principal strains. Only for compressive loads, the principal strains are multiplied by a compression factor to alleviate the damage in compression. The compression factor is calculated internally, based on the input properties of the material.

Failure input parameter properties and values of cast iron ²

Stress at damage initiation – tension (MPa), $σ^{0}$: 126.0
Ultimate stress – tension (MPa), $σ^{1}$: 210.3
Strain at ultimate stress - tension, $ε^{1}$: 0.008
Strain to failure – tension, $ε^{2}$: 0.008
Stress at damage initiation – compression (MPa), $σ_{c}^{0}$: 303.0
Ultimate stress - compression (MPa), $σ_{c}^{1}$: 443.3
Strain at ultimate stress - compression, $ε_{c}^{1}$: 0.010
Strain to failure – compression, $ε_{c}^{2}$: 0.010

Nonlinear material characterization is done with a Unnotched Tensile/Compression built-in macro simulation model. Two simulations are defined conforming to ASTM D3039, D3518 and D6641. One to simulate tensile behavior and one for compressive behavior. In the process, a unit mesh – solid cube is fixed on one end and subjected to x-direction displacement on the other end. The stresses are computed by extracting, the reaction forces divided by unit area.

Parameter and input values for unnotched tension/compression simulation

Loading rate – Tension (/s): 0.008
Maximum strain - Tension: 0.008
Loading rate – Compression (/s): -0.01
Maximum strain - Compression: -0.01

The loading rate is the strain rate for the test. For all-rate independent laws (this includes isotropic damage law – 3 piecewise Linear evolution), it is typical to set the loading rate equal to the maximum strain. The minimum number of increments for mechanical loads is defined to be 20. This means that the initial time-step is set as the total step time divided by minimum mechanical increments.

The output data files are generated in the material model directory. The file path can be changed in the Multiscale Designer settings. The corresponding file names and descriptions are availble in ‘Unit Cell Data Files’ of the Multiscale Designer User Manual.

Structural Analysis

The user material is simulated in OptiStruct with nonlinear quasi-static analysis of a unit CHEXA cube element connected to eight CELAS1 spring elements (Figure 6). The springs have very low stiffness and are fixed on one end. Four springs have a connection in the y-direction and four have connections in the z-direction. The springs ensure that there are no rigid body motions in y- and z-directions. The unit CHEXA cube element is constrained along the x-translation direction; x, y and z rotational directions on the side which is connected to the springs and on the other side, the element is subjected to contraction load = 0.009 mm and extension load =0.007 mm in subcase 1 and 2, respectively.

Integrate Multiscale Designer Files with OptiStruct

In Multiscale Designer, select the input file (.mic).
Select the Solver Interfaces tab.
In the option for OptiStruct, click the Multiscale Materials tab.
The Multiscale Designer solver interface for OptiStruct opens.
Make sure that the plugin “dll” and multiscale material data files are pointing to the material subroutine and Multiscale Designer model, respectively.

Example directory to the material subroutine and Multiscale Designer model are <hwinstallation_directory\hwsolvers\MultiscaleDesigner\win64\plugins\OptiStruct\umat.dll> and <working_directory\MultiscaleDesigner\model_name\Mechanical\model_name_mdsMAT.dat>, respectively.

The number of user-defined variables computed for isotropic damage law is 8, which the terms from damage state variable, equivalent strain, total strain, and Eigen strain.
Change the output folder directory for the plugin data to the model file path, <working_directory\model_name\Mechanical>.

The generated plugin data file (OptiStruct_plugin_data.fem) contains the LOADLIB I/O and MATUSR cards for running the structural analysis. The LOADLIB I/O entry is used to implement external subroutines and MATUSR is used to defined user material parameters and properties. These cards are later inserted into OptiStruct input model files (*.fem).
Note:
1. The input model file should be in the same folder as the multiscale material. The material subroutines are called into this database through LOADLIB.
2. The USUBID number in the MATUSR should refer to the multiscale material model ID.

Single-scale Results

Sample cards are generated for Multiscale Designer-OptiStruct integration, with the results of tension and compression test in OptiStruct with the user-defined material.

Elastic properties from homogenization and stress-strain curve from damage law are presented.

Linear Material Characterization

The parameters and values for Failure input properties of cast iron in Nonlinear Material Characterization show that the stress at damage initiation is 126 MPa for tension and 303 MPa for compression. The corresponding time-step, up to which the material is linear is 0.15 s and 0.30 s for tension and compression, respectively. Figure 7 shows the contour plots of x-direction stresses, x-direction strain and y-direction strain from which the elastic properties of the material can be calculated using elasticity equations. In this simulation, the homogenized elastic properties of the material are the same as input properties. This is because the material is assumed to be isotropic.

The calculated homogenized parameter properties and values are:

Tensile Young’s modulus (GPa), $E_{t}$: 95.5
Compressive Young’s modulus (GPa), $E_{c}$: 95.5
Poisson's value, $ν$: 0.26

Nonlinear Material Characterization

The stress-strain curve generated from Multiscale Designer is shown in Figure 8. The maximum difference between Multiscale Designer and experiment is 9.6 % at 0.004 strain. At strain values of -0.01 and 0.008, the models are fully damaged; therefore, it is recommended to use the material with a strain value from -0.095 to 0.0076. The stresses corresponding to the fully damaged strains are -0.96 MPa and 184.13 MPa, respectively. The results are plotted against data from experiments ² and Multiscale Designer.

Multiscale Designer-OptiStruct Integration

The OptiStruct plugin file generated from Multiscale Designer is illustrated in Figure 9. This file contains information in the LOADLIB I/O and MATUSR cards.

Structural Analysis

NLPARM and NLOUT cards are used for solution control and incremental solution output, respectively, for nonlinear analysis in OptiStruct. In this model, the incremental results are output for each load increment value of 0.05. The material stays linear up to a load factor of 0.175 for tension and 0.2875 for compression. Figure 10 shows the contour plots of x-direction stresses, x-direction strains and y-direction strains for the corresponding load factors. The wireframes in Figure 10 shows the undeformed boundaries.

Figure 11 depicts the stress-strain curve generated from OptiStruct using MATUSR and LOADLIB. The plot shows that the user-material from Multiscale Designer can be simulated well in OptiStruct.

Multiscale Model

The basic steps required to construct a multiscale material model.

Unidirectional fiber-reinforced polymer composite is subjected to tensile load in fiber-axial and fiber-transverse directions. The response of the material is output and validated with experimental data. The first two sections explain the input data required from the Multiscale Designer (MDS). The next two sections explain the procedure to integrate the material in OptiStruct (OS).

Unit Cell Model and Linear Material Characterization

The material model type is selected as multi-scale material characterization. The unit cell is modeled as a fibrous material with a square packing array. The volume fraction of the fiber phase is 65%. Figure 12 represents various unit cell models available in Multiscale Designer for fibrous composites.

The matrix is modeled with homogeneous elastic properties and the fiber is assumed to be transversely isotropic. Periodic boundary conditions are applied to the unit cell to obtain the homogenized stiffness matrix of the composite.

Linear elastic parameter properties and values of fiber and matrix ⁴

Young’s modulus of the matrix (GPa), $E^{m}$: 3.8
Poisson’s ratio of the matrix, $ν^{m}$: 0.32
Longitudinal Young’s modulus of fiber (GPa), $E_{1}^{f}$: 252.25
Transverse Young’s modulus of fiber (GPa), $E_{2}^{f}$: 13.45
Longitudinal Poisson’s ratio, $ν_{12}$: 0.02
Transverse Poisson’s ratio, $ν_{23}$: 0.3

Nonlinear Material Characterization

The matrix is assumed to obey isotropic damage – bilinear evolution model and the fiber is assumed to follow orthotropic damage – bilinear evolution, for simulating the nonlinear behavior of the material.

The nonlinear input parameter properties and values for damage law ⁴ are:

Stress at damage initiation (MPa), $σ^{0 m}$: 126.0
Strain at ultimate stress, $ε^{1 m}$: 0.1

Damage input properties of the fiber

Stress at damage initiation – longitudinal direction (GPa), $σ_{1}^{0 f}$: 4.2
Strain at ultimate stress – longitudinal direction, $ε_{1}^{1 f}$: 0.017
Stress at damage initiation – transverse direction (MPa), $σ_{2}^{0 f}$: 75.0
Strain at ultimate stress – transverse direction, $ε_{2}^{1 f}$: 0.05

For nonlinear material characterization in fiber-axial and fiber-transverse direction, two laminate layups with unit thickness are created with orientations 0° and 90°, respectively. Each laminate is subjected to Unnotched Tensile/Compression macro simulation with different loading rates.

The input values for the macro simulations are:

Loading rate – Fiber axial direction test (/s): 0.05
Maximum strain - Fiber axial direction test: 0.05
Loading rate – Fiber transverse direction test (/s): 0.017
Maximum strain - Fiber transverse direction test: 0.017

The output data files are generated in the material model directory and the stress-strain curve data will export to an Excel spreadsheet file in <material_model_directory\model_name\mechanical\model_name_NLmatl.xlsx>.

Integrate Multiscale Designer Files with Multiscale Designer-OptiStruct

In Multiscale Designer solver interface for OptiStruct, click the Homogenized Materials tab.
Set the card images to MAT2, MAT8, MAT9 or MAT9ORT.
Click the Multiscale Materials tab and set the output file path for the OptiStruct plugin “dll”.
In the multiscale material data file, browse the file path to <material_model_directory\model_name\mechanical\model_name_mdsMAT.dat>.

The number of user-defined variables computed for orthotropic damage law is 8, which involves the terms from the damage state variable, equivalent strain, total strain, and Eigen strain.
By default, the OptiStruct plugin data files are output to <material_model_directory\Macro\Mechanical\OptiStruct_plugin_data.fem>.

Multiscale Results

Sample cards are generated for Multiscale Designer-OptiStruct integration with OptiStruct test results.

Elastic properties from homogenization and stress-strain curve from damage law are presented.

Unit Cell Model and Linear Material Characterization

Figure 13 represents the square fiber packing array generated from Multiscale Designer. The relative radius of the fiber with respect to the unit cell size for the fiber volume fraction is 0.45.

Homogenized elastic properties of the fiber/matrix composite. Nonlinear material characterization. All these values are available in an Excel spreadsheet in <material_model_directory\model_name\mechanical\model_name_Lmatl.xlsx>.

Longitudinal Young’s modulus (GPa), $E_{1}^{c}$: 165.4
Transverse Young’s modulus (GPa), $E_{1}^{t}$: 8.8
Longitudinal Poisson’s ratio, $ν_{12}^{c}$: 0.11
Transverse Poisson’s ratio, $ν_{23}^{c}$: 0.34

Nonlinear Material Characterization

Figure 14 and Figure 15 show the stress-strain curve generated from Multiscale Designer for fiber-axial and fiber-transverse direction tensile tests. These values are plotted over experimental data. ⁴ The maximum difference in tensile yield strength between Multiscale Designer and experiment is 6.0 % for the fiber-axial direction test and 11.3 % for the fiber-transverse direction test.

Multiscale Designer-OptiStruct Integration

A MAT9ORT material file generated from Multiscale Designer is illustrated in Figure 16. These files are to be used in OptiStruct to run any structural analysis. The OptiStruct plugin file which contains the LOADLIB I/O and MATUSR cards is the same as in Figure 9.

¹ Altair Engineering Inc. 2018. Multiscale Designer: User Manual. Troy, MI

² Downing, S.D., 1984. “Modeling Cyclic Deformation and Fatigue Behavior of Cast Iron under Uniaxial Loading,” Report No. 11, University of Illinois at Urbana-Champaign, IL

³ Fish, J., 2014. Practical Multiscaling. John Wiley & Sons, Ltd.

⁴ Yuan, Z., Crouch, R., Wollschlager, J., Shojaei, A., Fish, J., 2016. “Assessment of Altair Multiscale Designer for damage tolerant design principles (DTDP) of advanced composite aircraft structures,” Journal of Composite Materials, 51(10): 1379-1391