This option enables the stochastic initialization of the material stiffness tensor and strength values of *MAT_ANISOTROPIC_ELASTIC_PLASTIC (*MAT_157) elements, and can be used for micro-, meso-, or macroscale models. It can also be used for both shell and solid elements. Additionally, this option now supports adding porosity to structural meshes.
This section covers the following:
| SourceFile = STRING | Define the name and, if needed, the path of the source file. This is typically a *.dynain file. |
| MappingResult = STRING | Define the result file name. The mapping result is written into this newly generated file. |
| NumSourcePIDs = INT | Define the number of parts in the source mesh of the meso or macroscale model. This option must be followed by SourcePID#i definitions. |
| SourcePID#i = INT | Define as many part IDs as given in NumSourcePIDs. These parts are considered for the mapping. |
| NumMatrixPIDs = INT |
Define the number of source-mesh parts that are micro model matrices. This option must be followed by MatrixPID#i definitions. |
| MatrixPid#i = INT | Define as many part IDs as given in NumMatrixPIDs. These parts are considered for the mapping. |
| NumFiberPIDs = INT | Define the number of source-mesh parts that are fibers in the micro model. This option must be followed by FiberPID#i definitions. |
| FiberPid#i = INT | Define as many part IDs as given in NumFiberPIDs. These parts are considered for the mapping. |
Note: The options above specifically narrow down the scope of the mapping procedure to defined part IDs. You must specify fiber-matrix PIDs to obtain correct stiffness matrices, especially in micro-scale models.
| Model_Scale = Micro Meso − Macro | This definition provides different initialization approaches. Micro provides an isotrophic stiffness tensor for matrix elements and an orthotropic stiffness tensor for fiber elements. Matrix and fiber PIDs must be declared with this option (see Matrix & Fiber Part IDs in Meso or Macro Scale). Meso-Macro initiates a homogenized fiber-matrix stiffness tensor for the model. Source PIDs must be declared with this option (see Source Part IDs in Meso or Macro Scale). |
| TargetMaterialModel = 157 | This option is required because of the mapping process. This is the only supported material model. |
|
IHIS = 2 16 18 | This option is required because of the mapping process. These are the only supported IHIS options. |
|
ElementType = Shell Solid | Define the element type of the source mesh. |
If ElementType = Shell
| NPLANE = INT |
1 - Reduced integrated shell elements. 4 - Fully integrated shell elements. |
| NTHICK = INT | Define the number of through-thickness integration points (IPs). This option is formerly known as NumberOfTARThroughThicknessIPs. |
|
IntegrationRule = Gauss Lobatto Autoform Moldflow | Define the through-thickness integration rule. This option directly affects the position of through-thickness integration points. |
|
TargetThickness = INT | Sets the result mesh thickness, and overrides thickness data from the source mesh. |
If ElementType = Solid
| ETYP = INT |
1 - Reduced integrated solid elements. 2 - Fully integrated solid elements. |
If IHIS = 2/18
The following options must be defined:
| E11F = DOUBLE | Fiber Young’s modulus in main direction. |
| E22F = DOUBLE | Fiber Young’s modulus in thickness direction. |
| RHOF = DOUBLE | Fiber density. |
| PRBAF = DOUBLE | Fiber in-plane Poisson’s ratio. |
| PRCBF = DOUBLE | Fiber out-of-plane Poisson’s ratio. |
| G12F = DOUBLE | Fiber shear modulus. |
| EM = DOUBLE | Matrix Young’s modulus. |
| RHOM = DOUBLE | Matrix density. |
| PRM = DOUBLE | Matrix Poisson’s ratio. |
| AspectRatio = DOUBLE |
Fiber aspect ratio of length to thickness. |
| FiberVolumeFraction = DOUBLE |
Fiber volume fraction as a percentage. For micro scale modelling, this value must be 100 to correctly generate fiber-part material models. |
|
InclusionShape = Ellipsoidal Spherical Needle Disc | Shape of the inclusions. |
|
HomogenizationMethod = Halpin − Tsai Tandon − Weng Voigt Kukuri Mori − Tanaka_1 Mori − Tanaka_2 Mori − Tanaka_3 | Define the homogenization method used to calculate the unidirectional stiffness matrix. For further information about these methods, see [10] or [16]. |
If IHIS = 16/18
The following options use the format OPTION=Fiber Value Matrix Value. The first value are for fibers, and second value are for matrices. In the meso-macro scale, matrix values are optional.
The following options must be defined:
| XT = DOUBLE DOUBLE |
Tensile Strength in a-direction. |
| XC = DOUBLE DOUBLE |
Compression Strength in a-direction. |
| YT = DOUBLE DOUBLE |
Tensile Strength in b-direction. |
| YC = DOUBLE DOUBLE | Compression Strength in b-direction. |
| SXY = DOUBLE DOUBLE |
Shear Strength in ab-direction. |
| ZT = DOUBLE DOUBLE |
Tensile Strength in c-direction. |
| ZC = DOUBLE DOUBLE |
Compression Strength in c-direction. |
| SYZ = DOUBLE DOUBLE | Shear Strength in bc-direction. |
| SZX = DOUBLE DOUBLE | Shear Strength in ca-direction. |
|
DistributionApproach = Global Local | Define the distribution approach of normal distribution (see Gaussian function). Global defines global deviation (σGlobal) and the number of generated points. Local defines local deviations and the number of generated random-values. |
If DistributionApproach = Global
|
Global_Deviation = INT | Global deviation value that is used to generate random values. |
|
Global_NumOfRandomValues = INT | Global number of random values to generate. |
If DistributionApproach = Local and
If IHIS = 2/18
|
E11F_Options = DOUBLE INT | Local deviation value and number of random values to generate for E11f. |
| E22F_Options = DOUBLE INT | Local deviation value and number of random values to generate for E22f. |
| G12F_Options = DOUBLE INT | Local deviation value and number of random values to generate for G12f. |
| EM_Options = DOUBLE INT | Local deviation value and number of random values to generate for Em. |
If DistributionApproach = Local and
If IHIS = 16/18
The following options use the format OPTION=Fiber DeviationFiber NumGenerate;Matrix DeviationMatrix NumGenenerate. The left side of the semicolon (;) are for fiber definitions, and the right side of the semicolon are for matrix definitions. Meso-macro scale does not require matrix options.
|
XT_Options = DOUBLE INT; DOUBLE INT XC_Options = DOUBLE INT; DOUBLE INT YT_Options = DOUBLE INT; DOUBLE INT YC_Options = DOUBLE INT; DOUBLE INT SXY_Options = DOUBLE INT; DOUBLE INT ZT_Options = DOUBLE INT; DOUBLE INT ZC_Options = DOUBLE INT; DOUBLE INT SYZ_Options = DOUBLE INT; DOUBLE INT SZX_Options = DOUBLE INT; DOUBLE INT | Deviation and number of random values for the fiber and matrix. |
|
DistributionFeedback = YES NO |
Set to YES to activate output of each generated random value for a certain elasticity parameter in the STOCHASTIC INIT Feedback.txt file. These values are used to form the distribution. |
| SORT = BUCKET |
Always use bucket sort for a significant speed-up of the search algorithm. |
| REPEAT = YES |
Enable this option to ensure that all elements and integration points receive mapped data. When there is a significant difference in element sizes between the source and target meshes, the default bucket refinement may be insufficient to cover all points, sometimes by design. In such cases, this flag must be set to guarantee complete data coverage. |
This method mimics how production proccesses create random pores in the structure. If an element is selected as a pore element, matrix material stiffness is modified according to the user-defined input. Therefore, if a micro scale model is used, only matrix elements are used to generate pores. In macro scale models, only matrix material stiffnes value are modified.
You can define an element set to limit the porous area. This can be done by ensuring the source file contains the element set definition, or by adding an element set file to the source file using the *INCLUDE keyword. The Envyo application recognizes an element set declaration automatically. Only one element set can be declared.
| MaxPorosity = DOUBLE | The maximum percentage of acceptable porosity with respect to active volume. |
| Pore_Size = DOUBLE DOUBLE | The first value represents the minimum allowable pore size, and the second value represents the maximum allowable pore size. Depending on a selected element's size, the maximum pore size is overriden. |
| PoreEffect = DOUBLE | The scaling factor of a pore. This value is directly multiplied by the matrix material stiffness value. An expected value v belongs to an interval I=[0,1]. The default value is 0.01. A value greater than 1.0 can be used to model randomly-distributed stiffer inclusions or particles. |
| NumIterations = INT | The maximum number of porosity routine iterations. The default value is 100000. The routine usually does not exceed 100 iterations. This option may be helpful depending on the mesh size and average element size. |