5.21.5.1. *Element_Shell

5.21.5.1.1. Specific Options

NPLANE = INT	1 - Reduced integrated shell elements 4 - Fully integrated shell elements
NTHICK = INT	Number of through-thickness integration points in the target mesh. If an even number is provided, and SCALARINT is set to CENTER IP and the two integration points closest to the mid-surface are averaged to determine the BETA angle for *ELEMENT_SHELL_BETA output. If an odd number is provided, and SCALARINT is set to CENTER IP, the Envyo application uses the mid-point as BETA for output.
IntegrationRule = Gauss Lobatto Autoform Moldflow Eq_Distr	Define the through-thickness integration rule for the mapping result. This option directly affects the positions of the through-thickness integration points on the target mesh.
MapStress = NO	Define whether INITIAL_STRESS_SHELL cards should be written. For the ELEMENT_SHELL_COMPOSITE option, set this flag to NO.
Thck_Avg_Opt = Ele_Avg Nodal_Avg	Thickness averaging option. When using *ELEMENT SHELL THICKNESS, nodes may hold different thickness information, depending on the element to which they belong. This is especially criticial for components with ribs. With the default setting (Ele Avg), the Envyo application calculates through-thickness integration points using the nodal thicknesses stored on the element nodes by interpolating the resulting thicknesses at the in-plane integration points via shape functions, allowing for the correct calculation of the local through-thickness integration points. By choosing the Nodal Avg option, the application first collects all thicknesses stored on one node from its attached elements and averages these thicknesses. Interpolation to the in-plane integration points using shape functions is then performed.
MapMainDir = YES	Activate the mapping of main directions to *ELEMENT_SHELL_COMPOSITE cards.
TargetThickness = DOUBLE	Define the thickness of the target part. If a SectionFile is included in the source mesh, this value is ignored. If the target mesh already has elements with thickness value, this option can again be ignored.
SCALARINT = AVG CENTER_IP	Define the interpolation method for transferred fiber-orientation angles derived from mapping the orientation tensors. AVG calculates the mean of all the fiber directions assigend to the intergation points through the mapping process. CENTER IP takes the mid-surface integration point information only, or calculates the average of the orientation from the two integration points closest to the mid-surface (see also NTHICK).
Shell_Option = Beta	Activates the output of *ELEMENT_SHELL_BETA cards.

Note: Stress, strain, and thickness mapping are all available for MOLDEX3D-SHELL mapping. MapStress must be activated for the *INITIAL_STRESS_SHELL output option. Map-Weldline is optional. Thickness mapping is not available. Instead, you may define a TargetThickness. MapMainDir activates the output of *ELEMENT_SHELL_COMPOSITE keywords carrying the main fiber direction. If special homogenization is necessary, TargetMaterialModel can be either *MAT_157 or *MAT_215.

INN = INT	This flag is similar to the invariant node numbering flag in the LS-DYNA application provided in the *CONTROL_ACCURACY card, see [19]. To properly calculate orientations with respect to the element coordinate system, the Envyo program needs information about how the LS-DYNA application calculates the element coordinate system. The default is Off, as is the case with the LS-DYNA application.
MapStress = YES NO	Activate stress mapping.
MapThickness = YES NO	Activate thickness mapping.
Thck_Avg_Opt = Ele_Avg Nodal_Avg	Thickness averaging option. When using *ELEMENT SHELL THICKNESS, nodes may hold different thickness information, depending on the element to which they belong. This is especially criticial for components with ribs. With the default setting (Ele Avg), the Envyo application calculates through-thickness integration points using the nodal thicknesses stored on the element nodes by interpolating the resulting thicknesses at the in-plane integration points via shape functions, allowing for the correct calculation of the local through-thickness integration points. By choosing the Nodal Avg option, the application first collects all thicknesses stored on one node from its attached elements and averages these thicknesses. Interpolation to the in-plane integration points using shape functions is then performed.
MapWeldline = YES NO	Activate detection of elements being assigned a WeldlinePID.
WeldlinePID = INT	Part-ID assigned to elements within a WeldlineRadius.
WeldlineRADIUS = DOUBLE	Define the radius for the weldline elements. This option enables adjustment of the weldline radius so that the number of elements within the weldline zone can be distinguished and a weld line PID assigned. If this option is not defined, Search Radius and Scale_SearchRadius options are used to determine weldline zone.
MapMainDir = YES NO	Only main orientation will be transferred. Output will be *ELEMENT_SHELL_COMPOSITE.
OUTPUT_OPTION = INITIAL STRESS ONLY	Only *INITIAL_OPTION cards will be written to the mapping result file. Nodes and elements are skipped.
TargetMaterialModel = 157 215	Specify which target material model is used in the subsequent analysis, if not initializing with *ELEMENT_SHELL_COMPOSITE. Options are 157 or 215 referring to respective material model IDs in LS-DYNA application’s material model manual [20].

5.21.5.1.2. MAT_ANISOTROPIC_ELASTIC_PLASTIC (MAT_157) Output (Standard Routine)

For *MAT_157, further mapping input data is required to enable initialization of orientation and further components at integration point level. Additional input parameters are dependent on the chosen IHIS - option.

5.21.5.1.2.1. IHIS Options

IHIS = INT	Flag defining the material parameter written to INITIAL_STRESS_SOLID cards for MAT_157, according to [20]. The following values are supported:
IHIS = 1 - q-values are written to the first two history variables.
IHIS = 3 - q-values are written to the first two history variables, tensor components Cij are written on history variables #7 - #27.
IHIS = 11 - q-values are written to the first two history variables, tensor components Cij are written to history variables #7 - #27, table IDs for strain rate dependent plasticity are defined in history variable #28.
For IHIS = 1, no further input is required.
If IHIS > 1, define the following variables:

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].

ClosureApproximation = Linear

Quadratic

Hybrid_A

Hybrid_B

ORF

ORS

Define the closure approximation method that is used to calculate the 4th-order orientation tensor from the 2nd-order orientation tensor given by Moldex3D. For further information about these methods, see [10] or [16]. ORF calls the orthotropic fitted closure approximation proposed by [12], distinguishing between different fiber interaction coefficients based on the equation provided [7]. ORS refers to the orthotropic smooth closure approximation.

The following elastic constants 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 (length/thickness).
FiberVolumeFraction = DOUBLE	Fiber volume fraction in precent.
InclusionShape = Ellipsoidal Spherical Needle Disc	Shape of the inclusions.

If IHIS > 3, you must define several direction-dependent curve files, representing different strain rates, so that the strain-rate and direction-dependent plasticity can be defined. The following input can be supplied:

5.21.5.1.2.2. Curve Input

NumberOfCurveFiles = INT	Define the number of curve files to be read.
CurveFileName#i = STRING	Define the name and, if needed, path of the curve files. This card must be written NumberOfCurveFiles times.

5.21.5.1.2.3. Strain Rate and Direction Information

NumberOfDirections = INT	Define the number of directions to which the curve files belong. The recommended value for short fiber reinforced plastic materials is 3.
Direction#i = DOUBLE	Define angles, with respect to the direction of flow, used to generate the plasticity curves. Typical angles are 0, 45, and 90 degrees. This card must be written NumberOfDirections times.
NumberOfStrainRates = INT	Define the number of strain rates to which the curve files belong.
StrainRate#i = DOUBLE	Define the strain rates that are considered by the defined curves. This card must be written NumberOf- StrainRates times.
StrainRate#iDirection#j = INT	Define the curve IDs that belong to the respective strain-rate/direction combination. This card must be written NumberOfDirections x NumberOfStrainRates times.

5.21.5.1.2.4. Equation Parser and History Variable Handling (Only for IHIS=1 Option)

HISV_HANDLING = YES

NO

CLEAR

Enables you to move and modify history variables manually. Refer to [20] and [12] for the meaning of histories. If CLEAR, all history variables are removed before generating the result file. If YES, define as many history variables as should be modified (see below).

MAX_NUM_HISV = INT

Define the new maximum number of history variables. This is an easy way to get rid of unwanted histories that are of no use for the new model, but also allows you to extend the number of histories output. If a history variable is moved to a position that is higher then the actual number of history variables in the input deck, the number of histories is extended automatically.

The Envyo application implements an equation parser based on the Shunting yard algorithm and is available as an MIT license [6]. This equation parser has been modified to work with common LS-DYNA variables such as histories, and effective plastic strains and stresses. Variables are declared using the & symbol and commands are executed in the order of input. The following variables are available:

&HISV#i	History variable at position i.
&EPS	Effective plastic strain (the last entry in *INITIAL STRESS SHELL which may have a different meaning than eff. plast. strain).
&ELELENGTH	Element length of the current element.
&SIG_IJ	Components of the 2nd order stress tensor.
&SIG_INIT	Enables initialization of a specific stress value that refers to all stress components.
exp	Exponent. An alternative input would be e**.

Example

The following example illustrates usage of the equation parser. The commands following the additional history are executed in the order of input:

&HISV#4 = abs(&HISV#3-&HISV#2)*0.000467354
&HISV#8 = &HISV#2
&HISV#9 = &ELELENGTH
MAX_NUM_HISV = 8

The value of history variable #4 is calculated using the absolute value of history #3 - #2, multiplied by a scale factor. Following these operations, history variable #8 is assigned the value at history variable #2 and the element length is stored at history variable #9. Nevertheless, only eight history variables are written to the final result file due to MAX_NUM_HISV.

5.21.5.1.3. Fiber Orientation Tensor Dependent Material Model Handling

The Envyo application supports two methods to assign material ID (or material properties) according to source fiber orientation tensors found during mapping process.

Method 1: Using *ELEMENT_SHELL_COMPOSITE (_LONG)

Since each through-thickness IP for composite elements can have a different material ID, you can define a list of fiber orientation tensors and material ID pairs to assign materials IDs for matching tensors. The following options must be defined:

NumOriTensorMIDs = INT	Define the number of parts in the target mesh that are considered within the mapping. This option must be followed by OriTensorMID#i definitions.
OriTensorMID#i = DOUBLE DOUBLE DOUBLE; INT	Define as many fiber orientation tensor and material ID pairs as specified in NumOriTensorMIDs. Three double values represent the a₁₁, a₂₂, and a₃₃ orientations of the tensor, respectively. The integer value seperated by a semicolon represents the material ID asigned for this orientation tensor.
MapMainDir = YES	This option must be defined. The output is *ELEMENT_SHELL_COMPOSITE. Fiber orientations are represented by BETA angles for each through thickness IP.

Method 2: Using the *MAT_157 IHIS Option

Independent of the previous options for *MAT_157, you can define IHIS=7 or IHIS=15 to activate fiber orientation-dependent mapping of material properties. *MAT_157 cards must be defined in the target mesh, and they can also be added to the target mesh as an include using the *INCLUDE keyword. Direction components q₁ & q₂ and material stiffnes parameters C_ij will be calculated by the Envyo application, and all parameters mentioned above for IHIS=3 option should therefore be defined. R₀₀, R₄₅, and R₉₀ values for IHIS=7 and an additional LCSS value for IHIS=15 are taken from included *MAT_157 cards. The fiber orientation tensors of material cards must be defined as the material card title using the following format:

EnvyoOrient:DOUBLE;DOUBLE;DOUBLE

where double values represent the a₁₁, a₂₂, and a₃₃ orientations of the tensor. The material ID is taken from the material model.

This method can be enhanced to define through-thickness IP material IDs using the *ELEMENT_SHELL_COMPOSITE keyword. The following options must also be defined:

Shell_Option = Composite	Activates the *ELEMENT_SHELL_COMPOSITE output routine
IntegrationRule = Eq Distr	Equally-distributed, through-thickness IP positions are used. A detailed explanation is provided under the IntegrationRule option above.

Note that the first method always overrides the second. To use the enhancements of the second method, the MapMainDir option should be either set to NO, or not defined at all.

5.21.5.1.4. MAT_4A_MICROMEC (MAT_215) Output

No further information is required when using *MAT 215 on the target side.

5.21.5.1. *Element_Shell_Beta Output