Available source and result file formats are listed below:

There are three available methods for performing mesh transformation:

The 4PCS method should be used with caution, as it is fully automatic and may not accurately transform stress tensors and fiber orientations between different coordinate systems. The ICP algorithm is the recommended approach.

The user-defined translation and rotation options are listed beneath TRAFO_OPTION.

Additionally, a custom sequence of user-defined transformations can be applied. These transformations are executed in the order in which they are specified and multiple transformations may be defined.

In addition to the transformation options, you can convert the unit systems:

ClosestPoint is the most commonly-used option and accounts for most of the mapping scenarios targeted by the Envyo application. Beginning with the target mesh, the next element or integration point is identified and its data transferred to the target mesh.

The ElementSizeSearchRadius option supports mapping of results from mesoscale process simulations using shell elements onto a target mesh. The target mesh element size is therefore used as a search radius, whereas the source mesh elements are projected onto the target mesh along the source-mesh normal and a check is performed to see if the intersection is within the target element. The element size can be scaled using Scale_SearchRadius (below).

The ConsiderOndulation option considers the through-thickness position of the identified fiber orientation. This information is therefore not considered as provided by user input, but by the position in the source mesh related to the target mesh. This option does not account for the ordering of the input parts - it first maps those that are closest to the target part, then the second closest and so on. No resinuous areas can be assigned with this option. If the MapThickness option (below) is enabled, the offset between the source layers is also considered, which usually leads to varying thicknesses throughout the part.

With RVE Detection, you can define specific criteria which allows the Envyo application to decide if a specific combination of fibers has been identified and therefore assigns a specific, user-defined material ID to the dedicated integration point.

CP - directly activates the closest point algorithm to transfer everything stored in the *INITIAL STRESS OPTION fields on the source side. This is the default algorithm.

AVG - the euclidean average is taken from the values found within a specific search radius. By default, the search radius is based on the average target mesh element length.

SHEPARD NO1 - activates the general Shepard's inverse distance weighting function. You may specify the exponent using the SHEPARD EXPONENT option.

SHEPARD NO2 - activates the Shepard's inverse distance weighting function, with a minimum of four and a maximum of ten points considered for the interpolation function. You may also specify the exponent using the SHEPARD EXPONENT option.

SHEPARD NO3 - activates the Shepard's inverse distance weighting function, with a minimum of four and a maximum of ten points considered for the interpolation function, including direction. You may also specify the exponent using the SHEPARD EXPONENT option.

SHEPARD NO4 - activates the Shepard's inverse distance weighting function, with a minimum of four and a maximum of ten points considered for the interpolation function, including direction and the slope. You may also specify the exponent using the SHEPARD EXPONENT option.

The search radius for the four options listed above is adjusted based on Shepard's proposal, see [22].

FE - activates the interpolation of values found in the *INITIAL STRESS OPTION fields based on finite element shape functions and point projection of the considered integration points into the plane of the source shells. If the source and target through-thickness integration rules are different, through-thickness interpolation is performed based on the method proposed in [24], minimizing the difference in the areas underneath the through-thickness integration rules on source- and target side for all values being transferred. This interpolation result can be visualized using the WriteTTInterpolationFile and TTInterpolationFile options.

FE NODAL AVG - activates the interpolation of values found in the *INITIAL STRESS OPTION fields based on finite element shape functions and point projection of the considered integration points into the plane of the source shells. In addition to the described method above, values of the connected elements on the source side are also considered through extrapolation of the integration point values onto the element nodes, taking the euclidean average and performing a value recovery on the target integration point.

Besides using the standard euclidean average (AVG), which is the default and recommended value, further interpolation methods based on tensor invariants have been investigated due to the fact that swelling effects are often seen when performing standard euclidean average of tensorial data (the tensor shape changes).

Based on the work of [9], several invariant sets have been implemented for the interpolation functions available in MapStress, and linear interpolation is performed for these invariant sets instead of the single tensorial values. These interpolated invariants allow you to recover the eigenvalues based on a closed form solution of the cubic function and together with the eigenvectors determined through linear interpolation of the originating tensors, the resulting tensor can be recovered.

Due to the boundaries of the recovery function, which is based on the arccosine defined between -1.0 ≤ x ≤ 1.0, this might lead to unexpected behavior with the current implementation.

INV-K refers to an orthogonal invariant set based the tensor trace, the Frobenius norm of the tensor's deviatoric (fractional anisotropy of the tensor), and the mode of the deviatoric.

INV-R refers to an orthogonal invariant set based the tensor norm, the relative anisotropy of the tensor, and the mode of the deviatoric as in INV-K.

INV-N is a non-orthogonal invariant set based on the tensor trace, the fractional anisotropy, and the tensor mode.

INV-U is a uniform invariant set based on the tensor trace, the scaled relative anisotropy of the tensor, and the scaled angular mode AM.

These invariant sets have been proposed in [9] for positive definite tensors gained in DT-MRI measurements. Generally, stress tensors are not positive definite. The Cauchy stress tensor invariant set INV-C is therefore added to the interpolation options, even though this might not solve the issue regarding the arccos in the recovery function.

For cases where the target mesh does not contain any information regarding the integration rules being used, such as element formulation and through-thickness integration points, you must define these manually. The input for this is as follows:

For the RVE DETECT algorithm, specific properties for representative volume elements must be defined:

Further options for the mapping of fiber orientations from *MAT 249 (*MAT REINFORCED THERMOPLASTIC) [20] are as follows:

The Lay=INT, IP=INT, Fib=INT definition should be handled differently for the *MAT 249 target material model. Since this material model can represent up to 3 distinct fiber directions, the direction averaging per target through the thickness integration point should also support up to 3 fiber directions.

The integer value for Fib is considered as a digit-wise value only if target material model is *MAT 249.

This digit-wise integer represented by,

As can be seen above, the digit position represents the store-position on the target mesh and the value represents which source fiber should be used to do averaging. An example is given in note 2.

An equation parser has been implemented in the Envyo applkication, based on the Shunting yard algorithm and is available as an MIT license [6]. This equation parser has been modified to work with common LSDYNA 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 supported:

The example below illustrates the usage of the equation parser in combination with lookup tables. The commands following the additional history and lookup table definition are executed in the order of input:

Example: History variable manipulation

AddEleHISVFile#1 = Results A.dyn
AddEleHISVFile#2 = Results B.dyn
LookupTable#1 = data A.txt,&COL#1,&COL#2,&COL#3
LookupTable#2 = data B.txt,&COL#1,&COL#2,&COL#3
&HISV#3 = &ADDELE HISV#2
&HISV#2 = &ADDELE HISV#1
&HISV#4 = abs(&HISV#3-&HISV#2)*0.000467354
&EPS = &LookupTable#1,linearInterpolation,&HISV#4,&ELELENGTH,&COL#3
&HISV#6 = &LookupTable#2,nextNeighbour,&EPS,&ELELENGTH,&COL#3
&HISV#8 = &HISV#2
&HISV#9 = &ELELENGTH
MAX_NUM_HISV = 8

Two additional element history files are loaded into the Envyo application and are stored internally. In addition, two lookup table files are read. For each of these, column one, two, and three are considered. These numbers can be different and it is also possible to have more than just three columns.

After reading the data, the following commands are executed:

Part clustering is available on arbitrary history variables or even stress values. The input is as follows:

CLUSTERID#i = STRING, STRING, DOUBLE, DOUBLE, INT (,INT)

Example: Clustering

CLUSTERID#500004 = &HISV3,MinMax,1.248,9.120E+02,12,6 

Target part ID 500004 is split based on history variable # 3. The MinMax option is chosen, so the application creates 6 equally spaced regions between 1.248 and 9.12E+02. Averaged values of history variable #3 are assigned part IDs starting at part ID 12.

CLUSTERID#500004 = &HISV3,AVG,1.248,2.803E+02,12 
CLUSTERID#500004 = &HISV3,AVG,2.803E+02,4.067E+02,13 
CLUSTERID#500004 = &HISV3,AVG,4.067E+02,5.330E+02,14 
CLUSTERID#500004 = &HISV3,AVG,5.330E+02,6.593E+02,15 
CLUSTERID#500004 = &HISV3,AVG,6.593E+02,8.857E+02,16 
CLUSTERID#500004 = &HISV3,AVG,8.857E+02,9.120E+02,17 

Target part ID 500004 is split based on the average values on each element of history varibale # 3. Averaged values within a range of 1.248 ≤ x < 2.803E + 02 are assigned the new part ID 12, values within the range of 2.803E + 02 ≤ x < 4.067E + 02 are assigned the new part ID 13, and so on.

Note 1:

As shown in Figure 4.3: Number of stacks, integration points and fiber IDs for *MAT 249, *MAT 249 outputs several fibers at each integration point. This must be considered in NTHICK or in the respective averaging options. In the example below, the source file consists of four stacked shell elements (Part 1 - 4), with three integration points through the thickness each, having three fibers each. A complete mapping for *ELEMENT SHELL COMPOSITE therefore leads to a total of 36 (4x3x3 ) layers and integration points. Averaging can be done as follows:

ThroughThicknessAveraging = YES 
NumberOfFiberBundles= 12
FiberBundle#1:
MatID=1001 
Lay= 1, IP= 1, Fib= 1 
Lay= 1, IP= 2, Fib= 1 
Lay= 1, IP= 3, Fib= 1 

... 
        
FiberBundle#4: 
MatID=1004 
Lay= 2, IP= 1, Fib= 1 
Lay= 2, IP= 2, Fib= 1 
Lay= 2, IP= 3, Fib= 1

... 
        
FiberBundle#12:
MatID=1012 
Lay= 4, IP= 1, Fib= 3 
Lay= 4, IP= 2, Fib= 3 
Lay= 4, IP= 3, Fib= 3 

This leads to a reduced number of twelve layers and integration points for *ELEMENT SHELL COMPOSITE after the mapping.

Each layer may have the same material ID or different material IDs.

Figure 4.3: Number of stacks, integration points and fiber IDs for *MAT 249

Note 2:

The main purpose of fiber bundle handling is explained in the previous note. If the target material model is defined to handle the *MAT 249 IHIS=1 option, fiber averaging can encapsulate up to three distinct fiber directions. The averaging of the directions of the fibers on the target side can be coupled using different source PIDs, through thickness integration points (IPs) and fibers.

Take, for example, a mapping process with two source PIDs, 10 and 20, which are defined as SourcePID#1 and SourcePID#2, respectively. Both source meshes have three through thickness IPs and all three fibers are provided in mesh *INITIAL STRESS SHELL fields at the respective history variable positions. It is necessary to map fiber directions on to five (NTHICK=5) through thickness target IPs, and the fiber bundles are defined as follows:

ThroughThicknessAveraging = YES
NumberOfFiberBundles= 5
FiberBundle#1:
MatID=28 
Lay= 1, IP= 1, Fib= 321 
Lay= 1, IP= 2, Fib= 321 
Lay= 1, IP= 3, Fib= 321 

FiberBundle#2:
MatID=82
Lay= 1, IP= 1, Fib= 123 
Lay= 1, IP= 2, Fib= 231
Lay= 1, IP= 3, Fib= 312

FiberBundle#3: 
MatID=28016 
Lay= 1, IP= 1, Fib= 321 
Lay= 1, IP= 2, Fib= 321 
Lay= 1, IP= 3, Fib= 321 
Lay= 2, IP= 1, Fib= 123 
Lay= 2, IP= 2, Fib= 123 
Lay= 2, IP= 3, Fib= 123 

FiberBundle#4: 
MatID=16
Lay= 2, IP= 1, Fib= 123 
Lay= 2, IP= 2, Fib= 123
Lay= 2, IP= 3, Fib= 123 

FiberBundle#5: 
MatID=61 
Lay= 2, IP= 1, Fib= 321 
Lay= 2, IP= 2, Fib= 321 
Lay= 2, IP= 3, Fib= 321

Fiber bundle material IDs are assigned to the respective through-thickness integration points in the *ELEMENT SHELL COMPOSITE( LONG) keyword.

Note 3

A specific clustering option has been implemented for the ARENA2036 Project - Digital Finger Print. The option aims to modify *ELEMENT SHELL COMPOSITE(LONG) integration point material IDs of certain target mesh elements, which are found using source mesh.

The mapping options should be defined as follows:

Algorithm=ElementSizeSearchRadius
Shell_Option=Composite (or, Composite Long)
NPLANE=<INT>
NTHICK=<INT>
MapStress=NO
MapStrain=NO
MapThickness=NO
NumIterations=<INT>
ClusterID#<INT>=&PID<INT>,<OPTION>,<DOUBLE>,<DOUBLE>,<INT> 

The integer on the left hand side indicates the target PID, to which clustering should be applied. The &PID option is supported only for this special case and the following integer defines the source PID to consider for clustering. <OPTION> can be ADDPID or AVG. The ADDPID option modifies the existing material ID by adding a user-defined value. The AVG option overwrites the existing material ID using the user-defined value. The following two <DOUBLE> entries have no effect on the routine, and any values can be defined that satisfy the format. The last <INT> value represents the user-defined value.