Virtual Subcomponent Tests for Validation

Damage behavior

Initiation (MPa) Evolution (kJ/m²) Stabilization (-)

t^max_n 110.0 GIc 1.564 η 0.00125*

t^max_s 300.0 G_IIc 4.3

t^max_t 300.0 G_IIIc 4.3

bkcoef f (-) 1.75**

Cohesive behavior Uncoupled traction separation behavior

Knn(MPa) 9500 Kss (MPa) 38000

Ktt (Mpa) 38000

*Viscosity stabilization coefficientη from Gao et al. [59]

**Benezeggagh-Kenane coefficientbkcoef f from Camanho et al. [60]

Figure 4.6: Midsurface model and dimensions to create a shell representation of the hat profile

(a) (b)

(c) (d)

Figure 4.7: 3PB/4PB test setups: (a) 3PB experimental; (b) 4PB experimental; (c) 3PB virtual; (d) 4PB virtual

interaction behavior. The strikers and supports were set as Master-Surfaces and the corresponding hat profile faces were assigned Slave-Surfaces. An overview of the input values for the contact property definition is given in Tab. 4.11.

Table 4.11: Strikers/supports-hat contact property input parameters Tangential behavior Normal behavior

Penalty: µ(-) 0.3 "Hard" Contact

The supports were fixed in all degrees of freedom (DOF), and the striker locked in all DOF except for movement in Y-axis direction. The load is applied displacement controlled (limit displacement of striker = 8 mm). To ensure an uniformly load appli-cation in the virtual 4PB tests, an additional reference point was created, labeled as RP-1 in Fig. 4.8, and a kinematic constraint was defined between this point and the corresponding striker points (see Fig. 4.8).

Figure 4.8: 4PB virtual test setup

Abaqus C3D8R 3D stress elements were used to mesh the hat profile geometry and to create the solid model. A global mesh size of 2 mm with 4 elements in thickness direction was defined, as pictured in Fig. 4.9 (b). Furthermore, the material orientations for each element were defined with the primary orientation in longitudinal direction and the using discrete orientation definition tool. 3D simulations were performed using the Abaqus/Standard static general solver.

(a) (b)

Figure 4.9: 3D modeled hat profile: (a) unmeshed; (b) meshed

A python script was programed usingPython 2.7 to create the shell models of the hat profile with various degrees of complexity in terms of the material modeling approaches.

The schematic of the developed script is given in Fig. 4.10.

Figure 4.10: Schematic of the virtual 2D model generation

The developed python program consists of 4 files: (i) a definition file, for selection of the desired simulation model (3PB, 4PB, mesh size, ply thickness an orientations, material properties, step properties, ...); (ii) a creation file to create the selected sim-ulation model by importing the values from the definition file; (iii) a file consisting of algorithms for generation of random or uniform ply thickness and orientation values;

(iv) and a simulation file for starting the simulations and evaluation of the results. The functionality of the developed script is explained in the following. The shell model of the hat profile is automatically partitioned into 7 regions (see Fig. 4.11(a)) byAbaqus due to face intersections. The script provides the option of further partitioning and generation of RRVEs with dimensions given in Tab. 4.12, see Fig. 4.11 (b)-(c).

Table 4.12: RRVE dimensions according to [1]

RRVE Length (mm) ×Width (mm) Number of regions

0 no partition 7

1 23.4×23.4 96

2 11.7×11.7 384

3 5.85×5.85 1512

(a) (b)

(c) (d)

Figure 4.11: Hat partition (a) RRVE-0; (b) RRVE-1; (c) RRVE-2; (d) RRVE-3 Fig. 4.12 (a)-(d) shows the partitioned hat profiles with the created RRVE regions colored.

(a) (b)

(c) (d)

Figure 4.12: Hat partition color map (a) no partition; (b) RRVE-1; (c) RRVE-2; (d) RRVE-3

In step (ii), the script assigns composite layups to each region. In a recently published work, Stelzer et al. [2] characterized the cured platelet thickness of CF-SMC to be on average by employing X-ray computed tomography scans of the material. This value was adopted for the calculation of the number of plies per thickness in the composite layup. The cured hat thickness divided by the cured platelet thickness resulted in 20 platelets through thickness. Therefore, 20 plies were generated for each RRVE and the material behavior was assigned.

In step(iii), the orientation algorithm is called. If uniform orientation values was de-fined, a quasi isotropic laminate model with angles of [0/±36/±72/90/]s adopded from Schürmann [55] was created. Irregular orientation values were defined using Pythons inbuilt pseudo-random module for generation of a random integer between (-90,90).

Subsequently, the thickness algorithm was called for either generation of constant or pseudo-random thickness values. A constant ply thickness of 0.15 mm was assigned to each ply of a RRVE if the thickness value was set to be uniform. The algorithm also provided the option to generation pseudo-random thickness values. The algorithm applied for pseudo-random thickness generation was adopted from [1]: (i) Fractions of platelets were generated for each ply (possible orientation) by using Pythons ran-dom.random() function; (ii) The fraction values were multiplied with the cured platelet thickness and added to the thickness of the corresponding ply; (iii) a loop repeated steps (i) and (ii) until the sum of thickness values from individual plies was equal to

The orientation and thickness algorithms returned arrays which were updated for every RRVE, therefore it was possible to assign different orientation and/or thickness values to each RRVE independently.

The script further provides the possibility of including a discrete field containing ro-tation values for each meshed element around the elements surface normal axis in the model. The script allows for mesh sizes variations, which leads subsequently to changes of element numbers. Therefore, discrete fields were created by (i) writing of an input file after the hat was fully defined and meshed; (ii) reading the number of elements from the input file; (iii) creation of a discrete field consisting of the element number and a corresponding randomly generated rotation value; (iv) assignment of the discrete field to the corresponding hat.

For inclusion of cohesive interface properties, the hat profile can be subdivided into a chosen number of sub-hat-layers (see Fig. 4.13). The corresponding sub-hat thickness was calculated according to Eq. 4.1:

t_hat,sub= t_hat,total

ninterf ace+ 1 (4.1)

, wheret_hat,total is the total hat thickness,t_hat,sub is the thickness of the sub-hat and n_{interf ace} is the number of desired interface regions. The script called the hat creation files ninterf ace+ 1 times for generation of the hat profiles. These layers were stacked and composite plies were assigned according to their thickness values. Furthermore, a surface cohesive interaction property was assigned between the layers starting from top (according to y-value) to the bottom hat profile, where the hat with the higher y-value was set as "Master" and the corresponding lower profile as "Slave" to simulate their interfacial behavior.

(a) (b)

(c) (d)

Figure 4.13: Stacking examples: exploded view of a) 2, b) 10 stacked hats; side view of accurately stacked c) 2, d) 10 hats

All 2D simulations were performed using the Abaqus/Standard dynamic implicit solver. A mesh sensitivity study was conducted utilizing the 2D-Stochastic approach (see Fig. 4.10) with M1 material behavior. Furthermore, a mesh sensitivity study has been performed using global mesh sizes of 0.5 mm, 1 mm, 2 mm, 3 mm, 4 mm and 6 mm with a virtual 3PB setup. Stiffness values from these tests were observed to remain unchanged after further decreasing of the mesh-size from 3 mm to values below, whereas the strength results were increased by approximately 25% when changing the mesh-size from 2 mm to 0.5 mm. Unfortunately, computation times are increased from several hours (mesh-size = 2 mm), up to several days (mesh-size = 1 mm /0.5 mm).

Computer specifications are shown in Tab. 4.13.

Table 4.13: Computer specifications OS: Windows 10 Pro, 64-Bit CPU: Intel Core i7-2600, 3.40 GHz

RAM: 8.00 DDR3

Therefore, it was decided to perform all simulations with a mesh-size of 2 mm (Fig. 4.14 (b)) because edges were expected to be meshed too coarse when using 4 mm elements.

3D simulations were performed with a meshsize of 2 mm with four elements in thickness

(a) (b)

Figure 4.14: Mesh sensitivity study: (a) mesh-size = 4 mm; (b) mesh-size = 2mm detection of several different influences on simulation results:

• RRVE size influence has been investigated by testing 4 sizes according to 4.12

• the effect of cohesive zone interfaces has been analyzed by comparison of simula-tion models incorporating one, three and nine cohesive interfaces

• for characterization of ply thickness influences, models exhibiting uniform ply thickness values were compared to simulations with randomized ply thicknesses

• random generated orientation values have been compared to fixed orientation values adopted from [55]

Additionally, the script was used to create a set of 8 specimens with the same setup, but different fiber orientations to investigate the models ability of generating stochastic meso-structures. The sensitivity study has been carried out in order to find the best fitting simulation model for the investigated CF-SMC material. Subsequently, 3PB and 4PB simulations have been performed utilizing this model employing M1 and M2 material behavior (see Section 4.2). The obtained results were validated by comparison with experimental data.