Schmailzl Anton, Amann Thomas, Glockner Markus, Fadanelli Martin, Prof. Dr.-Ing. Marcus Wagner: Head of FEM-Laboratory

Transcription

1 Finite element analysis of thermoplastic probes under tensile load using LS-DYNA compared to ANSYS Workbench 14 in correlation to experimental investigations Schmailzl Anton, Amann Thomas, Glockner Markus, Fadanelli Martin, Prof. Dr.-Ing. Marcus Wagner: Head of FEM-Laboratory Prof. Dr. Ing. Stefan Hierl: Head of LMP-Laboratory UNIVERSITY OF APPLIED SCIENCES Regensburg Regensburg, Germany Summary Joining thermoplastics is a popular technique to build sophisticated plastic applications. Therefore the laser-transmission welding process is used to join thermoplastic polymers where welds are often not visible at all. The clamping force in this case plays a decisive role when it comes to weld quality. Simulating the clamping pressure with finite element techniques is therefore highly attractive to optimize the principal of the process. Thermoplastic polymers under tensile load often show a brittle behavior coupled with softening. Simulating such materials is quite difficult for FEM-programs. In this paper a finite element study of the tensile test in LS-DYNA and ANSYS Workbench 14 with respect to the material models is analysed. The experimental data is validated in comparison with the FEMsolution for a tensile test. The material models and the problems in simulating softening behavior for thermoplastic polymers are discussed. Keywords thermoplastics, plastics, nonlinear material, material modeling, LS-Dyna, ANSYS, ABS, softening, NLISO, MAT 24, MAT 187, laser transmission welding

2 Motivation In nearly every kind of technical application thermoplastics are involved. Welding is a common joining technique for many plastic applications. Compared to other welding techniques the laser transmission welding offers significant advantages like no or low melt blow out, no vibration or ultrasonic load. Since more than ten years laser transmission penetrates the plastic welding marked and already has become an established joining technique. The process is shown in fig.1. Small joining zones and a good performance for visible welding zones make the process interesting for several industrial applications. The laser penetrates a transparent polymer and is fusing an absorbing polymer. The heated absorbing polymer heats the transparent polymer by heat conduction. The clamping pressure between the joining partners plays a decisive role regarding the quality of weld seam. [8] Fig. 1. Left: Principle of laser transmission welding (ltw), right: x-section of a weld seam To deal with these circumstances, FEM-methods to determine the clamping pressure between the joining partners are attractive for the technical use of the process. The material behavior during the welding process is essential for the FEM-analysis. Therefore, a benchmark for nonlinear FEMsimulation with ANSYS Wb 14 and LS-DYNA was materialized. A tensile test of an ABS (Acryl- Butadiene-Styrene) polymer was analysed to provide material parameters for the simulation with respect to the deformation speed. 1. Mechanical behavior of ABS The test specimen for the tensile test distiniguishes between brittle, ductile with and without a yield stress point. [2,5] Generally the mechanical behavior of ABS can be characterized as brittle. [7] First plastic strain occurs at the yield stress of MPa. At the Stress of 38 MPa strong sliding leads to a decrease in stress. The fracture behavior is crack induced because of crazes. [] The stress strain behavior analysed in the tensile test at a deformation speed of 1mm/min and a fractured probe is shown in fig Stress [MPa] Strain [%] Fig. 2. Tensile test of ABS specimen with deformation speed 1mm/min

3 The irreversible lateral contraction at fracture is not visible in a macroscopic analyses. According to the test specimen DIN 527 [2] the material properties for a specific probe are shown in Tab.1. Tab. 1. Material properties of ABS yield stress MPa nominal strain at break 6,5 % tensile modulus 20 MPa stress at break 34 MPa possions ratio 0,3 (assumption) The necking effect of this ABS specimen is slightly distinct. The elastic region before reaching the yield stress shows a good correlation between the six tensile tests. At a deformation speed of 500 mm/min fracture occurs earlier and the material behavior is more brittle without plastic flow. Elastic material models seem to be adequate to describe the mechanical behavior if focus is on the elastic region. Stress [MPa] Strain [%] Fig.3. Material behavior at a deformation speed of 500 mm/min Stress-strain values have to be implemented in true stress and true strain for fem analysis. [4] Therefore, the experimental data is transformed into Hencky-Strain, and Cauchy-stress. [3,6] εhtot = ln(1 + ε) τ = σ(1 + ϵ) 2. Simulation with ANSYS Wb Material models for elasto-plastic behavior There are several material models in ANSYS Wb 14 which describe elasto-plastic material behavior. To simulate the damage of the material beyond the yield stress there are difficulties to deal with. For example the decreasing stresses which cause convergence problems. The material models BLISO, MLISO as well as BLKIN and MLKIN can not handle the damage of the material. To simulate the elasto-plastic region in front of the yield stress point elasto-plastic models are adequate. The decreasing stresses disappear at high strain rates and the material acts more brittle so that an elastic material model is often adequate (compare to Fig.3). To simulate the elastic-plastic region for low strain rates the material model MLISO has been chosen. This model uses an isotropic hardening rule with a multilinear elastic-plastic model.

4 The data for plastic analysis in ANSYS have to be implemented in plastic strain and Cauchy stress. In this case the total strain has to be substracted from the elastic strain. [1] εp = εhtot τ E0 The material model MLISO therefore needs the tensile modulus and the Poissons ratio for the elastic model. For plastic analysis the plastic strain and the Cauchy stress are needed. The first calculated plastic strain should be set to zero so the calculation keeps running. [4] 2.2 Material models for the softening behavior ANSYS provides a material model that uses a non-linear-isotropic-hardening (NLISO) rule. It is possible to describe the hardening behavior in an exponential equation. σ = k + R0 epl + Rinf (1 e b epl ) Softening can be simulated if the Rinf parameter is negative. The visco-plastic formulations of Perzyna have to be implemented for a converging solution. εpl = γ σ 1 m σ0 1 It is possible to use the material model NLISO in an reversed way to describe softening. A computational fitting is needed to generate the material parameters. In fig. a NLISO fitting (red) and the experimental data (blue) of the tensile test are shown. Fig.4. Curve fitting for NLISO 2.3 Load Settings To analyze the mechanical behavior the geometry of the tensile test is modelled and analysed with a static-mechanic simulation (compare to fig.5). The mechanic load is a displacement of 2,05 mm and a restriction of a fixed support was implemented on the other side to create a mechanical model of the tensile test. Necking can occur several times due to the fact that there are many nodes where the stress is at the same level. The homogeneous zone was created with a concave radius of R=000 mm, which is still in the tolerance of DIN 527 [3], to create one necking zone.

5 Fig. 5. Geometry and loads of the tensile probes 2.4 Mesh Settings To get a homogeneous mesh the sweep setting is used to create a mesh with an element size of 1 mm. The used element type was SOLID Solution The deflection of ABS induced by the Poisson effect is at a low-level, the force reaction induced from the displacement can be used to calculate the stress in the homogeneous area. Since there is less Poisson deflection at fracture, this approximation is probably appropriate. The maximum stress in the detected zone can be analysed with the normal stress tool. The displacement of the homogeneous zone has to be identified to get the strain of the probe. Therefore, the displacement of the lines D and E in the global coordinate system are recorded. The induced geometric nonlinearity can be regarded with a tick at the option LARGE DEFLECTION. When simulating thermoplastic material, elastic material modelling is even at two percent strain not appropriate compareable according to Fig stress [MPa] / fault [%] linear material - large deflections off linear material - large deflections on fault linear material - large deflections off fault linear material - large deflections on experimental data strain [%] Fig.6. Deviation between elastic material formulation and experimental data As shown in fig.6., the linear material formulation in correlation to the nonlinear material behavior goes up to percent deviation. To show the deviation between experimental and the simulated values the experimental data in fig.6, 7, 8 was snipped at 2.5 percent strain. The deviation between experimental data and simulated values when using the MLISO material model is still under five percent as shown in fig.7. Therefore six stress strain points were implemented in the material model MLISO which uses a linear stress strain formulation between the data points.

6 stress [MPa] / fault [%] large deflection off large deflection on fault large deflection off fault large deflection on experimental data strain [%] Fig. 7. Deviation between elasto-plastic formulation and experimental data The elasto-plastic behavior in front of the yield stress is tested with a second load step. In the second load step the displacement was set to zero as shown in fig stress [MPa] Large deflection on Large deflection off Experimental data strain [%] Fig. 8. Elasto-plastic hysterese behavior The elasto-plastic behavior of the strains are appropriate when analysing the irreversible deformation induced by loads. 2.6 Results The elasto- plastic behavior models for ANSYS Wb 14 are adequate for analyses with brittle thermoplastic materials. When using an elastic material model the error can reach up to % because of nonlinear material behavior. For high strain rates elastic material models are appropriate. For the elasto- plastic material model MLISO the deviation is less than five percent.

7 3. Simulation in LS-DYNA LS-Dyna provides more than 0 material models. For the simulation of the tensile test a nonlinear material model is needed. There are several models which occur in connection to the simulation of thermoplastics. For example, Mat_003, Mat_019, Mat_024, Mat_076, Mat_081, Mat_082, Mat_089, Mat_112, Mat_123, Mat_141 and Mat_187. Two material models were selected for the simulation. Mat_024 because it is very common in use with the simulation of steel components. Mat_187 is one of the latest material models and is especially developed for thermoplastics. 3.1 Characteristics of Mat_024 and Mat_187 Mat_024 is an isotrop, strain rate dependent elasto-plastic material model that uses a user-defined stress versus strain curve. A failure criterion is implemented by using plastic strain or a minimum time step size. Mat_187 uses an isotrop yield surface and is a strain-rate dependent elasto-plastic material model. The yield point of typical thermoplastics is lower for pulling than for pushing. Therefore, material models that are based on uniaxial loading tests, as Mat_024 is, deliver to small values. For a better representation of thermoplastics. Mat_187 uses separate stress-strain curves for pressure, shear, bi-axial strain and uniaxial strain at different strain rates. Therefore, a lot of experimental investigations are necessary. The yield surface is a quadratic function defined by the four load curves as shown in Fig. 11. Fig.9. Yield surface [15] 3.2 Computation with Mat_024 and Mat_187 Hexahedron elements are used for meshing the geometry by sweep method. The element size is 1 mm. Solid elements with constant stress are used for the simulation. Explicit dynamic is used for short time phenomenas. For the tensile test referring to DIN a displacement velocity of 1 mm/min is recommended. To keep the computation time slow the displacement velocity is increased to 0mm/s. This results in oscillations, especially at fracture of the probe. Therefore, fracture is prohibited by not inserting a fracture criterion i.e. plastic strain at fracture. PRESCRIBED_MOTION_SET DOF=1 VAD=0 BOUNDARY X=1 ROTX=1 Y=1 ROTY=1 Z=1 ROTZ=1 BOUNDARY X=0 ROTX=1 Y=1 ROTY=1 Z=1 ROTZ=1 Fig.. Boundary conditions of the tensile test in LS-DYNA

8 3.3 Analysation and results For the analysis and comparison of simulation and experimental data with MATLAB some values are necessary. The cross section area of the tensile probe as well as the force in pulling direction can be written down by using plots. According to DIN the change of length in a tensile test with thermoplastics is related to a measuring length of 50 mm. Node history of two nodes (with 50 mm distance in pulling direction) shows the displacement of each node. The difference between both displacements is the resulting change of length of the tensile probe. Mat_024 and Mat_187 show almost the same characteristics until reaching the yield stress. There is a maximum deviation of 3% between experimental data and simulation in the linear elastic region as shown in Fig.13. Tension rapidly decreases at maximum stress. The curve is not computed correctly in this area. Necking occurs at both material models because of the negative curve gradient. Stress is decreasing in the plastic area with Mat_024 because of further stress localization at higher strains. Mat_187 shows a growing plastic zone instead of further stress localisation at higher strains, also shown at Fig.13. Therefore, Mat_187 is reflecting the true mechanical behavior of the experimental tests better than Mat_24 does. The deviation of Mat_187 is below 3% in the plastic area, compared to Mat_24 with a maximum deviation of.2%. Mat024 Mat187 Fault Mat024 Fault Mat187 Experimental Stress [MPa] / Fault [%] 0 Mat_187 Mat_187 Mat_ Strain [%] Fig.11. Experimental and simulated stress-strain curve with LS-DYNA The results show that simulation below the yield point, as needed for the simulation of the clamping pressure in the welding process, is possible with both material models but Mat_187 is the better choice if plastic area is needed. Both materials are not able to simulate the softening of the experimental data correctly. ABS shows a very untypical mechanical behavior at low strain rates as DIN recommends. The negative gradient usually disappears by transforming the engineering stress versus engineering strain in true values because the stress is related to the remaining instead of the original cross section area. ABS shows no increasing stress related to the remaining cross section area, which means that there

9 is still a slope. This slope leads to numerical problems. There are two possible solutions to fix this problem if needed: Fix the experimental data by removing the decrease in stress strain relation (positive gradient). This leads to a hardening. If necking is desired it is necessary to insert a slope in the modified true stress vs true strain curve. Introduce artificial visco-plasticity. To test the solution by fixing experimental data all experimental values behind the yield stress in the stress strain curve are deleted and one last curve point (stress) is added at maximum strain. This stress has to be higher than the yield stress to reach a positive gradient. The three curves in fig. 14 show the difference in the resulting stress-strain curve when using a stress value of 39 MPa, MPa and 42 MPa. The yield stress is 38.8 MPa MPa 42 MPa MPa 39 MPa True Stress [MPa] Set Point: 39MPa Set Point: MPa Set Point: 42MPa Simulation-39MPa Simulation-MPa 5 Same Simulation Results For Mat024 And Mat187 Simulation-42MPa Referenz True Strain [%] Fig.12. Modifying the experimental curve to a positive gradient Modifying the stress-strain curve seems to be very sensitive to the gradient and is therefore not recommended in this case. 4. Conclusions Simulating the clamping pressure between joning partners is highly attractive to optimize the laser transmission welding process. To cope with softening behavior of some thermoplastic materials the available material models of ANSYS Workbench 14 and LS-DYNA are analysed. Simulating the mechanical behavior of thermoplastics with elasto-plastic material models is quite simple for FEprograms. The deviation between simulated and experimental data for ANSYS Workbench 14 and LS DYNA is less then three percent. The material models of both programs have problems in solving the FE-equations when softening occurs. With ANSYS Workbench 14 it is possible to simulate softening behavior with the material model NLISO. Due to the fact that providing the parameters for the material model requires a computational fitting the awareness of the maximum strain to distinguish between the material models is useful. If the maximum strain is below the messured yield stress elasto-plastic material models are adequate. The material model MAT_24 and MAT_187 in LS- DYNA also can not handle mechanical behavior with decreasing stresses. Softening of the ABS is not computed correctly with both material models. Nevertheless, Mat_187 is reflecting the true mechanical behavior of the experimental tests better than Mat_24 does because of an increasing plastic zone instead of further necking. Deviation in the plastic area is beyond three percent with Mat_187.

10 5. References [1] A. Arriaga et. al. Finite-element analysis of quasi-static characterisation tests in thermoplastic materials: Experimental and numerical analysis results correlation with ANSYS. Polymer Testing 07(26): [2] Deutsches Institut für Normung. DIN 527 Bestimmung der Zugeigenschaften Teil 2 Prüfbedingungen für Form- und Extrusionsmassen; (527-2). Berlin: Beuth Verlag; 1996 [3] Ehrenstein GW. Polymer-Werkstoffe: Struktur - Eigenschaften - Anwendung. 3rd ed. München: Hanser, Carl;. [4] Gebhardt C. Praxisbuch FEM mit ANSYS Workbench: Einführung in die lineare und nichtlineare Mechanik. München: Hanser; 11. [5] Peter Eyerer et. al (ed.). VDI- Buch: Prüfung von Kunststoffen und Bauteilen. Berlin, Heidelberg: Springer Berlin Heidelberg; 08. [6] Stommel M, Korte W, Stojek M. FEM zur Berechnung von Kunststoff- und Elastomerbauteilen. München: Hanser; 11. [7] W.-S. Lee, H.-C Shen. Comparisons of deformation and fracture behavior of PC/ABS blend and ABS copolymer under dynamic shear loading. Maney for the Institute of Materials, Minerals and Nining 04. [8] Michaeli W, Potthoff A. L.,Gillner A. Konstruktive und verfahrenstechnische Aspekte zum Laserdurchstrahlschweißen großformatiger, dünnwandiger Kunststoffbauteile: Teil 1: Virtuelle Oprimierung von Kunststoffbauteilen für den Laserdurchstrahlschweißprozess. Joining Plastics (), Nr. 3-4, S [9] Tom V. Material Modeling Guidelines; Available from: ( ). [] Wolfgang R. Mechanik der Kunststoffe: die mechanischen Eigenschaften von Polymer- Werkstoffen. München: Hanser; 1991.