Finite Element simulation of vibrating plastic components

IEI

Mechanical Engineer - Solid Mechanics ISRN: LIU-IEI-TEK-A–13/01572–SE

Finite Element simulation of

vibrating plastic components

Master thesis

February 9, 2013

Author: Jesper Kihlander

Examiner: Larsgunnar Nilsson

Supervisor: Bo Torstenfelt

Abstract

For automotive plastic parts there is a clear demand on an increased quality of the FE models. This demand is related to the increased use of simulations, both due to a reduced number of prototypes and an increased number of load cases. There have been studies showing a change of dynamic properties in injection molded components. The conclusion from these studies are that the change depends on residual stresses built in during the injection process. This study use simple models to try to get a working method and from the results find out the basic relations between residual stresses and dynamic properties. A method was developed and the results showed that the residuals had a major impact on the dynamic properties. Continuation on this work would be to use more complex models, to try to mimic results from reference studies and tests.

Acknowledgements

I want to thank all people at Epsilon for helping me during the course of my master thesis. A special thank goes to Jens Weber, my supervisor, who helped throughout the process, even during evenings and weekends.

I also would like to thank my examiner Prof. Larsgunnar Nilsson from the department of solid mechanics, Linköping University for going through my report and giving me feedback and his thoughts on the overall state of this thesis.

Last, but not least, I want to thank all friends and family for help with proof-reading and overall support. You know who you are!

Göteborg February 9, 2013 Jesper Kihlander

Preface

This master theses is one part of a two part project, this thesis concerning residual stresses and their effect on dynamic behaviour and the other part/thesis examining the injection molding process. All results and parameters that are referred to the forming process and not stated otherwise is taken directly from the parallel project written by Andreas Östergren.

Copyright

The publishers will keep this document online on the Internet - or its possible replace-ment - for a period of 25 years starting from the date of publication barring exceptional circumstances.

The online availability of the document implies permanent permission for anyone to read, to download, or to print out single copies for his/hers own use and to use it unchanged for non-commercial research and educational purpose. Subsequent transfers of copyright cannot revoke this permission. All other uses of the document are conditional upon the consent of the copyright owner. The publisher has taken technical and administrative measures to assure authenticity, security and accessibility.

According to intellectual property law the author has the right to be mentioned when his/her work is accessed as described above and to be protected against infringement.

For additional information about the Linköping University Electronic Press and its pro-cedures for publication and for assurance of document integrity, please refer to its www home page: http://www.ep.liu.se/

c

NOMENCLATURE

G - Derivation of the shape function K - Stiffness matrix

Kσ - Stress stiffness matrix

L0 - Original length M - Mass matrix s - Stress matrix

f - Frequency

λn - Wavelength of the n:th harmonic

τ - Period of a sinus wave

υ - Wave propagation speed of a sinus wave ρ - Density

aT - Time temperature shift factor

αkl - Thermal expansion coefficients tensor

ξ(t) - Time scale cijkl - Stiffness tensor

cvrm_ijkl - Viscoelastic relaxations modulus P - Tension load t - Time T - Temperature σij - Stress tensor εkl - Strain tensor {φ} - Eigenvector µ - Eigenvalue ω - Circular frequency

ABBREVIATIONS

CAE - Computer aided engineering FE - Finite element

FEM - Finite element method

ABS - Acrylonitrile Butadiene Styrene d.o.f - Degree of freedom

List of Figures

1 Schematic picture of the injection molding process . . . 9

2 Full test rig with shelf and the laser vibrometer . . . 11

3 Picture showing the mounted front with shaker . . . 11

4 Frequency results for the front tested at Volvo GTT . . . 12

5 Picture showing the mounting of the shelf part . . . 12

6 Frequency results for the shelf tested at Volvo GTT . . . 12

7 String loaded in uniaxial tension . . . 16

8 Simulation result of the first eigenmode for a geometry with prescribed dis-placement (scale factor: 40) . . . 17

9 Simulation result of the second eigenmode for a geometry with prescribed displacement (scale factor: 40) . . . 17

10 Simulation result of the third eigenmode for a geometry with prescribed displacement (scale factor: 40) . . . 18

11 Simplified sheet geometry for fictional stress evaluation . . . 21

12 Deformation of the simplified geometry with applied fictional stresses and with boundary conditions preventing rigid body movement (scale factor: 50) 22 13 Master and slave node coupling used to simulate mounting . . . 22

14 Deformation of the mounted sheet, magnitude and lengthwise, with bound-ary conditions x- and y-position fixed at z and rotations set to 0 . . . 23

15 Deformation, magnitude and lengthwise, of the mounted sheet with approx-imated friction . . . 23

16 Simulation results of the six first eigenmodes, from left to right . . . 24

17 Geometry for the shell and solid models comparison . . . 25

18 Geometry used for Abaqus simulation . . . 26

19 Warpage results from Moldex 3D using a shell model (scale factor: 10) . . 27

20 The C3D10 element used in the solid FE model . . . 27

21 Deformation plots of the 3 layer model (scale factor: 10) . . . 28

22 Stress distribution after warpage of the three layer model . . . 29

23 Deformation plots of the five layer model (scale factor: 10) . . . 29

24 Stress distribution after warpage of the five layer model . . . 30

25 Deformation plots of the seven layer model (scale factor: 10) . . . 30

26 Stress distribution after warpage of the seven layer model . . . 31

27 Example on thickness loss with the use of shell elements . . . 32

28 Stresses (S11-S33) through the thickness of one of the vertical sides of the model . . . 33

29 Geometry used for Abaqus simulation . . . 34

30 Simulation setup with cooling channels used in Moldex 3D . . . 35

31 Boundary condition placement used in warpage analysis . . . 35

32 First 10 eigenmodes for closed u-profile model (displacement scale factor: 10) 37 33 Summary of the work flow developed in this master thesis . . . 40

List of Tables

1 Summery of material data for Terluran GP-22 . . . 9

2 Chemical configuration of the components in ABS . . . 10

3 Change in first eigenfrequency with change in tension . . . 16

4 Results and comparison from eigenmode simulation for a prescribed dis-placement . . . 18

5 Table showing the applied stresses (MPa) and their distribution in each element . . . 21

6 Frequency results from the simplified test cases . . . 24

7 Difference in frequencies between shell and solid formulations . . . 26

8 Summary of the deformations . . . 32

9 Frequency results for the first three free-free eigenmodes with and without residual stress . . . 33

10 Parameters used for the Moldex 3D study . . . 36

Contents

1.3.3 Test performed at Volvo GTT . . . 10

2 Theory 14 2.1 Residual stress and injection molding simulation . . . 14

2.2 Stress stiffening . . . 15

3 Software 19 3.1 Modal analysis and stress stiffening . . . 19

3.2 Moldex3D . . . 19

3.2.1 Assumptions . . . 20

4 Analyses 21 4.1 Simplified geometry with fictional residual stresses . . . 21

4.2 Switching from a shell model to a solid model . . . 25

4.3 Element type study for injection molding . . . 26

4.3.1 Shell . . . 27

4.3.2 Solids . . . 27

4.4 Effects of internal stress coming from an injection molding simulation . . . 34

5 Discussion 39

6 Future work 41

7 References 42

1

Introduction

For automotive plastic parts, mostly interior assemblies, there is a clear demand on an increased quality of the simulation models. The reason for this demand is an increased us of simulations related to both a reduced number of prototypes and an increased number of load cases as, e.g. Rattle and Squeak simulations and an increased demand on detail.

Based on test data it is known that dynamic properties of processed plastic parts can differ significantly from the material data given in a data sheet, which is based on a specimen. One explanation of the difference is the residual stresses caused by pre-processing/forming.

In this thesis a couple of simple models will be investigated to see if it is a viable method to use a structural FE simulation in combination with an injection molding simulation made to predict these changes in dynamic property. This project can be seen as a pre-study on the possibility to implement this kind of analysis for single parts with complex geometries or smaller interior assemblies of a car.

1.1

Objective

The objective of this master thesis is to investigate the effects of residual stress on a struc-ture, specifically dynamic properties such as eigenfrequencies. From physical testing there is evidence that show a significant change in eigenfrequency. In this thesis a component from a Volvo Truck will be used for the analysis.

This thesis will investigate the assumption that residual stresses affect the dynamic properties in processed components. These stresses are induced during the injection mold-ing process. By insertmold-ing these residual stresses in a modal analysis the assumption will be studied whether the residual stresses can lead to the observed change of the dynamic properties or not.

1.2

Approach

The major output from the injection molding simulation is a residual stress profile for the component, which then is input for the structural analysis. The residual stresses have to be mapped to the model as used for the structural, warpage and modal analyses.

The material and process parameters are taken from data sheets and information from the supplier/manufacturer. The software used for the injection molding simulation is Moldex3D [9]. The output from this analysis is a residual stress profile which is con-verted to an equivalent temperature load. This temperature load can then be imported into Abaqus [10] for the warpage analysis followed by the modal analysis.

1.3

Background

1.3.1 Injection molding

Injection molding is the most common method for manufacturing plastic components and is ideal for a high volume production. Injection molding is used to create a wide variety of parts such as packaging, bottle caps, some musical instruments parts, mechanical parts, and components for automotive interior. Some advantages of injection molding are the high production rates, repeatable high tolerances, the ability to use a wide range of materials, low labour cost, minimal scrap losses, and small need to finish parts after molding. Some

disadvantages with this process are expensive equipment, potential high running costs, and the need to design parts suitable to be produced by molding.

Figure 1: Schematic picture of the injection molding process

The injection molding process, Figure 1, starts with a hopper (1) being fed with plastic granulates. These granulates are then dropped into a heated barrel. In this heated barrel there is a screw-type plunger (2), the plastic granulates are then heated while forced trough the chamber. The melted plastic is then forced trough a nozzle (3) and into a two part mold (4/5, core/cavity) with the desired shape. The mold remains cold, often by the help of cooling channels, and the plastic therefore rapidly solidifies as the mold is filled. To avoid problems with shrinkage, when the material cools down, the filling process continues until solidification at the injection point.This, so called hold pressure, forces more material into the mold to counteract the shrinkage.

1.3.2 Material

The material used for the production of the above presented parts is Acrylonitrile Buta-diene Styrene or ABS. ABS is the polymerisation of Acrylonitrile, ButaButa-diene, and Styrene monomers. The advantage of ABS is high impact and mechanical strength, which is the reason for being highly used in automotive components. The specific type of ABS used in the studied parts is Terluran GP-22. This is an easy flowing grade ABS for injection molding with an impact modifier additive. In Table 1 a summery of the data sheet has been compiled with the common material data, for a full specification from the manufacturer, see Appendix A.

Table 1: Summery of material data for Terluran GP-22

Density 1.04 g/cm3

Tensile strength 45 MPa Hardness, Rockwell 103 HR Elongation to break 2.6% Vicat softening temperature 96 ◦C

Table 2: Chemical configuration of the components in ABS N CH2 Acrylonitrile H2C CH2 1,3-Butadine CH2 Styrene

1.3.3 Test performed at Volvo GTT

All comparisons in this paper will be made with results from the physical testing at Volvo GTT [7], the following chapter will summarise the testing and simulation done at Volvo GTT on this subject.

The tests where conducted on two components: the front part treated in this thesis and a related shelf which is included to further show the change in dynamic properties. The measuring equipment was a 3D laser vibrometer, because regular triaxial accelerometers were considered to add too much mass for this type of application. The positive effects of using a 3D laser vibrometer are that it does not add mass to the structure and that there is no limit on the number of measuring points, making it possible to capture even higher eigenmodes.

After the measurements with the vibrometer, mode shape identification was carried out at FRF peaks (running modes). Then a visual mode shape correlation between test and simulation has been performed, instead of a MAC-analysis. Since the parts are made from only one kind material the mode shapes are independent of the Young’s modulus.

If three to four mode shapes correlate in a relevant frequency range, then the Young’s modulus is the only free parameter to tune in order to correlate the frequencies according to the relation in (1).

ω ∼qk(E, t)/m (1)

A similar phenomenon was investigated in an article of Lieven and Greening (2001), but using a free-free setup.

Figure 2: Full test rig with shelf and the laser vibrometer

The front part was firmly screwed into place in each corner with a shaker at the lower left corner as seen in Figure 3.

Figure 3: Picture showing the mounted front with shaker

After the physical tests an FE-simulation was made for an equivalent setup. This simulation resulted in lower eigenfrequencies for the correlating mode shapes. An update of the Young’s modulus was then made, and seen in Figure 4. The Young’s modulus needed to be increased from the specified 2300 MPa to 3700 MPa in order for the frequencies to coincide with the physical test results.

Figure 4: Frequency results for the front tested at Volvo GTT

In the second test, the shelf showed the same phenomenon as the front. The properties were changed corresponding to a Young’s modulus of 2900 MPa. The test setup and results and be seen in Figures 5 and 6.

Figure 5: Picture showing the mounting of the shelf part

Figure 6: Frequency results for the shelf tested at Volvo GTT

From both these results it is observed, that with increased part complexity the increase in Young’s modulus is greater.

Based on the fact that the frequencies of all correlation mode shapes can be correlated by a single change of the Young’s modulus, the second conclusion was made, that the effect causing the dynamic property change obviously is isotropic. A similar phenomenon with change of dynamic properties was also seen in Lieven and Greening (2001). The conclusion after some further investigation was that this phenomenon probably is caused by residual stresses from the injection molding process, because it is directly connected to stiffness, which in turn depends on the Young’s modulus.

From both of these results one conclusion was drawn that with increased complexity the increase of Young’s modulus is greater.

According to the tests and analyses conducted at Volvo GTT there is a phenomenon affecting these two parts changing the Young’s modulus or properties that is connected to this physicality. A similar phenomenon with change in dynamic properties was also seen in Lieven and Greening (2001). The conclusion after some further investigation was that this phenomenon probably caused by residual stresses from the manufacturing process, because it is directly connected to stiffness, which in turn depends on Young’s modulus.

2

Theory

2.1

Residual stress and injection molding simulation

The prediction of residual stresses in injections molded products is highly demanded. Knowledge of residual stresses is essential to predict dimensional and shape inaccuracies of a product. Roughly there are three types of residual stresses that arise in the injection molding process.

• Flow induced stress. This affects on the molecular configuration of the material. • Pressure induced stress. This arises due to a fluid core that exists within the frozen

layer during the packing phase.

• Thermal induced stress. This arises from thermal contraction during the solidification process.

Of these three types of residual stresses , flow induced stress is an order of magnitude smaller than pressure and thermal induced stresses according to Baaijens (1991). But the flow induced stress has an important role as it contributes with large molecular orientation, which effects the mechanical behaviour of the finished product.

Residual stress models are generalisations of Hooke’s law, which according to Spencer (2004) has the form.

σij = ceijklεkl (2)

where σij are the stress tensor components, εkl are the total strain tensor components

and ce

ijkl are the stiffness tensor components. The small strain tensor is determined by

dif-ferentiating the components of the displacement vector u and the components are obtained as εij = 1 2 ∂ui ∂xj +∂uj ∂xi ! (3) According to Kennedy (2008) a formulation of the residual stress model, σij, can be

described with the viscoelastic constitutive relationship.

σij = t Z 0 cvrm_ijkl(ξ(t) − ξ(t0)) ∂εkl ∂t0 − αkl(ξ(t) − ξ(t 0 ))∂T ∂t0 ! dt0 (4) where cvrm

ijkl is the viscoelastic relaxation modulus, t is time, T is temperature, αkl is the

thermal expansion coefficients and ξ(t) is a time scale defined as

ξ(t) = t Z 0 1 aT dt0 (5)

where aT is the time temperature shift factor that accounts for the effect from

temper-ature on the material response.

A problem arises when Equation (4) is used for non-isothermal systems. Because of the complexity related to the viscoelastic data, it is common to approximate the problem with a viscous-elastic calculation in which the material is assumed not to sustain stress above

a certain temperature and is elastic below that temperate. Under this assumption σij can be obtained from σij =      0 for T ≥ Tt t R 0 cvrm,e_ijkl ∂εkl ∂t0 − αkl(t0)∂T_∂t0  dt0 for T < Tt (6) This equation is generally solved subjected to the following assumptions:

• The shear strains ε13= ε23 = 0 in local coordinates • The normal stress σ33 is constant across the thickness • As long as σ33 < 0, the material sticks to the mold walls

• Before ejection, the part is fully constrained within the plane of the part, i.e. the only non-zero component of the strain is ε33

• Mold elasticity is neglected

• The material behaves as an elastic solid after the part has been ejected

The residual stresses are calculated by FE analysis. The residual stress is then calcu-lated for each element at grid points through the thickness, which leads to

σij(e)(zi) =      0 for T ≥ Tt t R 0 cvrm,e_ijkl ∂εkl ∂t0 − αkl(t0)∂T_∂t0  dt0 for T < Tt (7) where (e) refers to the element and the stress is calculated in each grid point, zi. To

calculate the shrinkage of the part, the residuals are used as loading condition in a structural analysis. This requires specific boundary conditions to prevent rigid body motion. This is achieved by fixation of three non co-linear nodes.

Node 1: ux = uy = uz = 0

Node 2: ux = uy = 0

Node 3: uz = 0

These boundary condition will allow the part to shrink and deform freely, but yet prevent rigid body motion. Deformations can then be calculated to be used for the warpage and shrinkage determination.

2.2

Stress stiffening

The out-of-plane stiffness is highly affected by the in-plane stress in the structure. This coupling between stress and stiffening is known as stress stiffening and is most pronounced in thin, highly stressed structures.

The subsequent examples are used to show the stiffening effect on a simple geometry, before trying to apply it on more complex model.

A string that is loaded with some kind of pretension is an simple example to visualise the stiffening effect. In this example a string with uniaxial tension in x will be used, seen

in Figure 7.

Figure 7: String loaded in uniaxial tension

Analytical solution of this problem can be from the equation for the speed of wave propagation. The speed of wave propagation, υ, is given as wavelength, λ, divided by period, τ , or multiplied by frequency, f .

υ = λ

τ = λf (8)

If the string is of length, L0, the wavelength, λn, can be written as λn = 2L0/n of the n:th harmonic. Combined with Equation 8 the following expression for the n:th harmonic frequency can be derived.

fn=

nυ 2L0

(9) The wave propagation in a string is proportional to the square root of the tension, P , and the inverse of the square root of the density, ρ, of the string

υ = s

P

ρ (10)

Inserted into Equation 9

fn= n 2L0 s P ρ (11)

This equation can then be used to calculate any specific eigenfrequency for a given harmonic n. As comparison an FE simulation was made with three different load cases, using the above presented geometry. The results are presented in Figures 8, 9 and 10 along with Table 3.

Table 3: Change in first eigenfrequency with change in tension Case # Length (mm) Load (N) Simulation (Hz) Analytical (Hz)

1 300 0 16

-2 300 30 291 289

3 300 60 407 408

4 300 90 494 500

From Table 3 the major effect of stress is observed and how it affects stiffness is clearly illustrated.

As a second example of stress stiffening, the same string is used, but this time a pre-scribed displacement of 0.1% (0.3 mm) is used.

Figure 8: Simulation result of the first eigenmode for a geometry with prescribed displace-ment (scale factor: 40)

Figure 9: Simulation result of the second eigenmode for a geometry with prescribed dis-placement (scale factor: 40)

Figure 10: Simulation result of the third eigenmode for a geometry with prescribed dis-placement (scale factor: 40)

To compare these results a simulation of an unloaded geometry, without prescribed displacement, was made and the results can be seen in the table below.

Table 4: Results and comparison from eigenmode simulation for a prescribed displacement Mode # Without pretension (Hz) With pretension (Hz)

1 16 80

2 45 162

3 87 248

In this table if stress is introduced into the geometry, in this case by a prescribed displacement, the eigenfrequencies will change radically. In this example a displacement of 0.1% is used and the frequencies change with a factor of three to five.

So from these two examples a conclusion can be made that it doesn’t matter how the stress is presented into the geometry and how small it is, the eigenfrequencies and therefore part properties can change drastically.

3

Software

3.1

Modal analysis and stress stiffening

The eigenvalue problem for natural modes of small vibration is

(K − ω2M){φ} = 0 (12)

were M is the mass matrix, K is the stiffness matrix and {φ} is the eigenvector. Since all the problems in this master thesis all are under the influence of a stress stiffening effect. Too include this phenomenon the eigenvalue problem can be written as

({K + Kσ} − ω2M){φ} = 0 (13)

where Kσ is the stress stiffness matrix, see Cook et. al. (2002).

This stress stiffness matrix is directly linked to stress from the geometric stiffness. Cook et. al. (2002) uses the following expression

Kσ = Z GT     s 0 0 0 s 0 0 0 s     GdV (14)

where G is derived from the shape function

G = ∂N ∂X (15) and s =     σx τxy τzx τxy σy τyz τzx τyz σz     (16)

According to Abaqus Theory Manual (2012) the eigenvaule problem (13) can be solved in Abaqus with one of two approaches: the Lanczos algorithm or the subspace iteration method.

If one uses the method from the tests at Volvo GTT, presented in Section 1.3.3, the change in stiffness matrix will be isotropic with Young’s modulus. However there is nothing in above presented theory, Equation 14, hindering the change in stiffness to be anisotropic. To use residual stresses as a load case and to update the stiffness matrix, a non-linear simulation in Abaqus must be done. At the end of this non-linear warpage analysis a new stiffness matrix is calculated and this updated stiffness matrix is then used for the modal analysis in the following step.

3.2

Moldex3D

The injection molding simulation using Moldex3D can provide information on the thermo-mechanical properties and residual stresses. This information is written to interface files for subsequent FE stress analysis.

All mechanical properties and residual stresses are calculated by Moldex3D and written to the interface files as orthotropic constants at points through the thickness of the part. This means that each individual thickness section/layer will all have the same properties.

In order to capture the characteristics of the plastic flow it is important to have enough layers in an element, but at the same time the amount of layers should be kept at a minimum to reduce the computation time . Models without oriented fibres are referred to as "unfilled", as it is the case for this thesis.

Moldex 3D uses linear shell or solid elements, for the simulations. To reduce the problems and minimise errors due to mapping between different meshes the same element type will be used in the subsequent Abaqus simulation, with the modification of being second order triangular elements in the Abaqus simulation.

3.2.1 Assumptions

For three-dimensional solid simulations a number of assumptions regarding the topology and properties of the data is made in the Moldex3D simulation, to ensure compatibility with the Abaqus simulation. Only assumptions concerning the material and simulations in this thesis are listed below.

1. Moldex3D translates the tetrahedral elements to an identical mesh of Abaqus four node linear tetrahedron (C3D4) or 10-node quadratic tetrahedron (C3D10) elements. (a) C3D4 are known to be too stiff. Therefore it is recommended to always use parabolic elements when using tetrahedral elements, due to the errors with this added stiffness.

2. Orthotropic material constants are in terms of material principal directions. 3. Material properties are constant for each element layer.

4. The temperature of the model at the end of the analysis is taken to be uniform at the ambient temperature specified in the Moldex3D analysis.

(a) This assumption can be considered reasonable due to the thin nature of the used components

4

Analyses

4.1

Simplified geometry with fictional residual stresses

In this section a study is made to investigate if residual stresses causes the observed change in dynamic properties presented in Section 1.3.3.

One important aspect with correcting the frequencies through Young’s modulus is that one gets an isotropic change. This might not be the case as shown in Section 3.1.

For this analysis/example a simplified geometry of the shelf will be used. The geometry will be a rectangular sheet with the dimensions 950x250x3 mm as seen in Figure 11. This sheet will then be loaded with a fictional residual stress, which is linearly distributed through the thickness, from max value at one side to zero at the other. The magnitude of this stress will be determined from a desired warpage value of about 4 mm. The applied stresses can be seen in Table 5. This loaded geometry is then compared to an unstressed geometry with and without an adjusted Young’s modulus.

Figure 11: Simplified sheet geometry for fictional stress evaluation

Layer # σx (MPa) σy (MPa) τxy (MPa)

1 0 0 0

2 0.075 0.0375 0

3 0.15 0.075 0

4 0.225 0.1125 0

5 0.3 0.15 0

Table 5: Table showing the applied stresses (MPa) and their distribution in each element

The same boundary conditions as presented in Section 2.1 will be used for this geometry. The corners will be fixed in the following way, numbered from the lower left corner: corner 1 will be fixed in all directions x = y = z = 0, corner 2 will be fixed in x = y = 0, corner 3 in z = 0 and corner 4 free. This will not allow rigid body movement but will not hinder deformation.

Figure 12: Deformation of the simplified geometry with applied fictional stresses and with boundary conditions preventing rigid body movement (scale factor: 50)

With the above presented stress profile, a warpage magnitude of 3.96 mm is achieved, seen in Figure 12. A simulation of mounting the sheet was also made to mimic the setup used at Volvo GTT. This is achieved through a kinematic master and slave node coupling in each of the four holes, seen in Figure 13, and then controlling the master nodes to simulate screws going through the holes.

Figure 13: Master and slave node coupling used to simulate mounting

To capture the mounting process the z-coordinate along all rotations in the master node was set to 0, while x- and y-coordinates were fixed at the resulting modified position, as if they were allowed to move freely until pinned down between the screw and surface below. The result from this mounting process can be seen in Figure 14.

Figure 14: Deformation of the mounted sheet, magnitude and lengthwise, with boundary conditions x- and y-position fixed at z and rotations set to 0

This setup does not take into account that the screws movement will be hindered by friction from the underlying surface and contact pressure between screw and shelf. This value is very hard to approximate, but in this example a reduction a lengthwise deformation of 0.01 mm, about 20%, from -0.04 mm to -0.05 mm is used to simulate the effect. The resulting deformation and corresponding eigenmodes can be seen in Figures 15 and 16.

Figure 15: Deformation, magnitude and lengthwise, of the mounted sheet with approxi-mated friction

Figure 16: Simulation results of the six first eigenmodes, from left to right

All mode shapes are identical in the different cases, because all changes are made on a stress and not geometry level. In Table 6 a summary of all frequency results can be seen.

Table 6: Frequency results from the simplified test cases Mode # Without fictional stresses (Hz) Infinite friction (Hz)

1 5.7 2.6 2 14.0 11.7 3 15.8 13.1 4 29.9 27.2 5 31.2 28.0 6 49.1 46.6

Mode # No friction (Hz) 20% friction (Hz)

1 5.7 5 2 14.0 13.7 3 15.8 14.8 4 29.9 29.4 5 31.2 30.2 6 49.1 48.5

From Table 6 it is observed that the frequencies do not change without the friction. This is because all residual stresses in the structure may relax and cause deformation. Thus the impact from the stresses have on the stiffness is removed.

To find out if this fictitious stress renders the sought results in the case of 20% friction, a simulation with an adjusted Young’s modulus resulted in an approximate change to 2200 MPa. This is not the magnitude found at Volvo GTT [7], but due to the simplicity of the geometry and the magnitude of the applied stress the results can be seen as valid.

It is important to choose the correct friction coefficient, if friction should be included. For the extreme case of an infinite friction the results cannot be approximated with a Young’s modulus. Zero friction coefficient will almost nullify the effect from the residual stress because all residual stresses can convert into warpage.

The applied residual stress does not have an isotropic effect like the Young’s modulus, which makes it hard to approximate with an isotropic property. It should however be noticed that the geometry is a very simple and has a simplified residual stress profile.

4.2

Switching from a shell model to a solid model

In Section, 4.1, it was shown that fictional stresses on a shell model showed the observed phenomenon. The next step is to investigate how/or if a solid FE element changes the results.

Two identical plates, like in Section 4.1, were modelled, seen in Figure 17. One using shells elements and one using solid elements, both with a prescribed displacement load of 0.9 mm to investigate the different results when updating the stiffness matrix.

Figure 17: Geometry for the shell and solid models comparison Results from the dynamic simulation can be seen in Table 7.

Table 7: Difference in frequencies between shell and solid formulations

Shell with Solid with

Mode # Shell (Hz) displacement (Hz) Solid (Hz) displacement (Hz)

1 2.6 24.4 2.6 24.1

2 10.6 49.7 10.6 49.1

3 12.7 28.0 12.7 27.7

4 24.0 76.5 24.0 75.7

5 27.1 56.5 27.1 56.0

From the results in Table 7 the conclusion is that the type of element formulation does not affect the frequency results to a considerable amount. The decision of element formulation to be used is thus not dependent on element type.

4.3

Element type study for injection molding

In this section a brief study will be made trying to investigate what element formulation to use. With increased layers/elements in the thickness the results from Moldex 3D should become better, but at the cost of calculation time. So this section will investigate the optimal configuration for both accuracy and efficiency, i.e. if it is possible to do the simulations with a solid element or if a shell formulation is better.

All results vary from the different solvers (Moldex 3D/Abaqus) so the presented values are taken from Abaqus if not stated otherwise. The parameter of interest is stress. This due to the fact that stress is the contributing factor for tangential stiffness and change in dynamic properties.

The used geometry is an open u-profile, seen in Figure 18.

4.3.1 Shell

The warpage achieved with a shell model, with 15 thickness layers per shell element, in Moldex 3D was a maximum magnitude of 3.6 mm, see Figure 19.

Figure 19: Warpage results from Moldex 3D using a shell model (scale factor: 10) A problem arose with this shell model and the conversion to Abaqus, since the results acquired did not reflect any stress variations through the thickness of the elements. The only solution to this problem is to use a solid element model.

4.3.2 Solids

Figure 20: The C3D10 ele-ment used in the solid FE model

The positive effect of changing the element formulation from shell to solid is that the results now captures deformation through the thickness. Due to the solidification of outer layers while the middle layers still is liquid, the stress will be positive in the core while being negative on the surface. This leads to a contraction effect and creating an inward buckling on all surfaces.

Also cooling phenomena can be captured, example of these effects are seen in Figure 22(c). In this figure its seen that the outer side of the corners have lower stresses while the inner sides have an area of higher stresses. There is a collection of heat caused by having more material per cooling channel on the inside of corners, which create uneven cooling in these areas.

The major negative effect of using solids is the need for a

simulation, which leads to large models. So in this element study three cases will be presented, all using an Abaqus element called C3D10, see Figure 20, which is a 10-node tetrahedron. The first case is a solid model with three elements in the thickness direction, the second model has five and the third model has seven.

For the simulation with three elements in the thickness direction, the following results are acquired.

(a) Side view (b) Isometric view

(a) Isometric view (b) Side view

(c) Cut side view

Figure 22: Stress distribution after warpage of the three layer model

The next step is to increase the number of elements in the thickness direction, chosen number of elements is five. This will increase the number of nodes through the thickness from seven to 11, the deformation results from these simulations can be seen in Figures 23 and 24.

(a) Side view (b) Isometric view

(a) Isometric view (b) Side view

(c) Cut side view

Figure 24: Stress distribution after warpage of the five layer model

In the last model seven elements are used. This number is chosen in order to match the shell elements used in Section 4.3.1, which uses 15 calculation points through the thickness. More elements than this is deemed unnecessary, because these models will demand too long calculation times to be a viable option.

(a) Side view (b) Isometric view

(a) Stress, S11 (b) Stress, S22

(c) Stress, S33 (d) Isometric view

(e) Side view (f) Cut side view, Mises stress

Figure 26: Stress distribution after warpage of the seven layer model

As seen in Figure 22 there is a stress distribution in the thickness direction but with this resolution of the mesh the effects cannot be captured. To solve this lack of calculation points in the injection molding simulated in Moldex 3D, the number of calculation points in the thickness direction is increased, which will then increase the resolution of the flow simulated by Moldex 3D.

this model. The different stresses, tension and compression, are clearly defined and the zone were the change happens is clearly visible.

However there are still areas that would benefit from a mesh refinement, in Figure 25 and 26 the seven layer model can be seen.

The results from the seven layers model shows that the deformation results seem to have converged to around 4 mm for Abaqus and 3.6 for Moldex 3D. A problem arose using a model of this size, since injection molding calculation time increased significantly. The increase in calculation time has not improved the results by the same factor and therefore might not justify the increase of precision, both in the stress, Figure 26, and warpage, Figure 25.

A comparison of the results from the four cases, summarised in Tables 8 and 9, shows that the shell model from Moldex 3D gives reasonable warpage results but could not be transferred to Abaqus format and could therefore not be used for an eigenmode calculation.

Table 8: Summary of the deformations Case Abaqus (mm) Moldex 3D (mm)

Shell - 3.6

3 elements 4.5 4.0

5 elements 4.0 3.6

7 elements 3.9 3.6

Figure 27: Example on thick-ness loss with the use of shell elements

The stress created in the structure has a variation through the thickness of the structure and in the corners, see Figures 26(a)-26(f).

The stress variation seen is a compression stress on the surface and a tension stress in the core of the model. These forces create a negative pressure inside the structure causing an inward buckling, i.e. like removing the air in a closed container.

This effect can clearly be demonstrated by a simple plate example. A rectangular plate with an applied temperature difference, see Figure 27. A negative temperature, is applied in the middle of the block and this creates the same effect as is present for the solid model. The negative stress on the surface and the positive stress in the core forces the plate to deform inwards, an effect which is not present with our shell model formulation.

As previously mentioned, Section 2.2, it is the in-plane stress that is the biggest con-tributor to the stiffness. As seen in Figure 28 the in-plane stresses, S22 and S33, are very similar for all three solid models. This means that the stiffness will be similar and therefore also their eigenmodes. The small variation of the shape, due to the increase of simulation points, in the stress plot has a contribution. But seen in Table 9 this does not have any significant effect for this simple model.

Figure 28: Stresses (S11-S33) through the thickness of one of the vertical sides of the model To find a model that will result in decent results from all aspects, both in Moldex 3D and Abaqus, a model needs about five elements through the thickness. However this makes the solid model only usable for small models, due to high calculation times.

Since the primary goal is to investigate the effects of residual stress and the connected tangential stress, a solid model with three elements in the thickness direction seems suf-ficient to estimate stresses. However when using results from this model, one should be aware of the too high warpage values that comes from the increase of total stress, seen by comparing S22 and S33 in Figure 28.

Another indicator that points towards three elements being sufficient, is the frequencies. From the frequency evaluations there are only a small variation in the results between different solid element cases. This can be explained by studying the stress state of the models seen in Figure 28. A comparison between all solid cases, seen in Table 9, shows the difference in stress does not considerably affect the frequencies.

Table 9: Frequency results for the first three free-free eigenmodes with and without residual stress

Case Mode #1 (Hz) Mode #2 (Hz) Mode #3 (Hz)

Shell - - -3 elements 66.3 103.9 141.7 3 elements w. residuals 64.6 93.5 138.5 5 elements 66.1 103.5 140.8 5 elements w. residuals 64.0 92.1 137.9 7 elements 66.1 103.5 140.8 7 elements w. residuals 64.0 92.1 138.0

The conclusion is that the best thing would be to use a shell element model for the larger scale simulations. However since this is not possible, see Section 4.3.1, the only solution is to use a solid model. Results in Table 9 show the number of elements through the thickness direction does not affect the frequency change in any significant way, which leads to the final model using three elements through the thickness. With this choice it is known that the received deformation will be a too high estimation of the real value and must be used as such.

However this is only a recommendation for larger models. For the continuation of this project, seven elements through the thickness will be used to eliminate as many sources of errors as possible.

4.4

Effects of internal stress coming from an injection molding

simulation

A more complex geometry was chosen for this study but still kept at a low detail level. The geometry used in Abaqus and the setup in Moldex 3D can be seen in Figures 29 and 30. To capture the residuals inside the model some rigid constraints where added to the open end. This will prevent some stress to convert into warpage mimicking corners and ribs in real automotive geometries.

Figure 30: Simulation setup with cooling channels used in Moldex 3D

The boundary conditions used for all simulations using Abaqus are set at the location of the injection gate. Three points evenly distributed were fixed in all degrees of freedom seen in Figure 31. These points were chosen to simulate the cooling process of an injection molded part which often happens with residual gate plastic still attached.

Figure 31: Boundary condition placement used in warpage analysis

the parameters seen in Table 10.

Table 10: Parameters used for the Moldex 3D study

Property Value

Cooling channel temperature 50 ◦C Cooling channel flow 120 cm3_/s

Filling time 4.5 s

Mold temperature 50 ◦C Melt temperature 250 ◦C

Packing pressure 185 MPa

All frequency simulations uses a free-free setup to remove effects from outer sources, like boundary conditions. The results can be seen below in Figure 32 and a frequency comparison with stressed and unstressed geometries in Table 11

(a) Mode 1 (b) Mode 2 (c) Mode 3

(d) Mode 4 (e) Mode 5 (f) Mode 6

(g) Mode 7 (h) Mode 8 (i) Mode 9

(j) Mode 10

Table 11: Comparison of frequencies with and without residuals Closed u-profile Closed u-profile Mode # without residuals (Hz) with residuals (Hz)

1 151.2 149.4 2 285.8 279.6 3 463.6 470.4 4 471.7 449.2 5 614.6 582.4 6 671.5 639.0 7 675.3 647.5 8 706.0 673.0 9 748.9 728.2 10 969.3 999.2

Open u-profile Open u-profile without residuals (Hz) with residuals (Hz)

1 66.1 64.0 2 103.5 92.1 3 140.8 138.0 4 258.1 239.7 5 299.8 276.6 6 357.7 343.6 7 512.4 488.5 8 663.5 633.7 9 716.7 684.2 10 940.8 891.9

The internal stress has a clear effect on the eigenfrequencies, as seen in Table 11. All frequencies have changed a considerable amount. Notice that frequencies three and 10 have increased while the other eight have decreased. This fact show the anisotropic property of stress discussed in Section 3.1. This effect would be missed if the Young’s modulus is used as the correction parameter. When trying to estimate the property change with Young’s modulus a decrease from 2300 MPa to 2100 MPa was achieved.

From these results there is evidence that the internal stress could be the cause of the dynamic property change seen at Volvo GTT. Though frequencies have decreased rather than increased there is still a significant change. The stresses built into the material is geometry dependent which makes it hard to draw parallels between a decrease on this model and the increase measured in the physical tests at Volvo GTT.

5

Discussion

The first example was a plate with fictional stresses to investigate if it was possible to use stresses to change the Young’s modulus and thereby the dynamic properties. To get these tests as close to the known results as possible, the mounting process was also included in the simulation. It was concluded that both the stress and the mounting process had a big impact on the resulting eigenfrequencies. From this it was deiced to use a free-free setup for the following models to exclude the effects of mounting. The results from this was positive and a change in the dynamic properties was achieved.

From this an investigation of the effect from the element type was conducted. Two equivalent simulations were made, one using shell elements while the other used solid elements. From the simulation results the conclusion were that the choice of element did not affect the results, if the mesh was of a similar density.

The positive effects from using a solid element formulation is that thickness dependent properties could be seen, e.g. properties like thickness deformation and corner effects. Solid formulations also results in an better understanding of the stress distribution in the components. However the downside of using a solid element model was the increase in computing time and this created a precision versus time scenario. If more elements were added, the overall results got better, but the computing time became so long that it was deemed impossible to use more then three elements in the thickness direction, with our computational resources, to keep the simulation times in a realistic interval. This decision was made on the fact that the crucial parameters, stresses and eigenfrequencies, did not increase in precision at the same rate as the computing times went up. To be able to apply the method on bigger geometries the number of elements was kept at a minimum.

With two u-profile models the injection molding process were tested, including how the results should be converted to stress stiffening in Abaqus. If a solid model was used, all results converted nicely with all properties through the thickness. However with a shell model the results did not include stress variations through the thickness, but showed what was interpreted as a mean stress.

Because the stress profile could not be calculated, the effect from the injection molding process and, therefore, the correct change in stress stiffening and eigenfrequency was lost. The results from these analyses showed that Abaqus could translate stress into a modi-fied stiffness. While not being what were expected, the results showed a change in dynamic properties. From this we tried to recreate the results using a variable Young’s modulus to approximate the found results. It was concluded that it was possible to make an approx-imation with Young’s modulus, but the found change with residual stresses was clearly anisotropic. In some cases it was hard/impossible to approximate the correct eigenmodes with an isotropic constant like the Young’s modulus.

A closed u-profile is used to investigate if a trapping of the stress inside the geom-etry would increase the effect from the residual stress and might lead to an increase of eigenfrequencies.

Results showed that the magnitude of the change in frequency did not change this model. However, an interesting change was that the enclosing of stress made some eigen-frequencies increase, unlike previous results that showed a decrease in eigenfrequency. This points to the fact that a more complex geometry is needed to enclose the residual stresses and to receive an increase in eigenfrequency, i.e. the one found at Volvo GTT and by Lieven and Greening [8].

We have in this project through several small examples shown that the residual stress from injection molding has an effect on the dynamic properties. What the results did

not reflect was the increase in eigenfrequencies that first was observed at Volvo GTT and in related articles. However a significant change was found in all FE models, both with increase and decrease of eigenfrequencies. The conclusion from this is that the FE models used in this thesis were of too simple nature to show an increase in eigenfrequencies. The model the showed the effect most was a u-profile closed with rigid elements. Which showed that an increase could happen and that an increase requires a more complex model than the ones used.

The different models and varied results, that have all shown a change in eigenfrequen-cies. An understanding and a good work flow has been developed.

It is hard to exactly say if a corresponding phenomenon happened in the Volvo GTT test, but it is an indication that residual stresses have a great influence on the properties of injection molded products.

6

Future work

The next step for this project would logically be to use the parts presented in Section 1.3.3 for further analyse. Both of these parts would be good choices because they vary in complexity, manufacturer can supply some information on the process, and measurements have been done. These two components would then be controlled and example of real life models.

This would give a good picture on how certain parameters and geometrical features affect residual stresses. The models could be scaled down to be handled by a single testing machine, and should give a reasonable computational time.

These two components also give the possibility to test how residuals work as properties in an assembly. The injection molding simulation is the bottleneck in the process and because this will be done on part level, assembly tests would only require some more computing time to evaluate the frequencies and eigenmodes.

However the best choice to further deepen the understanding would be to contact a local producer to get better control/information of process parameters, placement of cooling channels and other process specific data. This would eliminate errors from old schematics and pictures.

If further analyses is to be done on this project, it would be wise to try to solve the problem with shell elements. Though the core process works with solid elements, it benefit from using the shell formulation.

7

References

[1] Abaqus, 2012. Theory Manual. Paris; Dassault Systems

[2] F.P.T. Baaijens. 1991. Calculation of residual stress in injection molded products. Rheologica Acta, Vol. 30, 284-299.

[3] A.J.M. Spencer. 2004.Continuum Mechanics. New York: Dover Publications

[4] P.K. Kennedy. 2008. Practical and scientific aspects of injection molding simulation. Eindhoven.

[5] R. D. Cook, D. S. Malkus, M. E. Plesha, R. J. Witt. 2002. Concepts and applications of Finite Element Analysis, 4th Edition. Wiley, pp. 646-647 and pp. 651-652

[6] P. Postawa, D. Kwiatkowski. 2006. Residual stress distribution in injection molded parts Journal of Achievements in Materials and Manufacturing Engineering, Vol. 18, 1-2, 171-174

[7] Volvo GTT. Access to company documents regarding physical test results, courtesy of Volvo GTT

[8] N. A. J. Lieven, P. Greening. 2001. Effects of experimental pre-stress and residual stress on modal behaviour. The Royal Society, 359, 97-111

[9] http://www.moldex3d.com/en/, 2013-02-04

Terluran® GP-22

Acrylonitrile Butadiene Styrene Styrolution

1 of 2

Copyright © 2011 - IDES - The Plastics Web ® | 800-788-4668 or 307-742-9227 |www.ides.com.

The information presented on this datasheet was acquired by IDES from the producer of the material. IDES makes substantial efforts to assure the accuracy of this data. However, IDES assumes no responsibility for the data values and strongly encourages that upon final material selection, data points are validated with the material supplier.

Revision History

Document Created:  Wednesday, November 30, 2011 Added to Prospector:  April, 1999

Last Updated:  9/22/2011

Product Description

Terluran GP-22 is an easy flowing grade of ABS for injection molding with high resistance to impact and heat deflection. General

Material Status • Commercial: Active

Availability • Asia Pacific • Europe • North America

Additive • Impact Modifier

Features • Good Flow_{• High Heat Resistance} • High Impact Resistance_{• Impact Modified}

Agency Ratings • EC 1907/2006 (REACH)_{• FDA Unspecified Rating} • NSF 14_{• NSF 51} • NSF 61_{• ULC Unspecified Rating}

RoHS Compliance • RoHS Compliant

Appearance • Natural Color

Forms • Pellets

Processing Method • Injection Molding

Multi-Point Data

• Creep Modulus vs. Time (ISO 11403-1)

• Isochronous Stress vs. Strain (ISO 11403-1)

• Isothermal Stress vs. Strain (ISO 11403-1)

• Secant Modulus vs. Strain (ISO 11403-1)

• Shear Modulus vs. Temperature (ISO 11403-1) • Specific Volume vs

Temperature (ISO 11403-2)

• Viscosity vs. Shear Rate (ISO 11403-2)

Physical Nominal Value Unit Test Method

Specific Gravity 1.04 g/cm³ ASTM D792_{ISO 1183}

Melt Volume-Flow Rate (MVR)  

200°C/5.0 kg 1.50 cm³/10min ASTM D1238

220°C/10.0 kg 19.0 cm³/10min ASTM D1238_{ISO 1133}

230°C/3.8 kg 4.80 cm³/10min ASTM D1238

Molding Shrinkage - Flow 0.55 % ASTM D955

Water Absorption (Saturation, 23°C) 1.0 % ASTM D570

Mechanical Nominal Value Unit Test Method

Tensile Modulus (23°C) 2300 MPa ASTM D638_{ISO 527-2}

Tensile Strength  

Yield, 23°C 45.0 MPa ASTM D638_{ISO 527-2}

Yield, -40°C 63.0 MPa ISO 527-2

Yield, 80°C 19.0 MPa ISO 527-2

Break 2 _{34.0 MPa ASTM D638}

Tensile Elongation  

Yield, 23°C 2 _{2.6 % ASTM D638}

Yield, 23°C 2.6 % ISO 527-2

Nominal Tensile Strain at Break (23°C) 10 % ISO 527-2

Flexural Modulus (23°C) 2300 MPa ASTM D790

Flexural Strength (23°C) 65.0 MPa ASTM D790_{ISO 178}

Terluran® GP-22

Acrylonitrile Butadiene Styrene Styrolution

Wednesday, November 30, 2011

2 of 2

Copyright © 2011 - IDES - The Plastics Web ® | 800-788-4668 or 307-742-9227 |www.ides.com.

The information presented on this datasheet was acquired by IDES from the producer of the material. IDES makes substantial efforts to assure the accuracy of this data. However, IDES assumes no responsibility for the data values and strongly encourages that upon final material selection, data points are validated with the material supplier.

Revision History

Document Created:  Wednesday, November 30, 2011 Added to Prospector:  April, 1999

Last Updated:  9/22/2011

Impact Nominal Value Unit Test Method

Charpy Notched Impact Strength ISO 179

-30°C 8.0 kJ/m²  

23°C 22 kJ/m²  

Charpy Unnotched Impact Strength ISO 179

-30°C 100 kJ/m²  

23°C 180 kJ/m²  

Notched Izod Impact ASTM D256

-30°C 60 J/m  

-18°C 100 J/m  

23°C 300 J/m  

Unnotched Izod Impact Strength (23°C) 26 kJ/m² ISO 180

Hardness Nominal Value Unit Test Method

Rockwell Hardness (R-Scale) 103   ASTM D785

Thermal Nominal Value Unit Test Method

Deflection Temperature Under Load  

0.45 MPa, Unannealed 91.0 °C ASTM D648

0.45 MPa, Unannealed 103 °C ISO 75-2/B

0.45 MPa, Annealed 104 °C ASTM D648

1.8 MPa, Unannealed 78.0 °C ASTM D648

1.8 MPa, Unannealed 99.0 °C ISO 75-2/A

1.8 MPa, Annealed 99.0 °C ASTM D648

Vicat Softening Temperature 96.0 °C ISO 306/B50_{ASTM D1525} 3

CLTE - Flow 0.000095 cm/cm/°C ISO 11359-2

Electrical Nominal Value Unit Test Method

Volume Resistivity > 1.0E+13 ohm·cm ASTM D257_{IEC 60093}

Dielectric Constant  

1.00 mm, 1 MHz 2.80   ASTM D150

100 Hz 2.90   IEC 60250

1 MHz 2.80   IEC 60250

Dissipation Factor IEC 60250

100 Hz 0.0048    

1 MHz 0.0079    

Comparative Tracking Index 600 V IEC 60112

Electric Strength (1.50 mm) 37 kV/mm IEC 60243-1

Notes

1 _{Typical properties: these are not to be construed as specifications.}

2 _{51 mm/min}