Modelling of Mixing in an Extruder using CFD

(1)

MASTER'S THESIS

Modelling of Mixing in an Extruder using

CFD

Gustaf Alnersson

2016

Master of Science in Engineering Technology Engineering Physics and Electrical Engineering

Luleå University of Technology

(2)

A

BSTRACT

Abstract

The mixing of wood-polymer composites inside an extruder was modelled using Com-putational Fluid Dynamics (CFD) and the software Ansys CFX. The motions of the mixing blocks inside the extruder were modelled using the immersed boundary method, which avoids re-meshing in each time step. Two different models were used; one with a stopping block and one without. The purpose of the stopping block is to ensure that the flow stays inside the mixing region for a longer time. The flow field was initialized in two different ways; one starting from a steady state-solution, and one starting directly from a specified flow field and specific volume fraction. The results indicate that the stopping block works as intended. The general conclusion is that immersed solids is a promising method, but more work is required.

(3)

(4)

P

REFACE

This work has been carried out at the Division of Fluid and Experimental Mechanics at Lule˚a University of Technology. I would like to thank my supervisor, Anders Andersson and my examiner, Staffan Lundstr¨om, for their help and support during this period. Gratitude should also be extended to Anton Burman and Jeroen Henrard for making the office space a better place. My family should also be thanked for their support.

Gustaf Alnersson Lule˚a, June 2016

(5)

(6)

C

ONTENTS

Chapter 1 – Introduction 1

1.1 Extrusion . . . 1

1.2 Wood-polymer composites . . . 1

1.3 Outline of this work . . . 2

Chapter 2 – Theory 3 2.1 Immersed solids . . . 3

2.2 The Courant-Freidrichs-Lewy condition . . . 4

2.3 Richardson extrapolation . . . 4

Chapter 3 – Model description 7 3.1 Geometry . . . 7 3.2 Meshing . . . 9 Chapter 4 – Setup 11 4.1 General assumptions . . . 11 4.2 Boundary conditions . . . 11 4.3 Materials . . . 12 4.4 Multiphase . . . 12 4.5 Transient conditions . . . 12

4.6 Grid convergence study . . . 13

Chapter 5 – Results 15 5.1 Richardson extrapolation . . . 15 5.2 Streamlines . . . 16 5.3 Volume fractions . . . 19 5.4 Shear flows . . . 22 Chapter 6 – Discussion 27 6.1 General . . . 27 6.2 Future work . . . 27 6.3 Conclusion . . . 28

(7)

(8)

C

HAPTER

1 Introduction

The purpose of this project has been to use Computational Fluid Dynamics (CFD) to simulate the flow of fluids inside an extruder; more specifically, the mixing of polymers with wood fibres.

1.1 Extrusion

Extrusion is a process in which molten material is forced through a die. In the case of polymer extrusion it is also used in order to homogenize the material [11]. However, since it is difficult to measure the flow inside the extruder it is necessary to use simulations to be able to understand the flow. There have been quite a few attempts at doing this using various methods. Eitzlmayr and Khinast [4] used Smoothed Particle Hydrodynamics and obtained results similar to CFD. Eitzlmayr et al. [5] modelled the process as a iD-problem and obtained results similar to experimental data. Gupta [7] used a process which allowed simulations of rotating screw in a twin screw extruder without having to regenerate the mesh between time steps.

1.2 Wood-polymer composites

Wood-polymer composites are materials based on polymers where wood fibres have been added to alter the properties of the material, for instance increasing the durability or making it resistant to mould. The creation of wood-polymer composites is an area that has grown substantially in the past 20 years, and there has thus been quite some research on the subject [12]. However, to the authors best knowledge, the absolute majority of this research has been focused on experimentally developing new polymers, and not on modelling the process itself.

(9)

1.3 Outline of this work

In this work, immersed solids have been used to model the motions of the mixing blocks in the extruder. Immersed solids is a method first proposed by Peskin [13], and it has since been used in a variety of applications [10]. This method has also recently seen use in the modelling of extruders [9], [8].

Two different geometrical models are tested; one with a stopping block and one without. The idea behind the stopping block is to ensure that the flow stays in the region with the mixing blocks for a longer time. To test the impact of this is one of the goals.

There are some limitations to the use of immersed solids in this works, however. This is mainly due to the fact that the software used, Ansys CFX, has some limitations to their implementation; for instance, it is not possible to model heat transfer from immersed solids to fluids, and particles do not respect immersed solids either.

(10)

C

HAPTER

2 Theory

The fundamental way of describing all flow is the Navier-Stokes equation ∂ui ∂t + uj ui xj = −ρ∂p ∂xi + ν ∂ 2_u i ∂xj∂xj + Fi (2.1)

where ui is the flow velocity, p is the pressure, ν is the kinematic viscosity and Fi is a

force term. The continuity equation

∂ui

∂xi

= 0 (2.2)

is also required [2]. Note that Eq. (2.2) is only valid for incompressible flow.

The turbulence model used is the k −ε model. This two-equation model is the probably most widespread one, since it is both relatively simple and relatively accurate for a wide range of different cases. It does not resolve the flow near walls, and uses wall functions instead [14].

2.1 Immersed solids

The use of immersed solids is a way of modelling solid objects that move inside a fluid. The method is an alternative to physically moving the object and creating a new mesh for every time step. Here instead all nodes that lie inside the solid are listed, and this list is updated for every time step.

In Ansys, the flow is modified by the immersed solid by adding an extra term Si to Eq.

(2.1), defined as

Si = −αβC ui− uFi

(2.3) uF

i are velocity components based the motion of the immersed body. C is called the

(11)

to be large. The symbol α is called the momentum source scaling factor. A lower value improves convergence, and a higher value improves accuracy at the cost of convergence. The solid itself is modelled by the β term, called a special forcing function, which will be 1 for nodes inside the solid and 0 for other nodes. It is possible to use this as a function for near-wall treatment as well, in which case the function is weighted for nodes near the boundaries to better represent the forcing [1].

2.2 The Courant-Freidrichs-Lewy condition

The Courant-Freidrichs-Lewy condition is one condition that must be fulfilled in order to ensure that a solution is stable. It can be described as following [6]:

u∆t

∆x ≤ Cmax (2.4) Here u is the speed of the flow, ∆t is the time-step, Cmax is the maximum allowed

Courant number, and ∆x is the length interval. In this case the length interval is the representative edge length, which is is calculated as

h = V N

1/3

(2.5) Here V is the volume of the entire mesh, and N is the number of elements.

It should be noted however that it is not strictly necessary to use 1 when solving in CFX because of the implicit solver it uses.

2.3 Richardson extrapolation

The purpose of Richardson extrapolation is to ensure that the discretization error tends towards zero as the mesh becomes infinitely fine [3]. Representative edge lengths (Eq. (2.5)) are calculated for three different meshes, and these meshes should ideally have a refinement factor of at least 1.3, calculated as

ri =

hi+1

hi

(2.6) Here the denominator is always larger than the nominator; thus ri is greater than 1. The

difference between the values of the studied parameter for the different meshes is then obtained from

εi = Fi+1− Fi (2.7)

where F is the variable that is studied in this case. The apparent order p is then computed, and in this case

(12)

p = ln ε2 ε1 + q ln(r2) (2.8) q = ln r p 2 − s rp₁ − s (2.9) s =sign ε2 ε1 (2.10) It should be noted that in this case the values of p and q must be calculated using an iterative procedure. Next the extrapolated values of the variable are calculated as

Fext,32= r₃₂p F3− F2 rp₃₂− 1 (2.11) Fext,21= r₂₁p F2− F1 rp₂₁− 1 (2.12) These extrapolated values are an estimation of what the studied parameter will be if an infinitely fine mesh is used.

(13)

(14)

C

HAPTER

3 Model description

Two different models have been used: one with a stopping block and one without. These stopping blocks are used to partly hinder the flow from leaving the mixing zone and thus enabling a better mixing.

3.1 Geometry

(15)

(a) No stopping block.

(b) With stopping block.

Figure 3.2: The model of the extruder.

(16)

In Fig. 3.1 the mixing blocks can be seen. Each individual block has a thickness of 4.0 mm, which means that the total length of the mixing zone is 16.0 mm. The length of each are 18.0 mm from tip to tip, and they are 4.0 mm wide at the widest.

In Fig. 3.2a, the different inlets and the outlet are defined. 1 points to the inlet for the polymer, 2 points to the inlet for the solvent and 3 points to the outlet. The inlets and the outlet are the same in the model with a stopping block.

The two different extruder models that have been used can be seen in Fig. 3.2. Each pipe has a diameter of 10.0 mm, and the distance from the midpoint of the pipes to the origin is 8.0 mm, which makes the total width of the extruder 36.0 mm.

The extruder without a stopping block has a total length of 32.0 mm, of which 16.0 mm are added to allow the flow to stabilize.

The extruder with the stopping block has a total length of 33.0 mm, with the thickness of the stopping block itself being 1.0 mm.

3.2 Meshing

(17)

Figure 3.4: The mesh of a mixing block.

The mesh seen in Fig. 3.3 is a schematic image of the mesh used for the extruder, while Fig. 3.4 is a schematic image of the mesh of the mixing blocks. Both meshes are built entirely of tetrahedral elements.

(18)

C

HAPTER

4 Setup

All simulations have been carried out in the software Ansys CFX.

4.1 General assumptions

Several assumptions were made during the modelling of the problem:

Both fluid were assumed to be Newtonian, i.e. that they have a constant viscosity. The particles that in reality are injected along with the non-polymer fluid are

neglected and assumed to be evenly distributed in the solvent.

All temperature-dependant phenomena, most notably the vaporization of the sol-vent, are neglected.

Many of these simplifications are due to the way immersed solids are implemented in CFX. The implementation does not, for instance, account for particles and temperature-dependant phenomena.

4.2 Boundary conditions

All walls have a no-slip condition, and this is also used on the stopping block. An opening boundary condition is used on the outlet, with zero gradient conditions for the multiphase flow. On both the inlets a specific mass flow was used, which can be seen in Table 4.1. The two mixing blocks were set as immersed solids with specified rotational speeds. No near wall treatment was used since it seems CFX cannot handle this forcing if there is more than one phase.

(19)

Volume fraction Water Volume fraction Polymer Mass flow [g/s]

Top inlet 1 0 0.51

Bottom inlet 0 1 0.17

Table 4.1: Boundary conditions on the two inlets.

Material Density [kg/m3_] _{Dynamic viscosity [P a · s]}

Water 997 8.899 · 10−4 Polymer 1240 2.208 · 10−3

Table 4.2: Some properties of the materials used.

4.3 Materials

The two materials used are water and a polymer called IngeoTMbiopolymer model 4032D. These biopolymers are created directly from plant material instead of from oil. Some material properties can be seen in Table 4.2.

4.4 Multiphase

For the interaction between the two fluids, the Mixing model in CFX was used. This is a simple way of modelling mixing between two liquid phases [1].

4.5 Transient conditions

As previously mentioned, it is not necessary to account for the Courant numbers (see Eq. 2.4) in great detail since CFX uses an implicit solver; however, the high rotational speeds of the mixing blocks necessitates the use of rather small time steps. In these simulations, a time step of 0.005 seconds was used, since this allows the motion of the blocks to be captured in a good way, and also results in low Courant numbers.

Two different methods of initialization were also tested, one where the simulations were initialized from steady state simulation where the blocks did not rotate, and one with a specified velocity field of zero and water in the entire domain. The transient simulations were initiated from steady state-simulations unless otherwise specified.

For the cases of steady state initialization a total simulation time of 4 seconds was used for cases without stopping block, and a total simulation time of 12 seconds was used for cases with a stopping block. For the cases with the alternative initialization a 4 seconds were used when no stopping block was present, and 6 seconds were used otherwise.

(20)

No. of elements Representative edge length [m] 5.8 · 105 _{2.554 · 10}−4

1.195 · 106 2.0071 · 10−4 2.706 · 106 _{1.5284 · 10}−4

Table 4.3: The meshes used and their representative edge lengths.

4.6 Grid convergence study

A grid convergence study was preformed where the shear velocity, ushear=

∂ui

∂xj

(4.1) along a line running from the origin along the z-axis were used for the extrapolation. The values were taken from steady state-simulations of a single phase flow. The evaluated meshes are listed in Table 4.3.

(21)

(22)

C

HAPTER

5 Results

5.1 Richardson extrapolation

Figure 5.1: Richardson extrapolation

As can be seen in Fig. 5.1, the difference between the finest mesh (2.706 million elements) and the extrapolated values is not that great, and the edge length from that mesh has thus been used in the rest of the simulations. A finer mesh could possibly have given

(23)

better results, but with the available computational power this would have been very time-consuming.

5.2 Streamlines

(a) The polymer. (b) The solvent.

Figure 5.2: Streamlines for the two fluids at a rotational speed of 150 rpm.

(24)

Figure 5.5: Streamlines for the two fluids at a rotational speed of 150 rpm with a stopping block.

(25)

Figure 5.6: Streamlines for the two fluids for a rotational speed of 150 rpm with the alternative initialization.

Figure 5.7: Streamlines for the two fluids for a rotational speed of 150 rpm with stopping block and the alternative initialization.

The streamlines in Figs. 5.2-5.7 portray the superficial velocity, i.e. the hypothetical velocity that the given phase would have if it was the only one flowing in the area. This means that more streamlines for one fluid compared to the other in a specific case means that the fluid with more streamlines represents a greater part of the total motion of the fluids. The streamlines are generated from 100 seed points for both fluids.

Looking at Figs. 5.2-5.4, it can be seen quite clearly that for lower rotational speeds there

(26)

are more streamlines for the solvent than for the polymer, and as the rotational speeds go up this relationship is reversed. This is probably related to the different viscosities of the fluids. It should be noted that the colour scales are different in the three figures, so the velocities are the lowest in Fig. 5.2 and the highest in Fig. 5.4. Given that the latter has the highest rotational speed, this is to be expected.

Looking at Fig. 5.5 it can be seen that a greater fraction of the streamlines stay in the area where the mixing blocks are placed. Since the intended purpose of the stopping block is to keep the flow circulating in this region for a longer time, this is to be expected. The alternative initialization does not seem to alter the existing trend to any great degree, since if Figs . 5.6 and 5.7 are compared to Figs. 5.2 and 5.6 respectively the difference is that in both cases there are fewer streamlines for the polymer and more for the solvent if the alternative initialization was used.

5.3 Volume fractions

(a) Two planes. (b) Slices.

Figure 5.8: The volume fraction of the polymer at 150 rpm represented in two different ways.

(27)

(28)

Figure 5.11: The volume fraction of the polymer at 150 rpm with a stopping block represented in two different ways.

(a) No stopping block. (b) Stopping block.

Figure 5.12: The volume fractions using the alternative initialization for both the case with a stopping block and without.

In Figs. 5.8 - 5.12, the scale denotes the volume fraction of the polymer; i.e. blue is all solvent and red is all polymer.

Comparing Figs. 5.8-5.10, the general trend for these three is the same, with a relatively even mixing at the outlet. The areas of higher and lower volume fractions are most likely due to transient effects.

(29)

outlet. Whether this mixing is better is hard to say.

In Fig. 5.12 it is seen quite clearly that almost no mixing has occurred for either case. If this is then related to the corresponding streamlines from Fig. 5.6 and 5.7, the conclusion could be drawn that the polymer has not moved enough to be properly mixed. The difference between this case and the one seen in Fig. 5.4 is that in the latter case the fluid had mixed to some degree already in the steady state-solution.

5.4 Shear flows

The volumes in Figs. 5.13-5.18 are the regions where

∂w ∂xi ≥ 15 [s−1] (5.1)

(a) x component. (b) y component.

Figure 5.13: The x and y components of the shear flow in the z-direction at 150 rpm.

(30)

Figure 5.14: The x and y components of the shear flow in the z-direction at 300 rpm.

(31)

Figure 5.16: The x and y components of the shear flow in the z-direction at 150 rpm with a stopping block.

Figure 5.17: The x and y components of the shear flow in the z-direction at 150 rpm with the alternative initialization.

(32)

Figure 5.18: The x and y components of the shear flow in the z-direction at 150 rpm with the alternative initialization and a stopping block.

Figs. 5.13-5.15 show that the higher shear velocities are at the edges of the mixing blocks. Given that the blocks move at relatively high speeds, and that the no-slip con-ditions on the walls means that the velocity there is zero, this means that the gradients between them will be large. The higher gradients along the edge of the intersection be-tween the two pipes could be attributed to the motion of the flow, which has rotational speed in the open region after the mixers, as can be seen in, for instance, Fig. 5.3.

Case Maximum ∂w_∂x [s−1] Maximum ∂w ∂y [s −1_] 150 rpm 66.38 80.63 300 rpm 144.7 145.7 600 rpm 390.7 521.7 150 rpm with stopper 86.88 68.05 150 rpm alt 76.95 71.60 150 rpm alt stopper 72.05 69.88

Table 5.1: The maximum observed shear flows for the different cases.

In Table 5.1, it can be seen that the highest shear velocities are seen at the highest rotational speeds, which is expected as mentioned earlier.

(33)

(34)

C

HAPTER

6 Discussion

6.1 General

Immersed solids is Ansys CFX are, to the extent of the authors experience, relatively easy to work with but somewhat limited in their implementation. For the purpose of further studies of this problem (mixing of wood-polymer composites) the main disadvantages are the inability to model heat transfer, the incompatibility with particle flows, and the somewhat limited compatibility with multiphase flows. Whether this is implemented in other widespread codes for CFD is not known to the author.

A more thorough investigation of the behaviour of the shear flows with respect to time should be performed.

The reason that the simulations with stoppers had longer simulation times is that, in the case of the case initialized from steady state, the flow had not fully stabilized. The case without a stopper had not entirely stabilized either, but the transient fluctuations were not as great in that case. It is unclear whether the flow in a process of this kind actually stabilizes at any point.

The model with the mixing blocks consistently had more streamlines in the region with the mixing blocks than the model without, which would indicate that the block is working as intended, in keeping the flow in the region with the mixing blocks.

A final conclusion that can be drawn is that more work and more simulation time is required to determine whether this approach is an appropriate way of modelling processes of this kind.

6.2 Future work

Several suggestions are made for future work:

Different ways of initializing the flow, i.e. not starting from a steady state-case but instead directly performing a transient simulation with various different initial

(35)

condition regarding the volume fractions of the two liquids.

Using a more conventional mesh deformation technique and comparing the results. Running the simulations, both the model with stopping blocks and the one without, for a longer total time to further study the flow evolution and find out whether the flow stabilizes at any point.

In reality, since the polymer has a higher melting point than the solvent, the solvent is vaporized in the extruder and the particles are deposited. Finding a way to model this process is one suggestion.

6.3 Conclusion

The mixing of wood-polymer composites has been modelled. The model is based on the concept of immersed solids, which avoids the necessity to generate a new mesh for each time step. Two different models have been tested, one with a stopping block and one without. The conclusions are that the stopping block seems to serve its purpose, that the highest shear velocities occur at the edges of the mixing blocks and that while immersed solids is a promising method for modelling the problem in Ansys CFX, the limitations of the current implementation will limit the ability to further model the problem.

(36)

Bibliography

[1] Ansys 17.0 help, 2016.

[2] Yunus A. C¸ engel and John M. Cimbala. Fluid Mechanics Fundamentals and Appli-cations. McGraw-Hill, 3rd edition edition, 2013.

[3] Ismail B. Celik, Urmila Ghia, Patrick J. Roache, and Christopher J. Freitas. Pro-cedure for Estimation and Reporting of Uncertainty Due to Discretization in CFD Applications.

[4] Andreas Eitzlmayr and Johannes Khinast. Co-rotating twin-screw extruders : De-tailed analysis of conveying elements based on smoothed particle hydrodynamics . Part 1: Hydrodynamics. Chemical Engineering Science, 134:880–886, 2015.

[5] Andreas Eitzlmayr, Gerold Koscher, Gavin Reynolds, Zhenyu Huang, Jonathan Booth, Philip Shering, and Johannes Khinast. Mechanistic modeling of modular co-rotating twin-screw extruders. International Journal of Pharmaceutics, 474(1-2):157–176, 2014.

[6] J.H. Ferziger and Peri´c. Computational Methods for Fluid Dynamics. Springer, 3rd edition edition, 2002.

[7] Mahesh Gupta. NON-ISOTHERMAL SIMULATION OF THE FLOW IN CO-ROTATING AND COUNTER-. pages 316–320, 2008.

[8] J. F. H´etu and F. Ilinca. Immersed boundary finite elements for 3D flow simulations in twin-screw extruders. Computers and Fluids, 87:2–11, 2013.

[9] F. Ilinca and J. F. H´etu. Solution of flow around complex-shaped surfaces by an immersed boundary-body conformal enrichment method. International Journal for Numerical Methods in Fluids, (69):824–841, 2012.

[10] R Mittal and G Iaccarino. Immersed boundary methods. ANNUAL REVIEW OF FLUID MECHANICS, 37:239 – 261, 2005.

(37)

[12] Kristiina Oksman Niska and Mohini Sain. Wood-polymer composites. Woodhead Publishing, 2008.

[13] Charles S Peskin. Flow patterns around heart valves: A numerical method. Journal of Computational Physics, 10(2):252–271, oct 1972.

[14] Stephen B. Pope. The k- model. In Turbulent Flows. Cambridge University Press, 1st edition edition, 2000.