FE analysis of a dog clutch for trucks withall-wheel-drive

(1)

FE analysis of a dog clutch for trucks with

all-wheel-drive

FE-analys av en klokoppling för allhjulsdrivna lastbilar

Växjö, 2010-05-28

15p

Mechanical Engineering/4MT01E

Handledare: Hans Hansson, SwePart Transmission AB

Handledare: Andreas Linderholt, Linnéuniversitetet, Institutionen för teknik

Examinator: Anders Karlsson, Linnéuniversitetet, Institutionen för teknik

Thesis nr: TEK 054/2010

Författare: Mattias Andersson, Kordian Goetz

(2)

Institutionen för teknik

Linnaeus University

School of Engineering

Dokumenttyp/Type of Document Handledare/tutor Examinator/examiner

Examensarbete/Master Thesis Andreas Linderholt Anders Karlsson

Titel och undertitel/Title and subtitle

FE-analys av en klokoppling för allhjulsdrivna lastbilar /

FE analysis of a dog clutch for trucks with all-wheel-drive

Sammanfattning (på svenska)

Examensarbetet är utfört för att försöka förbättra inkopplingen av allhjulsdrift på lastbilar. När en

lastbil kör på halt eller löst väglag kan hjulspinn uppstå vid bakhjulen. Om föraren kopplar in

allhjulsdriften när hjulen börjat slira uppstår en relativ rotationshastighet mellan halvorna i

klokopplingen. Om denna relativa rotationshastighet är för hög kommer halvorna i kopplingen

studsa mot varandra innan de kopplas ihop eller inte koppla ihop alls.

För att undvika detta problem har klokopplingens tandgeometri modifierats. FE simuleringar är

gjorda på den ursprungliga modellen samt alla nya modeller för att ta reda på vilken som kopplar

vid högst relativa rotationshastighet.

Resultaten visar att förbättringar kan göras. Enkla modifieringar på avfasningarnas avstånd och

vinklar visar att klokopplingen kan klara upp till 120 rpm i relativ rotationshastighet jämfört med

den ursprungliga modellen som endast klarar 50 rpm.

Nyckelord

Klokoppling, Allhjulsdrift, FE-analys

Abstract (in English)

The thesis is carried out in order to improve the transfer case in trucks with all-wheel-drive. When

the truck loses traction at the rear wheels, due to slippery surfaces, wheel-spin occurs. If the

driver engages the all-wheel-drive at a point where traction already has been lost, a relative

rotational speed in the dog clutch will occur. If this relative speed is too high the dog clutch

bounces of itself before coupling or it does not couple at all.

To avoid this problem, the geometry of the teeth is modified. FE simulations are done for the

existing model as well as for all the new models in order to find out which of them can handle the

highest relative rotational speed.

The results show that the original model is not the best one. Simple modifications of the teeth’s

chamfer distance and chamfer angle shows that the dog clutch can handle up to 120 rpm of

relative rotational speed whereas the original model only handles 50 rpm.

Key Words

Gleason type curvic coupling, Dog clutch, All-wheel-drive, FE analysis

Utgivningsår/Year of issue Språk/Language Antal sidor/Number of pages

2010 English 70

(3)

The thesis is carried out in order to improve the transfer case in trucks with all-wheel-drive. When

the truck loses traction at the rear wheels, due to slippery surfaces, wheel-spin occurs. If the driver

engages the all-wheel-drive at a point where traction already has been lost, a relative rotational speed

in the dog clutch will occur. If this relative speed is too high the dog clutch bounces of itself before

coupling or it does not couple at all.

To avoid this problem, the geometry of the teeth is modified. FE simulations are done for the

existing model as well as for all the new models in order to find out which of them can handle the

highest relative rotational speed.

The results show that improvements can be done. Simple modifications of the teeth’s chamfer

distance and chamfer angle shows that the dog clutch can handle up to 120 rpm of relative rotational

speed whereas the original model only handles 50 rpm.

(4)

The thesis is performed at Linnæus University and SwePart Transmission AB during the spring

semester 2010.

We would like to thank the following persons:

-

Andreas Linderholt, (Linnæus University, School of Engineering, Växjö) for supervision of

the whole project and many important hints when it comes to the computer software

-

Hans Hansson, (SwePart Transmission AB, Liatorp) for introducing the problem and

providing us with all necessary data

-

Johan Lundgren and Magnus Ragnarsson, (Linnæus University, Mechanical Department,

Växjö) for cooperation and many important observations from the experimental tests

(5)

1. INTRODUCTION ... 1

1.1 B

ACKGROUND

... 1

1.2 P

ROBLEM

D

ESCRIPTION

... 2

1.3 P

URPOSE AND

G

OAL

... 3

1.4 L

IMITATIONS

... 3

2. THEORY ... 4

2.1 T

HE

F

INITE

E

LEMENT

M

ETHOD

... 4

2.2 A

BAQUS

... 7

2.3 I

MPLICIT AND

E

XPLICIT

M

ETHODS

... 8

3. METHOD ... 12

3.1 M

ODELLING IN

S

OLID

W

ORKS

... 12

3.2 S

IMPLIFYING THE

P

ROBLEM

... 12

3.3 D

EFINING THE MODEL

... 14

4. RESULTS ... 18

4.1 E

XISTING

G

EOMETRY

... 18

4.2 M

ODIFIED

T

EETH

... 19

4.3 M

ODIFIED

C

HAMFERS

... 20

4.4 R

ESULTS

S

UMMARY

... 22

5. ANALYSIS ... 24

5.1 A

NALYSIS OF

E

XISTING

G

EOMETRY

... 24

5.2 A

NALYSIS OF

M

ODIFIED

T

EETH

... 25

5.3 A

NALYSIS OF

M

ODIFIED

C

HAMFERS

... 26

6. CONCLUSIONS ... 27

7. REFERENCES ... 28

(6)

1 Mattias Andersson, Kordian Goetz

1. Introduction

1.1 Background

This thesis is carried out on behalf of SwePart Transmission AB in Liatorp. SwePart designs and

manufactures precision grinded gears and customer specific gearboxes as well as other transmission

parts for vehicles and industry. SwePart Transmission AB shall by means of high competence and

cost efficiency remain a leading supplier of transmission products.

The main idea for this thesis is to investigate how improvements can be made to the transfer case in

trucks with all-wheel-drive. The transfer case is located between the gearbox and rear wheel axels as

shown in Figure 1.1. It is responsible for distributing power from the rear wheel drive shaft to the

front wheels, and by doing so it creates all-wheel-drive.

Figure 1.1. Drive train for trucks with all-wheel-drive

Normally a truck is driven by the rear wheels; when this is the case the front wheel driveshaft rotates

freely in the transfer case. When all-wheel-drive is engaged power is delivered through the transfer

case via three gears. The last gear then delivers power to the front wheel driveshaft through a dog

clutch shown in Figure 1.2. This dog clutch will be the focus of this thesis.

Figure 1.2. Dog clutch

(7)

2 Mattias Andersson, Kordian Goetz

1.2 Problem Description

Currently the all-wheel-drive system is engaged manually by the driver. This causes some issues to

appear in certain cases. One of these issues is when the truck loses traction at the rear wheels, due to

slippery surfaces, which creates wheel-spin. In many cases this even leads to the truck getting stuck.

Before this happens the driver can engage the all-wheel-drive allowing the truck to gain traction from

the front wheels. If the driver engages the all-wheel-drive at a point where traction already has been

lost, a relative rotational speed will occur in the dog clutch as shown in Figure 1.3. If this relative

speed is too high the dog clutch will bounce of itself before coupling or not couple at all.

Figure 1.3. Relative rotational speed

Two concepts to deal with this problem have been identified. The first concept involves

development of an automatic system for engaging all-wheel-drive. This solution could eliminate the

issue with the relative rotational speed altogether. The second concept involves re-design of the

geometry of the dog clutch to allow coupling at a higher relative speed.

The first concept would provide more advantages; nevertheless it is not going to be considered due

to the time limitations for the project as well as the demand from the industry side that the project

cannot result in an increased manufacturing cost.

(8)

3 Mattias Andersson, Kordian Goetz

1.3 Purpose and Goal

The purpose of this thesis is to understand the importance of the geometric shape of the teeth in a

dog clutch and to determine whether the design can be improved. Also an increased understanding

for FE modelling and the Abaqus software should be obtained. The thesis should after completion

provide a decent guideline for further research in similar problems.

The main goal of the project is to handle FE simulations of a dog clutch which is part of the transfer

case in all-wheel-drive trucks. The first part of the investigation is to create a 3D model of the

existing dog clutch and make FE simulations in order to determine at which maximal relative

rotational speed it couples. In further steps different shapes of the teeth will be considered which in

the end will allow a comparison of all results and selection of the best one. If any of the new designs

show an increase in performance, the next step (not necessarily part of this project) will be to

manufacture and provide tests in real conditions.

1.4 Limitations

One of the main limitations for this thesis is the use of theoretical models. To confirm the results

from this thesis, physical experiments should be made to correlate the results from the FE

simulations with actual results. This was not done in this thesis due to time and equipment

limitations.

Another limitation is the available computing power at the university. The computers used for

simulations are Intel® Core™2Duo CPU E8600 @ 3.33GHz with 3.25GB of RAM. This has led to

simulations taking up to 36 hours and thus limiting the pace of the entire thesis. Also a maximum of

five Abaqus licenses are available. As a result of these limitations simplifications were made in order

to obtain reliable results.

(9)

4 Mattias Andersson, Kordian Goetz

2. Theory

2.1 The Finite Element Method

Engineering problems rendering in differential equations are very often too complicated to be solved

analytically. The finite element (FE) method is a numerical approach by which these general

differential equations can be solved in an approximate manner (Figure 2.1).

Figure 2.1. Steps in engineering mechanical analysis

The differential equations, which describe the physical problem, are assumed to hold over a certain

region. These regions can be one-, two- or three-dimensional. It is a characteristic feature of the finite

element method that the region is divided into smaller parts, so called finite elements which allow

carrying out the approximation over each element (Figure 2.2).

Figure 2.2. Illustration of modelling steps

When the type of approximation for each element has been selected, the corresponding behaviour

can be determined. Having determined the behaviour of all elements, it is relatively simple to patch

them together in order to obtain an approximate solution for the behaviour of the entire body.

The FE method can be applied to various physical phenomena due to the fact that the main principle

is based on general differential equations. Thus the FE formulation is suitable for diverse problems

such as heat conduction, torsion of elastic shafts, diffusion, groundwater flow and the elastic

behaviour of one-, two- and three-dimensional bodies, including beam and plate analysis.

The approximation of the FE method is usually polynomial. It is in fact a kind of interpolation over

the element, where it is assumed that the variable is known at certain points in the element. These

points are called nodal points and usually they are located at the boundary of the element (Figure

2.3).

(10)

5 Mattias Andersson, Kordian Goetz

Figure 2.3. a) Four elements with linear T-value variation within each element

b) Resulting approximate T-value distribution along the element (linear approximation)

It is important to notice, that the approximate T-value distribution along the entire element is known

once the particular T-values at nodal points are known. In this way the original problem with

infinitely many unknowns (i.e. degrees of freedom) can be replaced by a problem with a finite

number of unknowns (5, for the case presented in Figure 2.3). Following this way of thinking it is

obvious, that the more unknowns, the more accurate the approximate solution. The system with a

finite number of unknowns is called a discrete system, while the continuous system corresponds to

the system with an infinite number of unknowns.

Having defined the model it is important to divide it into a finite number of elements, this is called to

mesh. There are several types of elements which are basically characterised by their shape (hexagonal,

tetragonal, wedge-based etc.). Basically a good mesh is one which consists of as high number of

elements as possible, none of them should have negative volume, and none of them should be

excessively distorted during the analysis. Figure 2.4 shows the FE mesh and the deflections of an

ordinary structural component due to lateral loading.

(11)

6 Mattias Andersson, Kordian Goetz

A good example of the mesh application can be a steel beam supported by rubber components, as

shown in Figure 2.5 a). In order to investigate its dynamic response in detail, the deformation modes

at some resonance frequencies of the rubber component itself were determined (Figure 2.5 b)).

Figure 2.5. a) Steel beam supported by rubber components

b) Deformation modes of rubber component at some resonance frequencies

All the problems listed above show that widely different physical phenomena can be analyzed by the

FE method. It is also important to mention that nowadays none of the calculations are done

manually and that is why complicated problems require sufficient calculation capabilities of the

computer equipment.

(12)

7 Mattias Andersson, Kordian Goetz

2.2 Abaqus

Abaqus is a set of powerful simulation programs, shown in Figure 2.6, used in engineering problems.

They are based on the finite element method and can solve problems ranging from simple linear

analyses to challenging nonlinear simulations. Abaqus is designed as a general-purpose simulation

tool and can be used to study more than just structural (stress/displacement) problems. Other areas

include heat transfer, mass diffusion, acoustics, and soil mechanics.

Figure 2.6. Abaqus products

Abaqus mainly consists of two analysis products. The first is Abaqus/Standard which is a

general-purpose analysis product that can solve linear and nonlinear problems involving the static, dynamic,

thermal, and electrical response of components. The second is Abaqus/Explicit which is a

special-purpose analysis product and uses an explicit dynamic finite element formulation. It is suitable for

modelling brief dynamic events such as impact and blast problems.

The difference between the two is that Abaqus/Explicit marches a solution forward through time in

small time increments without solving a coupled system of equations, or even forming a global

stiffness matrix at each increment. In contrast Abaqus/Standard solves a system of equations at each

solution increment using an implicit method. Explicit and implicit methods are discussed in the next

section.

Abaqus/CAE (Complete Abaqus Environment) is an interactive graphical environment that includes

capabilities for creating or importing models of the structure to be analysed and decomposing the

geometry into meshable regions. It contains eight modules that are used to define a model for the

analysis. In these modules physical and material properties are assigned to the geometry together with

loads and boundary conditions. The modelling process will be described further in section 3.3.

(Dassault Systèmes, 2008)

(13)

8 Mattias Andersson, Kordian Goetz

2.3 Implicit and Explicit Methods

In any finite element simulation the first step is to create a discretized model of the geometry which is

to be analysed, this is done by using a collection of finite elements. Each finite element is connected to

another by shared nodes and the collection of nodes and finite elements is called the mesh. It is the

displacements of these nodes which are the fundamental variables that Abaqus calculates in a stress

analysis. When these displacements are known, the stresses and strains in each finite element can be

calculated easily.

As mentioned earlier an implicit method, such as that used in Abaqus/Standard, requires that a

system of equations is solved at the end of each solution increment. The following example is an

attempt to create a conceptual understanding of how stresses are calculated in a bar using an implicit

method.

Figure 2.7. Cantilever Bar

The bar shown in Figure 2.7 is fixed at one end and loaded at the other. In this case it will be

modelled with two elements and the discrete model is shown in Figure 2.8.

Figure 2.8. Discretized model of the cantilever bar

For a model to be in static equilibrium, the sum of all forces in each node must equal zero, i.e. all

internal and external loads at each node must balance each other. The external load, P, and the

internal loads, I, will cause stresses in each node as shown in the free-body diagrams of each node in

figure 2.9.

(14)

9 Mattias Andersson, Kordian Goetz

Figure 2.9. Free-body diagrams

The strain in element 1 is given by

𝜀

₁₁

=

𝑢

𝑏

− 𝑢

𝑎

𝐿

where 𝑢

𝑎

and 𝑢

𝑏

are the displacements at nodes a and b, and 𝐿 is the original length. The stress is, for

a linear elastic problem obtained by

𝜎

₁₁

= 𝐸𝜀

₁₁

where E is the Young’s modulus. The stress, 𝜎

11

, is equal to the axial force, P, divided by the

cross-sectional area, A. From these expressions a relationship between displacements, internal force and

material properties is obtained:

𝐼

_𝑎1

_{= 𝜎}

11

𝐴 = 𝐸𝜀

11

𝐴 =

𝐸𝐴

𝐿

(𝑢

𝑏

− 𝑢

𝑎

)

Therefore equilibrium at node a can be written as

𝑃

_𝑎

+

𝐸𝐴

𝐿

𝑢

𝑏

− 𝑢

𝑎

= 0

For node b the internal forces in element 1 and 2 must be considered in the equilibrium equation.

This results in the following expression:

𝑃

_𝑏

−

𝐸𝐴

𝐿

𝑢

𝑏

− 𝑢

𝑎

+

𝐸𝐴

𝐿

𝑢

𝑐

− 𝑢

𝑏

= 0

The equilibrium equation for node c is

𝑃

_𝑐

−

𝐸𝐴

𝐿

𝑢

𝑐

− 𝑢

𝑏

= 0

To obtain displacements of all nodes, implicit methods require the equilibrium equations to be solved

simultaneously. This is best achieved by using matrix techniques and the equilibrium equations can

be written in matrix form as follows:

(15)

10 Mattias Andersson, Kordian Goetz

𝑃

_𝑎

𝑃

𝑏

𝑃

𝑐

−

𝐸𝐴

𝐿

1 −1

0 −1

2 −1

0 −1

1 𝑢

𝑎

𝑢

𝑏

𝑢

𝑐

= 0

or

𝐏 − 𝐊𝐮 = 𝟎

In this case the Young’s modulus, cross-sectional area, and length of the elements are assumed to be

identical. In other cases the term EA/L, known as the element stiffness, could be different for

different elements.

This example, however, describes a static problem. The corresponding dynamic problem requires the

addition of a mass matrix, 𝐌, and an acceleration matrix, 𝐮 . This results in the following system of

dynamic equilibrium equations:

𝐌𝐮 + 𝐊𝐮 = 𝐏(t)

By using an implicit method this system of equations can be solved to obtain the unknown variables.

Once they are known they can be used to calculate the stresses in the bar. Implicit finite element

methods require that these systems of equations be solved at the end of each solution increment.

An explicit method on the other hand does not require the solving of a simultaneous system of

equations or even the calculation of a global stiffness matrix. In an explicit method, such as that in

Abaqus/Explicit, the solution is advanced kinematically from one increment to another. This is

illustrated in the following example of how forces spread through a bar.

The bar shown in Figure 2.10 is fixed in one end and loaded at the other and the model is divided

into three elements.

Figure 2.10. Cantilever bar divided into elements

In the first time increment the force, P, will cause node 1 to have an acceleration, 𝑢

1

. Consequently

the acceleration causes node 1 to have a velocity, 𝑢

1

𝑢

1

=

𝑃

𝑀

1

⇒ 𝑢

1

= 𝑢

1

𝑑𝑡

(16)

11 Mattias Andersson, Kordian Goetz

This causes a strain rate in element 1

𝜀

_𝑒𝑙1

=

−𝑢

1

𝑙

By integrating the strain rate through the time of increment 1 the increment of strain is obtained

∆𝜀

𝑒𝑙1

= 𝜀

𝑒𝑙1

𝑑𝑡

The total strain, 𝜀

𝑒𝑙1

, is the sum of the initial strain, 𝜀

0

, and the increment of strain. When the total

strain in the element is known the element stress is obtained by

𝜎

𝑒𝑙1

= 𝐸𝜀

𝑒𝑙1

The stresses in element 1 apply internal forces to the connecting nodes as shown in Figure 2.11.

Figure 2.11. Internal forces in the bar

These element stresses are used in the second increment to calculate dynamic equilibrium at nodes 1

and 2.

𝑢

₁

=

𝑃 − 𝐼

𝑒𝑙1

𝑀

₁

⇒ 𝑢

1

= 𝑢

1𝑜𝑙𝑑

+ 𝑢

1

𝑑𝑡

𝑢

₂

=

𝑃

𝑀

₂

⇒ 𝑢

2

= 𝑢

2

𝑑𝑡

𝜀

𝑒𝑙1

=

𝑢

₂

− 𝑢

₁

𝑙

⇒ ∆𝜀

𝑒𝑙1

= 𝜀

𝑒𝑙1

𝑑𝑡

⇒ 𝜀

𝑒𝑙1

= 𝜀

𝑒𝑙1𝑜𝑙𝑑

+ ∆𝜀

𝑒𝑙1

⇒ 𝜎

𝑒𝑙1

= 𝐸𝜀

𝑒𝑙1

In the next increment there are stresses in both element 1 and 2 and the process continues until the

analysis reaches the specified time.

To sum up; an explicit method calculates each increment faster but needs smaller increments than an

implicit method. For the contact-type analysis in this thesis, very small increments are needed and

therefore an explicit method is used.

(17)

12 Mattias Andersson, Kordian Goetz

3. Method

3.1 Modelling in SolidWorks

The first step of the work is to model the geometry of the dog clutch. As the main tool SolidWorks

2009 Student Edition has been used.

SolidWorks is a 3D mechanical Computer Aided Design program which has been developed by

Dassault Systèmes Corporation. SolidWorks consists of three basic modes: part, assembly and

drawing. The first one, part, allows to create a part from the beginning. One begins with a simple 2D

sketch and then, by using some 3D functions, a complete model can be created. The assembly

module allows creating positional relations between the. The drawing module can be used in order to

create a 2D drawing which can be based either on a part model or on an assembly model.

The dog clutch, which is the main object of this thesis, consists of two separate parts which have

been created in the part module. Following technical drawings provided by SwePart Transmission

AB, the 2D cross-sectional sketch is created on one of the planes. Then, by using the revolve

function a 3D model is rolled out. The complete model is founded by using functions like: fillet,

chamfer, extrude, circular pattern and cut-revolve.

3.2 Simplifying the Problem

Most of the engineering problems taken from real working conditions require simplifications. These

simplifications are made to ensure that calculations can be performed in an acceptable way and still

obtain reliable results. They concern each point of the problem definition i.e. model geometry,

material properties, loads, boundary conditions, mesh creation, and solver settings.

The simplifications made in this thesis starts within the modelling of the original geometry of the dog

clutch in SolidWorks. Unnecessary geometry such as fillets, radiuses, and other details are removed to

allow a coarser mesh to be used and thus reduce simulation time significantly in Abaqus. A

comparison of original and simplified geometry is shown in Figure 3.1.

(18)

13 Mattias Andersson, Kordian Goetz

.

Figure 3.1. Original Geometry

Figure 3.2. Simplified Geometry

Translation of the files from SolidWorks to Abaqus does not require any simplifications i.e. exactly

the same models can be managed in both programs. The input file in Abaqus requires several

parameters to be specified which influence the solution. One of them is material properties. The

material has been assumed to be steel with general properties:

E=210 GPa

υ=0.3

ρ=7500 kg/m

3

where E – modulus of elasticity, υ – Poisson’s ratio and ρ – density. In fact, both parts of the dog

clutch are made of steel V-2250-96 which is characterized by properties which have been fulfilled by

presented assumptions; nevertheless it is not possible to achieve 100% accuracy in this field.

(19)

14 Mattias Andersson, Kordian Goetz

In order to divide the model into a finite amount of elements, the mesh needs to be created.

Infinitesimal elements demand substantial capabilities of the computers used and for that reason are

not possible to use in practise create. Here, the element size is decided not to be larger than 6 mm.

This assures a relatively fine and continuous mesh without any elements with negative volume.

The two halves of the dog clutch are mounted on the front wheel drive shaft and a gear in the

transfer case, respectively. This means that one halve rotates with the front wheels while the other

rotates with the rear wheels. Since the problem addresses relative speed between the two halves, the

halve corresponding to the rear wheels is set to rotate while the other halve is fixed in rotational

degrees of freedom as well as axial. The decision to fix one halve is a result of the axial force being

small enough to assume that it will cause the moving halve to bounce back rather than move the

fixed halve.

As for rotation, if the truck is standing still with wheel-spin and maximum traction at the front

wheels, the inertial mass of the front wheel driveline is assumed to be great enough to consider the

corresponding halve of the dog clutch to be fixed. I.e. if the clutch does not couple fully it will

bounce without delivering any power to the front wheels.

3.3 Defining the model

As mentioned earlier, Abaqus/CAE consists of several modules which each contain special functions

to define a model that describes the physical problem to be analyzed. An Abaqus model consists, at a

minimum, of: discretized geometry, element section properties, material data, loads and boundary

conditions, analysis type, and output requests. This section aims to describe the modules and

functions used to create the Abaqus models for this thesis.

In this case the modelling process in Abaqus begins with the two parts already created and imported

from Solid Works. In the module, named Part, further editing of the geometry can be made. The first

step is to achieve an acceptable geometry by removing redundant edges created in the translation

process. This is done by using the “Remove redundant entities” function. When an acceptable

geometry is obtained, material properties are created in the Property module. The material behaviours

used are density and elasticity. After a material is defined it must be assigned to an element section.

Since the material is steel, a solid, homogeneous section is created and assigned to the two parts.

At this point the two parts are not in the same viewport, an assembly has to be created. Using the

Assembly module dependant instances are created of the two parts i.e. if changes are made to the

parts, the instances will change as well. Next, position constraints are made to position the parts

correctly for the analysis and reference points are created as control points for the parts. The

assembly is shown in Figure 3.4.

(20)

15 Mattias Andersson, Kordian Goetz

Figure 3.4. Assembly of the dog clutch

The problem to be solved is a dynamic impact problem and therefore a time period must be set for

the analysis. This is done by creating a “dynamic, explicit” step in the Step module telling Abaqus that

the analysis is dynamic and that the explicit solver is to be used.

Once the step is created all interactions must be defined in the Interaction module. Since this is an

impact problem all surfaces that will experience contact must be specified. Firstly a contact-type

interaction property is created and in the contact property options a tangential behaviour is added.

The friction formulation is specified as “Penalty” and a friction coefficient is specified. Secondly the

interactions are defined by creating “Surface-to-surface contact“-type interactions and selecting the

first and second surface which will experience contact. Finally when this is done for each surface the

“Penalty contact method” is selected as the “Mechanical constraint formulation” and the interaction

property created earlier is selected as the “Contact interaction property”.

In the analysis one of the parts will have a constant axial velocity and rotational speed. To achieve

this by applying a force and moment a damper is used. The damper is created using the “Connector

builder” in the Interaction module. One of the ends is connected to the “ground” while the other is

connected to one of the control points created in the assembly. To be able to control both axial and

rotational speed the “Cylindrical” connection type, shown in Figure 3.5, was used. In the behaviour

options for the “Connector section”, damping is added and both force and moment are selected to

be able to specify the damping coefficients. The coefficients are calculated by

𝑐

₁₁

=

𝐹

𝑥

𝑐

₄₄

=

𝑀

𝜃

where 𝐹 is the force acting on the part, 𝑥 is the parts axial velocity, 𝑀 is the moment, and 𝜃 the

rotational speed.

(21)

16 Mattias Andersson, Kordian Goetz

Figure 3.5. Cylindrical connector

As mentioned previously, control points where created to control the parts in an easier way. These

control points are connected to the parts using “Constraints”. Three control points where created

and each of them are connected to the corresponding part using “Coupling”-type constraints. The

coupling is made between the point and the surface it shall control to simulate it being mounted on a

shaft, as shown in Figure 3.6.

Figure 3.6. Coupling constraint

The next step is to apply loads and boundary conditions to the model in the Load module. The loads

used are “concentrated force” and “moment”. These loads are applied at the control point associated

with the part that will move. After this is done the boundary conditions are applied to the two parts

in their respective control points. The boundary conditions used only allow one of the parts to rotate

around the global x-axis, shown in Figure 3.6, as if it is connected to a driving shaft.

(22)

17 Mattias Andersson, Kordian Goetz

The model is nearly complete and all that is left is to create a mesh of the geometry. The mesh is

created on each part individually in the Mesh module. The first step is to select the “element shape”

and mesh “technique”. In the mesh controls the tetrahedral element shape is selected as well as the

“Free” mesh technique. The second step is to specify the element size by placing “Seeds” on the

parts edges. This is done by specifying an approximate global element size. Finally the part is ready to

be meshed by selecting the command mesh part. The seeded and meshed parts are shown in figures

3.7 and 3.8.

.

Figure 3.7. Seeded part

Figure 3.8. Meshed part

The model is now ready to be analyzed. Since dual core processors where used in this thesis, a job

file was created in the Job module with the “Use multiple processors” option enabled. To summarize

it should be mentioned that this is the method of modelling chosen for this thesis and not necessarily

the best solution.

(23)

18 Mattias Andersson, Kordian Goetz

4. Results

In this chapter all of the analyzed geometries are presented as well as their corresponding results. The

first step of the FE analysis was to determine at which maximal relative rotational speed,

𝜃

𝑚𝑎𝑥

, the

existing solution would couple. After analyzing the behaviour of the original model several other

solutions where created in an attempt increase at which

𝜃

𝑚𝑎𝑥

the coupling would couple. A summary

of all results is presented in the last section.

4.1 Existing Geometry

After simulations in Abaqus/Explicit the maximal relative rotational speed for the original model,

shown in Figure 4.1, was determined to be between 50rpm and 60rpm. As the rotational speed

increases the point of impact moves towards the chamfers, this causes the parts to bounce of each

other and de-couple.

In an attempt to improve the performance of the original model simulations using double the axial

force (248N) where done. This resulted in a

𝜃

𝑚𝑎𝑥

of 70rpm.

(24)

19 Mattias Andersson, Kordian Goetz

4.2 Modified Teeth

In parallel with this thesis another project was carried in order to improve the geometry of the dog

clutch using physical testing (Lundgren et al, 2010). From this project three other solutions where

supplied and analyzed in Abaqus. Two of the models have modified tooth angles by 9° and 4,5°,

respectively, and the third model has a 9° tooth angle and a total amount of 12 teeth compared to the

original model where 14 teeth are used. The models are shown in Figure 4.2.

Figure 4.2. Models with angled teeth a) 9°, 14 teeth b) 4.5°, 14 teeth c) 9°, 12 teeth

After analyzing the behaviour of these models it is determined that angled teeth create a tendency to

de-couple. The only advantage from this modification is the increased gap between the teeth. All

these results will be discussed in detail in chapter 5. Technical drawings of all considered models are

presented in Appendices 1B, 1C, 1D.

(25)

20 Mattias Andersson, Kordian Goetz

4.3 Modified Chamfers

The second modification which has been implemented concerns chamfers. In order to check the

influence of chamfer geometry, two different parameters are adjusted: chamfer distances and chamfer

angles. The original model has chamfers which have the distance 1.5 mm and angle 45°. Modified

chamfers have distances 1 mm, 2 mm and 3 mm. Modified chamfer angles have values: 15°, 30° and

60°. The following models are compared:



C15_A30 – chamfer distance 1.5 mm, chamfer angle 30°



C15_A60 – chamfer distance 1.5 mm, chamfer angle 60°



C1_A45 – chamfer distance 1 mm, chamfer angle 45°



C2_A45 – chamfer distance 2 mm, chamfer angle 45°



C3_A15 – chamfer distance 3 mm, chamfer angle 15°



C3_A30 – chamfer distance 3 mm, chamfer angle 30°

Pictures of modified chamfers have been presented in Figures 4.3 and 4.4. Technical drawings of all

considered models are presented in Appendices 1E, 1F, 1G, 1H, 1I, 1J.

Figure 4.3. Models with modified chamfers

(26)

21 Mattias Andersson, Kordian Goetz

Figure 4.4. Models with modified chamfers

(27)

22 Mattias Andersson, Kordian Goetz

4.4 Results Summary

Altogether, in the entire calculation process 11 different models are calculated. Two of them are

based on the original geometry (A and A_Fx2), models B, C, D represent angled teeth and the rest of

them concern chamfer modifications. All detailed results have been presented in Table 4.1. The last

column shows the corresponding appendix number for each model.

A (REF) – original model (chamfer distance 1.5 mm, chamfer angle 45°, 14 teeth)

B – tooth angle 9°, no chamfer, 12 teeth

C – tooth angle 9°, no chamfer, 14 teeth

D – tooth angle 4.5°, no chamfer, 14 teeth

C1.5_A30 – chamfer distance 1.5 mm, chamfer angle 30°, 14 teeth

C1.5_A60 – chamfer distance 1.5 mm, chamfer angle 60°, 14 teeth

C1_A45 – chamfer distance 1 mm, chamfer angle 45°, 14 teeth

C2_A45 – chamfer distance 2 mm, chamfer angle 45°, 14 teeth

C3_A15 – chamfer distance 3 mm, chamfer angle 15°, 14 teeth

C3_A30 – chamfer distance 3 mm, chamfer angle 30°, 14 teeth

A_Fx2 – original model, the same geometry as A (REF), double axial force

Model name

Number

of teeth

Tooth

angle

[

°]

Chamfer

distance

[mm]

Chamfer

Angle

[

°]

𝜽

𝒎𝒂𝒙

[rpm]

Force

_[N]

Appendix

A (REF)

14

0 1,5

45

50

124 1A

B

12

9

0

0 -

124 1B

C

14

9

0

0 -

124 1C

D

14 4,5

0

0 -

124 1D

C1.5_A30

14

0 1,5

30

60

124 1E

C1.5_A60

14

0 1,5

60 <50

124 1F

C1_A45

14

0

1

45 <50

124 1G

C2_A45

14

0

2

45 <50

124 1H

C3_A15

14

0

3

15

120

124 1I

C3_A30

14

0

3

30

70

124 1J

A_Fx2

14

0 1,5

45

70

248 1A

Table 4.1. FE calculations results

The main output value from the described FE calculations is maximal relative rotational speed

𝜃

𝑚𝑎𝑥

which can be handled by the models. The original model, A (REF), can handle 50 rpm of relative

rotational speed e.g. one halve rotates with 50 rpm and the other with 100 rpm during the coupling

stage. Both Table 4.1 and Diagram 4.1 show the differences in

𝜃

𝑚𝑎𝑥

between all considered models.

(28)

23 Mattias Andersson, Kordian Goetz

Diagram 4.1. Maximal relative rotational speed which can be handled by the models

<50

0

10

20

30

40

50

60

70

80

90

100

110

120

130 [𝜽

𝒎𝒂𝒙

]

(29)

24 Mattias Andersson, Kordian Goetz

5. Analysis

5.1 Analysis of Existing Geometry

When studying the behaviour of the original model it is clear that, for the dog clutch to couple at

greater relative rotational speed, one of the following parameters should be modified:



Chamfer angles



Chamfer distances



Axial force

Whether the dog clutch couples or not depends on one thing – The chamfer edge (black line),

illustrated in Figure 5.1, must pass beyond the chamfer edge on the opposite halve (red line) before

the tooth edges cross each other (green lines).

Figure 5.1. Conditions for coupling

From a theoretical point of view, this means that the optimal solution would be a dog clutch with

straight teeth and without any chamfers. This type of geometry would be able to couple at virtually

any relative rotational speed. In reality, on the other hand, this might not work due to high stress

concentrations at the sharp edges. High enough stresses will cause failures in the teeth.

As mentioned in the previous chapter, the original model reached a 𝜃

𝑚𝑎𝑥

of 50-60rpm. This is a

result of the combination of aforementioned parameters. To investigate the effect of the parameters

a number of simulations where done regarding each parameter and several combinations.

𝜃

(30)

25 Mattias Andersson, Kordian Goetz

5.2 Analysis of Modified Teeth

Results have shown that angled teeth cause a tendency for the dog clutch to de-couple. The reason

for this is that, at impact a reaction force will occur between the teeth of the two halves. Because of

the angles, the reaction force will be directed in a negative direction, as shown in Figure 5.2. If the

x-component of the reaction force is greater than the sum of the axial force and x-x-component of the

friction force the clutch will de-couple.

Figure 5.2. Coupling requirement

The following expression describes the coupling requirement:

𝑅

_𝑥

<

𝐹

𝑛

+ 𝑇

𝑥

where 𝑅

𝑥

is the x-component of the reaction force, 𝐹 is the axial force pushing the two halves of the

clutch together, 𝑇

𝑥

the x-component of the friction force, and n the number of teeth. The only way

this type of geometry would work in reality is if the mass inertia of the front wheel driveline is low

enough i.e. the reaction force is low enough to fulfil the coupling requirement.

Another parameter that was tested in these models was the number of teeth, or gap width. It is clear

that the width of the gap between two teeth has significant effect regarding coupling i.e. a wider gap

lets the moving halve travel further in the x-direction before impact in the y-direction. Nevertheless

problems might occur when implementing this type of modification. The main concern is higher

impact stresses created when the clutch is coupled. The gap allows the clutch to move while coupled

e.g. when going from first gear to reverse. These impacts will also cause greater shocks in the

driveline which can lead to other transmission parts to take damage.

F

M

R

𝐑

𝒙

𝑹

_𝒚

𝑻

_𝒙

𝑻

𝒚

y

x

(31)

26 Mattias Andersson, Kordian Goetz

5.3 Analysis of Modified Chamfers

The last group of simulated models concern chamfer modifications. In order to check the influence

of the chamfer geometry, six different models have been considered.

The first pair consists of models C1.5_A30 and C1.5_A60 which have chamfer distances 1.5 mm,

which is exactly the same as the original model. The chamfer angles, however, have been modified to

30° and 60° respectively. These modifications did not result in significant improvements because

C1.5_A30 coupled with 𝜃 =60 rpm, whereas C1.5_A60 did not even couple at 𝜃 =50 rpm. During

the simulations one characteristic feature has been noticed: the smaller the chamfer angle, the easier

the coupling. It confirms the aforementioned conclusion that from a theoretical point of view the

best solution is teeth without any chamfer (angle 0°).

Models from the second pair (C1_A45 and C2_A45) have chamfer distances 1 mm and 2 mm

respectively, the chamfer angles have not been modified with respect to the original model and have

a value of 45°. None of these models coupled at 𝜃 =50 rpm which makes them significantly inferior

than the original model. The obvious conclusion out of this result is that modest changes of chamfer

distance without modifying other factors do not help to increase the relative rotational speed which

the dog clutch can handle.

The last pair consists of two models with modified chamfer distances and chamfer angles. Models

C3_A15 and C3_A30 have a chamfer distance of 3 mm and chamfer angles 15° and 30°, respectively.

After the tests it has shown up that both of these models are significantly better than the original

model. C3_A30 has coupled at 𝜃 =70 rpm, and C3_A15 even with 𝜃 =120 rpm. These results confirm

the conclusion, that the smaller the chamfer angle, the higher the relative rotational speed which the

clutch can handle. Furthermore, the longer chamfer distance affects the coupling conditions in a

positive way.

(32)

27 Mattias Andersson, Kordian Goetz

6. Conclusions

The complete FE simulations of the dog clutch, which are the core of this thesis, consist of three

different parts:



Analysis of existing geometry



Analysis of modified teeth



Analysis of modified chamfers

As mentioned before, there are four main factors which influence the coupling ability:



Teeth angles



Number of teeth



Chamfer angles



Chamfer distances



Axial force

Altogether, 11 different simulations have been done. After analysing the results the following

conclusions can be made:

1. The angled teeth influence the coupling ability in a negative way. They cause an additional

axial force which tends to de-couple the dog clutch (the direction of this additional axial

force is opposite to the axial force which is used to couple/de-couple the clutch).

2. The decreased amount of teeth creates a greater gap between them. Obviously it helps to

couple both halves but on the other hand it is dangerous from the material point of view. A

greater gap will cause significant impact loads which can decrease the life length of the whole

clutch.

3. Chamfers are the most important when it comes to the coupling ability. In order to obtain a

clutch which will handle maximal relative rotational speed both chamfer angles and chamfer

distances should be modified. The general trend is that the coupling abilities are better when

the chamfer angle is as small as possible and the chamfer distance as long as possible. The

original model has teeth with chamfers 1.5 x 45° and reached a 𝜃

𝑚𝑎𝑥

of 50 rpm while the

best tested model has teeth with chamfers 3 x 15° and reached a 𝜃

𝑚𝑎𝑥

of 120 rpm with the

same axial force.

4. When increasing the axial force, the relative rotational speed handled by the clutch increases

as well.

(33)

28 Mattias Andersson, Kordian Goetz

7. References

Ottosen, N.S. and Petersson, H. (1992) Introduction to the Finite Element Method. Pearson

Education Limited, Harlow, Essex

Dassault Systèmes. (2008) Abaqus Documentation; Getting Started With Abaqus version 6.8.

Dassault Systèmes Simulia Corp, Providence, RI

Juvinall, R.C. and Marshek, K.M. (2006) Fundamentals of Machine Component Design. John Wiley

& Sons, Asia

Lundgren, J. and Ragnarsson, M. (2010) Modification of claw coupling. School of Engineering,

Linnæus University, Växjö

(34)

29 Mattias Andersson, Kordian Goetz

8. Appendices

Appendix 1 (A-K): Drawings

Appendix 2: Abaqus Input File

(35)

1(11)

Appendix 1 - Technical Drawings

Appendix 1A - A (REF)

Appendix 1B - B

Appendix 1C - C

Appendix 1D - D

Appendix 1E - C1.5_A30

Appendix 1F - C1.5_A60

Appendix 1G - C1_A45

Appendix 1H - C2_A45

Appendix 1I - C3_A15

Appendix 1J - C3_A30

(36)

TITLE: DWG NO. SCALE:1:2 SHEET 1 OF 1

A4

C WEIGHT:

A (REF)

Appendix 1A

B C D 1 2 A B REVISION DO NOT SCALE DRAWING

MATERIAL: DATE SIGNATURE A LINEAR: DRAWN M.A, K.G CHK'D APPV'D MFG Q.A ANGULAR: FINISH: TOLERANCES: EDGES NAME UNLESS OTHERWISE SPECIFIED: DIMENSIONS ARE IN MILLIMETERS SURFACE FINISH: DEBUR AND BREAK SHARP

Linnéuniversitetet i Växjö (TEK)

A

A-A

28 CHAMFERS 1.5 X 45°

90 °

(37)

99 °

A4

C WEIGHT:

B

Appendix 1B

B C D 1 2 A B A DRAWN M.A, K.G SHEET 1 OF 1 SCALE:1:2 DWG NO. TITLE: REVISION CHK'D APPV'D LINEAR: MFG Q.A ANGULAR: FINISH: TOLERANCES: EDGES

NAME SIGNATURE DATE

MATERIAL:

DO NOT SCALE DRAWING UNLESS OTHERWISE SPECIFIED:

DIMENSIONS ARE IN MILLIMETERS SURFACE FINISH: DEBUR AND BREAK SHARP

Linnéuniversitetet i Växjö (TEK)

A

A-A

(38)

99 °

A4

C WEIGHT:

C

Appendix 1C

B C D 1 2 A B A DRAWN M.A, K.G SHEET 1 OF 1 SCALE:1:2 DWG NO. TITLE: REVISION CHK'D APPV'D LINEAR: MFG Q.A ANGULAR: FINISH: TOLERANCES: EDGES

NAME SIGNATURE DATE

MATERIAL:

DO NOT SCALE DRAWING UNLESS OTHERWISE SPECIFIED:

Linnéuniversitetet i Växjö (TEK)

A

A-A

(39)

94°

WEIGHT:

D

Appendix 1D

B C D 1 2 A B A DRAWN M.A, K.G CHK'D APPV'D C

A4

SHEET 1 OF 1 SCALE:1:2 DWG NO. MFG Q.A LINEAR: ANGULAR: FINISH: TOLERANCES: EDGES

NAME SIGNATURE DATE

MATERIAL:

DO NOT SCALE DRAWING REVISION

TITLE: UNLESS OTHERWISE SPECIFIED:

Linnéuniversitetet i Växjö (TEK)

A

A-A

(40)

WEIGHT:

C1.5_A30

Appendix 1E

A4

NAME SIGNATURE DATE

MATERIAL:

Linnéuniversitetet i Växjö (TEK)

A

A-A

28 CHAMFERS 1,5 X 30°

90 °

(41)

WEIGHT:

C1.5_A60

Appendix 1F

A4

NAME SIGNATURE DATE

MATERIAL:

Linnéuniversitetet i Växjö (TEK)

A

A-A

28 CHAMFERS 1,5 X 60°

90 °

(42)

WEIGHT:

C1_A45

Appendix 1G

A4

NAME SIGNATURE DATE

MATERIAL:

Linnéuniversitetet i Växjö (TEK)

A

A-A

28 CHAMFERS 1 X 45°

90 °

(43)

WEIGHT:

C2_A45

Appendix 1H

A4

NAME SIGNATURE DATE

MATERIAL:

Linnéuniversitetet i Växjö (TEK)

A

A-A

28 CHAMFERS 2 X 45°

90 °

(44)

WEIGHT:

C3_A15

Appendix 1I

A4

NAME SIGNATURE DATE

MATERIAL:

Linnéuniversitetet i Växjö (TEK)

A

A-A

28 CHAMFERS 3 X 15°

90 °

(45)

SHEET 1 OF 1

C3_A30

Appendix 1J

A4

TITLE: SCALE:1:2 DWG NO. MFG Q.A LINEAR: ANGULAR: FINISH: TOLERANCES: EDGES

NAME SIGNATURE DATE

MATERIAL:

WEIGHT: UNLESS OTHERWISE SPECIFIED:

Linnéuniversitetet i Växjö (TEK)

A

A-A

28 CHAMFERS 3 X 30°

90 °

(46)

*Heading

** Job name: A50 Model name: Model-1 ** Generated by: Abaqus/CAE Version 6.8-2

*Preprint, echo=NO, model=NO, history=NO, contact=NO ** ** PARTS ** *Part, name=big *Node 1, 0.0342181101, 0., 0. 2, 0.0342181101, -0.0500000007, 0. 3, 0.0342181101, 0., -0.0500000007 • • • 6590, 0.00716625992, 0.0595878214, -0.00549670681 6591, -0.00162207696, 0.056425292, 0.0042985105 6592, 0.0285064857, -0.00864811707, -0.0462547578 *Element, type=C3D4 1, 2685, 2686, 2687, 2688 2, 2685, 2689, 2687, 2690 3, 2685, 2691, 2689, 2692 • • • 31096, 3893, 4778, 4777, 5612 31097, 3893, 5887, 5612, 3965 31098, 3965, 4515, 3967, 3969

*Nset, nset=_PickedSet4, internal, generate 1, 6592, 1

*Elset, elset=_PickedSet4, internal, generate 1, 31098, 1

** Section: Steel

*Solid Section, elset=_PickedSet4, material=Steel

*End Part ** *Part, name=small *Node 1, 0.0170000009, 0., 0.050999999 2, 0.0309938379, 0.0091985222, -0.0638002381 3, 0.0309938379, 0.0193942059, -0.0614731535 • • • 5799, 0.0107407356, 0.047520332, -0.0215661433 5800, 0.0133662429, 0.0468277372, 0.00504350802 5801, -0.000581190921, 0.0388067998, 0.0171161611 *Element, type=C3D4 1, 2801, 2802, 2803, 2804 2, 2801, 2805, 2806, 2807 3, 2806, 2808, 2809, 2801 • • • 25982, 2852, 2657, 2639, 1088 25983, 1271, 1297, 4494, 4968 25984, 4492, 4493, 1278, 1229

*Nset, nset=_PickedSet5, internal, generate 1, 5801, 1

*Elset, elset=_PickedSet5, internal, generate 1, 25984, 1

** Section: Steel

*Solid Section, elset=_PickedSet5, material=Steel

*End Part ** **

(47)

**

*Instance, name=big-1, part=big

0.1322, 0., 0. *End Instance

**

*Instance, name=small-1, part=small

0.0954296114533829, 0., 0. *End Instance ** *Node 1, 0.176418111, 0., 0. *Node 2, 0.0824296102, 2.93905523e-18, -4.40872832e-18 *Node 3, 0.0724296123, 2.93905523e-18, -4.40872832e-18 *Element, type=CONN3D2 1, , 3

*Connector Section, elset=Wire-1-Set-1, behavior=Moving Cylindrical,

"Datum csys-1",

*Nset, nset=_PickedSet37, internal 1,

*Nset, nset=_PickedSet42, internal, instance=small-1 285,

*Nset, nset=_PickedSet44, internal, instance=big-1 1,

*Nset, nset=Wire-1-Set-1 3,

*Elset, elset=Wire-1-Set-1 1,

*Nset, nset=Wire-2-Set-1 1,

*Elset, elset=__PickedSurf6_S3, internal, instance=small-1

6154, 6853, 9230, 10217, 17150, 17659, 19379, 19380, 20094, 20652, 20658, 20707, 21006, 23587, 25550 *Elset, elset=__PickedSurf6_S1, internal, instance=small-1

14888,

*Elset, elset=__PickedSurf6_S4, internal, instance=small-1 16929, 20706

*Surface, type=ELEMENT, name=_PickedSurf6, internal __PickedSurf6_S3, S3

__PickedSurf6_S1, S1 __PickedSurf6_S4, S4

*Elset, elset=__PickedSurf7_S2, internal, instance=big-1

24, 153, 255, 272, 476, 537, 761, 809, 1201, 1735, 1743, 3976, 4273, 4972, 5048, 5297 5328, 5466, 5500, 5614, 6204, 6386, 6498, 6499, 6564, 7736, 8373, 8402, 8569, 8599, 8676, 9128 9212, 9236, 9276, 9342, 9650, 9825, 9878, 10464, 11029, 11615, 11619, 11688, 11788, 12274, 12664, 12683 12720, 13452, 13661, 13665, 13973, 14046, 14381, 14388, 15180, 15211, 15526, 15737, 15823, 16032, 16035, 16039 16085, 16269, 16287, 16300, 16311, 16376, 16659, 16821, 16848, 17079, 17399, 17644, 17831, 17955, 18082, 18086 18221, 18435, 18591, 18844, 18981, 19011, 19100, 19193, 19449, 19605, 19703, 19713, 20465, 20526, 20988, 22533 22832, 25290, 26086, 26667, 27159, 28985, 30708, 30735

160, 176, 668, 948, 1743, 3621, 3845, 4281, 4687, 4993, 5011, 5032, 5105, 5175, 6347, 6543 6616, 6646, 6734, 7458, 7531, 7628, 8282, 8376, 8382, 8623, 9280, 9288, 9924, 10495, 10526, 10589 11073, 11260, 11506, 11681, 12104, 12129, 12170, 13396, 13668, 14005, 14434, 15196, 15558, 15630, 15746, 16166 16284, 16823, 17018, 17079, 17199, 17258, 17291, 17439, 17599, 18382, 18448, 18689, 19952, 21063, 21373, 21428 21724, 22278, 23073, 23521, 24677, 24758, 24885, 26352, 27461, 29648, 29964, 30469, 30975

69, 277, 290, 317, 374, 519, 614, 621, 1149, 1285, 1576, 1695, 1877, 2431, 2433, 2639 2686, 3869, 3870, 3951, 3959, 3964, 3971, 4011, 4019, 4040, 4190, 4194, 4255, 4263, 4281, 4283 4297, 4299, 4311, 4356, 4648, 4699, 4724, 4738, 4770, 4778, 4806, 4850, 4873, 4895, 4920, 4943 • • • 25924, 25965, 26394, 26515, 26518, 27446, 27533, 27536, 27539, 27625, 27903, 27931, 28038, 28254, 28302, 28408

(48)

694, 924, 3228, 4830, 5369, 5460, 5627, 6564, 6616, 6853, 7696, 7835, 8565, 9211, 9271, 9368 9679, 9779, 9866, 10150, 11664, 11692, 12071, 12132, 13152, 13568, 13925, 14011, 14386, 14514, 14781, 15170 15736, 15991, 16039, 16999, 17075, 17201, 17632, 18277, 18446, 18575, 18705, 18712, 18975, 18977, 19008, 19101 19202, 19273, 19340, 19416, 19526, 19537, 19779, 22529, 23066, 24014, 24196, 24357, 24673, 24826, 25730, 26087 26923, 27405, 27824, 28360, 30315, 30411, 30566, 30907

__PickedSurf7_S4, S4 __PickedSurf7_S3, S3 __PickedSurf7_S1, S1

9229, 12175, 13331, 13674, 16164, 16928, 16983, 17315, 17338, 17340, 17552, 18415, 24362 *Elset, elset=__PickedSurf8_S2, internal, instance=small-1

9270, 14608, 21898

5095, 6433, 8152, 8199, 8385, 8389, 9231, 10623, 13225, 16210, 16670, 16962, 18844, 18872 *Elset, elset=__PickedSurf9_S2, internal, instance=small-1

14499,

*Elset, elset=__PickedSurf9_S1, internal, instance=small-1 16607,

1160, 1409, 2294, 2387, 10725, 12879, 12946, 12954, 15306, 18363, 19193, 20279, 21057, 21230 *Elset, elset=__PickedSurf10_S1, internal, instance=small-1

2749, 13455

7466, 9090, 12779, 13366, 13886, 17930, 18417, 18578, 18954, 19033, 19798, 20092, 21072, 21074, 23143, 23826 *Surface, type=ELEMENT, name=_PickedSurf11, internal

6381, 7268, 10473, 11694, 11705, 11706, 11930, 12215, 12218, 15687, 16319, 21039, 25599 *Elset, elset=__PickedSurf12_S4, internal, instance=small-1

15203, 15427, 19388

621, 7223, 7406, 9156, 11342, 15338, 15870, 17141, 17188, 17195, 21916, 24146 *Elset, elset=__PickedSurf13_S4, internal, instance=small-1

9990, 11241, 16387

*Elset, elset=__PickedSurf14_S4, internal, instance=small-1 427, 12616, 20734