Chassis calculations for Frame design

(1)

Chassis calculations for Frame design

FU14-116

August 2, 2015

Erik Olofsson

(2)

Copyright

The publishers will keep this document online on the Internet – or its possible re-placement –from the date of publication barring exceptional circumstances. The on-line 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 copy-right 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 ad-ministrative 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 Link¨oping 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

(3)

This is a Masters Thesis report of a project carried out at Scania AB in S¨odert¨alje. The project concerns rationalizing Chassis calculations for use in truck Frame design. The subject for analysis is a six-wheeled articulated truck, and the load cases under study is Lateral Loading, Frame Torsion and Vertical Load on Kingpin. Making robust deformation and stress models with a calculation time sufficiently short and accuracy consistently high for efficient design work is an arduous task. This report presents several approaches to tackle this type of problem. By means of simplifying contemporary modeling approaches and methods and automating the setup process, a method that enables short calculation iterations on a chassis frame of a truck is achieved. This is done using the Catia GAS framework in conjunction with several other licences commonly used by designers.

(4)

Acknowledgements

A lot of support has been put in to this project, both from the university and from Scania. The author of this report is therefore eager to show his appreciation.

First of all Martin Hede (Scania) deserves to be shown gratitude for the helpful discussions and support throughout the project. So too does Uno Andersson (Scania) for the generous availability of courses and software. Also the supervisor of the project, Bo Torstenfelt (LiU) deserves a special mentioning for the sound advice and encouragement. A special mentioning also to the members of the steering commitee at Scania: Henrik Bruce for all the valuable input, Jonas Hagsj¨o for all the help with verifying models and to Mikael Thellner. Thank you also Christian Skoog (LiU) for the corrective reading, fresh perspective, and excellent opposition.

Erik Olofsson S¨odert¨alje, August 2, 2015

(5)

1 Introduction 8 1.1 Background . . . 8 1.2 Purpose . . . 9 1.3 Goal . . . 9 1.4 Problem specification . . . 10 1.5 Restrictions . . . 10 1.6 Method . . . 10 1.7 Other considerations . . . 11 2 Theoretical Background 12 2.1 Sources of Nonlinearity . . . 12 2.2 Submodeling . . . 13 2.3 Element formulations . . . 13 3 Method 15 3.1 Element formulation for beam structure . . . 15

3.2 Script aided analysis setup . . . 19

3.3 Verification . . . 21

3.4 Load Cases . . . 22

4 Results and Discussion 29 4.1 Verification of Load Cases . . . 29

4.2 Overall methodology . . . 36

4.3 Future work . . . 37

5 Conclusions 38

A Appendix I

A.1 General Analysis Connection and Rigid connection property . . . II A.2 One-Click-Publish A Series of Publications . . . VI A.3 One-click-create a series of General Analysis Connections and Rigid

Connection properties between series of publications . . . IX A.4 Submodeling . . . XIV

(6)

List of Figures

1.1 Picture of the Chassis Frame. . . 9

2.1 Principal sketches of elements . . . 14

3.1 Picture showing principle of load case application. . . 15

3.2 Picture showing 10-node Tetrahedron mesh. . . 16

3.3 Picture showing 10-node Tetrahedron mesh combined with a Beam element. . . 16

3.4 Picture showing 6-node Triangle mesh combined with a Beam element. 17 3.5 10-node Tetrahedron . . . 18

3.6 Procedure for running submodel . . . 21

3.7 Picture showing coordinate system alignment and points used for elimination of rigid body rotations. . . 22

3.8 Picture showing principle of Cornering load. . . 23

3.9 XY-view of free body diagram. . . 23

3.10 ZY-view of symbolic axle. . . 24

3.11 Boundary conditions for Lateral Load . . . 24

3.12 Boundary conditions for Frame Torsion . . . 25

4.1 ISO view of Von Mises Stress field from Catia Lateral Loading Load Case . . . 29

4.2 ISO view of Von Mises Stress field from Abaqus Reference Lateral Loading Load Case . . . 30

4.3 Collocation of deformation on top right flange edge due to Lateral Loading according to method in Section 3.3 . . . 30

4.4 ISO view of Von Mises Stress field from Catia Frame Torsion Load Case . . . 31

4.5 ISO view of Von Mises Stress field from Abaqus Reference due to the Frame Torsion Load Case . . . 32

4.6 Collocation of deformation on top right flange edge due to Frame Torsion according to method in Section 3.3 . . . 32

4.7 ISO view of Von Mises Stress field from the Catia Vertical Load on Kingpin case . . . 33

4.8 ISO view of Von Mises Stress field from Abaqus Reference due to Vertical Load on Kingpin . . . 34

4.9 Comparison of nodal displacement on top right flange edge due to Vertical Load on Kingpin according to method in Section 3.3 . . . . 34

4.10 Collocation of nodal displacement on top right flange edge due to taking Nonlinear geometry into account in Lateral Loading loadcase 35 4.11 Difference in nodal displacement due to taking Nonlinear geometries into account in Lateral Loading loadcase . . . 35

(7)

4.12 Collocation of nodal displacement on top right flange edge due to taking Nonlinear geometry into account in Frame Torsion load case . 36 4.13 Difference in nodal displacement due to applying Linear Perturbation

(8)

List of Tables

2.1 Governing parameters of the beam element . . . 14 3.1 Mean deflection in loaded direction of nodes on edge face due to unit

force [N] or torque [Nxm]. . . 19 3.2 100U −Uref

Uref using 10nodeTET as reference. . . 19 3.3 Convergence study . . . 19

(9)

Introduction

1.1 Background

Scania AB is one of the world’s leading manufacturers in the heavy transport seg-ment. The company has been developing Trucks and associated support systems since 1911 and has a sales and service organisation spanning more than a hundred countries.

An integral part of the truck is the Chassis frame. Being the main load bearing structure of the truck, well-conditioned design of the Chassis frame is paramount to the success of the truck as a whole.

The Chassis frame, pictured in Figure 1.1 is the foundation on which the rest of the truck is mounted. It comes in many configurations, where the needs of the customer are reflected in the payload that the Frame is fitted with and what combi-nation of driving condition and speed it is to handle. The Frames varies in length, thickness of members and number of crossbeams but has several governing charac-teristics.

• Characteristics

– Steel and cast iron is used for both cross and lengthwise beams – The lengthwise beams have a “C” shaped cross section

– The crossbeams run in an orthogonal direction between the lengthwise beams

– Rivets are used, where applicable, for attaching non-removable geometries – Bolts are used for removable geometries

(10)

CHAPTER 1. INTRODUCTION

Figure 1.1: Picture of the Chassis Frame.

The Frame is subject to continuous improvements, where any development which leads to a more light-weight structure enables bigger payloads and less fuel con-sumption. This goal, while also considering the requirements on stiffness, price and respecting the modular boundary reserved for the Frame, makes for a complex task. It is worth mentioning that the production methodologies and fundamental design principles of the Frame can be considered mature, seeing as the Frame, in its many variants, has been iterated upon for decades.

In construction of Chassis frames there is great demand for exploratory and ver-ifying calculations complementing the experience and testing schemes guiding the designers in their effort. In contemporary methodologies calculations are performed by designers, generally with limited and usually linear models, and calculation en-gineers, using more intricate and often non-linear models. A central challenge is to shorten the iteration time, i.e. the time from identification of the need for calculation and the result, in order to make reviewing of changes to the design configuration more effective. This can be done by either increasing the computational power or relaxing the computational problem and thereby cut the amount of CPU-hours re-quired. The current computer aided design tool (CAD) used at Scania is Catia [1] , where simulation is performed in the Catia Generative Assembly Structural analy-sis tool (GAS). In this tool, geometries can be assembled for analyanaly-sis directly from the CAD interface, whereupon structural, modal and thermal calculations can be performed on the structures [2].

1.2 Purpose

The purpose of this thesis is to investigate ways of simplifying frame calculation models currently being used for verification into something that can be used iter-atively during design. Furthermore, the thesis is to meet the requirements for a degree project - Master’s Thesis at Link¨oping University.

1.3 Goal

The goal of the project is to, at the conclusion of the project, present a recom-mendation on how to approach using finite element (FE) analysis when designing

(11)

chassis frames. The recommendation is concerning both the effective setup of the analysis, verification of the model using comparisons to a similar model in Abaqus and handling the result.

1.4 Problem specification

The geometry for investigation is a six-wheel truck frame mounted with a Kingpin subjected to a 210 [KN] vertical force representing a standard trailer. Three load cases that historically have proven to be dimensioning for side- and crossbeams, Vertical Load on Kingpin, Lateral Loading and Frame Torsion, are investigated. Can simplifications to contemporary analysis setups for the investigated load cases be used to enable both the accuracy and computation times that is needed for effective iterative frame design using a standard computer?

1.5 Restrictions

Well posed restrictions are crucial in order to attain a depth of detail sufficient enough to be both comprehensible and universal so that the methodology presented herein can be mimicked on similar problems.

1.5.1 Restriction on physical magnitudes for investigation

The analysis is restricted to only obtain deformation and stress levels. This is in part due to limitations in the software. The results are intended to give a good basis for verification but at the same time limit the amount of theoretical knowledge needed to use the method compared to, say, cycles-to-failure-estimations.

1.5.2 Restriction on material- and deformation models

The analysis will assume small deformations and linear stress-strain relationships only. This is in part due to limitations in the software. This is a reasonable assump-tion for the three load cases in quesassump-tion. The method and result of the investigaassump-tion of the well-posedness of this assumption is presented in Section 3.4.5 and Section 4.1.4 respectively.

1.5.3 Restriction on software

Apart from the verification only the tools and methods found in Catia GAS and associated licenses are used in the analysis. No external tools will be used for meshing, post-analysis or other. This is intended to keep the method close to the one envisioned to be the standard method for future design work at Scania.

1.5.4 Restriction on domain of investigation

The geometry and boundary conditions are restricted in order to, for the three chosen load cases, describe the deformation and stress with sufficient accuracy for the side-and crossbeams. All other geometry is considered to be of secondary importance.

1.6 Method

The method is to, with Scania best practice documents for load cases as a guide, establish load cases in Catia GAS, and find ways of making the calculation time

(12)

suffi-CHAPTER 1. INTRODUCTION

ciently short and accurate for efficient design work. The verification comprises com-parisons of deformation and stress levels with similar results provided from Abaqus models. In addition, analytical calculations are performed on particular geometries where applicable. In addition to this exploring ways of enhancing the speed at which the analysis case can be established via automating parts of the analysis setup will be explored.

1.7 Other considerations

No ethical or gender related questions are raised by the thesis. It has no direct connection to environmental or social effects.

(13)

Theoretical Background

In the following chapter, the necessary theory used in the method will be displayed.

2.1 Sources of Nonlinearity

In linear analysis [K]{D} = {R} has a unique solution where the deflection is linearly proportional to the applied force. In the instance of nonlinearities, where either of or both [K] and {R} are functions of {D} a solution to [K]{D} = {R} can only be found using methods where [K] and {R} are updated iteratively [3]. The following section describes the relevant types of different terms.

2.1.1 Geometric Nonlinearity

Geometric nonlinearities are stiffness variations caused by large deformation or ro-tations during loading or unloading of a structure. FE-softwares generally gives the option of making “small-displacement” assumptions. This means ignoring geomet-ric nonlinearities in the element calculations, and linearizing the kinematic relation-ships. The elements are formulated in the initial configuration and does not update during the analysis. In the case of Catia GAS, this assumption is the standard [4]. Using Abaqus on the other hand this is only optional. Abaqus gives, even in the case of linear element formulations, the option of utilizing large-sliding contact tracking algorithms to account for rotations and large displacements [5].

2.1.2 Material Nonlinearity

Material nonlinearity is present in all material formulations where the stress-strain relationship is not linear. Factors like plastic flow, where a loading induces change to the microscopic structure of the material or history dependence, i.e. a material’s response being sensitive to previous loading are sources to nonlinearities.

2.1.3 Boundary Nonlinearity

Boundary nonlinearities stem from either gaps opening or closing or sliding with or without friction occurring between surfaces of two structures, or between internal surfaces of a structure. Such nonlinearities are prevalent in analysis using bolt tightening. The accuracy, robustness and computational complexity varies with the discretization and sliding tracking approach [6]. In Catia GAS the only available method for approximating slider connections uses a “node-to-surface” discretization combined with a “small-sliding” tracking approach [7]. Because the Elfini solver, the Catia standard issue solution engine, does not allow for large displacement[4],

(14)

CHAPTER 2. THEORETICAL BACKGROUND

all sliding and rotations are considered infinitesimal. Abaqus/Standard allows for a plethora of different approaches to contact discretization, tracking approach and enforcement. The general contact formulation in Abaqus/Explicit utlilizes ”surface weighting”-, ”surface polarity”- and ”finite sliding”-approaches by default [8].

2.2 Submodeling

Submodeling is a technique that enables studies of a local region of a large model using boundary conditions based on an interpolation from the solution of the large model. In the case of nodal deformation-based submodeling, according to Cook[3] the procedure usually is as follows: A global model with a mesh refinement suf-ficient for ensuring confidence in accuracy of the global deformation is run. The displacement of the nodes surrounding the local region designated for subanalysis is exported. The exported displacement is imposed on the boundary of the local region via an interpolation scheme. This allows for mesh refinement in the local region to an extent which can give a very high resolution description of the stress field, at a relatively low computational cost. The submodeling approach is suitable in cases where the detail of modeling in the studied region has a small effect on the overall solution. If changes are to be made to the submodel structure, they need to be sufficiently small as to not change the overall stiffness of the adjacent structure, else they invalidate the submodel, calling for another global analysis[3]. Catia does not support node-based export of deformation to submodel by default. There are, however, methods of exporting and imposing nodal deformations. Such capabilities in conjunction with a palette of possibilities of assigning master and slave node rela-tionships, with both kinematically and least square approaches, opens up for, albeit somewhat reduced, methodologies that are similar in effect to submodeling.

2.3 Element formulations

The following elements are used:

For 3D-elements, 10-node iso-parametric Tetrahedrons as seen in Figure 2.1a are used. This element has four gauss points [9].

For shell-elements, 6-node Parabolic Triangles as seen in Figure 2.1b are used. This element has three gauss points [10].

For Beam elements, a two-node straight beam element with traverse shear based on Timoshenko theory is applied[11]. The principle sketch of the beam can be seen in Figure 2.1c. Catia presents several methods of assigning the governing parameters seen in Table 2.1 of the beam element according to different types of cross-sections. One of those, the ”Beam from surface” approach allows for the selection of an arbitrary cross-section as basis for an automatic assignment of the beam parameters [12].

The Kinematic spider, or rigid spider, connects a series of slave nodes to a mas-ternode using kinematic relationships[13]. A kinematic spider-element containing only one slave node is called a kinematic beam-, or rigid beam-element.

(15)

Table 2.1: Governing parameters of the beam element

Symbol Unit Property

A m2 Cross-sectional Area

Cy m y-coordinate of the shear center of the beam

Cz m z-coordinate of the shear center of the beam

qxy − Ratio of Y shear area over cross-sectional area

qxz − Ratio of Z shear area over cross-sectional area

Ixx m4 xx-component of the inertia matrix of the beam

Iyy m4 yy-component of the inertia matrix of the beam

Izz m4 zz-component of the inertia matrix of the beam

(a) 10-node Tetrahedron (b) 6-node Triangle

(c) Beam (d) Kinematic Spider

(16)

Chapter 3

Method

3.1 Element formulation for beam structure

Analysis run times are closely related to the number of unknowns in the structure. Computation times can therefore be reduced by, where suitable, utilizing elements that use fewer nodes while still accurately describing the structure. As the model described in Section 3.4 is comprised of mainly beams with a more or less non variable cross-section in different constellations, the analysis run time can be reduced by utilizing the less heavy beam element formulation. The studied beam is a typical cast iron beam used for stiffening the structure immediately surrounding the bogie suspension. It has a somewhat uneven cross-sectional area, making it an interesting specimen for investigating the effect of different discretizations. The beam is studied using three levels of complexity. All three setups has one side clamped at the hole edges, while the other side’s face is subject to four sets of forces. The four load cases applied are unit loads (1 [N]) in the X-, Y- and Z-directions and torque (1 [Nm]) in Y-direction applied evenly distributed on all nodes of the beam’s end face as shown in Figure 3.1. The evaluation is in the form of measuring the displacement of the end - face nodes separately for all the loads applied.

(17)

3.1.1 10-node iso-parametric Tetrahedron

This element formulation follows the CAD- geometry of the beam as shown i Figure 3.2. Setup times are short, seeing as the procedure for applying an auto-mesh and applying the appropriate boundary conditions is trivial. This approach also has a certain intuitiveness, since stress field renditions can, when studied critically, give a hint of the well-statedness of the studied problem. The convergence of the end face displacement with respect to element size is studied. The setup time for this configuration is approximately 15 minutes.

Figure 3.2: Picture showing 10-node Tetrahedron mesh.

3.1.2 10-node Tetrahedron / Beam element

This setup utilizes the 10-node Tetrahedron for the parts of the beam with a variable cross section area, and the Beam element formulation for the more or less constant cross sectional mid portion of the beam as seen in Figure 3.3. The beam properties are established to mimic the cross section at the mid portion of the beam using the built in “Beam From Surface” tool in conjunction with kinematic spider elements connecting the beam to the end surface of the Tetrahedron portions of the structure. The converged mesh density of 10-node tet-element were used for the variable cross-section portion. The setup time for this configuration is approximately 90 minutes.

Figure 3.3: Picture showing 10-node Tetrahedron mesh combined with a Beam element.

(18)

CHAPTER 3. METHOD

3.1.3 6-node Parabolic Triangle / Beam element

This setup utilizes the 6-node parabolic triangle element with a shell property for modeling the end plates of the beam. A beam element connects the two end plates using a property established with the ”Beam from Surface” tool in conjunction with kinematic spiders connecting the beam end nodes to a delimitation of the end surface mesh that is a projection of the mid cross section of the beam onto the end plates. The setup time for this configuration is approximately 90 minutes and the mesh can be seen in Figure 3.4.

Figure 3.4: Picture showing 6-node Triangle mesh combined with a Beam element.

3.1.4 Element choice Evaluation

The following section is an evaluation of the three discretization approaches. As seen in Table 3.1 and visually in Figure 3.5d the difference in end-face defor-mation is negligable when comparing the 10-node TET to the Beam/10-node Tet formulation. The differences in deformation is, as seen in Table 3.2, not consistent between the four load cases.

The effect from using a kinematic spider to connect the beam element to the end piece structure does not seem significant for this type of composition. Since the kinematic-spider approach effectively creates an infinitely stiff cross-section, it is likely that such an approximation would be unsuitable for beams where the local deformation at or near the cross section is important to the global behaviour. This can be seen in comparing Figures 3.5a and 3.5b where the local stiffening from the rigid spider affect the deformation and stress distribution in close vicinity to the spider.

Another source to the difference in stiffness is that the beam element formulation assumes a constant cross section. The Tri/Beam configuration, seen if Figure 3.5c is affected to a greater extent from this compared to the Tet/Beam seen in Figure 3.5b. The cross section is more uneven and gets progressively thicker closer to the end plates. This could be better described by using a multitude of cross-sections as basis for the beam elements, giving a greater stiffness closer to the end plates. Another approach could be some form of linear scaling of the stiffness. The suitability of such approaches could be put into question since the setup-time of such endeavours far exceeds the gain in computation time, as seen in Table 3.1.

One important item to consider is the fact that the Tet10/Beam configuration takes longer time than the pure Tet10 approach to compute. This is in spite of

(19)

having 4/5 the amount of nodes. This is likely due to restrictions to the Catia solver where multithreading (i.e. parallel computation) is restricted to the factorization computation, Direct method and frequency solution steps. All other solution steps, namely the ones associated with setting up the problem, are single threaded [14]. This punishes approaches where one part is replaced by several less complex parts, as theese attempts show. The computational time cost saving from reducing the amount of degrees of freedoms is more than made up for by the additional time spent in the slower single threaded solver steps on one hand and the considerable extra time spent on analysis setup on the other hand. One can therefore argue that the most efficient way of shortening the analysis iteration time is to streamline the analysis setup process. If, on the other hand, a less strict criterion for convergence were to be used, the difference in the amount of nodes of the mesh between the 10-node TET to the Beam/10-node Tet would be bigger. See Table 3.3 for the convergence study. This is due to the a behaviour of the automatic mesh procedure where regions of the structure with sharp surface curvatures are prioritised over non-complex parts of the structure in the mesh distribution. In the example using 10-node TET elements, the mesh refinement is mostly focused at in the structure that is not approximated by the beam element. The Beam/10-node Tet-approach would with this reasoning be more efficient at lower degrees of mesh refinement.

(a) Tet V M stress in de-formed state. (b) Tet/Beam V M stress in deformed state. (c) Tri/Beam V M stress in deformed state. (d) Tet : Blue Tet/Beam : Red Tri/Beam : Green Figure 3.5: 10-node Tetrahedron

(20)

CHAPTER 3. METHOD

Specimen Ux[m] Uy[m] Uz[m] αy[◦] CPU/Walltime [s] Nr of nodes [-]

TET10 6.37e-8 -2.74e-9 0.89e-7 3.23e-5 70.3/35.3 158197 TET10/Beam 6.33e-8 -2.78e-9 0.89e-7 3.17e-5 72.7/35.4 132469 TRI6/Beam 8.86e-8 -2.13e-9 1.28e-7 3.84e-5 1.98/1.47 2864

Table 3.1: Mean deflection in loaded direction of nodes on edge face due to unit force [N] or torque [Nxm].

Specimen Xf ault[%] Yf ault[%] Zf ault[%] αyf ault[%]

10nodeTET - - -

-10nodeTET/Beam/Rigid -0.6198 1.3589 -0.2608 -1.7970 6nodeTRI/Beam/Rigid 39.2541 -22.2929 43.5319 18.7680

Table 3.2: 100U −Uref

Uref using 10nodeTET as reference.

Prescribed element width [m] 7e-2 4e-2 2.5e-2 1.5e-2 7e-3

Number of nodes [-] 41341 81474 141999 158197 277866

10nodeTET CPU-/Wall time [s] 12.7/7.6 24.6/13.9 53.9/28.2 70.3/35.3 187.0/85.5 10nodeTET Ux[m] 6.2770e-8 6.3074e-8 6.3513e-8 6.3649e-8 6.3692e-8

Table 3.3: Convergence study

3.2 Script aided analysis setup

The results from attempts described in Section 3.1.4 suggest that the amount of time spent running the analysis is small compared to setting it up. Given Catias well documented integrated macro script functionality, one method of speeding up the setup process is automating repetitive or time-consuming steps of the process. It is conceivable to automate most if not all stages of the analysis setup, as the human interaction with Catia can be substituted with scripting, given the right input. The following section is dedicated to descriptions of the automation developed during this thesis. The codes can be found in Appendix A.

3.2.1 Automated Analysis Connections, Connection Properties

In Catia the interconnectivity between different mesh bodies is governed by differ-ent combinations of analysis connections and connection properties. The connection keeps track of what parts of the structure are to be connected while the connec-tion properties determine the type of connecconnec-tion (sliding, kinematic, spring, etc.). Making one Analysis Connection/Property couple is a procedure that when done manually takes 8-12 mouse clicks. In the case of the kinematic spider, the proce-dure found in Appendix A.1 reduces this to two (2) clicks. This principle can be used to automate all legal combinations of analysis connection and properties.

3.2.2 One-Click-Publish A Series of Publications

In Catia geometrical features can be assigned tags which, among other things, allows for geometries with similar function to become interchangeable. This operation is called publication. The script and procedure found in Appendix A.2 enables estab-lishment of publication series, where the features shares a common name, followed

(21)

by a unique index. This allows for quick-switching a geometry subjected to a mul-titude of analysis connections with another in the analysis context in an effective manner, or applying a large quantity of analysis connections in one operation as described in Section 3.2.3.

3.2.3 Automated Analysis Connections, Connection Properties be-tween Series of Publications

The script and procedure found in Appendix A.3 combines the principles of the scripts found in Sections 3.2.1 and 3.2.2. The result is an example of a script that applies a series of analysis connections and properties between two series of published geometries. The example can be modified into supporting any legal combination of connection and property.

3.2.4 Submodeling

As seen in Section 3.4.4 most beams are connected using kinematic spiders at each screw hole. The rigid spider element, as described in Section 2.3, has the property that it connects a masternode to any amount of slave-nodes as if fastened by infinitely stiff beam elements. This property, in conjunction with the capacity of exporting and/or enforcing any nodal displacement and rotations enables a method similar in principle to submodeling as seen in software like Abaqus. There are however a few limitations. The portion of the structure that is the subject of the submodel must be entirely delimited by either or a combination of:

1. Connections that use a master-slave node relationship. In Catia, examples of these are rigid connection properties, smooth connection properties, rigid virtual parts and smooth virtual parts.

2. Boundary conditions of any kind.

Any use of other connections like gliding with friction, surface pressure or surface contact will not render a result analogous to that of submodeling. The method goes as follows and has been automated to some extent with scripting, see Appendix Section A.1.1 for the code.

1. Run the global analysis.

2. Export the displacement and rotation on the master nodes of the connections delimiting the structure of the submodel from the global model.

3. Enforce the displacement and rotations on the masternodes of the submodel manually or by using the script in Appendix A.1.1.

4. Run the submodel

(22)

CHAPTER 3. METHOD

(a) Global analysis (b) Export displacement

(c) Enforce displacement (d) Run Submodel

Figure 3.6: Procedure for running submodel

This approach allows for changes to the mesh definitions of the submodel, giving access to stress pictures of great detail. Increasing the mesh density of the geometry feature subject to a connection property increases the amount of slave nodes in the master/slave relationship. In this respect, the method is totally analogous to submodeling interpolation schemes used in, for example, Abaqus.

3.3 Verification

For verification of the three load cases the global deformation of the side beams is studied. The Catia models and their respective Abaqus reference is compared. To this end, a generalized method of comparing global deformations have been estab-lished. The method is comprised of applying a limited amount of post processing using nodal deformation data. The following are the intended effects:

• It allows for comparisons between two different post processors.

• It enables comparison between two local deformations, with the option of elim-inating any rigid body translations or rotations from the result.

• As long as the node numbering goes unchanged, it can be rerun, offering a quick way to quantify the effect on deformation from a change.

In the case of the three load cases at hand the following procedure is used: 1. The nodal deformations are exported in whatever coordinate system that is

the default one.

2. Three nodes, A, B and C, are chosen in an area of small local deformation. A is the origo, norm(B-A) acts as the e1 direction and norm(B-A x C-A) is the e3 direction. (B-A)x(B-A x C-A) is the e2 direction.

(23)

3. Both the non-deformed and the deformed coordinates are translated into the coordinate system.

4. Plotting the non-deformed and the deformed state in their respective coordi-nate system renders a deformation picture which effectively has the rigid body rotation eliminated.

3.4 Load Cases

This section starts with a description of the three load cases under study. There are several governing characteristics of the models. All descriptions of vectors like forces and displacements will be notated in RH coordinate system with principal directions according to Figure 3.7, i.e. with the x-direction in the negative driving direction, and the y-direction aligned in the right. Furthermore, unless otherwise stated, the method of coordinate system transformation presented in Section 3.3 have been applied using the points A, B and C marked with blue arrows in Figure 3.7 on the data of all data plots displaying nodal deformations. This has the effect that point A acts as origo for all data plots. After the description of the load cases follows a description of the considerations made during the establishment of the model. The section ends with a description of the method for gauging the effect of the non-linearities not taken into account by the Catia model.

Figure 3.7: Picture showing coordinate system alignment and points used for elimination of rigid body rotations.

3.4.1 Cornering

The cornering load case stems from the phenomenon of considerable lateral bending occurring when driving vehicles with three or more axles slowly in sharp corners, visualised in Figure 3.8. Lateral reaction forces on the front axle wheels increase as they are being steered into an angle. This, in conjunction with the back wheels being aligned rigidly in the forward direction, generates large lateral forces on all wheel pairs as seen in Figure 3.9. This results in a considerable z-aligned torque on the bogie as well as a lateral bending of the frame. The severity is increased in configurations with non-steered rear axles, as this increases lateral forces on the rear axles and thus the z-aligned torsion of the bogie.

(24)

CHAPTER 3. METHOD

Figure 3.8: Picture showing principle of Cornering load.

Fy1r+ Fy1l− (Fy2r+ Fy2l) + Fy3r+ Fy3l= 0 (3.1)

− (Fy1r+ Fy1l) Ad+ (Fy3r+ Fy3l) Bd= 0 (3.2)

Where Fyn = µgenFzn (3.3) (Fynr+ Fynl) Wrd− (Fznr+ Fznl) Tnd 2 = 0 (3.4) Fznl+ Fznr = 9.81Pn (3.5)

Where Pnis the technically allowed weight on axle n. Assuming center of gravity of

both truck and trailer are centered gives equal contact pressure between wheelpairs on all axles.

Fznl= Fznr (3.6)

(25)

Figure 3.10: ZY-view of symbolic axle.

(26)

CHAPTER 3. METHOD

3.4.2 Frame Torsion

The frame Torsion Load Case is used to dimension the frame to handle the twisting deformation that is associated with uneven road conditions. When the truck drives over a bump with one wheel, the frame deflection is dependant on the frame torsional stiffness. The established method of testing this property is for articulated trucks divided into two steps. For the first step, a forced displacement couple is applied on the front wheels, and in the second step, the displacement is reversed, see Load Case Vertical Load on Kingpin. As a mid load, force equivalent to 1g of the motor, cab and bogie weight is applied in each center of gravity respectively. See Figure 3.12 for a description of the boundary conditions. The resulting stress tensors are then used to identify the mean and amplitude of the stress levels of critical components, which can then be compared to material data to ensure the expected load cycles to failure related metrics.

Figure 3.12: Boundary conditions for Frame Torsion

3.4.3 Vertical Load on Kingpin

The Vertical Load on Kingpin load case is, while most commonly used as a mid load in fatigue-analysis Load Cases, in itself interesting. The load case is often used as a ”first probe” when deciding upon whether to attempt a new type of configuration. To this end, tools have evolved around the idea of automating calculations using custom built software to solve this load case specifically. The ease of implementa-tion and comparison to other configuraimplementa-tions is it’s major advantages. The forces equivalent to the weight of the motor, cabin and trailer under the influence of 1g are applied to their respective centers of gravity. In this implementation, the mid load is investigated by using the mean tensor field of two load steps from the frame torsion load case according to Equation 3.7.

Tmid=

T1+ T2

(27)

The first load step is the one described in Figure 3.12. The second load step has reversed enforced displacements in the vertical direction compared to the first, and is identical in all other respects. This results in a non symmetrical deformation seeing as the boundary conditions of the Frame Torsion Load Case is not symmetrical.

3.4.4 Modeling considerations

The model is comprised of 35 unique parts discretized by 245271 TRI- and 358561 TET-elements. The parts are connected by 763 spider elements, 18 bar elements and 4 springs.

Non-script assisted setup of such a model would take approximately one week’s time. The run time of the Cornering and Frame Torsion load cases analysis is 60 minutes for a mesh density sufficient for converged deformation along the sidebeams. The Vertical Load on Kingpin load case takes 120 minutes as two load steps are needed for the result. During modeling, several considerations have been made. The following section describes them.

Constant thickness geometries

All structure with a predominately constant thickness were modeled using 6node TRI elements. This is intended to give a reasonable estimation of the stiffness while also enabling renditions of the stress field, a feature not available for beam elements. The alternative, i.e. modeling for example the sidebeams using TET10 elements would require a large amount of elements if a healthy element width ratio is to be maintained. This is especially true if more than one layer of elements is to be applied across the cross-section, which could be useful if studying stress fields at or around screw holes. It would be possible to succesfully model the deformation of the structure using beam elements and springs only. Such an approach would, while efficient computational-time wise, be impractical in other respects. For one, doing this would not allow for pictures of the stress field, making the result usable only as far as comparisons using global deformation goes. Secondly, this would effectively nullify the biggest strength of the Catia GAS calculation engine, i.e. the close connection with the Catia Enovia Geometry database that contains all parts of virtually all Scania products. This connectivity allows for quick analysis where the mesh definition can be applied directly onto the geometries using the pre-defined positioning of the parts from the database. The geometries modeled using TRI6-elements include: Side-beams, 1:st through 3:rd cross beams, rear plate, rear axle housings, bumper and 5-th wheel brackets.

Variable thickness geometries

The 10node TET elements were reserved for geometries with uneven cross sections that could not easily be satisfactorily modeled using beam elements. This includes front axle and leaf springs, parts of the cab and bogie suspension brackets. Following the result in Section 3.1 no additional attempts (except the beam already simplified) were made to break up parts into sub-elements, as the returns in terms of shortened computational time was small compared to the increase in setup time.

Stiff structure

Kinematic spider elements were used to simulate the bolts and rivets holding the structure together. While Catia offers several options for estimating screw connec-tions, these other approaches were not used in order to keep the complexity of the

(28)

CHAPTER 3. METHOD

model at a minimum. The kinematic spider elements is a representation that is far more stiff than any screw or bolt can possibly be. Kinematic spiders were also used to transfer forces from their application point in space onto the structure. One example of this is the wheels. This approach more or less behaves as expected in the sense that the force is transferred along with the resulting torque. This is rea-sonable in loadcases where the force is applied directly and not through an enforced displacement. In the case of enforced displacement however, the non-deformation of the kinematic transferal can lead to a disproportionally large resultant force on the actual frame. Kinematic elements are also used in the motor-node and the kingpin as those parts of the structure were initially considered high-stiffness areas.

Suspension

The front suspension was modeled with a shape and positioning of the blades and linkage that represents normal, straight road driving conditions. No pre-tensioning was applied to the springs. The stress result of the spring blades should therefore not be expected to be accurate. The suspension blades transfers a predominately vertical load between the blades while gliding against each other when subjected to lateral loading. This gliding and at what loads it is initiated in conjunction with the large deformations associated with pre-tensioning of the springs is a complex and nonlinear phenomenon. With the solver being limited to small deformations and rudimentary contact definitions the following scheme is applied: The spring blades are discretizised using TET10 elements. The blades are fastened directly unto the first axle using kinetic spiders. Furthermore the spring is connected to the frame in the front using a pin connection with one rotational degree of freedom released, and the rear using a link that transfers vertical and lateral load along with x-aligned torsion. Because only small deformations are defined in the used solver, the linkage is not expected to rotate in a fashion resembling any real life event.

3.4.5 Evaluation of nonlinearites

Seeing as the Catia solver is strictly linear an attempt is made to visualize the effects of nonlinearities on the Abaqus reference. This is intended to give a measure of the magnitude of the effects that the Catia solver does not account for. It is important to note that these nonlinearities are far from the only difference between the Abaqus reference and the Catia models. Nevertheless it can act as a gauge of the impact from the differences in assumptions that are permanent restriction due to the choice of software.

Geometric nonlinearities

In terms of geometric nonlinearities, Abaqus gives the option of not taking into account the geometric nonlinearities geometry for a certain loadstep by toggling the property NLGEOM=yes/no. NLGEOM=no closely mimics the procedure used by the Catia solver and NLGEOM=yes is the one used in the Abaqus reference of this thesis. It should be noted that toggling NLGEOM=no does not render a wholly linear analysis, since this procedure still allows for time dependent effects like contact initiation, large sliding and other nonlinear phenomenons. In order to make the comparison the nodal displacement of the top flange on the right side beam is plotted without any coordinate transformation. This was chosen so as to not eliminate any rigid body motion, seeing as such behaviour is integral to geometric nonlinear phenomenons.

(29)

Boundary- and Material nonlinearities

In order to study the effect of boundary nonlinearities as well as material nonlin-earities a similar setup was chosen. By performing a static linear perturbation step, which assumes linear elastic material response as well as linear contact formulations and infinitesimal deformation a linear problem is achieved[15] (albeit a linearization around a pre-tensioned state). The initial load step involved with pre-tensioning of bolts and initiating contact is performed without any modifications. The resulting tensioned state is then used as basis for a transient load step that is linear. No con-tact can be initiated, and a linear material response is assumed [5]. The comparison is made by comparing the nodal displacement of the top flange on the right side beam and this time using the procedure of eliminating the rigid body motion of the frame as seen in Section 3.3. This is done because sliding is expected to occur in and around the suspension structure.

(30)

Chapter 4

Results and Discussion

4.1 Verification of Load Cases

4.1.1 Lateral Loading

Figure 4.1: ISO view of Von Mises Stress field from Catia Lateral Loading Load Case

(31)

Figure 4.2: ISO view of Von Mises Stress field from Abaqus Reference Lateral Loading Load Case

−4 −2 0 2 4 −0.01 0 0.01 0.02 0.03 0.04 Deformed X Coordinate [m]

Nodal displacement in Y direction [m]

Abaqus U

y

Catia U

y

(a) Displacement in Y di-rection −4 −2 0 2 4 −0.005 0 0.005 0.01 0.015 0.02 0.025 0.03 0.035 Deformed X Coordinate [m]

Nodal displacement in Z direction [m]

Abaqus U z Catia U z (b) Displacement in Z di-rection

Figure 4.3: Collocation of deformation on top right flange edge due to Lateral Loading according to method in Section 3.3

As seen in Figure 4.3 the nodal displacement of the top right sidebeam’s flange-edge of the Catia model follows the characteristic of the Abaqus reference in the Lateral Loading case. This indicates that the models have a similar lateral stiffness, at least insofar as this set of boundary conditions are concerned. It should be noted that this metric can be unintuitive in the sense that the cause of a region with a

(32)

CHAPTER 4. RESULTS AND DISCUSSION

large difference in nodal displacement can lie in a wholly other part of the structure. For instance, the difference in the x = −1 to x = −4 section is likely due to a misrepresentation of the stiffness in the region around the fifth wheel. It should also be noted that this load case is likely considerably less sensitive to inaccuracies in stiffness surrounding the front suspension than the Frame Torsion case because the principal force is applied in the form of force vectors as opposed to enforced displacements. The Von Mises stress rendering in Figure 4.1 exhibits the same characteristics with a few notable exeptions. Many screw holes connecting cross beams with side beams shows considerable stress concentrations in the Catia model. The Abaqus model has more continuous stress fields close to side beam hole pattern groups. This is likely due to the relatively high stiffness of the Catia rigid spiders compared to the more fine tuned screw approximation models used in the reference in Abaqus.

4.1.2 Frame Torsion

Figure 4.4: ISO view of Von Mises Stress field from Catia Frame Torsion Load Case

(33)

Figure 4.5: ISO view of Von Mises Stress field from Abaqus Reference due to the Frame Torsion Load Case

−4 −2 0 2 4 −0.07 −0.06 −0.05 −0.04 −0.03 −0.02 −0.01 0 0.01 Deformed X Coordinate [m]

Nodal displacement in Y direction [m]

Abaqus U

y

Catia U

y

(a) Deflection in Y direc-tion −4 −2 0 2 4 −0.01 0 0.01 0.02 0.03 0.04 0.05 Deformed X Coordinate [m]

Abaqus U z Catia U z (b) Deflection in Z direc-tion

Figure 4.6: Collocation of deformation on top right flange edge due to Frame Torsion according to method in Section 3.3

As seen in Figure 4.6 there is a great discrepancy between the Catia result and the reference. Figure 4.6a shows that Y-aligned displacement of the Catia result is more than three (3) times that of the Abaqus equivalent. The lateral stiffness of the front suspension, axle and wheels are disproportionally big, leading to the vertical push of the enforced displacement translating into a lateral deformation. The effect of this

(34)

disproportionate twisting is propagating along the frame and is visible in Figure 4.6b where the local stiffening of the crossbeams yields a distinct waveform of a larger amplitude than the one that can barely be made out on the reference. Comparing Figures 4.4 and 4.5 it can be seen that they tell the same story. All stress levels of the Catia model is above what can be expected. This is especially prevalent in the zones surrounding the interface between side- and cross-beam. However, when disregarding the actual stress-level, the distribution is very much similar between the Catia model and Abaqus reference.

4.1.3 Vertical Load on Kingpin

Figure 4.7: ISO view of Von Mises Stress field from the Catia Vertical Load on Kingpin case

(35)

Figure 4.8: ISO view of Von Mises Stress field from Abaqus Reference due to Vertical Load on Kingpin

−4 −3 −2 −1 0 1 2 3 −0.005 0 0.005 0.01 0.015 0.02 0.025 0.03 0.035 Deformed X Coordinate [m]

Abaqus U_z Catia U_z

Figure 4.9: Comparison of nodal displacement on top right flange edge due to Vertical Load on Kingpin according to method in Section 3.3

The vertical load in the Kingpin load case does, as seen in Figure 4.9, result in a relatively small deformation in the front portion of the frame in the Catia model. The effect is, however, not as pronounced as it may seem from the graph alone. The dominant force in this load case is applied vertically onto the structure very close to the node that acts as origo of the coordinate system, i.e. the A-node seen in Figure 3.7. Therefore, what may seem as a problem with the front portion of the structure is the result of a poor ratio of vertical stiffness between the front-and bogie-suspensions. The relatively high vertical stiffness of the bogie suspension

(36)

pushes up the mid section of the truck to a disproportionate degree. Likewise, the relatively low vertical stiffness of the front suspension also adds to the phenomenon. Lastly, the stiffness of the frame could be overestimated due to the stiffness added from the motor- and/or kingpin-node being too high. The stress rendering seen in Figure 4.7 has a similar distribution to that of the relevant Abaqus reference in Figure 4.8 albeit as expected from the deformation result, the overall stress level is lower. 4.1.4 Evaluation of nonlinearities −1 0 1 2 3 4 5 −5 0 5 10x 10 −3 Deformed X Coordinate [m]

Nodal displacement in X,Y&Z direction [m]

Nlgeom=yes u_x Nlgeom=yes u_y Nlgeom=yes u_z Nlgeom=no u_x Nlgeom=no u_y Nlgeom=no u_z

Figure 4.10: Collocation of nodal displacement on top right flange edge due to taking Nonlinear geometry into account in Lateral Loading loadcase −1 0 1 2 3 4 5 −5 −4 −3 −2 −1 0 1 2 3x 10 −5 Deformed X Coordinate [m]

Difference in Nodal displacement [m]

Nlgeom=yes u_x − Nlgeom=no u_x Nlgeom=yes u_y − Nlgeom=no u_y Nlgeom=yes u_z − Nlgeom=no u_z

Figure 4.11: Difference in nodal displacement due to taking Nonlinear ge-ometries into account in Lateral Loading loadcase

As seen in Figures 4.10 and 4.11, no significant difference in the global deformation of the side beams were introduced from assuming linear geometries. This does not necessarily mean that there is no effect at all, as large movements of for example the front springs could affect the stress-levels in close vicinity to that part of the structure. This result does lend some credence to the validity of the assumption of small deformations made in Section 1.5.2.

(37)

−4 −3 −2 −1 0 1 2 3 −0.03 −0.02 −0.01 0 0.01 0.02 0.03 0.04 0.05 Deformed X Coordinate [m]

Nodal displacement in X,Y&Z direction [m]

LnPerturb=no u_x LnPerturb=no u_y LnPerturb=no u_z LnPerturb=yes u_x LnPerturb=yes u_y LnPerturb=yes u_z

Figure 4.12: Collocation of nodal displacement on top right flange edge due to taking Nonlinear geometry into account in Frame Tor-sion load case

−4 −3 −2 −1 0 1 2 3 −20 −15 −10 −5 0 5x 10 −3 Deformed X Coordinate [m]

Difference in Nodal displacement [m]

LnPerturb=yes u_x − LnPerturb=no u_x LnPerturb=yes u_y − LnPerturb=no u_y LnPerturb=yes u_z − LnPerturb=no u_z

Figure 4.13: Difference in nodal displacement due to applying Linear Per-turbation to Frame Torsion load case

As seen in Figures 4.12 and 4.13, the effect of the Linear Perturbation is more severe than that of geometrical nonlinearities. The effect seems to affect the lateral deformation response at a significant rate. This could be due to the front suspension being sensitive to change from large to small sliding assumptions. The lack of wavy shape in the Z-aligned deformation can be explained as an effect of the relatively small lateral deformation and is not a separate phenomenon. The ”waves” are due to the otherwise continuous deformation of the top right side beam flange being interrupted by the local stiffening where the side beam meets the crossbeams. This is only visible during large lateral deformations.

4.2 Overall methodology

After it became apparent that the setup time of the analysis was significantly more costly than the simulation time, and that simplifications to the discretization re-sulted in minor gain to simulation speed, a shift in focus occured. Instead of only

(38)

focusing on finding simplifications to the discretization an effort was made to auto-mate the analysis setup, and later evaluation, using scripting.

4.3 Future work

The following items could be appropriate focuses for future development of the methodology that has been developed during this thesis.

During the verification phase of the project, several points were revealed where the Catia model behaves differently than the Abaqus reference. One idea for future work is therefore adjusting the lateral and vertical stiffness of the front suspension. This could lead to better results on load cases where the load is applied via enforced displacement.

Another approach could be to investigate the notion of replacing the whole front suspension with kinematic relationships coupled with spring elements. This could be made effective for load cases where the deformation is induced via load vectors.

(39)

Conclusions

A method for performing design oriented calculations investigating the three load cases, Lateral Loading, Frame Torsion and Vertical Load on Kingpin have been developed.

• Three load cases have been established in the Generative Assembly Structural analysis module of Catia (GAS). The setup of the model is by a large margin the most time consuming part of the process.

• The load cases have been verified by comparisons to Abaqus references. The difference in deformation and stress levels between the Catia model and Abaqus reference are varying depending on the load case. The Lateral Loading case shows less sensitivity to the differences in suspension stiffnesses compared to the Frame Torsion case.

• The impact from differences in calculation software have been considered and highlighted. The effect on the global deformation of the Abaqus reference due to Geometrical nonlinearities is negligable. The effect due to contact nonlinearities is considerable.

• The analysis setup time have been made considerably shorter by use of script based automation. This approach to analysis setup is a potent time saving possibility. Implementing fully automated analysis setup is conceivable. • A method of utilizing submodeling for reducing the computation time has been

implemented. The method allows for importing deformations from other FEM software.

(40)

Bibliography

[1] Scania Supplier Portal. Scania CAD/PDM Standards. url: https://supplier. scania.com/wps/portal/Home/Supplying-to-Scania/CAD-PDM/Engineering-Platform/.

[2] Dassault Systems. Product Highlights Catia GAS. url: http://www.3ds.com/ products- services/catia/products/v5/portfolio/domain/Analysis/ product/GAS/.

[3] Michael E. Plesha Robert D. Cook David S. Malkus and Robert J. Witt. Concepts and Applications of Finite Element Analysis. 4th ed. John Wiley & Sons, Inc, 2002.

[4] Catia V5 R20 Generative Analysis Documentation. What Type of Hypotheses are Used for Analysis? url: http://catiadoc.free.fr/online/estug_C2/ estugbt0614.htm.

[5] Abaqus Analysis User’s guide. 6.1.3 General and linear perturbation proce-dures. url: http://abaqus.ethz.ch:2080/v6.14/books/usb/default. htm?startat=pt03ch06s01aus44.html#usb- anl- alinearnonlinear (vis-ited on 06/21/2015).

[6] Abaqus Analysis User’s guide. 38.1.1 Contact formulations in Abaqus/Standard. url: http : / / abaqus . ethz . ch : 2080 / v6 . 14 / books / usb / default . htm ? startat=pt09ch38s01aus177.html (visited on 06/21/2015).

[7] Catia V5 R20 Generative Analysis Documentation. Creating Slider Connec-tion Properties. url: http : / / catiadoc . free . fr / online / estug _ C2 / estugbt0602.htm.

[8] Abaqus Analysis User’s guide. 38.2.1 Contact formulation for general contact in Abaqus/Explicit. url: http://abaqus.ethz.ch:2080/v6.14/books/usb/ default.htm?startat=pt09ch38s02aus180.html (visited on 06/21/2015). [9] Catia V5 R20 Generative Analysis Documentation. Obtaining Section

Parame-ters. url: http://catiadoc.free.fr/online/femug_C2/femugbt0206.htm. [10] Catia V5 R20 Generative Analysis Documentation. Obtaining Section Parame-ters. url: http://catiadoc.free.fr/online/femug_C2/femugbt0202.htm. [11] Catia V5 R20 Generative Analysis Documentation. Obtaining Section Parame-ters. url: http://catiadoc.free.fr/online/femug_C2/femugbt0207.htm. [12] Catia V5 R20 Generative Analysis Documentation. Obtaining Section Parame-ters. url: http://catiadoc.free.fr/online/ucfug_C2/ucfugbt7505.htm. [13] Catia V5 R20 Generative Analysis Documentation. Obtaining Section Parame-ters. url: http://catiadoc.free.fr/online/femug_C2/femugbt0212.htm. [14] Martin Roswall - Senior Technical Specialist at SIMULIA Nordics CSE. private

(41)

[15] Cambridge University Engineering Dept. What is the difference between Gen-eral and Perturbation steps? url: http://www- h.eng.cam.ac.uk/help/ programs/fe/abaqus/faq68/abaqusf10.html (visited on 08/02/2015). [16] Catia V5 R20 Generative Analysis Documentation. Analysis Assembly

Method-ology. url: http://catiadoc.free.fr/online/estug_C2/estugbt1603. htm.

(42)

Appendix A

Appendix

(43)

'--- Språkval, dokumentval ---

Language="VBSCRIPT"

Sub CATMain()

Set analysisDocument1 = CATIA.ActiveDocument

Set analysisManager1 = analysisDocument1.Analysis

Set analysisSets1 = analysisManager1.AnalysisSets

Set analysisSet1 = analysisSets1.ItemByType("ConnectionDesignManager")

Set analysisSets2 = analysisSet1.AnalysisSets

Set analysisSet2 = analysisSets2.Item(analysisSets2.Count,1)

'--- Etablering av G_A_C ---

Set analysisEntities1 = analysisSet2.AnalysisEntities

Set analysisEntity1 = analysisEntities1.Add("SAMGenericConnDesign")

Set basicComponents1 = analysisEntity1.BasicComponents

Set basicComponent1 =

basicComponents1.GetItem("SAMConnectionDesigner1.1")

basicComponent1.SetDimensions 0, 1, 1

Set analysisLinkedDocuments1 = analysisManager1.LinkedDocuments

Set productDocument1 = analysisLinkedDocuments1.Item(1)

Set reference1 = analysisDocument1.Selection.Item(1).Value

'--- reference1 läggs in i ruta 1 ---

Set product1 = analysisDocument1.Selection.Item(1).LeafProduct

basicComponent1.AddSupportFromProduct product1, reference1

'--- reference2 läggs in i ruta 2 ---

Set productDocument1 = analysisLinkedDocuments1.Item(1)

Set reference2 = analysisDocument1.Selection.Item(2).Value

basicComponent2.AddSupportFromProduct product2, reference2

'--- namn sätts ---

A.1 General Analysis Connection and Rigid connection

property

(44)

analysisEntity1.name=("G_A_C -

("&analysisDocument1.Selection.Item(1).LeafProduct.definition&"

("&analysisDocument1.Selection.Item(1).LeafProduct.name&") connected to "&analysisDocument1.Selection.Item(2).LeafProduct.definition&"

("&analysisDocument1.Selection.Item(2).LeafProduct.name&"))")

'--- SLUT C_G_A_C , C_R_C_P börjar - Analysmodell etableras ---

Set analysisModels3 = analysisManager1.AnalysisModels

Set analysisModel3 = analysisModels3.Item(1)

Set analysisSets3 = analysisModel3.AnalysisSets

Set analysisSet3 = analysisSets3.ItemByType("PropertySet")

Set analysisEntity3 = analysisEntities3.Add("SAMDistantRigid")

'---Ersätts med analyssettet från C_G_A_C ---

Set analysisEntity4 = analysisEntity1

Set reference1 =

analysisManager1.CreateReferenceFromObject(analysisEntity4)

Set reference2 =

Set reference1 = reference1.Parent

Dim bSTR1

bSTR1 = reference1.Name

Dim bSTR2

Dim bSTR3

Dim bSTR4

analysisEntity3.AddSupportFromReference reference1, reference2

analysisEntity3.name=("R_C_P - ("&analysisDocument1.Selection.Item(1).LeafProduct.definition&" ("&analysisDocument1.Selection.Item(1).LeafProduct.name&") connected to "&analysisDocument1.Selection.Item(2).LeafProduct.definition&" ("&analysisDocument1.Selection.Item(2).LeafProduct.name&"))") End Sub APPENDIX A. APPENDIX

(45)

Used License: MD2+MDN+GAS+SPA

Used Macro: C_GAC&RCP.catvbs

One-Click-Connection

General Analysis Connection &

Rigid Connection Property

in CATIA GAS

2015-06-09 RTCB / Erik Olofsson / Simulation Driven Design

1

Introduction

In this guide you will learn how to apply a General Analysis

Connection and Rigid Virtual Property via the use of a

macro.

For efficient use of this method it is recommended to assign

this macro to a hotkey.

1. only has to be performed if no Analysis Connection set

exists.

2

(46)

1. Create Analysis

Connections Set

1. Right-click on Analysis Connection Manager

2. Select Insert Analysis Connections Set

3. The Analysis Connections Set is now created

3

2. Execute macro

1. Select (Ctrl + Click) any two features you wish to connect 2. Run Macro

3. The General Analysis Connection and Rigid Virtual Property is now created

4

2 Standard procedure

APPENDIX A. APPENDIX

(47)

Language="VBSCRIPT"

Sub CATMain()

Set partDocument1 = CATIA.ActiveDocument

Set part1=partDocument1.Part

fileName = part1.Name

Set product1=partDocument1.Product

Set publications1 = product1.Publications

publname =Inputbox("Namnge publiceringen")

Set oSelection = CATIA.ActiveDocument.Selection

For i=1 to oSelection.Count

Set reference1 =

product1.CreateReferenceFromName(part1.name&"/!"&oSelection.Item(i).Value .Name)

Set publication1 = publications1.Add(publname&"_"&i)

publications1.SetDirect publname&"_"&i, reference1

End Sub

A.2 One-Click-Publish A Series of Publications

(48)

Used Macro: One_Click_Publish.catvbs

One-click-Publish

A series of features

using macro

in CATIA

1

Introduction

In this guide you will learn how to publish a series of features

in a part via the use of a macro.

For efficient use of this method it is recommended to assign

this macro to a hotkey.

A suffix index is applied in the publication name on the form

”_#” starting at #=1 and increasing with the number of

publications in the series.

The order of selection determines the order of #.

2

(49)

1. Select features for

publication

1. Open the Part in New Window 2. Select (Ctrl + Click) the features to

be published in the tree or in feature window.

Note: The selection order determines the suffix index.

3

2. Execute macro

1. Run Macro

2. Name the publication series by typing in the window

3. Press OK

4. The series publication is made

4

1 Standard procedure (See separate guide)

(50)

'--- SprÃ¥kval ---

Language="VBSCRIPT"

Sub CATMain()

'--- Dokumentval ---

Set analysisDocument1 = CATIA.ActiveDocument

Set analysisManager1 = analysisDocument1.Analysis

On Error Resume Next

Set analysisSets1 = analysisManager1.AnalysisSets

Set analysisSet1 = analysisSets1.ItemByType("ConnectionDesignManager")

Set analysisSets2 = analysisSet1.AnalysisSets

Set analysisSet2 = analysisSets2.Item(analysisSets2.Count,1)

'Produkterna sniffas frÃ¥n selection

publname1 =Inputbox("Ange publiceringarnas namn 1")

'--- Kan avkommenteras ifall två olika publiceringsserienamn skall kopplas ihop ----

'publname2 =Inputbox("Ange publiceringarnas namn 2")

'--- Skall avkommenteras om rad ovan bockas ur

publname2=publname1 For i = 1 To publications1.Count Set publication1=publications1.Item(publname1&"_"&i) Set publication2=publications2.Item(publname2&"_"&i) If Err.Number = 0 Then '--- Etablering av G_A_C ---

Set analysisEntity1 = analysisEntities1.Add("SAMGenericConnDesign")

'--- Namnsättning ---

Set basicComponents1 = analysisEntity1.BasicComponents

A.3 One-click-create a series of General Analysis

Con-nections and Rigid Connection properties between

series of publications

(51)

'Set analysisLinkedDocuments1 = analysisManager1.LinkedDocuments

'Set productDocument1 = analysisLinkedDocuments1.Item(1)

basicComponent1.AddSupportFromPublication product1, publication1

basicComponent2.AddSupportFromPublication product2, publication2

analysisEntity1.name=("G_A_C - ("&analysisDocument1.Selection.Item(1).LeafProduct.definition&" ("&analysisDocument1.Selection.Item(1).LeafProduct.name&") connected to "&analysisDocument1.Selection.Item(2).LeafProduct.definition&" ("&analysisDocument1.Selection.Item(2).LeafProduct.name&"))") '---

'--- SLUT C_G_A_C , C_R_C_P bÃ¶rjar ---

'---

'--- Analysmodell etableras ---

Set analysisModels3 = analysisManager1.AnalysisModels

Set analysisModel3 = analysisModels3.Item(1)

Set analysisSets3 = analysisModel3.AnalysisSets

Set analysisSet3 = analysisSets3.ItemByType("PropertySet")

Set analysisEntity3 = analysisEntities3.Add("SAMDistantRigid")

'--- ErsÃ¤tts med analyssettet frÃ¥n C_G_A_C ---

Set analysisEntity4 = analysisEntity1

Set reference1 =

Set reference2 =

Dim bSTR1

(52)

Dim bSTR2

Dim bSTR3

Dim bSTR4

analysisEntity3.AddSupportFromReference reference1, reference2

analysisEntity3.name=("R_C_P - ("&analysisDocument1.Selection.Item(1).LeafProduct.definition&" ("&analysisDocument1.Selection.Item(1).LeafProduct.name&") connected to "&analysisDocument1.Selection.Item(2).LeafProduct.definition&" ("&analysisDocument1.Selection.Item(2).LeafProduct.name&"))") End If Next End Sub APPENDIX A. APPENDIX