A Practical Approach to a Cad Implementation on a SME (Small
& Medium Enterprise)
Manuel Contero, Pedro Company and Nuria Aleixos
Departamento de Tecnología, Universitat Jaume I
Campus del Riu Sec - E12071 Castellón Spain
e-mail: contero@tec.uji.es
Abstract
This paper presents a methodology to be used to implement a complex 3D CAD
system (as PTC's Pro/ENGINEER) in an automotive sector subsidiary company of the
‘Comunidad Valenciana’ (Spain). It is believed that such a methodology is needed because
the transition from classic “design-by-drawing” methodology to full CAD methodology is
rather complex. In other words, managing large assemblies or complex parts just can be done
with a wise modelling approach.
Three steps have been considered in our approach:
• Strategies to create part models;
• Strategies to organise the assemblies, and
• Strategies to unify and simplify the management of the whole design process.
In this paper, some general ideas of those strategies will be summarised. Nevertheless,
we will focus on part modelling.
1.
INTRODUCTION
The low technological profile of many SMEs at Spain, suppose a big problem when
compare them with other higher competitors or from other countries. Competitiveness can be
improved in many different ways. One of them is raising the technological level of the
enterprise, using more advanced tools, like 3D CAD systems. But the available commercial
software have reached such a complexity that few SMEs decide to change from the old
design philosophies to new tools and methods; for example from 2D design to solid
modelling. The reasons of this barrier to change could be resumed in critical elements like:
inability to quantify return on investment, lack of qualified personnel, problems of
information interchange, previous failures and unknown information of implementing
process.
In this context, we are involved in a project titled "Implementing Design and
Manufacturing Advanced Technologies in a Concurrent Engineering Environment.
Application to an Automotive Components Manufacturing Company" supported by a
FEDER-CICYT grant (9I068.01). The principal objective this project proposes is determining
the procedure to follow for a successful implementation of the new technologies and
methodologies that support concurrent engineering.
In the first phase of the project, we have to define a methodology to implement a
complex 3D CAD system. Our industrial partner in the project wants to make a transition
from the 2D-design methodology, using Autocad R14 to a parametric 3D system like PTC's
Pro/ENGINEER.
To help us to carry out this objective, we made an Internet search looking for "good
practice" documents. Based on these documents [1],[2],[3],[4],[5],[6],[7] and our own
experience, we propose some strategies that can be very valuable in an implementation
process. Although the following methodology is focused in PTC's Pro/ENGINEER cad
system, it can be applied to similar parametric 3D CAD systems.
2.
STRATEGIES TO CREATE PART MODELS
Modelling methodology is a little documented topic. Big companies have internal
modelling guidelines, because reusing models is an important item due to many applications
that take advantage of the solid model, as CAM and CAE software. Also, sharing models
among designers, is a difficult question if there is not a common modelling strategy across
the enterprise and some documentation rules.
A lot of information is hidden in the solid model. Design intent is important to be
explicit; otherwise, model reuse and sharing become difficult or impossible. Modern CAD
systems allow the designer name the features or provide notes in order to document their
behavior. This is very important, because many times, the parent-child relations between
features are difficult to track, and the tools provided to analyze them, are at a very primitive
developing stage. Usually, these systems provide some kind of querying tool, to find the
parents and children of a feature, but it is difficult to have a whole vision of the
interdependencies. A model tree (see figure 1) provides some graphical description of the
model structure, but actually it is a historic record of modeling operations, not reflecting the
parent-child relations, better represented by a complex graph.
These limitations for understanding the model can produce serious problems when we
face the modeling of a complex part. A model with hundreds of features, soon become prone
to error when modifications are made. Assuring the quality of models is becoming a very
important topic, and one quality indicator is the use of standard design practices to improve
the effectiveness of downstream users and design reuse. There are some commercial tools
devoted to analyse the modelling rules and control the geometric quality, like Rand
Worldwide's ModelCHECK [10], International TechneGroup Incorporated's CAD/IQ [9] and
Prescient Technologies's DesignQA [8]. This means that there is a clear need in the industry
to define and control the modelling methodology for improving the models quality.
2.1.
Configuration files and start parts
Is commonly accepted that modern CAD systems have got high flexibility to address
many different design problems, but this flexibility usually implies many configuration
options to be established by the user. Certainly, CAD vendors claim to offer default
configurations optimised to get a compromise between maximum efficiency and extreme
simplicity. Nevertheless, this “homogenisation” may involve a serious penalty on efficiency
for advanced users. Consequently, the use of strategies to reconfigure the CAD systems to
better fit the particular needs is the first key to maximise efficiency. The CAD system
administrator must do this task because, usually, the CAD users would not be able to alter
that, and also it is a complex task, these users are not able to do. With common configurations
files, all users will have the same options, default layer structure and datums organisation.
Also it is important noting, that everybody must use the same start parts. Start parts
are equivalent to Autocad prototype drawings, or Microstation seed files. Of this way, some
items, like the layer structure, default datums and view orientations will be available to all the
CAD users, making easier to manage models built by other people.
Figure 1. Part and its associated model tree
2.2.
Datums
PTC’s Pro/ENGINEER is a parametric CAD system that heavily uses the concept of
datums to drive modelling process. Usually, the default datum planes are the first feature in
the model (figure 2). Points, axes, curves and planes can be used as datums that are
references for constructing models but they are not geometry features. Their both sides
(yellow and red) are used in assembling components, sketching references and orienting
views. In Pro/E, you can use datums as items in the model tree or you can make them belong
to any feature (also called datums on the fly). The datums on the fly are not shown and
selectable, and any dimension related to these datums are just shown with the feature to
which they belong. The datum axes are used for making datum planes, for placing items
concentrically and for making radial patterns. Axes are also automatically created for features
as revolved features and extruded circles and arcs.
Some guidelines are given below to make the best use of Datums in Pro/E:
• To avoid a stackup or undesirable relations in the part model, you should relate
datums back to principle datums.
• To avoid clutter on the screen you can use datums on the fly for cross-sectional
datums.
• In the case you use datums on the fly to create a pattern, be aware of pattern options
can only be chosen if the angle of offset and plane datum constraints are chosen.
• It is recommended to rename datums to make easier their selection by menu and the
understanding by other users.
Figure 2. Default datum planes
2.3.
Creating Parts
In this section, we will consider the best use of the sketcher and some critical aspects
of model part creation. The sketcher is the kernel of geometry creation in Pro/ENGINEER.
So, there are some critical aspects to take into account. These aspects have to do with the
definition of the sketch and orientation planes, and dimensions and alignments to existing
geometry. Making the wrong selection of any of the earlier aspects can strongly affect the
feature flexibility, parent/child relations and robustness. But you can make a good use of the
sketcher following the next recommendations.
• The use of a dimension scheme will make the sketch meaningful; as required on the
final drawing where shown dimensions can be used. You should also avoid
dimensioning to unrelated features and sketcher relations to make it more flexible
and independent.
• Keeping sketches simple will allow you to make operations such as modification and
regeneration (more simple sketches better than a complex one) easier. Even with
simple sketches you will reduce the risk of failure during modification. You also
can make sketches simple by creating the feature in a different way. Later, you can
make complex sketches from simple ones if you want.
• To align the sketch is very useful the 3D view to select alignment edges, especially
when they are coincident in 2D view. Be sure you do not create undesirable
relationships by choosing alignments, and you are recommended to use the preset
ones if you can.
• The rounds and chamfers creation is not advisable within sketcher. Their use make
hard their later suppression for analysis, may be difficult to modify the sketch
without affecting other features in the part and intersecting rounds may not behave
correctly.
The most important things to take into account when creating parts are the control of
parent/child relations, the control of the external references and the use of a dimension
scheme that represents the design intent. If you ignore these three aspects the part can become
inflexible and very hard to modify.
• For sketching planes the first choice should be the default datums unless this
conflicts with the design intent. Also the new datums should be related back to
principle datums to avoid stackup and undesirable relations. Do not create major
datums from part surfaces, but from default datums. Use datums planes to
reference features and avoid using small features such as fillets, holes, rounds, etc.
as references. If references other than datums must be used, reference features to
the fundamental geometry. This will avoid complex parent/child relations, which
create problems when these small features are suppressed or deleted for analysis.
• Regarding to the parent/child relations, you should avoid unnecessary and deep
ones, this will make easier to modify the part. To remove unwanted parent/child
relations use Reroute.
• Is very useful to name dimensions used in relations and comment relations for user
understanding.
• All the rounds and chamfers you need to create in the part should be added as late as
possible in the part model creation. This will reduce the risk of referencing
tangential edges and creating a feature that can not be suppressed.
You must suppress rounds and chamfers when additional features are created, to
avoid referencing them.
• Avoid nested features.
• After the creation of the feature name it for future use and introduce parametric
dimensions as relations, tolerances, etc. At this point you can add cosmetic
features, geometric dimensioning and tolerancing, notes and material parameters
as hardness, density, etc.
• Last task you should do (if you need it) is to organise features on layers.
2.4.
Layers
The use of a layer convention guide when a design is shared among several people is
very useful to allow people to get the control on the model visualisation without loosing time
looking for the layer structure, what can become very complex (see figure 3, for an example
of complex visualization). Layers allow to group items in the model tree so that operations
can be performed on them as a group.
Figure 3. Asembly with or without datum visualization
The configuration file ‘config.pro’ can define standard layer names, allowing to many
items of the design be automatically placed on those layers. The main suggestions we give to
work properly with layers in Pro/E are the following:
• The use of the standard layer names speeds up file management time. If no standard
layers name exist, you should chose easily recognisable names for other users to
understand the design as easy as possible.
• The use of standard layering to share data is an important key to get success in
Pro/E. Moreover, the mixture of files using layers and those not using layers
causes display problems, mainly in assembly mode.
• Developing a common ‘config.pro’ file for use across the site will enhance the
concurrency among users.
• The use of the primary display controls of layers, BLANK and DISPLAY, causes all
items on a selected layer to be “turned off” or to be shown just those items,
respectively. As the use of the two controls causes viewing problems, so our
recommendation is that you use BLANK control instead of DISPLAY control. If
same item is on more than one layer you may have to use DISPLAY to show one
or the other.
• You should move some features, as patterns for example, so they can be suppressed
for efficiency.
• For improved control you should move miscellaneous datums on their appropriate
layers.
• We suggest as well that you place cosmetic features in a particular layer because
they are placed automatically in a layer with some other items, and may be you
want to control them separately.
• All holes, rounds and chamfers should be placed on their appropriate layer to
suppress them for simplification for some analysis.
• The use of nested layers allows controlling several layers at one.
• To layer an item before suppressing it will allow you to resume only those you are
interested in by selecting the corresponding layer.
• To suppress several items of the model you can use a common layer to place them.
This reduce assembly lag time when some features do not need to be shown in the
assembly but are necessary, for example, in the detailing of the part.
3.
STRATEGIES TO ORGANIZE THE ASSEMBLIES
Some strategies are given at this point to avoid the more important critical aspects of
an assembly in Pro/ENGINEER. These aspects are the control of parent/child relations, the
control of the external references and the independence of the parts in an assembly. Ignoring
these three aspects can lead to interdependence among parts and assemblies, which can
prevent the reuse of engineering data. Some general recommendations are considered below
to carry out a proper use of the assemblies in Pro/ENGINEER.
• Avoid creating parts in assembly if possible. Otherwise, use reference viewer to
track external references and skeletons to carry shared references.
• Do not use coordinate systems for assembling cause this method is inflexible and
does not have any design intent.
• Use skeletons since they are means to share common geometry and to create a
framework for component positioning.
• Proper use of layers, allows controlling a complex assembly visualization.
4.
CONCLUSIONS
This paper presents an initial work about modelling methodology. Future development will
be available at our web site http://www.tec.uji.es including guidelines for assembly
management and integration with PDM systems. We have noticed that providing a modelling
methodology is very useful for people making the transition from classic “design-bydrawing” methodology to 3D parametric CAD. Most CAD vendors provide basic training
oriented to learning their systems modelling capabilities, forgiving the importance of a
correct modelling strategy. Many times, an implementation support is offered but with an
expensive additional cost. It is important remarking that there are many paths conducting to
the same geometric model, but only part of them provide a robust basement for downstream
applications like CAM and CAE software.
Changing from classic “design-by-drawing” methodology to a solid modelling one requires
a strong training plan. Many times, enterprises believe than buying modern workstations and
powerful software is enough to assure a successful transition. Both modelling skills and
modelling methodology training are as important as having the right hardware and software
tools.
ACKNOWLEDGEMENTS
The present paper has been realized as part of the research project under the financial
support of the Comisión Interministerial de Ciencia y Tecnología (CICYT) and the European
Comission (FEDER Programm) (Project 1FD97-0784, titled “Implantación de Tecnologías
Avanzadas de Diseño y Fabricación en el Ámbito de la Ingeniería Concurrente. Aplicación a
una Empresa de Componentes para Automoción”).
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