SolidWorks Surfacing and Complex Shape Modeling Bible

Part I

Laying the Groundwork

In This Part

Chapter 1 Understanding Basic Concepts

Chapter 2 Surfacing Primer

Chapter 1: Understanding Basic Concepts

In This Chapter

Assumed basic skills

Concepts, tools, techniques, and strategies

Understanding the difference between design and modeling

Everyone has a different idea of what the words basic and advanced mean. In general terms, some users might consider everything in this book advanced, and others might consider it basic. Still, in order to progress, the concepts have to start from somewhere, and so the initial concepts will form the basis for the more advanced material to come later.

SolidWorks probably has more surface and complex shape functionality than you realize, especially if you are coming to this book from a machine design background. Some of the tools are matured, having been available for quite some time, and some are newly added to the software, with some occasional kinks still left to work out.

Regardless of how you have arrived here, surfacing and complex shapes are areas of the SolidWorks software that have been flourishing in recent years, and improve with each new release of the software. Still, it is an area that doesn’t get as much traffic as, say, the extrudes, revolves and fillets, and so bugs, or quirky functionality, can still be found from time to time.

Figure 1.1 shows an example of some of the modeling that you will find in the pages of this book. This is a SolidWorks model of the SolidWorks Roadster, a Shelby Cobra kit car built by SolidWorks employees, and displayed at SolidWorks World 2007. This rendering was done by Matt Sass for the PhotoWorks contest on Rob Rodriguez’s site, www.robrodriguez.com.

Figure 1.1

Model of the SolidWorks Roadster

Rendering by Matt Sass

Assumed Basic Skills

The SolidWorks Surfacing and Complex Shape Modeling Bible is intended for a diverse cross-section of readers. The first type of reader is the SolidWorks user who is otherwise knowledgeable about the software, but wants to learn about surfacing and complex shape-creation techniques. This reader may have come from another type of design, and is more mechanical than artistic in method. The second is the user of another surfacing program who has learned SolidWorks basics and wants to transfer surfacing skills from the other program to SolidWorks. This reader is more likely an industrial designer or otherwise artistically inclined. This book assumes you already have a good grasp on the basics, such as sketching and sketch relations, the basics of parametric relations between features, and commonly used terminology in SolidWorks. The SolidWorks Bible can help bring you to this level, and is a great companion to this book for reference on the more basic concepts.

You will find a small amount of overlap between the current edition of the SolidWorks Bible and the SolidWorks Surfacing and Complex Shape Modeling Bible. The overlapping topics are splines and multi-body modeling. Both of these skills are essential to working with surfaces and complex shapes, which is why you find them again here, although discussed from a slightly different perspective.

This book was written using early versions of SolidWorks 2008, but most of the concepts discussed can be effectively applied to versions earlier and later. I have tried to make minimal references to version-specific aspects of the interface, but have pointed out where necessary the functional differences if any between features in prior versions.

Assemblies are only discussed in this book in a couple of areas, such as master modeling techniques and multi-body techniques. You will find no reference to any of the specialty techniques such as sheet metal or weldments.

Beyond that, a firm grasp of high school geometry concepts and terminology is necessary. Analytical geometry and simple calculus concepts come into play in the form of tangency, rate of change, and derivatives discussions. Because this book is primarily for actual users of the SolidWorks software, and actual users may or may not have an engineering math background, I will not involve any math or equations directly except for c = 1/r (curvature equals the inverse of radius).

You will find plastic-molded part terminology sprinkled throughout this book, with common references to parting lines, draft, and direction of pull. I have assumed that the reader has a passing familiarity with some form of plastic molding process such as thermoforming, injection molding, rotational molding, or blow molding. A background in metal injection molding, casting, or even forging may also be helpful, as many of the same concepts employed by these manufacturing techniques are also applicable to plastics processes.

Although you will not find drawings discussed in this book, basic mechanical drawing skills are required to get the most out of this book. You must understand basic terminology, such as section, projected view, and orthogonal views.

I intend this book to be primarily for the use of professional CAD operators, whether artist or technical, as opposed to casual or hobbyist users. If you are looking to make characters or equipment for games, SolidWorks may not be your best option. One of the polygonal modelers would be a better bet. Any type of casual user will probably find that complex shapes are easier to create in other software because, as CAD software, SolidWorks tends to require more precision than a tool like Maya or modo, or any of the freeware mesh modelers available.

Concepts, Tools, Techniques, and Strategies

The SolidWorks Surfacing and Complex Shape Modeling Bible is organized into four parts that discuss the concepts and tools (two sections are dedicated to the tools), and finally combine techniques and strategies into a series of longer hands-on model walk-throughs. I believe that this approach answers the how and why questions in addition to explaining and demonstrating what individual button clicks do. Tutorials on their own do not explain the decision-making process, but they do demonstrate the workflow. Lectures on their own do not demonstrate the tools in action. Concepts, of course, are useless without application to realistic scenarios.

Demonstrating techniques and strategies gives you, the reader, a head start with visualizing the application of the tools to real-world modeling scenarios. Most of the models used as examples have been adapted from real-world work projects, to keep them as realistic as possible. Techniques in particular will cover topics such as capping rounded ends, making blends at complex intersections, making sharp edges fade into smooth faces, how to use images as reference, how to deal with draft at the edges of complex surfaces, and many other commonly encountered situations.

Strategies refer to some of the bigger picture questions, like Where do I start? On a complex model, it is often difficult to know where to start. Also, if you need to make an assembly where the parts all contain an overall shape, how does modeling of that sort work? The model walk-through chapters in Part 4 answer these questions for you and are meant to spark your imagination to come up with new applications for the tools and techniques, and your own modeling strategies.

SolidWorks corporate documentation explains where to find the tools and generally what they do in the Help documentation. The official SolidWorks training materials offered by resellers are basically instructor-guided tutorials, which are valuable, but they stop short of arming the student with the ability to make modeling decisions based on thorough knowledge of the options. The training materials are also not generally available without paying for the reseller class.

You may also find tutorials on the Web that are either simplistic step-by-step instructions or heady and difficult to comprehend. Again, this book fills the gap between them and tries to do it in a more conversational language that conveys the necessary concepts without talking over your head or down to you.

In the course of talking about concepts, tools, techniques, and strategies, most of the individual topics are covered twice, or even three times from different angles. For example, the Fill surface is a tool that I discuss in Chapter 2 to illustrate the concept of trimmed surfaces, again in detail in Chapter 6, and again in multiple chapters of Part 3 as a practical application in tutorials.

As important as knowing positively what types of features work in which types of situations, it is also important to know the kinds of things that do not work the way you might expect. The purpose of talking about limited functionality is not to be derisive to the software or the parent company, but rather to offer the reader of this book as complete a picture as possible of the capabilities of the software. Often when using software, I have felt that if limitations were spelled out completely in the documentation, I could save a lot of time by avoiding figuring out the limitations for myself. In this book, I have made every attempt to be fair to the software, and if it works, I want to tell the story of how well it works and how to use it to its best advantage. On the other hand, if it doesn’t work as you might expect, I feel the obligation to do my readers the service of letting them know where the reliable limits of the software lie.

The point is that whether you use this book as a text to read straight through, or as a reference to look up topics as needed, I hope you find the information well presented and laid out logically. It is not possible to arrange all of the topics in sequential order.

Understanding the Difference Between Design and Modeling

The SolidWorks Surfacing and Complex Shape Modeling Bible, as the name suggests, focuses on modeling parts in SolidWorks with the purpose of manufacturing those parts. This is not a book about design. The act of modeling assumes that the design (or a starting place for the design) already exists. The design may exist in one of many forms. It could be sketched on paper, scanned into a digital image format, or modeled in clay or foam. It could be taken from a digital camera, the back of an envelope or napkin, or a whiteboard. It could already be drawn or modeled in a different 2D or 3D software, it could exist as a 3D point cloud from a 3D scanner, or it may simply exist only in your head. Wherever the design comes from, it probably exists somewhere else before it shows up in SolidWorks.

Dividing the tasks into design and modeling reflects the way that some companies divide their work force. Industrial designers often create a design in a given media, and modelers build a manufacturing model from the design data. There are some industrial design folks who can do their own manufacturing models, but this usually requires some form of engineering input. The modeler is often an engineer, or from a mechanical discipline in any case.

My background is as a mechanical engineer, and in my work as a consultant/contractor, I have often taken conceptual data from industrial designers and converted it to an engineering or manufacturing model. My point of view throughout this book will be just that: as an engineer re-creating or interpreting design data to prepare it for manufacturing. I avoid using the term design when what I am really talking about is simply modeling. While making the interpretations sometimes necessary in this kind of work, it is always important to remain sensitive to the original intent of the design. Other groups within an organization may also have some input into the design, such as branding established by marketing, stacking features introduced by shipping, material or finish costs driven by accounting, geometrical changes driven by molders, or structural changes made by mechanical engineers. Designs very rarely originate from only a single source. In this book, the design data is treated as if it is complete, and all that is required is the 3D CAD model.

In the course of this book, most of the modeling you will do centers around copying an existing form in one of the media mentioned above into a detailed model in SolidWorks. In some cases the models you finish will be ready for prototyping or manufacturing, and in others you will complete only a sampling of a certain technique.

In many of the tutorials in this book, the designer did not execute the provided design information perfectly. This is often also the case in the real world, where the designer creating two orthogonal views of a shape has drawn views that are incompatible with one another. In many cases, the modeler has to make subjective interpretations. I recommend consulting the original designer in cases when there is some discrepancy, but in situations of this sort encountered in this book, you will apply your own judgment to the model to fill in the gaps.

Summary

SolidWorks software is in many areas surprisingly full of powerful functionality to help you with your surfacing and complex shape modeling. This book will help you understand which functions are available, which to use in certain situations, and which to avoid through describing the underlying concepts at play with surfacing and complex shape modeling, the functions of specific individual tools and options, how the tools can be strung together into techniques, and how to plan out an overall strategy to accomplish your modeling goal efficiently.

You should also be clear that this is not a book about design in general. I do not cover how design should progress, the sources of design inspiration or design styles, but rather the details of creating 3D models with SolidWorks. The end goal in mind is creating models that are ready for manufacture or prototyping. Sample designs are presented in this book to be used as practice, creating 3D parametric models that update reliably through changes.

Chapter 2: Surfacing Primer

In This Chapter

What are surfaces?

Surfacing: One stop in the evolution of CAD

Choosing solids or surfaces

Surfacing theory and concepts

Understanding curvature continuity

Solid modeling has introduced an entire generation of engineers and designers to working in 3D. Today you can find younger users who have never drawn on the drawing board with a pencil and instruments, or even done much work in 2D CAD applications. Solid-modeling software takes the underlying power of surface modeling and automates its application to common types of mechanical geometry. In addition to modeling mechanical parts more quickly, this also allows many more people to gain entry into the world of 3D design because less specialized knowledge is required. Solid modeling removes many of the tedious modeling tasks that you would otherwise need to go through by using a surfacing approach.

SolidWorks users who are just beginning to venture into the use of surfacing techniques may find that a new world awaits them. Learning the concepts, tools, and language of the trade can initially be a daunting task, but one that ultimately pays off in many ways. This surfacing primer aims to introduce you to the things you need to know when using surfacing functions in SolidWorks.

What are Surfaces?

In the early days of automobiles, an integral part of knowing how to drive a car was knowing how to tinker with the engine. Modern design and manufacturing now allow us to drive a car without knowing how it works. These days you might still tinker with the engine if you want to improve the performance. Think of surfacing as tinkering with the engine with both goals in mind—troubleshooting the inner workings, and getting it to do things it otherwise would not have been able to do.

If up until now you have worked exclusively in solids, the use of surfaces may be a bit of an eye opener for you. If you are already a surfacing veteran from another CAD software, you may be surprised at some of the underlying power of SolidWorks for this type of work.

The answer to the question, what are surfaces? is that surfaces serve as the infinitely thin boundary of faces that encloses a solid. A solid could not exist without something to separate the inside from the outside. In the same way that endpoints are the boundaries of a line or edge, and edges form the boundary around a surface, surfaces are the boundary around a solid. So, surfaces are derived from two aspects—infinitely thin boundaries and stand-alone faces.

Infinitely thin

Although surfaces exist in 3D space, they do not take up any volume. They are infinitely thin, mathematically-represented skins. Even when a surface is a closed loop, such as the face of a cylinder, the surface itself does not have any thickness. Surface models in themselves cannot have the property of volume; volume is a property that only solids have. A surface can only have the property of area.

With the exception of a shape such as a sphere, more than one surface is usually required to enclose a volume. A single surface is usually but not always created by a single feature, and each new feature creates a body.

Working with bodies is an integral part of surface modeling. You can find information about the concept of bodies in Chapter 13

Stand-alone faces

Another way of thinking about surfaces is to think of them as stand-alone faces. When working with solid models, you are already familiar with the difference between the model and a face of the model. Surfaces can be thought of as a single face taken out of the context of the rest of the faces of the solid. Thinking of surfaces as stand-alone faces is probably conceptually better than thinking of surfaces as abstract infinitely thin boundaries, because it more closely reflects how practical surface features are used in real modeling.

When SolidWorks first added surfacing capabilities in SolidWorks 1997, the commands fell under the Reference Geometry header. In my view, this reflected how surfaces are used in real-world modeling. Surfaces are not an end to themselves, but are a means to create a finished solid model. Thinking of surfaces as reference geometry works well when combined with seeing them as stand-alone faces, because individual faces are of little use unless combined with other faces to make a complete solid model.

Surfacing: One Stop in the Evolution of CAD

Surfaces are one of the stops in the evolution of CAD. The practice of representing mechanical objects as lines on paper had been around for thousands of years, before the 2D process was replicated on a computer in the 1960s or thereabouts. From 2D computer representations, the state of the art moved to 3D wireframe, where sharp edges of objects were represented by lines in space. To represent the area between the edges of the wireframe, we started using surfaces. Wireframe models are sufficient to represent faces with curvature in only one direction but cannot fully describe more complex curvature. Representing this more complex curvature is really where the first necessity of 3D surface models came from.

Surface modeling represents the area between the wireframe edges in 3D space, giving even more information about a part that cannot be conveyed with a drawing in sand or on paper. One of the shortcomings of surface modeling, however, is that the model does not understand the inside from the outside, and does not guarantee that enough faces exist to fully represent an actual object. Taking this a step further created solid modeling, where the volume between the surfaces is represented. Solid modeling just turns out to be surface modeling with a lot of automated rules built into it, and so it makes sense to understand solids in terms of surfaces. The automation maintains the enclosed volume and the other solid aspects of the surface model.

Surfaces can be used in several different ways to achieve the end goal, which is usually to create a solid. One common method in which surfaces are used is to build a shape, face by face. Solid features build all of the faces needed to enclose a solid, all at the same time. However, this can be limiting sometimes because the shape that you need to build does not lend itself nicely to that method; adjacent faces may need to be created by using different feature types or techniques. In situations like this, surfaces are used to build a model one face at a time, and then knit the faces together into a single body.

Knitting is described in detail as a method for joining surface bodies in Chapter 11.

Another method for using surfaces is to deconstruct a solid into surfaces, then make changes to the surface body by removing, changing, adding, or replacing faces, and finally to knit the surface body back into a solid body.

A third method that is used frequently is to use surface bodies to alter the solid body directly. Solids may be cut with a surface, faces of the solid can be replaced with faces of a surface, or a surface can be used as an end condition for a solid using an Extrude Up To option. Modeling techniques that make use of both solid and surface geometry are often called hybrid modeling.

Hybrid modeling is described as combining solid and surface techniques in Chapter 10.

An example of using a surface as reference geometry would be copying a face of a solid early on in the feature tree, so that the whole face can be reused later after cuts, bosses, or fillets may have broken it up. Figure 2.1 shows an example of using surface geometry as reference geometry.

Figure 2.1

Using a surface as reference geometry

An example of using a surface as construction geometry would be to create a skirt surface around the parting line of a plastic part so that the faces of the part may be created with the appropriate draft on them. Figure 2.2 shows a ruled surface created as a skirt around a complex part, where it has been used as construction geometry.

The skirt technique is shown in Chapter 9.

Figure 2.2

Using a surface as construction geometry

In the end, your goal is usually to end up with a solid model.

Choosing Solids or Surfaces

Surface modeling is clearly a lot more work than solid modeling. Surface modeling forces you to work face by face, and faces must be manually fit together. These actions are all performed automatically in solid modeling. Where surfacing techniques become beneficial is in situations where solid modeling becomes clumsy or inefficient, or when a given modeling task is simply impossible with solids.

Assessing strengths and weaknesses

When learning surface modeling, it can be difficult to tell the difference between situations where surfacing should be used and where it is simply overkill. Learning to differentiate the strengths and weaknesses of the two methods is important.

One of the strengths of solids is prismatic shapes. A series of prismatic shapes is shown in Figure 2.3. Any shape that can be created with an extrude or revolve operation typically offers a great opportunity for using a solid feature. Solid features usually (although not always) produce shapes with flat-capped ends. In some situations this is a strength, while in others it can be considered a weakness. In the realm of creating complex, curvy models, it is usually seen as undesirable.

Figure 2.3

Examples of prismatic shapes

In the same way, the main strength of surfaces can also be described as its main weakness: Shapes and volumes can (or must, depending on your point of view) be created piece by piece. Although the can side of that statement offers additional capabilities by allowing you to build a model face by face and giving you ultimate control over the finished solid, the must side forces you into certain obligations, requiring you to work face by face, which can be a slow and tedious process. A common choice when working with surface model is control or speed.

How to choose

Sometimes, you don’t have to choose; you can use both solids and surfaces. You can choose a workflow that works exclusively in solids or surfaces, completely transforming your model from one to the other, or you can work with solids and surfaces at the same time.

The use of both solids and surfaces is often called hybrid modeling. Most of the mainstream CAD modeling tools available today fit into this category, such as SolidWorks, Solid Edge, Pro/ENGINEER, Unigraphics NX, and Catia. There are few modelers that use exclusively solids or surfaces. Rhino is an example of a surface-only modeler. Alibre is an example of a solid-only modeler.

Many people have told me that looking at SolidWorks as a hybrid modeler rather than just a solid modeler, and coming to grips with what surfacing brings to the table, has changed the way they approach almost every modeling task. Several of the examples that you see in this book are not complex shapes at all, but certainly benefit from surfacing techniques. By that I mean that surface modeling can be used for more than just complex shapes, but also for certain types of features on simple prismatic geometry.

Still, for many tasks, you must choose one method or the other. One sign that you are using solids when you should be using surfaces is when you find yourself drawing extra sketch lines that don’t actually create any geometry, or creating clumsy and awkward cuts to get rid of little bits of extra geometry. The sketch lines are still creating geometry, but it is geometry that is inefficiently swallowed up by other parts of the model.

Consider the model in Figure 2.4. The goal is to make a rectangular hole with a hemi-spherical bottom. This can be accomplished by using a combination of a cut-revolve and an extrude with the clumsy sketch as shown, or by simply cut-extruding to a hemi-spherical surface feature.

Figure 2.4

Extra sketch elements indicate a possible need for a surface technique

The reason that the extra sketch elements indicate the need for a different technique is that these extra lines actually create geometry. The way this works is that the shape is created as defined by the extrude feature as a separate body, and then that body is either joined to or subtracted from the main body, depending on the feature type. The processing time depends on the number of faces, the curvature of faces, and the types of features used to create the faces.

Much of this behind-the-scenes manipulation is taken care of by the Parasolid kernel, the geometry engine behind SolidWorks. The SolidWorks application turns out to be predominantly a user interface for the Parasolid kernel.

Another sign to indicate that you should be using surfaces is when you find yourself wanting a solid feature that could cut away part of the model created by another feature that ended awkwardly.

In the image of the coffee mug shown in Figure 2.5, notice that the handle breaks through to the inside of the mug when the handle is created. The use of surface features can avoid or repair this awkward geometry.

Figure 2.5

Surface functions can be used to avoid awkward modeling situations

A more efficient way to deal with cutting off this little extra nub of material is either to use a Cut with Surface tool using a memory surface, or to use the Delete Face tool.

The Cut with Surface and Delete Face tools are described in more detail in Chapters 10 and 12, respectively.

If you need to model a shape, and cannot identify a solid feature that enables you to create all of the faces at once, this may be another indication that you need some surface modeling.

It takes some practice, but after you have worked with a few techniques, you will begin to recognize models that you have already done where you could have benefited from surface techniques.

Surfacing is not just a set of esoteric functionality that is used by elitists who want to make things look more difficult than they really are. In some cases surfacing can actually save you a lot of work, and in other cases it simply makes something possible that otherwise would not be possible.

One of the little secrets about solids and surfaces is that geometrically, they are (or can be) identical. Also, when a solid model is translated into a neutral file format such as IGES, there is absolutely no difference between the solid model and a surface model. What it becomes when read by the second CAD system is completely up to that CAD system, as long as it follows the rules for solid models. Simply put, a solid model has certain requirements:

• The faces form a fully watertight boundary (no gaps or overlaps).

• It is composed of a single body.

• All of the face normals point the same direction (the inside is distinguished from the outside).

A face normal is a vector, or arrow, that points to one side of the face. Because faces can only have two sides, there are only two options for the direction of the arrow. For example, notice that if you use shaded planes in SolidWorks, one side of the plane is green and the other is red. Other than this, face and plane normals cannot be directly observed or manipulated in SolidWorks.

The watertight condition is more technically referred to as manifold. A surface body that does not meet the watertight condition is referred to as non-manifold. In this book I use the watertight terminology because it is a more intuitively understandable term, and due to the ambiguity that may be associated with various meanings of the word manifold. A model can be exported from one software as a surface and imported into another as a solid, and vice versa, as long as it meets the requirements. The only real difference is in how the modeling software treats the data. That needs to be said once more for emphasis. The only real difference between a solid and a surface model is how the modeling software treats it. They are otherwise geometrically identical.

Even in the SolidWorks import options, shown in Figure 2.6, you find the option to import IGES models as solids, knit surfaces, or un-knit surfaces.

To you, the user, this means that a solid model is really just a surface model where the software is automating many of the otherwise manual surfacing tasks that you would need to go through, and automatically maintains the conditions that define the solid. Features that cannot maintain those conditions result in model errors. Sometimes the conditions aren’t met due to the geometry-checking feature, allowing something to slip through the automated checking routines. This can in turn cause geometry errors that are unseen and yet may cause other features to fail.

Figure 2.6

SolidWorks import options enable you to choose between solids and surfaces.

Surfacing Theory and Concepts

Surface geometry breaks into several general categories, but this book is mainly concerned with two of them. Two of those types are called algebraic (sometimes referred to as analytical) and NURBS surfaces.

Algebraic and NURBS surfaces

Algebraic surfaces are defined by fairly simple mathematical expressions. In SolidWorks, this translates into shapes that can be created using lines and arcs in operations such as extrude and revolve. Planar, cylindrical, spherical, conical, toroidal, and other types of surfaces are examples of this type of geometry. Algebraic surfaces are attractive because they are fast for the software to calculate, they offer exactly predictable and perfectly extensible geometry, and certain types have special properties. Planar faces can be selected to sketch on, or used in other ways like reference planes. Cylindrical faces produce a temporary axis, and can be used for concentric mates in assemblies.

On the other hand, algebraic surfaces are limited in the types of shapes they can create, and in particular are not very useful when you want to build complex shapes. In product design, algebraic shapes are often avoided, and are often described using words like boxy or harsh.

The other type of geometry is referred to as NURBS surfaces. NURBS stands for non-uniform rational b-spline. NURBS is a method of using math to interpolate curves and surfaces between control points. In SolidWorks and many other CAD programs, NURBS is used to create shapes that fall outside of the algebraic regime, which is to say general complex shapes.

U-V isoparameter curves

NURBS works by interpolating a surface between curves in two roughly perpendicular directions. These curves are called the U-V isoparameters, which are roughly similar to the longitude and latitude lines on a globe. The term isoparameter simply means that the curves in the U direction lie along a fixed parameter of the V direction. When all of these curves are displayed, it looks like a grid. Figure 2.7 shows a Fill surface preview that displays these curves on the surface being created.

Figure 2.7

U-V isoparameter curves shown in a Fill surface preview

The Fill surface is described in more detail in Chapter 6.

The U and the V stand for the two directions of the grid—where one direction is called U and the other is called V. Positions along the U and V directions are called the parameter of the curve, and range from 0 to 1. The curve shown in Figure 2.8 is on the .5 isoparameter of the V direction.

The U-V isoparameter curves for any face can be seen by using the Face Curves tool on the Sketch toolbar. Understanding the orientation of the U-V grid of the existing faces can be instrumental in fitting other surfaces to closely match the existing faces.

You don’t need to know any of this in order to simply run the software, but knowledge of the inner workings can often help you troubleshoot features that are not working as you might expect.

Figure 2.8

Curve at the .5 isoparameter of the V direction

Transitions between surfaces are discussed in more detail in the chapters of Part 4, in particular Chapters 18 and 19. Face Curves are described in more detail in Chapters 4 and 14.

The degenerate condition

One of the implications of creating surfaces from a grid of curves in perpendicular directions is that the resulting surfaces have the tendency to be four-sided. This is in fact a common limitation of NURBS that CAD designers and programmers struggle against. Because it is a NURBS limitation, it affects all CAD programs that use NURBS, not just SolidWorks.

In reality, though, surfaces come in all shapes, including shapes that are not four-sided. One option for creating non-four-sided surfaces is to use trimmed surfaces, which are discussed later in this chapter. Another way is to collapse all of the U-V lines on one side into a single point. When this happens, that side of the four-sided patch is said to be a zero-length side. Zero-length sides are called degenerate, or it may be said to contain a singularity. Fillet features commonly create geometry of this type, as shown in Figure 2.9, where you can see what happens to the U-V grid when faces of 3, 2, or even zero are created.

The problem with degenerate faces is the number zero. Mathematics and computers have difficulty with the number zero, and of course these surfaces are made using both. Degeneracies may cause features such as shells, fillets, offsets, scales, or moves to fail because the surrounding geometry cannot deal with the singularity. Sometimes in SolidWorks, you can identify degenerate faces visually, without showing the face mesh because there is an odd discoloration or shading at or near the singularity.

Recent versions of SolidWorks have become much better at handling degeneracies, but they still can cause problems.

Figure 2.9

Degenerate faces

An example of working past degeneracies is shown in Chapter 16, as a part of capping off a handle.

Trimmed surfaces

Surfaces want to be four-sided, but they are sometimes forced into other shapes. Surfaces that must be some other shape have one of two options: degenerate condition or trimmed surfaces. Trimmed surfaces are the preferable choice, because of the problems I have just outlined with degenerate surfaces.

Understanding the B-rep

Trimmed surfaces offer a lot of advantages. Essentially, trimmed surfaces are composed of two elements: the underlying surface and some definition of its boundary. This combination of surface and boundary is sometimes referred to as the boundary representation, or b-rep.

A working understanding of the b-rep is important for three reasons. First, when building surfaces, it is common practice to overbuild the surface (meaning to make it bigger than it needs to be), and then to trim it back to fit. This is a technique unique to working with surfaces that is not used with solid modeling. Many reasons exist for using this technique. A surface that is too small is difficult to work with, but a surface that is too large, once trimmed, is never a problem. Also, making a surface larger than it needs to be helps to prevent extra edges from showing up in the model. The one thing that gives SolidWorks surfacing users the most problems is building smooth transitions between faces and across edges. The best way to eliminate this difficulty is to eliminate the edges as much as possible.

One of the best ways to visualize trimmed surfaces in action is to observe the Fill surface. The Fill surface builds a four-sided patch, fits it into whatever shaped gap is to be filled, and then trims the surface to fit the gap. The situations in which this tool works are sometimes amazing. Figure 2.10 shows the Fill surface automatically overbuilding a surface that will be trimmed back when the feature is accepted.