CHAPTER 7

Modeling with Primary Features

The most frustrating part of a complex modeling job is to be able to envision a result, but not be able to create it because you do not have the tools to get it done. Worse yet is to actually have the tools but either not understand how to use them or not even realize that you have them. Getting the job done is so much more satisfying when you use the right tools and get the job done right — not just so that it looks right, but so that it really is right.

SolidWorks offers so many tools that it is sometimes difficult to select the best one, especially if it is for a function that you do not use frequently.

This chapter helps you identify which features to use in which situations, and in some cases, which features to avoid. It also helps you evaluate which feature is best to use for a particular job. With some features, it is clear when to use them, but for others, it is not. This chapter guides you through the decision-making process.

I have split the list of SolidWorks features into two groups: primary features and secondary features. Primary features are, of course, the ones you use most frequently, and secondary features are used less frequently. Of course, my definition of primary and secondary may be different from yours, and this subject is too big for a single chapter.

Identifying When to Use Which Tool

I am always trying to think of alternate ways of doing things. It is important to have a backup plan, or sometimes multiple backup plans, in case a feature doesn't perform exactly the way you want it to. You may find that the more complex features are not as well behaved as the simple features. You may be able to get away with only doing blind extrudes and cuts with simple chamfers and fillets for the rest of your career, but, even if you could, would you really want to?

As an exercise, I often try to see how many different ways a particular shape might be modeled, and how each modeling method relates to manufacturing methods, costs, editability, efficiency, and so on. You may also want to try this approach for fun or for education.

As SolidWorks grows more and more complex, and the feature count increases with every release, understanding how the features work and how to select the best tool for the job becomes ever more important. If you are only familiar with the standard half-dozen or so features that most users use, your options are limited. Sometimes simple features truly are the correct ones to use, but using them because they are the only things you know is not always the best choice.

Using the Extrude feature

Extruded features can be grouped into several categories, with extruded Boss and Cut features at the highest level. When you use Instant 3D, extruded bosses can be transformed into cuts by simply dragging them with the Instant 3D handle in the other direction. It is unclear what advantage this has in real-world modeling, but it is an available option. As a result, the names of newly created extrude features are simply Extrude1 where they used to be Extrude-Boss1 or Extrude-Cut1.

The “Base” part of the Extruded Boss/Base is a holdover from when SolidWorks did not allow multi-body parts, and the first feature in a part had special significance that it no longer has. This is also seen in the menus at Insert Boss/Base. The Base feature was the first solid feature in the FeatureManager, and you could not change it without deleting the rest of the features. The introduction of multi-body support in SolidWorks has removed this limitation.

Creating a solid feature

In this case, the term solid feature is used as an opposite of thin feature. This is the simple type of feature that you create by default when you extrude a closed loop sketch. A closed loop sketch fully encloses an area without gaps or overlaps at the sketch entity endpoints. Figure 7.1 shows a closed loop sketch creating an extruded solid feature. This is the default type of geometry for closed loop sketches.

Creating a thin feature

The Thin Feature option is available in several features, but is most commonly used with Extruded Boss features. Thin features are created by default when you use open loop sketches, but you can also select the Thin Feature option for closed loop sketches. Thin features are commonly used for ribs, thin walls, hollow bosses, and many other types of features that are common to plastic parts, castings, or sheet metal.

Even experienced users tend to forget that thin features are not just for bosses, but that they can also be used for cuts. For example, you can easily create grooves and slots with thin feature cuts.

Figure 7.2 shows the Thin Feature panel in the Extruded Boss PropertyManager. In addition to the default options that are available for the extrude feature, the Thin feature adds a thickness dimension, as well as three options to direct the thickness relative to the sketch: One-Direction, Mid-Plane, and Two-Direction. The Two-Direction option requires two dimensions, as shown in Figure 7.2.

FIGURE 7.1 A closed loop sketch and an extruded solid feature

FIGURE 7.2 The Thin Feature portion of the Extrude PropertyManager

You can create the simplest cube from a single sketch line and a thin feature extrude. However, because they are more specialized in some respects, thin features may not be as flexible when the design intent changes. For example, if a part is going to change from a constant width to a tapered or stepped shape, thin features do not handle this kind of change. Figure 7.3 shows different types of geometry that are typically created from thin features.

Exploring sketch types

You may see the words loop, contour, region, and profile used interchangeably in various areas of the software. In this book I try to standardize some of the more confusing terminology, but in this case, each of the four terms tends to be used in different situations.

FIGURE 7.3 Different types of geometry created from thin feature extrudes

A loop is a selection of edges or sketch entities that touch end-to-end without gaps or overlaps. A contour can mean the same thing as a loop or it may also mean an area enclosed by a loop of sketch entities that may not meet the “touch end-to-end without gaps or overlaps” part of the definition. Contours can also refer to an enclosed area selected for a feature such as an extrude or revolve, as you will see later in this chapter. A region is typically the same thing as a contour, but the term is only found in error messages and is probably nonstandard terminology left over from previous versions of SolidWorks. Technically, a profile is only found in a loft or sweep feature, but various sources of documentation might use it to refer to any sketch or selection of entities that are used to create a feature.

I have already mentioned several sketch types, including closed loop and open loop. Closed loop sketches make solid features by default, but you can also use them to make thin features. Open loop sketches make thin features by default, and you cannot use them to make solid features. A nested loop is one closed loop inside another, like concentric circles. Self-intersecting sketches can be any type of sketch where the geometry crosses itself. SolidWorks also identifies sketches where three or more sketch elements intersect at a point by issuing an error if you try to use the sketch in a feature. Figure 7.4 illustrates these different types of sketches. Some of these examples are errors and some are just warnings.

FIGURE 7.4 Identifying different types of sketches in SolidWorks

Sketch contours

Sketch contours enable you to select enclosed areas where the sketch entities themselves actually cross or otherwise violate the usual sketch rules. One of these conditions is the self-intersecting contour.

There are several types of contour selection, as shown in Figure 7.5.

3D sketch

You can make extrusions from 3D sketches, even 3D sketches that are not planar. While not necessarily the best way to do extrudes, this is a method that you can use when needed. You can establish direction for an extrusion by selecting a plane (normal direction), axis, sketch line, or model edge.

When you make an extrusion from a 3D sketch, the direction of extrusion cannot be assumed or inferred from anything — it must be explicitly identified. The default extrusion direction from a 2D sketch is always perpendicular to the sketch plane unless otherwise specified.

Non-planar sketches become somewhat problematic when you are creating the final extruded feature. The biggest problem is how you cap the ends. Figure 7.6 shows a non-planar 3D sketch that is being extruded. Notice that the end faces are, by necessity, not planar, and are capped by an unpredictable method, probably a simple Fill surface. This is a problem only if your part is going to use these faces in the end; if it does not, then there may be no issue with using this technique. If you would like to examine this part, it is included on the DVD as Chapter 7 Extrude 3D Sketch.sldprt.

FIGURE 7.5 Types of contour selection

FIGURE 7.6 Extruding a non-planar 3D sketch

If you need to have end faces with a specific shape, and you still want to extrude from a non-planar 3D sketch, then you should use an extruded surface feature rather than an extruded solid feature.

One big advantage of using a 3D sketch to extrude from is that you can include profiles on many different levels, although they must all have the same end condition. Therefore, if you have several pockets in a plate, you can draw the profile for each pocket at the bottom of the pocket using planes offset at different levels, and extrude all the profiles Through All; as a result, they will all be cut to different depths.

Three-dimensional sketches also have an advantage when all the profiles of a single loft or boundary are made in a single 3D sketch. This enables you to drag the profiles and watch the loft update in real time.

Understanding the workflow

The Extrude feature workflow offers several options:

1. From within an active sketch with appropriate geometry, click the Extrude toolbar icon.
2. Set the Extrude feature options.
3. Click OK.

Or:

1. With no sketch active, click the Extrude toolbar icon.
2. Select an existing sketch with appropriate geometry.
3. Set the Extrude feature options.
4. Click OK.

Or:

1. With no sketch active, click the Extrude toolbar icon.
2. Select a plane on which to create a sketch to extrude.
3. Create your sketch.
4. Exit the sketch using the Confirmation Corner icon.
5. Set the Extrude feature options.
6. Click OK.

Understanding Instant 3D

Instant 3D is the tool that enables you to use the mouse to pull arrows or handles on the screen to establish various dimension parameters for features like extrude, revolve, fillet, and even move face. Not every dimension feature parameter is editable in this way. In some cases Instant 3D offers you convenient ways to edit geometry without needing to figure out which feature is responsible for which faces. With Instant 3D, you simply pull on handles on the screen to move and resize sketches, and features including fillets.

Creating extrudes with Instant 3D

Instant 3D enables you to select a sketch or a sketch contour and drag the Instant 3D arrow to create either a blind extruded boss or cut. The workflow when using this function requires that the sketch be closed. Instant 3D cannot be used to create a thin feature, and any sketch or contour that it uses must be a closed loop. Sketches must also be shown (not hidden) in order to be used with Instant 3D.

Figure 7.7 shows Instant 3D arrows for extruding a sketch into a solid and the ruler to establish blind extrusion depth. These extrusions were done from a single sketch with three concentric circles, using contour selection.

FIGURE 7.7 Identifying Instant 3D interface elements

Even after you create an extruded boss, you can use Instant 3D to drag it in the other direction to change the boss into an extruded cut. When you do this, the symbol on the feature changes, but the name does not.

If you have a sketch that requires contour selection, SolidWorks automatically hides the sketch, and to continue with Instant 3D functionality using additional contours selected from that sketch, you will have to show the sketch again. This interrupts the workflow and makes using this functionality less fluid than it might otherwise be. I only mention it here so that you are aware of what is happening when the sketch disappears and the Instant 3D functionality disappears with it.

You can also continue to create extrudes using contours of a consumed sketch by just clicking on the sketch so that it displays highlighted, and is only shown temporarily. This is a shortcut so that you don't have to repeatedly show the sketch every time — you just select it.

If geometry already exists in the part, and you drag a new feature into the existing solid, SolidWorks assumes you want to make a cut. However, maybe you are really trying to make a boss that comes out the other side of the part. These context toolbars enable you to do this. Options include boss, cut, and draft. The draft option enables you to add draft to a feature created with Instant 3D.

While Instant 3D can only create extruded bosses and cuts, it can edit revolves. If you create a revolved feature revolving the sketch, say, 270°, the face created at the angle can be edited by Instant 3D dragging. You can also drag faces created by any under-defined sketch elements.

Editing geometry with Instant 3D

Instant 3D enables you to edit 2D sketches and solid geometry. You can also edit some additional feature types using Instant 3D, such as offset reference planes. It can neither create nor edit surface geometry or 3D sketches in some situations. To edit solid geometry, click a face, and an arrow appears. Drag the arrow, and SolidWorks automatically changes either the sketch or the feature end condition used to create that face. If a dimensioned sketch was used to create that face, SolidWorks will not allow you to use the Instant 3D arrow to move or resize the face. An option exists that enables Instant 3D changes to override sketch dimensions at Tools Sketch Settings Override Dims on Drag.

Instant 3D offers different editing options depending on how a sketch is selected.

• A sketch is selected from the graphics window. The pull arrow appears, enabling you to create an extruded boss or cut.
• A sketch is selected from the FeatureManager. If the sketch has relations to anything outside of the sketch, the sketch is highlighted with no special functionality available. If no external relations exist, a box with stretch handles enable scaling the sketch, and a set of axes with a wing enables you to move the sketch in X or Y or X and Y. Figure 7.8 shows this situation.

When Instant 3D is activated, double-clicking a sketch in either the FeatureManager or on a sketch element in the graphics window opens that sketch. While you are in a sketch, if you double-click with the Select cursor in blank space in the graphics window, you close the sketch. This only works for 2D sketches; 3D sketches can be opened, but not closed, this way.

FIGURE 7.8 Sketch scaling and moving options with Instant 3D.

Working with the Revolve feature

Like all other features, revolve features have some rules that you must observe when choosing sketches to create a revolve:

• Draw only half of the revolve profile. (Draw the section to one side of the centerline.)
• The profile must not cross the centerline.
• The profile must not touch the centerline at a single point. It can touch along a line, but not at a point. Revolving a sketch that touched the centerline at a single point would create a point of zero thickness in the part.

You can use any type of line or model edge for the centerline, not just the centerline/construction line type.

Understanding end conditions

There are five Revolve end conditions. Some of the following options are new in SolidWorks 2011:

• Blind
• Up to Vertex
• Up to Surface
• Offset from Surface
• Midplane

There is no equivalent for Up to Next or Up to Body with the Revolve feature. Figure 7.9 shows the new Revolve feature PropertyManager for SolidWorks 2011.

FIGURE 7.9 Using the Revolve PropertyManager in SolidWorks 2011

SolidWorks 2011 changes the way that you create two-direction revolves. The options in the end conditions list used to be One Direction, Two Directions, or Midplane. Starting in 2011 the end conditions for revolve are more similar to the end conditions for extrude, with the five options listed for revolve, and controls for separate directions.

Workflow

The workflow for the Revolve feature is exactly the same as for the Extrude feature.

Using contour selection

Like extrude features, revolve features can also use contour selection; and as with the extrude features, I recommend that you avoid using contours for production work.

Introducing loft and boundary

Loft and boundary are known as interpolated features. That means that you can create profiles for the feature at certain points, and the software will interpolate the shape between the profiles. You can use additional controls with loft, such as guide curves or centerlines, and establish end conditions to help direct the shape. A loft with just two profiles is a straight line transition. If you have more than two profiles, the transition from one profile to another works more like a spline.

Many users struggle when faced with the option to create a loft, boundary, or sweep. Some overlap exists between the three features, but as you gain some experience, it becomes easier to choose between them. Generally, if you can create the cross-section of the feature by manipulating the dimensions of a single sketch, a sweep might be the best feature. If the cross-section changes character or severely changes shape, loft or boundary may be best. If you need a very definite shape at both ends and/or in the middle, loft and boundary are better choices because they enable you to explicitly define the cross-section at any point. However, if the outline is more important than the cross-section, you should choose a sweep. In addition, if the path between ends is important, choose a sweep.

Both types of features are extremely powerful, but the sweep has a tendency to be fussier about details, setup, and rules, while the loft and boundary can be surprisingly flexible. I am not trying to dissuade you from using sweeps, because they are useful in many situations. However, in my own personal modeling, I probably use about ten lofts or boundary features for every sweep. For example, while you would use a loft or combination of loft features to create the outer faces of a complex laundry detergent bottle, you would use the sweep to create a raised border around the label area or the cap thread.

A good example of the interpolated nature of a loft is to put a circle on one plane and a rectangle on an offset plane and then loft them together. This arrangement is shown in Figure 7.10. The transition between shapes is the defining characteristic of a loft, and is the reason for choosing a loft instead of another feature type. Lofts can create both Boss features and Cut features.

FIGURE 7.10 Interpolation inside a loft

Notice how the cross-sectional shape of the loft transitions from the circle to the rectangle. The default setting, shown in Figure 7.10, is for the interpolated transition to happen evenly across the loft, but the distribution of change from one end to the other could be altered, which might result in the transitions shown in Figure 7.11.

FIGURE 7.11 Adding end conditions to a loft alters how the interpolation is distributed.

Both shapes are two-profile lofts. The two-profile loft with default end conditions always creates a straight transition, which is shown in the image to the left. A two-point spline with no end tangency creates a straight line in exactly the same way. By applying end conditions to either or both of the loft profiles, the loft's shape is made more interesting, as seen in the image to the right in Figure 7.11. Again, the same thing happens when applying end tangency conditions to a two-point spline: it goes from being a straight line to being more curvaceous, with continuously variable curvature.

The Loft PropertyManager interface is shown in Figure 7.12.

FIGURE 7.12 The Loft PropertyManager

Comparing the Loft and Boundary features

The Boundary feature is relatively new to SolidWorks. The Boundary surface feature was added first, and was a big hit in surfacing applications, so boundary solid was added later. In my view, the solid feature is not as effective as the surface feature, and solid loft probably offers fewer advantages over boundary than surface loft does. Chapter 20 has more information on the surfacing functionality.

An important difference between boundary and loft is that there are more options for setting up boundary features in terms of the geometrical layout of profiles and guide curves. A second major difference is that there is no such thing in boundary as profiles and guide curves — the two directions are treated equally, and are simply called Direction 1 and Direction 2. In the Loft feature, you don't have as much continuity control across the guide curve direction. This is less meaningful with solid features than with surfaces.

The geometrical layout of profiles is the most important difference between boundary and loft. With loft, you must have a profile at the beginning and end of the feature. With boundary, you can lay out the profile sketch planes like an X. You could also lay the feature out like a T, which would act like a sweep. Using a layout shaped like an F actually combines the functionality of a loft with that of a sweep. So boundary is a very powerful feature, with new options for creating interpolated solid shapes. Face-by-face control, however, still has to come from using surfacing features.

Figure 7.13 shows the boundary PropertyManager and features made with F and X layouts of sketches. These two features represent functionality that doesn't exist with the Loft feature.

FIGURE 7.13 Using different profile arrangements for boundary solid features

Using entities in a loft

For solid lofts, you can select faces, closed loop 2D or 3D sketches, and surface bodies. You can use sketch points as a profile on the end of a loft that comes to a point or rounded end. For surface lofts, you can use open sketches and edges in addition to the entities that are used by solid lofts, but you cannot combine open and closed contours.

Some special functionality becomes available to you if you put all the profiles and guide curves together in a single 3D sketch. In order to select profiles made in this way, you must use the SelectionManager, which is discussed later in this chapter.

The Sketch Tools panel of the Loft PropertyManager enables you to drag sketch entities of any profile made in this way while you are editing or creating the Loft feature, without needing to exit and edit a sketch.

Comparing lofts and splines

The words loft and spline come from the shipbuilding trade. The word spline is actually defined as the slats of wood that cover the ship, and the spars of the hull very much resemble loft sections. With the splines or slats bending at each spar, it is easy to see how the modern CAD analogy came to be.

Lofts and splines are also governed by similar mathematics. You have seen how the two-point spline and two-profile loft both create a straight-line transition. Next, a third profile is added to the loft and a third point to the spline, which demonstrates how the math that governs splines and lofts is also related to bending in elastic materials. Figure 7.14 shows how lofts and splines react geometrically in the same way that bending a flexible steel rod would react (except that the spline and the loft do not have a fixed length).

FIGURE 7.14 Splines, lofts, and bending

With this bit of background, it is time to move forward and talk about a few of the major aspects of loft features in SolidWorks. It is possible to write a separate book that only discusses modeling lofts and other complex shapes. This has in fact been done. The SolidWorks Surfacing and Complex Shape Modeling Bible (Wiley, 2008) covers a wide range of surfacing topics with detailed examples. In this single chapter, I do not have the space to cover the topic exhaustively, but coverage of the major concepts will be enough to point you in the right direction.

Understanding the need for surfaces

In this chapter, I deal exclusively with solid modeling techniques because they are the baseline that SolidWorks users use most frequently. Surfaces make it easier to discuss complex shape concepts because surfaces are generally created one face at a time, rather than by using the solid modeling method that creates as many faces as necessary to enclose a volume.

From the very beginning, the SolidWorks modeling culture has made things easier for users by taking care of many of the details in the background. This is because solids are built through automated surface techniques. Surface modeling in itself can be tedious work because of all the manual detail that you must add. Solid modeling as we know it is simply an evolutionary step that adds automation to surface modeling. The automation maintains a closed boundary of surfaces around the solid volume.

Because surfaces are the underlying building blocks from which solids are made, it would make sense to teach surfaces first, and then solids. However, the majority of SolidWorks users never use surfacing, and do not see a need for it; therefore, surface functions are generally given a lower priority.

Exploring loft end constraints

Loft end conditions control the tangency direction and weighting at the ends of the loft. Some of the end constraints depend upon the loft starting or ending from other geometry. The optional constraints are covered in the following sections.

None

The direction of the loft is not set by the None end constraint, but the curvature of the lofted faces at the ends is zero. This is the default end constraint for two-section lofts. This means that at the ends of the loft using the None end constraint, the loft has no curvature, and is tangent to some direction controlled by the location of the previous profile.

Default

The Default end constraint is not available for two-section lofts, only for lofts with three or more sections. This end constraint applies curvature to the end of the loft so that it approximates a parabola being formed through the first and last loft profiles.

Tangent to Face

The Tangent to Face end constraint is self-explanatory. The Tangency to Face option includes a setting for tangent length. This is not a literal length dimension, but a relative weighting, on a scale from 0.1 to 10. The small arrow to the left of the setting identifies the direction of the tangency. Usually, the default setting is correct, but there are times when SolidWorks misidentifies the intended tangency direction, and you may need to correct it manually.

The Next Face option is available only when lofting from an end face where the tangency could go in one of two perpendicular directions. This is shown in Figure 7.15.

Apply to All refers to applying the Tangent Length value to all the tangency-weighting arrows for the selected profile. When you select Apply to All, only one arrow displays. When you deselect it, one arrow should display for each vertex in the profile, and you can adjust each arrow individually.

Curvature to Face

The difference between tangency and curvature is that tangency is only concerned with the direction of curvature immediately at the edge between the two surfaces. Curvature must be tangent and match the radius of curvature on either side of the edge between surfaces. This is often given many names, including curvature continuity and c2 or g2. Lofted surfaces do not usually have a constant radius; because they are like splines, they are constantly changing in local radius.

Direction Vector

The Direction Vector end constraint forces the loft to be tangent to a direction that you define by selecting an axis, edge, or sketch entity. The angle setting makes the loft deviate from the direction vector, as shown in Figure 7.15. The curved arrows to the left identify the direction in which the angle deviation is going.

FIGURE 7.15 Examples of end constraints

Displaying isoparameter U-V lines

The mesh or grid shown in the previous images appears automatically for certain types of features, including lofts. The grid represents isoparameter lines, also known as NURBS mesh or U-V lines. This mesh shows the underlying structure of the faces being created by the feature. If the mesh is highly distorted and appears to overlap in places, then it is likely that the feature will fail.

You can show or hide the mesh through the right mouse button (RMB) menu when editing or creating a Loft feature, unless the SelectionManager is active. In this case, you can see only SelectionManager commands in the RMB menu. In addition, planar faces do not mesh, only faces with some curvature.

Using guide curves

Guide curves help to constrain the outline of a loft between loft profiles. Although it is best to try to achieve the shape you want by using appropriately shaped and placed loft profiles, this is not always possible. The most appropriate use of guide curves for solid lofts is at places where the loft is going to create a hard edge, which is usually at the corners of loft profile sketches. Guide curves often (but not always) break up what would otherwise be a smooth surface, and you should avoid them in these situations, if possible.

Although guide curves can be longer than the loft, they can not be shorter. The guide curve applies to the entire loft. If you need to apply the guide curve only to a portion of the loft, then split the loft into two lofts: one that uses the guide curve and one that does not. The guide curve must intersect all profiles in a loft.

If you have more than one guide curve, the order in which they are listed in the box is important. The first guide curve helps to position the intermediate profiles of the loft. It may be difficult to visualize the effects of guide-curve order before it happens, but remember that it does make a difference, and depending on the difference between the curves, the difference may or may not be subtle.

Guide curves are also used in sweeps, which I address later in this chapter. Figure 7.16 shows a model that is lofted using guide curves. The image to the left shows the sketches that are used to make the part. There are two sketches with points; you can use points as loft profiles. The image in the middle shows the Loft feature without guide curves, and the one to the right is the part with guide curves. If you would like to examine how this part is built, you can find it on the DVD with the filename Chapter 7 Guide Curves.sldprt.

FIGURE 7.16 A loft with and without guide curves

Using centerline lofts

The Centerline panel of the Loft PropertyManager is used to set up a centerline loft. You can use the centerline of a loft in roughly the same way that you use a sweep path. In fact, the Centerline loft resembles a sweep feature where you can specify the shape of some of the intermediate profiles. Centerline lofts can also create intermediate profiles. You may prefer to use a centerline loft instead of either a sweep or a regular loft because the profile may change in ways that the Sweep feature cannot handle, and the loft may need some guidance regarding the order of the profiles, or how to smooth the shape between the profiles. While most of the functionality you find in the Loft feature can be duplicated and improved upon by the Boundary solid feature, the Boundary feature cannot do anything like the Centerline loft.

I cover sweep features in this chapter. If you are creating a centerline loft, you may want to examine the sweep functionality as well.

You can use centerlines simultaneously with guide curves. While guide curves must touch the profile, there is no such requirement for a centerline; in fact, the centerline works best if it does not touch any of the profiles.

The slider in the Centerline Parameters panel enables you to specify how many intermediate sections to create between sketched profiles.

Using the SelectionManager

The SelectionManager simplifies the selection of entities from complex sketches that are not necessarily the clean, closed loop sketches that SolidWorks works with most effectively.

The SelectionManager has been implemented in a limited number of features. Selection options in the SelectionManager include the following:

• OK. Accepts the selection. This feature is also available on the RMB menu.
• Cancel. Quits the SelectionManager.
• Clear All. Clears the current selection set.
• Push Pin. Keeps the SmartSelection window available, even when it is not required for sketch entity selections.
• Select Closed Loop. You can select two different types of loops with this tool:
  • A parametric closed loop in a 2D or 3D sketch
  • A parametric loop of edges around a surface
• Select Open Loop. Selects a chain (end-to-end sketch entities).
• Select Group. Selects entities individually. If you click the Propagate symbol, all tangent edges are selected.
• Select Region. Works like the Contour Selection described earlier in this chapter.
• Standard Selection. Disables special functions of the SelectionManager. This feature works like a regular selection tool.
• Auto OK Selections. Becomes enabled when you use the Push Pin. Auto OK Selections works for closed and open loop selection.

Choosing loft options

You can choose from the following Loft options, as shown in Figure 7.17:

FIGURE 7.17 Loft options

• Merge tangent faces. Merges model faces that are tangent into a single face. This is done behind the scenes by converting profiles into splines, which make approximations but are smoother than sketches with individual tangent line and arc entities.
• Close loft. The loft is made into a closed loop. At least three loft profiles must exist in order to use this option. Figure 7.18 shows a loft where the Close Loft option is used, and the loft sections are shown. This model is on the DVD with the filename Chapter 7 — Closed Loft.sldprt.

  FIGURE 7.18 A closed loft

  

• Show preview. Selecting and deselecting this option turns the preview of the Loft feature on or off, respectively, if the feature is going to work. All the following loft preview options are system options and remain selected until you deselect them.
  • Transparent/Opaque Preview is available from the RMB menu when you edit a loft, if the SelectionManager is not active.
  • Mesh Preview is also available on the same RMB menu.
  • Zebra Stripe Preview is also available on the same RMB menu, and is covered in more depth in Chapter 12.
• Merge result. Merges the resulting solid body with any other solid bodies that it may contact.

Workflow

The workflow for the Loft feature is as follows:

1. Create or have available a set of profiles, including sketches or faces. All sketches must be closed loop and not active.
2. Select profiles and guide curves as necessary.
3. Select the required options as the situation requires.
4. Click OK to accept the feature.

Controlling Sweep features

The Sweep feature uses multiple sketches. A sweep is made from a profile (cross-section) and a path, and can create a boss or a cut feature. If you want, you can also use guide curves. Sweeps can run the gamut from simple to complex. Typical simple sweeps are used to create wire, tubing, or hose. Sweeps that are more complex are used for creating objects such as bottles, involutes, springs, and corkscrews.

The main criteria for selecting a sweep to create a feature are that you must be able to identify a cross-section and a path. The profile (cross-section) can change along the path, but the overall shape must remain the same. The profile is typically perpendicular to the path, although this is not a requirement.

Using a simple sweep

An example of a simple sweep is shown in Figure 7.19. The paper clip uses a circle as the profile and the coiled lines and arcs as the path.

FIGURE 7.19 The sweep profile follows the path.

Using a sweep with guide curves

Sweeps that are more complex begin to control the size, orientation, and position of the cross-section as it travels through the sweep. When you use a guide curve, several analogies can be used to visualize how the sweep works. The cross-section/profile is solved at several intermediate positions along the path. If the guide curve does not follow the path, the difference between the two is made up by adjusting the profile. Consider the following example. In this case, the profile is an ellipse, the path is a straight line, and there are guide curves that give the feature its outer shape. Figure 7.20 shows all these elements and the finished feature.

FIGURE 7.20 The sweep profile follows the path and is controlled parametrically by guide curves.

The PropertyManager for the Sweep function includes an option for Show Sections, which in this case creates almost 200 intermediate cross-sections. These sections are used behind the scenes to create a loft. You can think of complex sweeps with guide curves or centerlines as an automated setup for an even more complex loft. It is helpful to envision features such as this when you are troubleshooting or setting up sweeps that are more complex. If you open the part mentioned previously from the DVD, you can edit the Sweep feature to examine the sections for yourself.

In most other published SolidWorks materials that cover these topics, sweeps are covered before lofts because many people consider lofts the more advanced topic. However, I have put lofts first because understanding them is necessary before you can understand complex sweeps, as complex sweeps really are just lofts.

Using a Pierce relation

The Pierce sketch relation is the only sketch relation that applies to a 3D out-of-plane edge or curve without projecting the edge or curve into the sketch plane. It acts as if the 3D curve is a length of string and the sketch point is the hole in the center of a bead where the string pierces the hole in the bead. The Pierce relation is most important in the Sweep feature when it is applied in the profile sketch between endpoints, centerpoints, or sketch points and the out-of-plane guide curves. This is because the Pierce relation determines how the profile sketch will be solved when it is moved down the sweep path to create intermediate profiles.

Figure 7.21 illustrates the function of the Pierce relation in a sweep with guide curves. The dark section on the left is the sweep section that is sketched. The lighter sketches to the right represent the intermediate profiles that are automatically created behind the scenes and are used internally to create the loft.

FIGURE 7.21 The effects of the Pierce relation

Figure 7.21 shows what is happening behind the scenes in a sweep feature. The sweep re-creates the original profile at various points along the path. The guide curve in this case forces the profile to rebuild with a different shape. Pierce constraints are not required in simple sweeps, but when you start using guide curves, you should also use a pierce.

Figure 7.22 shows a more complicated 3D sweep, where both the path and the guide curve are 3D curves. I cover 3D curves in Chapter 8; you can refer to these sections to understand how this part is made.

This part is created by making a pair of tapered helices, with the profile sketch plane perpendicular to the end of one of the curves. The taper on the outer helix is greater than on the inner one, which causes the twist to become larger in diameter as it goes up.

FIGURE 7.22 A 3D sweep

To make the circle follow both helices, you must create two pierce relations, one between the center of the circle and a helix, and the other between a sketch point that is placed on the circumference of the circle and the other helix. This means that the difference in taper angles between the two helices is what drives the change in diameter of the sweep.

Using a cut sweep with a solid profile

The Cut Sweep feature has an option to use a solid sweep profile. This kind of functionality has many uses, but is primarily intended for simulating complex cuts made by a mill or lathe. Figure 7.23 shows a couple of examples of cuts you can make with this feature. The part used for this screen shot is also on the DVD.

FIGURE 7.23 Cuts you can make with the Cut Sweep feature using a solid profile

The solid profile cut sweep has a few limitations that I need to mention:

• It uses a separate solid body as the cutting tool, so you have to model multi-bodies.
• The path must start at a point where it intersects the solid cutting tool body (path starts inside or on the surface of the cutting tool).
• The cutting tool must be definable with a revolved feature.
• The cutting tool must be made of simple analytical faces (sphere, torus, cylinder, and cone; no splines).
• You cannot use a guide curve with a solid profile cut (cannot control alignment).
• The cut can intersect itself, but the path cannot cross itself.

You can create many useful shapes with the solid profile cut sweep, but because of some of the limitations I've listed, some shapes are more difficult to create than others. For these shapes, you might choose to use regular cut sweep features. Figure 7.24 shows an example of a cam-like feature that you may want to create with this method, but may not be able to adequately control the cutting body.

FIGURE 7.24 Controlling a cam cut can be a challenge.

Workflow

Use the following general steps to create sweep features:

1. Create the path first. It may be tempting to create the profile first, but as a general rule, things work out better if you make the path first.
2. Create guide curves. Again, these work out better if you create them before the profile.
3. Create the profile (sweep cross-section) and relate it to the path with a Pierce sketch relation. Select a point in the sweep profile that you want to be driven down the path, like a bead follows a string.
4. Make sure that, as the profile is driven down the path (with the profile sketch plane maintaining its original relationship with the path), the profile has the flexibility to change the way it needs to. The sketch is re-evaluated at each point along the path. Use relative relations (parallel, perpendicular, and so on) instead of absolute ones (horizontal, vertical, fixed).
5. Start the Sweep feature from the toolbar or menu (all sketches must be closed).
6. Select the profile first, then the path. SolidWorks automatically toggles from the profile selection box to the path selection box as soon as a profile is selected, so take advantage of this automation to help you work quickly. Pay attention to any tool tip warnings or error messages that come up. If you are not able to select something, it is usually because there is something about that entity that is inappropriate for the purpose you are trying to assign to it.
7. Use the preview to check that it is performing the way you want it to. Click OK when you are satisfied with the result.

Understanding Fillet Types

SolidWorks offers very powerful filleting functions. The Fillet feature comprises various types of fillets and blends. Simple fillets on straight and round edges are handled differently from variable radius fillets, which are handled differently from the single or double hold line fillet or setback fillets. Once you click the OK button to create a fillet as a certain type, you cannot switch it to another type. You can switch types only before you create an established fillet feature.

Many filleting options are available, but most of them are relatively little used or even known. In fact, most users confine themselves to the constant radius or variable radius fillets. The following section describes all the available fillet types and options:

• Constant radius fillet
  • Multiple radius fillet
  • Round corners
  • Keep edge/Keep surface
  • Keep feature
• Variable radius fillet
• Face fillet
  • Curvature continuous fillet
  • Face fillet with Help Point
  • Single hold line fillet
  • Double hold line fillet
  • Constant width fillet
• Full round fillet
• Setback fillet
• Setback fillet with variable radius

Figure 7.25 shows the Fillet PropertyManager. Other options affect preview and selection of items, and these options are discussed in this section.

FIGURE 7.25 The Fillet PropertyManager

Creating a constant radius fillet

Constant radius fillets are the most common type that are created if you select only edges, features, or faces without changing any settings. When applying fillets in large numbers, you should consider several best practice guidelines and other recommendations that come later in this chapter.

There are still some longtime users who distinguish between fillets and rounds (where fillets add material and rounds remove it). SolidWorks does not distinguish between the two, and even two edges that are selected for use with the same fillet feature can have opposite functions; for example, both adding and removing material in a single feature.

Selecting entities to fillet

You can create fillets from several selections, including edges, faces, features, and loops. Edges offer the most direct method and are the easiest to control. Figure 7.26 shows how you can use each of these selections to create fillets on parts more intelligently.

FIGURE 7.26 Selection options for fillets

Faces and Features selections are useful when you are creating fillets where you want the selections to update. In Figure 7.27, the ribs that are intersecting the circular boss are also being filleted. If the rib did not exist when the fillet was applied, but was added later and reordered so that it came before the Fillet feature; then the fillet selection automatically considers the rib. If the fillet used edge selection, this automatic selection updating would not have taken place.

Using tangent propagation

By default, fillets have the Tangent Propagation option turned on. This is usually a good choice, although there may be times when you want to experiment with turning it off. Tangent propagation simply means that if you select an edge to fillet, and this edge is tangent to other edges, then the fillet will keep going along tangent edges until it forms a closed loop, the tangent edges stop, or the fillet fails.

FIGURE 7.27 Deselecting the Tangent Propagation option

If you deselect Tangent Propagation, but there are still tangent edges, you may see different results. One possible result is that it could fail. One of the tricks with fillet features is to try to envision what you are asking the software to do. For example, if one edge is filleted and the next edge is not, then how is the fillet going to end? Figure 7.27 shows two of the potential results when fillets are asked not to propagate. The fillet face may continue along its path until it runs off the part or until the feature fails.

Dealing with a large number of fillets

Figure 7.28 shows a model with a bit of a filleting nightmare. This large plastic tray requires many ribs underneath for strength. Because the ribs may be touched by the user, the sharp edges need to be rounded. Interior edges need to be rounded also for strength and plastic flow through the ribs. Literally hundreds of edges would need to be selected to create the fillets if you do not use an advanced technique.

FIGURE 7.28 A plastic tray with a large number of fillets

Selecting entities

Some of the techniques outlined previously, such as face and feature selection, can be useful for quickly filleting a large number of edges. Another method that still selects a large number of edges, but is not as intuitive as the others, is window selection of the edges. To use this option effectively, you may want to first position the model into a view where only the correct edges will be selected, turn off the Select Through Faces option, and use the Edges selection filter.

Using the FilletXpert

The FilletXpert is a tool with several uses. One of the functions is its capability to select multiple edges. A part like the one shown in Figure 7.28 is ideal for this tool. To use the FilletXpert, click the FilletXpert button in the Fillet PropertyManager. Figure 7.29 shows this. When you select an edge, the FilletXpert presents a popup tool bar giving you a choice of several selection options. Notice that Figure 7.29 shows the majority of the edges selected that are needed for this fillet.

FIGURE 7.29 Using the FilletXpert selection technique

The FilletXpert is also a tool that automatically finds solutions to complex fillet problems, particularly when you have several fillets of different sizes coming together.

The Corner tab of the FilletXpert enables you to select from different corner options, which are usually the result of different fillet orders. To use the CornerXpert, make sure the FilletXpert is active; then click the corner face, and toggle through the options.

Using preview

I like to use the fillet preview. It helps to see what the fillet will look like, and perhaps more important, the presence of a preview usually (but not always) means that the fillet will work.

Unfortunately, when you have a large number of fillets to create, the preview can cause a significant slowdown. Deselecting and using the Partial Preview are both possible options. Partial Preview shows the fillet on only one edge in the selection and is much faster when you are creating a large number of fillets.

Using folders

When you have a large number of fillet features, it can be tedious to navigate the FeatureManager. Therefore, it is useful to place groups of fillets into folders. This makes it easy to suppress or unsuppress all the fillets in the folder at once. Separate folders can be particularly useful if the fillets have different uses, such as fillets that are used for PhotoWorks models and fillets that are removed for FEA (Finite Element Analysis) or drawings.

Making multiple fillet sizes

The Multiple radius fillet option in the Fillet PropertyManager enables you to make multiple fillet sizes within a single fillet feature. Figure 7.30 shows how the Multiple radius fillet feature looks when you are working with it. You can change values in the callout flags or in the PropertyManager.

FIGURE 7.30 Using the Multiple radius fillet option

This may seem like an attractive way to group several fillets into as small a space on the FeatureManager as possible, but I cannot think of a single reason that would drive me to use this option. While there may be a small performance benefit to condensing several features into one, many more downsides adversely affect performance:

• Loss of control of feature order.
• A single failed fillet causes the whole feature, and thus all the fillets, to fail.
• Troubleshooting is far more difficult.
• Smaller groups of fillets cannot be suppressed without suppressing everything.
• You cannot change the size of a group of fillets together.

Rounding corners

The Round corners option refers to how SolidWorks handles fillets that go around sharp corners. By default, this setting is off, which leaves fillets around sharp corners looking like mitered picture frames. If you turn this setting on, the corner looks like a marble has rolled around it. Figure 7.31 shows the resulting geometry from both settings.

FIGURE 7.31 The Round corners option, both on and off

Using the Keep edge/Keep surface toggle

The Keep edge/Keep surface toggle determines what SolidWorks should do if a fillet is too big to fit in an area. The Keep edge option keeps the edge where it is and tweaks the position (not the radius) of the fillet to make it meet the edge. The Keep surface option keeps the surfaces of the fillet and the end face clean; however, to do this, it has to tweak the edge. There is often a tradeoff when you try to place fillets into a space that is too small. Sometimes it is useful to try to visualize what you think the result should look like. Figure 7.32 shows how the fillet would look in a perfect world, followed by how the fillet looks when cramped with the Keep edge option and how it looks when cramped with the Keep surface option.

FIGURE 7.32 The Keep edge option and the Keep surface option

The Default option chooses the best option for a particular situation. As a result, it seems to use the Keep edge option unless it does not work, in which case it changes to the Keep surface option.

Using the Keep Feature option

The Keep Feature option appears on the Fillet Options panel of the Fillet PropertyManager. By default, this option is turned on. If a fillet surrounds a feature such as a hole (as long as it is not a through hole) or a boss, then deselecting the Keep Feature option removes the hole or boss. When Keep Feature is selected, the faces of the feature trim or extend to match the fillet, as shown in Figure 7.33.

FIGURE 7.33 The Keep Feature option, both selected and unselected

Creating variable radius fillets

Variable radius fillets are another powerful weapon in the fight against boring designs; they also double as a useful tool to solve certain problems that arise. Although it is difficult to define exactly when to use the variable radius fillet, you can use it when you need a fillet to round an edge, and it has to change in size to fit the available geometry.

In some ways, variable radius fillets function like other fillets. For example, they offer propagation to tangent edges and preview options.

Applying the values

When you first select an edge for the variable radius fillet, the endpoints are identified by callout flags with the value unassigned. A preview does not display until at least one of the points has a radius value in the box. You can also apply radius values in the PropertyManager, but they are easier to keep track of using the callouts. Figure 7.34 shows a variable radius fillet after the edge selection, after one value has been applied, and after three values have been applied. To apply a radius value that is not at the endpoint of an edge, you can select one of the three colored dots along the selected edge. The preview should show you how the fillet will look in wireframe display.

FIGURE 7.34 Assigning values to a variable radius fillet

By default, the variable radius fillet puts five points on an edge, one at each endpoint, one at the midpoint, and one each halfway between the ends and middle. If you want to create an additional control point, there are three ways to do it:

• Ctrl+drag an existing point.
• Select the callout of an existing point and change the P (percentage) value.
• Change the Number of Instances value in the Variable Radius Parameters panel of the PropertyManager.

If you have selected several edges, and several unassigned values are on the screen, then you can use the Set Unassigned option in the PropertyManager to set them all to the same value. The Set All option sets all radius values to the same number, including any values that you may have changed to be different than the rest. Figure 7.35 shows the Variable Radius Parameters panel.

FIGURE 7.35 The Variable Radius Parameters panel of the Fillet PropertyManager

Another available option with the variable radius fillet is that you can set a value of zero at an end of the fillet. You need to be careful about using a zero radius, because it is likely to cause downstream problems with other fillets, shells, offsets, and even machining operations. You cannot assign a zero radius in the middle of an edge, only at the end. If you need to end a fillet at a particular location, you can use a split line to split the edge and apply a zero radius at that point. (Chapter 8 covers split lines.) Figure 7.36 shows a part with two zero-radius values.

The image on the right shows Instant3D being used to edit a variable radius fillet. Select the face of the fillet with Instant3D turned on, and blue dots appear where ever radius values are assigned. You can move these dots to dynamically edit the corresponding value of the variable radius.

FIGURE 7.36 Zero-radius values in the variable radius fillet

Using straight versus smooth transitions

Variable radius fillets have an option for either a straight transition or a smooth transition. This works like the two-profile lofts that were mentioned earlier in this chapter. The names may be somewhat misleading because both transitions are smooth. The straight transition goes in a straight line, from one size to the next, and the smooth transition takes a swooping S-shaped path between the sizes. The difference between these two transitions is demonstrated in Figure 7.37.

FIGURE 7.37 Straight versus smooth transitions of a variable radius fillet

Recognizing other uses for the variable radius fillet

Variable radius fillets use a different method to create the fillet geometry than the default constant radius fillet. Sometimes using a variable radius fillet can make a difference where a constant radius fillet does not work. This is sometimes true even when the variable radius fillet uses constant radius values. It is just another tool in the toolbox.

Using face fillets

Face fillets may be the most flexible type of fillet because of the range of what they can do. Face fillets start as simply an alternate selection technique for a constant radius fillet and extend to the extremely flexible double hold line face fillet, which is more of a blend than a fillet.

Under normal circumstances, the default fillet type uses the selection of an edge to create the fillet. An edge is used because it represents the intersection between two faces. However, there can sometimes be a problem with the edge not being clean or being broken up into smaller pieces, or any number of other reasons causing a constant radius fillet using an edge selection to fail. In cases like this, SolidWorks displays the error message, “Failed to create fillet. Please check the input geometry and radius values or try using the ‘Face Fillet’ option.”

Users almost universally ignore these messages. In the situation shown in Figure 7.38, the Face Fillet option suggested in the error message is exactly the one that you should use. Here the face fillet covers over all the junk on the edge that prevents the fillet from executing.

FIGURE 7.38 A face fillet covering a bad corner

Face fillets are sometimes amazing at covering over a mess of geometry that you might think you could never fillet. The main limitation on fillets of this type is that the fillet must be big enough to bridge the gap. That's right, I said big enough. Face fillets can fail if they are either too small or too large. Figure 7.39 shows a complex fillet situation that is completely covered by a face fillet.

FIGURE 7.39 A face fillet covering complex geometry

Using continuous curvature face fillets

Curvature continuity refers to the quality of a transition between two curves or faces, where the curvature is the same or continuous at and around the transition. The best way to convey this concept is with simple 2D sketch elements. When a line transitions to an arc, you have non-continuous curvature. The line has no curvature, and there is an abrupt change because the arc has a specific radius.

To make the transition from r = ∞ to r = 2 smoothly, you would need to use a variable radius arc if such a thing existed. There are several types of sketch geometry that have variable curvature, such as ellipses, parabolas, and splines. Ellipses and parabolas follow specific mathematical formulas to create the shape, but the spline is a general curve that can take on any shape that you want, and you can control its curvature to change smoothly or continuously. Splines, by their very definition, have continuous curvature within the spline, although you cannot control the specific curvature or radius values directly.

All this means that continuous curvature Face fillets use a spline-based variable-radius section for the fillet, rather than an arc-based constant radius. Figure 7.40 illustrates the difference between continuous curvature and constant curvature. The spikes on top of the curves represent the curvature (1/r, and so the smaller the radius, the taller the spike). These spikes are called a curvature comb.

FIGURE 7.40 Using curvature combs to evaluate transitions

In comparison to Figure 7.41, notice how the curvature comb immediately jumps from no curvature to the constant arc radius, but the spline image ramps up to a curvature that varies.

Using face fillets with the Help Point

The Help Point in the Face Fillet PropertyManager is a fairly obscure option. However, it is useful in cases where the selection of two faces does not uniquely identify an edge to fillet. For example, Figure 7.41 shows a situation where the selection of two faces could result in either one edge or the other being filleted (normally, I would hope that both edges would be filleted). The fillet will default to one edge or the other, but you can force it to a definite edge using the Help Point.

In some cases, the Help Point is ignored altogether. For example, if you have a simple box, and select both ends of the box as selection set 1, and the top of the box as selection set 2, then the fillet could go to either end. Consequently, assigning a Help Point will not do anything in this case, because multiple faces have been selected. The determining factor is which of the multiple faces is selected first. If this were a more commonly used feature, the interface for it might be made a little less cryptic, but because this feature is rarely, if ever, used, it just becomes a quirky piece of trivia.

FIGURE 7.41 Using a Help Point with a face fillet

Applying a single hold line fillet

A single hold line fillet is a form of variable radius fillet. Rather than the radius being driven by specific numerical values, it is driven by a hold line, or edge, on the model. The hold line can be an existing edge, forcing the fillet right up to the edge of the part, or it can be created by a split line, which enables you to drive the fillet however you like. Figure 7.42 shows these two options, before and after the fillets. Notice that these fillets are still arc-based fillets; if you were to take a cross-section perpendicular to the edge between filleted faces, it would be an arc cross-section with a distinct radius.

However, in the other direction, hold line fillets do not necessarily have a constant radius, although they may if the hold line is parallel with the edge between faces.

You can select the hold line in the Fillet Options panel of the Face Fillet PropertyManager, as shown in Figure 7.43. The top panel, Fillet Type, is available only when the feature is first created. When you edit it after it has been created, the Fillet Type panel does not appear. As a result, you cannot change from one top-level type of fillet to another after it has been initially created.

FIGURE 7.42 Single hold line fillets

FIGURE 7.43 The PropertyManager interface for the hold line face fillet

Using a double hold line fillet

There are times when a single hold line does not meet your needs. The single hold line controls only one side of the fillet, and in order to control both sides of the fillet, you must use a double hold line fillet. SolidWorks software does not specifically differentiate between the single and double hold line fillets, but they are radically different in how they create the geometry. When both sides of the fillet are controlled, it is not possible to span between the hold lines with an arc that is tangent to both sides unless you were careful about setting up the hold lines so that they are equidistant from the edge where the faces intersect. This means that the double hold line fillet must use a spline to span between hold lines, as shown in Figure 7.44.

To get this feature to work, you need to use the curvature continuous option in the Fillet Options panel. Remember that this option creates a spline-based fillet rather than an arc-based fillet, which is exactly what you need for a double hold line fillet. This makes the double hold line fillet more of a blend than a true fillet. This requirement is not obvious to most users and may not even be documented in the SolidWorks Help, nor is it exactly intuitive. To get the double hold line fillet to work, you must use the curvature continuous option. Figure 7.45 shows examples of the double hold line fillet.

FIGURE 7.44 A double hold line uses a spline, not an arc.

FIGURE 7.45 Examples of the double hold line fillet

Using a constant width fillet

The Constant width option of the Face Fillet PropertyManager drives a fillet by its width rather than by its radius. This is most helpful on parts where the angle of the faces between which you are filleting is changing dramatically. Figure 7.46 illustrates two situations where this is particularly useful. The setting for constant width is found in the Options panel of the Face Fillet PropertyManager. The part shown in the images is on the DVD as Chapter 7 Constant Width.sldprt.

FIGURE 7.46 The constant width fillet

Applying a full round fillet

The full round fillet is very useful in many situations. In fact, it may actually work in situations where you would not expect it to. It does require quite a bit of effort to accomplish the selection, but it compensates by enabling you to avoid alternate fillet techniques.

To create a full round fillet, you have to select three sets of faces. Usually one face in each set is sufficient. The fillet is tangent to all three sets of faces, but the middle set is on the end and the face is completely eliminated. Figure 7.47 shows several applications of the full round fillet. Notice that it is not limited to faces of a square block, but also propagates around tangent entities and can create a variable radius fillet over irregular lofted geometry.

FIGURE 7.47 A full round fillet

Building a setback fillet

The setback fillet is the most complex of the fillet options. You can use the Setback option in conjunction with constant radius, multiple radius, and variable radius fillet types. A setback fillet blends several fillets together at a single vertex, starting the blend at some “setback” distance along each filleted edge from the vertex. At least three, and often more, edges come together at the setback vertex. Figure 7.48 shows the PropertyManager interface and what a finished setback fillet looks like. The following steps demonstrate how to use the setback fillet.

FIGURE 7.48 The Setback Fillet interface and a finished fillet

Setting up a setback fillet can take some time, especially if you are just learning about this feature. You must specify values for fillet radiuses, select edges and vertices, and specify three setback distances for every vertex. If you are using multiple radius fillets or variable radius fillets, then this becomes an even larger task. The steps are as follows:

1. Determine the type of fillet to be used:
   • Constant radius fillet
   • Multiple radius fillet
   • Variable radius fillet
2. Select the edges to be filleted. Selected edges must all touch one of the setback vertices that will be selected in a later step.
3. Assign radius values for the filleted items. Figure 7.49 shows a sample part that illustrates this step.

   FIGURE 7.49 The setback fillet setup for Steps 1 through 3

   

4. Select the setback vertices. In the Setback Parameters panel of the PropertyManager, with the second box from the top highlighted, select the vertices. Although this box looks like it is only big enough for a single selection, it can accept multiple selections.
5. Enter setback values. As shown in Figure 7.50, the setback callout flags have leaders that point from a specific value to a specific edge. Alternately, you could use the Set All or Set Unassigned options in a similar way to how they are used with the variable radius fillet interface. The dimensions refer to distances, as shown in the image to the right in Figure 7.50. The setback distance is the distance over which the fillet will blend from the corner to the fillet.

   FIGURE 7.50 Entering setback values

   

   Caution

   When you select multiple vertices, the preview arrows that indicate which edge you are currently setting the setback value for may be incorrect. The arrows can only be shown on one vertex; therefore, you may want to rely on the leaders from the callouts to determine which setback distance you are currently setting.

6. Repeat the process for all selected setback vertices. If you are using a preview, then you may notice that the preview goes away when starting a second set of setback values. Don't worry. This is probably not because the feature is going to fail. Once you finish typing the values, the preview will return. When you have spent as much time setting up a feature as you will spend on this, seeing the preview disappear can be frustrating; however, persevere, and it will return.

Using Chamfers

Chamfers in SolidWorks are not as flashy as fillets, but they do have some useful functionality. Some similarities exist between chamfers and fillets, such as the propagation to tangent edges, selecting faces to select the loop of edges around the face, and the ability to see full, partial, or no preview of the finished feature. Many of the best practice ideas you can apply to fillets also apply to chamfers. Figure 7.51 shows the PropertyManager for chamfers.

FIGURE 7.51 Working with chamfer features

You can specify a chamfer using either an angle and a distance or two distance values. For most common situations, these methods are adequate. The situation becomes less definite if you are creating a chamfer between faces that are not at right angles to one another or may not even be planar. These situations require some experimentation to find the correct geometry.

When you create chamfers at angles other than 45 degrees, you can use the Flip Direction option to control the feature. It is important to note the difference between having direct control (angle the chamfer from this face) and indirect control (angle the chamfer from the other face). Indirect control is essentially trial and error. If you don't like what you are given automatically, you can try the other option.

The Flip Direction option flips the direction of all of the chamfers being created by a particular feature. This is obviously only important when you have chamfers that are made at an angle that is not 45 degrees, or unequal distances in the case of a distance-distance chamfer. So in some situations, where the default directions of more than a single edge are going in opposite directions, your only recourse is to create multiple chamfer features and control them independently.

One of the most interesting functions of the Chamfer tool is the vertex chamfer, shown in Figure 7.52. You can chamfer a corner with equal distances or distances along each edge. This feature can only be used at corners where three edges come together — standard block corners.

FIGURE 7.52 Applying a corner chamfer

Tutorial: Bracket Casting

When you follow this tutorial, you are encouraged to follow the directions the first time to make sure that you understand the concepts involved, and then to go through it again, this time deviating from the instructions to see if you can expand your understanding by experimentation. To try bracket casting, follow these steps:

1. Open a new part using an inch-based template.
2. On the Right plane, draw a circle centered at the origin with a diameter of 1.50 inches, and a second circle placed 4.000 inches vertically from the first, with a diameter of 2.250 inches.
3. Exit the sketch, and make sure Instant 3D is selected. The Instant 3D icon is on the Features toolbar, and looks like a ruler with an arrow. Click the sketch in the graphics window, and pull the Instant 3D arrow to create a solid. Edit the feature (right- or left-click the feature either in the graphics window or in the FeatureManager and click the Edit Feature icon, which is the yellow and green block with a hand pointing to it). Now enter numbers by hand so that you extrude the sketch 1.000 inch using a From condition of Offset by 1.000 inch, such that the offset and the extrude depth are in the same direction. Rename this feature Bosses in the FeatureManager. Figure 7.53 shows the results of these steps.

   FIGURE 7.53 The results of Steps 1 to 3

   

   Note

   These steps produce multiple bodies that will be merged in a later step. Multi-body parts are covered in more detail in Chapter 19. You can tell that there are multiple bodies by looking at the Solid Bodies folder near the top of the tree and expanding the folder. The bodies are listed in the folder.

4. On the Top plane, open a new sketch and draw a horizontal construction line across the cylinder, from the midpoint of one side to the midpoint of the other side. To pick up the automatic relations for the midpoints more easily, it is recommended that you orient the view, normal to the sketch, or use the Top view. It does not matter if you make the relations to the top or bottom cylinder, because the midpoints of the sides are in the same place when they are projected into the sketch plane.
5. Next, draw an ellipse (Tools Sketch Tools Ellipse) centered at the midpoint of the construction line and that measures .700 inches horizontally and 1.375 inches vertically. You may want to assign a relation between the center of the ellipse and one of the control points to prevent the ellipse from rotating and fully define the sketch Exit the sketch when you are satisfied with the result.
6. Show the sketch for the Bosses feature. Click the plus icon next to the Bosses extrude to show the sketch, and then right-click the sketch and select Show.
7. Create a plane parallel to the Top plane at the center of the larger circle. You can access the Plane creation interface by choosing Insert Reference Geometry Plane. If you pre-select the Top plane from the flyout FeatureManager and the center of the larger sketch circle from the graphics window, the interface automatically creates the correct plane. Click OK to create the plane. Rename this plane Top Boss Plane.
8. Draw a second ellipse on the Top Boss Plane. Do not draw a construction line as you did for the first ellipse; instead, you can just make the centerpoint of the second ellipse directly on top of the first ellipse's centerpoint. The dimensions should be 1.000 inch horizontal by 1.750 inches vertical. Figure 7.54 shows the results up to this point.

   FIGURE 7.54 The results up to Step 8

   

   Tip

   When you are sketching on parallel planes that are separated by some distance and trying to pick up automatic relations, it is often very helpful to be looking “normal to” the sketch, so that you can see how other entities are projected into the sketch plane.

9. Use the Loft feature to loft between the two ellipses. Be sure to select the ellipses in approximately the same location so that they do not twist. If the loft preview accidentally twists, then use the connectors (light-blue square dots on the sketches that are connected by a straight line) to straighten out the loft.

   Note

   Notice that this feature joined together the other two disjoint bodies with the body that was created by the loft into a single body. This is a result of selecting the Merge Result option in the Options panel.

   Tip

   If you want to experiment, expand the Start/End Constraints panel and apply end conditions for the loft. This causes the loft to change from a straight loft to a curved loft.

10. Right-click all sketches that are showing, and select Hide. Do the same for the Top Boss Plane. This cleans up the display to prevent it from becoming confusing. However, if you prefer to see the sketches, then you can leave them displayed.

    Tip

    You can either hide or show different types of entities in groups by using the View menu. Hide All Types hides everything, and disables the options for individual entity types to be used.

11. Open a sketch on the Right plane. Sketch an ellipse such that the center is oriented 1.750 inches vertically from the Origin, and the ellipse measures .750 inches horizontally and 1.500 inches vertically.
12. Extrude this ellipse using the Up To Next end condition. If Up To Next does not appear in the list, then change the direction of the extrude and try it again.
13. Show the sketch of the Bosses feature by expanding the feature (click the “+” next to it), right- or left-clicking the sketch icon, and clicking the Hide/Show icon (eyeglasses). Next, open a sketch on the Right plane. Sketch two circles that are concentric with the original circles, with the dimensions of .875 inches and 1.250 inches. Exit the sketch.
14. Use Instant 3D to create an extruded cut that goes through the large circular bosses. This feature will look like a boss extrusion at first, so when you have finished dragging its depth, a small toolbar with two icons appears. One of the icons enables you to add draft; the other enables you to turn the boss into a cut. Figure 7.55 shows the state of the model up to this step.

    FIGURE 7.55 The results up to Step 14

    

15. Start a fillet feature, and select the face of the Loft feature. Assign a radius of .200 inches.

    Note

    Although this fillet is created by selecting a face, it is not a face fillet. Selecting a face for a regular constant radius fillet simply fillets any edge that is on the face.

16. Create a mirror feature, using the Right plane as the mirror plane. In the Mirror PropertyManager, expand the Bodies To Mirror panel, and select anywhere on the part. Make sure that the Merge Solids option is selected. Click OK to accept the mirror.
17. Orient the view to the Front view, and then turn the view on its side (hold down Alt and press the left- or right-arrow key six times).
18. Open a new sketch on the Front plane. From the View menu, make sure that Hide All Types is not selected, and show Temporary Axes. Draw and dimension a horizontal construction line, as shown in Figure 7.56.

    FIGURE 7.56 The results up to Step 18

    

19. With the construction line selected, start the Sketch Text command (Tools Sketch Entities Text). Make sure that the line appears in the Curves selection box.
20. Click in the text box, and type Made in USA (or your name or company name). Select the text and click the Bold button. Deselect the Use Document Font option, change the font to use units, and set the height to .175 inches.
21. Click OK to exit the Sketch Text PropertyManager, and click OK again to exit the sketch. You can turn off the Temporary Axis display.
22. Choose Insert Features Wrap. You should be prompted to select a plane or a sketch. Use the Flyout FeatureManager to select the sketch that you just created with the sketch text in it. Next, select the cylindrical face of the boss to see a preview of the text wrapped onto the face. If the text appears backward, then select the Reverse Direction option in the Wrap PropertyManager.
23. Select the Emboss option, and assign a thickness of .025 inches. Click in the Pull Direction selection box and select the Front plane. Click OK to accept the feature.
24. Save the part and close it. If you would like to examine the reference part, you can find it on the DVD with the filename Chapter 7 Tutorial Bracket Casting.sldprt. The finished part is shown in Figure 7.57.

    FIGURE 7.57 The finished part

    

Summary

SolidWorks has a wide selection of feature types to choose from, ranging from simple extrudes and revolves to more complex lofts and sweeps. Some features have so many options that it may be difficult to take them all in at once. You should browse through the models on the DVD for this chapter and use the Rollback bar (described in detail in Chapter 12) to examine how the parts were built. You can then try to create a few on your own. The best way to learn these features is to use them on practice parts, and through experimentation. Curiosity is your greatest teacher.