CREATING A SOLID FEATURE

In this case, the term solid feature is used as an opposite of thin feature. A solid feature is the 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.

CREATING A THIN FEATURE

The Thin Feature option is available in several features, but it's 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 or sketches with mixed types. 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 thin features. 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.

You can create a 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 will not handle this kind of change. Figure 7.2 shows different types of geometry that are typically created from thin features.

UNDERSTANDING THE WORKFLOW

SolidWorks offers multiple ways to do things in most functions. Most of the time, there is no one way that is better than the others. Having a lot of ways to do things makes remembering ways to do things easy, but sometimes it is hard to teach or learn because the options get overwhelming quickly. My suggestion is to find a way that works for you and use it. Learn other ways if something stops working for you. Here's an example.

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.

Different types of features and geometry require different types of sketches, as shown in Figure 7.3. Some sketch types can't be used directly for making features at all, but may be used as reference. Closed, Open, and Nested contours are the types you will probably use the most in SolidWorks.

In addition to extruding 2D sketches, SolidWorks can also extrude 3D sketches. SolidWorks will automatically fill in the 3D sketch to form a solid face. You need to define a direction such as a plane (the plane normal is used as direction) or an edge, line, or axis, as shown in Figure 7.4.

USING END CONDITIONS

End conditions control how the extrude starts and stops. In most situations, the extrude starts from a sketch plane and goes a specified distance, but there are other options.

Start conditions

• From sketch plane
• From offset distance/vertex
• From selected plane
• From 3D sketch
• From selected face

End conditions

• Distance (blind)
• Through all (up to the furthest face)
• Up to a selected vertex
• Up to a selected surface
• Offset from surface (either near or far offset, and either offset or translated)
• Up to a selected body
• Midplane (divides distance in half about start plane)

Direction

• In addition to the start and end conditions, you can control the direction of the extrude.
• If you want to push a profile along a curve, you can use either a revolve or a sweep, as appropriate, which are both covered later in this chapter.

UNDERSTANDING END CONDITIONS

There are five Revolve end conditions:

• 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 7.5 shows the Revolve PropertyManager.

WORKFLOW

This is the workflow for the Revolve feature:

1. Create a sketch.
2. Invoke the Revolve feature.
3. Select an axis (typically a construction line).
4. Set the end conditions.
5. Click OK.

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.

COMPARING THE LOFT AND BOUNDARY FEATURES

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 are no profiles and guide curves in boundary—the two directions are treated equally, and they 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. In fact, the Boundary feature is used far less often than its surfacing-related cousin, the Boundary Surface.

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. Boundary is a very powerful feature, with options for creating interpolated solid shapes. Face-by-face control, however, still must come from using surfacing features.

Figure 7.8 shows the features made with F and X layouts of sketches. The F layout resembles the letter F, and the sketches lie on the planes Right YZ, FrontXY, and Plane1. The X layout uses sketches on RightYZ and Plane2. These two features represent sketch layouts that you can't use with the Loft feature.

Loft does have two conditions that Boundary cannot answer:

• Centerline loft: All boundary profiles must intersect.
• Closed loop loft without Direction 2 (guide) curves: To make a closed-loop boundary, you must have Direction 2 curves that intersect Direction 1 curves.

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.

I discuss 3D sketches in more detail in Chapter 6, “Getting More from Your Sketches.”

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 ribs of the hull very much resemble loft sections. With the splines or slats bending at each rib, 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 7.9 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).

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. 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.

USING A SIMPLE SWEEP

An example of a simple sweep is shown in Figure 7.10. The paper clip uses a circle as the profile and the coiled lines and arcs as the path. Simple sweeps keep the same size and shape profile along the entire path. This sweep could use the previously mentioned option for Circular Profile, also shown in Figure 7.10.

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 7.11 shows all these elements and the finished feature.

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. Once you open the Chapter7 Bottle.sldprt part, 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, because 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. 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 7.12 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 7.12 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 7.13 shows a more complicated 3D sweep, where both the path and the guide curve are 3D curves. I cover 3D curves in Chapter 8, “Selecting Secondary Features”; 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.

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 it's primarily intended for simulating complex cuts made by a mill or lathe. Figure 7.14 shows a couple of examples of cuts you can make with this feature. The part used for this screen shot, called Chapter 7 - cut sweep solid profile.sldprt, is also in the website download material.

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

• It requires two bodies: the target and a cutting tool.
• 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 path must be tangent within itself (no sharp corners).
• 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 (because you 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.

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, as 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 change. The sketch is reevaluated at each point along the path. Use relative relations (parallel, perpendicular, and so on) instead of absolute ones (horizontal, vertical, or fixed).
5. Start the Sweep feature from the toolbar or menu. All sketches must be closed.
6. Select the profile first and 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. Note that for circular profiles centered on the path, there is no longer a need to create a sketch.
7. Use the preview to check that it is performing the way you want. Click OK when you are satisfied with the result.

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 7.16 shows how you can use each of these selections to create fillets on parts more intelligently.

Faces and features selections are useful when you are creating fillets where you want the selections to update. In Figure 7.16, the ribs that intersect 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 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 take 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 keeps going along tangent edges until it forms a closed loop, the tangent edges stop, or the fillet fails.

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 7.17 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 7.18 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 also need to be rounded for strength and plastic flow through the ribs. Literally, hundreds of edges will need to be selected to create the fillets if you do not use an advanced technique.

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 that all meet the same criteria. Another method 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.

The first option in the Fillet PropertyManager is the Selection toolbar. This toolbar highlights several selection options based on types of selections similar to your initial selection. For example, if you selected an edge, the Selection toolbar might highlight edges parallel to the selected edge, faces that touch the selected edge, or edges tangent to the selected edge.

USING THE FILLETXPERT

The FilletXpert automatically finds solutions to complex fillet problems, particularly the problems that can arise when you have several fillets of different sizes coming together. It also allows you to select multiple edges. A part like the one shown in Figure 7.18 is ideal for this tool.

To use the FilletXpert, click the FilletXpert button in the Fillet PropertyManager (Figure 7.19). When you select an edge, the FilletXpert presents a pop-up toolbar, giving you several selection options. Notice that Figure 7.19 shows the majority of the edges selected that are needed for this fillet. This is the same type of functionality you will find in the Selection toolbar, in fact; the Selection Toolbar toggle is found in the FilletXpert PropertyManager shown in Figure 7.19.

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. Folders also allow the bulk-selection of such features if they were saved in selection sets.

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 7.20 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.

Although you may see a small performance benefit when condensing several features into one, many more downsides adversely affect performance:

• You lose control of feature order.
• A single failed fillet causes the whole feature, and therefore 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 7.21 shows the resulting geometry from both settings.

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 visualize what you think the result should look like. Figure 7.22 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.

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 7.23.

USING SYMMETRIC OR ASYMMETRIC FILLETS

Standard fillets are symmetrical on either side of the selected edge. An asymmetrical fillet can have a different radius on either side of the selected edge. This makes for a more complex-looking fillet and may also complicate troubleshooting in complex parts. Figure 7.24 illustrates the concept of asymmetrical fillets, along with the Fillet Parameters panel of the Fillet PropertyManager associated with specifying this type of fillet.

Asymmetrical fillets can also be used in variable-radius fillets, described later in this chapter. In addition to specifying the two radius values, you can also flip the sides of the values using the opposing arrows icon.

SELECTING A FILLET PROFILE

Within the Symmetric and Asymmetric fillets, you also have some profile options:

• Circular (only symmetric)
• Elliptic (only asymmetric)
• Conic rho (symmetric and asymmetric)
• Conic radius (only symmetric)
• Curvature continuous (symmetric and asymmetric)

You can think of these profiles as being the fillet cross sections. Circular cross sections can be defined with a single radius. This should make intuitive sense. You should also be familiar with the shape of an ellipse, although this is not directly specifiable with a radius value, SolidWorks uses the radius value to approximate. The cross sections are shown in Figure 7.25.

The Circular profile is the normal type of fillet specified with a single radius. This is what we think of as a default fillet.

The Elliptic profile is available only when specifying asymmetric fillets. The two radius values determine an ellipse, which is used to round the selected edge instead of the usual arc.

The Conic rho profile is driven by rho (ρ). Conic in the name refers to the conic sections from classical geometry–circle, ellipse, hyperbola, parabola—but as driven by the parameter rho in many other CAD systems. Rho runs between 0 and 1. Figure 7.26 shows the effect of the range of rho values on the profile of the fillet. If you want to experiment with this, the file used to create this screen capture is in the download materials under the filename Conic rho fillet.sldprt.

The Conic radius profile is specified by the main radius value and a conic radius value, which can be any positive number. The Conic radius value is the radius of the conic section curve at the shoulder, which in this case means the middle of the curve. This works in a way similar to the rho value, and the range of effects is similar to what you see in Figure 7.26.

Curvature Continuous profile is available on edge-selected fillets. This is new. Previously, curvature continuity was available only on face fillets, as discussed next. Curvature Continuity (c2) is a spline-based profile that matches the curvature of the faces on either side of the selected edge. This edge-selected c2 fillet is a big convenience over needing to select faces. Any old c2 face fillets you have should still work, but going forward in most cases, the edge-selected fillets will be easier to create.

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 noncontinuous curvature. The line has no curvature, and there is an abrupt change because the arc has a specific radius.

To make the transition from to 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 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 fillets use a spline-based profile for the fillet, rather than circular or elliptical. Figure 7.27 illustrates the difference between continuous curvature and constant curvature. The spikes on top of the curves represent the curvature (, so the smaller the radius, the taller the spike). These spikes are called a curvature comb.

Some of these fillet profile options may seem esoteric to you, but there are people who are glad to have these options, and the options are available in some other CAD programs.

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 7.28 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.

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, 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 from the rest. Figure 7.29 shows the Variable Radius Parameters panel.

You can set an end of a variable-radius fillet to a value of zero, but you need to be careful 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, “Selecting Secondary Features,” covers split lines.) Figure 7.30 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 wherever radius values are assigned. You can move these dots to dynamically edit the corresponding value of the variable radius.

USING STRAIGHT VS. 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 7.31.

RECOGNIZING OTHER USES FOR VARIABLE-RADIUS FILLETS

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 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 7.34 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, 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.

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 7.35 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 to the edge between faces.

You can select the hold line in the Fillet Options panel of the Face Fillet PropertyManager. 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.

USING A DOUBLE HOLD-LINE FILLET

Sometimes, 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 7.36.

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 7.37 shows 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 7.38 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 can be found in the download material as Chapter 7 Constant Width.sldprt.