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.

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 7.1. A closed loop sketch and an extruded solid feature

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 7.2. The Thin Feature portion of the Extrude PropertyManager

Thin feature sketches are typically simpler than closed loop sketches, which usually means that they are more robust through changes. 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, they are not 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.

Figure 7.3. Different types of geometry created from thin feature extrudes

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.

Sketch contours

Best Practice

SolidWorks works best with well-disciplined sketches that follow the rules. Therefore, if you plan to use sketch contours, you should make sure that it is not simply because you are unwilling to clean up a messy sketch.

When you define features by selecting sketch contours, they are more likely to fail if the selection changes when the selected contour's bounded area changes in some way. It is considered best practice to use the normal closed loop sketch when you are defining features. Contour selection is best suited to "fast and dirty" conceptual models, which are used in very limited situations.

There are several types of contour selection, as shown in Figure 7.4.

Figure 7.4. Types of contour selection

The terminology used by SolidWorks is not always logical, for example, the heading of the PropertyManager panel that you use is called Selected Contours, but the item in the selection box is called a Region. This is why you may sometimes hear Contours referred to as Regions.

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. 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 7.5 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 CD-ROM as Chapter 7 Extrude 3D Sketch.sldprt.

Figure 7.5. Extruding a non-planar 3D sketch

If you need to have ends 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, and extrude all the profiles Through All, and they will all be cut to different depths.

3D 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.

Cross-Reference

Surfacing features are covered in detail in Chapter 27. Chapter 4 contains additional details on extrude end conditions, thin features, directions, and the From options. Chapter 31 also has more information on 3D sketches.

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 7.6 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.

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.

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 heads-up display icons 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 underdefined sketch elements.

Figure 7.6. Identifying Instant 3D interface elements

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 on 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

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

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 7.7. Sketch scaling and moving options with Instant 3D

There are three Revolve end conditions:

There is no equivalent for Up to Vertex, Up to Next, Up to Surface, or Up to Body with the Revolve feature.

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.

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.

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.

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 7.10 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 7.10. 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 examples in far detail. 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.

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.

Cross-Reference

Refer to Chapter 27 for surfacing information. For a comprehensive look at surfacing and complex shapes, see the SolidWorks Surfacing and Complex Shape Modeling Bible (Wiley, 2008).

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.

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 7.11. The curved arrows to the left identify the direction in which the angle deviation is going.

Figure 7.11. Examples of end constraints

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.

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.

Best Practice

Do not try to push the shape of the loft too extremely with guide curves. Use guide curves mainly for tweaking and fine-tuning rather than coarse adjustments. Use loft sections and end constraints to get most of the overall shape correct. Pushing too hard with a guide curve can cause the shape to kink unnaturally.

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 7.12 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 CD-ROM with the filename Chapter 7 Guide Curves.sldprt.

Figure 7.12. A loft with and without guide curves

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.

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.

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:

You can choose from the following Loft options, as shown in Figure 7.13:

Figure 7.13. Loft options

An example of a simple sweep is shown in Figure 7.15. The paper clip uses a circle as the profile and the coiled lines and arcs as the path.

Figure 7.15. The sweep profile follows the path.

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 7.16 shows all these elements and the finished feature.

On the CD-ROM

The part shown in Figure 7.16 is on the CD-ROM with the filename Chapter7 Bottle.sldprt.

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 CD-ROM, you can edit the Sweep feature to examine the sections for yourself.

Figure 7.16. The sweep profile follows the path and is controlled parametrically by guide curves.

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.

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 thread and the sketch point is the eye of a needle where the thread pierces the needle eye. 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 7.17 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 7.17. The effects of the Pierce relation

Figure 7.17 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 7.18 shows a more complicated 3D sweep, where both the path and the guide curve are 3D curves. I cover 3D curves toward the end of this chapter; you can refer to these sections to understand how this part is made.

On the CD-ROM

The part shown in Figure 7.18 is on the CD-ROM with the filename Chapter 7 3D Sweep.sldprt.

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.

Figure 7.18. A 3D sweep

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 7.19 shows a couple of examples of cuts you can make with this feature. The part used for this screen shot is also on the CD-ROM.

Figure 7.19. 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:

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 7.20 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 7.20. Controlling a cam cut may be a challenge

The Tapered Helix panel in the Helix PropertyManager enables you to specify a taper angle for the helix. The taper angle does not affect the pitch. If you need to affect both the taper and the pitch, then you can use a variable pitch helix. Figure 7.22 shows how the taper angle relates to the resulting geometry.

Figure 7.22. The tapered helix panel

You can specify the variable pitch helix either in the chart or in the callouts that are shown in Figure 7.23. Both the pitch and the diameter are variable. The diameter number in the first row cannot be changed, but is driven by the sketch. In the chart shown, the transition between 4 and 4.5 revolutions is where the pitch and diameter both change.

Figure 7.23. The variable pitch helix

A spiral is a flattened (planar) tapered helix. The pitch value on a spiral is the radial distance between revolutions of the curve.

The Sketch On Faces option is the easiest to explain, so I will describe this one first. With this option set, the projected curve is created by projecting a 2D sketch onto a face. The sketch is projected normal (perpendicular) to the sketch plane. This is like extruding the sketch and using the Up To Surface end condition. The sketch can be an open or closed loop, but it may not be multiple open or closed loops, nor can it be self-intersecting. Figure 7.24 shows an example of projecting a sketch onto a face to create a projected curve.

Figure 7.24. A projected curve using the Sketch On Faces option

This is the concept that most frequently causes difficulty for users. The Sketch Onto Sketch Projected Curve option can be visualized in a few different ways.

Intersecting surfaces visualization method

A second method used for visualizing Sketch On Sketch projected curves is the intersecting surfaces method. In this method, you can see the curve being created at the intersection of two surfaces that are created by extruding each of the sketches. This method is shown in Figure 7.26.

Figure 7.25. The reverse 2D drawing visualization method for projected curves

Figure 7.26. Using intersecting surfaces to visualize a Sketch on Sketch projected curve

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

Figure 7.30. Selection options for fillets

Tip

To select features for filleting, you must select them from the FeatureManager. The Selection Filter only filters edges and faces for fillet selection. You can select loops in two ways: through the right-click Select Loop option, or by selecting a face and Ctrl+selecting an edge on the face.

Another option for selecting edges in the Fillet command is the Select Through Faces option, which appears on the Fillet Options panel. This option enables you to select edges that are hidden by the model. This can be a useful option on a part with few hidden edges, or a detrimental option on a part where there are many edges due to patterns, ribs, vents, or existing fillets. You can control a similar option globally for features other than fillets by choosing Tools

Options

Display/Selection, Allow Selection In HLR [Hidden Lines Removed], and Shaded Modes.

Faces and Features selections are useful when you are creating fillets where you want the selections to update. In Figure 7.31, 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.

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.

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 7.31 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.

Best Practice

In general, fillets should be the last features that are applied to a model, particularly the small cosmetic or edge break fillets. Larger fillets that contribute to the structure or overall shape of the part may be applied earlier.

Be careful of the rock-paper-scissors game that you inevitably are caught up in when modeling plastic parts and deciding on the feature order of fillets, draft, and shell. Most fillets should come after draft, and large fillets should come before the shell. Draft may come either before or after the shell, depending on the needs of the area that you are dealing with on the part. In short, there is no single set of rules that you can consistently apply and that works best in all situations.

Figure 7.31. Deselecting the Tangent Propagation option

Figure 7.32 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 7.32. A plastic tray with a large number of fillets

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.

Figure 7.33. Using the FilletXpert selection technique

Performance

For rebuild speed efficiency, you should make fillets in a minimum number of features. For example, if you have 100 edges to fillet, it is better for performance to do it with a single fillet feature that has 100 edges selected rather than 100 fillet features that have one edge selected. This is the one case where creating the feature and rebuilding the feature are both faster by choosing a particular technique. (Usually if it is faster to create, it rebuilds more slowly.)

Best Practice

Although creation and rebuild speed are in sync when you use the minimum number of features to create the maximum number of fillets, this is not usually the case. (There had to be a downside.) When a single feature has a large selection, any one of these edges that fail to fillet will cause the entire feature to fail. As a result, a feature with 100 edges selected is 100 times more likely to fail than a feature with a single edge. Large selection sets are also far more difficult to troubleshoot when they fail than small selection sets that fail.

The Multiple Radius Fillet option in the Fillet PropertyManager enables you to make multiple fillet sizes within a single fillet feature. Figure 7.34 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 7.34. 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:

Best Practice

While this may be more personal opinion than best practice, I believe that there are good reasons to consider using techniques other than single features that contain many fillets, or single features that drive fillets of various sizes. Best practice would lean more toward grouping fillets that have a similar use and the same size. For example, you may want to separate fillets that break corners on ribs from fillets that round the outer shape of a large plastic part.

Another consideration is feature order when it comes to the fillet's relationship to draft and shell features. If the fillets are all grouped into a single feature, then controlling this relationship becomes impossible.

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 7.35 shows the resulting geometry from both settings.

Figure 7.35. The Round corners option, both on and off

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 7.36 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.

Figure 7.36. The Keep edge option and the Keep surface 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 7.37.

Figure 7.37. The Keep Feature option, both selected and unselected

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 7.38 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 7.38. 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:

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 7.39 shows the Variable Radius Parameters panel.

Figure 7.39. 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. Figure 7.40 shows a part with two zero-radius values.

Figure 7.40. Zero-radius values in the variable radius fillet

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 7.41.

Figure 7.41. Straight versus smooth transitions of a 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.

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 7.44 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 7.44. Using curvature combs to evaluate transitions

In Comparison to Figure 7.45, 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.

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 7.45 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.

Figure 7.45. Using a Help Point with a Face Fillet

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.

A single hold line fillet is a form of variable radius fillet, but instead of it being defined using the variable radius fillet type, it is created using the face 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 7.46 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.

Figure 7.46. Single hold line fillets

You can select the Hold line in the Fillet Options panel of the Face Fillet PropertyManager, as shown in Figure 7.47. 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 7.47. The PropertyManager interface for the hold line face 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 7.48.

Figure 7.48. A double hold line uses a spline, not an arc.

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. Figure 7.49 shows examples of the double hold line 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 7.50 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 CD-ROM as Chapter 7 Constant Width.sldprt.

Figure 7.49. Examples of the double hold line fillet

Figure 7.50. The constant width fillet

Scribe is the simplest of the options to explain, and understanding it can help you understand the other options. Scribe creates a split line-like edge on the face.

Several requirements must be met in order to make a wrap feature work:

Scribes can be created on solid or surface faces. Scribed surfaces are frequently thickened to create a boss or a cut.

The Wrap Emboss option works much like the scribe, but it adds material inside the closed loop sketch, at the thickness that you specify in the Emboss PropertyManager. Embossing can only be done on solid geometry. If the feature self-intersects, then the intersecting area is simply not embossed, and is left at the level of the original face. One result is that creating a full wrap-around feature, such as the geometry for a barrel cam, requires a secondary feature. This is because the Wrap feature always leaves a gap, regardless of whether the sketch to be wrapped is under or over the diameter-multiplied-by-pi length.

When you use the Emboss option, you can set up the direction of pull and assign draft so that the feature can be injection molded. This limits the size of the emboss so that it must not wrap more than 180 degrees around the part.

Deboss is just like emboss, except that it removes material instead of adding it. Figure 7.58 demonstrates all these options. The part shown in the images is available on the CD-ROM with the filename Chapter 7 Wrap.sldprt. For each of the demonstrated cases, the original flat sketch is shown to give you some idea of how the sketch relates to the finished geometry.

Figure 7.58. The Wrap feature options

Keep in mind that this feature is not like the projected sketch. A projected sketch is not foreshortened on the curved surface, but is projected normal from the sketch plane. A sketch that is one-inch long will measure one-inch along the curvature of the surface and will measure less than one inch linearly from end to end.

The scribed part in the previous figure was created on a conical surface body. The surface was then thickened as a separate body and patterned.

Cross-Reference

Chapter 26 covers working with multi-bodies, and Chapter 27 covers surfaces.

The embossed cam employed a workaround with a revolve feature to close the gap that is always created when wrapping all the way around a part.

The example with the debossed text employs a direction of pull and draft so that the geometry can be molded.

The Point deform option enables you to push a point on the model, and the model deforms as if it were rubber. Figure 7.62 shows the PropertyManager, as well as a before-and-after example of the Point deform function. The key to using this feature is to ensure that the Deform region option is unselected. Aside from that, you just have to use trial and error when applying the Point deform option. The depth, diameter, and shape of the deformation are not very precise. Also, you cannot specify the precise location for the point to be deformed. Again, this is best used for "looks-like" models, not production data.

Figure 7.61. The PropertyManager interface for the Curve to curve deform

Figure 7.62. The Deform Point PropertyManager and a before-and-after example

In the model from Figure 7.62, two Point deform features are used, one to apply some shape to the back and one to apply some shape to the seat.

Because the Curve to curve uses curve (or sketch or edge) data, it is a more precise method than the other deform types. The main concept here is to transform a curve on the original model to a new curve, thus deforming the body to achieve the new geometry.

The model shown in Figure 7.63 has been created using the Curve to curve deform. The part starts as a simple sweep (sweep an arc along an arc), and then a split line is created to limit the deform to a specific area of the model. The model is on the CD-ROM with the filename Chapter 7 Deform Curve to Curve.sldprt.

Figure 7.63. Using the Curve to curve deform option

I do not go into much detail on the Surface push deform type because it is not one of the more useful functions in SolidWorks. In order to use it, you must have the body of the part that you are modeling, and a tool body that you will use to shape the part that you are modeling. The finished shape does not fit the tool body directly, but looks about half-way between the model and the tool body, blended together in an abstract sort of way. It looks like the dent that would result from an object being thrown very hard at a car fender, in that neither the thrown part nor the fender is immediately recognizable from the result.