Symmetry is an important aspect of design intent. Taking advantage of symmetry can significantly reduce the time needed to model the part. Symmetry can exist on several levels:

This is probably the most important question. Primary or functional features include how the part mounts or connects to other parts, motion that it needs to accommodate, and additional structure to support loads.

Often it is a good idea to create a special sketch as the first feature in the part that lays out the functional features. This could be as simple as a straight line to denote the bottom and a circle to represent the position and size of a mating part, or as complex as full outlines of parts and features from all three standard planes. This technique is called a layout sketch, and it is an important technique in both simple and complex parts. You can use layout sketches for anything from simply drawing a size-reference bounding box to creating the one point of reference for all sketched features in the part. You can use multiple layout sketches if a single sketch on one plane is not sufficient.

When the marketing department gets out of their meeting at 4:45 pm, what changes do you need to be prepared for so that you can still be out the door by 5:00 pm? No one expects you to be able to tell the future, but you do need to model in such a way that your model easily adapts to future changes. As you gain experience with the software and keep this idea in mind, you will develop some instincts for the type of modeling that you do.

Modeling for the casting process is very different from modeling for the machining process. When possible, the process should be evident in your modeling. There are times when you will not know which process will be used to create the part when you start to create a model. If you are simply making an initial concept model, you may not need to be concerned about the process. In these cases, it may or may not be possible to reuse your initial model data if you need to make a detailed cast part from your non-process-specific model. Decisions like this are usually based on available time, how many changes need to be made, and a determination of the risk of making the changes versus not making the changes as well as which decision will cost you the most time in the long run.

Sometimes it makes sense to allow someone else to add the manufacturing details. A decision like this depends on your role in the organization and your experience with the process compared with that of other people downstream in the manufacturing process. For example, if you are not familiar with the Nitrogen Gas Assist process for molding polypropylene, and you are modeling a part to be made in that process, you might consider soliciting the help of a tooling engineer or passing the work on to someone else to add engineering detail.

Best Practice

As engineers, we are typically perfectionists. However, there always needs to be a balance between perfection and economy. Achieving both simultaneously is truly a rare event. Still, you should be aware that problems left by the designer for other downstream applications to solve (such as machining, mold making, and assembly) also have an impact on the time and cost of the project.

The best practice in this case is a judgment call. When faced with assembling a model sloppily or remodeling it perfectly, I usually choose to remodel because doing it the second time is always faster. In addition, if additional changes are required, you do not need to struggle with the sloppily assembled model. You can easily copy sketches from one part to another, while keeping the old part open as you build the new part. As a result, you may be surprised how quickly things go.

When working with any manufacturing process, some secondary processes are generally required. For example, if you have a cast part, you may need to machine the rough surface to create a flat face in some areas. You may also need to ream or tap holes. In plastic parts, you may need to press in threaded inserts.

SolidWorks includes special tools you can use to document secondary operations:

Sometimes size-based versions of parts have to be created or versions based on additional features. If these are simple, they can also be handled with configurations, but you need to plan this flexibility in advance.

The first feature that you create should be positioned relative to the Origin. Whether there is a corner of a rectangle that is coincident to the Origin, the rectangle is centered on the Origin, or dimensions are used to stand the rectangle off from the Origin at some distance, you need to lock the first feature to the Origin with every part you build.

When working with a simple part, the entire part can usually be described as rectangular or cylindrical. In cases like these, it is easy to know where to start: you simply draw a rectangle or a circle, respectively. On complex parts, it may not be obvious where to start, and the overall part cannot be said to have any simple shape. In cases like these, it may be best to select the (or a) prominent feature, mounting location, functional shape, or focus of the mechanism. For example, if you were to design an automobile, what would you designate as the 0,0,0 Origin? The ground might be a reasonable location as would the plane of the centers of the wheels. As long as everyone working on the project agrees, many different reference points could work. With that in mind, it seems logical to start the rectangular part by sketching a rectangle. Select the Top plane and sketch a rectangle centered on the part Origin.

Your next decision is about part symmetry. This part is not completely symmetrical: modeling a quarter of it and mirroring the entire model twice is not going to be the most effective technique. Instead, you should build the complete part around the Origin and mirror individual features as appropriate. To start this type of symmetry, you need to sketch a rectangle centered on the Origin. The centered rectangle is something that you will create frequently.

Figure 4.2 shows a centerpoint rectangle that has been sketched with the centerpoint at the part Origin. This creates symmetry in both directions. You can use additional construction geometry and sketch relations to make the rectangle only symmetrical side to side.

Best Practice

If you are dimensioning a horizontal line, the best way to do it is to simply select the line and place the dimension. Selecting the line endpoints can also work, but selecting the vertical lines on either side of the horizontal lines is not as robust. The problem is that if you use this third method, deleting either of the vertical lines causes the dimension to be deleted. In the first two dimensioning methods, dimensions are not deleted unless you remove one of the endpoints, which requires deleting two lines: the horizontal line and one of the vertical lines.

Figure 4.2. Using a center point rectangle to build symmetry about the Origin

One of the attractive things about Instant 3D is that it allows you to make changes to parts quickly without any consideration for how the part was made. For example, the cylindrical part was made from a series of extrudes, with a hole cut through it with draft on the cut feature. The flat faces can be moved, and the cylindrical faces offset. Behind the scenes, SolidWorks figures out which sketches or feature parameters of which features have to be edited. This saves you time searching the FeatureManager to figure out which features or sketches control a given face. As you work through more complex parts, you will see how handy this can be at times. You can activate or deactivate Instant 3D using the icon on the Features toolbar.

Figure 4.3. Using Instant 3D and Live Section

Instant 3D also offers a tool called Live Section. Live Section enables you to section a part with a plane, and you can drag the edges of the section regardless to which features the edges belong. To activate Live Section, right-click a plane that intersects the part and select Live Section Plane.

Instant 3D can also be an effective tool when used in conjunction with the direct editing type of tools such as Move Face. In fact, Instant 3D mimics some of the direct edit type of functionality found in applications such as Sketchup and Spaceclaim.

Chapter 30 discusses the direct edit theme in more detail, and revisits the Instant 3D manipulators in that light.

Going back to the sketch in Figure 4.2, I will show you how to continue building the part using the newly learned tools. By centering the sketch on the Origin and extruding by using a Mid Plane end condition, the initial block is built symmetrically about all three standard planes, with the part Origin at the center. In many parts, this is a desirable situation. It enables you to create mirrored features using the standard planes, and helps you to assemble parts together in an assembly later, when parts must be centered and do not have a hard face-to-face connection with other parts. Figure 4.4 shows the initial feature with the standard planes.

Figure 4.4. An initial extruded feature centered on the standard planes

The next modeling step is to create a groove on the back of the part. How is this feature going to be made? You can use several techniques to create this geometry. List as many techniques as you can think of, whether or not you know how to use them. Later, I will go through several techniques that work.

Figure 4.5 shows multiple methods for creating the groove. From the left to the right, the methods are a thin feature cut, a swept cut, and a nested loop sketch.

Figure 4.5. Methods for creating the groove

With a thin feature cut, you sketch the centerline, and in the Cut-Extrude feature, select the Thin Feature option and assign a width and depth. The option on the right is what is called a "nested loop," because it has a loop around the outside of the slot and another around the inside. Only the material between the loops is cut away. The method in the center is a sweep where the cross section of the slot is swept around a path to make the cut.

Another potential option could include a large pocket being cut out, with a boss adding material back in the middle. Each option is appropriate for a specific situation. The thin feature cut is probably the fastest to create, but also the least commonly used technique for a feature of this type. Most users tend to use the nested loop option (one loop inside another).

Hole Wizard

The next features that you will apply are a pair of counterbored holes. SolidWorks has a special tool that you can use to create common hole types, called the Hole Wizard. The Hole Wizard helps you to create standard hole types using standard or custom sizes. You can place holes on any face of a 3D model or constrain them to a single 2D plane or face. A single feature created by the Hole Wizard may create a single or multiple holes, and a feature that is not constrained to a single plane can create individual holes originating from multiple faces, non-parallel, and even non-planar faces (holes may go in different directions). All holes in a single feature that you create by using the Hole Wizard must be the same type and size. If you want multiple sizes or types, you must create multiple Hole Wizard features.

To apply counterbored holes to your part, follow these steps:

1. 
   

   Figure 4.10. The Hole Wizard Hole Specification interface

2. Next, click to select the Positions tab at the top of the PropertyManager. This is where you place the centerpoints of the holes using sketch points. It is often useful to create construction geometry to help line up and place the sketch points. Make sure the plane or face that the holes originate from is selected in the Positions tab.

3. Draw two construction lines, horizontally across the part, with Coincident relations to each side. Select both lines and give them an Equal relation. The point of this step is to evenly space holes across the part without dimensions or equations.

   Tip

   Although several methods exist to make multiple selections, a box or window selection technique may be useful in this situation. If the box is dragged from left to right, only the items completely within the box are selected. If the box is dragged from right to left, any item that is at least partially in the box is selected.

   Tip

   SolidWorks displays an error if you try to place a sketch point where there is an existing sketch entity endpoint. If you build construction geometry in a sketch and want to place a sketch point at the end of a sketch entity, you have to create the sketch point to the side where it does not pick up other incompatible automatic sketch relations, and then drag it onto the endpoint.

4. Place sketch points at the midpoint of each of the construction lines. If there is another sketch point other than the two that you want to make into actual holes, delete the extra points. Dimension one of the lines down from the top of the part, as shown in Figure 4.11. All the sketch relation icons display for reference. Click OK to accept the feature once you are happy with all the settings, locations, relations, and dimensions.

Figure 4.11. Placing the centerpoints of holes

Cutting a slot

The Hole Wizard does not specifically enable you to cut slots. However, SolidWorks has Slot sketch entities or you can use one of the following methods to cut a slot:

• 

• Explicitly drawing the slot. Draw a line, press A to switch to the Tangent Arc tool, draw the tangent arc, and press A to switch back to the Line tool, and so on. Although you can press the A key to toggle between the line and arc functions, you can also toggle between a line and a tangent arc by returning the cursor to the line/arc first point.

• Rectangle and arcs. Draw a rectangle, place a tangent arc on both ends, and then turn the ends of the rectangle into construction entities.

• Thin feature cut. As you did earlier with the groove, you can also create a Thin Feature slot, although you need to follow additional steps to create rounded ends on it.

• Offset in Sketch. By drawing a line, and using the Offset with Bi-directional, Make Base Construction, and Cap Ends settings, it is easy to create a slot from any shape by drawing only the centerline of the slot.

• Library feature. A library feature can be stored and can contain either simple sketches or more complex sets of combined features. The library feature is a good option for the counterbored slot used in this example. Library features are discussed in depth in Chapter 19.

Hole Wizard: Using 2D versus 3D sketches

Hole Wizard holes use either a 2D or a 3D sketch for the placement of the hole centers. You can define the centers by simply placing and dimensioning sketch points. Starting with SolidWorks 2010, the 2D sketch type is used by default, with the 3D sketch type only being used when you specify it in the Positions tab of the Hole Wizard tool.

Cross-Reference

In Chapters 17 and Chapter 31, 3D sketches are discussed. Chapter 17 also gives a more detailed description of the Hole Wizard. Chapter 22 has additional information on the display of threads.

The following image shows a part with various types of holes created by the Hole Wizard, including counterbored, countersunk, drilled, tapped, and pipe-tapped holes. The part is shown in section view for clarity; however, the drilled hole is not shown in the figure.

Holes created by the Hole Wizard

To cut slots in your part, follow these steps:

1. In this case, use the Centerpoint Straight Slot option. Slots are easiest to create with the Click-click method rather than Click+drag. Click near where you want the center of the slot. Click again for the center of one end; then click a third time for the width/end radius. The Slot PropertyManager is shown in Figure 4.12.

   Create a horizontal sketch relation between the origin and the center point of the slot. Add dimensions as shown in Figure 4.12.

Note

Using the Add dimensions option in the Slot PropertyManager can help you size the slot more quickly. This does not require the Enable on screen numeric input option to be turned on.

1. From this sketch, create an extruded cut that extrudes up to the surface of the counterbore in the holes. The through hole for the counterbored slot is also a slot, and so you can use the same technique.

   

   Figure 4.12. Creating a slot

2. Open a sketch on the bottom of the previous slot, and draw a straight slot. Make the new slot 0.05 inch smaller than the first slot. You can create a cut using the Through All end condition.

Tip

Picking up relations automatically may seem difficult at first, but with some practice, it becomes second nature. When trying to find the center of an arc, the centerpoint is usually displayed and is easy to select. However, when making a relation to an edge, the centerpoint does not display by default. To display it, hold the cursor over the arc edge for a few seconds; a marker that resembles a plus sign inside a circle will show you where the center is, thus enabling you to select it with a sketch tool and pick up the automatic relations.

In Figure 4.13, the first centerpoint has already been referenced, and the cursor is trying to find the centerpoint of the other end of the slot.

Fillets and chamfers

As mentioned earlier, it is considered a best practice to avoid using sketch fillets when possible, using feature fillets instead. Another best practice guideline is to put fillets at the bottom of the design tree, or at least after all the functional features. You should not dimension sketches to model edges created by fillets unless there are no better methods available. Several chapters could be written just about fillet types, techniques, and strategies in SolidWorks. Chapter 7 deals with more complex fillet types.

Best Practice

Do not dimension sketches to model edges that are created by fillets. While the previous best practice about relations to sketch entities instead of model edges was a mild warning, you must heed this one more carefully.

Figure 4.13. Applying automatic relations to a circular edge

To add fillets and chamfers to your part, follow these steps:

1. Initiate a Fillet feature, and select the four short edges on the part. Set the radius value to .600 inches. Click OK to accept the Fillet feature.

Tip

When selecting edges around a four-sided part, the first three edges are usually visible and the fourth edge is not. You can select invisible edges by expanding the Fillet Options panel of the Fillet PropertyManager, and selecting the Select through faces option. When you have a complex part with many hidden edges, this setting can be bothersome, but in simple cases like this, it is useful. Figure 4.14 shows this option in action.

1. Apply chamfers to the edges of the angled slot through the part, as indicated in Figure 4.15. Make the chamfers .050 inches by 45 degrees.

   Chamfers observe many of the same best practices as fillets.

Tip

Feature order is important with features like chamfers and fillets because of how they both tend to propagate around tangent edges. Although you can turn this setting off for both types of feature, it is best to get the correct geometry by applying the features in order.

Cross-Reference

The Fillet Xpert, which helps you to manage large numbers of overlapping fillets by automatically sorting through feature order issues, is discussed in detail in Chapter 27.

Figure 4.14. Selecting an edge through model faces

1. Select the four edges that are indicated for fillets in Figure 4.15. Apply .050-inch-radius fillets.

2. Apply a last set of .050-inch chamfers to the backside of the counterbores and slot.

The finished part is simple, but you have learned many useful techniques along the way. In the rest of this chapter, you will put the part together with other parts to form an assembly and then create a quick 2D drawing of the part and the assembly to document the design.

Figure 4.15. Edges for fillet and chamfer features