CHAPTER 4

Creating Simple Parts and Drawings

Good modeling practice is based on robust design intent. This just means that you should try to build parts that can adapt easily to changes. This section of the book begins with questions that you need to ask to make good models.

Beginning to create simple parts will help you understand techniques used in more complex modeling projects. Learning on simple tools and then expanding your skills helps you to understand best practice issues, which makes you a better contributor to a team environment.

Discovering Design Intent

By asking questions about the part's function before you start modeling or designing, you can create a model that will be easier to edit, easier to properly place into an assembly, easier to detail in drawings, and easier for other SolidWorks users to understand when someone else has to work on your models. Whether you are doing the modeling for someone else or doing the design and modeling for yourself may make a difference in how you approach the modeling task.

The purpose of these questions is to help you establish design intent. The term design intent is a statement of how the part functions and how the model reacts to modeling changes.

It may help if you try to put the design intent into words to help you focus on what is important in the design. An example of a statement of design intent is “This part is symmetric about two planes, is used to support a 1.00” diameter shaft with a constant downward load of 150 pounds using a bronze bushing, and is bolted to a plate below it.” This does not give you enough information to design the part, but it does give you information about two surfaces that are important (a hole for the bushing and the bottom that touches the mounting plate), as well as some general size and load requirements. The following questions can help you develop the design intent for your own projects.

Using symmetry

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:

• Sketch symmetry
• Individual feature symmetry
• Whole-part symmetry
• Axial symmetry (a revolved part)
• “Almost” symmetry (the whole part is symmetrical, except for a few features)
• Left and right symmetrical versions of the part
• Assembly symmetry

Determining primary or functional features

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.

Predicting change

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 engineering design processes, keep this idea in mind; you will develop some instincts for the type of modeling that you do.

Determining the manufacturing method

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.

Identifying secondary operations

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:

• Configurations. This SolidWorks technique enables you to create different versions of a part. For example, one configuration may have the features for the secondary operations suppressed (turned off) and showing just the part as cast, while the other configuration shows the part as machined.

• Insert Part. This SolidWorks technique enables you to use one SolidWorks part as the starting point for a second part. For example, the as-cast part has all the features to make the part, but it is inserted as the first feature in the as-machined part, which adds the cuts required by the machining process.

Creating multiple versions

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.

Creating a Simple Part

You need to practice some of the skills you will learn on simple parts. Chapter 2 introduced the tools and features you will use, and this chapter teaches you how to string the simple features together intelligently. In this section, I'll show you how to build the simple part shown in Figure 4.1. While the shape is simple, the techniques used and discussed here are applicable to a wide variety of real-world parts. The discussion on how to model the part contains information on some of the topics you need to understand in order to do the work.

FIGURE 4.1 A simple machined part

Deciding where to start

Deciding where to start can be more difficult than it sounds, especially for new users. For this reason, I will go through some sample parts and discuss possible starting points. Figure 4.2 shows the first part. For reference, all of these parts are found on the DVD included with this book.

FIGURE 4.2 Deciding where to start

When you are trying to decide how to model geometry in SolidWorks, you should be thinking of a 2D shape and a process. You typically create prismatic shapes by using an Extrude feature and round shapes by using a Revolve feature. Features can also add material (boss) or remove material (cut). Obviously, your first feature has to add material.

If you look at the 3D geometry and see it as a series of 2D drawing views arranged in 3D space (as shown in Figure 4.2), you are on your way to deciding where to start.

The part in Figure 4.2 has flat and round faces, but if you examine it, you can create the overall shape using a single extrude. The best option in this case would be to start with a sketch like the one in the lower-right corner, and extrude it. This is a good beginning. Although you can make the same part starting from any of the three sketches, the one in the lower-right corner gets you closest to the final shape.

Also realize that you don't need to make all of the geometry in a single feature. It is often best to use multiple features for elements such as holes, fillets, chamfers, and other groups of geometry that can be separated out from the main shape.

You might look at the part and see many ways to create it, but the most straightforward way is to use a main extrude, a rectangular cutout, and four chamfers, as shown in Figure 4.3.

FIGURE 4.3 Breaking down the features in this part

Also notice where the part is placed in relation to the Origin. Different people might do this differently, and the same person might even do it differently depending on the function of the part. In this case, the Origin is aligned with the center of the round shape and at the bottom of the flat face. The placement of the Origin suggests that this part sits on the flat face of another part and may hold a cylindrical face of another part.

If you open the part from the DVD, you will notice that the Origin is also placed in the middle of the extrusion depth. This suggests that the part is symmetrical from front to back.

If you are new to 3D modeling, this might be a lot to take in all at once, but you should try to keep the ideas presented here in mind as you work through your first several parts, or when you examine SolidWorks parts made by more-experienced users.

FIGURE 4.4 shows another part with other features. Again, you can choose from several ways to make this part.

FIGURE 4.4 Identify the best starting point for this part.

In this case, the best option is to use the one on top. This is because the other two profiles would add geometry that you would have to remove later. Notice that the holes in the part are not represented in any of the profiles. This is because holes are often added as separate features later.

Returning to the part in Figure 4.1, it should be clear enough that this part would be best started from a rectangle, although the rectangle could come from any of the three directions. I personally try to use the biggest sketch that will create a solid that requires the fewest number of cuts. The first feature that you create should also 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 sometimes 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 centerpoint rectangle centered on the part Origin.

Building in symmetry

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.

Figure 4.5 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.

FIGURE 4.5 Using a centerpoint rectangle to build symmetry about the Origin

Beginning with the rectangle you sketched in the previous section, apply one horizontal dimension by clicking the Smart Dimension tool on a single horizontal line, placing the horizontal dimension (4.00 inches), by clicking a vertical line, placing the vertical dimension (6.00 inches). The sketch is fully defined at this point because both the size and position of the rectangle have been established.

Making it solid

Next, click Extrude in the Features toolbar or choose Insert Boss/Base Extruded. In the Direction 1 panel, select Mid Plane as the end condition. SolidWorks takes the distance that you entered and extrudes it symmetrically about the sketch plane. Enter 1.00 inch as the distance.

Extrude Feature Options

The Extrude feature is one of the staples of SolidWorks modeling. Depending on the type of modeling that you do, the Extrude feature may be one of your main tools.

The Extrude interface

Extruding from a selection

The From panel establishes where the Extrude feature starts. By default, SolidWorks extrudes from the sketch plane. Other available options include:

• Surface/Face/Plane. The extrude begins from a surface body, a face of a solid, or a reference plane.
• Vertex. The distance from the sketch plane to the selected vertex is treated as an offset distance.
• Offset. You can enter an explicit offset distance, and you can change the direction of the offset.

Extruding from a surface

Cross-Reference

Surface features are discussed in detail in Chapter 20.

Understanding Direction 1 and Direction 2

Direction 1 and Direction 2 are always opposite one another. Direction 2 becomes inactive if you select Mid Plane for the end condition of Direction 1. The arrows that display in the graphics window show a single arrow for Direction 1 and a double arrow for Direction 2. For the Blind end condition, which is described next, dragging the arrows determines the distance of the extrude.

Each of the end conditions is affected by the Reverse Direction toggle. This toggle simply changes the default direction by 180 degrees. You need to be careful when using this feature, particularly when using the Up to end conditions, because if the entity that you are extruding up to is not in the selected direction, an error results.

Following is a brief description of each of the available end conditions for the Extrude feature:

• Blind. Blind in this case means an explicit distance. The term is usually used in conjunction with holes of a specific depth, although here it is associated with a boss rather than a hole.
• Up to Vertex. In effect, Up to Vertex works just like the Blind end condition, except that the distance is parametrically controlled by a model vertex or sketch point.
• Up to Surface. Up to Surface could probably be better named Up to Face, because the end does not necessarily have to be an actual surface feature. This end condition may display a warning if the projection of the sketch onto the selected face extends beyond the boundary of the face. In that case, it is advisable to knit several faces together into a surface body and to use the Up to Body end condition.
• Offset from Surface. By default, Offset from Surface extrudes until it reaches a specified distance from a selected surface. There are two methods for determining the type of offset and one to determine direction.
  • The default offset method behaves as if the selected surface were offset radially, so that a surface with a 4-inch radius and a 1-inch offset would give a curvature on the end of the extrude of a 3-inch radius.
  • The second method, called Translate Surface, behaves as if the surface were moved by the offset distance.
  • Reverse Offset refers to when the offset stops short of the selected face or when it goes past it.
• Up to Body. The Up to Body end condition is very useful in many situations, especially when receiving the error message, “The end face cannot terminate the extrusion,” from the Up to Surface end condition.
• Mid Plane. The Mid Plane end condition eliminates the Direction 2 options and divides the extrude distance equally in both directions; for example, if you specify a 1.00-inch Mid Plane, SolidWorks extrudes .50 inches in one direction and .50 inches in the other direction.
• Through All. The Through All end condition is available only when there is already solid geometry existing in the part. When used for an extruded boss (which adds material), it extrudes to the distance of the farthest point of the solid model in a direction perpendicular to the sketch plane. When used for a cut, it simply cuts through everything.

  

  Offset from surface using the default and Translate Surface options

  

  The Reverse Offset option

• Up to Next. Up to Next extrudes the feature until it runs into a solid face that completely intercepts the entire sketch profile. If a portion of the sketch hangs over the edge of the face, the extrude feature will keep going until it runs into a condition that matches that description, which may be the outer face of the part in the direction of the extrusion.

The Up to Next end condition used with a Cut extrude

By default, the Direction of Extrusion is normal to the sketch plane, but you can also select a linear entity such as an edge or axis as the direction. All the end-condition options are still available when you manually define the Direction of Extrusion as something other than the default.

You can also assign a draft option to an extrusion as it is created, and you can control the draft separately for Direction 1 and Direction 2.

Best Practice

When dealing with molded or cast parts, certain types of features, such as draft, fillets, and shells, are often the targets of users trying to assign best practices. This is partially because using draft, fillets, and shells is very much like playing Rock, Paper, Scissors; the only way to win this game is by luck. Arranging the features in the correct order so that the model is efficient and achieves the desired results is challenging. It is usually best to apply draft as a separate feature rather than using it in the definition of the Extrude feature. It is also best to apply draft after most of the modeling is done, but before you apply the cosmetic fillets and before you use the shell feature.

Using the Thin Feature Panel

The Thin Feature panel is activated by default when you try to extrude an open loop sketch (a sketch that does not fully enclose an area). The end-condition options remain the same. What changes is the feature applies a thickness to the sketch elements in the manner of a sheet metal part, thin-walled plastic part, or a rib. The Thin Feature panel of the Extrude PropertyManager, along with a representative thin feature extrusion.

The Thin Feature panel and a thin feature extrusion

The Cap Ends option is available only when you specify a Thin Feature to be created from a closed loop sketch. This creates a hollow, solid body in a single step. You can also use Thin Features with cuts, and they are very useful for creating slots or grooves.

Using contour selection

Contour selection enables you to select areas completely bounded by sketch entities for use with features such as Extrude. For example, you could use a sketch like the number sign (#). You can use contour selection to select the box in the center, which is completely bound by sketch elements. The image below shows an extrude feature making use of contour selection in a sketch.

Using contour selection

The part used in the above image is on the DVD, and is called Chapter 4 — Contour Selection.sldprt.

SolidWorks works best when the sketches are neat and clean, when nothing overlaps, and when no extra entities exist. However, when you need to use a sketch that does not meet these criteria, you can use this alternative method.

Best Practice

I believe this feature was introduced into SolidWorks only to keep up with other CAD packages, not because it is a great feature. I do not recommend using contour selection on production models. It is useful for creating quick models, but the selection is too unstable for data that you may want to rely on in the future. The main problem is that if the sketch changes, the selected area may also change, or SolidWorks may lose track of it entirely.

Using Instant 3D

Instant 3D enables you to pull handles to create extrusions and to drag model faces to change the size and location of features. Several feature types enable you to use arrows to adjust elements visually of parametric features and sketches. The function largely replaces and expands on the older functionality called Move/Size Features. Figure 4.6 shows the arrows added by Instant 3D, which are the handles that you pull on to create a solid from a sketch or edit an existing feature. Notice also that you can make cut features with Instant 3D. In fact, you can change a boss feature into a cut. I'm sure this is a neat sales demo trick, but I'm not aware of any practical application of changing a boss into a cut.

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.

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. Live Section is shown on the cylindrical part in Figure 4.6.

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

FIGURE 4.6 Using Instant 3D and Live Section

Making the first extrude feature

Going back to the sketch in Figure 4.5, 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 4.7 shows the initial feature with the standard planes.

FIGURE 4.7 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 4.8 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 4.8 Methods for creating the groove

With a thin feature cut, you sketch the centerline of the groove, 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).

Controlling relative size or direct dimensions

You can control the size of the groove as an offset from the edges of the existing part or you can drive the dimensions independently. Again, this depends on the type of changes you anticipate. If the groove will always depend on the outer size of the part, the decision is easy — go with the offset from the outside edges. If the groove changes independently from the part, you need to re-create dimensions and relations within the sketch to reflect different design intent.

Creating the offset

You need to consider one more thing before you create the sketch. What should you use to create the offset — the actual block edges or the original sketch? The answer to this is a Best Practice issue.

To create the offset for your part, follow these steps:

1. Open a sketch on the face of the part. To create the offset, expand the Extrude feature by clicking the plus icon next to it in the FeatureManager so that you can see the sketch. Regardless of how it displays here, this sketch appears before the extrude in the part history. Right-click the sketch and select Show.

   Tip

   You can view individual sketches and reference geometry entities such as planes from the RMB menu. The global settings for the visibility of these items are found in the View menu. You can access these items faster by using the View toolbar, or by linking the commands to hotkeys.

2. Right-click the sketch in the graphics window and click Select Chain. This selects any non-construction, end-to-end sketch entities. Click Offset Entities on the Sketch toolbar. Offset to the inside by .400 inches. Apply .500-inch sketch fillets to each of the corners.
3. Click Extruded Cut on the Feature toolbar. By default, the extruded cut will cut away everything inside the closed profile of the sketch. Look down the FeatureManager window and select the check box on the top bar of the Thin Feature panel. Make the cut Blind, .100 inch. The Thin Feature type should be set to Mid Plane with a width of .400 inches. The PropertyManager and graphics window should look like Figure 4.9.

FIGURE 4.9 Creating the groove with a thin feature cut

Using sketch techniques

Although you could create the next two features more easily and efficiently using a cut, I will show you how to create them as two extrudes. The intent here is to show some useful sketch techniques rather than optimum efficiency. Begin with the part from the previous section and follow these steps:

1. Open a new sketch on the large face opposite from the groove. Draw a corner rectangle picking up the automatic coincident relation to one corner and then dragging across the part and picking up another coincident to the edge on the opposite side. Figure 4.10 shows the rectangle before and after this edit.

   Tip

   If you want to continue using the recommended best practice mentioned earlier of making relations to sketches rather than model edges, here are a few tips. In some situations (such as the current one), the sketch plane is offset from the sketch that you want to make relations to, and the best bet is to use the Normal To view. The next obstacle is making sure that automatic relations pick up the sketch rather than the edge, and so you can use the Selection Filter to select sketch entities only.

2. Delete the Horizontal relation on the line that is not lined up with an edge. This enables you to drag it to an angle or apply the dimensions shown in Figure 4.10.
3. Extrude sketch to a depth of 0.25 inch.

   You can delete the Horizontal relation by selecting the icon on the screen and pressing Delete on the keyboard. As a reminder, you can show and hide the sketch relation icons from the View menu. You can check to ensure that the relations were created to the sketch rather than the model edges by clicking the Display/Delete Relations button on the Sketch toolbar, clicking the relation icon to check, and expanding the Entities panel in the PropertyManager. The Entities box shows where the relation is attached to, as shown in Figure 4.11. In this case, it is a point in Sketch1. Without custom programming, there is no way to identify items in a sketch by name, but you already know which point it is; you just needed to know whether it was in the sketch or on the model. The second sketch trick involves the use of a setting.

   FIGURE 4.10 Edits to a rectangle

   

   FIGURE 4.11 The Display/Delete Relations dialog box

   

4. Choose Tools Options Sketch and ensure that Prompt to Close Sketch is turned on; then click OK to close the dialog box.
5. Open another new sketch on the same face that was used by the last extrusion. Draw an angled line across the left and bottom sides of the box with the dimensions shown in Figure 4.12. In this case, for this technique to work, the endpoints of the line have to be coincident with the model edges rather than the sketch entities.

   This line by itself constitutes an open sketch profile, meaning that it does not enclose an area and has unshared endpoints. Ordinarily, this results in a Thin Feature, as described earlier, but when the endpoints are coincident with model edges that form a closed loop and the setting mentioned previously is turned on, SolidWorks automatically gives you the option of using the model edges to close the sketch. This saves several steps compared to selecting, converting, and trimming manually.

   FIGURE 4.12 Using the prompt to close a sketch setting

   

6. Click the Extrude tool on the Features toolbar. Answer yes to the prompt, and double-click the face of the previous extrusion. SolidWorks automatically uses the face that you double-clicked for an Up to Surface end condition. This is a simple way of linking the depths of the two extrusions automatically. Again, this entire operation could have been handled more quickly and efficiently with a cut, but these steps demonstrate an alternative method, which in some situations may be useful.

Using the 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. Select the face that the groove feature was created on, and click the Hole Wizard tool on the Features toolbar. Then set the hole to Counterbored, set the type to Socket Head Cap Screw, the size to one-quarter, and the end condition to Through All, as shown in Figure 4.13.

   FIGURE 4.13 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 4.14. 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 4.14 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:

• Use one of the Slot sketch tools. SolidWorks has straight and arc slot options on the sketch toolbar.
• 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.

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 4.15.

   Create a horizontal sketch relation between the origin and the centerpoint of the slot. Add dimensions as shown in Figure 4.15.

   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.

2. 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.
3. 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.

FIGURE 4.15 Creating a slot

In Figure 4.16, the first centerpoint has already been referenced, and the cursor is trying to find the centerpoint of the other end of the slot.

FIGURE 4.16 Applying automatic relations to a circular edge

Creating 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.

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 4.17 shows this option in action.

   FIGURE 4.17 Selecting an edge through model faces

   

2. Apply chamfers to the edges of the angled slot through the part, as indicated in Figure 4.18. 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 20.

3. Select the four edges that are indicated for fillets in Figure 4.18. Apply .050-inch-radius fillets.
4. Apply a last set of .050-inch chamfers to the backside of the counterbores and slot.

FIGURE 4.18 Edges for fillet and chamfer features

The finished part is simple, but you have learned many useful techniques along the way.

Tutorial: Making a Simple Drawing

In SolidWorks, drawing views are created from the 3D model. Even the most complex section views are almost free, because they are simply projected from the 3D model. When you make changes to the 3D model, all 2D views update automatically. You can handle dimensions in a couple of ways, either using the dimensions that you used to create the model or placing new dimensions on the drawing (best practice for modeling is not necessarily the same as best practice for manufacturing drawings). To make a simple drawing of a SolidWorks native part, follow these steps:

1. Click the New button from the Standard toolbar or choose File New. From the New SolidWorks Document window, select the Drawing template. The template contains all the document-specific settings.
2. After selecting the drawing template, the Sheet Format/Size dialog box appears, as shown in Figure 4.19. Select the D-Landscape sheet size, as well as the format that automatically associates with that sheet size, and click OK. If the Model View PropertyManager appears, click the red X icon to exit.

   FIGURE 4.19 The Sheet Format/Size dialog box

   

3. Before creating any views on the drawing, set up some fields in the format to be filled out automatically when you bring the part into the drawing. Right-click anywhere on the drawing sheet (on the paper) and select Edit Sheet Format.
4. Zoom in to the lower-right corner of the drawing. Notice that there are several variables with the format $PRPSHEET:{Description}. These annotations are linked to custom properties. Some of them have properties with values (such as the Scale note), and some of the properties do not have values (such as the Description).
5. Add an annotation in the Drawn row, in the Date column. You can add annotations by choosing Insert Annotations Note, or by activating the Annotations toolbar in the CommandManager and clicking the Note button. Type today's date as the text of the note.

   Caution

   If you are using a SolidWorks default template and a circle appears around your note, and then use the Text Format PropertyManager that appears when you are creating a note, expand the Border panel, and change the Circle option to None.

6. Add another note, this time to the Name column. Do not type anything in the note, but click the Link to Properties button in the Note PropertyManager to create a link to a custom property. In the Link to Property dialog box, click the Model in View Specified option in Sheet Properties. Type user in the drop-down text box below the option. This now accesses a custom property in a part or assembly that is put onto this drawing and called “user,” and will put the value where the note is placed.
7. To return to Edit Sheet mode (out of Edit Format mode), select Edit Sheet from the RMB menu. A little text reminder message appears in the lower-right corner on the status bar to indicate whether you are editing the Sheet or the Format.
8. From the Drawings toolbar, click the Standard 3 View button, or through the menus, choose Insert Drawing View Standard 3 View. If the Chapter4SimpleMachinedPart document does not appear in the list box in the PropertyManager, then use the Browse button to select it. When you click the OK button, the three drawing views are created.
9. Drawing views can be sized individually or for each sheet. The Sheet Properties dialog box in Figure 4.20 shows the sheet scale. If this is changed, all the views on the sheet that use the sheet scale are updated. If you select a view and activate the Drawing View PropertyManager, you can use the Scale panel to toggle from Use Sheet Scale to Use Custom Scale.

   FIGURE 4.20 First angle versus third angle projections

   

   Caution

   In the United States, drawings are traditionally made and understood using the Third Angle Projection, which is the ANSI (American National Standards Institute) standard. In Europe, drawings typically use First Angle Projection, which is the ISO (International Organization for Standardization) standard. If you are not careful about making and reading your drawings, you could make a serious mistake. There are times when in the United States, the SolidWorks software will install with ISO standard templates, which will project views using First Angle Projection. When you're using a template that you are unfamiliar with, it is a good idea to check the projection method. To do this, right-click the drawing sheet and select Sheet Properties. The Type of projection setting appears in the top middle of the dialog box, as shown in Figure 4.20. This dialog box looks similar to the Sheet Format/Size dialog box, but it has some additional options, including the projection type.

10. To create an Isometric view, activate the Drawings toolbar in the CommandManager, and click the Projected View button. Then select one of the existing views, and move the cursor at a 45-degree angle. If you cannot place the view where you would like it to go, press the Ctrl key to break the alignment and place the view where you want it.
11. You can change the appearance of the drawing view in several ways.
    • View Display Tangent Edges with Font uses phantom line type for any edge between tangent faces.
    • View Display Tangent Edges Removed completely removes any tangent edges. This is not recommended, especially for parts with many filleted edges, because it generally displays just the outline of the part.
    • Shaded or Wireframe modes can be used on drawings, accessed from the View toolbar.
    • Perspective views must be saved in the model as a named view and placed in the drawing using the view name.
    • RealView drawing views are not available on a drawing except by capturing a screen shot from the model and placing this screen shot in a drawing. The same applies to PhotoWorks renderings.
12. Look at the custom properties that you created in the title block. The date is there because you entered a specific value for it, but the Name field is not filled in. This is because there is no User property in the part. Right-click the part in one of the views and select Open Part. In the part window, choose File Properties, and in the Property Name column, type the property name user, with a value of your initials, or however your company identifies people on drawings. The Properties dialog box, also called Summary Information, is shown in part in Figure 4.21.

    FIGURE 4.21 The Custom Properties entry table

    

    Cross-Reference

    When used in models and formats, Custom Properties are an extremely powerful combination, especially when you want to fill in data automatically in the format, in a BOM (Bill of Materials), or a PDM (Product Data Management) product. These topics are discussed in more detail in Chapter 14.

13. When you flip back to the drawing (using Ctrl+Tab), the Name column now contains the value of your initials.
14. Click the Section View button on the Drawings toolbar. This activates the Line command so that you can draw a section line in a view. When sketching, a line can go either on the Sheet or in a view. This is similar to the distinction between the Sheet and the Format. To make a section view, the section line sketch must be in the view. You will know that you are sketching in a view when a pink border appears around the view. You may also use Lock View Focus from the RMB menu to lock view focus manually.
15. Bring the cursor down to the circular edge of the slot to activate the centerpoint of the arc. Once the centerpoint is active, you can use the dotted inference lines to ensure that you are lined up with the center. Another option is to create manually sketch relations. Turning on temporary axes displays center marks in the centers of arcs and circles. Figure 4.22 shows the technique with the inference lines being used. Draw the section line through the slot and then place the section view.

    FIGURE 4.22 Creating a section view

    

16. As mentioned earlier, you can use two fundamentally different methods for dimensioning drawings:
    • Model Items imports the dimensions used to build the SolidWorks model and uses them on the drawing. These dimensions are bidirectionally associative, meaning that changing them on the drawing updates the model, and changing them on the model updates them in the drawing. On the surface of things, this sounds too good to be true, and it is. The potential problems are that you might not model things the way you would dimension them for the shop. You have to answer several questions for yourself, such as do the leader lines go to the right locations or can they be moved, and the dimensions usually come in in such a way that they require quite a bit of moving them around.
    • Reference (driven) Dimensions can be applied to the drawing view directly. These are only associative in one direction, meaning that they measure what is there, but they do not drive the size or position of the geometry. All changes must be made from the model. Again, on the face of things, this appears to be redundant and a waste of time, but in my personal estimation, by the time you finish rearranging dimensions, checking to ensure that you have everything you need and hiding the extraneous dimensions, you are usually far better off using reference dimensions.

      Best Practice

      Users have strong opinions on both sides of this issue. The best thing for you to do is to use both methods and decide for yourself.

17. If you choose to use the Model Items approach, you can do this by choosing Insert Model Items. Then specify whether the dimensions should come from the entire model or just a selected feature. You also need to ask whether the dimensions should come into all views or just the selected one, and whether you want just a certain type of dimension, annotation, or reference geometry.
18. Once the dimensions are brought in, you need to move some of them from one view to another, which you can do by Shift+dragging the dimension from the old location to the new location. Ctrl+dragging predictably copies the dimension. You can move views by dragging an edge in the view.

Summary

This chapter helps to lay the foundation for the more detailed information that will follow. The chapters in Part I include recommendations and answers to questions that help you to develop an intuition for how SolidWorks software operates, which is the most crucial kind of knowledge when troubleshooting a modeling or editing problem.

This chapter has glossed over many of the important details in order to give you a quick overview of the basic functionality in SolidWorks for the three main data types: Parts, Assemblies, and Drawings. Later chapters expand on this information significantly.