FIGURE 3.50
Creating the extrusion from the new sketch
Summary
Sketching in SolidWorks is something that you will do almost every time you open the software. A lot of automated functions are available that you can allow to do much of the work for you. You also have a lot of control to make changes manually. Remember that the best way to create most sketches is to use automatic relations when you can, sketch the approximate shape that you want to make, and then either drag it to pick up automatic relations, add dimensions, or add relations manually.
The options for creating intelligent relationships that establish your design intent, as well as SolidWorks’s capabilities in laying out mechanisms, is only limited by your imagination. The more familiar you become with the tools in your toolbox, the more of a craftsman you can become with this software.
Reference geometry is an essential part of creating and controlling relationships in any parametric model. Reference geometry is usually more stable than solid geometry, so sketch relations and dimensions should use reference geometry as references when possible.
Creating Simple Parts, Assemblies, and Drawings
IN THIS CHAPTER
Establishing design intent Building a simple part Creating a simple assembly
tutorial
Making a simple drawing tutorial
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 model effectively.
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 prop- erly 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
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.
Is the part symmetrical?
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:
l Sketch symmetry
l Individual feature symmetry
l Whole-part symmetry
l Axial symmetry (a revolved part)
l “Almost” symmetry (the whole part is symmetrical, except for a few features)
l Left and right symmetrical versions of the part
l Assembly symmetry
What are the 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 fea- tures from all three standard planes. This technique is called a layout sketch, and it is an impor- tant 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.
In what ways is the part likely to 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 keep this idea in mind, you will develop some instincts for the type of modeling that you do.
What is 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 pro- cess. 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 addi- tional 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. n
Will there be 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:
l 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.
Cross-Reference
Chapter 10 discusses configurations and feature suppression in depth. n
l 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.
Will there be other 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 flexibil- ity 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
The first feature that you create should be positioned relative to the Origin. Whether there is a cor- ner 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 cylin- drical. 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 log- ical to start the rectangular part by sketching a rectangle. Select the Top plane and sketch a rectan- gle 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.
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.
Tip
To make a rectangle work like a square, use an Equal sketch relation on two adjacent sides. This only requires a single dimension to drive the size of the square. n
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.
Best Practice
If you are dimensioning a horizontal line, the best way to do it is to simply select the line and place the dimen- sion. 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
FIGURE 4.2
Using a center point rectangle to build symmetry about the Origin
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.
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
Extrude feature options
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:
l Surface/Face/Plane. The extrude begins from a surface body, a face of a solid, or a reference plane.
Extruding from a surface
Cross-Reference
Surface features are discussed in detail in Chapter 27. n
l Vertex. The distance from the sketch plane to the selected vertex is treated as an offset distance.
l Offset. You can enter an explicit offset distance, and you can change the direction of the offset.