Using the Assembly Layout Sketch

In SolidWorks, layout sketches are a great way to simulate mechanisms or to locate the major components of an assembly. Figure 16.1 shows three examples of assemblies created with the assistance of an assembly layout sketch.

The bicycle example is used throughout this book, and the layout sketch was instrumental in establishing the geometry of the frame, wheels, and fork. Most of the components of a bicycle are purchased as off-the-shelf items that may come in different sizes but are not custom-created for individual bikes. The only parts that are generally custom-built for a particular size are the frame and possibly the fork. Therefore, to design the frame, you must lay out all the data that you are given for the individual components, such as wheels, stem, crank set, and seat. When you put everything together, additional pieces of information determine the frame geometry before the detail design of the frame can be started. You need to know the following:

• The size of the wheels
• The wheelbase (distance between the wheel centers)
• The length of the pedal arm
• The necessary clearance between the bottom of the pedal and the ground
• The head angle (effective pivot angle of the front fork)
• The distance between the center of the crank and the center of the rear wheel

The workflow for using an assembly layout sketch is as follows:

1. Open a new assembly.
2. Create sketches on the standard planes, or create new reference planes (you cannot use sketch pictures in assembly sketches).
3. Mate existing parts to the sketch and reference geometry (bottom-up method).

As previously mentioned, the assembly-level sketches from Chapter 15, “Patterning and Mirroring Components,” that we used to create chain patterns were assembly layout sketches used in a slightly different way. Alternatively, you can build parts in place using the layout sketches as references (top-down or in-context method).

First, you start with the wheels. In this example, you want to design an urban utility bike based on mountain bike components, with dual suspension, but using narrow tires, and that means 26-inch wheels. You need a certain amount of ground clearance as the pedals rotate, and you need clearance between the rider's toes and the back side of the front wheel. You will design the frame to fit a rider who is about 5-feet, 8-inches tall.

The size information is important because the distance between the wheel centers (wheelbase) creates certain characteristics for riders of different heights. A longer wheelbase generally means a more stable and comfortable ride, but the bike is less maneuverable and heavier. In this case, based on other research, you want the wheelbase to be 41 inches.

Those specifications allow you to create the sketch shown in Figure 16.2.

The next set of information you can put into the sketch has to do with the height of the top bar (which is important when you stand over the bike with your feet on the ground) and clearance between the frame and front wheel for the travel of the front suspension fork. This establishes most of what you need to know to design the frame, but you still have to work out the rear suspension arm.

With this information, the layout sketch looks like Figure 16.3.

With this data, you have all the critical point locations to design the actual frame. The first step in creating the frame is to place reference geometry (sketch planes) from which to make sketches for the individual tubes of the frame. The frame will be a carbon fiber monocoque, but it still relies on tubular geometry, with smooth blends between the tubes to reduce stress concentrations. The layout with the planes and the initial tubes is shown in Figure 16.4.

When all the tubes are created in-place in the assembly from the assembly layout sketch, the top of the assembly FeatureManager looks like Figure 16.5.

The arrow symbol (→) indicates that there is an external reference from the part to the assembly sketch. (External references are covered in more detail in Chapter 21, “Editing, Evaluating, and Troubleshooting Assemblies.”) Using the assembly layout sketch technique, an external reference is made every time a relationship is made from the part to the assembly sketch. Many users prefer to avoid external references, mainly because of the file management issues they cause, the difficulty in repairing them when broken, and rebuild speed performance issues. However, references to an assembly sketch are more stable than references between two parts in an assembly.

When you use an assembly layout sketch for either the in-context part building or simply part positioning, the main advantage that it offers is to give you a single driving sketch that enables you to change the size, shape, and position of the parts. You can use as many layout sketches as you want, and you can make them on different sketch planes. This enables you to control parts in all directions.

One of the drawbacks of this technique is that you give up dynamic assembly motion. When you create the parts in the context of the assembly and create relationships between sketches or features and the assembly sketch, you cannot move the parts by just dragging them with the cursor. To move the parts, you must move the sketch and rebuild. The part does not move until the sketch is updated. If you need to combine layout functionality with dynamic assembly motion, you can add more instances of the in-context parts that are mated in the traditional way. However, when using this method, be very careful about which instance you make your edits to, because in-context relations are driven by the original instance.

Another drawback of the assembly-level sketch in general is that you cannot use a sketch picture inside the sketch. Sketch pictures can contain important reference information for building a model. The lack of this capability is certainly noticeable. You can put your sketch picture in a part or even a virtual component.

Using Master Model

The master model technique is covered in depth in Chapter 33, “Employing Master Model Techniques,” but it is mentioned here because it works as an alternative method with the layout idea. The term master model can mean a couple of different things: It could be a single part where multiple bodies are created and then later split into multiple parts. Also, it is sometimes used as the name for inserting a single part with sketches and reference geometry into one or more other parts to have a single reference without creating that reference in the assembly.

This still creates an external reference, but it creates only a single external reference instead of possibly dozens, and updates of the inserted part can be locked. Performance problems with this technique are less serious. Also, if the file management fails and SolidWorks cannot find the inserted part, you can still keep working. SolidWorks keeps enough data in the child part that it does not need to constantly access the parent part.

The master model technique seems to have more advantages and fewer disadvantages than the methods that use assemblies. The dynamic assembly motion problem doesn't exist in a master model arrangement, nor does the lack of sketch picture functionality.

An example of this kind of work is shown in the derailleur assembly in Figure 16.6.

The part shown on the left is the master model. Notice that it contains sketch, plane, and surface data. The image on the right shows some parts superimposed on the master model part.

Using the Layout Workflow

With most functions in software of any type, you tend to get better results when you can use the software in the way it was intended. Generally, developers have a workflow in mind when they design the function itself and the interface. Working with the software is usually easier than working against the software.

Here is the general workflow for using the Layout feature:

1. Open a new or existing assembly.
2. Click the Layout toolbar button on the Layout tab of the CommandManager.
3. Sketch on the plane in the 3D sketch to create 2D sketches representing parts of a mechanism or other assembly.
4. Make selections of the sketch into blocks representing individual parts.
5. Insert multiple instances of the blocks to represent multiple instances of the parts.
6. Use sketch relations to put the blocks together like mating parts in an assembly.
7. Test the mechanism by dragging sketches. (Blocks function as a single sketch entity, so you can drag them within the sketch like parts in an assembly.)
8. Right-click the block (from inside or outside the Layout), and select Make Part From Block (also a button on the Layout toolbar).

Working with Virtual Components

Virtual components always exist with in-context workflows and frequently with the Layout workflow. Virtual components are parts or subassemblies that are created within the assembly. You can save a virtual component externally, and you can make an externally saved part into a virtual component. The advantages of virtual components are that you don't have to worry about saving out additional files and that the assembly will never lose track of any virtual component.

Some SolidWorks users use virtual components to represent non-geometric parts such as glue or paint. Anytime you choose Insert ➢ Component ➢ New Part from the menus and select a template and a plane to put the part on, the part is placed immediately into the assembly, and you can start working without worrying about having to save the assembly and the part. This saves lots of time initially. Later, when you save the assembly, SolidWorks will prompt you to save the parts externally and name them as well, or you may choose to leave the parts internal to the assembly.

Virtual components are named Part1 Assem1, where Part1 and Assem1 are default names. You can easily rename the part by clicking the RMB menu and selecting Rename Part. You cannot do this for external parts (unless this option is enabled). If you make an external part virtual, the name in the assembly becomes Copy offilename Assem1, where filename is the name of the external file. The name of the assembly is always included (and cannot be removed) to ensure that if you have subassemblies that also have virtual components, you always have unique filenames for all the parts.

Virtual components can also be accessed in their own window, which makes them easier to edit for some purposes. Bills of Materials (BOMs) and numbered balloons work correctly with virtual components, but they cannot have their own drawings.

Balancing Advantages and Limitations

In theory, the Layout feature has several advantages:

• You can make parts from blocks within the Layout.
• You can move parts by moving blocks in the Layout.
• It is a great way to structure your relations within an assembly.
• A single 3D sketch doesn't have the history concerns that multiple 2D sketches have.
• It is useful for motion analysis studies in 2D, using stick sketches, before any 3D components are created.

In practice, this feature needs some enhancements before it is ready for use on real assemblies. Using 2D sketches as assembly layout sketches may still be a better idea than trying to avoid the following limitations of the formal Layout feature:

• The 3D sketch used for Layout has all the limitations that come with 3D sketches.
• Sketch relations are listed in the Mates folder.
• Gaining access to edit the Layout after it has been closed requires a method you don't expect from a sketch: You click the Layout button on the toolbar rather than right-click and edit an icon in the FeatureManager.
• It requires that you use blocks to access all the functionality.
• A fully defined 3D sketch with blocks is very unstable.
• Part creation from blocks doesn't save time.
• You cannot paste copied sketch entities from a 2D sketch into the Layout.
• You cannot use sketch pictures in the Layout.
• You cannot use auto-dimension (or polygons or ellipses) in the Layout.

Although the formal Layout feature has serious advantages over regular layout sketches, at this time, the limitations outweigh the advantages. The rest of the discussion on layouts addresses the generic layout technique rather than the formal feature.