SolidWorks 2010- P10

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SolidWorks 2010- P10: Whether you are a new user of SolidWorks or a professional who wants to improve your skills, this book was written for you. Learning any software can be difficult at times. You launch the software for the first time, and you feel overwhelmed, not knowing how to even start a new document. In 3D CAD programs, it can be especially difficult. Many times a whole new vocabulary and a whole new creative environment are introduced.

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Model a Washer 239 faces that are perpendicular to the neutral plane, and without an added draft, they will cause issues for the molding process. F i g U r e 6 . 6 Selecting which surfaces to draft 9. Click the green check mark to create the drafted surfaces. Check the Draft of a Part Now that you have added draft to the washer, you need to ensure that it is indeed drafted properly to meet the manufacturing requirements. You can check the draft and how it is applied to your part by using the Draft Analysis tool. This tool not only verifies the draft but can show the angle changes on a face as well as determine the optimal areas for the parting lines, injection, and ejection surfaces in parts. The Draft Analysis tool uses colors to show whether faces on the part have a pos- itive draft, have a negative draft, or have the needed draft based on the draft angle specified and the neutral plane selected. Faces that have a positive draft meet the minimum angle required for the mold to be pulled in the direction specified; these faces are shown green by default. Faces shown in red are designated as having neg- ative draft and are faces that cannot be extracted with the mold being pulled in the designated direction. Often, the faces shown as having negative draft are ones that will sit on the other half of the mold, unless the surface or features is an undercut. Flipping the direction of pull will often swap the colors. Faces that are shown in yellow require more draft applied to them, or the draft angle in the Draft Analysis PropertyManager needs to be decreased. The great thing about the Draft Analysis tool is that it allows you to continue making modifications to your part while the tool is active. This gives you real-time
240 Chapter 6 • Creating a Subassembly feedback while you modify the model. The colors designating positive, negative, and needed draft will remain on the part until the tool is deselected. The following steps will set your requirements for the draft of the washer, and you will leave the analysis running while you finish your part to ensure that changes you make do not affect the overall moldability. 1. Select the Mold Tools tab in the CommandManager, and click the Draft Analysis button. 2. With the Direction Of Pull field active in the Draft Analysis PropertyManager, select the face of the washer that was used as You can also enable the Draft Analysis the neutral plane. Then click the Reverse Direction button to match tool in the menu by the direction you specified when creating the draft. selecting View ➢ Display ➢ Draft Analysis. 3. Set the Draft Angle option in the Analysis Parameters section to 1°. This will represent the minimum draft that is required by the manu- facturer. Then click the green check mark to finish selecting options. Add Multiple Fillets Using FilletXpert With the Draft Analysis tool running, you are now going to add some radii to the edges of the washer. Running the Draft Analysis tool while you finish your model will allow you to see whether the drafted faces need to be tweaked as the fillets are added. As in an earlier chapter, you’ll use the FilletXpert to add the radii to the washer because it allows you to add the fillets without needing to select the tool after each fillet. After adding the necessary fillets, you will also be adding a cham- fer to one of the edges. Unfortunately, the Chamfer tool does not have an Xpert
Model a Washer 241 option like the Fillet tool does, but that won’t slow you down this time since you only need to add one chamfer. To add radii to the washer, do the following: 1. Select Fillet in the shortcut bar. 2. Click the FilletXpert button at the top of the Fillet PropertyManager. 3. In the Radius Value field, enter the value .010, and select the top-outside edge of the washer, as in Figure 6.7. Click Apply in the FilletXpert PropertyManager. F i g U r e 6 . 7 Adding a fillet to the washer model 4. Change Radius value to .025, and select the outer and inner edges of the lip of the washer, as in Figure 6.8. Click the green check mark to create the second set of fillets, and close the Fillet PropertyManager. F i g U r e 6 . 8 Adding another fillet to the washer model 5. Select Chamfer in the shortcut bar, and change the value of the chamfer distance to .010. There is no need to specify the angle since the default is already set to 45°. Then select the upper-inner edge on the inner diameter of the washer, as in Figure 6.9. Click the green check mark to exit the Chamfer PropertyManager.
242 Chapter 6 • Creating a Subassembly 6. Once you have confirmed that the additional fillet and chamfer fea- tures did not affect the draft requirements of the part, deselect the Draft Analysis button on the Mold Tools tab by clicking it once again. F i g U r e 6 . 9 Adding a chamfer to the washer model Configure a Part Configurations in parts are extremely helpful when you want to create different versions of a part. Instead of creating multiple parts that are only variations of the original, you can include those variations in the parent part. Take the washer, for instance. You may have different sizes of the washer that are used in your company, but instead of having multiple models, you can include the dimensional variations within configurations of the original washer. You can use a part configuration for more than just dimensional variations with a part. You can use configurations to specify different materials, custom properties, suppressed or resolved features, or even appearances. This can be extremely helpful when you have whole families of parts, and it is also a great time-saver since you will not need to create multiple models. You can use configurations in a variety of ways, and there are even a few different ways to create them. We will not be able to get to each version here, but we can at least get you started exploring configurations. In the following steps, you’ll create a second configuration to the washer that will contain a larger diameter version. You will be using the Modify Configurations window in SolidWorks to create the configuration and also modify the dimensions in each version. Although there are a couple of ways to create configurations, we find this method the quickest and easiest way since it allows you to create configu- rations on the fly and it gives you a tabular view of the dimensions being modified. 1. Click the plus (+) next to the Revolve1 feature in the FeatureManager to show the child sketch.
Model a Washer 243 2. Select the sketch, and click the Edit Sketch button in the context menu. 3. While holding the Ctrl key, select the three diameter dimensions and the overall height in the sketch, as shown in Figure 6.10. F i g U r e 6 . 1 0 Selecting the dimensions to configure in the sketch t I p If only one dimension needs to be configured, you can skip the step of opening the sketch. Selecting the sketch in the FeatureManager will dis- play the dimensions used in the sketch without opening it. You can then right-click one of the dimensions to configure it. 4. Right-click, and select Configure Dimension in the menu. 5. In the Modify Configurations window, select the field labeled , and type Config2 (see Figure 6.11). F i g U r e 6 . 1 1 Modify Configurations window
244 Chapter 6 • Creating a Subassembly 6. Since the new Configuration is named Config2, you might as well change the name of the original configuration that is currently named Default to Config1. Right-click the field labeled Default, and select Rename Configuration in the menu. 7. In the Rename Configuration window, type Config1, and click OK. t I p Renaming the configurations makes it easier to determine which configuration is being referenced in drawings and assemblies. In many organizations, the configuration names match the part number for the con- figuration of the part. 8. Change the values for the dimensions in the Modify Configurations window by selecting each cell and typing in the new value. Change the values to those shown in Figure 6.12. F i g U r e 6 . 1 2 New values for washer configurations 9. Click OK to accept the changes. You may be prompted to rebuild the document; click Rebuild in the window to continue. The Modify Configurations window is not exclusive to configuring dimensions. You can configure features of a part and parts in an assembly using the same process. When you right-click a feature in a part and select Configure Feature, you can specify whether the specified feature is suppressed or resolved in a part. In assemblies, you can use the Modify Configurations window to specify the part configuration used in the assembly as well as specify that the part is suppressed or resolved in each assembly configuration. Switch Between Configurations When a part contains configurations, the graphics area will update depend- ing on the active configuration. As you switch between configurations in the part, the model will change to include the variations specified, whether they are dimensional variations or just a simple appearance change to the part. The FeatureManager will also display the active configuration being shown in the graphics area. Figure 6.13 shows how the name of the active configuration appears next to the part name at the very top of the tree.
Model a Washer 245 F i g U r e 6 . 1 3 Name of active configuration in FeatureManager The configurations in a part can be viewed, modified, and activated in the ConfigurationManager. In Figure 6.14, you will see a tab that is available above the FeatureManager design tree to give you access to the ConfigurationManager. Clicking the tab will hide the FeatureManager design tree and show the ConfigurationManager. F i g U r e 6 . 1 4 ConfigurationManager tab in FeatureManager View the FeatureManager Design Tree and ConfigurationManager at the Same Time Sometimes it is helpful to be able to view the FeatureManager design tree and the ConfigurationManager at the same time. Instead of switching back and forth between the two tabs, it is possible to show both of the panes at the same time. This allows you to continue to make modifications to your features and then switch between configurations quickly. To show them both at once, do the following: 1. Move the mouse pointer to the double line directly above the FeatureManager until the mouse pointer changes to include double lines. The double line bar is referred to as the horizontal split bar and is used to split the left pane into two windows.
246 Chapter 6 • Creating a Subassembly 2. While holding the left mouse button, drag the split bar down below the rollback bar, and release the mouse button. The FeatureManager is now shown in both sections of the pane (Figure 6.15). F i g U r e 6 . 1 5 FeatureManager split into two panes 3. Click the ConfigurationManager tab in the lower pane of the FeatureManager to view the available configurations. t I p Double-clicking the horizontal split bar will return it to its last position. If the FeatureManager is split, it will return to the top of the FeatureManager. If the FeatureManager is not split, double-clicking it will place the split bar at its last position. 4. In the ConfigurationManager, the available configurations will be dis- played. The active configuration will be shown in black, and the rest of the configurations will be shown in gray. To activate a configuration, double-click the configuration name, and the part will be updated in the graphics area.
Model a Washer Cover 247 Something to keep in mind when switching between configurations is that changes made to the model can impact other configurations. Depending on the option selected in the Modify Dimension window, changes to dimensions can apply to the active configuration only, to all configurations, or even to selected configurations. The same holds true to applying appearances, suppressing and resolving features, and adding new features. Model a Washer Cover O It’s a good idea to The washer from the previous section will more than likely be made of a black switch between rubber-like material that does not really add to the appearance of the overall configurations desk lamp. The washer cover model you are about to create has no other pur- occasionally to see pose other than covering the washer to provide a clean look to the overall prod- whether you have uct. The cover will be made of the same brass material that will be used on the inadvertently made changes to other other metallic parts on the lamp. configurations. The washer cover also gives you an opportunity to explore another way to create a revolved part. Up to this point, you have been creating revolved parts with closed profile sketches to create a solid cross section. Most of the revolved features you will need to create will indeed require a closed profile, but there are times when you can create what is referred to as a thin feature. A thin feature is when a feature, such as a revolve, is created from an open profile, and the thick- ness is added at the feature level. Using a thin feature is equivalent to offsetting the sketch to the required thickness and closing the ends to create a closed profile. But instead, the sketch can be left open, and the thickness is specified in the PropertyManager, saving you the time it would take to close the sketch. The following steps should make it easier to understand the concept of using thin features as you create the model for the washer cover: 1. Open a new part template, and save the file as Washer Cover. 2. Set the number of decimal places used in length to three places in the document properties. 3. Select Revolved Boss/Base feature, and create a sketch on the front plane. 4. Create a vertical centerline originating from the sketch origin that is approximately .300 long. 5. Using the dimensions shown in Figure 6.16, create the sketch of the washer cover.
248 Chapter 6 • Creating a Subassembly F i g U r e 6 . 1 6 Sketch of washer cover Add Sketch Fillets Up to this point, you have been adding fillets using the fillet tool on the model. This is usually the preferred method since too many fillets added at the sketch level will affect the overall speed performance of parts and assemblies. However, sometimes it is more beneficial to add fillets at the sketch level, especially for models such as the washer cover. Since the feature that will be used to create the model is a thin feature, it is better to add the fillet in the sketch to keep from having to create multiple fillets on both sides of the part. By adding the fillet in the sketch, when the thickness is added to the feature, the outside fillet on the model will change in radius depending on the thickness specified. In this sketch, you require two different radii to be specified for the fillets. But instead of using the same method for both, we want to illustrate a couple of dif- ferent ways of adding the radii. The first method requires selecting two adjacent sketch entities. After specifying the radius and selecting both entities, the sharp corner will be replaced with a radius. The second method only requires specify- ing the radius and then selecting the point where the two adjacent sketch enti- ties meet. Both methods are accepted practices, but we find the second method a lot quicker and easier, and we are sure you will see why. 1. Select the Sketch Fillet tool in the shortcut bar. 2. In the Sketch Fillet PropertyManager, set the Radius value to .050. 3. Select the bottom line of the sketch and the angled line that is con- nected to it, as in Figure 6.17.
Model a Washer Cover 249 F i g U r e 6 . 1 7 Adding a sketch fillet 4. If the preview of the fillet, shown in yellow, meets your expectations, click the green check mark in the PropertyManager to create the fillet. This method is probably the most widely used approach to adding fillets in sketches, but in our opinion it is not always the best way. The next method is often quicker and provides the same result, and we always prefer the faster method as long as the integrity of the part is not sacrificed. 5. Change the Radius value in the Sketch Fillet PropertyManager to .020, and select the point that makes the top corner of the sketch, as shown in Figure 6.18. Click the green check mark to add the sketch fillet. F i g U r e 6 . 1 8 Adding sketch fillet by selecting point 6. When you are finished adding the fillets, click the green check mark once again to exit the command.
250 Chapter 6 • Creating a Subassembly Create a revolved Thin Feature The sketch is now complete and ready to be revolved to make the cover. You probably have a nagging feeling that the sketch is incomplete, but we assure you that as long as the sketch is fully defined, it is more than sufficient to create the necessary model. To create a thin feature, you don’t need to select any spe- cial tool. You will be able to use the same Revolve Boss/Base tool that you have already used in previous chapters. The only difference is that you will specify the thickness of the revolve in the PropertyManager. 1. Click the Exit Sketch button in the conformation corner to begin the Revolve command. 2. When prompted to automatically close the sketch, click No. W a r N I N G It is important that you do not select to automatically close the sketch when prompted. If you select Yes, SolidWorks will attempt to create a closed profile resulting in a model that does not meet the design intent of the part. 3. In the Revolve PropertyManager, the check box in the header of the Thin Feature section should be selected. If it is not already expanded, click the chevron in the header to view the Thin Feature options (Figure 6.19). F i g U r e 6 . 1 9 Revolve PropertyManager 4. In the Direction1 Thickness field, enter the material thickness of the washer cover as .025, and click the green check mark to create the part. 5. Look at the preview in the graphics area (Figure 6.20). The sketch you drew is supposed to represent the inner surface of the part. If the preview does not show the sketch being the inner surface, click the Reverse Direction button in the PropertyManager.
Create a Subassembly 251 F i g U r e 6 . 2 0 Preview of revolved thin feature 6. Click the green check mark to create the revolved part. 7. Save your changes by pressing Ctrl+S or by clicking the Save button on the menu bar. The model for the washer cover is now complete. Since you included the fillets in the sketch, you don’t need to add any fillet features. To see the advantage of adding the fillet at the sketch level, take a look at the inside and outside faces of the part. The same fillet now has different radii depending on the direction of the offset. Create a Subassembly With the parts you created in the previous sections, you can now begin to build your first assembly. As far as assemblies go, this one will be one of the easiest ones you can possibly make, so it is good one to use to introduce the process. In the assembly, you’ll mate the washer and washer cover together to allow you to quickly insert them into the top-level assembly later. You could actually individually insert the components into the top-level assembly, but that approach is not considered good practice for a couple of reasons. First, the more components that are individu- ally inserted into the top-level assembly, the more it can affect the overall system performance. Next, in our opinion, the more parts that you have showing in the FeatureManager, the more overwhelming it can be, especially on very large assem- blies. Also, think about how many extra times you need to apply mates to all the instances of the part in a large assembly. So, to build the assembly, follow these steps: 1. If you did not close the washer from the earlier section, press Ctrl+Tab on the keyboard to switch between the open documents. If you closed the washer, open it at this time.
252 Chapter 6 • Creating a Subassembly t I p Pressing R on your keyboard will display a thumbnail for the most recent documents opened in SolidWorks. Selecting one of the thumbnails will open that document in the graphics area. 2. Click the downward-pointing arrow next to the New button on the menu bar, and select Make Assembly From Part/Assembly. 3. In the New SolidWorks Document window, select the assembly tem- plate, and click OK. 4. In the Begin Assembly PropertyManager, select the file named Washer in the Part/Assembly To Insert section, and click the green check mark. The part will automatically be inserted at the origin in the new assembly file. 5. Save the assembly as Washer Sub-Assembly, Desk Lamp. In the FeatureManager, instead of listing features for the part, the parts that make up the assembly are shown. Since you have only one part added to the assembly so far, there is only one listed. On the same line that shows the name of the part that exists in the assembly is a wealth of information. First, in front of the name of the part is the symbol showing the document type of the model. Since the washer is a part document, the symbol for a part is shown. If you inserted another assembly, the icon would show the symbol for an assembly. After the icon, in parentheses, is the letter f. This shows that the part is fixed in place and cannot be moved. At least one part in an assembly should be fixed, and the other components are then mated to the base part — otherwise, the whole assembly will be able to move, and that is not a good thing. Because you created the assembly from a part, the part is automatically fixed. If you were to create a blank assembly and insert the part manually, it would not necessarily be fixed. After the name of the component shown in the FeatureManager, inside the brackets, is the number of instances of the component. If you were to insert more washers into this assembly, this number would increment up with each subsequent part. This number cannot be changed and will not be reused in the assembly for the part named even after a component is deleted from the assembly. Last, inside the parentheses following the instance count, the active configura- tion and display state names appear. In later chapters, we will be covering display
Create a Subassembly 253 states, so for the time being you can concern yourself only with the configuration that is displayed. When you created the model for the washer, you made it with two configurations. This is the time that you need to specify which configuration the current assembly will be utilizing. The next section describes the process for selecting the configuration of a part in an assembly. Select a Part Configuration As we mentioned in the previous section, since you created the washer with two configurations, you need to specify which one will be used in the assembly. Depending on the active configuration when the part was saved, the correct con- figuration may very well be displayed in the FeatureManager at this point, but just in case, follow these steps for specifying the configuration in the Component Properties window: 1. Select the washer in the FeatureManager, and select Component Properties in the context toolbar. 2. In the Reference Configuration section of the Custom Properties win- dow, ensure that Config1 is selected. 3. Click OK to accept the selected configuration, and close the window. After clicking OK in the Custom Properties window, the name of the configu- ration in the FeatureManager should now show Config1. Once the washer is set to the appropriate configuration, move to the next section to learn how to insert the washer cover into the assembly.
254 Chapter 6 • Creating a Subassembly insert Components into Assembly Now it is time to insert the washer cover into the assembly. There are a couple of quick and easy ways to insert components into an assembly, and we will be addressing a few of them in later chapters, but for now you will be using the Insert Components tool. When you initiate the command, the PropertyManager might seem familiar to you, and in fact it should. The Insert Component PropertyManager is the same as the Begin Assembly PropertyManager. The only difference is the name. 1. Press S on the keyboard, and select Insert Components in the short- cut bar. 2. In the Part/Assembly To Insert section of the Insert Component PropertyManager, select the washer cover . The washer cover will be present only in the Open Documents field if the model is currently opened in SolidWorks. If you closed the model for the washer cover after creating it, you will need to select the Browse button in the Part/Assembly To Insert section and select the model in the Open window. 3. In the graphics area, place the washer cover by clicking and releas- ing the left mouse button (see Figure 6.21). Once the washer cover is placed, there is no need to exit any command. F i g U r e 6 . 2 1 Inserting washer cover into assembly There may be times in the future while you are using SolidWorks that you will need to insert multiple components into your assembly. Instead of selecting the Insert Components tool each time you need to add a model, you can keep the PropertyManager open. Selecting the pushpin icon next to the red X at the top of the PropertyManager will keep the pane open as long as you need it. Once you are finished inserting all your components, clicking the red X will close the pane.
Add Mates in Assemblies 255 Move Floating Components in an Assembly Until the position of a component in the assembly is fully defined, you can freely move the part around the graphics area. To determine whether the component’s position is fully defined, just look at the component in the FeatureManager. If there is a minus (-) shown between the component icon and the component name, the position is not fully defined. Moving components in an assembly is really simple. In fact, you don’t even need to use any commands other than the buttons of your mouse. Using the left and right mouse buttons, you can rotate and move a floating component in your assembly. For example, to move the washer cover, select the washer cover with the mouse pointer while clicking and holding the left mouse button. Move the mouse around, and the part moves in the X and Y directions in relation to the viewing plane. Release the left mouse button to place the part. To rotate the washer cover, select the washer cover with the mouse pointer while clicking and holding the right mouse button. Move the mouse around, and the part will rotate in the direction the mouse moves. Add Mates in Assemblies Parts as they are entered into an assembly have six degrees of freedom. Degrees of freedom refer to the directions a part can freely move in 3D space. In 3D environ- ments, there are three basic directions; X, Y, and Z. For a graphical representation of these directions, one does not have to look further than the reference triad in the lower-left corner of the graphics area. The red arrow shows the X direction, which is horizontal. The Y direction, shown in green, is the vertical direction. The Z direc- tion, shown in green, is the direction moving either toward or away from you. The other three degrees of freedom are how a part rotates around the x-, y-, and z-axes. To fully define a part in an assembly, you must restrict all six degrees of freedom. This is done by using mates, which are the geometric relationships added to a part in relation to other parts or planes. For example, in the Washer Sub-Assembly part, the washer cover needs to be mated to the washer. The way we like to describe mates to new users is that mates can be used to replicate the way that the parts would interact with each other in real life. In real life, the washer and the washer cover would have a threaded post inserted through their inner diameters. This would make the washer and washer cover concentric, and there is a mate for that. Next, when the washer and washer cover are installed, the inside-top face of the washer cover will be touching the top face of the washer. In SolidWorks, this can be
256 Chapter 6 • Creating a Subassembly done with a coincident mate. The next few steps will show you how to apply these mates to the washer cover to complete the subassembly. 1. Press S on the keyboard, and select Mate in the shortcut bar. 2. Select the conical faces on both the washer and the washer cover. The two components will become concentric based on the selected faces (see Figure 6.22). F i g U r e 6 . 2 2 Concentric components You can use the concentric mate with any circular edge or cylindrical or conical face. There are many edges and faces in the two components that could have been used to make the two components concentric. The only reasons we chose these two faces is because they had the larg- est surface area and they were easier to select, but feel free to select other faces to see how they work for the mate. 3. Click the green check mark in the PropertyManager or the context menu to accept the mate. 4. Click the top face of the washer. Then select the top-inside face of the washer cover to make the two surfaces coincident. Accept the mate by clicking the green check mark, and click the green check mark once again to exit the Mate command. 5. You can confirm how the two parts mate together by creating a cross section. Select the Section View button in the Heads-up View toolbar. 6. In the Section View PropertyManager, click the Front Plane button, and click the green check mark (see Figure 6.23). 7. On the reference triad in the lower-left corner of the graphics area, click the z-axis to change the orientation of the view to be able to see the cross section of the assembly.
Add Mates in Assemblies 257 F i g U r e 6 . 2 3 Section View PropertyManager 8. Instead of zooming in on the part, press G on the keyboard to display the magnifying glass. The magnifying glass allows you to zoom in to areas of the model without needing to change the overall scale of the graphics area (see Figure 6.24). F i g U r e 6 . 2 4 Viewing cross section with magnifying glass 9. The mouse pointer will be able to move freely inside the magnifying glass, but when the mouse reaches the outside of the circle, it will push the view around the graphics area. 10. Spinning the scroll wheel on your mouse will cause the view in the magnifying glass to zoom in and out depending on the direction you spin the wheel. t I p Pressing and holding the Alt key while spinning the scroll wheel on your mouse will create a section view within the magnifying glass normal to the viewing angle.
258 Chapter 6 • Creating a Subassembly 11. To exit the magnifying glass, click and release the left mouse button. 12. To exit the section view, deselect the Section View button on the Heads-up View toolbar by clicking the button once again. As you work in SolidWorks, you may discover that the two most common mates you will apply to assemblies are the concentric and coincident mates. That is because these two mates match the most common ways parts are put together in real life. However, as you may have noticed, there are many more mates to choose from in the Mates PropertyManager. In later chapters, you will be taking a look at a few of the other available mates as well as alternate meth- ods to apply the most commonly used mates. Change the Appearance of Parts in an Assembly In the previous section, when you sectioned the part to see how the mate was applied, you might have thought that is was difficult to tell the difference between the two components. This is actually a very common issue when you have multiple components that all have the same color or appearance. Luckily, there are a couple really easy ways to change how a part looks in your assembly. Some may think that changing the color of components in assemblies, or even adding material appearances, is a waste of time, but we do not agree. The ability to quickly determine where one component ends and the other begins can some- times be difficult, especially in very large assemblies. You may not have problems telling components apart, but remember that there may be other users or even vendors who will be studying your assemblies and they won’t know the compo- nents as intimately as you will. Anything that can make things easier for all par- ties involved, we are always a fan of doing. Change Colors Using Appearances The most common way to change the appearance of your components in an assembly is to simply change the color. In our opinion, there is no drawback to applying colors to components in an assembly. It’s quick and easy, makes it easier for users, and has absolutely no effect on the system performance. The following steps will show you the easiest way to apply a color to a component: 1. Select the washer in the graphics area by clicking and releasing the left mouse button.