CHAPTER 5

Using Visualization Techniques

Visualizing geometry is part of the overall mission of SolidWorks software. Visualizing 3D CAD data is more than seeing shaded solids or shiny surfaces; it includes being able to see the interior and exterior at the same time and using sections, transparency, wireframe, and other tools or techniques. SolidWorks takes it so much further than just being able to see things in 3D; you can look at some parts of an assembly in wireframe while others are transparent and others are opaque. You can see a part with a reflective appearance. You can create section views in parts and assemblies to visualize internal details.

My aim with this chapter is to show you important capabilities that will expand how you can use SolidWorks, and maybe even change the way you use the tools or look at modeling tasks. At the same time, these techniques may provide some of the awe and wonder we sometimes experience while using incredible 3D tools to do actual work. If I sound a little enthusiastic about this topic, it is because visualization is the part of this software that really brings your imagination to life. It can be the source of real inspiration and allows you to communicate geometrical ideas with other people that might not be possible any other way.

Manipulating the View

One of the most important skills in SolidWorks is manipulating the view. This is something you'll do more frequently than any other function in SolidWorks; so learning to do it efficiently and effectively is very important, whether you look at it as rotating the model or rotating the point of view around the model. The easiest way to rotate the part is to hold down the middle mouse button (MMB) or the scroll wheel and move the mouse. If your mouse does not have a middle button or a scroll wheel that you can use as a MMB, then you can use the Rotate View icon on the View toolbar, or the icon on the Heads-up View toolbar. The Heads-up View toolbar is shown in its default state in Figure 5.1.

FIGURE 5.1 Use the Heads-up View toolbar to easily access most visualization tools.

The Heads-up View toolbar can be customized and disabled using the same method that you use for all other toolbars, through the Tools Customize dialog.

Using arrow keys

You can use the arrow keys on the keyboard to manipulate the view in predictable and controllable ways. You can use the Shift, Ctrl, and Alt keys to add to the behavior.

The arrow keys enable you to rotate to the following views:

• Arrow. Rotate 15 degrees. To customize this setting, choose Tools Options View.
• Shift+arrow. Rotate 90 degrees.
• Alt+arrow. Rotate in a plane flat to the screen.
• Ctrl+arrow. Pan.

Using the middle mouse button

Most, if not all, mice sold today have middle mouse buttons (MMBs), usually in the form of a clickable scroll wheel.

The MMB or scroll wheel has several uses in view manipulation:

• MMB alone. Rotate.
• Click or hover on edge, face, or vertex with MMB, and then drag MMB. Rotate around selected entity.
• Ctrl+MMB. Pan.
• Shift+MMB. Zoom.
• Double-click MMB. Zoom to fit.
• Scroll with wheel. Zoom in or out. To reverse direction of the zoom setting, choose Tools Options View.
• Alt+MMB. Rotate in a plane flat to the screen.

Using mouse gestures

Mouse gestures are an interface method that you can customize to do anything a SolidWorks toolbar button can do, but by default, it controls view orientation. Figure 5.2 shows the default configuration of the mouse gesture donut.

FIGURE 5.2 Click+drag the right mouse button (RMB) to access the commands on the donut.

It may take a little time for you to get used the interface. It works best when you understand what the commands are before you use them, so that you can invoke the Top View command in a single motion. It does not work well if you have to initiate the interface with a very short RMB drag, then drag again to select the command. For this reason, it might be better to limit the donut to four commands rather than eight, and set it up intuitively such that the top view is an RMB stroke up, a right view is an RMB stroke to the right, and so on.

You can customize the mouse gesture donut in the Tools Customize Mouse Gestures. This works much like the Keyboard (hotkey) customization, where you can turn gestures on or off, set the mouse gesture donut to four or eight sections, and any gesture direction to any available command.

Using the View toolbar

The View toolbar, shown in its entirety in Figure 5.3, contains the tools that you need to manipulate the view in SolidWorks. Not all of the available tools are on the toolbar by default, but I have added them here for this image. To customize your own View toolbar, you must use choose Tools Customize from the menu and select the Commands tab. Then click the View toolbar, and either drag items from the Customize dialog box to the View toolbar to add them or from the View toolbar into the empty graphics area to remove them. You can use all of these tools with part and assembly models but only a few of them with drawings.

The toolbar that holds tools for direct access to standard named views such as Front, Top, and Normal To is called the Standard Views toolbar and is described later in this chapter.

FIGURE 5.3 The View toolbar

Adding scrollbars and splitters

An option exists to add scrollbars and view pane splitters to the graphics window. To use it, choose Tools Options Display/Selection, Display Scrollbars in graphics view. This selection will be grayed out if any SolidWorks documents are open (so you must close all SolidWorks documents to change it). When you zoom in such that the part/assembly/drawing is partially off the screen, the scrollbars will activate on the right side and bottom of the SolidWorks window, enabling you to scroll up and down as well as left and right to pan the view. Scrollbars and splitters are turned off by default. You cannot turn off one or the other; scrollbars and splitters come as a package deal.

Figure 5.4 shows a detail of the bottom-right corner of the SolidWorks graphics window, where you find the scrollbars and splitters. Notice the cursor in the lower right over one of the splitters. The splitters can be easy to miss if you do not know what they look like.

FIGURE 5.4 Scrollbars and splitters controls can be turned on or off.

The splitters enable you to split the main graphics window into multiple view ports. The options are two ports horizontally, two ports vertically, or four view ports. The splitter bars are located at the intersection of the scrollbars in the lower-right corner of the graphics window. Of course, you can also use the icons on the Standard Views toolbar for splitting the view into two vertical ports, two horizontal ports, or four ports, the Heads-up View toolbar, or the View Orientation flyout.

Once a viewport has been split, you can remove the split with the toolbar icons, either by dragging the border back to the edge of the display window or by double-clicking the split border. If the view has been split into four, you can set it back to a single viewport by double-clicking the intersection of the horizontal and vertical port borders.

Using the Magnifying Glass

You can invoke the Magnifying Glass by pressing G, and dismiss it when you select something or when you press Esc. To change the hotkey it is associated with, choose Tools Customize Keyboard. Magnifying Glass is listed in the Other category. The Magnifying Glass is intended to magnify a small area of the view to enable you to make a more precise selection.

The magnified area follows your cursor as it moves, and you can zoom in and out by scrolling the MMB. Ctrl-dragging the MMB keeps the Magnifying Glass centered on the cursor. Pressing Alt creates a section view parallel to the view, and scrolling the wheel with Alt pressed moves the section plane farther away or closer. Figure 5.5 shows the Magnifying Glass in operation, cutting a section view through a part.

FIGURE 5.5 Using the Magnifying Glass with the section view

Clicking the Triad axes

The Triad is the multicolored coordinate axis in the lower-left corner of the SolidWorks graphics window. You generally use it passively to see how the view is oriented and to get X, Y, Z reference directions for features that need it.

To use the Triad to control the view orientation, try the following:

• Click an axis. The view will rotate to point this axis out of the screen.
• Click an axis a second time. This axis will point into the screen.
• Shift-click an axis. This view will spin 90 degrees about that axis (using the right-hand rule).
• Alt-click an axis. This view will spin 15 degrees (or the default view rotation angle) around the axis.

When you are in a named view, a little box in the lower-left corner shows the name of the view. This includes standard named views and custom named views. Anything that shows up in the View Orientation box (accessed by spacebar) displays a name in the corner. Figure 5.6 shows the Triad and the named view box in the lower-left corner.

FIGURE 5.6 The Triad and named view box

By Shift-clicking an axis of the triad, the view is rotated 90 degrees from the original orientation. Alt-clicking rotates the view around the clicked axis by the view rotation increment set in Tools Options View, which is 15 degrees by default. Pressing Ctrl in conjunction with any of these causes the view to rotate in the opposite direction. Therefore, if pressing Shift-click makes the view rotate against the right-hand rule about the clicked axis, pressing Ctrl+Shift-click makes the view rotate with the right-hand rule.

Using the View Tools

SolidWorks has many additional tools for managing the view, and you can easily access them through the Heads Up View toolbar, hotkeys, or the normal toolbars and menus.

The tools in this section will help you to control how you view parts and assemblies. The following tools are mainly found in the View, View Display, and View Modify menu areas.

• Zoom to Fit. Resizes the graphics window to include everything that is shown in the model. You can also access this command by pressing the F key, or double MMB-clicking.
• Zoom to Area. When you drag the diagonal of a rectangle in the display area, the display resizes to fit it. The border size around the fit area is fixed and cannot be adjusted. This only zooms in, not out.
• Zoom In/Out. Drag the mouse up or down to zoom in or out, respectively. You can also access this command by holding down the Shift key and dragging up or down with the MMB. The hotkey Z and Shift+Z work for Zoom Out and Zoom In, respectively. The percentage of the zoom is a fixed amount and cannot be adjusted. You can also use the scroll wheel to zoom in and out, and if you are accustomed to using a different CAD product where the scroll works the opposite way, a setting exists at Tools Options View that allows you to reverse the function of the scroll wheel.
• Zoom to Selection. Resizes the screen to fit the selection. You can also access this command by right-clicking on a feature in the FeatureManager. For example, if you select a sketch from the FeatureManager and right-click and select Zoom to Selection, the view positions the sketch in the middle of the screen and resizes the sketch to match the display. The view does not rotate with Zoom to Selection.

• Zoom about Screen Center. Enables you to zoom straight in and straight out. This tool is off by default. The default behavior is that zooming works around the cursor. If the cursor is off to one side, zooming in and out can cause the view to “walk” away from that side. This command is only found in the menus at View Modify and does not have an icon.
• Draft, Undercut, and Parting Line Analysis. Evaluates the manufacturability of plastic and cast parts. These three types of geometric analysis are discussed in more detail in the discussion on model evaluation in Chapter 12.
• Rotate View. Enables you to orbit around the part or assembly using the left mouse button (LMB). You can also access this command by using the MMB without the Toolbar icon.
• Roll View. Spins the view on the plane of the screen.
• Pan. Scrolls the view flat to the screen by dragging the mouse. You can also access this command by holding down the Ctrl key and dragging the MMB without using the Toolbar icon, or with Ctrl+arrow.
• 3D Drawing View. Enables you to rotate the model within a drawing view to make selections that would otherwise be difficult or impossible. This is of no use in part and assembly models.
• Standard Views flyout toolbar. The Standard Views toolbar is discussed later in this chapter. The flyout enables you to access all the Standard Views tools. This button is also called the View Orientation flyout, depending on where you see it.
• Wireframe. Displays the model edges without the shaded faces. No edges are hidden.
• Hidden Lines Visible (HLV). Displays the model edges without the shaded faces. Edges that would be hidden are displayed in a font.
• Hidden Lines Removed (HLR). Displays the model edges without the shaded faces. Edges that are hidden by the part are removed from the display.
• Shaded with Edges. The model is displayed with shading, and edges are shown using HLR. Edges can either be all a single color that you set in Tools Options Colors (typically black), or they can match the shaded color of the part. Tools Options Document Properties Colors is where you find the document specific setting to use the same color for shaded and wireframe display, which becomes very useful in an assembly when all the parts shown in wireframe are the same color as they are when they are shaded, instead of all being black.
• Shaded. The model is displayed with shading, and edges are not shown.
• Shadows in Shaded Mode. When the model is displayed shaded, a shadow displays “under” the part. Regardless of how you rotate the model, when Shadows are initially turned on, the shadow always starts out parallel to the standard plane that is closest to the bottom of the monitor. As you rotate the model, the shadow moves with it. If Shadows are turned off and then on again, they again display parallel to the standard plane that is closest to the bottom of the monitor.
• Section View. Sections the display of the model. Figure 5.7 shows the Section View command at work. You can use up to three section planes at once. Solid and surface models as well as assemblies can be sectioned. You can use the spin boxes, enter numbers manually, or drag the arrows that are attached to the section planes to move the section through the model. Section planes can also be rotated by dragging the border of the plane.

  FIGURE 5.7 The Section View tool

  

  Clicking the check mark icon in the Section View PropertyManager enables you to continue working with the sectioned model, although you may not be able to reference edges or faces that are created by the section view. It is only a displayed section; the actual geometry is not cut.

  Section Views can be saved either to the View Orientation box or to the Annotation View folder, which enables section views to be reused on the drawing. Annotation Views are described in more detail in Chapter 16.

  Once you are working in a section view, if you want to alter it, you can access Modify Section view through the menus at View Modify Section View. You should notice that no toolbar icon exists for modifying a section view. You have to access this command through the menus, or by turning off then turning back on the Section View tool. You might also notice that a Modify Section View is available in the hotkey assignment area, Tools Customize Keyboard.

• RealView. Creates a more realistic reflective or textured display for advanced material selections. This feature does not work with all graphics hardware, so check the SolidWorks system requirements Web site to see if it supports your hardware. An entire section of this chapter is devoted to the various tools available with RealView graphics.
• Edit Appearance. Edit Appearance enables you to apply colors, textures, and materials to faces, bodies, features, parts, and components. Appearance and display issues comprise a large portion of the SolidWorks interface.

Zebra Stripes

Another geometrical analysis tool that helps you visualize the quality of transitions between faces across edges. Zebra Stripes simulates putting a perfectly reflective part in a room that is either cubic or spherical and where the walls are painted with black-and-white stripes. In high-end shape design, surface quality is measured qualitatively using light reflections from the surface. Reflecting stripes makes it easier to visualize when an edge is not smooth.

The three cases that Zebra Stripes can help you identify are as follows (see Figure 5.8):

• Contact. Surfaces intersect at an edge but are not tangent across the edge. This condition exists when stripes do not line up on either side of the edge.
• Tangency. Surfaces are tangent across an edge but have different radius of curvature on either side of the edge (non-curvature continuous). This condition exists when stripes line up across an edge, but the stripe is not tangent across the edge.
• Curvature continuity. Surfaces on either side of an edge are tangent and match in radius of curvature. Zebra Stripes are smooth and tangent across the edge.

FIGURE 5.8 Zebra Stripes

In Figure 5.8, the Zebra Stripes in example A do not match across the edge labeled A at all. This is clearly the non-tangent, contact-only case. Example B shows that the stripes match in position going across the indicated edge, but they change direction immediately. This is the tangent case. Example C shows the stripes flowing smoothly across the edge. This is the curvature continuous case.

You can use the remaining icons in the View toolbar to toggle the display of various types of entities from reference geometry to sketches.

View Orientation

You can activate the View Orientation box by pressing the spacebar. View Orientation, shown in Figure 5.9, keeps all named views, saved section views, and standard views. Tools in the box also enable you to update standard views to the current view or to reset standard views to their defaults. Be aware that a toolbar button on the View toolbar is also called View Orientation.

FIGURE 5.9 The View Orientation dialog box

The Standard Views flyout is called either Standard Views or View Orientation, depending on where you see it. The View Orientation dialog box contains the following controls:

• Push Pin. Keeps the dialog box active.
• New View. Creates a new custom-named view.
• Update Standard Views. Sets the current view to be the new Front view; all other views update relative to this change. This also updates any associated drawing views, but does not move any geometry or change plane orientation.
• Reset Standard Views. Resets the standard views so that the Front view looks normal to the Front plane (Plane1, XY plane).
• Previous View (undo view change). You can access this tool by pressing the default hotkey Shift+Ctrl+Z.

The Standard Views toolbar

I have already mentioned the Standard Views flyout on the View toolbar, but here I describe the tools it contains in detail. Figure 5.10 shows the Standard Views toolbar in its default configuration.

By default, the Standard Views toolbar contains the View Orientation button, a tool from the View toolbar. The View Orientation button is discussed in detail earlier in this section.

FIGURE 5.10 The Standard Views toolbar

Normal To has three modes of operation:

• First Mode. Click a plane, planar face, or 2D sketch. When you click Normal To, the view reorients normal to the selected plane, face, or sketch and zooms to fit the model in the view. This method is shown in Figure 5.11.

  FIGURE 5.11 The result of using Normal To on the end rib angled face

  

• Second Mode. Click Normal To a second time. The view rotates 180° to display the opposite direction.
• Third Mode. After making the first selection, Ctrl+select another planar entity. The view is normal to the first selection, and the second selection is rotated to the top. This method is shown in Figure 5.12.

FIGURE 5.12 Using Normal To with Second Selection to define the top

Annotation views

Annotation views enable you to group annotations that were made in the 3D model into views that will be used on the drawing. They are collected under the Annotations folder in the FeatureManager for parts and assemblies. Annotation views can be created either automatically, when 3D annotations are added, or manually. An Unassigned Items annotation view acts as a catchall for annotations that are not assigned to any particular views. In the 3D model, you can use the views to reorient the model and display annotations. As mentioned earlier, annotation views can also capture a model section view to be shown in a drawing view. The Annotation views are shown for the Chapter5SampleCasting part in Figure 5.13.

FIGURE 5.13 Annotations views for Chapter5SampleCasting.sldprt

Using the DisplayManager

The DisplayManager is new in SolidWorks 2011. It organizes all of the display and visual information into a form that makes it easier to understand and control. The DisplayManager has buttons that you click to separately list Appearances, Decals, and Scenes, Lights, and Cameras. You can find the DisplayManager as a tab in the FeatureManager window area. Figure 5.14 shows the Appearances data for a part with a material and color applied to two faces and a feature.

FIGURE 5.14 Using the DisplayManager to manage appearances

Appearances in SolidWorks are a combination of color and texture, along with a property that looks like material but is not. Just think of appearance as being color and texture, and the topic is easier to understand.

In order to have appearances display and sort in the DisplayManager, you have to first apply appearances. Most of the appearances are meant to look like idealized materials in real life. Polished, cast, knurled, machined, sand blasted, and other surface finish types are available to add realism to your models. However, you might simply want each part to be a different color to help identify the different parts, using an abstract scheme in place of a realistic one.

Applying appearances

You can apply appearances to faces, bodies, features, parts, assembly components, or even the top-level assembly. Even if you don't apply an appearance, every part and assembly template starts with a default appearance, which is white, glossy plastic. If you use old SolidWorks templates, this default appearance may not apply to you.

You can apply appearances in several ways:

• Double-click: Double-clicking an appearance in the Appearances panel of the Task Pane applies the appearance to the document (part or assembly).
• Drag-and-drop: Dragging an appearance from the Appearances panel of the Task Pane enables you to drop it on geometry in the graphics window. When you do this, a toolbar pops up and presents you with several options. Figure 5.15 shows this toolbar with the options for Face, Feature, Body, and Part.

  FIGURE 5.15 Determining a target for the appearance

  

• Context toolbar: You can also invoke the Appearance function from the context bars (left- or right-click). You can do this with pre-selection or no selection. This method also gives you options for the target to which to apply the appearance, the face, feature, body, or part. Figure 5.16 shows this method.

FIGURE 5.16 Using context toolbars to apply an appearance

Differentiating appearances and materials

It is easy to confuse appearances and materials. The biggest reason for this is that in many cases, appearances have the same names as materials, and the texture associated with the appearance typically also has the name of a material. SolidWorks has appearances with names such as high gloss plastic, wrought iron, and chromium plate.

It may become even more confusing because materials (which you can assign from the FeatureManager on the left) have appearances (which you assign from the Task Pane on the right) assigned to them. For example, you could assign an appearance called polished aluminum to a material called AISI 304.

You cannot use appearances to assign mass properties (such as density or stiffness) to a part, but you can use materials to assign an appearance as well as mass properties to a part. Figure 5.17 shows the RMB menu for editing material, which you invoke from the Material folder in the FeatureManager.

FIGURE 5.17 Editing a material

Materials assign properties to your parts for drawing hatch and mass properties, as well as simulation. Notice in Figure 5.18 that the second tab allows you to assign an appearance to the material. You can use this interface to create your own custom materials.

FIGURE 5.18 Editing or creating custom materials

Understanding appearances

Appearances are made up of a combination of color, illumination properties, a surface finish image, and image mapping settings. You can control all these options in the Advanced interface of the Appearances PropertyManager, as shown in Figure 5.19. To access this interface, click the Appearance icon in the Heads Up View toolbar, and click the Advanced button at the top of the PropertyManager.

FIGURE 5.19 Controlling the components of appearance

You can adjust the default appearances that install with SolidWorks when you apply them to your models. For example, you can apply a shiny, reflective appearance such as Stainless Steel, but then adjust its color to blue or red. You could apply a cast iron appearance and then increase the roughness. You might apply a brushed aluminum appearance, and change the direction of the brush lines. You could apply a reflective glass appearance, then reduce the reflectivity and increase the transparency. You might apply a knurled steel appearance to a cylindrical part, and adjust the mapping so that the knurled image does not smear improperly across a face. Figure 5.20 shows the contents of the Color/Image, Mapping, Illumination, and Surface Finish tabs of the Appearances PropertyManager, where you can adjust all of these settings and more.

FIGURE 5.20 Adjusting the display properties in the Appearances PropertyManager

Understanding overrides

Keeping track of colors and appearances in SolidWorks can be difficult. The scheme and terminology seem to change with every release, and SolidWorks 2011 is no exception in this regard. For example, many users have difficulty understanding when one color overrides another color, and how to remove layers of applied colors or appearances. The functionality called Overrides existed in previous versions, but is now more prominent in 2011.

Here is the hierarchy that SolidWorks uses when applying colors (appearances):

• Default
• Part
• Body
• Feature
• Face
• Component
• Assembly

You should read this list with the words “...is overridden by...” between the items. So the default appearance is overridden by anything else, and an appearance that you apply to the assembly overrides everything else. You can also think of this list as being sorted from the weakest to the strongest.

In Figure 5.14, the DisplayManager shows the colors and appearances listed by history, which refers to the order in which they were added to the model. Figure 5.21 shows the appearances sorted by hierarchy, using the order established by Overrides. The Sort Order drop-down list allows you to select from History, Hierarchy, and Alphabetical sorting.

FIGURE 5.21 Sorting appearances and colors by hierarchy

There is no simple way of describing the entire appearances method. It is unnecessarily complex and does not always work as described. You may find times where a face clearly has an altered appearance, but SolidWorks says it does not and moreover won't allow you to remove or change the appearance.

Using appearances with Display States

Display States are covered in more detail later in this chapter. You will also need to understand configurations (see Chapter 11) to completely grasp the use of appearances with Display States. You can assign appearances to apply to all Display States or just to the current Display State. Display States in turn can be linked or unlinked to configurations, and some display properties such as color can be controlled by configurations. The control of appearances and colors for Display States and configurations is convoluted at best. This is a warning that mixing changes to these four items can result in colors that you can either not remove or not apply. It is difficult to say how much of this is due to bugs and how much is due to convoluted logic and too many sources of control. You can control the setting for which Display States an appearance change will apply to. You do this in the Display States panel at the very bottom of the Appearances PropertyManager, as shown in Figure 5.22 on the left.

You can find the Display States interface at the bottom of the ConfigurationManager, as shown in Figure 5.22 on the right.

FIGURE 5.22 Controlling appearances with Display States

Removing appearances

Once you have applied appearances to a part, you may want to remove them later. You can think of multiple appearances applied to various overrides within the part as an old chair with many layers of paint. In this case, you can remove those layers of paint one by one until you get down to the base material, which in this case would be the default material.

Look at Figure 5.23. Notice that there is a red X to the right of each entity — face, feature, body, and part — and another one at the bottom. Each red X enables you to remove a layer of paint from this part. This example is hopefully more extreme than what you will normally deal with, where separate colors have been applied to each entity: white to the face, blue to the feature, pink to the body, and gray to the part. You can remove any color applied at any level just by clicking the red X. Clicking the bottom red X removes all of the overrides (all of the face, feature, body, part, and other colors that have been applied) and assigns the default appearance for that part.

FIGURE 5.23 Removing layers of appearances from a part

You can assign the default appearance in a part or assembly template, or reassign it in an existing part. To do this, open the Appearances, Scenes, and Decals tab in the Task Pane, find an appearance that you like, and right-click it. Figure 5.24 shows the menu that appears.

FIGURE 5.24 Assigning a default appearance

To save this appearance to a part template, assign the default appearance in an empty part document with settings that you want to use, set the default appearance, and save the empty part as a part template.

Using decals

Starting in SolidWorks 2011, decals have been moved into SolidWorks Standard (base level SolidWorks) and no longer require rendering software. All decals used in a model are listed in the Decal area of the DisplayManager.

To apply a decal, you can use the Appearances, Scenes, and Decals tab of the Task Pane to access the stock or sample images, or you can right-click in the open area of the Decals DisplayManager and select Add Decal. This brings up the Decals PropertyManager, shown in Figure 5.25.

You can use *.bmp, *.jpg, *.tif, and *.png images as decals in SolidWorks. The images can be mapped onto flat, cylindrical, or spherical surfaces. You can uses masks or images with an alpha channel to create transparent parts of the decal. You can also select a color of the image to set to transparent. Only *.tif and *.png images can use alpha channel transparency.

You can size, position, and rotate the decal on the screen with handles, as shown in Figure 5.26. You can use any of the corner nodes on the image to resize the decal. Dragging anywhere inside the image border moves the decal, and dragging the yellow ball in the center of the image rotates it.

FIGURE 5.25 Working with the Decals PropertyManager

FIGURE 5.26 Sizing and positioning the decal

Using scenes, lights, and cameras

Scenes, lights, and cameras are important for visualization and rendering. Rendering is not covered in this book because PhotoView 360 (the replacement for the now-defunct PhotoWorks 2) is not part of the SolidWorks Standard package. The Scene, Lights, and Cameras DisplayManager is shown in Figure 5.27.

FIGURE 5.27 Using the Scene, Lights, and Cameras DisplayManager

Controlling scenes

In SolidWorks, a scene is composed of three things: a background, which may be an image, a gradient, or a color; a floor, on which shadows and reflections are cast; and an environment, which is a wraparound 3D image (*.hdr or *.hdri — high dynamic range images) that provides light to the model in a rendering and will reflect on the model if the model is a highly reflective material. If the environment is hidden, you only see the background. You can also hide the floor so there are no shadows or reflections and the model appears to hang in space.

Be aware that the small, square image shown for each scene in the Task Pane is a rendering of the scene and does not reflect how the scene will look in the graphics window. For most of this book, I have used the Plain White scene, but my screenshots do not look at all like the preview image.

Floors and environments may only appear when you do a rendering. If you want to remove shadows from the modeling window while you work, use the View Settings icon in the Heads Up View toolbar to do this. This is shown in Figure 5.28.

FIGURE 5.28 Turning off shadows in the modeling window

When you are using Shadows in shaded mode you can take advantage of a special scene called Ambient Occlusion. With this combination, the SolidWorks model can throw shadows on itself, and holes in the model will appear in shadow. It gives some of the effect of a rendering, but it is just the RealView display.

Ambient Occlusion has some limitations, such as it does not show shadows on the part while rotating, only when you stop rotating the view. It also only works when in shaded mode (with or without edges), and when the Shadows in shaded mode option is turned on in the View Display menu.

Figure 5.29 shows a part using Ambient Occlusion, along with the studio scenes folder showing that scene.

FIGURE 5.29 Ambient Occlusion scene gives more realistic shadows without rendering

If you want to turn off reflections on the floor while modeling, you can apply a Basic scene or turn off the reflective floor in the Scene PropertyManager, as shown in Figure 5.30. From here you can also perform other common tasks such as aligning the floor with a different plane, offsetting the floor, and adjusting the brightness of the scene.

FIGURE 5.30 The Scene PropertyManager allows you to turn off the reflective floor while modeling.

To apply a scene to a document, you can use the Appearances, Scenes, and Decals tab of the Task Pane, expand the Scenes heading, choose from Basic, Studio, or Presentation scenes, and double-click or drag the scene into the graphics area. The differences between Basic, Studio, and Presentation scenes are as follows:

• Basic scenes use only a background color.
• Studio scenes use a gradient background.
• Presentation scenes use an HDRI image, so that the image rotates with the part as you rotate the view.

In a recent version, SolidWorks made scenes a document property, so they are now controlled by each individual document, and made that the default option. You can override the default with a system option, Tools Options Colors, and change the Background Appearance setting to anything except the first option: Plain, Gradient, or Image.

Turning on the lights

Lights for the model display in the graphics window are slightly different from the lights for rendering. A certain amount of overlap between OpenGL graphics (normal display) and PhotoView 360 exists. The main difference is that the environment (spherical HDRI image) does not affect the lighting in the model. It does reflect on the model, but does not illuminate it. The lighting in a rendering is predominantly from the environment. You can observe this by editing the scene, going to the Advanced tab, and using the Environment Rotation slider to see what happens. The bright and dark faces do not change, but the reflections do change.

You can add separate lights by right-clicking on the Lights folder in the DisplayManager and selecting one of the new light options shown in Figure 5.31.

FIGURE 5.31 Adding lights to the scene

The light appears as an icon in 3D space, which you can drag around. You can also use the PropertyManager for editing the light to key in a specific XYZ location for the light source or direction.

The symbols shown in Figure 5.30 to the left of the Directional 17 and Directional 18 lights show that the light is On in SolidWorks, and Off in PhotoView.

The easiest and most effective thing to do when you have a part that just displays dark for some reason is to add a single Point light to a model.

The Ambient setting raises the overall brightness of the part, the Brightness setting refers to just the light, and the Specularity slider controls how lights shine or create “hot spots” on curved faces of models. You can even edit the color of a light to give a part a two-tone effect. If you have a blue part and apply a red light that sits to one side of the model, you can get very interesting color effects where the red light reflects off of the surfaces of the part. Lighting effects are most dramatic on curved parts. Parts that are made mostly of flat faces do not reflect light as smoothly as curved faces. This is why even adding small fillets to a rectangular model can help make the part look nicer (more realistic) for presentation purposes. Figure 5.32 shows a comparison of a model with filleted edges compared to a model with perfectly sharp edges.

Working with cameras

You create cameras through the RMB menu on the Scene, Lights, and Cameras DisplayManager, as shown in Figure 5.33. When you add a camera, an interface displays in the PropertyManager, as shown in Figure 5.34.

FIGURE 5.32 Demonstrating the difference between the appearance of a part with fillets and a part with sharp corners

FIGURE 5.33 Adding a new camera with the Camera PropertyManager

In this interface, you can position the Camera object by dragging the triad. To resize the Field of View box, use the controls in the Field of View panel in the PropertyManager. In the graphics window, you can use the left panel to target and position the camera, while the right panel shows the view through the camera.

FIGURE 5.34 Positioning a camera with split windows

You get the most lifelike perspective from a lens setting of about 50 mm. Shorter distances produce wide angle or fish eye lens effects. Larger settings make it look like a telephoto lens. It should be noted that perspective within SolidWorks works much differently. Within SolidWorks, the setting is based on how many object lengths you are away from the object. So if a person is approximately 6 feet tall, and you are rendering that person, you would set your perspective as a factor of six. Three object lengths would be 18 feet.

The Depth of Field panel of the Camera PropertyManager is not shown, because it requires that PhotoView be added in. Depth of field can make objects outside of the focus area slightly out of focus, which can greatly add to the realism of renders.

You can use three methods to switch the graphics window to the Camera view:

• Through the View Orientation dialog box (which you access through the spacebar)
• Through the View Orientation popup menu (in the lower-left area of the graphics window)
• Through the RMB menu on the camera in the Lights, Cameras, and Scene folder in the FeatureManager

When you switch the view to the Camera view, the regular Rotate View command does not function. Rotating the view means moving the camera. You can move the camera by editing the Camera properties, reposition the camera by dragging the triad, or rotate the view while looking through the camera using the Turn Camera tool.

• Camera View. Views the model through a camera. You can use cameras for:
  • Viewing the model from a particular point of view.
  • Creating renderings with perspective and depth-of-field (focus) blur; this feature is only available when PhotoView 360 is added in.
  • Animating the position and target of the point of view in an animation. This feature is only available when a Motion Study is active.
• Turn Camera. Enables you to rotate the camera view when looking through the camera without editing the Camera properties. You must be looking through the camera and it must be unlocked for this to work. Dragging with the MMB does the same thing if the camera is unlocked.
• Draft Quality HLR/HLV. Toggles between low-quality (draft) and high-quality edge Hidden Lines Removed (HLR) or Hidden Lines Visible (HLV) display. This affects display speed for complex parts or large assemblies. When in draft-quality mode, edge display may be inaccurate.
• Perspective. Displays the model in perspective view without using a camera. If you want to create a perspective view on a drawing, you must create a custom view in the View Orientation dialog box with Perspective selected. You can adjust perspective through View Modify Perspective by adjusting the relative distance from the model to the point of view. Relative distance is measured by the size of the bounding box of the model; therefore, if the model fits into a box roughly 12 inches on a side and the perspective is set to 1.1, the point of view is roughly 13 inches from the model. For more accurate perspective, you can use a camera.

• Curvature. A geometrical analysis tool that applies a color gradient to the part based on the local curvature. You can also apply curvature display to individual surfaces through the RMB menu. With some hardware, curvature display can take more time to generate for complex models.

Using RealView

RealView is the display technology behind the fancy appearances of SolidWorks models. The reflections and lighting depend on RealView. If you turn off RealView or if you don't have hardware that supports it, you can't get the great displays. RealView does not affect rendering, just the live display. Check the system requirements listed on the SolidWorks Web site for information about whether your video card supports RealView.

In some situations, you can use RealView instead of rendering. In these cases, RealView acts as a real-time renderer. The main advantages that rendering software such as PhotoView 360 holds over RealView are improved anti-aliasing control, improved shadow control, indirect illumination, global illumination, caustics, and effects such as depth of field from a camera.

You can even use RealView as a diagnostic tool for smooth transitions between surfaces because RealView appearances apply a reflective surface to a part and then apply a reflective background. This is essentially what the Zebra Stripes functionality is doing, but Zebra Stripes applies a specific reflective background to make examining curvature continuity across edges more straightforward.

You can turn RealView on or off by using the golden sphere icon that displays by default on the Heads Up View toolbar. If this icon is grayed out, then your system is not equipped with an appropriate RealView-capable graphics card. Generally, you need an nVidia Quadro series or higher to get RealView capabilities, and an appropriate graphics driver must be installed with the hardware. (NVS series cards are not 3D cards and will not enable RealView.) Some ATI FireGL cards and all FirePro cards will also work.

Exploring the Display Pane

The Display Pane flies out from the right side of the FeatureManager and displays a quick list of which entities have appearances, transparency, or other visual properties assigned. It also shows hidden parts or bodies for assemblies and multibody parts. The Display Pane is shown in Figure 5.35

FIGURE 5.35 The Display Pane allows you to control display elements of your SolidWorks model.

This tool to some extent duplicates the DisplayManager, but it also provides a quick summary of most of the display information, including wireframe/shaded display mode, transparency, hide/show state, and color. It works in both parts and assemblies, and is a highly valuable tool. Between the DisplayManager and the Display Pane, you can easily manage one of the most confusing areas of the SolidWorks software: Appearances.

Applying Color Automatically to Features

You can use the settings found at Tools Options Document Properties Model Display to automatically color certain types of features with specific colors. For example, you can color all Shell features red as you create them.

This function has worked intermittently for many years. For example, you can assign Boss features to always be red, and that works. You can assign surface features to always be yellow, and it works for Extrude, Revolve, Planar, Offset, Loft, and Sweep surfaces, but not for Boundary, Fill, or Ruled.

Using Edge Display Settings

Earlier in this chapter, I discussed the Shaded with Edges display style. Some people think that this makes the parts look “cartoony.” I agree, especially when the default black edges are used, but the display improves when the edge color matches the shaded part color. In any case, sometimes this method is necessary to see the breaks between faces, especially fillets. Cartoony or not, it is also useful.

Taking this one step further, you can also make use of the tangent edge settings. These settings are found in the View Display menu. The settings are

• Tangent Edges Visible. Displays tangent edges as solid lines, just like all other edges.
• Tangent Edges as Phantom. Displays tangent edges in a phantom line font.
• Tangent Edges Removed. Displays only non-tangent edges.

The tangent edges removed setting leaves parts looking like a silhouette. I prefer the phantom setting because I can easily distinguish between edges that will actually look like edges on the actual part and edges that only serve to break up faces on the model. The tangent edges visible setting conveys no additional information and is the default setting. Figure 5.36 shows a sample part with all three settings.

FIGURE 5.36 Samples of the tangent edge settings

Tutorial: Applying Visualization Techniques

Visualization is a key factor when working with SolidWorks software. Whether it is for a presentation of your design to customers or management or simply checking the design, it is important to be able to see the model in various ways. This tutorial guides you through using several tools and techniques.

1. If the part named Chapter5Sample.sldprt is not already open, open it from the DVD. If it is open and changes have been made to it, choose File Reload OK.
2. Practice using some of the controls for rotating and zooming the part. In addition to the View toolbar buttons, you should also use Z and Shift+Z (Zoom Out and In, respectively), the arrow keys, and the Ctrl+, Shift+, and Alt+arrow combinations.
3. Use the MMB to select a straight edge on the part, and then drag it with the MMB. This rotates the part about the selected entity. Also, apply this technique when selecting a vertex and a flat face.
4. Select the name of the part at the top of the FeatureManager.
5. Click the Appearance button from the Heads-up View toolbar at the top of the graphics window.
6. Click the color you want in the Favorite panel. The model should change color. If you click and drag the cursor over the colors, the model changes color as you drag over each new color. You can also drag appearances from the Task Pane. Figure 5.37 shows interfaces for both methods.

   FIGURE 5.37 Use the Appearances PropertyManager to change color and material.

   

7. If the Color panel is not expanded, click the double arrows to the right to expand it. Select the colors you want from the continuous color map. Again, click and drag the cursor to watch the part change color continuously.
8. Create a swatch. In the Favorite panel, select the Create New Swatch button and call the new swatch color file BibleColors.
9. Select a color from the Color Properties continuous map; the Add Selected Color button becomes active. Clicking the button adds the color to the swatch palette. You can add several colors to the palette to use as favorites later on.

   Tip

   You will be able to access these colors again later by selecting BibleColors from the drop-down list in the Favorite panel. You can transfer the colors to other computers or SolidWorks installations by copying the file BibleColors.slddclr from the <SolidWorks installation directory>langenglish folder (or the equivalent file for your installed language).

10. In the Appearance panel, move the Transparency slider to the right, and watch the part become transparent.
11. To prevent the Appearance window from closing after every change, click the pushpin at the top of the window.
12. Click the green check mark icon to accept the changes; note that with the pushpin icon selected, the window remains available.
13. Expand the flyout FeatureManager in the upper-left corner of the graphics window, as shown in Figure 5.38, so that all the features in the part are visible.

    FIGURE 5.38 The flyout FeatureManager

    

14. Select the features Extrude1, Fillet7, and Fillet6 from the FeatureManager so that they are displayed in the Selection list of the Appearances window. Select a color from the BibleColors swatch palette that you have just created.
15. Click the check mark icon to accept the changes and clear the Selection list.
16. Select the inside face of the large cylindrical hole through the part and assign a separate color to the face.
17. Click the check mark icon to accept the changes, and click the red X icon to exit the command.
18. Expand the Display pane (upper-right area of the FeatureManager). You should see color and transparency symbols for the overall part, and color symbols for three features. There is no indication of the face color that is applied.
19. Remove the colors. Open the Appearances window again, re-select the three features (Extrude1, Fillet7, and Fillet6), and click the Remove Color button below the Selection list. Do the same with the colored face. Return the part transparency to fully opaque.
20. Click the check mark icon to accept the changes.
21. Change the edge display to Shaded (without edges). Then change to a Wireframe mode. Finally, change back to Shaded with Edges.
22. Choose View Display Tangent Edges as Phantom. Figure 5.39 shows the difference between Tangent Edges Visible, as Phantom, and Removed settings.

    Tip

    Using the Tangent Edges as Phantom setting is a quick and easy way to look at a model to determine whether face transitions are tangent. It does not help to distinguish between tangency and curvature continuity; you need to use Zebra Stripes for that.

23. Switch back to Shaded display.
24. If you do not have a RealView-capable computer, then skip this step. Ensure that the RealView button in the View toolbar is depressed. Click the Appearances/Scenes tab on the Task Pane to the right of the graphics window. Expand Appearances Metal Steel; then in the lower pane, scroll down to the Cast Carbon Steel appearance.
25. Turn the part over, select the bottom face, and drag and drop the appearance from the Task Pane. Apply the appearance just to the bottom face using the popup toolbar that appears. The rest of the part should retain the semi-reflective surface, as shown in Figure 5.40. Click the check mark icon to accept the change.

    FIGURE 5.39 Tangent Edge display settings for a shaded model

    

    FIGURE 5.40 Applying an appearance to a face

    

26. Click the Section View button on the View toolbar. Drag the arrows in the middle of the section plane back and forth with the cursor to move the section dynamically through the part, as shown in Figure 5.41.

    FIGURE 5.41 A section view

    

27. Select the check box next to the Section 2 panel name and create a second section that is perpendicular to the first.
28. Click the green check mark icon to accept the section. Notice that while in the Section View PropertyManager, the RealView material does not display, but once you close the dialog box, RealView returns.

Summary

Visualization is a key function of the SolidWorks software. It can either be an end to itself if you are showing a design to a vendor or client or it can be a means to an end if you are using visualization techniques to analyze or evaluate the model. In both cases, SolidWorks presents you with an astounding list of tools to accomplish the task. The tools range from the analytical to the cosmetic, and some of the tools have multiple uses.