IN THIS CHAPTER
Using notes
Using blocks
Using symbols
Using center marks and centerlines
Tutorial: Using annotations
Annotations and symbols are a major component of communicating a design through a drawing. SolidWorks has several options available to help you manage these entities to make engineering drawings look good and communicate effectively.
Sometimes users have difficulty working through some of the interfaces in SolidWorks. This is not necessarily the fault of the software, but is often because users may not fully understand how the workflow of a particular feature is supposed to function. The Model View interface from the last chapter is one that can be confusing until you have been through it a few times and gain a more intuitive feel for how it works.
Understanding the workflow is paramount to being able to use the software efficiently. I sometimes find myself using the Annotations clumsily, and sometimes wind up with blank notes, double notes, or extra lines at the ends of notes. After using the tool a few times, I get back in the groove.
For these reasons, I have added some step-by-step suggestions here to help you establish expectations that will enable you to use a fast workflow with annotations.
Follow these steps to create a note:
Click the Note toolbar button on the Annotations toolbar.
Click in the graphics window where you want to create the note or click an entity that you want the note leader to point to, and then click where you want the note.
Type the note. Press Enter at the end of a line, or, if you intend to force the note to wrap, just allow the line of text to be as long as it wants to be. While you create the note, the text box expands to the right until you press Enter, and it expands down every time a line is added.
At the end of the last line of the note, do not press Enter again (this creates extra lines) and do not press Esc (this causes the entire note to disappear).
To finish the note, click the mouse outside of the text box. After that, if you are done, press Esc. If you want to continue with another note, click again to place it, and start typing. If you want to place the same note as the first one again, the text is already there, so click a second time.
If you are a long-time SolidWorks user, you will be pleased to know that in recent versions of the software, different pieces of text within a single note can be formatted with multiple fonts, multiple sizes, bold, italics, underline, and so on.
The Fonts toolbar displays with two different names. If you use it in the CommandManager, it displays with the Fonts name, with the icon shown at the beginning of this Fonts section. In Tools, Customize, the Fonts toolbar displays as the Formatting toolbar. The Formatting toolbar also appears in the graphics area immediately over your text every time you either insert a new note or edit an existing note, unless the toolbar is already docked somewhere. The Formatting toolbar is shown in Figure 22.1.
Text boxes are a more recent addition that enables the user to limit the size, particularly the width, that a note can occupy. This enables notes to wrap in tight spaces on title or revision blocks, as well as other places.
You can size text boxes immediately after placement, even while they are blank; the text then wraps as you type it. The text box expands downward automatically. Blank text boxes can be left on the drawing to provide a placeholder for future text. The blank text box has a rectangular border that contains an X, both of which are removed when you add text. If spaces are added to a text box, the text box becomes invisible, although you can select it if you know where it is. When you move the cursor over the text box, the cursor displays the note symbol. Text boxes do not highlight when window selected.
While typing a note, it is not possible to resize the note using the middle handle on the right end of the box; you should use the lower-right corner handle, as shown in Figure 22.2.
If a custom property is used to populate a note, and the value of the property is long, you may have difficulty getting the text of the property to wrap. One way to accomplish this is to make the font of the note very small, then size the box to the appropriate size, then set the note font back to the original size. The text now wraps to fit the box.
When you start to place a note, a preview shows the text box with or without a leader depending on the position of the cursor. If the cursor is over a blank section of the drawing, the note is placed without any leader. If the cursor is over a face, edge, or vertex, then a leader is added using the arrow controlled by the settings at Tools
Figure 22.3 shows the preview that is displayed by the cursor when you place a note over a face, over an edge, and over blank space on the drawing.
You can also change settings for bent leaders in the Tools
Some minor but basic functionality appears to be missing from notes in SolidWorks. Single-clicking inside an active text box places the cursor between letters, as expected. Double-clicking inside an active text box selects the entire word that you click, again as expected. Triple-clicking in Microsoft applications such as Word and PowerPoint generally selects the whole paragraph or the contents of the text box. However, the triple-click option is not available in SolidWorks notes. Ctrl+A does work to select all of the text inside a text box. To format the entire note, do not activate the text box; instead, only select the note, and apply the setting to the entire note rather than to selected text within the note.
You also cannot drag-and-drop selected text to move it within a text box. However, you can Ctrl+C, Ctrl+X, and Ctrl+V the text.
To add a leader to a note that was created without a leader, click the note and select the leader options in the Leader panel of the PropertyManager, as shown in Figure 22.4. After you add the leader, you can reposition the handle at the end of the leader to attach it to an entity on the drawing.
You can also attach multiple leaders to notes. To create a new note with multiple leaders, preselect the entities that the leaders are to be attached to, and then click the Note toolbar button.
To add a leader to an existing note, first click the note, and then Ctrl-drag the handle on the end of the leader to the second location. A note with multiple leaders is shown in Figure 22.5. To remove one of multiple leaders from a note, click the handle at the end of the arrow and press Delete.
Jogged leaders have come a long way since their introduction many releases ago. You can switch a regular leader to a jogged leader by selecting an option in the PropertyManager. In Figure 22.4, the middle icon in the top row is the Jogged Leader icon. The icon to the left simply turns on the default leader, and the icon to the right turns off leaders altogether.
Once you activate the jogged leader option, you can add a jog from the leader RMB menu. Notice in Figure 22.6 that two options give you control over the jogged leader.
Selecting the Add Jog Point command adds a new handle to the leader that you can move around. You can add multiple jog points to the leader.
The Insert New Branch command enables you to create a new jogged leader that ends in another arrow from the selected point. This arrangement with multiple branches in a jogged leader is shown in Figure 22.7.
For notes, a favorite can apply a font, an underline or bold formatting, or any other setting from the Formatting (Fonts) toolbar.
To create a note that uses the favorite setting from another existing note, pre-select the existing note before starting the Note command; SolidWorks applies the favorite to the new note.
Note
Sometimes adding a favorite to a note can make other changes that you may not expect, such as turning off the leaders if a note has multiple leaders. In particular, if the favorite is made from a note with a jogged leader, then it turns off leaders for regular multiple leaders. Favorites that are created from regular leader notes do not turn off jogged leaders.
Making a change to the leader of a note after you apply the favorite removes the favorite from the note, although the formatting remains. This does not apply to adding multiple leaders, only to changing the type of leader.
Applying a favorite may also remove the ability of the text to wrap, as well as any changes to the text box shape. You cannot move the corner of a text box of a note to which you have applied a favorite.
Favorites exist only in the document in which they were created, but they can be shared to other documents by saving the favorite out as a separate file. Note favorites use the extension, *.sldnotefvt. Once you save the favorite, you can load it into other documents. The Favorites panel of the Note PropertyManager interface is shown in Figure 22.8.
The Favorites panel contains the following buttons:
Favorites can be loaded into document templates so that for every document created from the template, those Favorites will be available.
You can link notes to custom properties. The custom properties can be from the drawing, or from the model that is referenced by the drawing. This kind of link is also mentioned briefly in Chapter 20, but I discuss it more thoroughly here.
Figure 22.9 shows a note on a drawing with custom property links pulling data from the model shown on the drawing. To add these links, driven by the syntax $PRPSHEET:"material", click the icon indicated in the image to the right in Figure 22.9.
In this case, text has been combined with custom properties, but custom properties can also appear alone. The Custom Properties interface is found at Tools, Properties.
Hyperlinking text is sometimes useful on drawings to provide a link to reference documentation, specification, test results, and so on. The first button in the Text Format panel enables you to add a hyperlink to text in the note. Either copy the URL to the hyperlink dialog box that appears, or browse to it from the dialog box.
Notes and symbols are regularly combined in SolidWorks. Symbols are discussed more fully later in this chapter, but are mentioned here because of the frequency with which they are used with notes. The image to the right in Figure 22.9 shows the Text Format panel, which contains a button to the interface where you can add symbols.
Blocks in SolidWorks can contain sketch elements and notes. When used in drawings, blocks have several common uses, including the following:
Standard note blocks for tolerances, disclaimers, or default requirements
You can put together a mechanism in 2D where each block represents a part
Flow direction for fluid systems
Drawing stamps such as "Not For Release," "Preliminary," "Obsolete," and so on
Symbols for schematics which can be snapped together
You can save drawing templates as blocks to make them easier to place as a single entity
Like favorites, blocks reside in the document in which they are created, but you can save them out to a *.sldblk file, load them into other documents, and save them as a part of a document template.
Each block has an insertion point, which snaps to any sketch entity endpoint, even if it is in another block. This makes schematics easy to snap together. If the default insertion point is not the point that you need to snap to the other geometry, then you can place the block anywhere on the drawing and drag the point that needs to snap.
Once blocks are snapped together, to detach them from one another, you can click the point at which they touch; a Coincident sketch relation displays in the PropertyManager. Deleting the sketch relation enables you to drag the block away from the other geometry.
When blocks are inserted, you can control several options in the PropertyManager. This function may be somewhat hidden because it does not appear automatically when you place the block. After you place the block, SolidWorks wants you to place another copy of the block. If you press Esc to cancel out of placing additional blocks, then the first placed block is not selected, and so the PropertyManager does not display. Figure 22.11 shows the Block PropertyManager.
This panel lists the sketch relations that are linked to the block. These may cause the block to not move properly when you drag it. This feature is most helpful when the block is being used as a representation of a part in a simulated 2D mechanism.
Blocks can be linked to an external file, which enables all linked instances of a block to be updated at once, even if they are being used in other drawing documents. The path box for the Link to File option only displays if you select the check box.
The Edit button refers to editing the block. A toolbar button also exists for editing blocks. The Leader & Insertion Points button enables you to edit both of the controls. You can use the For Construction option to change any sketch entities in the block to construction entities.
The top field with the two circles to the left controls the scale of the block. This number affects the entire block, including the text. You also have the option to scale dimensions.
The Lock Angle option refers to the rotation of the block. If the Lock Angle option is not selected, then you can rotate the block if one point on it is coincident to a stationary object, such as a vertex in a drawing view.
You will recognize these options from the Notes leaders. The leader is attached to the block where the angled black handle was placed when you created the block.
The Display Dimensions option controls whether or not any notes and dimensions in the block are displayed or hidden.
Note
Sketch Blocks have been covered in some detail in Chapter 4. The current chapter is limited to a discussion of blocks that may be found on drawings rather than those used in model sketches.
By default, when you create a block, the Insertion Point panel of the PropertyManager does not expand. If you expand this panel, the blue Origin symbol represents the insertion point that is attached to the cursor during block insertion, as shown in Figure 22.12. The angled line hanging off of the left side of the block is the leader attachment point for the block. You can also drag this line around the block and snap it to sketch geometry. By default, this block does not use a leader, but if one is required, then you can turn it on when you place the block.
The Edit Block toolbar button on the Blocks toolbar
The Edit button in the Block PropertyManager
Through the menus at Tools, Block, Edit
From the RMB menu of the block in the Blocks folder in the drawing FeatureManager
The standard edit function gives you access to the sketch and note elements that make up the block.
SolidWorks symbols are different from symbols that are a part of a font family. SolidWorks symbols fall into several categories including, weld, surface finish, hole, modifying symbols, GD&T, and several flag symbols. You can also construct custom symbols.
You can use symbols in notes and dimensions. They also are an intrinsic part of weld symbols and surface finish symbols. Hole Callouts use symbols extensively, as do GD&T (geometric dimensioning and tolerancing) frames.
Figure 22.13 shows the Text Format panel from the Note PropertyManager and the Dimension Text panel from the Dimension PropertyManager. Both of these interfaces give you access to the symbol library.
You can create custom symbols in SolidWorks, but creating them may not be as simple as you expect. In the langenglish subfolder of the SolidWorks installation directory is a file called Gtol.sym. This is the file that stores the representations of all of the SolidWorks symbols. This is also the file where you can create symbols of your own. You can edit the file in Notepad.
As a warning, unless you enjoy writing scripts for the command line, or you are a fan of DOS 5.0, then you may not want to create custom symbol projects. The format for creating symbols is simple enough, but it is what you might call somewhat arcane. It is effective at creating line-art symbols that can be used with text and can even be used to contain text. If you are a little inventive with this, then you can create interesting shapes that integrate with your notes and dimensions.
Keep in mind that this topic does not appear in the Help files, but all of the instructions you need are inside the file itself. You may have to experiment a little to discover what the rules are in terms of making shapes outside of the limits of the 1X1 matrix.
Note
Starting with 2007, there is now an option in Tools
Figure 22.14 shows some of the options that are available for center marks.
Center marks propagate well to patterns, and you can dimension to them individually. You can rotate center marks in views where they need to be referenced from an edge that is not parallel to horizontal. You can also place center marks into layers.
You can apply centerlines to any geometry that has a temporary axis that is perpendicular to the drawing sheet. Centerlines can also be placed automatically when you place the part into the drawing. You can create centerlines by selecting a face or a pair of parallel lines or concentric arcs. Centerlines may be displayed improperly on parts that are created by mirroring, as shown in Figure 22.15.
This tutorial shows you how to use some of the tools that were discussed in this chapter. It does not cover every feature, and so you should explore a little on your own, and not necessarily follow the instructions exactly. Start here:
From the CD-ROM, open the file named Chapter 22 – Tutorial.slddrw. This is a drawing file with views of the part from Chapter 21, but it does not contain dimensions or annotations.
Click the Center Mark tool on the Annotations toolbar. (If the button is not there, then use Tools, Customize, Commands to place it on the toolbar, along with the Centerline tool.) Click one of the holes in the pattern of three, and click the Propagate symbol to propagate the center marks to all three holes in the pattern. The view should look like Figure 22.16 when you are done.
Activate the Centerline tool to add two centerlines to the right view, in the lower-left area. Select the cylindrical faces for each feature to place the centerlines. Click the vertical centerline and drag the ends past the edges of the part.
Select the edge that is indicated in Figure 22.17, and initiate a note from the Annotations toolbar. Type the text shown, all in one line. You can place the degree and diameter symbols from the symbol library, which you can access using the indicated button in the PropertyManager. Both symbols are in the Modifying Symbols library, also shown in Figure 22.17. Drag the lower-right corner of the text box to make the text wrap as shown.
Draw an arrow with a text note inside it, as shown in Figure 22.18. Make the sketch and text into a block by window-selecting all of it and clicking Make Block from the Blocks toolbar, or by selecting Tools
Place the block using the Insert Block function, so that the block is to the right of the right view. Once you place it, press Esc to cancel the placement of more blocks. Then select the block to activate the PropertyManager. Deselect the Lock Angle option, and set the angle to 270 degrees.
Annotations and symbols in SolidWorks have many options for connection, creation, and display. Recent releases have brought major improvements to text box–driven annotations. Custom properties and hyperlinks allow the user to populate drawing annotations with content and links to content. Sharing favorites in templates is a great idea for readily available note styles.
Blocks have several flexible uses and can be updated from external files across many documents. Their use for simulating mechanisms, piecing together schematics, and annotating drawings, in addition to the Belts and Chains functionality discussed in Chapter 13, make blocks one of the most flexible functions available.