CHAPTER 14

Automating Drawings: The Basics

Engineering drawings include a lot of repetitious information from one drawing to the next. The information is not always exactly the same, but it is usually in the same format and of the same type. For example, part drawings always include information about who made the drawing, when the person made it, what the material and surface finish of the part are, and some basic notes that depend on the use of the drawing (manufacturing, assembly, or inspection).

All this information needs to appear consistently on each drawing, every time. However, humans are not always good at following dull routines, which is why we have computers to help with these boring or difficult tasks.

SolidWorks drawing templates and formats enable you to automate some of these tasks. SolidWorks can insert information on a drawing's creator and the materials to be used, and start similar types of drawings from a consistent starting point. Drawing templates and formats also save settings that you may want to reuse.

Comparing Templates and Formats

Simply put, templates are collections of document-specific settings and default views saved in the *.prtdot (part template), *.asmdot (assembly template), and *.drwdot (drawing template) file types. In this chapter, I cover the *.drwdot file type.

Formats, more formally called “sheet formats,” are exclusive to drawing documents and contain the sheet size, the drawing border-line geometry, and the text/custom property definitions that go with the text in the drawing border. You can think of a sheet format as an underlay beneath a clear drawing sheet. Formats can also include company logo images.

You can save formats in drawing templates; in fact, this is the method that I use and recommend. Using SolidWorks' default drawing templates, the templates and formats are initially kept separate. You specify the size and the format when creating a new drawing from a blank template. However, when the format is already in the template, the size has already been determined, and so the templates end up being saved as sizes. Of course, you can change formats later if you need to use a larger drawing sheet, but you cannot change templates.

A SolidWorks drawing template can have multiple sheets, which can be the same or different sizes. You can use a different format for each sheet. For example, if you want a default two-page drawing, you can save it as a template, with different formats for the first and second sheets.

Changing existing templates

Currently, once you create any kind of document from whatever kind of template, you cannot change the underlying template. However, you can change all the settings, which is for the most part equivalent.

SolidWorks offers custom drafting standards, which provide some of the functionality that the ability to swap templates would achieve. You can take a drafting standard such as ISO (International Organization for Standardization) or ANSI (American National Standards Institute), make adjustments to it, and save the standard out to a file that you can distribute to other users. You can change the standard by choosing Tools Options Document Properties Drafting Standard from the menus. You can load and save standards from the same location. More details on what you can actually change within the drafting standard come later in this chapter.

While templates cannot be reloaded, formats can be. You might want to reload a format (drawing border and associated annotations) if you have made changes to the information or line geometry. You can also reload a format to change the sheet size for a drawing.

Maintaining different templates or formats

Different formats must be maintained for different sheet sizes. If you do contract design or detailing work, then you may need to maintain separate formats for different customers. Some people also choose to have different formats for the first sheet of a drawing and a simplified format for the following sheets.

If you put formats on the templates, then you are making separate templates for various sized drawings. Also, separate templates are frequently created for different units or standards because templates contain document-specific settings. I also keep a blank drawing template with a blank format on it just to do conceptual scribbles or to make an informal, scalable, and printable drawing without the baggage that typically accompanies formal drawings.

If you work for a company that does a lot of work for manufacturing in Europe, then you may have to deal this issue more frequently. The setting that controls the projection angle is not in Tools Options (where you might expect it to be) but in the Sheet Properties, which you can access by right mouse button (RMB)+clicking anywhere on the blank drawing sheet and selecting Properties.

FIGURE 14.1 Third Angle versus First Angle Projection

Creating custom drafting standards

In my experience, in companies that work in the real world, very few companies follow any of the single drafting standards perfectly. Each company seems to have its own interpretation of, or exceptions to, the standards. SolidWorks is coming to grips with this in a practical way. In SolidWorks, you can create your own custom drafting standards, equivalent to the established ISO and ANSI standards. These standards allow you to save all the settings found in Tools Options Document Properties to a single standard that you can then transfer to other users.

To make your own custom standard, make changes to the various settings for annotations, symbols, dimensions, and so forth, and then go back to the Drafting Standard page of the Document Properties tab, rename the Overall Drafting Standard, and save the standard to a file. I have created a new standard, which is shown in Figure 14.2.

FIGURE 14.2 Creating a new customized drafting standard

The drafting standard file type has the extension of *.sldstd. If someone else has sent you a standard file, you can read it in to your drawing using the settings shown on the right of Figure 14.2 and assign it as the active standard; your drawing will assume all the customized properties.

Creating Drawing Formats

Creating drawing formats can be either simple or difficult, depending on your requirements. Generally, copying existing drawing borders from other drawings imported through DXF (Data eXchange Format) or DWG format is the easiest way to go. Trying to edit an existing border into a different size is usually much more difficult. Adding all the automated annotation information is much easier than editing the lines in the border and title block. What's difficult about it is that SolidWorks is not very good at handling very large sketch data, which is what it considers a drawing format to be. If you disable sketch relations, moving sketch entities correctly can be difficult, and if you enable sketch relations, the performance is very slow.

Customizing an existing format

The simple solution is to customize an existing format of the size or sizes you require for your own use. This generally works well, and you can usually finish the task in a few minutes, depending on your requirements. The easiest option is to take the existing SolidWorks sample formats and add a few things such as a company name, logo, and tolerance block to them. You can also use formats from other drawings, editing and saving them out as your own. If you really need to make extensive edits to a format or create a new one from scratch, I would consider using DraftSight, a free 2D AutoCAD clone provided by Dassault Systèmes, the parent company of SolidWorks.

Using sample formats

The sample formats installed with SolidWorks include ANSI sizes A through E, and ISO sizes A0 through A4. You can probably find enough space on the formats to place a company logo and some standard notes. These templates are located in different directories in Windows XP, Windows Vista, and Windows 7. Choose Tools Options File Locations to locate the path for your templates.

You cannot open a format directly — it must be on a drawing — and, so, to get a closer look at the format, you must make a new drawing using the format.

FIGURE 14.3 Selecting a format

Editing a format

In the drawing, you are either editing the sheet or editing the format. You can think of the sheet as being a piece of transparent Mylar over the top of the drawing border format. In order to get to the format, you have to peel back the Mylar layer. Drawing views go onto the sheet, so when you edit the format, any drawing views that may be there disappear.

To peel back the sheet and gain access to the format, right-click a blank area of the sheet and select Edit Sheet Format. Alternatively, you can also access the sheet format by right-clicking on the sheet tab in the lower-left corner of the SolidWorks window. This RMB menu is shown in Figure 14.4. Be careful of the terms here, which include Sheet and Sheet Format. The sketch lines of the format light up like a sketch becoming active, and the “Editing Sheet Format” message appears at the lower-right corner on the status bar.

FIGURE 14.4 Selecting the edit sheet format

The lines in the format border are regular SolidWorks sketch entities, but they display a little differently. Also, sketch relations are sometimes disabled in formats because solving the relations causes the software to be a bit sluggish. Typically, Trim, Extend, and Stretch functions are the best sketch tools for editing lines.

You can use most common image types to insert logo or other image data onto your drawing or format by choosing Insert Picture. Not all compression styles are supported, however. I have had difficulty with compressed TIFF (Tagged Image File Format) images. Be aware of the file size of the image when you put it into the format, as images can be large, and all that extra information will travel around with each drawing that you create from the format. Figure 14.5 shows a bitmap placed in the format.

You can resize the image by dragging the handles in the corners and move it by simply dragging it. The bottom image in Figure 14.5 was taken from the Print Preview window. I included it here to show that the outline around the image that displays while you are working in SolidWorks does not print out.

FIGURE 14.5 Placing an image

Managing text

SolidWorks allows you to make a text box of a specific size that causes text to wrap. This is particularly useful in drawings. The upper image in Figure 14.6 shows a new annotation being added. The lower image shows the same text box after the corner has been dragged.

FIGURE 14.6 Adding an annotation and wrapping the text

Using custom properties

The most important part of the drawing format is the custom properties. While the rest of the format is just for display, custom properties use automation to fill out the title block using matching custom properties in either the model or the drawing document. Custom properties can pull items such as filenames, descriptions, materials, and other properties from the model associated with the sheet, or they can pull data from the drawing itself, such as the sheet scale, filename, sheet number, and total sheets. If you are seriously looking to automate drawings, you cannot overlook custom properties.

Entering custom property data

Custom property data entry happens at the part or assembly level. This information is then reused in the drawing format and in tables such as BOMs (Bills of Materials) and revision tables, as well as searches using the FeatureManager filter, and all PDM (Product Data Management) systems make use of SolidWorks custom properties. You can enter the data several ways, but the two most prominent ways are through the Summary Information dialog box and through the Custom Properties Tab in the Task Pane.

Using the Summary Information dialog box

Figure 14.7 shows the Summary Information dialog box. This functionality has existed in SolidWorks for several releases. You access this dialog box by choosing File Properties from the menus. You can select Property Names from a drop-down list or type in your own, assign types of data, and enter in a specific value for the property. The Value/Text Expression column also has a drop-down list from which you can select several preset variables, such as mass, density, and even link values used in the part.

FIGURE 14.7 The Summary Information dialog box

This is a perfectly functional way of entering data, but the fact that it is somewhat out of the way, hidden in the menus, means that it does not get used as much as it should. So SolidWorks came up with another way of entering data.

Using the Custom Properties tab

The Custom Properties tab of the Task Pane enables you to quickly and easily access and assign custom properties within a document. Figure 14.8 shows the process of building your own Custom Properties tab. You can start the Custom Property Tab Builder by either clicking the Create button on the Custom Properties tab or choosing Start Programs SolidWorks SolidWorks Tools Property Tab Builder from the menus.

FIGURE 14.8 Using the Custom Properties Builder and Custom Properties tab

The interface enables you to add drop-down lists, toggles, and text entry boxes. This gives you a lot of flexibility with custom property data entry and is a very nice addition to the software.

Displaying property links

Figure 14.9 shows the existing custom property formatting in the default format being used for this example.

FIGURE 14.9 Custom property formatting in the title block

The syntax $PRP or $PRPSHEET indicates that the property that follows the syntax is to be pulled from either the current document (drawing) or from the model specified in the Sheet Properties, respectively. This is an important distinction to make. Most of the time, you can type custom properties in at the part or assembly level so that you can reuse the data by drawing properties, BOM, or even design tables.

Notice that all the notes in the format that are showing raw syntax are pulling data from the model. “Draw2” and the Scale notes are driven by the drawing. When no value exists for the property to display, you have an option of what to show. The top portion of Figure 14.10 shows the settings in the View menu that control the display of syntax of the custom property links. In general, it is common to deselect the error display and to show the link variables.

FIGURE 14.10 The link variable's display options and effects

Displaying errors and link variables

The errors in Figure 14.10 are caused by links to the local document for which there is no corresponding property. For example, the “ERROR!: COMPANYNAME” message is linked to “$PRP: COMPANYNAME,” but the local custom property COMPANYNAME does not exist. If it existed but had a null or space value, the error would disappear.

Likewise, with the option to display link variables selected, the syntax that calls model custom properties displays until there is some value for it to pull from. If a part is put onto the drawing, then some of the properties are filled in because properties and values exist to pull from, and the rest of the properties simply disappear to make space. Notice in Figure 14.11 that the Material property has been filled in, but the Finish property has not. This is because either there is no Finish property in the part on the drawing or there is a null value in the Finish property.

FIGURE 14.11 Custom properties filled in by a part

Creating linked properties

It is easy to create annotations that are linked to properties. Begin as if you are creating a note:

1. Click the Note toolbar button on the Annotations toolbar, or choose Insert Annotations Note.
2. Place the note on the drawing. The Formatting toolbar appears.
3. Click the Link to Property button in the Text Format pane of the Note PropertyManager. This displays the Link to Property dialog box, as shown in Figure 14.12, which gives you the option of linking to a custom property in the current (drawing) document or in the model (part or assembly) that is on the drawing.

   FIGURE 14.12 The Link to Property dialog box

   

4. If the desired custom property is not in the drop-down list shown to the right, then you can type it into the text box or click the File Properties button to edit the properties. If the property is added to the part file or a part file with that property is used on the drawing, this linked annotation will pick it up. This button is not available for the model if there is no model on the drawing, in which case you must type in the name of the property manually.

Using the Title Block function

The Title Block enables the person who sets up the sheet format to specify an area that contains notes that are easy to access without editing the format. (Many CAD administrators prefer that the users not have to deal with the details inside the Sheet Format.) You can even cycle through these notes in a specific order by pressing Enter or Tab. Figure 14.13 shows the resizable black border of the Title Block, the Title Block PropertyManager, and where the Title Block sits in the drawing FeatureManager.

FIGURE 14.13 Using the Title Block function

You can access the Title Block to edit or define it by right-clicking in the Sheet Format (while editing the Sheet Format, not the sheet) and selecting either Define Title Block or Edit Title Block, as the situation requires.

The Title Block can be any size you like, but it must remain rectangular, and you can only create one Title Block area per sheet format. The area bounded by the Title Block box is used to zoom the display to make it easier to fill in the text boxes. If you want to include areas in different corners of the drawing in the Title Block area, you will need to make the Title Block box as big as the entire sheet, and the user will have to manually zoom to each corner.

Select each Note item to add it to the list in the PropertyManager selection box. Use the arrows to the left of the box to assign the order in which the user cycles through the boxes. The idea is that the user clicks in a box within the Title Block area, fills it in, then presses Enter or Tab to get to the next box. The order will loop if the user does not start on the first box listed in the PropertyManager.

Creating a format from a blank screen

SolidWorks is not good at manipulating a lot of 2D sketch-line data, such as what you find when drawing title blocks. I have gone through the process of making my own formats, as well as the process of importing DWG data from which to create them. If you choose to custom build one size and then use it to create the rest of the sizes, you need to be patient. SolidWorks typically turns off the most useful parametric sketch functions when working with a format (what SolidWorks considers a large sketch) because of speed problems. If you would like to turn on these settings, you can find them by choosing Tools Sketch Settings.

If you insist on creating your own borders and title blocks, set aside some time for it and have an idea of what you are trying to achieve, maybe sketched out by hand or in a printout of a title block that you would like to replicate. You can also use the free 2D tools DWG Editor or DraftSight, which are much better suited to this kind of work.

The Modify Sketch tool may be useful for moving entities around the screen, and even scaling them. You can also access a useful hidden command by right-clicking the name of the drawing in the FeatureManager and selecting Move from the menu, as shown in Figure 14.14. A small dialog box appears that enables you to move the entire format by a specified distance.

FIGURE 14.14 The Move Drawing dialog box

Creating a format from an imported DWG/DXF file

If you want to create your format from an imported DWG or DXF file, choose File Open to locate the file that you would like to import and then click to open it. The DXF/DWG Import screen appears, as shown in Figure 14.15.

FIGURE 14.15 The DXF/DWG Import screen

You can find the sample files used for this example on the DVD for Chapter 14 if you are interested in following along. You will find five *.dwg format files. You can use any of them to create a format, but I suggest either the A or B size. To make a drawing format, you can select the Create New SolidWorks drawing and Convert to SolidWorks entities options. Although one of the other options contains the word format, it is not being used in the same sense, so do not be misled. When this selection is complete, click Next. Figure 14.16 shows the next screen.

FIGURE 14.16 The Drawing Layer Mapping screen

Select the Layers selected for sheet format option. Select the TB layer, leaving the other layers unselected. Every imported file will be different in this respect, because layers used by title blocks vary widely. Click Next when you have made these selections. Figure 14.17 shows the Document Settings screen.

FIGURE 14.17 The Document Settings screen

The important features in the Document Settings screen are the Document template selection and the Geometry positioning options.

Document template selection is only important if you plan to save the format with a template. Be sure to select a template that does not already have a format saved in it. In the Geometry positioning section, if you can get the software to center the title block for you, definitely take advantage of this functionality and use the Center in sheet option. Once you are happy with these settings, click Finish. The resulting format is shown in Figure 14.18.

FIGURE 14.18 The finished imported format

From here, you can add the links to custom properties as described earlier, as well as logo images, loading favorites, and blocks. You can now save the format as described in the next section.

Saving the format

You can save drawing formats in two ways: either with the template or separate from the template. You cannot edit formats separate from a template, but they do have their own file type, *.slddrt.

Saving templates is covered in the next section. To save a format, choose File Save Sheet Format. You can do this with or without the format being active. Save the format into a location with other formats and give it a descriptive but unique name. If you have not yet done so, this is a good opportunity to create a separate folder, outside of your SolidWorks installation folder, that contains your most frequently used files. Remember also to tell SolidWorks where this library location is by choosing Tools Options System Options File Locations Sheet Formats.

Even if you have saved a format with a template, it is a good idea to also save the format on its own. This is because you might want to use that format on an existing drawing that has a different format on it or use it on a second sheet.

Using second sheet formats

When you have multi-sheet drawings, it is often important to have a simplified or specialized format for the second sheet. Figure 14.19 shows sample page-one and page-two formats side by side.

FIGURE 14.19 First and second sheet formats

Adding new sheets

You can add sheets to a drawing by clicking the Add Sheets icon to the right of the sheet tabs at the bottom of the SolidWorks window or through the RMB menu of the sheet tab at the lower-left corner of the drawing window. If you right-click the first sheet tab, the sheet that is added gets the format that is used on the first sheet. If you right-click the second sheet tab, the added sheet gets the second sheet format.

Reloading formats

If a format has been changed, and you would like to update a drawing to the new format, this option is available in the Sheet Properties, as shown in Figure 14.20.

FIGURE 14.20 Updating a format through the Sheet Properties

Creating Drawing Templates

Document-specific settings are an important part of the template, and it is probably best to get one drawing size completely set up the way you want it, and then create the other sizes from this drawing. This helps to ensure that the settings, such as bent leader length, font, and line weight, are the same for all the templates. Uniform settings on drawings give them a consistent look and make them easier to read. An in-depth discussion of document-specific settings at Tools Options Document Properties can be found in Appendix B. Drafting standards are also controlled by drawing templates.

Using Pre-defined Views in drawing templates

When I use drawing templates, one of my favorite techniques to get to a multi-view drawing quickly is to put one Pre-defined View on the template along with appropriate views projected from the Pre-defined View. A Pre-defined View establishes an orientation and location on the drawing sheet. You can add multiple Pre-defined Views and align them with one another on the drawing sheet so that a drawing is automatically populated by the model, but this is not recommended because if you decide to change the orientation of the drawing, you have to change each Pre-defined View independently. If you set up a single Pre-defined View and make the rest of the views with Projected Views, changing the orientation of the Pre-defined View causes all the Projected Views to update associatively. You cannot directly change the orientation of a Projected View. Pre-defined Views and views projected from Pre-defined Views appear blank until they are populated with model geometry. The pre-defined part of a Pre-defined View is the orientation and placement of the view.

Figure 14.21 shows a template using Pre-defined and Projected Views. You can access Pre-defined Views on the Drawings toolbar; although it is not there by default, you can place it on the toolbar by choosing Tools Customize Commands and using the interface. You can also access Pre-defined Views by choosing Insert Drawing Views Pre-defined. Projected Views are also accessed from the Drawings toolbar.

FIGURE 14.21 Pre-defined Views on a template

Once a Pre-defined View has been placed, you can select an orientation for it from the PropertyManager. Figure 14.22 shows the Drawing View PropertyManager. The orientation for a view is set in the top Orientation panel. In addition to orthogonal views, you can also create isometric and other custom views as Pre-defined Views.

After the view has been oriented, you may want to create more views on the drawing that also become populated by model geometry. This is where the Projected Views are used. Make sure that the drawing properties are set to the correct projection angle.

Because the rest of the views have been created relative to the Front view, none of the views needs to be rotated as it would if, for example, the Top view was placed above the Back or Right view.

Although it is not on this drawing, many drawing templates include a Third Angle Projection symbol as a part of the Title Block, which is in the format. Figure 14.23 shows First and Third Angle Projection symbols. These are included as blocks with the sample data in the SolidWorks installation. Blocks are discussed in more detail in Chapter 16.

FIGURE 14.22 The Drawing View PropertyManager

FIGURE 14.23 Projection angle symbol blocks

Aligning Pre-defined Views

You can align views to one another through a view's RMB menu, as shown in Figure 14.24. Projected Views are aligned to one another automatically, but if you chose to use a Pre-defined View rather than a Projected View to one side of the original Pre-defined View, you can use the Align Vertical by Origin or the Align Horizontal by Origin command. This ensures that the parts in each view are aligned. Aligning by center should not be used for Projected Views on an engineering drawing, because it is not guaranteed to line up edges in adjacent views.

FIGURE 14.24 Selecting view alignment options

Populating a drawing with Pre-defined Views

Four methods exist to populate a drawing with Pre-defined Views:

• Drag-and-drop. Drag a part or assembly from the FeatureManager and drop it in the drawing window. All Pre-defined Views are automatically populated.
• Insert Model. Right-click a view and select Insert Model. From the interface, browse for the model to be displayed in all the related (projected) views.
• PropertyManager. Select a Pre-defined View, and from the PropertyManager, select Browse in the Insert Model panel.
• Make Drawing from Part/Assembly. Click the Make Drawing From Part/Assembly button in the Standard toolbar and select a template that uses Pre-defined Views.

Scaling Pre-defined Views

When Pre-defined Views are created, they are set to follow the sheet scale by default; however, you can manually set them to have a custom scale. If you are using the automatic scaling option (found at Tools Options System Options Drawings Automatically Scale New Drawing Views), the sheet scale is automatically changed when the drawing views are populated to make a nice fit of the model geometry on the drawing. The scales used by the automatic feature are all standard multiples of two, so you do not have to worry about odd scale factors on your drawings.

Understanding the limitations of Pre-defined Views

The function and expectations of Pre-defined Views are fairly straightforward, although there are a few things that could be improved. For example, SolidWorks does not allow you to create pre-defined section or detail views. Also, the View Palette does not preview the populated Pre-defined Views.

Using styles and blocks in templates

The functionality formerly known as favorites is now known as styles in certain parts of SolidWorks, although you will find other parts where the term favorites is still used. In SolidWorks, styles function like styles and formatting in Microsoft Word, or other word-processing software, by adding underlines, bold formatting, and even items such as tolerances and symbols. Hole Wizard Styles are described in Chapter 13, and work similarly to Dimension and Note Styles (described in Chapter 16). This chapter addresses the fact that styles can be saved to files and loaded to documents. In particular, they can be loaded to documents that can be saved as templates, thus maintaining the loaded styles. Several types of styles can be loaded into and saved with drawing templates, including dimension, note, GD&T, weld, and surface finish symbols.

When a style is loaded into a template, any document that you create from that template can use any of the loaded styles. The many file types for styles exist mainly to transfer styles from one document to another, but they are not needed once the style is loaded. As a result, before saving a template, you should gather together your styles into your library folder and load them into the template.

You can load styles by going to the interface for the type of favorite; for example, dimensions or notes. Figure 14.25 shows the top of the Note PropertyManager interface, which contains the Styles panel.

FIGURE 14.25 The Styles panel for the Note PropertyManager

The buttons in the Styles panel of the Note PropertyManager interface have the following functions, from left to right:

• Apply the default attributes to the selected notes
• Add or update a style
• Delete a style
• Save a style
• Load a style

This section is concerned with the last function, Load a style. After clicking this button, you can load multiple styles at once by Shift+selecting them through the Open dialog box that appears.

Even symbol types that can be applied by dragging-and-dropping from the Design Library can also be loaded as styles. However, I prefer dragging from the Design Library because you get a preview of the symbol; with the styles, you just see a text tag.

Blocks can also be loaded into a template or used from the Design Library as drag-and-drop items.

Using custom properties in templates

Part of the usefulness of templates is that you can do work once and have it replicated many times. This is an excellent example of process automation. One of the ways that you can take advantage of this feature is by putting default custom properties in your templates. In many cases, simply having a default value for something is better than no value, and a default value may even prompt you to put a value with real significance in the property. For example, the Description of a document is extremely important, especially if you are using sequential part numbers for your filenames. A custom property named Description can be added to your template, and the default value is used unless it is changed when the template is used in a document.

You have already seen how custom properties used in parts can be instrumental in filling out a title block on a drawing. Custom properties in part and assembly documents work exactly the same as they do in drawings. The custom properties interface is shown in Figure 14.26.

FIGURE 14.26 The custom properties Interface

Saving a template

To save drawing templates, choose Save As Files of Type and then select Drawing Templates from the drop-down list. This automatically takes you to the folder for the templates, as specified in Tools Options File Locations Templates.

In the case where a template and format have been saved together and are being saved together, but the format also needs to be saved to its own file, saving the template with the changed format only changes the format for documents that are made from that point forward with that template.

You may also save out the format to its own file from the edited template. Formats are needed in their own file (in addition to existing within a template) for situations when you have an existing drawing and want to change the size of the sheet and then need a format to put on the sheet. Another situation is when a drawing may come in to your organization from an outside contractor, and they have not used your format; in this case, you can simply replace their format with yours, or you can send them your format (and template, for that matter), from which the contractor can create all drawings for you.

Separate formats are important for when you have multi-sheet drawings. When adding a sheet, you also need to add a format. You can save multi-sheet drawing templates in which the first and second sheets have different formats on them.

Creating Blocks

Blocks are an important aspect of automating drawing creation. They enable you to combine text and sketch geometry and to annotate common features on drawings. Blocks are discussed in Chapter 4 and also in Chapter 16 (creation, editing, and placement). Blocks can be used for many purposes, including the following:

• Tolerance blocks on drawings that might change with the process (if you do not have separate formats that already contain this information)
• Electrical or pneumatic schematic symbols that can be snapped together
• Flowchart type symbols
• Fluid flow-direction arrows
• Special markers calling attention to a specific detail
• Sheet formats that can be created as a block, enabling you to move it around as a single entity much more easily

You can create blocks by selecting a group of sketch entities, annotations, or symbols and then choosing Tools Block Make.

Summary

Getting your templates and formats correct creates an excellent opportunity to save some time with drawings by automating many of the common tasks using templates, Pre-defined Views, multiple formats, blocks, favorites, and linked custom properties. Setup becomes more important when you are administering a larger installation, but is also important if it is just for yourself. One of the most important things that you can do is to establish a file library and direct your Tools Options File Locations paths to the files. There is nothing quite as productive as having something that works right the first time, and every time.