Autodesk Mechanical Desktop: Annotation Standards By Bill Fane
In the last article, Mechanical Desktop? 5: It Is Not Your Default, we covered most of the major areas involved in setting up a Mechanical Desktop drawing. These include the layers you should create to make it easier to work in part-modelling mode and how to set up the major options for drawing mode. Now we're going to look at the annotation standards available in Mechanical Desktop Releases 4 and 5.
Of course each drawing must implement an annotation standard—for symbols, parts lists, text, and so on—and Mechanical Desktop provides all the major international standards, including ANSI.
Mechanical Desktop Release 4 Here's how you access the annotation standards in Mechanical Desktop 4: 1. From the main menu bar, click Annotate > Symbols > Symbol/BOM standards. Clicking a standard makes it current. 2. Right-click on any standard and select Properties from the shortcut menu. A dialog box appears from which you can control text size and color, arrowhead style, and so on. (In earlier releases, these items were controlled by the current dimension style.) 3. Access more standards options by clicking the + sign, then right-click to select options in each category.
Note: Symbols and parts lists are inserted in the current drawing layer, and their color is set independently by the symbol standard. Mechanical Desktop Release 5 To access the annotation standards in Mechanical Desktop 5:
View Larger Image Figure 1: The Standards tab of the "Mechanical Options" dialog box.
1. Select any pop-down menu that is unique to Mechanical Desktop (such as Part, Assembly, Drawing, or Annotate) from the main window. 2. Click ...Options located at the bottom of any of these pop-down menus. The Mechanical Options dialog box appears (see Figure 1, showing the Standards tab). 3. Pick any standard from the drop-down list in the Standard field. 4. Double-click the standard in the right-hand pane to expand it. 5. Double-click any section of the standard to adjust its properties. Release 5 has several more sections than Release 4, the most significant of which is Layer/Objects. In Mechanical Desktop 5, many annotation objects have predefined layers instead of using the current one.
View Larger Image Figure 2: Some of the layers that Release 5 creates automatically.
If you right-click on Layer/Objects, the Layer/Objects dialog box opens, from which you can set the properties of the layers for each type of symbol or portion of annotation (see Figure 2). Release 4 and earlier used an AM_xxx format for layer names, where "xxx" described the layer's purpose; for example, it would be fairly obvious that AM_PARDIM held parametric dimensions. New layers defined by Release 5 use an AM_n format, where "n" is a number; it's no longer obvious which layer is used for what. The good news is that you can use the drop-down list in the Filter field to filter groups of layers. Or you can select the Objects tab in this dialog box in conjunction with Filter to get a better idea of what each layer does.
You could use the Layer functions to predefine annotation layers whose properties you wanted to be different from the default values. But if you've got Release 5, I recommend using the Standards tab to predefine layers. With the Standards tab:
View Larger Image Figure 3: The Dimensioning dialog box can set the default dimensioning style for use in 2D drawing views.
Layers are created only as they are needed. If you let Standards do it then your drawing will not be cluttered with unused layers. More significantly, Release 5 creates its new annotation layers based solely on the AM_n layers; it will ignore your predefinitions and use the Standards settings. Thus any effort you put into predefining layers using the Layer function will be discarded.
Drawing View Dimensioning Styles Also in the last article I said that the Layout dimension style could be different from the Model style in a Mechanical Desktop drawing. Use the Dimensioning dialog box to set this up (see Figure 3).
The significant item here is in the upper-left corner. Simply select a suitable style from the Base Dimension Style drop-down list, then check the Force Usage of Predefined Dimension Styles box. Now, whenever you create 2D views, the software automatically switches to the selected dimension style. Helpful Hints for Creating Annotation Standards As you're using the annotation standards in any release of Mechanical Desktop software, keep in mind that:
You should set the 2D layout dimension style for circle and arc centerlines to none so the Standards can generate parametric ones. Once you have a drawing set up the way you want it, save it as a template then use that template to start all new drawings. All Mechanical Desktop option settings are stored in the drawing. Annotation standards, like most rules, can be broken when the occasion calls for it. Fortunately, there is a "panic button" if your changes get out of hand. In Release 4, each dialog box that can change standards options also includes a Default button; look in the lower left corner. For Release 5, take a look at the right-hand window of Figure 1. Simply right-click on the name of the standard or of any subsection within the standard, then click Default. All the original specifications will be restored.
Conclusion Now that you know how to set up annotation standards, layers for part modelling, and other options for when you're in drawing mode, there's nothing holding you back. Dig in.