Drawing Styles and Standards30 Sep, 2003 By: Jeff Wymer
Autodesk Inventor's drawing environment is based on standards. The drafting standard you choose when you start a drawing will determine the behaviors and settings available during the drawing creation and documentation phases. But the companies or clients you work for probably have their own standards and requirements for drawings. This column will show you how to modify the standards to match your employers' or customers' criteria.
In Inventor, items such as color, line style, text height, and standard symbols can all be controlled within the drawing standards. Text attributes (such as color and font) are controlled by text styles, and dimension attributes by dimension styles. When starting a new drawing, you choose a drawing template to predefine the drafting standard to use. For instance, when ANSI is chosen, all drawing view projections will be third-angle projections and the symbols will meet the ANSI drafting standard. By the same token, if you choose DIN, the drawing view projections will be first-angle projections and the symbols will comply with the DIN drafting standard. But all of these attributes and elements can be modified.
To start, create a new drawing file and choose the default drafting standard. For this article, let's choose ANSI-MM from the Metric tab. To modify any of the drawing attributes, you need to access the drafting standards dialog, as shown in Figure 1, by choosing the Format pulldown menu and then Standards.
Figure 1. Access the drafting standards dialog located in the Format pulldown menu, to modify the attributes of a drawing file.
The Common tab allows control over line properties such as line type, color, and line weight for each type of line element. AutoCAD uses layers to determine these types of settings. Since Inventor uses objects, each object type or definition can have different color and line type properties, and these properties are defined within the drafting standards.
Users often inquire how they can change the default sheet color, since this cannot be defined as an application option or color setting; it is defined as a sheet standard. Within the drafting standards dialog, you can modify the default sheet color by choosing the Sheet tab. Here you can control the sheet color, outline, highlight, and selection color properties.
Figure 2. As with AutoCAD, dimension formatting in inventor can be controlled and defined using the Dimension Style dialog.
The Parts List tab allows you to predefine the parts list output based on your requirements. This can be defined within the template file for consistent parts list output. Items that can be predefined within the drawing template are the default text style to use, the direction of the parts list, and the settings for all rows and columns (including columns to display). By defining this within your template file, you will save time and have consistency among all parts lists created. Other items that may be controlled via standards are hatch patterns, balloons, center marks, surface finish, feature control frames for GD&T, and so on.
Out with the Old; In with the New
To create a new standard based on an existing one, scroll down the list of standards until you see "Click to add new standard." You will be prompted to supply the new standard's name and select the existing standard you want to use as a basis. You can now modify all attributes of this new standard. But remember: this standard is only being defined within this drawing file. If you want to use this standard for other drawing files, you will need to save this file as a drawing template within the template directory. By default the template directory will be under Program Files\Autodesk\Inventor (Version #)\Templates.
To control dimension formatting you will need to use the Dimension Style dialog, as shown in Figure 2. You can access this via the Format pulldown menu and the Dimension Styles option. You can define new dimension styles or modify the existing dimension styles Inventor uses by default. Within dimension styles you can define the dimension offset, text height, prefix. suffix, and so on. When creating a dimension, you can toggle or change the active dimension style by selecting the format pulldown menu within the default toolbar of Inventor, as shown in Figure 3. After the dimension is placed, if you want to change the dimension style, select the dimension and select the new dimension style from the style pulldown menu. This will automatically update all formatting of the dimension to the new style chosen.
If you need to modify an existing dimension, it's best to modify or change its active dimension style. Most Inventor users double-click the dimension to change the tolerance or units formatting. When doing this you are creating a dimension override of the dimension style. This method might not be the best if the file is going to be exported to an AutoCAD DWG file. When exported to a DWG file, there will be additional dimension styles created with many dimension overrides (to override the dimensions in Inventor). Therefore, if you are exporting your Inventor file to a DWG file, it's best to change its active dimension style.
Figure 3. You can toggle or change the active dimension style using the format pulldown menu within the default toolbar.
Autodesk Inventor provides a variety of predefined text styles for documenting designs. In the Text Styles dialog box (choose Format pulldown menu and Text Styles) you can define the properties of the text such as color, font, size, rotation, placement, and justification settings. Dimensions can have text settings separate from text styles; however, a dimension style can use text styles. You can also use text styles with dimension tolerances to define different styles (dimension text and tolerance text) within the same dimension style.
There may be times when you need to leverage or use text or dimension style information from another drawing document. The drawing organizer allows you to easily copy text and dimension styles defined within another drawing file to your current drawing document. To access the drawing organizer, go to the Format pulldown menu and choose Organizer. You can browse for the desired drawing file you want to copy from, and select which styles you want to copy. This will save you time and the hassle of creating this style information from scratch.
Autodesk Inventor's drawing manager uses drafting standards to control the formatting of objects such as weld symbols, geometric dimensioning, tolerancing, surface finish symbols, and so on. These standards can be easily defined or modified to meet your company standards through the Standards dialog. As with AutoCAD, all formatting of text and dimensions can easily be controlled with text styles and dimension styles in Inventor.