CATIA V5 Admin Mode, Part 2: Customizing Drafting Standards

In my previous post CATIA V5 Admin Mode, Part 1: Setting Up  I explained how to set up CATIA to run in admin mode. In this post, I will explain how to use the admin mode to customize drafting standards.

IMPORTANT: Please make sure you read my previous post first, otherwise a lot of the info below may not make sense. CLICK HERE for Part 1.

There are two categories of drawing standards in CATIA:

• Drafting Standards: These define all the attributes for the default drafting elements used in CATDrawings, such as dimensions, texts, annotations, etc. For example – Which units should be used for the dimensions? How the tolerances should be displayed? What kind of arrows should be used in the dimension lines? How are threaded holes displayed? Etc.
  • Upon installation, CATIA provides several default drafting standards, such as ISO, ANSI, ASME, and JIS.
• Generative View Styles: These define how the drawing views are generated from 3D. I.e. – What should be the line type and thickness for the cross-section views? How should the fillets be represented? Etc.

Drawing standards in CATIA are stored in plain XML files. While an XML file can be opened and modified with any freely available XML editor, or even with a text editor such as Notepad, I do not recommend doing so, because tag names in the standard’s XML file do not necessarily match the drafting attribute names described in the CATIA’s documentation. Instead, you should use CATIA’s native Standard Definition editor, which requires running CATIA in admin mode.

In this post, we will discuss customization of the Drafting Standards, while in my next post I will explain how to work with the Generative View Styles.

Before you start customizing drafting standards, you need to set an environment variable, as well as create a directory to store the customized standards.

Open the global environment file in Notepad, locate the line that contains the CATCollectionStandard variable, and edit it so now it points to the directory that will contain all the customized standards, such as in the example shown below.

Create the actual directory on your hard drive, with the path as defined in the CATCollectionStandard variable. In that directory, create two sub-directories, named as following:

• drafting: This one will store all customized Drafting Standard files
• generativeparameters: This one will store all customized Generative View Styles

The sample directory structure is shown below.

Now start CATIA in admin mode and select Tools > Standards to open the Standard Definition dialog box.

Select drafting in the Category pull-down list. The File pull-down list now shows the default drafting standards provided with CATIA.

The recommended practice is to use one of the existing standards for the customization. Select an existing standard in the list (for example, ANSI.xml) and click Save As New.

Select a name for the new standard (for example, MyANSI) and click Save. The new file is saved into the drafting sub-directory.

The new standard will now display in the File pull-down list in the Standard Definition dialog box, and you can start editing it.

There are hundreds of drafting attributes that let you customize the drafting standard in a myriad of ways. You can find the full description of all the attributes, along with their valid values, in the CATIA’s Help Documentation, in the Interactive Drafting > Administration Tasks > Setting Standard Parameters and Styles section. A sample page, describing attributes for the Dimensions and Annotations is shown below.

As just an example, in this blog post I will show you how to modify the standard to have a new linear dimension style that displays the value in both millimeters and inches, like shown below.

Select Length/Distance Dimension heading in the Styles section of the standard and click Create Style.

Select a name for the new dimension style (for example, DualValue) and click OK. A new dimension style is created, as a duplicate copy of the Default style.

Expand the Styles > Length/Distance Dimension > DualValue section in the standard. Select the Dual Value Display attribute and set the value to Fractional.

Set the Value Display Format > Dual Value > Name attribute to in.

Set the Value Display Format > Dual Value > Precision attribute to 0.001. This attribute will control number of decimal places in the value in inches.

Set the Associated Texts > Dual Value > Before attribute to ( and Associated Texts > Dual Value > After to ). This will add the opening and closing parentheses to the dimension value in inches.

Click OK to close the Standard Definition dialog box and save the standard.

Now start a new drawing using the MyANSI standard and create a drawing view.

Select  (Length/Distance Dimension) and select the new DualValue style in the pull-down list in the Style toolbar, usually located at the top left corner of CATIA’s window.

Create a length or distance dimension. Note that the dimension displays values both in millimeters and inches, as was specified in the modified drafting standard.

Stay tuned. In my next post, I will be explaining how to use CATIA’s admin mode to customize generative view styles.

About the Author

Senior Technical Training Engineer<br><br>As a senior member of the Rand 3D team with a doctorate degree in Finite Element Analysis (FEA) and over 35 years of experience, Iouri provides design, consulting, and training services to those in the aerospace, automotive, electronics, and consumer goods industries. Iouri is a seasoned pro in 3D parametric design and prototyping using knowledge-based engineering methods, and has worked on a wide range of projects including BOM automation, CMM points generation, automated 3D annotation creation, and die tooling automation design. He is also a sought-after instructor and holds the designations of both CATIA Certified Professional (Expert level) and CATIA Certified Instructor.

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