CATIA V5 Admin Mode, Part 3: Customizing Generative View Styles

July 22, 2021 Iouri Apanovitch

In my previous posts: CATIA V5 Admin Mode, Part 1: Setting Up  and CATIA V5 Admin Mode, Part 2: Customizing Drafting Standards I explained how to set up CATIA to run in admin mode, as well as how to use the admin mode to customize drafting standards.

In this post, we will discuss customization of the Generative View Styles.

Generative View Styles in CATIA define how the drawing views are generated from your 3D model. I.e. – How should the fillets be represented? Should center lines and axes be displayed? What should be the line type and thickness for the section profile? Etc.

There are workbench-specific view style parameters (i.e., HVAC Design, Tubing, Sheet Metal, Composites, etc.) and general drafting parameters. The general drafting parameters fall into the following two categories:

  • Generate parameters: These specify which 3D entities should be shown in the view. For example – should the wireframe elements be projected? Or – should the plies of the composite part be shown?
  • ViewDressup parameters: These define the style of the dress-up details. For example – what should be the line type and thickness for the section views? Or – which color should be used for the fillets?

You can find the full description of all the parameters in the CATIA’s Help Documentation, in the Generative Drafting > Administration Tasks > Setting Generative View Style Parameters section.

Before you start customizing generative view styles, make sure you have set the CATCollectionStandard environment variable, as well as have created a directory to store the customized styles, as explained in my blog post CATIA V5 Admin Mode, Part 2: Customizing Drafting Standards.

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

Select generativeparameters in the Category pull-down list. The recommended practice is to use one of the existing styles for the customization, therefore, select DefaultGenerativeStyle.xml in the File pull-down list and click Save As New.

Select a name for the new style (for example, MyGenerativeStyle) and click Save. The new file is saved into the generativeparameters sub-directory.

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

As an example, in this blog post we will modify the view style to have the center lines of the holes shown, as well as the fillets shown in symbolic representation.

Expand the Drafting > Generate section in MyGenerativeStyle.xml. Select the CenterLines parameter and set its value to Yes.

Select the Fillets parameter and set its value to Symbolic.

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

The next step is to enable the use of generative view styles. Go to Tools > Options > Mechanical Design > Drafting > Administration, and toggle off the Prevent generative view style usage option.

Now start a new drawing and select  (Front View) to create a view. In the Generative view style pull-down list that pops up on the screen, select MyGenerativeStyle.

Proceed to create the view the usual way. Note that the new view displays center lines for the holes as well as shows the fillets symbolically, as specified in the modified generative view style.

 

This completes my series of posts about using CATIA’s admin mode to customize drawing standards and styles. The general use of the Drafting workbench for design documentation and detailing is covered in the Rand 3D training course CATIA: Generative Drafting.

About the Author

Iouri Apanovitch

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.

Follow on Linkedin Visit Website More Content by Iouri Apanovitch
Previous Article
CATIA V5 Admin Mode, Part 2:  Customizing Drafting Standards
CATIA V5 Admin Mode, Part 2: Customizing Drafting Standards

Next Article
CATIA Assembly Design: Flexible vs. Rigid Sub-Assembly
CATIA Assembly Design: Flexible vs. Rigid Sub-Assembly

Learn about Flexible vs. Rigid Sub-Assembly in this CATIA Assembly Design software tip.

×

Sign up for email updates

First Name
Last Name
Country
Thank you!
Error - something went wrong!