Customizing a Drawing View

The Generative View Style (GVS) gives you access to dress-up capabilities in the Drafting workbench when working on Electrical Harness Flattening documents. It allows the user to store the customizing options of drawing (Single / Double Line, 2D Detail, 3D Projection, etc.).

2D details showing pre-defined Support Section Views are automatically generated as defined in GVS.

To customize a Drawing View, you can use General Parameters but it is highly recommended to use the Generative View Style. Make sure the Drafting > View options are set as described in View, in the Settings Customization Guide.

1. When the Generative View Style is not activated (Tools > Options > Drafting > Administration), select the following options in the Drawing tab of the General Parameters dialog box:

   
   

   • Double line: For segment and For protective covering representation.

   • 2D detail option for For device graphical representation (splice and support).

   The aim of these settings, stored in the Flattening Parameters, is to customize the Drawing.

2. Open the Tools > Options... menu, then the Mechanical Design > Drafting > View tab. In the Geometry generation / Dress-up frame, select the following options:

   
   

   • Project 3D wireframe

   • Project 3D points

3. Click OK to validate.

   Note that the Generative View Style only works on Electrical Harness Flattening data, that is to say after extraction from the 3D data.

   GVS allows to generate the drawing with:
   

   • 2D Detail for Ends of Protective Coverings

     The same 2D detail is used for both ends of the protective covering. This is why, when defining the detail, the administrator must respect detail symmetry about the x-axis.

     
     
     

     The center of the detail is placed on the end point of the protective covering and the OX axis of the detail follows the tangency of the curve at the previous point.

     When generating the drawing, 2D details are sized according the layer of protective covering to which they are applied.

     You can take the 2D detail into account, the user must set the attribute, External reference, to the name of the catalog detail.

     By default, if the External reference value is set on a protection reference, then instantiating a protection feature from this protection reference should set the same value on the External reference of the instantiated protection feature.

     You can also do as follows:
     

     1. Right-click the instantiated protective covering and select Properties from the contextual menu.
     2. Click More... in the Properties dialog box that opens.
     3. Select the Electrical tab and enter the name of the 2D detail in the drawing catalog in the External Reference field.
     4. Click OK when done.

     Important: In V6 the External reference parameter is not available on the support. Thus the user has to make sure that the support name and the 2D Detail / Support Section name is same.

     To better visualize the various overlapping layers of protective covering on your drawings, you can use different Line Types and 2D Details. For more information, please refer to Distinguishing Overlapping Protective Coverings. For more information, see About Customizing a Drawing View.

   • 2D Details for Support Section Views

     By default, one 2D detail per support section will be generated. Details are positioned on the drawing on a grid. Details of support sections are oriented according to the orientation of the support in the 3D view.

     Supports are identified by a letter and corresponding details are identified using the same identifier plus a prefix, if desired.
     
     

     2D Details for Support Section Views

     In this example, the arrow on the right side is a 2D Detail is superposed on the 3D projection of the support.

     The symbols used will either be:
     

     • images from the catalog if you filed the External_Reference field in your protective covering properties with a Knowledge parameter
     • or a symbol named after the support part number

     The Automatic Generation leads to the creation of:
     

     • a balloon with a letter

     • Section View with a 2D Detail

     For more information, see About Customizing a Drawing View.

     In this example, the arrow on the right side is a 2D Detail is superposed on the 3D projection of the support.

     The Automatic Generation leads to the creation of:
     

     • a balloon with a letter

     • Section View with a 2D Detail

     For more information, see About Customizing a Drawing View.

   • 2D Clocking View

     A 2D Clocking View displays the relative position between a Backshell and a SIC (the SIC being connected to this Backshell). The orientation of the Backshell with respect to the SIC is taken into account in the drawing generation / update. Thus, the drawing contains three 2D Details: Backshell, SIC and Datum.

     To generate 2D Clocking View in the drawing, you need to:
     

     1. Open a flatten geometry.
     2. Set the GVS parameters: activate the GVS and complete the 2D Clocking View options under the Device node.
     3. Generate a Front View.
     4. Run the Automatic Generation and Update Dress-Up to respectively generate and update the drawing according to the GVS.

     Here is an example:

     3D flatten geometry data	Drawing view
     	Note: Annotations have been added on this image to help you distinguish the different elements in the drawing.
     Rotation of the SIC	2D Clocking View is updated

     To measure the relative angle between the Backshell and the SIC, the system uses the local axis of the 3D Part. The angle value will be correct only if constraints (defined at the Backshell Connection Point) are up to date.

     2D Details of the Backshell and the SIC should exist in catalog with a part number following this naming rule: SIC / Backshell + _Clocking, in geometry data. 2D Detail for Datum should also be present in catalog, with the same name as mentioned in the GVS.

     2D Detail representing Clocking View is created in the direction of the segment connected to the Backshell. Datum and Backshell 2D Details are the reference (no rotation is applied to them) and the SIC 2D Detail is rotated according to the relative angle applied in geometry data.

     Note: The orientation between the Backshell and the SIC can be computed even if the orientation constraint is not defined at the Backshell Connection Point. The angle computation is based on the transformation between local axis system of the Backshell and the 3D part (SIC).

     Warning: If you create a circle and a rectangle as 2D Details for the Backshell and the SIC respectively, as shown in the image below, then it will not be possible to appreciate the orientation between the two 2D Details. The generation / update of the Backshell / SIC orientation will be correct only if constraints of the Backshell Connection Point are up to date in the 3D Design geometry. If one of the overlapping 2D details (i.e. of datum, Backshell or SIC) is moved, then the other 2D Details will not follow it because the 2D Clocking View does not create 2D Details by grouping. Each 2D Detail is a separate entity that can be dragged within the drawing. After moving a 2D Detail, if you use the Update Dress-Up command, the 2D Detail remains in the last position chosen by the user. If the 2D Details of Clocking View are moved under / beyond the offset value as defined in GVS and if one of the 2D Details is deleted, then when you use the Update Dress-Up command, the deleted 2D Detail will be created at the offset value mentioned in GVS. And the existing 2D Details and datum will remain at their original location.

4. Open the Tools > Standards... menu. The Standard Definition dialog box opens.

   1. Select generativeparameters in the Category list.
   2. Select GVS_sample_1.xml in the File list.

      The electrical components are displayed with their representation.

      For example, the graphic representation is:
      

      • Single line for segments

      • Double line for protective coverings

      • 2D detail from the previously defined catalog for single insert connectors

5. In the Standard Definition dialog box, now select the DefaultGenerativeStyle.xml in the File list. The electrical components are displayed with their representation.

   If you select this generative view style to generate a Front View drawing , the drawing looks like this:
   
   

You can create your own line type standard for protective coverings that gives a different aspect to these components in your drawing and lets you better visualize the various overlapping coverings. This functionality is only available when generating drawings using Generative View Style parameters.

For each basic line type, you must define more than one bi-dimensional line type, increasing its size as you go in order to obtain one line type per layer of protective covering.

When generating your drawing, the system maps the appropriate line type to each layer of protective covering using a simple formula.

The above illustration also shows 2D details applied to the ends of protective coverings that likewise vary in size according to the covering layer. For more information, see Integrating Generative View Style.

Before you begin:

• you must run a CATIA session in administrator mode (see CATIA Installation and Administration User's Guide).
• Have specified the location of customized standards by setting the CATCollectionStandard variable. To learn more about the CATCollectionStandard variable, see About Standards.

1. Select the Tools > Standards... menu item.

   The Standard Definition dialog box pops up.

2. In the Category list box, select drafting. And in the File list box, select ANSI.xml.

   
   
   The Save As New command is now available.

3. Select LineTypes in the left-hand list:

   
   
   

4. Click Save As New and save the document with another name in the folder you specified by the CATCollectionStandard variable.

   This way you can customize more than one line type standard, that for example, will allow you to produce drawings having different line types for different customers.

5. Then double-click a line in the list and modify its aspect. Define more than one bi-dimensional line type per basic line type you want to create, increasing its size as you go so that you will obtain one linetype per layer of protective covering.

   Your document is updated.

   When creating protective coverings, line types offered in the Line type list are taken from the Tools > Options > General > Display > Linetype tab.

   To map line types in the standard you have just created to those in the Tools > Options dialog box, you must update the list in the Linetype tab.

6. To update line types in the Linetype tab, select the Tools > Options menu item. The Options dialog box displays:

7. Select the General > Display > Linetype tab.

8. Double-click one of the line types you created in the steps above. The Linetype editor dialog box opens.

9. Select the corresponding line type number previously created and click OK to validate. The list in the Options dialog box is updated.

10. Repeat for other line types.

11. Click OK to validate the changes in the Options dialog box. You can now use this line type standard for your drawings.

    For more information, see:

    Interactive Drafting User's Guide - User's Tasks - Administration Tasks - Administering Standards and Generative View Styles

    Interactive Drafting User's Guide - User's Tasks - Administration Tasks - Setting Standard Parameters and Styles - Setting Standard Parameters - Linetype Definition.

You can declare Business Rules and electrical catalogs in the Project Resource Management (PRM) in order to build your product definition and context. Please refer to Wire Harness Flattening Resources in Project Resource Management