Using Tools      

This task gives detailed information on tools helpful for creating any interactive element. Using multi-selection can also be very useful.

Tools Toolbar

The Tools toolbar displays a number of options. This toolbar is situated at the bottom right of screen. If you cannot see it properly, just undock it.
  The Tools toolbar provides the following options:

Snap to Point

When activated, this option makes your geometry (as well as 2D components) begin or end on the points of the grid. As you create geometry, points are forced to the intersection points of the grid. Note that this option is also available via Tools  > Options> Mechanical Design> Drafting> General tab (Snap to point check box).
 

 

In this example, the black spline was created with the Snap to Point option activated. The points are on the grid.

Conversely, the highlighted spline was created with the option deactivated. The points are not necessarily on the grid.

 

You can use auto-detection even if this option is activated
 

From V5 R15 onwards, the Snap to Point option no longer applies to annotations.
Now, only the Snap by default (Shift toggles) setting in Tools > Options is used to specify whether snapping should be activated by default for annotations. For more information, refer to Annotation and Dress-up in the Customizing Settings chapter.
 

Create Associative Dress-up

 
This command is active provided you installed a Generative Drafting license.
  When activated, this option lets you create persistent graphical dress-up.

To restore 3D graphical dress-up in a view, right-click on the view frame to open the contextual menu then select View object > Restore Properties. For more information, read the Restoring Overloaded Properties/Deleted Elements user task in the Generative Drafting User Guide.

By default, the Create Associative Dress-up icon is activated.

Visualization Toolbar

The Visualization toolbar displays a number of options. This toolbar is situated at the bottom right of screen. If you cannot see it properly, just undock it.
  The Visualization toolbar provides the following options:
  • Sketcher Grid
  • Show Constraints (See chapter on Constraints)
  • Display View Frame as Specified for Each View
  • Filter Generated Elements
  • Analysis Display Mode

Sketcher Grid
Activate this option to display the grid in your session. The grid will help you draw geometry in given circumstances. For example, the grid will make it easier to draw profiles requiring parallel lines. Note that this option is also available via Tools > Options> Mechanical Design> Drafting> General tab (Display check box).
 

Display View Frame as Specified for Each View

When activated, this option lets you display the view frame which is available for each view, as specified in each view's properties (Edit > Properties, View tab, Display View Frame check box). In this case:

  • the view frame will be displayed for all views for which the Display View Frame check box is selected.

  • the view frame will be hidden for all views for which the Display View Frame check box is cleared.

Deactivating this option hides the view frame for all views.
 

Filter Generated Elements

This option lets you differentiate 2D elements (Interactive Drafting workbench) from the geometrical elements generated from the 3D (Generative Drafting workbench) within the same view. This can prove very helpful when you need to add purely interactive elements onto generated views.

Open the GenDrafting_part.CATDrawing document.

This command is active provided you installed a Generative Drafting license.

  1. Click Filter Generated Elements . The generated geometrical elements appear in gray (all other elements including generated dress-up elements remain black).

  2. Create 2D elements in the front view. For instance, create a diameter dimension and a datum feature.
    The 2D elements appear in black.
 

Analysis Display Mode

This option lets you visualize the colors assigned to the different types of dimensions. 

These displayed colors correspond to the colors customized in the Options dialog box. To modify these colors, go to Tools> Options> Mechanical Design> Drafting (Dimension tab). Then select the Activate analysis display mode check box and, if needed, click the Types and colors switch button to assign the desired color(s) to the desired dimension types.
   
 

Tools Palette

The Tools Palette appears whenever you select a command for which specific options or value fields are available. This enables you to know immediately when tools are available for a command.

 
The options or fields available in the Tools Palette depend on the command you selected. Only a few examples are provided here.
 

Example when creating dimensions

For example, if you select the Dimensions command, the Tools Palette may provide the following options:
 

Projected/Forced/True Length Dimension

Projected Dimension (according to the cursor position) 

Force Dimension on Element

Force Horizontal Dimension in View

Force Vertical Dimension in View

   Force Dimension along a direction

True Length Dimensions (for isometric views only)
Remember that as you create the dimension in one mode, you can use the contextual menu and select another mode.
 

Example when creating geometry

Another example would be when creating a line. The values of the elements you are sketching appear in the Tools Palette as you move the cursor. In other words, as you are moving the cursor, the Length (L) and Angle (A) fields display the coordinates corresponding to the cursor position.

 
The Horizontal (H) and Vertical (V) fields are optionally displayed, depending on whether the Show H and V fields in the Tools Palette option is selected in Tools > Options > Mechanical Design > Drafting > Geometry tab.

You can also use these fields for entering the values of your choice. In the following scenario, you are going to sketch a line by entering values in the appropriate fields.

  1. Click the Line icon from the Geometry Creation toolbar.

    The Tools Palette displays information on value fields.

  2. Enter the length (L) of the line and press enter.

  3. Enter the value of the angle (A) between the line to be created and the horizontal axis and press enter. The line is created.

Make the Most of Multi-selection
When you need to create and/or modify an element, you can either select the element or the command first. Multi-selection can only be used for given commands. You are therefore allowed to select element(s) before these given commands.
Open the Brackets_views06.CATDrawing document.

  1. Multi-select 2D elements. For example, four circles.

  2. Click the desired command, Threads for example.

    Four threads are automatically applied to the selected circles.