View Attributes

These attributes define how the various entities are displayed in views. The defaults for these attributes are defined in the View Attributes Preferences.

View Attributes dialog

The View Attributes dialog is displayed (additional information is displayed in the dialog when a view of an assembly is created (see the Assembly View - View Attributes dialog below).

1. In the View Attributes dialog, set the visibility attributes of the entities by selecting or deselecting the appropriate checkboxes.

The view attributes of the following entity categories can be defined: Model visible (always selected) Model hidden Model sectionedModel sectioned(an edge created using the Boolean operation of the section view function). Tangent visible/hiddenTangent visible/hidden(a tangent edge whose normals of the faces it separates are parallel for all positions along the edge). Model Wireframe Thread visible/hidden Exploded Ejectors Cylinder Axis visible/hidden, including Extension. ShadingShading(Shading can be applied to any part or assembly part, and can be adjusted with color and transparency controls. Entire views or selected components can be viewed as shaded. The shaded attribute works in tandem with other attributes such as hidden lines. Views derived from a shaded view will keep the same attributes as the shaded view). Prefer Color from Vertical faces Always Show Manufacturing Technique Attributes Reset line attributes See also: Assembly view - view attributes Editing view attributes

2. Click OK to apply the selected attributes.

 

Attribute types

For most entities, the following attributes can be assigned. The Preview column shows how the resulting entity will be displayed.

• Special (see Special visibility attributes below)

• Pen

• Style

• Color
   

For Shading, the following attributes are available:

• Special

• Transparency level (Wireframe, Transparent, Shade, or Render Mode)

• Color

Each of these entities has one or more of the following Special visibility attributes that can be set from the adjacent drop-down list.

Special visibility attributes

None	When this option is selected, the Pen, Style and Color attributes become available for that entity. These attributes can also be changed individually for each sheet and view in the menu bar. A Preview column displays a preview of the attribute as it will be displayed with the current settings. When this option is selected for the Shading attribute, the transparency level (Wireframe, Transparent, Shade, and Render Mode) and also the color attribute options are still available. When editing the attribute of an entire view, all faces will be colored in the selected color. ExampleExample
As Hidden	Use the attributes from the hidden edges definition.
As Visible	Use the attributes from the visible edges definition.
Grey Scale	Shade the model in grey scale. This visibility attribute appears for the Shading entity.
As Model Color	Create views with the color of the model. With this option, the Color drop-down list for the row is disabled. When this option is selected for the Shading attribute, each face gets the color it has in the model and the Color attribute option is disabled. The transparency level (Wireframe, Transparent, Shade, and Render Mode) attribute option is still available. ExampleExample
As Model Attributes	Create views with the attributes of the model.
Prefer Color from Vertical faces	When a hole is perpendicular to the drawing plane, it is drawn as a circle. The color applied to the circle may be: The color of the surface that the hole penetrates. The wall face color. This setting provides control of the hole edge color in the drawing. When selected, the color seen in the view will be based on the hole’s cylinder. When deselected, the color of the face with the hole will be used. Note: The option will only be available when model visible or model hidden is set as model color, or if Always show manufacturing technique color is selected.
Always Show Manufacturing Technique Attributes	Enabled by default to display the attributes of a model with attached Manufacturing Technique attributes. If you deselect this checkbox you must also Reset line attributes. Editing this setting may also Reset Manufacturing Attributes. When this value is edited (selected or deselected), Reset Manufacturing Attributes option is enabled.  Settings Change made to Always Show Manufacturing Technique Attributes value Reset Manufacturing Attributes status Behavior selected OR deselected Reset Manufacturing Attributes is selected Reset Manufacturing Attributes is selected deselected selected Manufacturing Attributes will not be seen deselected deselected No Action selected selected Manufacturing Attributes will be seen
Reset line attributes	This option removes all the view's existing attributes and recreates them according to what is selected in the View attributes dialog. (Removes all manually set changes.)

Assembly View – View Attributes

If a view of an assembly is created, the name section of the Assembly Tree is also displayed in the View Attributes dialog and additional options appear at the bottom of the dialog (highlighted in the example below). See Assembly View for an explanation of the additional options in this dialog.

Model Wireframe

The Model Wireframe view attribute (see the View Attributes dialog above) enables you to define the visibility of wireframe entities in Drafting. Display or hide wireframe entities, as required, using the checkbox in the dialog. 

Cylinder Axis

The Cylinder Axis view attribute (see the View Attributes dialog above) enables the display of center lines automatically for all holes and shafts in a simple and section view. The Extension parameter defines the amount the center line "extends" both sides beyond the cylinder.

The defaults below are applied to the Cylinder Axis attributes. These defaults are defined in Preferences (Tools > Preferences > Drafting > Drawing and Sheet > View Attributes).

Cylinder Axis visible: Checked Cylinder Axis hidden: Unchecked Extension: 5 mm or 0.25 inch Pen: 1 Style: symmetry line (grayed out – cannot be changed) Color: black If the Model hidden attribute is not checked, Cylinder Axis hidden is grayed out (not checked).

The Cylinder Axis attribute shows a symmetry line (with a defined extension) for every cylindrical and cone face in the model which is represented in the view by two lines. This symmetry line can be edited using the Symmetry Line function and dimensioned using the Symmetry Line Dimension dialog.

If a hole/shaft is not visible in the view, the related center line is also not visible.

The definition of a cylindrical/cone face (to show a center line) is every cylinder/cone face in the model that is at least 180 degrees (or more). In the examples below, all the yellow faces will not get a center line (the round faces are 90 degrees and the other yellow faces are less than 180 degrees). All the green faces will get a center line in the view.

A split face in the model is recognized as one face (the examples below are valid and will get a center line).

For clarity, a single center line is displayed in cases where multiple center lines with the same direction may completely or partially overlap each other. In the example below, there are several holes/shafts with different depths and radii, however, only a single center line is displayed.		The base length of the center line (without the extension) is according to the longest side (face boundary) of the cylinder.

Editing View Attributes

Once the view attributes of a specific view have been defined, the View Attributes item in the Drawing tree can be edited, cut, copied or deleted by right-clicking on it, or dragged within the Drawing Tree to another view in any sheet in the file (see the image below).

A warning message is displayed and when approved, the target view is immediately displayed with the newly-applied view attributes.

Some functionality may be dependent on the product package. Contact your Reseller if you require a license.