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NX 11 Drafting - Secondary Geometry Representations

Phenom
Phenom

Use Secondary Geometry representations to visually distinguish secondary objects from primary objects in accordance with commonly accepted industry standards.

 

Create Secondary Geometry representations to illustrate selected components in an assembly drawing as:

1) Primary Geometry - The objects of focus

2) Secondary Geometry - The background or reference objectsNX 11: 'Secondary Geometry' shown by the dotted lineNX 11: 'Secondary Geometry' shown by the dotted lineWith a drill, for example, the plastic casing is secondary–you still want to see it and know that it's there, but the moving parts are truly what you are concered with. Thus, the mechanical components are primary. 

 

Toggle on the 'Secondary Geomtery' option in the drafting preferences.

If views are created prior to this preference setting, then you cannot specify the SG's in those particular views.

 

NX 11: 'Secondary Geometry'  location in the 'Drafting Preferences' dialogNX 11: 'Secondary Geometry' location in the 'Drafting Preferences' dialog

 

Specifying Secondary Geometry

You can specify the secondary geometry by following three ways.

 

I) Globally assign an object as secondary geometry

In the Drafting application itself, you can toggle on the 'Secondary Geomtery' option under the component properties from assembly navigator. 

 

NX 11: 'Secondary Geometry' location in the component properties dialogNX 11: 'Secondary Geometry' location in the component properties dialog

II) Specify the secondary geometry in Base View dialog

While creating the base view, you can specify the components as primary/secondary geometry components.

 

NX 11: Selection of 'Secondary Geometry' in the 'Base View' dialogNX 11: Selection of 'Secondary Geometry' in the 'Base View' dialog

III) By 'Seconday Geometry in View' command

Menu > Edit > View > Secondary Geometry in View

 

With this command, you can redefine or update the SG specification in the selected views. You can select the view in which it is needed to specify the SG.

 

For any projected view created from a view in which SG is already specified, then projected views will also show the SG representation.

 

NX 11: 'Secondary Geometry in View' dialogNX 11: 'Secondary Geometry in View' dialog

Secondary Geometry column in the Assembly Navigator

You can add the 'Secondary Geometry' column to the Assembly Navigator to identify the SG status of a component in the assembly.

(SG icons can be seen in the SG column within the drafting application only. If the application is switched from drafting to any other then SG column will not show the respective SG icons.)

 

NX 11: SG icon representation in the ASN (Drafting application)NX 11: SG icon representation in the ASN (Drafting application)

 

The symbols that appear in this column indicate the secondary geometry status of a component.

 

Secondary Geometry - The component is globally marked in the drawing part as secondary geometry.

 

View Specific - The component's global secondary geometry status has been overridden in one or more views. 

 

Points to Note: 

  • There is separate color, font, and width settings for primary and secondary geometry in the view that helps to differentiate visually. These settings can be applied to all exact and smart lightweight views. 
  • Primary and secondary geometry renderings are associative to model edits and they dynamically update to display the correct color, font, and width settings if the model geometry is changed or rearranged in the view. 
  • Secondary Geometry representations cannot be applied to pre-NX8.5 exact or legacy lightweight views. Nor should they be confused with Secondary Content in drawing booklets as they are not the same and should not be used together in a booklet.

 

Refer to the link "Secondary Geometry-FAQ" for more information.

Ganesh Kadole, QA Analyst (PLM), SQS
Testing: NX 10 | NX 11 | Teamcenter-NX Integration
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