In this Article:

Insert Standard View

Insert > 3D View (Drawing Sheet Level)

Use this command to create a standard orthographic layout view from a 3D part. If the part has named views created using the View Manager, they can also be inserted as a standard view.

3D Part

Insert Standard View

Required Inputs

• File/Part
  The drop-down list contains the VX files currently opened by the active session. The active file is selected by default. You can select another file from the list or pick the folder icon to select another file using the File Browser. The list contains the parts in the selected file. Select a part to layout.
  
  
• Preview
  Setting the preview mode to Graphics or Attributes will display the selected part in the preview window or the part?s attributes in the Part Attributes Form. These options are similar to the Object Browser and the Root Object Browser.
  
  
• View
  Enter the name of the view or select a view from the drop-down list. If the selected part contains named views (created with the View Manager.), they will also listed for selection. Layer visibility is maintained if it is stored with the named view.
  
  
• Location
  Select the view location.

Options Tab

• General, Label, Line, Comp
  See View Attributes Form for a description of each attribute.
  
  
• File/Bundle
  See Attribute Bundles and Form Commonalities.
  
  
• Other Options
  See Command Options Forms for additional options not listed here.

Advanced Tab

• Origin
  Use this option to select from the list of alternate datums from the 3D part. The origin of the selected datum is used instead of the part?s world origin (0,0,0). For example, if you select an alternate datum attached to the part and then move the part in 3D, the view of the part will not move on the drawing. The Location point for the view corresponds to the origin of the alternate datum. You should also provide descriptive names for your datums to help define their position.
  
  
  
  Using the Insert Layout "Origin" option for distant parts.
  This option is very helpful when the part you want to layout is far away from the part?s world origin.  A good example would be if you want to layout the headlamp of a car.  The headlamp component may be located far away from the car?s world origin.  With this option, you can select an alternate datum that you attached to the headlamp.  Preferably one that properly orients the headlamp for detailing on the drawing sheet.
  
  
  
• Config
  This option allows you to specify an assembly configuration to use for the layout. Select a configuration from the list. Configurations have to exist in the assembly before this option is available.
  
  
• State
  Use this option to create a view based on a certain state in the history defined by a Backup Feature. Select from the list of Back Features.
  
  
• Calculate part center
  Use this option when the part you are attempting to layout is located far from 0,0,0.  Checking this box causes VX to calculate the center of the part based on its geometry and to use that center point to position any views of the part on the drawing.

Notes

1. Use Caution when Deleting Layout Views (see CAD Tips & Techniques).
   
   
2. Adding Dimensions to 3D Layout Views (see CAD Tips & Techniques).

1. Section Views (2D)
2. Insert View Layout
3. Associate/Disassociate 2D Entities with a View
4. Create Detail View
5. Insert Auxiliary View
6. Insert Projection View
7. Hide Component Entity