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Part Section Views

Tools Tooltab > Section Views (Part Level)

ZW3D supports a Section View Display Mode.  This means that you can work on a part while previously defined cutting planes are active.  The part is not physically altered in any way.  Only the display of the part is affected.  This is very convenient when you need to work on areas of a part that are not readily visible in Wireframe Display Mode or Hidden Line Display Mode.  This command does not work on open shapes, only closed solids.

Required Inputs

Select the type of section to display.

Display a section at a single plane.

 

 

Display a slice section at two planes.

 

 

Display a section with an envelope encompassing 6 individual section planes.

 

 

Display a section with a profile.

 

Optional Inputs

• Align plane
  Use this option to define the alignment of the section planes.  By default, the section planes are aligned with the default XY plane.  You can select any datum plane or planar face.  The section planes will align with the selected plane.
  
  
• Plane activation
  Use this option to toggle the display of each section plane.  There is always an active section plane.  By selecting an icon (i.e., it is depressed), that plane is activated.

 Activate top plane.
 Activate front plane.
 Activate right plane.
 Activate left plane.
 Activate back plane.
 Activate bottom plane.

• Offset
  For Section at plane and Section with slice (see Required Inputs above), use this option to offset the section plane relative to the alignment plane.
  
  
• Thickness
  For Section with slice use this option to define the slice thickness.
  
  
• Top, Front, Right, Left, Back, Bottom
  For Section with envelope, use these options to locate each plane of the envelope.
  
  
• Reset planes
  Use this option to reset all planes to their default locations and values.
  
  
• Profile
  Select a closed profile to create a section. You can select face, wireframe geometry, face edges or a sketch. Extrude the selected profile to cut the overlapped portion of the base part or assembly. This section mode is similar to the Extrude command with the remove boolean operation.
  
  
• Type
  Specify the extrude type from the following.
  

  1 side
  The start position is decided by the selected Profile, and to specify the End position to determine the extrude length.
  
  2 sides
  Specify the Start and End positions to determine the extrude length.
  
  Symmetrical
  This type is similar to the "1 Side", but it will extrude the same length along the opposite direction decided by the End position.
  

• Start, End
  Specify the start and end of the extruded profile. You can enter the exact values, drag the preview echo on the screen or right-click for additional input options.
  
  
• Sectioned shape
  Use this option to decide how to display the portion of the part that is sectioned away.  Select from the following.

 Make the sectioned shape invisible.
 Display the sectioned shape as Wireframe geometry.
 At the ZW3D CAM Level, use this option to only section the tool paths.  Using this option, you can look at the different levels of cuts.  In conjunction with the Thickness option, you can look at just one level of cuts at a time and still see the solid.

• Interference
  This is the color of the area of intersecting between shape/components.
  
  
• Hatch color
  Show section color with Body color or Specify color.
  
  
• Hatch style
  Use this option to define the type of cap overlay to display on the part section plane.  Select one of the following.

 Do not display a cap overlay.
 Display a hatch pattern for the cap overlay.
 Display a grid pattern for the cap overlay.

• Spacing
  If a Cap overlay is selected (see above), use this option to define the pattern spacing.
  
  
• Opaque
  Use the slider to change the transparency of the section plane (on the part).  Left is less transparent and right is more.  Al the way to the right will result in a solid section plane.
  
  
• Display section planes
  Place a check in this box if you want the section planes displayed.  Remove the check to hide them.
  
  
• Display hatch for non-closed shapes
  This option is only valid for non-closed shapes. Check this box to display hatch for non-closed shapes.
  
  
• Insert datum
  Use this option to place a datum plane on and at the center of the active section plane.
  
  
• Insert curves
  Use this option to create section curves and place them on the active section plane.
  
  
• Insert view
  Use this option to create a saved view from the current section view.  This is the same as selecting the New option from the View Manager.  You can store the current layer visibility and current section plane along with the saved view.  All parameters of this command are stored with the view. If you save multiple section views, they can all have different slices, offsets, inference colors, cross hatching, hatch spacing, etc.

Optional Inputs (Insert View Option)

• Store current layer visibility
  Use this option to save the current layer visibility with the stored view. An attempt will be made to set the layer visibility according to the stored settings when the view is activated. Views can be stored, activated, renamed, deleted or inquired. Stored views can be inserted as standard layout views at the Drawing Sheet Level.
  
   
• Store current section planes
  Use this option to store the current section planes (if any are defined) with the stored view.  To Activate the view from the View Manager and display the section you must be in the Section Display Mode.
  
  

1. Load a component assembly.
2. Use the Drag Component command to drag a component through its range of motion to a location where you want to check for an intersection.
3. Execute this command and set the Color of intersection from the Optional Input section of the Input Manager.
4. Click on one of the displayed section planes and drag it through the assembly. If an intersection among two or more components is found, it will be displayed in the intersection color you specified. 
   
   Refer to the example shown below.
   
   
   
   

   Step 1: Load Assembly	Step 2: Drag Component
   Step 3: Preview Intersection