When points defining the section are selected, Quick Pick is activated and input constraints are stored with the section definition.

 

If you select the center point of circle as a section definition point and the referenced 3D part is modified, the section definition point is automatically regenerated at the new location.

 

By default, section views inherit the view attributes of the view they are derived from except in the case of the section view label.  It is always initially displayed due to drawing standard requirements.  You can turn off the label by selecting Attributes > Edit and setting the Layout View Attributes Form accordingly.

 

 

 

 

 

Use this command to redefine a section view created with the Insert Section View command above. Select the section arrows to redefine. The Options Form is displayed containing the required and optional inputs (see below) used to create the section. Modify the inputs as desired and then pick OK to redefine the section view.

 

 

 

• Type - Select the type of section to insert.
  
  Full - The view is fully sectioned in one direction (shown above).
  Aligned - The view is sectioned in two directions and then aligned.
  Revolved - The view is fully sectioned in one direction and then superimposed on top of the view (e.g., a section of a cylinder superimposed on top of its side view).
  3D Named - This type inserts a named section created in the part using the Named Section Feature command. Select this option and then select the feature from the 3D Name list of features (see below).  The Named Section Feature must be created with a sketch that consists of lines with zero or more bend points at 90 degrees.
  Bent -This type also inserts a named section created in the part using the Named Section Feature command. Select this option and then select the feature from the 3D Name list of features (see below).  The Named Section Feature must be created with a sketch that consists of lines with bend points at other than 90 degrees.

 

• Base View - Select a layout view to section.

• 3D Name - If 3D Named is selected for Type (see above) and sections exist for the part, enter the name of the section or pick the folder icon to select a section. Only sections that are parallel with the section direction are listed. The section geometry is evaluated for connectivity and the section echo is displayed.

• Base Point - Select the base point of the section. For example, if you are sectioning through a hole, the base point would be the center of the hole. For aligned sections, the base point would be where the two section planes meet.

• Base Dir - Select a point to define the base direction. This point along with the base point defines the primary cutting plane.

• Align Dir - If Aligned is selected as the Type (see above), select a point to define the align direction. This point along with the base point defines the aligned cutting plane.

• Location - Select a point on the drawing sheet to locate the section view.

 

 

 

• Method - Select the display method.
  
  Section Curves - Shows the cross section profile only.
  Trimmed Part - Shows a hidden line view of the entire part with the sectioned volume removed.
  Trimmed Surface - This method can use less than perfect geometry. It shows the section curves of trimmed surfaces (open or closed).  Use this method if the Trimmed Part method fails due to invalid or "suspect" geometry (e.g., imported geometry).

 

• View Label - Enter a view label (example: "A" becomes "Section A-A"). The next available system generated label is provided by default.

• Flip Arrow - Check this box to flip the section arrows (e.g., the cutting direction).

• Base Arrow - Use this option to position the base arrow. Select the button and then drag the base arrow to the desired location and select a point.

• Align Arrow - Use this option to position the align arrow (opposite the base arrow for all types). Select the button and then drag the align arrow to the desired location and select a point.

• Base Offset - Use this option to offset the arrows. Select the button and then drag the base arrow to the desired location and select two points to define the start and end of the offset. Middle-click to continue.

• Align Offset - Use this option to offset the section arrows during the Aligned section type. Select the button and then drag the arrows to the desired location and select two points to define the start and end of the offset. Middle-click to continue.

• Location- Use this option to select the method of determining where on the base view the section will be located.  Select from the following:
  
  Horizontal - The section view will be placed at a user defined point horizontal to the base view.
  Vertical - The section view will be placed at a user defined point vertical to the base view.
  Orthogonal - The section view will be placed at a user defined point orthogonal (perpendicular) to the section definition line.
  None - The section view will be placed at a user defined point.

 

 

 

 

 

• System generated labels start with the letter "A" and ignores the letters "I", "O" and "Q." After the letter "Z" is used, labeling switches to "AA", "BB", "CC", etc. If you accept a system generated label, the next available unused letter in the alphabet will be used.

• Use Caution when Deleting Layout Views (see CAD Tips & Techniques).

• Adding Dimensions to 3D Layout Views (see CAD Tips & Techniques).

• If "Do not section" is checked on the Part Attributes Form, the part will not be sectioned (or hatched) by these Section View commands.  Instead, it will be displayed projected onto the section view.