TechDraw SectionView

BrokenView

ComplexSection

TechDraw

Description

The TechDraw SectionView tool inserts a cross-section view based on an existing part view.

Sectioning an already placed view, which shows the internal holes and a hatched cut surface.
The top image shows the ANSI arrow format.
The bottom image shows the ISO arrow format.

Usage

1. Select a part view in the 3D view or Tree view.
2. There are several ways to invoke the tool:
   • Press the Insert Section View button.
   • Select the TechDraw → TechDraw Views → Insert Section View option from the menu.
3. A task panel opens which will help calculate the various properties. Reasonable values for the view Direction are calculated, but these can be changed.

Taskview to define the sectional cut of a view

Properties

See also: Property editor.

In the properties of the DataBase View you can change the appearance of the section line.

A Section View, formally a TechDraw::DrawViewSection object, is derived from a Part View, formally a TechDraw::DrawViewPart object, and inherits all its properties. It also has the following additional properties:

Data

Appearance

• DataSection Line Stretch (FloatConstraint): Adjusts the length of the section line. 1.0 is normal length, 1.1 would be 10% longer, 0.9 would be 10% shorter. introduced in version 1.0

Cut Operation

• DataFuse Before Cut (Bool): Fuse the source shapes before performing the section cut.
• DataTrim After Cut (Bool): Additionally trim the resulting shape after the section cut to remove any unwanted pieces. introduced in version 0.21
• DataUse Previous Cut (Bool) Use the cut shape from the base view instead of the original object. introduced in version 1.0

Cut Surface Format

• DataCut Surface Display (Enumeration): Appearance of the cut surface. Options:
  • Hide: Hides the cut surface, only the outline will be displayed.
  • Color: Colors the cut surface using the setting of Cut Surface Color in the TechDraw preferences.
  • SvgHatch: Hatches the section cut using a hatch
  • PatHatch: Hatches the section cut using a geometric hatch
• DataFile Hatch Pattern (File): Full path to SVG hatch pattern file.
• DataFile Geom Pattern (File): Full path to PAT pattern file.
• DataSvg Included (FileIncluded): Full path to the included SVG hatch pattern file.
• DataPat Included (FileIncluded): Full path to the included PAT pattern file.
• DataName Geom Pattern (String): Name of the PAT pattern to use.
• DataHatch Scale (Float): Hatch pattern size adjustment.
• DataHatch Rotation (Float): Rotation of hatch pattern in degrees counter-clockwise. introduced in version 0.21
• Data (Hidden)Hatch Offset (Vector): Hatch pattern offset. introduced in version 0.21

Section

• DataSection Symbol (String): The identifier for this section.
• DataBase View (Link): The view on which this section is based.
• DataSection Normal (Vector): A vector describing the direction normal to the cutting plane.
• DataSection Origin (Vector): A vector describing a point on the cutting plane. Typically the centroid of the original part.
• DataSection Direction (Enumeration): The direction in the Base View for this section. Options: Aligned, Right, Left, Up or Down.

View

Cut Surface

• ViewCut Surface Color (Color): Solid color for surface highlight. Used if DataCut Surface Display is set to Color.
• View (Hidden)Show Cut Surface (Bool): Show/hide the cut surface.

Surface Hatch

• ViewGeom Hatch Color (Color): The color of the Geometric hath pattern.
• ViewHatch Color (Color): The color of the Svg hatch pattern.
• View (Hidden)Hatch Cut Surface (Bool): Hatch the cut surface.
• ViewWeight Pattern (Float): Line weight of the Geometric hatch pattern.

Notes

• Section Line Format: two section line formats are supported (as depicted above) and controlled by the Preference setting "Section Line Standard" on the Annotation tab. The ANSI option uses "pulling arrows" (known as the "traditional format" in some areas) and the ISO option uses "pushing arrows" (also known as the "reference arrow format").
• Fuse Before Cut: the section operation sometimes fails to cut the source shapes. If Fuse Before Cut is true, the source shapes are merged into a single shape before the section operation is attempted. If you encounter problems with the section operation, try flipping this value.
• Trim After Cut: the section cut operation sometimes leaves behind a portion of the source shape. If Trim After Cut is true, an additional cut operation is performed on the result of the first cut which should remove any unwanted pieces.
• Cut Surface Display: the cut surface can be hidden, painted in a solid color, hatched using an Svg pattern (default) or hatched using a PAT pattern. See Hatching.

Scripting

See also: Autogenerated API documentation and FreeCAD Scripting Basics.

A SectionView can be created with macros and from the Python console by using the following functions:

doc = FreeCAD.ActiveDocument
box = doc.Box
page = doc.Page

view = doc.addObject("TechDraw::DrawViewPart", "View")
page.addView(view)
view.Source = box
view.Direction = (0, 0, 1)

section = doc.addObject("TechDraw::DrawViewSection", "Section")
page.addView(section)
section.Source = box
section.BaseView = view
section.Direction = (0, 1, 0)
section.SectionNormal = (-1, 0, 0)

doc.recompute()

Examples

For some more information about section views and some use cases, have a look at: TechDraw section examples.

BrokenView

ComplexSection

TechDraw

TechDraw

• Pages: Insert Default Page, Insert Page using Template, Update template fields, Redraw Page, Print All Pages, Export Page as SVG, Export Page as DXF
• Views:
  • TechDraw views: Insert View, Insert Broken View, Insert Section View, Insert Complex Section View, Insert Detail View, Insert Projection Group, Insert Clip Group, Insert SVG Symbol, Insert Bitmap Image, Share View, Turn View Frames On/Off, Project Shape
  • Views from other workbenches: Insert Active View, Insert Draft Workbench Object, Insert BIM Workbench Object, Insert Spreadsheet View
• Stacking: Move view to top of stack, Move view to bottom of stack, Move view up one level, Move view down one level

---

• Dimensions: Insert Dimension, Insert Length Dimension, Insert Horizontal Dimension, Insert Vertical Dimension, Insert Radius Dimension, Insert Diameter Dimension, Insert Angle Dimension, Insert 3-Point Angle Dimension, Insert Area Annotation, Create Arc Length Dimension, Insert Horizontal Extent Dimension, Insert Vertical Extent Dimension, Create Horizontal Chain Dimensions, Create Vertical Chain Dimensions, Create Oblique Chain Dimensions, Create Horizontal Coordinate Dimensions, Create Vertical Coordinate Dimensions, Create Oblique Coordinate Dimensions, Create Horizontal Chamfer Dimension, Create Vertical Chamfer Dimension, Insert Balloon Annotation, Insert Axonometric Length Dimension, Insert Landmark Dimension, Dimension Repair, Link Dimension to 3D Geometry

---

• Hatching: Hatch Face using Image File, Apply Geometric Hatch to Face,
• Annotations: Insert Annotation, Add Leaderline to View, Insert Rich Text Annotation, Add Cosmetic Vertex, Add Midpoint Vertices, Add Quadrant Vertices, Add Centerline to Faces, Add Centerline between 2 Lines, Add Centerline between 2 Points, Add Cosmetic Line Through 2 points, Add Cosmetic Circle, Change Appearance of Lines, Show/Hide Invisible Edges, Add Welding Information to Leader, Add Surface Finish Symbol, Add Hole or Shaft Tolerances

---

• Extensions:
  • Attributes and modifications: Select Line Attributes, Cascade Spacing and Delta Distance, Change Line Attributes, Extend Line, Shorten Line, Lock/Unlock View, Position Section View, Position Horizontal Chain Dimensions, Position Vertical Chain Dimensions, Position Oblique Chain Dimensions, Cascade Horizontal Dimensions, Cascade Vertical Dimensions, Cascade Oblique Dimensions, Calculate the area of selected faces, Calculate the arc length of selected edges, Customize format label
  • Centerlines and threading: Add Circle Centerlines, Add Bolt Circle Centerlines, Add Cosmetic Thread Hole Side View, Add Cosmetic Thread Hole Bottom View, Add Cosmetic Thread Bolt Side View, Add Cosmetic Thread Bolt Bottom View, Add Cosmetic Intersection Vertex(es), Add an offset vertex, Add Cosmetic Circle, Add Cosmetic Arc, Add Cosmetic Circle 3 Points, Add Cosmetic Parallel Line, Add Cosmetic Perpendicular Line
  • Dimensions: Insert '⌀' Prefix, Insert '□' Prefix, Insert 'n×' Prefix, Remove Prefix, Increase Decimal Places, Decrease Decimal Places

---

• Miscellaneous: Remove Cosmetic Object

---

• Additional: Line Groups, Templates, Hatching, Geometric dimensioning and tolerancing, Preferences

User documentation

• Getting started
• Installation: Download, Windows, Linux, Mac, Additional components, Docker, AppImage, Ubuntu Snap
• Basics: About FreeCAD, Interface, Mouse navigation, Selection methods, Object name, Preferences, Workbenches, Document structure, Properties, Help FreeCAD, Donate

---

• Help: Tutorials, Video tutorials
• Workbenches: Std Base, Assembly, BIM, CAM, Draft, FEM, Inspection, Material, Mesh, OpenSCAD, Part, PartDesign, Points, Reverse Engineering, Robot, Sketcher, Spreadsheet, Surface, TechDraw, Test Framework

---

• Addons: Addon Manager, External workbenches, Scripting and macros

---

• Hubs: User hub, Power users hub, Developer hub