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Insert View

In one sentence: Creates a standard orthographic projection of a selected 3-D object onto the drawing page — the fundamental TechDraw operation.

Overview

Workbench: TechDraw
Menu: TechDraw → Views → Insert View

Every TechDraw drawing starts with at least one view. A view is a live link to the 3-D geometry — it re-projects automatically when the model changes.

What can be projected

  • A PartDesign Body
  • A Part Shape (any object with a Shape property)
  • An Assembly (projects the full assembled state)
  • A Part::Feature (any solid, shell, or compound)

Step-by-step

  1. Select the 3-D object(s) in the model tree.
  2. Choose TechDraw → Views → Insert View.
  3. The view appears on the active page. The default direction looks down the −Y axis (a front view in FreeCAD's coordinate convention).
  4. Click the view on the page to select it. Drag it to reposition.
  5. In the Data panel, change Direction to set the projection direction.

Common projection directions

View Direction
Front (0, -1, 0)
Top (0, 0, 1)
Right (1, 0, 0)
Isometric (1, -1, 1) (normalised)

View properties (Data panel)

Property Description
Direction Projection direction vector
Scale Drawing scale ratio (1.0 = 1:1)
Scale Type Custom / Page / Automatic
Rotation Rotation of the view on the page (degrees)
CoarseView Faster rendering at lower quality (useful for large assemblies)
ShowHidden Show hidden edges as dashed lines
ShowSmoothLines Show smooth (tangent) edge transitions
ShowSeamLines Show seam lines on surfaces

Python API

import FreeCAD as App
import TechDraw

doc = App.ActiveDocument
page = doc.getObject("Page")
body = doc.getObject("Body")

view = doc.addObject("TechDraw::DrawViewPart", "FrontView")
page.addView(view)
view.Source = [body]
view.Direction = App.Vector(0, -1, 0)   # Front view
view.Scale = 1.0
doc.recompute()

Common mistakes and pitfalls

Default front view looks along –Y

TechDraw's default front view looks along −Y. FreeCAD's PartDesign convention places the XY plane as the sketch plane, so the default front view of a PartDesign body often shows the bottom face. Adjust the Direction property or set a custom direction in the task panel.

Renaming or deleting the source body breaks the view

If you rename or delete a body that a view references, the view displays a red warning and stops updating. Re-select the source object in the view's Source property.

See also