Leave Sketch¶

In one sentence: Create a new 2-D sketch on a plane or face, enter its edit mode to draw and constrain geometry, then leave edit mode when the sketch is fully constrained and ready to drive a solid feature.

Overview¶

Workbench: Sketcher · Menu: Sketch → New Sketch
Toolbar: Sketcher · Shortcut: none

These three commands control the lifecycle of a sketch object: you create it, work inside it, and then step back out. They are always the first and last actions of any sketching session.

Intuition¶

Think of a sketch as a tracing-paper overlay placed on a flat surface. You flip it down onto a face (New Sketch), draw on it with constraint-aware tools (edit mode), and then flip it back up when you are done (Leave Sketch). The tracing paper remembers everything you drew, and Part Design can pick it up to extrude or revolve it into 3-D solid geometry.

The three commands are deliberately separate so that you can return to a sketch at any point — even after a Pad or Pocket has been built on top of it — and revise the 2-D geometry without losing the 3-D feature.

When to use New Sketch¶

You are starting a new feature (Pad, Pocket, Revolution, …) and need a 2-D profile as its input.
You want to add a cross-section sketch for a Pipe or Loft spine.
You need a standalone sketch to drive a datum constraint or a ShapeBinder.

When NOT to use New Sketch¶

You already have a sketch and want to revise it — double-click the sketch in the model tree or select it and press Edit Sketch instead.
You want to attach an existing sketch to a different face — use Map Sketch to Face instead of creating a new sketch.

Step-by-step walkthrough¶

Creating a new sketch¶

Switch to the Sketcher workbench (or remain in Part Design — Part Design embeds Sketcher for sketch creation automatically).
Activate New Sketch via menu Sketch → New Sketch or the toolbar button.
Select the attachment plane. A dialog appears asking which plane to use:
- XY, XZ, or YZ — the global coordinate planes.
- A face on an existing solid in the viewport.
- A datum plane you previously created.
Click a plane or face. FreeCAD enters sketch edit mode immediately.
Draw geometry and apply constraints using the tools described in this workbench documentation.
Leave edit mode when finished — see Leaving a sketch below.

Tip

When working in Part Design, you can activate New Sketch while a Body is active and select any planar face of the current solid. FreeCAD positions the sketch automatically relative to that face.

Editing an existing sketch¶

Double-click the sketch in the Model tree, or select it and choose Sketch → Edit Sketch from the menu (shortcut: none).
The viewport switches to sketch edit mode: the XY grid appears, the 3-D model is partially hidden, and the Sketcher toolbar becomes active.
Revise geometry and constraints.
Leave edit mode as below.

Leaving a sketch¶

When you have finished drawing and the sketch is fully constrained (green):

Press the Close button in the Tasks panel, or
Choose Sketch → Leave Sketch from the menu, or
Click anywhere outside the sketch viewport area.

Leaving with remaining degrees of freedom

You can close a sketch that is not fully constrained — FreeCAD will not stop you. However, Part Design features built on an under-constrained sketch may produce unpredictable geometry when other dimensions change. Always aim for "Fully constrained" (DoF = 0, all geometry green) before closing.

Parameters¶

New Sketch has no persistent parameters. The Attachment (which plane the sketch is attached to) is set at creation time and can be changed later via Map Sketch to Face.

Advanced usage¶

Creating a sketch without a Part Design body¶

When Sketcher is the active workbench (not Part Design), New Sketch creates a standalone Sketcher::SketchObject in the document without a Body container. This is useful for sketches that drive Part workbench operations or ShapeBinders, but do not use standalone sketches as Part Design feature profiles — always have them inside a Body.

Attachment offset¶

After creating a sketch, you can fine-tune its attachment position by selecting the sketch, opening the Data panel, and adjusting the Map Path Parameter or Attachment Offset properties. This moves the sketch along or perpendicular to its attached plane without detaching it.

Common mistakes and pitfalls¶

Sketch not fully constrained before closing

Cause: Some geometry was drawn but not given enough constraints.
Fix: Watch the DoF counter in the Solver panel. Apply constraints until it reads "Fully constrained". Use Sketch → Select Under-Constrained Elements to highlight the remaining free geometry.

New sketch created outside any Body

Cause: The Sketcher workbench (not Part Design) was active when New Sketch was invoked, and no Body was selected.
Fix: Switch to Part Design, activate a Body, then create the sketch inside it. Alternatively, drag the standalone sketch into the Body in the Model tree.

Sketch attached to the wrong face

Cause: The wrong face was clicked during the attachment dialog.
Fix: Use Map Sketch to Face to reattach the sketch to the correct face or plane without losing its geometry.

Python API¶

Minimal example¶

import FreeCAD as App
import Sketcher

doc = App.newDocument()

# Create a standalone sketch on the XY plane
sketch = doc.addObject("Sketcher::SketchObject", "Sketch")
sketch.AttachmentSupport = (doc.XY_Plane, [""])
sketch.MapMode = "FlatFace"
doc.recompute()

# Add a line from (0,0) to (10,0)
import Part
sketch.addGeometry(Part.LineSegment(App.Vector(0, 0, 0),
                                    App.Vector(10, 0, 0)), False)
doc.recompute()

print("Sketch has", sketch.GeometryCount, "geometry elements")

Key properties¶

Property	Type	Description
`AttachmentSupport`	`App::PropertyLinkSubList`	The face, plane, or axis the sketch is attached to.
`MapMode`	`App::PropertyEnumeration`	How the sketch aligns to its attachment (`"FlatFace"`, `"NormalToEdge"`, etc.).
`AttachmentOffset`	`App::PropertyPlacement`	Fine-tune translation and rotation of the sketch relative to its attachment.
`MapPathParameter`	`App::PropertyFloat`	Position along a path edge for edge-based attachment modes.
`FullyConstrained`	`App::PropertyBool`	Read-only. `True` when the sketch has zero remaining DoF.