New Sketch¶

In one sentence: Create a new Sketcher sketch attached to a plane or face and open it for editing inside the active Part Design Body.

Overview¶

Workbench: Part Design · Menu: Sketch → New Sketch
Toolbar: Part Design Helper Features (via the "Create Datum" dropdown) · Shortcut: none

New Sketch creates a Sketcher::SketchObject inside the active Body and immediately opens it in the Sketcher editor. The sketch is attached to a chosen plane or planar face, which defines its coordinate system. Once closed, the sketch is available as a profile for any sketch-based feature such as Pad, Pocket, Revolution, or Additive Pipe.

Intuition¶

Think of a sketch as a sheet of graph paper fixed to a surface. Before you can draw on it you must first decide which surface to stick it to — a principal plane (XY, XZ, or YZ), a datum plane you have already created, or a flat face on an existing solid. That choice determines which direction your 2-D drawing will face in 3-D space.

New Sketch is the entry point for almost every Part Design workflow. Every solid feature that requires a profile begins here. Unlike the Sketcher's own "New Sketch" command (which creates a freestanding sketch outside any Body), this command always creates the sketch inside the active Body so that subsequent features can use it.

The command checks what you have selected when you invoke it. If a face or plane is already selected, FreeCAD attaches the sketch there immediately and opens the editor. If nothing is selected but the Body has exactly one valid plane, the sketch is placed on that plane without asking. If multiple valid planes exist, a plane-picker dialog appears so you can choose.

When to use it¶

You are starting a new Body and need to draw the first profile for a Pad or Revolution.
You want to add another sketch mid-way through a feature tree to serve as a profile for a later Additive Pipe or Loft.
You want to draw on a specific planar face of an existing solid — for example, the top face of a Pad — to build the next feature on top of it.
You need a new sketch on a datum plane you have created with Part Design Plane.
You are restarting after closing the Sketcher and want to edit a different cross-section without touching existing features.

When NOT to use it¶

You want to edit an existing sketch — double-click the sketch in the model tree, or use Sketch → Edit Sketch instead.
You want to reattach a sketch to a different plane — use Sketch → Map Sketch to Face (Sketcher_MapSketch).
You are working outside a Body and want a freestanding 2-D sketch — use the Sketcher workbench's own New Sketch command. Part Design's New Sketch always requires an active Body.

Step-by-step walkthrough¶

Prerequisites: An open FreeCAD document. A Body will be created automatically if one does not exist yet.

Optionally pre-select a plane or face. Click a principal plane (XY, XZ, or YZ in the Origin), a PartDesign Plane datum, or a flat face on an existing solid in the viewport before invoking the command. Pre-selecting skips the plane-picker dialog.
Invoke New Sketch. Go to Sketch → New Sketch in the menu bar, or click the New Sketch icon in the "Part Design Helper Features" toolbar (inside the "Create Datum" dropdown group).
Select a plane if prompted. If you had nothing pre-selected and multiple valid planes are available, a plane-picker dialog appears. Click the desired plane and press OK.

No valid planes error

If no Body exists and one cannot be created, or if the Body has no valid plane (which can happen in edge cases with misplaced insert points), FreeCAD will show a warning. Create a Body manually first, or select a face before invoking the command.
Draw in the Sketcher. The Sketcher editor opens. Draw your geometry and apply constraints until the sketch is fully constrained (all lines turn green).
Close the Sketcher. Click "Close" in the task panel or press Esc. The sketch appears in the model tree under the Body, ready to be used as a profile for a feature.

Tip

If you click a flat face on an existing solid before invoking New Sketch, the sketch is attached directly to that face with MapMode = FlatFace. This is the fastest way to build stacked features — click the top face of a Pad, then invoke New Sketch.

Parameters¶

New Sketch itself has no task-panel parameters — the command creates a Sketcher::SketchObject and opens it for editing. The resulting sketch object has the following key properties visible in the property panel after closing the editor:

Property	Type	Default	Description
`AttachmentSupport`	`App::PropertyLinkSubList`	—	The plane, face, or datum the sketch is attached to. Set automatically when you choose a plane.
`MapMode`	`App::PropertyString`	`FlatFace`	Attachment mode. `FlatFace` when attached to a face or plane. `ObjectXY` when attached to another sketch.
`MapReversed`	`App::PropertyBool`	`False`	Flips the sketch normal (reverses which side of the support plane the Z axis points).
`Placement`	`App::PropertyPlacement`	—	Computed from the attachment; normally read-only while mapped.

Advanced usage¶

Sketching on an external face¶

If you pre-select a face that belongs to a solid outside the active Body, FreeCAD asks whether to create a cross-reference (an xref link), an independent copy, or a dependent copy. Choose:

Cross-reference to keep a live link — the sketch attachment updates when the external solid moves.
Independent copy to capture the face geometry once without any ongoing link.
Dependent copy to create a Shape Binder of the face and attach to that.

Multiple sketches on the same plane¶

A Body can contain any number of sketches on the same plane. Each is an independent object in the feature tree. The insertion point (the "Tip" marker) determines which features are visible at any given time, but all sketches remain in the tree.

Using datum planes as sketch supports¶

Creating a datum plane (Part Design → Datum Plane) before invoking New Sketch gives you complete freedom to place the sketch at any position and angle. Once the datum plane exists, it appears in the plane-picker dialog alongside the principal planes.

Common mistakes and pitfalls¶

Sketch created outside the Body

Cause: No Body was active when New Sketch was invoked, and FreeCAD created a new Body automatically, but you already had features in a different Body.
Fix: Activate the intended Body first (double-click it in the model tree), then invoke New Sketch again.

Sketch is not fully constrained but was closed

Cause: Lines are still blue (under-constrained) or red (over-constrained) when you close the Sketcher.
Fix: Re-open the sketch (double-click it), add the missing constraints, and close again. Attempting to create a Pad or Pocket from an under-constrained sketch will succeed but the shape will change if you later edit the sketch.

Non-planar face selected as support

Cause: A curved face (cylinder, sphere) was selected before invoking New Sketch.
Fix: Select only flat (planar) faces, or use a datum plane positioned tangent to the surface.

MapMode resets unexpectedly after model change

Cause: The face the sketch is attached to was renumbered by a topology change (topological naming problem).
Fix: Use a datum plane instead of a direct face reference, or enable toponaming features available in FreeCAD 1.0+.

Python API¶

Minimal example¶

import FreeCAD as App
import Part
import Sketcher

doc = App.newDocument()

# Create a Body
body = doc.addObject("PartDesign::Body", "Body")

# Create a sketch attached to the XY plane
sketch = body.newObject("Sketcher::SketchObject", "Sketch")
sketch.AttachmentSupport = (doc.XY_Plane, [""])
sketch.MapMode = "FlatFace"
doc.recompute()

# Add a rectangle 20 × 10 mm centred on the origin
sketch.addGeometry([
    Part.LineSegment(App.Vector(-10, -5, 0), App.Vector(10, -5, 0)),
    Part.LineSegment(App.Vector(10, -5, 0),  App.Vector(10,  5, 0)),
    Part.LineSegment(App.Vector(10,  5, 0),  App.Vector(-10,  5, 0)),
    Part.LineSegment(App.Vector(-10,  5, 0), App.Vector(-10, -5, 0)),
], False)

doc.recompute()
print(f"Sketch is fully closed: {sketch.Shape.isClosed()}")

Key properties on the resulting sketch object¶

Property	Type	Description
`AttachmentSupport`	`App::PropertyLinkSubList`	Plane or face the sketch is attached to.
`MapMode`	`App::PropertyString`	Attachment mode string (e.g. `"FlatFace"`, `"ObjectXY"`).
`MapReversed`	`App::PropertyBool`	`True` to flip the sketch normal.
`Geometry`	`Part::PropertyGeometryList`	The geometric elements (lines, arcs, …) inside the sketch.
`Constraints`	`Sketcher::PropertyConstraintList`	All Sketcher constraints applied to the geometry.