Mirror¶

In one sentence: Mirror selected features across a plane to create a symmetrical copy without duplicating sketches or parameters.

Overview¶

Workbench: Part Design · Menu: Part Design → Transformation Features → Mirror
Toolbar: Part Design Modeling Features · Shortcut: none

Mirror takes one or more existing Body features and creates a reflected copy of each across a chosen plane. The result is fused back into the Body — it adds or removes material exactly as the originals do, just on the opposite side of the mirror plane. Because it references the originals parametrically, any change to the original feature is automatically reflected in the mirrored copy.

Intuition¶

Think of placing a pocket or boss next to a mirror: you see the original on one side and its exact reflection on the other, perfectly equidistant from the glass. The "glass" is the mirror plane — a flat reference that Mirror uses to flip the geometry.

The key point is that Mirror operates on features, not on the entire Body. You choose which features to mirror (e.g. a single countersunk hole) and Mirror creates reflected copies of only those features, leaving the rest of the Body unchanged. If you want to mirror everything, you either select all features or use the Transform body mode in the task panel.

When to use it¶

Your part is symmetric and you have modelled one half: mirror the additive and subtractive features to complete the other half without re-drawing them.
You need a hole, boss, or slot to appear symmetrically on both sides of a datum plane (e.g. two mounting holes either side of a centreline).
You want to enforce symmetry parametrically — if the original feature moves, the mirrored copy follows.
You are working inside a MultiTransform and want one stage of the chain to be a reflection.

When NOT to use it¶

You need more than two copies, or copies arranged in a line — use Linear Pattern instead.
You need copies arranged around an axis — use Polar Pattern instead.
You want to combine several kinds of transformation in one operation — use Multi-Transform instead.
The part itself (not individual features) needs to be mirrored as a solid operation — use Part → Mirror from the Part workbench.

Step-by-step walkthrough¶

Prerequisites: An active Body containing at least one sketch-based feature (Pad, Pocket, Revolution, etc.) and a suitable mirror plane — either the Body's built-in origin planes (XY, XZ, YZ), a Datum Plane, or a planar face of the solid.

Select the feature(s) to mirror. Click one or more features in the model tree or 3D view. You can also make no selection and add features inside the task panel.
Activate Mirror. Go to Part Design → Transformation Features → Mirror. The task panel opens.
Choose the transform scope. At the top of the task panel two radio buttons appear:
- Transform body — the transformation is applied to the whole Body shape.
- Transform tool shapes — the transformation is applied only to the listed features (individual pads, pockets, etc.).
  Select Transform tool shapes for feature-level mirroring (the default for most cases).
Add or remove features in the list. Use Add Feature and Remove Feature to populate the feature list with the features you want mirrored. The list shows the features' labels.
Select the mirror plane. In the Plane dropdown, choose:
- An origin plane (XY, XZ, or YZ) of the Body.
- A Datum Plane you created earlier.
- A planar face on the existing solid (click Select reference and then pick a face in the viewport).
- A sketch axis (horizontal, vertical, or a named construction axis).
Click OK. FreeCAD computes the mirror and adds a Mirrored feature to the model tree.

Tip

If the mirrored copy causes a BREP validation failure (e.g. the original and its reflection are tangent or nearly overlapping), try using a face that is clearly offset from both features. Mirror requires that the reflected copy does not coincide with the original.

Parameters¶

The common header section (shared by all transformation features) controls which features are transformed. The Mirror-specific section controls the plane.

Common transformation controls¶

Parameter	Type	Default	Description
Transform body / Transform tool shapes	Radio buttons	Transform tool shapes	When Transform body is selected (`TransformMode = "Whole shape"`), the entire Body solid is mirrored. When Transform tool shapes is selected (`TransformMode = "Features"`), only the listed features are mirrored.
Feature list	Ordered list	—	The features whose solid contributions (add or subtract) will be mirrored. Use Add Feature / Remove Feature buttons to modify the list.
Recompute on change	Checkbox	checked	Triggers an immediate recompute whenever a parameter changes. Uncheck for large models to defer recomputation until OK.

Mirror-specific controls¶

Parameter	Type	Default	Description
Plane	Dropdown / link	V_Axis of profile sketch (or XY origin plane)	The plane across which features are reflected. Accepts a Datum Plane, an origin plane (XY / XZ / YZ), a planar face of the solid, or a sketch axis.

Advanced usage¶

Mirroring inside Multi-Transform¶

When Mirrored is used as a sub-transformation inside a Multi-Transform, it does not show the feature list or the transform-scope radio buttons — those are controlled by the parent Multi-Transform. Only the Plane dropdown is shown.

Using a sketch axis as the plane¶

When the profile sketch is available (i.e. the original feature is sketch-based), you can select the sketch's horizontal axis (H_Axis) or vertical axis (V_Axis) as the mirror reference. The mirror plane is then the plane that contains that axis and is perpendicular to the sketch plane. Named construction lines in the sketch appear as Axis0, Axis1, etc.

Common mistakes and pitfalls¶

Mirror fails with 'could not be created' error

Cause: The mirrored copy overlaps or is coincident with the original, producing a degenerate OCCT shape.
Fix: Check that the mirror plane does not pass through the original feature. If it does, offset the plane or redesign the feature so that the reflected copy is cleanly separated.

No plane reference specified error

Cause: The Plane dropdown is blank — typically because the task panel was opened without a valid sketch or origin in the Body.
Fix: Make sure the Body has an origin (all Bodies created via Part Design → Create Body do). Re-open the task panel and pick a plane from the dropdown.

Wrong side is mirrored

Cause: The mirror plane normal points in the opposite direction from what was expected.
Fix: Mirror has no Reversed option. Change the reference plane or reposition the original feature so it ends up on the correct side after reflection.

Mirrored feature disappears in the model tree

Cause: Mirror operates on features, not standalone objects. If the selected feature is removed from the Body, the Mirror feature will fail on the next recompute.
Fix: Keep the original feature in the Body and above the Mirror feature in the feature tree (as a dependency).

Python API¶

Minimal example¶

import FreeCAD as App
import PartDesign
import Sketcher
import Part

doc = App.newDocument()

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

# Profile sketch on XY plane
sketch = doc.addObject("Sketcher::SketchObject", "Sketch")
body.addObject(sketch)
sketch.addGeometry(Part.Rectangle(App.Vector(-5, 0, 0), App.Vector(5, 10, 0)), False)
doc.recompute()

# Pad the sketch 5 mm
pad = doc.addObject("PartDesign::Pad", "Pad")
body.addObject(pad)
pad.Profile = sketch
pad.Length = 5.0
doc.recompute()

# Mirror the Pad across the YZ plane (Body origin)
mirrored = doc.addObject("PartDesign::Mirrored", "Mirrored")
body.addObject(mirrored)
mirrored.Originals = [pad]
origin = body.getOrigin()
mirrored.MirrorPlane = (origin.getYZ(), [""])  # TODO: verify sub-element string
doc.recompute()

Method signature¶

doc.addObject("PartDesign::Mirrored", "<name>")

Resulting feature properties¶

Property	Type	Description
`Originals`	`App::PropertyLinkList`	The features to be mirrored. Inherited from `Transformed`.
`TransformMode`	`App::PropertyEnumeration`	`"Features"` mirrors only listed features; `"Whole shape"` mirrors the entire Body solid. Inherited from `Transformed`.
`MirrorPlane`	`App::PropertyLinkSub`	The plane reference. Can point to a `PartDesign::Plane`, `App::Plane` (origin plane), a planar `Part::Feature` face, or a `Part::Part2DObject` axis sub-element.
`Refine`	`App::PropertyBool`	When `True`, removes redundant edges from the resulting shape. Inherited from `FeatureRefine`.