Move Feature After…¶

In one sentence: Change the position of a feature within a Body's feature tree so that it is evaluated after a different feature.

Overview¶

Workbench: Part Design · Menu: (context menu only — right-click a feature in the model tree)
Toolbar: none · Shortcut: none

"Move Feature in Tree" is the common informal name for the Move Feature After… command (PartDesign_MoveFeatureInTree). It changes the order in which features are evaluated within a single Body by repositioning the selected feature (or features) after a target feature that you choose from a list. Because Part Design evaluates features in tree order, changing that order changes the resulting solid shape.

Intuition¶

A Body's feature tree is an ordered sequence of operations. FreeCAD evaluates them from top to bottom: each feature receives the shape produced by all features before it and adds or removes material from it. If you place a Fillet before a Pocket, the fillet is on a face that the pocket may later destroy. Placing the Fillet after the Pocket changes the outcome.

Think of it as rearranging steps in a recipe. The ingredients (the features) stay the same, but the order in which you apply them produces a different final dish. Move Feature After… is the tool that lets you change that order after the fact, without having to delete and recreate anything.

When to use it¶

You created a feature at the end of the tree but it logically belongs earlier — for example, a Fillet that should come before a subsequent Pocket.
You want to reorder a datum plane or datum line so that it appears before the features that reference it, making the dependency chain explicit.
You need to fix evaluation order after copying or importing features that arrived in the wrong sequence.
You want to group related features visually in the tree, even when the reorder does not change the geometry (e.g. moving datum planes together at the top of the tree).

When NOT to use it¶

You want to move a feature to a different Body — use Move Object To… instead; Move Feature After… only works within the same Body.
You want to suppress all features after a given point — use Set Tip instead.
You want a copy rather than a reorder — use Duplicate Object to create a copy at a new position.
The BaseFeature (the imported solid at the base of the Body) needs to be moved — the command explicitly blocks this; the BaseFeature must always remain at the start of the tree.

Step-by-step walkthrough¶

Prerequisite: A Body with at least two features in the model tree.

In the Model panel (model tree), select the feature or features you want to reorder. You can Ctrl-click to select multiple features.

All selected features must belong to the same Body

If any selected feature is in a different Body, the command shows an error and does nothing.
Right-click the selection and choose Move Feature After… from the context menu.
A dialog appears listing all features currently in the Body, plus a special entry "Beginning of the body" at the top of the list. Select the feature you want the moved feature to follow, then click OK.
- Choosing "Beginning of the body" places the feature at the very start of the tree (before all other features).
- Choosing any named feature places the moved feature immediately after it.
FreeCAD performs a dependency-order check. If moving the feature would place it before another feature that it depends on — violating causality — the command is aborted and a Dependency violation dialog describes the conflict.
If the moved feature lands after the current Tip, a confirmation dialog asks: "Set tip to last feature?". Clicking Yes advances the Tip to the moved feature; clicking No leaves the Tip unchanged.
The model tree reflects the new order and FreeCAD recomputes the Body.

Tip

When reordering multiple features at once, they are inserted in their original relative order immediately after the chosen target feature. Their sequence relative to each other is preserved.

Parameters¶

Move Feature After… has a single input: the position within the tree where the feature should be placed.

Input	Description
Target position (dropdown list)	The feature after which the selected feature(s) will be inserted. The list includes every feature in the Body plus "Beginning of the body" as the first entry.

Advanced usage¶

What counts as a valid feature to move¶

The command accepts:

Any PartDesign::Feature (Pad, Pocket, Fillet, etc.)
App::DatumElement objects (datum planes, datum lines, datum points)
App::LocalCoordinateSystem objects (coordinate systems)

It does not accept the Body's BaseFeature (the external solid, if any, that the Body is built upon).

Dependency-order enforcement¶

After the reorder, FreeCAD checks every PartDesign::Feature in the new tree order. If any feature depends on an object that appears later in the tree — a dependency violation — the command is rolled back entirely and the tree is restored to its previous state. The error dialog lists the specific feature pairs that conflict.

This means you cannot, for example, move a Pad before the Sketch it extrudes. You would need to move both the Sketch and the Pad together.

Interaction with the Tip¶

If the moved feature ends up after the current Tip, FreeCAD offers to advance the Tip to cover the moved feature. This is the expected behaviour when you are inserting a late-arriving feature and want it included in the final shape. You can decline and manually adjust the Tip using Set Tip instead.

Common mistakes and pitfalls¶

Dependency violation — Early feature must not depend on later feature

Cause: The reorder would place a feature before something it references. For example, moving a Pocket before the Pad whose face it uses.
Fix: Include all dependent objects in the selection so they move as a group, or restructure the sketch to reference a datum plane instead of a body face before reordering.

Impossible to move the base feature of a body

Cause: The Body's BaseFeature (an imported solid at position 0 of the tree) was included in the selection.
Fix: Deselect the BaseFeature and reorder only the features above it.

Select one or more features from the same body

Cause: The selection includes features from different Bodies, or includes an object that is not inside any Body.
Fix: Select only features that belong to the same Body before invoking the command.

Reorder silently changes the shape without an obvious error

Cause: Moving a feature that modifies geometry which later features also modify can change the final solid shape in non-obvious ways. The model recomputes without error but produces a different result.
Fix: After reordering, inspect the 3-D viewport carefully and step through the tree using Set Tip to verify that each stage still produces the intended geometry.

Python API¶

Move Feature After… uses the removeObject and insertObject methods on the Body. There is no dedicated Python function — you call these methods directly.

Minimal example¶

import FreeCAD as App

doc = App.activeDocument()
body = doc.getObject("Body")  # replace with your Body name

feature = doc.getObject("Fillet")       # the feature to move
after   = doc.getObject("Pad")          # insert after this feature

# Remove the feature from its current position
body.removeObject(feature)  # TODO: verify method name is removeObject

# Re-insert it after the target feature
# The third argument (True) inserts *after* the given object
body.insertObject(feature, after, True)  # TODO: verify signature and third-argument semantics

doc.recompute()

Body methods¶

Method	Description
`removeObject(feature)`	Remove the feature from the Body's ordered group without deleting it from the document.
`insertObject(feature, after, after_flag)`	Re-insert the feature into the Body's group. When the third argument is `True`, the feature is placed after the specified object. When `False` or omitted, placement semantics differ.