Pad¶

In one sentence: Extrude a closed 2-D sketch into a 3-D solid by pushing it along its normal direction.

Overview¶

Workbench: Part Design · Menu: Part Design → Additive Features → Pad
Toolbar: Part Design Modeling Features · Shortcut: none

Pad is the most fundamental additive feature in Part Design. It takes a closed sketch (or a face selected from an existing solid) and extrudes it in a straight line, fusing the resulting solid into the active Body. The extrusion distance can be a fixed length, symmetric about the sketch plane, or driven by existing geometry in the model — giving precise control over how far and in which direction the material grows.

Intuition¶

Think of a cookie cutter pressed into dough: the cutter's outline (the sketch) determines the shape of the result, and how far you push it down (the length) determines the thickness. You get a solid with the sketch's profile on the bottom face, the same profile on the top face, and vertical walls connecting them.

The sketch plane is the starting face of the solid. The default direction is perpendicular to that plane — the sketch's normal. If the sketch lies flat on the XY plane, the pad grows in the Z direction. You can override this with a custom direction or a reference axis if you need an oblique extrusion.

One important concept: Pad always adds material. If the sketch is larger than the existing solid, the result is unioned with it. If you need to remove material with the same straight-extrusion logic, use Pocket instead.

When to use it¶

You have drawn the outline of a part (a bracket, plate, or boss) and want it to have physical thickness.
You are building a model parametrically and want the height of a feature to be driven by a named dimension.
You need a solid to grow symmetrically on both sides of a sketch plane (use the Symmetric mode).
You want a pad to stop exactly at an existing face in the model, regardless of how that face moves parametrically (use the Up to face or Up to shape mode).
You need draft angles on the walls of a moulded or cast feature (use the taper angle option).

When NOT to use it¶

The cross-section rotates around an axis — use Revolution; it is the right tool for axisymmetric solids such as shafts, flanges, and rings.
The cross-section needs to follow a curved path — use Additive Pipe, which sweeps a profile along an arbitrary spine.
The solid should blend through several profiles in 3-D space — use Additive Loft.
You want to cut material — use Pocket, which has identical parameters but removes material from the Body instead of adding it.

Step-by-step walkthrough¶

Prerequisite: An active Body containing at least one sketch with a single closed wire. The sketch should be fully constrained.

Select the sketch in the model tree or by clicking it in the viewport. The sketch must be closed — an open wire produces an error.
Activate Pad via the menu Part Design → Additive Features → Pad, or click the Pad button in the toolbar.
Set the Mode (top of the task panel) to one of:
One side — extrude in one direction only (default).
Two sides — configure side 1 and side 2 independently.
Symmetric — extrude equal distances in both directions from the sketch plane.
Set the Type for Side 1 (and Side 2 if applicable). See the Parameters table for all options. The most common choice is Dimension, where you type in an explicit length.
Enter the length in the Length field (visible when Type is Dimension). The default is 10 mm.
Adjust optional settings if needed:
Taper angle — adds draft to the extruded walls.
Reversed — flips the extrusion direction.
Direction/edge — change from the sketch normal to a custom axis.
Click OK. The pad is created and fused into the Body. The sketch becomes a child of the Pad feature in the model tree.

Tip

If you activate Pad without pre-selecting a sketch, FreeCAD will ask you to select a profile. You can click a sketch in the model tree or click a planar face directly in the viewport — a face selection pads the entire face outline.

Parameters¶

The task panel is divided into a Mode selector, sections for Side 1 and (optionally) Side 2, a Reversed toggle, and a Direction group.

Mode¶

Parameter	Type	Default	Description
Mode	Dropdown	One side	Controls how the two extrusion sides are configured. `One side`: only Side 1 is active. `Two sides`: Side 1 and Side 2 can be configured independently with different types and lengths. `Symmetric`: Side 1 settings apply equally in both directions; the total length is the Side 1 length.

Side 1 (and Side 2 when Mode = Two sides)¶

These controls appear for each active side.

Parameter	Type	Default	Description
Type	Dropdown	Dimension	Extrusion method. See the type descriptions below.
Length	Length	10 mm	Extrusion length. Active only when Type is Dimension. Accepts negative values (reverses direction).
Offset to face	Length	0 mm	Signed offset applied when the pad ends at a face or shape (types To last, To first, Up to face, Up to shape). Positive moves the end face away from the sketch; negative moves it toward the sketch.
Taper angle	Angle	0°	Draft angle applied to the extruded walls. A positive angle expands the cross-section as it grows away from the sketch; a negative angle contracts it. Valid range is just under ±90°. Active only when Type is Dimension.
Select Face / Select Shape	Button	—	Opens selection mode to pick the target face or shape for Up to face / Up to shape types.

Type values:

Type (UI label)	Internal value	Description
Dimension	`Length`	Extrude by a fixed distance set in the Length field.
To last	`UpToLast`	Extrude until the last face of the Body that the extrusion axis intersects.
To first	`UpToFirst`	Extrude until the nearest face of the Body that the extrusion axis intersects.
Up to face	`UpToFace`	Extrude until a specific selected face, following its shape.
Up to shape	`UpToShape`	Extrude until one or more selected faces or an entire solid.

Type in depth¶

The Type dropdown determines when the extrusion stops. Dimension gives you an explicit number; the other four modes let the Body's existing geometry decide the termination point.

Dimension (default)¶

You specify the exact height as a length value. Think of pressing a stamp down by precisely 10 mm — the depth is fully under your control.

Use this mode when: - You know the exact depth from a drawing or design intent - You want a taper angle on the extruded walls (only available in Dimension mode) - The pad height is an independent design variable, not derived from other geometry

Watch out for: If the base solid is later redesigned and its thickness changes, Dimension does not auto-adapt — you must update the length manually.

To last¶

The pad grows until it hits the geometrically last face of the Body in the extrusion direction. Think of filling a box right to the brim: however tall the box is, the pad always reaches the top.

Use this mode when: - A boss or rib should always span the full depth of the solid, even as that depth changes parametrically - You want the pad to self-adjust when the base part is redesigned

Watch out for: "Last" means the farthest face the extrusion axis crosses in the Body. In a model with internal voids or disconnected regions the result can be surprising — use Up to face if you need to pick a specific face.

To first¶

The pad stops at the first face it encounters in the extrusion direction. Like filling a box only up to an inner shelf — it stops the moment it hits something.

Use this mode when: - You need the pad to stop at the nearest internal boundary - A wall or floor already exists at the correct depth and you want the pad to end flush with it

Watch out for: "First" is evaluated across the entire Body, not just the nearest visible face in the viewport. Use Up to face if you need to target a specific face rather than whichever happens to be closest.

Up to face¶

You select a specific named face; the pad grows exactly to that face and follows its shape, even if the face is curved or angled. Like pressing clay against a mould — the top surface of the pad adopts the mould's shape.

Use this mode when: - The termination surface is curved or angled (not flat and perpendicular) - You need the pad top to track a named face parametrically as the model changes - Multiple faces exist along the extrusion axis and you must pick exactly one

Watch out for: The selected face must actually intersect the extrusion volume. If the face never crosses the pad's path — e.g. it is parallel to the extrusion direction — FreeCAD will report "Feature could not be computed".

Up to shape¶

Like Up to face but you can select multiple individual faces or an entire solid as the boundary. The pad stops at the nearest point of any selected surface.

Use this mode when: - The termination boundary spans more than one face - Stopping at the outer hull of an imported STEP body - Combining with a negative Offset to face to recess the pad slightly inside the boundary

Watch out for: Over-selecting faces can produce ambiguous results. Start with the minimum set that completely covers the intended stopping boundary.

Reversed and Direction¶

Parameter	Type	Default	Description
Reversed	Checkbox	Off	Flips the extrusion direction. For One side mode this pushes the pad to the opposite side of the sketch plane. Has no effect in Symmetric mode.
Direction/edge	Dropdown	Sketch normal	Sets the extrusion axis. `Sketch normal`: uses the sketch plane's perpendicular. `Select reference…`: pick an edge or axis from the model tree. `Custom direction`: activates the X/Y/Z vector fields.
Length along sketch normal	Checkbox	On	When using a custom direction, controls whether the Length value measures along the sketch normal or along the custom direction vector.
X / Y / Z	Float	(0, 0, 1)	Components of the custom direction vector. Active only when Direction/edge is Custom direction.

Direction/edge in depth¶

By default, Pad extrudes perpendicular to the sketch plane. The Direction/edge dropdown lets you override that axis to extrude at any angle.

Sketch normal (default)¶

Extrudes straight out of the sketch plane — perpendicular to the surface the sketch is drawn on. Think of pressing a stamp directly away from the paper.

Use this mode when: - A boss, plate, or rib should grow perpendicularly out of its sketch (the overwhelming majority of pads) - You want the simplest, most predictable behaviour

Watch out for: Nothing — this is the safe default. Only change if you genuinely need an oblique extrusion.

Select reference¶

You pick an existing straight edge, datum line, or origin axis from the model and use its direction as the extrusion axis.

Use this mode when: - The pad must run parallel to an existing model edge (e.g. a diagonal rib that follows the slope of a nearby face) - You set up a datum line specifically to define a reusable direction

Watch out for: If the referenced edge is deleted or renamed in a later edit, the Pad fails. A dedicated Datum Line is more robust than picking a raw model edge.

Custom direction¶

You enter X/Y/Z components to define an arbitrary extrusion vector that is independent of any model geometry.

Use this mode when: - The extrusion angle is defined analytically (e.g. exactly 30° from vertical) - No existing edge in the model has the correct orientation - The direction must not change if other geometry is later redesigned

Watch out for: The Length along sketch normal checkbox controls what "Length" measures. Checked: length is the perpendicular height (constant wall thickness regardless of angle — usually what you want). Unchecked: length is measured along the custom vector (the pad grows that many mm in the vector's direction, so the perpendicular height varies with the angle).

Advanced usage¶

Symmetric mode and taper¶

When Mode is Symmetric and a non-zero Taper angle is set, FreeCAD creates two separate extrusion prisms — one in each direction — and fuses them. Each prism tapers from the sketch plane outward, so the draft originates correctly at the sketch and expands (or contracts) symmetrically on both sides.

Without a taper angle, the symmetric extrusion is built as a single prism extending from −L/2 to +L/2 along the sketch normal.

Up to shape vs. Up to face¶

Up to face targets a single named face. If the face moves parametrically (e.g. it is the top face of another Pad whose length is changing), the Pad automatically updates to track it.

Up to shape is more flexible: you select an entire solid or choose several individual faces. The pad stops at the nearest point on any of the selected faces. This is useful when the termination boundary is an irregular or multi-face surface that cannot be represented as a single flat face.

Custom direction for oblique pads¶

Setting a custom direction allows pads that are not perpendicular to their sketch plane. This is useful for angled ribs or wedge features. Set Direction/edge to Custom direction, enter a direction vector, and decide whether the Length measures along the sketch normal (perpendicular height) or along the actual extrusion vector. For most machined parts, measuring along the sketch normal gives the most intuitive parametric behaviour.

Combining Two sides with different types¶

In Two sides mode, Side 1 and Side 2 can have completely different types — for example, Side 1 as Dimension (a fixed depth for a boss) and Side 2 as To last (filling up to the opposite wall). This avoids needing a separate Pocket to trim the other direction.

Common mistakes and pitfalls¶

Sketch is not closed

Cause: The profile sketch has an open wire — a gap between two endpoints or an open arc — so FreeCAD cannot form a solid face.
Fix: Open the sketch, close every open wire (add a line or arc to fill the gap), and confirm that the Sketcher status bar reports zero open edges before closing.

Pad with zero total length

Cause: In Dimension mode, the sum of Side 1 and Side 2 lengths is zero (for example, +5 mm on Side 1 and −5 mm on Side 2).
Fix: Ensure at least one side has a non-zero length, or change the mode.

Direction is orthogonal to the sketch normal

Cause: A custom direction vector was entered that lies flat in the sketch plane. The extrusion cannot have any height in the normal direction.
Fix: Choose a direction vector that has a non-zero component along the sketch's normal axis.

Up to face / Up to last produces unexpected result

Cause: The target face is on the wrong side of the sketch plane, or the extrusion axis does not intersect any face in the correct direction.
Fix: Toggle Reversed to flip the extrusion direction so it points toward the intended termination face.

Taper angle causes invalid geometry

Cause: The taper angle is large enough that the extruded walls converge before reaching the specified length, creating a zero-area tip or a self-intersecting solid.
Fix: Reduce the taper angle, shorten the extrusion length, or scale up the profile.

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

# Draw a 20×10 mm rectangle centred at the origin
sketch.addGeometry(Part.LineSegment(App.Vector(-10, -5, 0), App.Vector(10, -5, 0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(10, -5, 0), App.Vector(10, 5, 0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(10, 5, 0), App.Vector(-10, 5, 0)), False)
sketch.addGeometry(Part.LineSegment(App.Vector(-10, 5, 0), App.Vector(-10, -5, 0)), False)
# Add coincident constraints to close the rectangle  # TODO: verify full constraint set
sketch.addConstraint(Sketcher.Constraint("Coincident", 0, 2, 1, 1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 1, 2, 2, 1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 2, 2, 3, 1))
sketch.addConstraint(Sketcher.Constraint("Coincident", 3, 2, 0, 1))
doc.recompute()

# Create the Pad
pad = doc.addObject("PartDesign::Pad", "Pad")
body.addObject(pad)
pad.Profile = sketch
pad.Length = 15.0          # 15 mm extrusion
doc.recompute()

print(f"Volume: {pad.Shape.Volume:.1f} mm³")
# Expected: 20 × 10 × 15 = 3000.0 mm³

Key properties¶

Properties are organised into property groups. Side1 and Side2 groups hold per-direction settings; Pad holds shared settings.

Property	Type	Default	Description
`Profile`	`App::PropertyLinkSub`	—	The sketch or face used as the extrusion profile. Inherited from `ProfileBased`.
`SideType`	`App::PropertyEnumeration`	`"One side"`	Overall mode. Values: `"One side"`, `"Two sides"`, `"Symmetric"`.
`Type`	`App::PropertyEnumeration`	`"Length"`	Extrusion type for Side 1. Values: `"Length"`, `"UpToLast"`, `"UpToFirst"`, `"UpToFace"`, `"UpToShape"`.
`Type2`	`App::PropertyEnumeration`	`"Length"`	Extrusion type for Side 2 (used when `SideType` is `"Two sides"`). Same values as `Type`.
`Length`	`App::PropertyLength`	`10.0`	Extrusion length for Side 1 in mm. Accepts negative values.
`Length2`	`App::PropertyLength`	`10.0`	Extrusion length for Side 2 in mm.
`TaperAngle`	`App::PropertyAngle`	`0.0`	Draft angle for Side 1 in degrees. Range: just under ±90°.
`TaperAngle2`	`App::PropertyAngle`	`0.0`	Draft angle for Side 2 in degrees.
`UpToFace`	`App::PropertyLinkSub`	—	Target face for Side 1 when `Type` is `"UpToFace"`.
`UpToFace2`	`App::PropertyLinkSub`	—	Target face for Side 2 when `Type2` is `"UpToFace"`.
`UpToShape`	`App::PropertyLinkSubList`	—	Target shape/faces for Side 1 when `Type` is `"UpToShape"`.
`UpToShape2`	`App::PropertyLinkSubList`	—	Target shape/faces for Side 2 when `Type2` is `"UpToShape"`.
`Offset`	`App::PropertyLength`	`0.0`	Signed offset from the termination face for Side 1.
`Offset2`	`App::PropertyLength`	`0.0`	Signed offset from the termination face for Side 2.
`Reversed`	`App::PropertyBool`	`False`	When `True`, reverses the extrusion direction.
`UseCustomVector`	`App::PropertyBool`	`False`	When `True`, uses the `Direction` vector instead of the sketch normal.
`Direction`	`App::PropertyVector`	`(1, 1, 1)`	Custom extrusion direction vector. Normalised internally. Active only when `UseCustomVector` is `True`.
`ReferenceAxis`	`App::PropertyLinkSub`	—	Reference edge or axis to derive the extrusion direction from.
`AlongSketchNormal`	`App::PropertyBool`	`True`	When `True` and a custom direction is set, `Length` is measured along the sketch normal rather than along the custom vector.
`Midplane`	`App::PropertyBool`	`False`	Deprecated since FreeCAD 1.1. Use `SideType = "Symmetric"` instead. Setting this property emits a deprecation warning.

TwoLengths type is deprecated

The "?TwoLengths" value is present in the internal enum for file compatibility only (it was replaced by SideType = "Two sides" in FreeCAD 1.1 — see PR #21794). Do not set Type to "TwoLengths" in new scripts; use SideType = "Two sides" with separate Length and Length2 values.