Flexible and Indented Geometry in 3D CAD

Overview

• The Flex feature is an advanced 3D modeling tool used to apply freeform deformations to solid bodies
• It enables four types of complex shape modifications — bending, twisting, tapering, and stretching — that are difficult or impossible to achieve with standard sketch-based features (extrusions, sweeps, lofts)
• It works on any solid body, whether natively modeled or imported from an external system

Key Concepts

• Bending – deflects a model around a designated axis by a specified angle
• Twisting – rotates geometry around a central longitudinal axis
• Tapering – scales geometry outward or inward from a central point along a defined vector
• Stretching – elongates or compresses a localized region over a specified distance
• Trim Planes – two boundary planes that isolate the region of the model affected by the deformation
• Triad – a local 3D coordinate system that controls the center, orientation, and direction of the deformation

Feature Constraints & Rules

• Single Operation Rule – only one deformation type (bend, twist, taper, or stretch) can be applied per feature instance
• Sequential Application – to combine multiple effects on a single part, apply the feature multiple times in sequence (e.g., taper first, then stretch)
• Universal Compatibility – the feature works on any solid body regardless of origin (native or imported geometry)

Core Elements

Trim Planes

• Two boundary planes (Plane 1 and Plane 2) that define the limits of deformation
• Only the geometry between the two planes is affected; regions outside remain rigid and undeformed
• Planes can be positioned by:
  • Dragging interactively
  • Entering exact distance values
  • Snapping to reference vertices on the model

The Triad (Local Coordinate System)

• Acts as the center and pivot of the flex operation
• Defines the orientation of trim planes and the operational axes
• Blue Axis (Trim Plane Axis):
  • Always perpendicular to the trim planes
  • Serves as the longitudinal direction for twisting and tapering
• Red Axis (Bend Axis):
  • The explicit pivot vector for bending operations
• Center Point:
  • Defines the physical center of the deformation effect

Executing Specific Operations

Bending

• Controlled by a Bend Angle parameter
• Geometry folds around the Red Axis
• To change bend direction, rotate the Triad so the Red Axis faces the desired pivot orientation

Twisting

• Controlled by a Twist Angle parameter
• Rotation is exclusively locked around the Blue Axis

Tapering

• Controlled by a Taper Factor (scalar multiplier)
  • Positive factor → expands geometry outward along the Blue Axis
  • Negative factor → shrinks/compresses geometry inward
• Operates along the Blue Axis

Stretching

• Controlled by a Stretch Distance parameter
• Effect is strictly isolated to geometry trapped between the two trim planes

Triad Manipulation Techniques

• Free Dragging – click and pull the center point or individual axes to reposition freely in 3D space
• Snapping – use rotation rings to lock to fixed increments (e.g., 90° or 180°)
• Align to Selection – force an axis to become perpendicular to a selected face, or parallel to a selected edge/line
• Move to Selection – snap the triad center to a specific vertex or reference point
• Align to Principle – automatically center the triad at the geometric centroid and align axes with the part's principal global axes

Geometry Output Types

• Analytical Geometry – standard mathematically pure shapes (cylinders, flat planes, cones)
• Hard Edges Toggle:
  • Enabled → software attempts to maintain analytical geometry (e.g., curved faces retain measurable, constant radii)
  • Disabled → geometry converts to smooth spline surfaces; original analytical faces permanently lose standard measurable properties (e.g., fixed diameter)
• Disabling hard edges creates smooth freeform transitions but destroys geometric purity

Flex Operation Comparison

Triad Components

Hard Edges Toggle Comparison

Diagrams

Flex Feature Workflow

flowchart TD
    A[Start Flex Feature] --> B[Select Target Solid Body]
    B --> C{Choose Deformation Type}
    C -->|Bend| D1[Set Bend Angle]
    C -->|Twist| D2[Set Twist Angle]
    C -->|Taper| D3[Set Taper Factor]
    C -->|Stretch| D4[Set Stretch Distance]
    D1 --> E[Position Trim Planes]
    D2 --> E
    D3 --> E
    D4 --> E
    E --> F[Align & Position Triad]
    F --> G[Configure Hard Edges Toggle]
    G --> H[Confirm & Generate Feature]

Axis–Operation Relationship Map

flowchart LR
    T[Triad] --> R[Red Axis]
    T --> B[Blue Axis]
    T --> CP[Center Point]
    R --> Bend[Bending Operation]
    B --> Twist[Twisting Operation]
    B --> Taper[Tapering Operation]
    CP --> Pos[Deformation Origin Point]

Triad Positioning Methods

flowchart TD
    TP[Triad Positioning] --> FD[Free Dragging]
    TP --> SN[Snapping to Increments]
    TP --> AS[Align to Selection]
    TP --> MS[Move to Selection]
    TP --> AP[Align to Principle Axes]
    AS --> F1[Perpendicular to Face]
    AS --> F2[Parallel to Edge]
    MS --> V[Snap to Vertex/Reference Point]
    AP --> GC[Auto-Centre at Geometric Centroid]

Key Terms

• Flex Feature – an advanced deformation tool enabling bending, twisting, tapering, and stretching of solid bodies
• Triad – a manipulatable 3D coordinate system used to position and orient the deformation centre and axes
• Trim Planes – virtual boundary planes isolating a specific region of the model for localised modification
• Bend Axis (Red Axis) – the explicit vector around which geometry is folded during bending
• Trim Plane Axis (Blue Axis) – the axis perpendicular to trim planes; governs twist and taper direction
• Taper Factor – a scalar multiplier dictating the intensity of expansion (positive) or contraction (negative)
• Stretch Distance – the specified length by which a region is elongated or compressed
• Analytical Geometry – mathematically pure standard shapes (planes, cylinders, cones) with measurable properties
• Spline Surfaces – smooth, interpolated freeform surfaces that lack fixed geometric measurements
• Hard Edges – a toggle controlling whether output retains analytical geometry or converts to smooth spline surfaces

Quick Revision

• The Flex feature provides four deformation modes: Bending, Twisting, Tapering, and Stretching
• Only one mode can be active per feature instance; combine effects by applying the feature multiple times sequentially
• Trim Planes act as boundary fences — only geometry between them deforms; everything outside stays rigid
• The Triad is the steering mechanism controlling the centre, orientation, and direction of the deformation
• Bending pivots around the Red Axis; Twisting and Tapering operate around the Blue Axis
• Taper Factor: positive expands, negative compresses
• Stretching is confined strictly to the region between trim planes
• The Triad can be repositioned via free dragging, snapping, align-to-selection, move-to-selection, or align-to-principle
• Disabling Hard Edges converts analytical geometry into smooth spline surfaces — creating freeform transitions but permanently losing measurable geometric properties
• The feature is universally compatible with both natively modelled and imported solid bodies

Overview

• The Indent Feature is a modeling tool that reshapes a solid body by pressing the geometry of a second intersecting body into it
• It creates precise pockets, deformations, or cuts based on the exact contours of a secondary shape
• Requires at least two distinct bodies in the workspace to function

Key Concepts

• Target Body – the primary solid body that will be modified or reshaped
• Tool Body – the secondary body (solid or surface) whose shape drives the indent or cut
• Clearance – an offset distance added between the tool body and the resulting indented surface to allow tolerance
• Thickness – the specified wall thickness of the indented geometry when forming a pocket
• Keep Selections – creates the indent pocket around the region of the tool body that was clicked
• Remove Selections – inverts the logic, forming the pocket on the opposite side of the clicked tool body region
• Cut Option – changes the operation from a deformation into a material removal (boolean-style slice)

Basic Indent Operation

• Prerequisites:
  • The workspace must contain at least two distinct bodies
  • When creating the Tool Body, the merge result (boolean add) option must be unchecked to keep bodies separate
• Accessing the tool:
  • If not on the standard toolbar, it is typically found under the top menu path: Insert > Features > Indent
• Selection logic:
  • Selecting a Tool Body Region defines two things simultaneously:
    1. Which body acts as the tool
    2. Which side/face of the tool body dictates the resulting shape
• Keep vs. Remove:
  • Keep – wraps the indent around the face you clicked
  • Remove – applies the indent to the opposite side of the face you clicked
• Direction control:
  • A reverse direction toggle determines whether the resulting geometry wraps larger than the tool body or offsets smaller

Handling Multiple Tool Bodies

• The Indent feature cannot be directly patterned
• Correct workflow:
  1. Create a pattern of the Tool Bodies first
  2. Apply the Indent feature to all patterned tool bodies at once
• Performance optimisation:
  • Selecting multiple tool bodies triggers real-time preview generation, which can cause lag
  • Select Tool Body regions first, then select the Target Body last so the system only calculates the complex preview once
• After completing the feature, hide the tool bodies to clearly inspect the resulting indents

Managing Multiple Tool Regions

• When the Target and Tool bodies intersect in complex ways (e.g., passing through a grid of ribs), the software divides the tool into multiple distinct regions
• Selective indenting: click specific regions individually to apply the indent only where needed
• Efficiency shortcut for selecting all regions:
  1. Select the single, unbroken face of the tool body from the opposite side (e.g., the top)
  2. Switch the setting to Remove Selections
  3. This inverts the logic, effectively keeping all regions on the other side with a single click

Surfaces and the Cut Option

• Valid body combinations:
  • Solid Target + Solid Tool → Allowed
  • Solid Target + Surface Tool → Allowed
  • Surface Target + Surface Tool → Not Allowed (at least one solid body is required)
• Cut option behaviour:
  • Changes the operation from deformation to material removal
  • When enabled, the Keep/Remove selections toggle disappears
  • Select a surface as the tool body, then choose which side of the solid target body to cut away
  • The surface acts as the slicing boundary
  • Clearance offsets can still be applied in Cut mode

Feature Options Reference

Valid Body Combinations

Indent Feature Workflow

flowchart TD
    A[Start Indent Feature] --> B[Ensure two separate bodies exist]
    B --> C[Select Target Body]
    C --> D[Select Tool Body Region]
    D --> E{Choose Selection Mode}
    E -->|Keep| F[Indent wraps around clicked face]
    E -->|Remove| G[Indent applied to opposite side]
    F --> H[Set Thickness and Clearance]
    G --> H
    H --> I[Toggle Direction if needed]
    I --> J[Confirm Feature]
    J --> K[Hide Tool Body to inspect result]

Multiple Tool Bodies Workflow

flowchart TD
    A[Need to repeat an indent pattern] --> B[Create Tool Body geometry]
    B --> C[Pattern the Tool Bodies first]
    C --> D[Select all Tool Body regions]
    D --> E[Select Target Body last]
    E --> F[Apply Indent Feature]
    F --> G[Hide Tool Bodies]

Cut Option Decision Flow

flowchart TD
    A[Enable Cut Option] --> B{Tool Body Type?}
    B -->|Surface| C[Select surface as slicing boundary]
    B -->|Solid| D[Select solid tool body]
    C --> E[Choose which side of target to remove]
    D --> E
    E --> F[Apply Clearance offset if needed]
    F --> G[Confirm Cut]

Key Terms

• Multi-body Part – a single file containing more than one contiguous solid or surface volume
• Feature Manager / Tree – the UI panel listing the chronological history of operations and bodies in a part
• Section View – a temporary visual slice of the model used to inspect internal geometries and clearances
• Boolean Operation – a set operation (add, subtract, intersect) combining two or more bodies
• Merge Result – a toggle that, when enabled, automatically combines a new body with an existing one into a single volume
• Patterning – duplicating a feature or body in a linear or circular array

Quick Revision

• The Indent feature reshapes a Target Body using the geometry of a Tool Body
• Always uncheck "merge results" when creating the tool body to maintain separate bodies
• The Indent feature cannot be patterned directly — pattern the tool bodies first, then apply Indent to all at once
• Keep selections forms the indent around the clicked face; Remove selections forms it on the opposite side
• To quickly select many intersecting sub-regions, select the opposite face and choose Remove
• Select Tool Body regions first and the Target Body last to minimise preview lag
• Valid combinations: Solid + Solid or Solid + Surface — never Surface + Surface
• The Cut option converts the indent into a boolean-style slice that removes material
• Clearance adds a tolerance gap between the tool shape and the resulting surface
• After completing the indent, hide tool bodies to clearly view results