Assembly Structures, Subassemblies and Configurations

Overview

Managing complex 3D models requires robust organizational tools and advanced modeling techniques. This document covers universal principles for structuring parametric CAD assemblies using sub-components and folders, applying features at the assembly level to simulate real-world manufacturing processes, and leveraging advanced tools — including kinematic mechanisms (belts/chains), weld beads, multi-part hole operations, and smart components — to automate complex mechanical relationships and reduce repetitive work.

Key Concepts

• Sub-Assembly – A standalone assembly file nested within a higher-level master assembly, functioning as a single modular unit to simplify the main design tree.
• Assembly Feature – A geometric modification (cut, hole, fillet, chamfer) applied directly in the assembly environment rather than at the individual part level.
• Feature Scope – Settings that determine exactly which components within an assembly are affected by an assembly-level feature.
• Flexible Component – A state where a sub-assembly's internal degrees of freedom are permitted to function within the parent assembly.
• Kinematic Mechanisms (Belts/Chains) – Automated generation of paths and motion relationships between rotational components (pulleys, sprockets) without manual mathematical calculation.
• Weld Beads – Digital representations of physical welds used to seal gaps or join bodies, complete with industry-standard annotations.
• Multi-Part Features (Hole Series) – A single machining operation that propagates appropriate hole dimensions (clearance, tapped, counterbore) through an entire stack of assembly components.
• Smart Components – Reusable modular parts that package the primary component, its associated mounting hardware, and necessary machining features into a single deployable unit.

Assembly Structure and Organization

Creating Sub-Assemblies

• Key point: Sub-assemblies group related parts together (e.g., a motor assembly within a larger machine).
• They reduce visual clutter in the main design tree and improve software performance by treating the group as a single solved unit.
• They mirror physical manufacturing modules, reflecting how real products are built.

Flexible vs. Rigid Sub-Assemblies

• Key idea: By default, sub-assemblies behave rigidly — their internal parts cannot move relative to one another once placed in a parent assembly.
• Enabling flexible mode allows internal mechanisms (like a sliding piston or a hinge) to articulate within the top-level assembly.
• This is essential for testing kinematics and checking clearances.

Empty Sub-Assemblies

• Key idea: An empty sub-assembly acts as a structural placeholder.
• Primarily used in top-down design workflows, where the designer creates the assembly framework first and then builds or inserts individual parts into those designated spatial placeholders later.

Sub-Assemblies in Drawings

• Key point: Sub-assemblies uniquely impact 2D documentation and Bills of Materials (BOMs).
• A BOM can be set to:
  • Top-Level Only – Shows the sub-assembly as a single purchased/manufactured line item.
  • Indented – Expands the sub-assembly to show every individual component inside it.

Assembly Features

Creating Assembly Features

• Key point: Used for post-assembly manufacturing operations.
• If two plates are welded together and then match-drilled on the shop floor, the hole should be modeled as an Assembly Feature — modeling the hole in individual part files would imply the holes were drilled before assembly, violating the design intent.
• Generic examples: Match-drilling, post-weld machining, aligning pins through multiple stacked brackets.

Feature Scope and Propagation

• Key idea: The designer retains total control over what an assembly feature alters.
• When creating an assembly cut, the Feature Scope dictates whether the cut slices through all intersecting parts or only selected ones.
• Designers can choose to propagate the feature to the part file:
  • Propagated – The physical part file is permanently modified.
  • Not propagated – The part file remains completely intact; the cut only exists virtually within that specific assembly file.

Assembly Fillets and Chamfers

• Key point: Edge treatments applied across multiple distinct parts.
• Useful for creating weld preparations (V-grooves created by chamfering two adjoining parts) or removing sharp edges that only form once multiple parts are bolted together.

Belts and Chains

• Instead of manually calculating belt lengths and applying individual gear relationships to simulate motion, modern CAD systems automate this process.
• Path Generation – By selecting the cylindrical faces of pulleys or sprockets, the software automatically maps the tangent path and calculates the total belt length.
• Face Selection Order – The order in which faces are selected dictates the belt's path; direction can be flipped for crossed belt configurations.
• Nominal Adjustments – The driving diameter of any selected wheel can be manually overridden to simulate different pulley sizes without altering the underlying 3D model.
• Kinematic Engagement – Enabling the "engage belt" option applies dynamic relationships automatically; rotating one pulley will physically drive the rest of the system based on their relative diameters.
• Physical Part Creation – The software can use the generated 2D sketch path to automatically create a new, physical 3D belt part, allowing for thickness and extrusion definitions.

Weld Beads

• Weld beads are assembly-level features used to visually and structurally represent physical welding processes.
• Selection Methods – Faces can be selected manually or via automated "smart selection" tools by dragging the cursor along the intended joint gap.
• Sizing – The physical volume of the weld is controlled by defining a bead radius.
• Industry Annotation – The feature allows direct input of standardized weld symbols and annotations, ensuring accurate manufacturing drawings.
• Data Organization – Once created, weld beads are typically grouped into an isolated "Weld" directory within the assembly's feature tree for workspace organization.

Multi-Part Hole Series

• A multi-part hole feature intelligently cuts through a stack of assembly components, varying its internal geometry based on the component's position in the stack.
• Assembly-Level vs. Part-Level – Though created at the assembly level, the operation dynamically modifies the individual part files via external references.
• Configuration Control – If a part is used multiple times in an assembly, configurations must be used to prevent the hole from propagating to unintended instances.

Smart Components

• Smart components eliminate the repetitive work of placing identical cutouts and hardware every time a specific component is used.
• Component Packaging – A smart component is a primary "parent" file that contains structural features (extrude cuts) and "child" components (screws, nuts).
• Configurator Tables – These tables allow designers to map different sizes of the parent part to corresponding sizes of the child components (e.g., an 8mm cover automatically triggers 8mm screws and an 8mm cutout).
• Deployment – When dragged into a new assembly, the user activates the smart feature, selects a reference face, and the software automatically machines the required holes and populates the hardware.

Folder vs. Sub-Assembly Comparison

Hole Series Parameter Workflow

Diagrams

Feature Scope and Propagation Workflow

flowchart TD
    A[Create Assembly Cut/Feature] --> B{Scope: Apply to All?}
    B -- Yes --> C[Feature intersects all parts in its path]
    B -- No --> D[Manually select target components]
    C --> E{Propagate to Part Level?}
    D --> E
    E -- Yes --> F[Individual part files are permanently modified]
    E -- No --> G[Parts remain intact — modification exists ONLY in the assembly]

Assembly Structure Hierarchy

graph TD
    A[Master Assembly] --> B[Folder: Fasteners]
    A --> C[Sub-Assembly: Motor]
    B --> D[Bolt 1]
    B --> E[Nut 1]
    C --> F[Rotor Part]
    C --> G[Stator Part]

Smart Component Creation Process

flowchart TD
    A[Start: Build Master Assembly] --> B[Position Parent Component on a Reference Plate]
    B --> C[Create Necessary Machining Cuts]
    C --> D[Add Associated Hardware]
    D --> E[Activate Smart Component Tool]
    E --> F[Select Parent Component]
    E --> G[Select Associated Features and Hardware]
    G --> H[Generate Configurator Table for Sizing]
    H --> I[Save Parent Part for Future Reuse]

Belt/Chain Kinematic Workflow

flowchart TD
    A[Select Cylindrical Faces of Pulleys/Sprockets] --> B[Software Calculates Tangent Path and Belt Length]
    B --> C{Crossed Belt Needed?}
    C -- Yes --> D[Flip Direction on Selected Face]
    C -- No --> E[Standard Path Generated]
    D --> F[Override Nominal Diameters if Needed]
    E --> F
    F --> G{Enable Kinematic Engagement?}
    G -- Yes --> H[Rotating One Pulley Drives All Others]
    G -- No --> I[Static Belt Path Only]
    H --> J[Optionally Create Physical 3D Belt Part]
    I --> J

Key Terms

• Top-Down Design – A modeling approach where the assembly dictates the size and shape of individual parts, often starting with empty sub-assemblies or master layout sketches.
• Bottom-Up Design – A traditional approach where individual parts are completely modeled first and then brought together into an assembly.
• Feature Propagation – The act of pushing a change made at the parent assembly level down to the base component file level.
• Feature Scope – The parameters defining which bodies or components are subjected to a specific CAD operation.
• Rigid State – An assembly condition where all internal motion of a nested sub-assembly is locked.
• Kinematic Engagement – A simulated mechanical relationship where the movement of one body mathematically drives the movement of another.
• External Reference – A link created when a feature in a localized part file is driven by geometric data from a higher-level assembly file.
• End Condition – The parameter that dictates how and where a 3D extrusion or cut terminates (e.g., blind, through-all, up-to-surface).
• Smart Fastener – Assembly hardware (bolts, nuts, washers) that dynamically reads surrounding geometry to automatically adjust its length and diameter.
• Bill of Materials (BOM) – A structured list of all components required to build an assembly, configurable as top-level or indented.

Quick Revision

• Sub-assemblies group physical parts into modular units; folders simply clean up the visual design tree.
• Enable flexible mode on a sub-assembly to allow its internal moving parts to function in the main assembly.
• Empty sub-assemblies are structural tools for top-down design planning.
• Use Assembly Features to represent physical manufacturing steps that happen after parts are put together (match-drilling, post-weld grinding).
• Feature Scope allows you to exclude certain parts from being cut by an assembly feature.
• Propagating an assembly feature modifies the original part file; leaving it unchecked keeps the modification isolated to the assembly file only.
• Assembly fillets and chamfers are ideal for preparing weld joints across the seams of multiple combined components.
• Belts/Chains automate pulley relationships — calculate belt length instantly, select faces in sequence, enable "engage" for kinematic motion.
• Weld Beads are added via face selection, defined by bead radius, and allow input of manufacturing-standard weld symbols.
• Hole Series configures a start (counterbore), middle (clearance), and last (tapped) hole through stacked parts in one operation; edits automatically update referenced part files.
• Smart Components bundle a base part, mounting cuts, and hardware together; configurator tables link sizes of the main component to appropriate hardware sizes.

Overview

Assembly configurations allow multiple variations of an assembly model to be stored and managed within a single file. Each configuration can represent a different size, component arrangement, operational position, or suppression state — enabling efficient design exploration and documentation without duplicating files. Configurations work alongside display states, design tables, and performance tools to streamline complex assembly management.

Key Concepts

• Configuration – a distinct variation of an assembly (dimensions, mates, component states) saved within the same file
• Configuration Manager – the dedicated interface panel for creating, selecting, and managing configurations
• Active Configuration – the configuration currently displayed and editable in the modelling environment
• Display State – a visual-only setting (hide/show, transparency, colour) that can be linked to a configuration or managed independently
• Derived Configuration – a child configuration linked to a parent; parent changes cascade down, but child changes do not cascade up
• Design Table – a spreadsheet-based tool embedded in the model file that controls multiple configuration parameters simultaneously
• SpeedPak – a lightweight, simplified representation of an assembly configuration that loads only selected geometry into memory to improve performance

Creating Configurations Manually

1. Open the Configuration Manager tab.
2. Right-click the top-level assembly name.
3. Select Add Configuration.
4. Enter a configuration name and optional description.
5. Set Bill of Materials (BOM) options to control how the part number displays in a BOM.
6. Confirm with the green checkmark.
7. The new configuration becomes the active configuration.
8. Modify the assembly for this configuration (add/remove mates, suppress/unsuppress components, change dimensions).

Derived (Child) Configurations

• Created as a child linked to a parent configuration
• Parent → Child: changes to the parent propagate to the child
• Child → Parent: changes to the child do not propagate to the parent
• Useful for creating minor variations from a common baseline

Advanced Configuration Options

Advanced options in the Configuration Properties control how a configuration reacts when new elements are added while a different configuration is active.

• Suppress new features and mates – any feature or mate added in another active configuration is automatically suppressed in this configuration
• Hide new components – any component added in another active configuration is automatically hidden in this configuration
• Suppress new components – any component added in another active configuration is automatically suppressed in this configuration

These settings prevent unintended changes from bleeding across configurations during active modelling.

Mapping Part Configurations to Assembly Configurations

When a part file contains its own configurations, each assembly configuration can reference a specific part configuration.

1. Ensure the part file already has the required configurations defined.
2. Insert the part into the assembly.
3. Right-click the component in the FeatureManager Design Tree.
4. Select Component Properties.
5. In the Referenced configuration section, choose the part configuration to link to the current assembly configuration.
6. Use the Change properties in dropdown to specify scope:
   • This configuration
   • All configurations
   • Specify configurations

Design Tables

Design tables provide a spreadsheet interface for managing many configurations and parameters at once.

Creating a Design Table

1. Navigate to Insert → Tables → Design Table.
2. Choose a source:
   • Auto-create – extracts existing configurations and parameters automatically
   • Blank – starts with an empty spreadsheet
3. Select the dimensions, mates, or suppression states to control.
4. The spreadsheet opens inside the graphics area.

Design Table Structure

• Rows represent individual configurations
• Columns represent controllable parameters (dimensions, suppression states, part configurations)
• Suppression values: S = Suppressed, R = Resolved
• Part configuration reference syntax: $CONFIGURATION@ComponentName

Applying Changes

• Edit cell values to modify existing configurations
• Add new rows to create new configurations
• Click outside the spreadsheet to close it and rebuild the model

SpeedPak

SpeedPak creates a performance-optimised representation of an assembly configuration by loading only a subset of faces and bodies into memory. Remaining geometry appears as a visual "ghost" but cannot be selected for mating or dimensioning.

Creating a SpeedPak

1. Activate the target configuration.
2. Right-click the configuration name in the Configuration Manager → select Add SpeedPak.
3. In the PropertyManager, select the faces, bodies, or components that must remain selectable (e.g., mating faces for higher-level assemblies).
   • Use the Quick Include slider to auto-select geometry based on size or visibility.
4. Confirm with the green checkmark.
5. A SpeedPak configuration is created (indicated by a specialised icon).

Updating a SpeedPak

• If the original geometry changes, the SpeedPak must be manually refreshed.
• Right-click the SpeedPak configuration → select Update SpeedPak.

Configuration Management Methods Compared

Advanced Options Behaviour Matrix

Design Table Syntax Reference

Configuration Hierarchy

graph TD
    A[Assembly File] --> B[Configuration 1 - Default]
    A --> C[Configuration 2]
    A --> D[Configuration 3]
    B --> B1[Display State A]
    B --> B2[Display State B]
    C --> C1[Derived Config 2a]
    C --> C2[Derived Config 2b]
    D --> D1[SpeedPak of Config 3]

Manual Configuration Creation Workflow

flowchart TD
    A[Open Configuration Manager] --> B[Right-Click Assembly Name]
    B --> C[Select Add Configuration]
    C --> D[Enter Name and Description]
    D --> E[Set BOM Options]
    E --> F[Confirm]
    F --> G[New Config Becomes Active]
    G --> H[Modify Assembly for This Config]

Part-to-Assembly Configuration Mapping

flowchart TD
    A[Part File with Multiple Configs] --> B[Insert Part into Assembly]
    B --> C[Right-Click Component]
    C --> D[Open Component Properties]
    D --> E[Select Referenced Part Configuration]
    E --> F[Set Scope via Change Properties In Dropdown]
    F --> G[Mapping Applied]

SpeedPak Creation Workflow

flowchart TD
    A[Activate Target Configuration] --> B[Right-Click Config in Manager]
    B --> C[Select Add SpeedPak]
    C --> D[Select Faces / Bodies / Components to Include]
    D --> E[Optional: Use Quick Include Slider]
    E --> F[Confirm]
    F --> G[SpeedPak Created — Non-Included Geometry Becomes Ghost]

Design Table Workflow

flowchart TD
    A[Insert → Tables → Design Table] --> B[Choose Source: Auto-Create or Blank]
    B --> C[Select Parameters to Control]
    C --> D[Spreadsheet Opens in Graphics Area]
    D --> E[Edit Cells / Add Rows]
    E --> F[Click Outside to Close]
    F --> G[Model Rebuilds with Updated Configurations]

Key Terms

• Configuration – a saved variation of an assembly's state (geometry, mates, suppression) within a single file
• Configuration Manager – the interface panel for creating and switching between configurations
• Active Configuration – the configuration currently loaded and editable
• Display State – visual appearance settings (visibility, colour, transparency) that may or may not be linked to a configuration
• Derived Configuration – a child configuration that inherits from a parent configuration
• Design Table – an embedded spreadsheet that controls configuration parameters in bulk
• Suppression – disabling a feature, mate, or component so it is excluded from the model rebuild
• Resolved – the normal, active state of a feature, mate, or component (opposite of suppressed)
• SpeedPak – a lightweight configuration that loads only selected geometry for improved performance
• Quick Include – a SpeedPak tool that auto-selects geometry based on size or visibility thresholds
• Ghost Geometry – non-selectable visual representation of excluded bodies in a SpeedPak
• BOM (Bill of Materials) – a structured list of components in an assembly, often used in manufacturing documentation
• FeatureManager Design Tree – the hierarchical tree listing all features, components, and mates in a model

Quick Revision

• Configurations store multiple assembly variations (dimensions, mates, suppression states) in a single file
• Display states control visual appearance only and can be linked to or independent of configurations
• Derived configurations inherit from a parent; parent changes cascade down, child changes do not cascade up
• Advanced options determine whether new features, mates, or components are automatically suppressed or hidden in a configuration when added from a different active configuration
• Part configurations map to assembly configurations via Component Properties → Referenced Configuration
• Design tables use an embedded spreadsheet (rows = configs, columns = parameters) for bulk management
• Design table syntax: S = suppressed, R = resolved; $CONFIGURATION@ComponentName maps part configs
• SpeedPak creates a lightweight representation by loading only selected faces/bodies, improving performance in large assemblies
• SpeedPak geometry not explicitly included appears as a non-selectable visual ghost
• SpeedPaks must be manually updated when the underlying geometry changes