## Overview CAD part design begins with creating 2D profiles (sketches) on reference planes, then transforming them into 3D solids using features such as extrusions and revolutions. The **Sketcher** environment is used to draw, constrain, and dimension 2D geometry. Once a sketch is complete, features like **Boss**, **Cut**, **Shell**, and **Convert Entities** are applied to build and refine the final 3D part. Mastery of both sketching and feature-based modelling is essential for parametric solid modelling. --- ## Key Concepts - **Fully Defined Sketch** – A sketch where every entity's size and position is locked by dimensions or relations; entities display in black - **Under Defined Sketch** – A sketch with missing constraints, allowing entities to be dragged freely; entities display in blue - **Geometric Relations** – Constraints (horizontal, vertical, tangent, etc.) that govern how sketch entities behave relative to each other - **Dimensions** – Precise numerical values controlling entity size and position - **Extrusion** – Extending a 2D profile along a linear path to create a 3D solid - **Revolution** – Rotating a 2D profile around a centerline axis to create a 3D solid - **Entity Conversion** – Projecting existing 3D geometry (edges or faces) onto a new sketch plane - **Shelling** – Hollowing out a solid body to produce a thin-walled structure --- ## Detailed Notes ### 1. The Sketching Workflow Creating a 3D part follows a standard sequence: 1. **Select a Plane** – Choose a default reference plane (front, top, or right) or a flat face on an existing part 2. **Enter Sketch Mode** – Activate the sketch environment via the command manager 3. **Draw Entities** – Use tools such as lines, rectangles, circles, and arcs 4. **Apply Relations** – Add constraints to define geometric behaviour (e.g., making two lines parallel) 5. **Add Dimensions** – Use the **Smart Dimension** tool to assign exact numerical values 6. **Exit Sketch** – Confirm changes via the confirmation corner to save and close the sketch --- ### 2. Sketch Entities #### Lines - **Standard Line** – Used for the actual part geometry - **Centerline** – A construction line used for mirroring, symmetry, or as a revolution axis; does not contribute to 3D feature geometry - **Inference Lines** – Temporary yellow dashed lines that appear automatically to assist alignment (e.g., vertical or horizontal snapping) #### Rectangles - **Corner Rectangle** – Defined by two diagonally opposite corners - **Center Rectangle** – Defined by a center point and one corner; automatically generates construction lines - **3-Point Corner Rectangle** – Defined by three points, allowing angled orientation - **Parallelogram** – Defined by three points where sides are not necessarily perpendicular #### Circles and Arcs - **Circle** – Defined by a center point and a radius - **Perimeter Circle** – Defined by three points lying on the circumference - **Centerpoint Arc** – Defined by a center, a start point, and an end point - **Tangent Arc** – Begins from an existing endpoint and automatically maintains tangency with the previous segment - **3-Point Arc** – Defined by two endpoints and a third point that sets the radius --- ### 3. Geometric Relations Relations reduce the number of dimensions needed by defining geometric behaviour between entities. - **Horizontal / Vertical** – Forces a line to be perfectly level or upright - **Coincident** – Pins a point to another point or to an entity - **Parallel / Perpendicular** – Constrains the angular relationship between two lines - **Tangent** – Ensures a smooth, continuous transition between a curve (circle or arc) and another entity - **Equal** – Forces two or more entities to share the same length or diameter --- ### 4. Dimensions The **Smart Dimension** tool is the primary dimensioning method. It auto-detects the type of measurement based on selection. - **Linear Dimensions** – Distance between two points or the length of a line - **Angular Dimensions** – Angle between two non-parallel lines - **Radial / Diametric Dimensions** – Size of circles and arcs - **Modifying Dimensions** – Double-clicking a dimension opens a modification dialogue where values can be typed directly, adjusted with a scroll input, or calculated with simple expressions (e.g., `10 + 5`) --- ### 5. Extruded Boss/Base The most common method for converting a 2D sketch into 3D geometry. - **Process** – Select a completed sketch → activate the extrude command → define depth and direction - **End Conditions:** - **Blind** – Extrudes to a user-specified numerical depth - **Mid-Plane** – Distributes the total depth equally on both sides of the sketch plane - **Up to Vertex / Surface** – Terminates the extrusion at a chosen reference point or face - **Editing** – Right-clicking the feature in the history tree allows real-time modification of depth or sketch dimensions --- ### 6. Revolved Boss/Base Used for creating axially symmetric parts (e.g., shafts, wheels, cylindrical containers). - **Requirements** – A 2D profile sketch and a **centerline** serving as the axis of revolution - **Execution:** 1. Sketch the cross-sectional profile and the centerline on the same plane 2. Activate the revolve command 3. Define the revolution angle (e.g., 360° for a full solid, 180° for a half-section) --- ### 7. Convert Entities A tool that streamlines sketching by reusing existing geometry. - **Functionality** – Projects edges, loops, or faces from an existing 3D feature onto the current active sketch plane - **Parametric Link** – Converted entities maintain an **"On Edge"** relation; if the parent geometry changes size or shape, the projected sketch updates automatically --- ### 8. Sketches on Faces - Sketches do not always require a default reference plane - **Any flat (planar) face** on a solid model can serve as a sketch plane - The software treats the selected face as an **infinite geometric plane**, so sketch geometry can extend beyond the physical boundaries of that face --- ### 9. Shell Feature Transforms a solid body into a hollow, thin-walled structure. - **Wall Thickness** – A uniform thickness is applied to all remaining faces - **Faces to Remove** – Selecting a face during the shell operation deletes that face, creating an opening - **Multi-Thickness** – Individual faces can be assigned different wall thicknesses from the default value --- ## Tables ### Comparison of Sketch Entity Types | Entity Type | Defined By | Typical Use | |---|---|---| | **Standard Line** | Two endpoints | Part geometry edges | | **Centerline** | Two endpoints (construction) | Symmetry axis, revolution axis | | **Corner Rectangle** | Two opposite corners | Rectangular profiles | | **Center Rectangle** | Center point + one corner | Symmetric rectangular profiles | | **Circle** | Center + radius | Holes, cylindrical features | | **Perimeter Circle** | Three circumference points | Circles through known points | | **Tangent Arc** | Existing endpoint + tangent direction | Smooth transitions between segments | ### Comparison of Boss Features | Feature | Primary Input | Typical Result | |---|---|---| | **Extrude** | 2D profile + linear depth | Prismatic shapes, blocks, pads | | **Revolve** | 2D profile + rotation axis | Cylinders, spheres, axially symmetric parts | ### Extrusion End Conditions | End Condition | Description | When to Use | |---|---|---| | **Blind** | Extrudes to a fixed numerical depth | Known, specific depth required | | **Mid-Plane** | Splits total depth equally on both sides of the sketch plane | Symmetric parts centred on the sketch plane | | **Up to Vertex** | Terminates at a selected point | Depth must match an existing reference point | | **Up to Surface** | Terminates at a selected face | Depth must match an existing face boundary | ### Geometric Relations Summary | Relation | Effect | |---|---| | **Horizontal** | Forces a line to be perfectly level | | **Vertical** | Forces a line to be perfectly upright | | **Coincident** | Locks a point onto another point or entity | | **Parallel** | Makes two lines run in the same direction | | **Perpendicular** | Makes two lines meet at 90° | | **Tangent** | Ensures smooth continuity between a curve and another entity | | **Equal** | Forces two entities to share the same length or diameter | --- ## Diagrams ### Process: Creating a Fully Defined Sketch ```mermaid flowchart TD A[Select a Reference Plane] --> B[Enter Sketch Mode] B --> C[Draw Rough Geometry] C --> D[Automatic Relations Applied] D --> E[Add Manual Geometric Relations] E --> F[Add Smart Dimensions] F --> G{All Entities Black?} G -- No --> E G -- Yes --> H[Sketch Fully Defined] H --> I[Exit Sketch] I --> J[Apply 3D Feature] ``` ### Process: Creating a Hollow Component ```mermaid flowchart TD A[Create 2D Sketch on Plane] --> B[Extrude Sketch into 3D Solid] B --> C[Select a Planar Face on the Solid] C --> D[Apply Shell Feature] D --> E[Define Wall Thickness] E --> F{Remove Any Faces?} F -- Yes --> G[Select Faces to Remove] G --> H[Hollow Component Complete] F -- No --> H ``` ### Concept Map: Sketch to 3D Feature Relationships ```mermaid flowchart LR A[2D Sketch] --> B[Extrude Boss] A --> C[Revolve Boss] A --> D[Other Features] B --> E[3D Solid Body] C --> E D --> E E --> F[Shell] E --> G[Cut Features] E --> H[Sketch on Face] H --> I[New 2D Sketch] I --> B I --> C ``` ### Entity Conversion Parametric Link ```mermaid flowchart TD A[Existing 3D Feature] --> B[Select Edge or Face] B --> C[Convert Entities Command] C --> D[Projected Sketch on New Plane] D --> E[On Edge Relation Maintained] E --> F[Parent Changes → Sketch Auto-Updates] ``` --- ## Key Terms Glossary | Term | Definition | |---|---| | **Origin** | The fixed (0,0,0) reference point of the coordinate system; used to anchor sketches | | **Inference** | Automatic snapping behaviour that suggests geometric relations while drawing | | **Construction Geometry** | Dashed lines used for layout and reference purposes; ignored during 3D feature creation | | **Feedback Cursor** | Icons appearing near the mouse pointer indicating which relation will be applied | | **Boss** | Any feature that adds material to a part | | **Cut** | Any feature that removes material from a part (opposite of Boss) | | **Planar Face** | A flat surface on a 3D model that can serve as a sketch plane | | **Feature Manager Tree** | The sidebar history list showing all sketches and features in the part, in order of creation | | **End Condition** | The rule that determines how far an extrusion extends (Blind, Mid-Plane, Up to Surface, etc.) | | **Centerline** | A construction line used as a mirror axis or revolution axis | | **On Edge Relation** | A parametric link created by Convert Entities that keeps a projected sketch aligned with its source geometry | --- ## Quick Revision - Always anchor at least one sketch point to the **Origin** to prevent the entire sketch from floating - **Blue entities** = under defined (can still be moved); **Black entities** = fully defined (locked) - Use **Centerlines** for symmetry operations and revolve features; they do not generate 3D geometry - The **Smart Dimension** tool automatically detects whether you are measuring a line, angle, or circle - **Geometric relations are often more efficient than dimensions** — use "Equal" instead of dimensioning multiple identical entities separately - **Extrude** adds depth linearly; **Revolve** adds depth rotationally around an axis - **Blind** end conditions require a manual depth value; **Mid-Plane** splits the depth symmetrically - Use **Convert Entities** to ensure new sketches remain parametrically aligned with existing geometry - **Shelling** is more efficient than manually sketching and cutting internal material - You can sketch on **any flat surface** of a 3D model, not just default reference planes - Right-clicking a feature in the history tree allows property editing without recreating the feature - Right-clicking while drawing provides shortcut menus for ending chains or switching tools