CAD Lab (ME-605) Unit 2 Notes - RGPV

2.1 Advanced Sketching & Reference Geometry

2.1.1 Sketch Entities

Lines & Arcs: Standard creation tools. Use 3-point arc for greater control.
Splines: Curves defined by data points. Used for organic shapes. Fit point splines pass through points; control vertex splines are defined by a polygon.
Conics: Ellipses, parabolas, hyperbolas. Defined by major/minor axes or foci.

2.1.2 Sketch Relations/Constraints

Relations: Geometric rules (e.g., Parallel, Perpendicular, Concentric, Tangent, Coincident, Equal, Symmetric).
Fully Defined Sketch: All degrees of freedom are constrained. Sketch color changes to black (default). Under-defined = blue; Over-defined/conflict = yellow/red.
Conflict Resolution: Use Display/Delete Relations to find and remove conflicting or redundant relations.

2.1.3 Sketch Tools

Offset Entities: Creates parallel copies at a specified distance. Can offset as construction geometry.
Convert Entities: Projects edges, curves, or faces from existing geometry into the active sketch.
Trim/Extend: Remove or extend sketch entities to other entities or a boundary.
Mirror: Creates symmetric copies about a centerline. The centerline must be a construction line.

2.1.4 Reference Geometry

Planes: Primary (Front, Top, Right) and user-defined.
- Offset Plane: At a distance from an existing plane.
- Parallel Plane: Parallel to a face/plane at a distance.
- Tangent Plane: Tangent to a cylindrical/conical face at a point.
Axes: Created from cylindrical faces, lines, or two points.
Points: Can be reference points (on a face/edge/vertex) or intersection points.

2.1.5 3D Sketching

Applications: Creating sweep paths, loft guide curves, weldment layouts, routing (pipes, wires).
Tools: 3D sketch plane is implicit. Use 3D sketch points, 3D lines, 3D splines. Relations like Pierce (point on face) are critical.

[!TIP] Exam Focus: Be able to distinguish between construction geometry (light blue, for reference only) and solid geometry (black, contributes to feature). Know how to create an offset plane and a tangent plane.

2.2 Fundamental 3D Part Modeling - Feature-Based Approach

Feature Type	Primary Use	Key Parameters/Options
Extruded Boss/Base	Adds material by pulling a sketch perpendicular to its plane.	Direction (1/2), Depth (Blind/Through All/Up to Vertex/Up to Surface), Draft (taper), Thin Feature (thin-walled).
Extruded Cut	Removes material by cutting through or into a solid.	Same as Boss, plus "Flip side to cut" option.
Revolved Boss/Base	Adds material by rotating a sketch about an axis.	Axis (must be in sketch or reference), Angle (Full/Partial), Thin Feature.
Revolved Cut	Removes material by revolving a sketch profile about an axis.	Same as Revolved Boss.
Swept Boss/Base	Adds material by moving a profile along a path.	Profile (must be closed for solid), Path (must be tangent continuous), Guide Curves (control cross-section shape).
Lofted Boss/Base	Adds material by blending between multiple profiles.	Profiles (ordered), Centerline (optional, guides twist), Guide Curves (control shape).
Hole Wizard	Creates standard, industry-standard holes.	Hole Type (Counterbore, Countersink, Tap, Straight Tap), Standard (ISO, ANSI, etc.), Size, Fit, Depth, Boss/Countersink diameters.
Fillet/Chamfer	Adds rounds or bevels.	Constant/Variable radius, Face/Edge selection, Full Round fillet (replaces selected face).
Shell	Creates a thin-walled part by hollowing out and removing faces.	Wall Thickness, Faces to Exclude (openings).
Draft	Tapers faces to facilitate molding.	Draft Angle, Draft Direction (neutral plane/face), Parting Line selection.
Patterns	Duplicates features/faces/bodies.	Linear (direction & spacing), Circular (axis & spacing), Sketch-Driven (points in sketch), Table-Driven (from spreadsheet).
Mirror	Mirrors features or bodies.	Mirror Plane/Axis, Copy/Mirror option (keep original or not).

[!TIP] Exam Focus: Extruded Cut and Revolved Cut are inverse operations of their Boss counterparts. Hole Wizard is a specialized, intelligent feature—know its callout format (e.g., M8x1.25). Loft requires ordered profiles; use Centerline to control twist. Thin Feature option is available in Extrude/Revolve to create sheet-metal-like parts quickly.

2.3 Editing & Modifying Features

2.3.1 Feature Manager Tree

Reordering: Drag-and-drop feature to change build order (affects downstream features).
Suppressing: Temporarily removes feature from model (grayed out in tree). Useful for troubleshooting or creating configurations.
Rolling Back: Right-click a feature → Roll Back. Hides all subsequent features, allowing edits to that feature's sketch/definition.

2.3.2 Editing Sketches and Features

Edit Sketch: Double-click sketch in tree or on model. Modifies the 2D profile.
Edit Definition/Feature: Right-click feature → Edit Feature. Modifies parameters (depth, angle, etc.) without entering sketch.
Edit Sketch Plane: Change the plane a sketch is on via Sketch → Edit Sketch Plane.

2.3.3 Design Intent

Parameters/Equations: Link dimensions via D1@Sketch1, D2@Extrude1. Use = for equations (e.g., "D2" = 2*"D1").
Global Variables: User-defined variables (e.g., "Thickness") accessible across part/assembly. Created in Tools → Equations.
Purpose: Maintains relationships when model changes (e.g., hole diameter always 1/4 of part width).

2.3.4 Failure Diagnostics

Common error: "Could not create this feature".
Causes: Invalid sketch (open, self-intersecting), missing references, geometry too small/thin, topological errors.
Resolution: Use "What's Wrong" (yellow lightbulb), check sketch validity, roll back to find failing feature, ensure sufficient material exists for cut.

[!TIP] Exam Focus: Roll Back is the primary tool for editing early features. Equations (Tools > Equations) are the backbone of parametric design. Always check the "FeatureManager Design Tree" for error symbols (red/yellow).

2.4 Introduction to Bottom-Up Assembly Modeling

2.4.1 Assembly Environment

Interface: Assembly window, FeatureManager Assembly Tree (lists components/mates), Mates Toolbar.
Assembly Tree: Shows components and their mates (sub-tree under each component).

2.4.2 Inserting Components

Insert → Component → Existing Part/Assembly.
Initial Placement: First component is "Fixed" (grounded). Subsequent components are "Floating" until mated.
Component Properties: Set "Fix" (make fixed), "Suppress", "Lightweight" (for large assemblies).

2.4.3 Mating Fundamentals

Mate Type	Constraint	Typical Use
Standard Mates
Coincident	Two faces/planes/edges/points touch.	General positioning.
Concentric	Axes/cylindrical faces share centerline.	Shafts in holes, pins.
Parallel	Two faces/planes/axes are parallel.	Aligning blocks.
Perpendicular	Two faces/planes/axes are perpendicular.	90° joints.
Tangent	Curved face tangent to planar/curved face.	Ball in socket, shaft in V-block.
Distance	Sets a specific gap between two entities.	Spacing between plates.
Angle	Sets a specific angle between two entities.	Hinged connections.
Advanced Mates
Width	Centers a part between two parallel faces.	Centering a block in a slot.
Path	Constrains a point/vertex/edge to follow a path (edge/curve).	Piston rod following cylinder axis.
Profile Center	Centers a profile (sketch) on a path.	Cam follower on cam profile.
Symmetry	Mirrors components about a plane.	Symmetric placement of bolts.
Mechanical Mates
Hinge	Allows rotation about a single axis (like Concentric + Limit).	Door hinge.
Slot	Constrains a point to move within a slot (path + distance).	Slider in a slot.
Rack and Pinion	Translational motion of rack linked to rotational motion of pinion.	Steering mechanism.
Cam	Follows a cam profile with a follower.	Engine valve train.
Gear	Rotational motion of two gears with defined ratio.	Gearbox.

2.4.4 Assembly Visualization

Interference Detection: Tools → Interference Detection. Finds overlapping solid bodies.
Clearance Analysis: Tools → Clearance Verification. Checks for minimum gaps between components.
Collision Detection: Move Component → Collision tab. Checks for collisions during motion (with/without stop).

2.4.5 Sub-Assemblies

Create a separate .sldasm file for a logical group of parts.
Insert into top-level assembly as a single component.
Mates are defined within the sub-assembly and between sub-assembly and top-level.

[!TIP] Exam Focus: Coincident and Concentric are the most frequently used mates. Mechanical mates (Hinge, Slot, Gear) simulate real motion. Always check for "Over-defining" (red mate icon) which causes rigidity.

2.5 Component Manipulation & Analysis within Assemblies

2.5.1 Moving/Rotating Components

Drag: Click and drag a component (temporarily breaks mates).
Rotate Component: Move Component tool → Rotate mode (about a point/axis).
Move Component: Move Component tool → Translate mode (along axis/plane).

2.5.2 Dynamic Clearance

Use Move Component with Collision and Clearance options enabled.
Set "Stop at collision" and specify clearance value to find valid motion ranges.

2.5.3 Exploded Views

Tools → Exploded View.
Select components and drag them apart along a triad (XYZ axes).
Explode Steps: Create multi-stage explosions.
Save Exploded View: Saves view orientation and step state.
Animated Explode: Motion Manager (if available) or Tools → Motion Study to animate explosion/implosion.

2.5.4 Section Views in Assemblies

View Layout → Section View.
Assembly Section: Cuts through entire assembly along a plane.
Section with Cap: Cuts and removes one side, optionally capping the sectioned faces.

[!TIP] Exam Focus: Exploded views are for documentation; Dynamic Clearance is for design verification. Understand the difference between a static Section View and a dynamic Collision Detection.

2.6 Introduction to Drawing/Detailing from 3D Models

2.6.1 Creating Drawing Views

Standard 3-View: Front, Top, Right (orthographic).
Projected View: Projected from an existing view (e.g., auxiliary from front).
Auxiliary View: Shows features inclined to principal planes. Uses an auxiliary plane.
Section View: Full, half, offset, aligned. Defined by a section line.
Detail View: Enlarged view of a small area. Uses a broken-out circle.

2.6.2 Model-Based Definition (MBD) & 3D Annotations

Concept: Add dimensions, tolerances, notes, and PMI (Product Manufacturing Information) directly on the 3D model.
Tools: Dimension tool (3D), Tolerance tool (GD&T), Note tool.
Benefit: Reduces or eliminates 2D drawing dependency; supports digital manufacturing.

2.6.3 Automated View Creation

Model View tool: Select a face/plane in the 3D model → automatically creates a primary view (usually front) and allows projection of standard views.

2.6.4 View Manipulation

Align: Aligns a projected view to its parent.
Breaking Out: Creates a broken view (shows interior of long part).
Crop View: Creates a view from a portion of an existing view, with a crop boundary.

[!TIP] Exam Focus: Know the difference between an Auxiliary View (for inclined features) and a Detail View (for small features). MBD is the future of digital manufacturing but may not be in all curricula.

2.7 Basic Dimensioning & Annotation

2.7.1 Dimensioning Schemes

Scheme	Description	Use Case
Baseline	All dimensions originate from a common baseline (datum).	High precision, minimizes error accumulation.
Chain	Dimensions are placed end-to-end.	Simple parts, but error propagates.
Ordinate	Dimensions are taken from a common origin (0,0).	For parts with many similarly spaced features (e.g., hole patterns).

2.7.2 Smart Dimension Tool

Associative Dimensions: Linked to model geometry. Changes in model update drawing.
Driven Dimensions: Read-only dimensions derived from geometry (e.g., overall length from endpoints). Cannot be modified.

2.7.3 Geometric Tolerances (GD&T) - Basic Symbols

Frame: Rectangular box containing tolerance data.
Symbol: e.g., Ⓜ (Position), Ⓘ (Flatness), Ⓢ (Straightness), Ⓤ (Roundness/Cylindricity).
Tolerance: Value (e.g., 0.1).
Datum: Reference letter(s) (e.g., A, B, C).
Application: Select feature → Tolerance tool → choose symbol, enter value, assign datum.

2.7.4 Annotations

Notes: General text. Can have leader.
Surface Finish: Symbol with texture direction, roughness value.
Weld Symbols: Basic fillet weld (triangle) or groove weld (cross-section). Specify size, length, pitch.

2.7.5 Bill of Materials (BOM)

Automatic Generation: Insert → Tables → Bill of Materials. Populates from assembly tree.
Editing: Can add columns (Part Number, Description, Qty), edit cells.
Tabular Note: BOM table placed on drawing sheet.

[!TIP] Exam Focus: GD&T symbols are highly examinable. Know Position (Ⓜ) and Flatness (Ⓘ). Ordinate dimensioning is common for hole patterns. A BOM is assembly-specific, not part-specific.

2.8 File Management & Best Practices

2.8.1 File Structure

Part (.sldprt): Single solid body or multi-body part.
Assembly (.sldasm): Contains references to .sldprt and .sldasm (sub-assemblies) files.
Drawing (.slddrw): Contains references to .sldprt or .sldasm files.
Key Principle: Drawing and Assembly files do NOT contain geometry; they reference external part files.

2.8.2 Referencing & Path Management

"Where Used" (Right-click file in Windows Explorer or CAD software): Finds all assemblies/drawings using a part.
Pack and Go: File → Pack and Go. Collects a part/assembly and all its referenced files into a single folder or ZIP for transfer.

2.8.3 Design Tables & Configurations

Configurations: Different variations (size, feature suppression) within a single part file.
Design Table: Excel/CSV table embedded in part. Controls dimensions and feature suppression for each configuration.
Creation: Insert → Tables → Design Table. Link to Excel or create internally.

2.8.4 CAD Standards

Naming Conventions: Consistent part numbers (e.g., ASSY-001-01, PART-002-A).
Template Files (.prtdot, .asmdot, .drwdot): Pre-set with company standards (units, fonts, title blocks, layers).
Layers: (If used in software like AutoCAD or Fusion 360) Organize entities by function (e.g., 0, DIMENSIONS, CENTERLINES).

[!TIP] Exam Focus: "Broken references" are a common problem—always use Pack and Go to move projects. Configurations are essential for families of parts (e.g., bolts of different lengths). Understand the difference between a part file and its configurations.

2.9 Introduction to Advanced Topics (Survey Level)

2.9.1 Weldments

Structural Member: Creates welded frames from standard profiles (IPE, UB, etc.) along a 3D sketch path.
Weld Beads: Added as separate features between structural members.
Cut List: Automatically generates a table of all structural members with profile type, length, quantity.

2.9.2 Sheet Metal

Base Flange: Starting feature from a sketch, defines thickness and bend radius.
Edge Flange: Adds a flange to an existing edge. Controls angle, position, relief.
Gusset: Adds a triangular support between flanges.
Flat Pattern: Unfolds the sheet metal part into a 2D pattern for manufacturing. K-Factor determines bend allowance.

2.9.3 Mold Tools (Basic Workflow)

Parting Line: Defines the split between mold halves.
Shut-off Surfaces: Create surfaces to close holes/cavities.
Core/Cavity: Generates the two mold halves (tooling blocks) from the parted solid.

2.9.4 Surface Modeling Overview

Boundary Surface: Creates a surface bounded by 2, 3, or 4 curves/edges (like a loft).
Fill: Creates a surface patch within a closed boundary (can be planar or curved).
Trim Surface: Cuts a surface with another surface/sketch.
Knit: Combines multiple adjacent surfaces into a single surface or solid (if volume enclosed).

[!TIP] Exam Focus: Weldments produce a Cut List, not a BOM. Sheet Metal requires understanding of K-Factor (bend allowance calculation). Surface modeling is for complex, non-standard shapes that cannot be made with solid features.