SolidWorks Sketch, Part Modeling, and Equation-Driven Design

SolidWorks · Part Modeling

Overview

Part modeling in SolidWorks follows a two-step "sketch → feature" structure. If the sketch is off, no amount of advanced feature work will fix it.

Conversely, on top of a properly constrained sketch you can model most mechanical parts with nothing more than the basic features: Extrude, Revolve, Sweep, and Loft.

This guide covers sketch-state management, the main feature commands, and how to carry design intent into the file itself by linking dimensions together with Equations and Global Variables.

1. Sketch State and Color Conventions

Sketch entities are color-coded to reflect their constraint and dimension state.

In practice, leaving a sketch blue is like planting a bomb that goes off later.

Color	Meaning	Action
Blue	Under Defined	Add relations/dimensions
Black	Fully Defined	The ideal finished state
Red	Over Defined	Remove conflicting relations
Pink	Not Solved	Redefine the relation
Yellow	Dangling	Reference entity lost — reattach or delete
Brown	Invalid Solution	Pick the opposite solution

Tip Every sketch should be finished in black (Fully Defined). Blue sketches get dragged around unintentionally and are the most common cause of rebuild errors.

2. Geometric Relations

The standard relation set is:

Horizontal / Vertical
Coincident (point-point, point-line)
Collinear (on the same line)
Perpendicular / Parallel
Tangent
Concentric
Equal (matching length or radius)
Midpoint
Merge (combine points)
Symmetric (mirrored about a centerline)
Fix — avoid where possible
Intersection / Coradial

Tip Add relations before dimensions. With enough relations in place, the number of dimensions naturally drops to the minimum.

Tip In the Display/Delete Relations dialog, set the filter to Dangling and you can isolate only the relations whose references are broken. An essential tool for repairing imported sketches.

Note The Fix relation effectively nails an entity to global coordinates, so it breaks easily when the origin moves or features are reordered. The rule is to define position with a combination of relations instead of Fix.

3. Using Smart Dimension

A single command that auto-detects linear / angular / radial / diameter dimensions.
Two points → linear, two lines → angle, a single circle → diameter.
Typing = in the Modify dialog enters formula mode → you can reference global variables or other dimensions.
Dragging the spin box next to the number reflects the value in real time, which is handy for verifying design intent.

Tip If you need dual mm/inch dimensioning on drawings, set primary/secondary units under Tools → Options → Document Properties → Dimensions → Dual Dimensions.

4. Sketch Helper Tools

Sketch Picture: Place a PDF capture or hand drawing on a plane and Auto Trace (Professional or higher) to turn the outline into a sketch automatically.
Convert Entities (recommended shortcut Ctrl+E): Project edges or sketches onto the current plane. Automatically applies the On Edge relation.
Offset Entities (recommended Ctrl+Shift+O): Offsets an entity by a set distance. Bidirectional, reversed, and Cap ends options.
Sketch Contour: Within a single sketch, pick individual closed regions for separate extrudes — don't overuse it, though, because it becomes hard to maintain.
3D Sketch: Essential for pipe routing, weldment paths, wire routes, and the like. Use Tab to cycle through XY/YZ/ZX planes.
Equation Driven Curve: Supports Explicit (y=f(x)) and Parametric (x=f(t), y=f(t)). Use it for curves defined by equations — involute gears, cycloids, etc.

Note If you want to remove the On Edge relation on an entity created with Convert Entities, delete only the relation and leave the entity itself alone. Deleting the entity makes downstream features lose their reference.

5. Extrude / Revolve / Sweep / Loft

5.1 Extrude

Boss/Base adds solid; Cut removes it.
End Condition: Blind / Through All / Up To Next / Up To Vertex / Surface / Body / Mid Plane / Offset From Surface.
Up To Next conveys design intent more accurately than Through All. Even when bodies are added later, it only passes through the intended extent.
Mid Plane extrudes symmetrically in both directions from the sketch plane. Essential for symmetric geometry.

5.2 Revolve

An axis of rotation plus a profile sketch. If the profile crosses the axis, you get a self-intersection error.
One-Direction / Two-Direction / Mid-Plane.
Drawing a Centerline alongside the profile lets the axis be picked up automatically.

5.3 Sweep

A profile plus a path. Adding a Guide Curve enables deformation along the path.
The Twist option creates threads and springs.
The path sketch must have a Pierce relation to the profile's center or endpoint.

5.4 Loft

Smoothly connects two or more profiles.
Supports Guide Curves, Centerline, and Start/End Constraints (Normal/Tangent).
If the profiles' Connectors are misaligned, the loft twists — drag the connectors to line them up.

5.5 Boundary Boss/Base

An advanced version of Loft. It drives the surface with curve networks in both directions and lets you specify Contact / Tangent / Curvature continuity.
Useful for Class-A surface-grade shapes → Detailed surfacing techniques: /cad-tips/solidworks/sheetmetal-weldments-surface

6. Fillet, Chamfer, Shell, Draft, Rib

6.1 Fillet

Four modes: Constant / Variable / Face / Full Round.
Apply large fillets first, then add smaller ones. The reverse doesn't let the large fillet fully absorb the smaller ones.
Apply fillets before Shell or Draft to get natural-looking interior fillets.
Overusing cosmetic fillets degrades graphics performance and breaks Shell.

6.2 Chamfer

Distance-Distance / Distance-Angle / Vertex / Offset Face.
The Partial Chamfer in 2019+ lets you chamfer only part of an edge.

6.3 Shell

Hollows out the interior to create walls of uniform thickness.
The Multi-thickness option lets you set a different thickness on specific faces.
Apply Cut-Extrude after Shell to get the actual hole geometry.
If a convex fillet radius is smaller than the wall thickness, Shell fails → increase the fillet radius or handle it as a Multi-thickness exception.

6.4 Draft

Essential for injection and cast tooling. Neutral Plane / Parting Line / Step Draft.
DraftXpert is available as an automated tool.
Recommended order: Draft → Fillet. The reverse order produces unnatural edges.

6.5 Rib

Thin reinforcing wall. Created from an open-profile sketch line.
Linear / Natural types; specify Draft angle and thickness direction.
Since a rib sketch is automatically extended to the outer edges, it is cleaner to define only positional constraints rather than forcing it to be fully defined.

7. Pattern and Mirror

Type	Purpose
Linear Pattern	1- or 2-direction, Up to Reference, Pattern Seed Only
Circular Pattern	Around an axis, Equal Spacing / Instances to Skip
Mirror	Symmetric copy across a plane. Keep Merge solids checked
Sketch Driven	Copies at sketch point locations
Curve Driven	Equally spaced along a curve
Table Driven	Based on an Excel coordinate table
Fill Pattern	Fills a designated area with a honeycomb/circular layout

Tip Checking Geometry Pattern skips feature recomputation and simply copies the body. This is 10–20× faster on bulk patterns of 100+ instances.

8. Reference Geometry and Specialty Features

Plane: Many creation methods — offset, angle, 3-point, perpendicular, tangent.
Axis: Two points / two planes / cylindrical face / point-plane perpendicular.
Point: Arc center, face center, intersection.
Coordinate System: Datum for Export/Import.
Combine: Multi-body Add/Subtract/Common.
Split: Slice a body with a plane/face, then Save Bodies to split into separate files.
Intersect: Create or remove an intersection region between bodies or faces.
Wrap: Emboss/Deboss/Scribe a sketch onto a 3D surface. Used for logos and grip patterns.
Thread: Choose between Cosmetic Thread and Real Geometry Thread. Cosmetic is enough if drawing representation is the goal. Real Geometry is resource-intensive.

Tip Turning on View → Hide/Show → Temporary Axes surfaces the automatic axes of cylindrical faces so you can use them directly as circular-pattern axes.

9. Equations and Global Variables — Formula-Driven Design

9.1 Global Variable

In the Modify dialog, type =variableName → click the "Create Global Variable" button.
The variable can then be referenced by any dimension.
Variable names accept letters, digits, and underscores only. Use meaningful names (HoleDiameter, PlateThickness).

9.2 The Equations Manager

Tools → Equations, or right-click the Equations node in the FeatureManager. Three tabs:

Global Variables: Define variables
Features: Feature suppression conditions
Equations: Relations between dimensions

Examples:

"D1@Sketch1" = "D2@Sketch1" * 2
"D1@Hole1" = "PlateThickness" * 1.5
"State@Rib1" = "PlateThickness" < 3 ? "Unsuppressed" : "Suppressed" — auto-activates the rib for thin plates.

9.3 Functions and Units

Supported functions: sin, cos, tan, asin, acos, atan, sqrt, log, log10, exp, abs, int, sgn, if, min, max, floor, ceil, mod.

Trig functions are in radians. Convert degrees with sin(45 * pi/180).
The pi constant is supported.
Unit conversion is manual: inch→mm is * 25.4.

9.4 Linking to an External Text File

When multiple parts share the same size, link the Global Variables from an external .txt file.

Tools → Equations → Link to External File. Change one dimension and every linked part updates.

Tip Custom Properties can also be populated by Equations. For example, $PRP@Description = "Plate " & "PlateThickness" & "mm" auto-generates the part description.

10. Sketch and Modeling Best Practices

Relations first, dimensions second. Minimum-constraint principle.
Tie at least one or two points to the origin (Coincident, Midpoint).
Break a complex sketch into several simple sketches.
Use Construction lines liberally to establish symmetry and centerline relations.
Fillets and chamfers belong to features, not sketches.
Build the tree in this order: big features first → detail → standard features (Hole Wizard) → Draft → Fillet → Shell → Cosmetic.
Declare key dimensions as Global Variables → change once, update everywhere.

Field Checklist

Every sketch is Fully Defined (black)
Fix relations used minimally
Key dimensions centrally managed via Global Variables
Fillets placed before Shell and Draft
Large fillets first, small fillets later
Convert Entities entities never deleted — only their relations adjusted
Geometry Pattern checked for patterns over 100 instances
Thread chosen as Cosmetic or Real Geometry based on purpose
Equations placed at the top of the FeatureManager for visibility