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Slider Crank Mechanism Design

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Dr. Sam Macharia's avatar Sila Mulwa's avatar
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Master parametric CAD design by creating a complete slider crank mechanism, one of engineering’s most fundamental motion conversion mechanisms. Learn FreeCAD from scratch through real-world mechanical design. #FreeCAD #SliderCrank #ReciprocatingMotion #KinematicDesign

🎯 Learning Objectives

By the end of this lesson, you will be able to:

  1. Navigate the FreeCAD interface and understand workbenches
  2. Create fully constrained 2D sketches with geometric and dimensional constraints
  3. Build parametric 3D parts controlled by spreadsheet parameters
  4. Assemble multi-part mechanisms with motion constraints
  5. Generate professional technical drawings for documentation

🔧 Engineering Context: Why This Mechanism Matters

Slider Crank Mechanism

The slider crank mechanism is one of the most fundamental and widely used motion conversion mechanisms in mechanical engineering. It converts continuous rotational motion into reciprocating linear motion (or vice versa), powering everything from internal combustion engines to reciprocating compressors and pumps.

Real-World Applications

The slider crank appears everywhere in engineering:

The Engineering Problem

Design Challenge: Given a rotating crankshaft, how do we create linear reciprocating motion with controlled stroke length and predictable motion characteristics?

📚 Mechanism Fundamentals

Components and Motion

A slider crank consists of four elements working together:

1. Crank (Link 2)

  • Rotates about fixed pivot (crankshaft)
  • Radius r determines stroke length

2. Connecting Rod (Link 3)

  • Transmits motion between crank and slider
  • Length l affects motion profile

3. Slider (Link 4)

  • Moves linearly along fixed path
  • Provides reciprocating output

4. Frame (Link 1)

  • Fixed reference
  • Provides pivot and guide

🎯 What You’ll Build

By completing this lesson, you’ll create:

Parametric Parts

Four fully constrained parts controlled by spreadsheet parameters

Working Assembly

Complete mechanism with motion constraints that actually moves

Technical Drawing

Professional engineering drawing suitable for manufacturing

Parameter Control

Change two values, entire mechanism updates automatically

🚀 Part 1: Getting Started with FreeCAD

Installing FreeCAD

  1. Download FreeCAD 0.21 or later

    Visit www.freecad.org

    Free & Open Source Cross-Platform

  2. Install and launch

    Follow the installer for your operating system

  3. Verify installation

    You should see the Start Page with recent files and examples

Understanding the Interface

When you first open FreeCAD, you’ll see four key areas:

Top toolbar

  • Workbench selector (dropdown)
  • Common tools and commands

Left sidebar (Model Tree)

  • Shows all objects in your document
  • Hierarchical organization
  • Click to select, double-click to edit

Center (3D Viewport)

  • Where you see and interact with your model
  • Navigate in 3D space
  • Primary design area

Bottom (Report View)

  • Console messages
  • Python console access
  • Error reporting

💡 Part 2: Parametric Design Strategy

Unlike direct modeling where you just “draw shapes,” parametric design means defining design intent through relationships, controlling geometry with parameters, and ensuring changes propagate correctly throughout your model. This is how professionals design—build it once, change it instantly.

Our Design Approach

🎯 Two-Parameter Control Philosophy

We’ll control the entire slider crank mechanism with just two parameters:

CrankRadius = 30 mm RodLength = 100 mm

Change these two values → entire mechanism updates automatically!

This is the power of parametric design.

Design Workflow

  1. Create Spreadsheet - Parameter table

  2. Create Crank - Part 1

  3. Create Connecting Rod - Part 2

  4. Create Slider - Part 3

  5. Create Frame - Part 4

  6. Assemble with constraints

  7. Create technical drawing

  8. Test parametric control

📊 Part 3: Creating the Parameter Spreadsheet

Building Your Parameter Table

  1. Create a new document

    File → New (or Ctrl+N)

    Save it as SliderCrank.FCStd

  2. Switch to Part Design workbench

    Use the workbench dropdown at top

  3. Insert a spreadsheet

    Insert → Spreadsheet

    A “Spreadsheet” object appears in the left tree

  4. Double-click to open the spreadsheet

    Click on “Spreadsheet” in the tree

Entering Parameters

In the spreadsheet, create this table:

CellValueMeaning
A1ParameterHeader
B1ValueHeader
C1UnitHeader
A2CrankRadiusParameter name
B230Numeric value
C2mmUnit (documentation)
A3RodLengthParameter name
B3100Numeric value
C3mmUnit

Close the spreadsheet when done (click the Close button).

Your parameter foundation is ready!

🔩 Part 4: Creating the Crank

Design Intent

⚙️ Crank Requirements

The crank is a rotating disc with:

  • Central hole for the fixed pivot (shaft)
  • Offset hole for the connecting rod pin
  • Parametric control - radius driven by Spreadsheet.CrankRadius

Step-by-Step: Crank Part

  1. Create a Body

    • Ensure you’re in Part Design workbench
    • Click Create Body button (or Body → Create body)
    • A “Body” object appears in the tree
    • Right-click → Rename → type Crank

  2. Create a Sketch

    • Select the “Crank” body in tree
    • Click Create Sketch button
    • Dialog asks: Choose a plane
    • Select XY_Plane
    • Click OK

    You’re now in Sketcher workbench (automatic switch)

Understanding the Sketcher

The Sketcher is where you create 2D profiles that become 3D parts.

Key Concept: Constraints

A sketch is “fully constrained” when every dimension is defined—zero degrees of freedom (DOF). This is the goal!

Why full constraints matter:

  • ✅ Predictable behavior when parameters change
  • ✅ No unexpected movement or sizing
  • ✅ Professional parametric design

Drawing the Crank Profile

  1. Draw the outer circle

    • Click Circle tool (or press C)
    • Click at the origin (look for white/yellow dot at center)
    • Move mouse outward and click to complete circle
    • Press Escape

  2. Draw the shaft hole

    • Circle tool again
    • Click at origin
    • Draw a smaller circle inside
    • Press Escape

  3. Draw the rod pin hole

    • Circle tool again
    • Click somewhere to the right of center
    • Draw a small circle
    • Press Escape

    You now have 3 circles, but they’re not constrained properly yet!

Adding Geometric Constraints

Make shaft hole concentric with origin:

  1. Click Coincident constraint tool
  2. Click the center of the inner small circle
  3. Click the origin point
  4. Press Escape

The shaft hole is now locked to the center!

Adding Dimensions (The Parametric Part!)

  1. Click Radius constraint tool
  2. Click the outer circle
  3. Dimension appears - type: 40
  4. Press Enter

Crank disk is now 40mm radius.

Finalizing the Sketch

  1. Check the solver

    Look at “Solver Messages” panel (left side):

    • Should say “Fully constrained”
    • If it says “X degrees of freedom”, you’re missing constraints

  2. Close the sketch

    Click the Close button in the toolbar

    The sketch is now a 2D profile visible in the 3D view

Creating 3D: Pad Operation

📦 Pad Operation

Pad extrudes a 2D sketch into a 3D solid by adding thickness perpendicular to the sketch plane.

Think: “Push the sketch upward to create volume”

🔗 Part 5: Creating the Connecting Rod

Design Intent

The connecting rod is a rectangular plate with circular holes at each end for pins.

🔧 Rod Requirements

  • Parametric length - Controlled by Spreadsheet.RodLength
  • Holes at both ends - For crank pin and slider pin
  • Rectangular body - Structural beam between holes

Creating the Rod

  1. Create new Body

    • Part Design workbench
    • Create Body
    • Rename: ConnectingRod

  2. Create Sketch

    • Select ConnectingRod body
    • Create Sketch → XY_Plane

Drawing the Rod Profile

Draw a reference line:

  1. Line tool (press L)

  2. Click at origin (0, 0)

  3. Move horizontally to the right

  4. Click to place endpoint

  5. Press Escape

  6. Select the line

  7. Make it horizontal: Press H key

  8. Dimension the length:

    • Distance constraint
    • Click both endpoints
    • Click ƒx button
    • Type: Spreadsheet.RodLength
    • Enter

Line is now 100mm long and parametric!

📦 Part 6: Creating the Slider

Design Intent

The slider is a block that moves linearly, with a hole for the connecting rod pin.

Quick Creation Steps

  1. Body: Create and rename to Slider

  2. Sketch on XY_Plane:

    • Rectangle: Draw centered at origin

    • Symmetric constraints: Center about X and Y axes

    • Dimensions: Width = 40 mm, Height = 30 mm

    • Circle: At origin for pin hole

    • Coincident: Circle center to origin

    • Radius: 6 mm

  3. Check: Fully constrained

  4. Pad: Length = 20 mm

Slider complete!

🏗️ Part 7: Creating the Frame

Design Intent

The frame provides:

  • Pivot mount for the crank
  • Linear guide for the slider

Creating the Frame

  1. Body: Frame

  2. Sketch on XY_Plane:

    • Rectangle below origin: 160mm × 20mm
    • Circle at origin: radius = 8 mm (crank pivot)
    • Optional: Add slider guide features (rails)

  3. Pad: 15 mm

Frame complete!

All four parts are now ready for assembly!

🧩 Part 8: Assembly

Assembly is where your individual parts come together as a functioning mechanism. FreeCAD’s Assembly workbench uses constraints to define how parts relate to each other, allowing you to test motion and verify your design before manufacturing.

Assembly Strategy

🎯 Assembly Constraints Plan

  1. Frame: Fixed (ground link)
  2. Crank: Rotates about fixed pivot at origin
  3. Connecting Rod: Pivots on crank pin and slider pin
  4. Slider: Constrained to linear horizontal motion

Creating the Assembly

  1. Switch to Assembly workbench

    Use workbench dropdown

  2. Create new assembly

    Assembly → Create Assembly

  3. Add parts

    Drag parts from tree or use “Add Part” button:

    • Frame
    • Crank
    • ConnectingRod
    • Slider

📐 Part 9: Technical Drawing

Creating Professional Documentation

  1. Switch to TechDraw workbench

  2. Create a page:

    • Insert Page
    • Choose template: A4_Portrait

  3. Add views:

    • Insert View → Select Crank body
    • Position the view by dragging

  4. Add dimensions:

    • Use Dimension tools: Horizontal, Vertical, Radius
    • Click features to dimension them

  5. Title block:

    • Double-click text fields
    • Enter: Part name, material, scale, your name, date

  6. Export:

    • Right-click page → Export as PDF

You now have professional engineering documentation!

✅ Part 10: Testing Parametric Control

This is the moment of truth! A truly parametric model updates correctly when you change parameters. Let’s verify your design is intelligent and responsive.

Verification Tests

  1. Open Spreadsheet

    Double-click Spreadsheet in tree

  2. Change CrankRadius

    • Click cell B2
    • Type: 40
    • Press Enter

  3. Recompute

    Press Ctrl+R or click Recompute button

  4. Observe changes:

    • Crank pin moves outward!
    • Stroke increases to 80mm!
    • Rod adjusts!
    • Assembly updates!

✅ Success! Your model is parametric!

🎓 Learning Outcomes

Congratulations! By completing this lesson, you have:

✅ Navigated FreeCAD

Interface, workbenches, 3D navigation

✅ Created Constrained Sketches

Geometric and dimensional constraints

✅ Built Parametric Parts

Spreadsheet-driven design

✅ Assembled Mechanisms

Motion constraints and testing

✅ Generated Drawings

Professional documentation

✅ Tested Parametric Control

Verified intelligent updates

Most importantly: You’ve designed a complete, functional mechanism from scratch using professional parametric CAD methodology!

🔍 Design Verification Checklist

Use this checklist to verify your design:

🚀 Extension Challenges

Ready for more? Try these enhancements:

  1. Add fillets

    Use Fillet tool to round sharp edges (3mm radius)

  2. Change materials

    Assign different materials to parts (steel, aluminum)

  3. Add more parameters

    Control crank thickness, rod width, slider size via spreadsheet

❓ Common Issues and Solutions

“Sketch not fully constrained”

“Cannot pad sketch”

📚 Next Steps

In Lesson 2: Four-Bar Linkage Mechanism, you’ll explore:

Master Sketch Approach

Control multiple parts from one kinematic layout

Construction Geometry

Reference-only geometry for design intent

Grashof's Theorem

Link length relationships and motion types

External References

Parts referencing shared geometry

Each lesson builds on these fundamentals while introducing new mechanisms and CAD techniques!

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