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Pantograph Mechanism

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Dr. Sam Macharia's avatar Sila Mulwa's avatar
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Master parametric CAD design by creating a pantograph mechanism: an elegant linkage that scales motion through similar triangle geometry. Learn ratio-driven design and expression-based parametric control in FreeCAD. #FreeCAD #Pantograph #MotionScaling #SimilarTriangles

🎯 Learning Objectives

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

  1. Design mechanisms based on ratio relationships and similar triangle geometry
  2. Implement expressions to link multiple dimensions mathematically
  3. Create master sketch approach for coordinated multi-part design
  4. Control motion scaling with single parameter (scaling ratio k)
  5. Verify geometric relationships through parametric testing

🔧 Engineering Context: Why This Mechanism Matters

Pantograph Mechanism

A pantograph is an elegant mechanical linkage that scales motion through similar triangle geometry. It can enlarge, reduce, or exactly copy a path traced by one point as output at another point, with applications ranging from engraving to drafting tools.

Real-World Applications

The pantograph appears in diverse engineering applications:

The Engineering Problem

Design Challenge: Given a path traced by an input stylus or pointer, reproduce that path at a different scale while maintaining geometric similarity and smooth motion.

📚 Mechanism Fundamentals

Pantograph Principle

Core Geometric Principle:

A pantograph consists of four links forming a parallelogram-like structure with specific length ratios.

Key Setup:

  • One pivot is fixed (O)
  • Input point (I) traces a path
  • Output point (P) is positioned on an extension of link OI

Magic Relationship:

This ratio k is the scaling factor!

🎯 What You’ll Build

By completing this lesson, you’ll create:

Ratio-Driven Design

All dimensions controlled by scaling ratio k and base length

Expression-Based Parts

Automatic dimension calculation using spreadsheet formulas

Master Sketch

Single reference sketch controlling all link geometries

Scalable Mechanism

Change k value, entire pantograph 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. Create new document

    Launch FreeCAD File → New (Ctrl+N) Save as Pantograph.FCStd

  3. Switch to Part Design workbench

    Use workbench dropdown at top

Workbenches We’ll Use

Key Workbenches for This Lesson:

  • Part Design - Creating individual parametric parts
  • Sketcher - Creating 2D constraint-based sketches
  • Spreadsheet - Parameter tables with formulas
  • Assembly - Combining parts with constraints
  • TechDraw - Creating engineering drawings

💡 Part 2: Parametric Design Strategy

The pantograph is our first ratio-driven mechanism where geometric relationships are more complex. We’ll use a master sketch to define the kinematic layout, then reference it from all parts. This ensures geometric consistency and simplifies the parametric control to just two values: base length and scaling ratio.

Our Design Approach

🎯 Ratio-Based Control Philosophy

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

BaseLength = 100 mm ScalingRatio = 2

All other dimensions calculated automatically using expressions!

This is parametric design at its most powerful.

Design Workflow

Our Pantograph Configuration:

  • Fixed pivot O at origin
  • Scaling ratio (output is 2× input)
  • Input stylus at point I
  • Output tracer at point P

Link Naming:

  1. Base - Fixed ground (mounting plate)
  2. Link OA - From fixed pivot O to moving pivot A
  3. Link OB - From fixed pivot O to moving pivot B
  4. Link AB - Connecting moving pivots A and B
  5. Input Arm (OI) - From O through A to input point I
  6. Output Arm (OP) - From O through B to output point P

📊 Part 3: Creating the Parameter Spreadsheet

Building Your Parameter Table with Formulas

  1. Ensure you’re in Part Design workbench

    Use the workbench dropdown at top

  2. Insert a spreadsheet

    Insert → Spreadsheet

    A “Spreadsheet” object appears in the left tree

  3. Double-click to open the spreadsheet

    Click on “Spreadsheet” in the tree

Entering Parameters with Expressions

In the spreadsheet, create this table:

CellValueMeaning
A1ParameterHeader
B1ValueHeader
C1UnitHeader
D1Formula/NoteHeader
A2ScalingRatioParameter name
B22Numeric value (k)
C2ratioUnit
D2k (output/input)Note
A3BaseLengthParameter name
B3100Numeric value
C3mmUnit
D3Length OA = OBNote

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

Your expression-based parameter foundation is ready!

🎨 Part 4: Creating the Master Sketch

Design Intent

🗺️ Master Sketch Purpose

The master sketch defines the kinematic layout of the pantograph:

  • All critical points (O, A, B, I, P)
  • All link lengths with parametric control
  • Geometric relationships between components

Think of it as the “blueprint” that all parts will reference.

Step-by-Step: Master Sketch

  1. Create standalone sketch

    • Ensure you’re in Part Design workbench
    • Click Create Sketch (don’t create a Body first!)
    • Select XY_Plane
    • This sketch won’t belong to any body - it’s purely reference geometry

Drawing the Kinematic Layout

The center of rotation:

The origin (0, 0) is our fixed pivot point O.

No need to draw anything - the origin marker is already there!

  1. Close the sketch

    Click Close button in toolbar

  2. Rename for clarity

    • Find “Sketch” in the tree
    • Right-click → Rename → MasterSketch

Master sketch complete! This defines all key points for the entire mechanism.

🔩 Part 5: Creating Link OA

Design Intent

⚙️ Link OA Requirements

Link from fixed pivot O to moving pivot A:

  • Holes at O and A for pin joints
  • Rectangular body connecting the holes
  • References master sketch for exact positioning

  1. Create Body

    • Part Design workbench
    • Click Create Body button
    • Right-click → Rename → Link_OA

  2. Create Sketch

    • Select Link_OA body
    • Create Sketch → XY_Plane

  3. Reference master sketch points

    • Click External Geometry tool (or press E)
    • In the tree, find and select MasterSketch
    • Click on points O and A in the 3D view
    • They appear as purple reference points

  4. Draw the link profile

    • Circle at point O: Radius constraint → ƒx → Spreadsheet.PinRadius
    • Circle at point A: Radius constraint → ƒx → Spreadsheet.PinRadius
    • Rectangle connecting them, symmetric about the OA line
    • Width dimension: ƒx → Spreadsheet.LinkWidth

  5. Close sketch

  6. Pad the link

    • Select the sketch
    • Click Pad tool
    • Length: ƒx → Spreadsheet.LinkThickness
    • OK

Link OA complete!

🔗 Part 6: Creating Link OB

Same process as Link OA, but reference points O and B:

  1. Body: Create and rename to Link_OB

  2. Sketch on XY_Plane

  3. External Geometry:

    • Reference MasterSketch
    • Select points O and B

  4. Draw profile:

    • Circles at O and B (PinRadius)
    • Rectangle connecting them (LinkWidth)

  5. Pad: LinkThickness

Link OB complete!

📏 Part 7: Creating Link AB

The connecting link between moving pivots A and B:

  1. Body: Link_AB

  2. Sketch on XY_Plane

  3. External Geometry:

    • Reference MasterSketch
    • Select points A and B

  4. Draw profile:

    • Circles at A and B (PinRadius)
    • Rectangle body (LinkWidth)

  5. Pad: LinkThickness

Link AB complete!

✏️ Part 8: Creating Input Arm (OI)

Design Intent

📍 Input Arm Purpose

This arm extends from O through A all the way to I (input stylus):

  • Pivot at O (shares with base links)
  • Passes through A (coordinates with Link OA)
  • Extends to I (input point for user to control)
  • Stylus holder at point I

Step-by-Step: Input Arm

  1. Body: Create and rename to InputArm

  2. Sketch on XY_Plane

  3. External Geometry:

    • Reference MasterSketch
    • Select points O, A, and I

  4. Draw arm profile:

    • Long rectangle from O to I
    • Holes at O and A for pin joints (PinRadius)
    • Width: LinkWidth (or slightly narrower if needed)
    • Stylus holder at I: Small protrusion or marking hole

  5. Pad: LinkThickness

Input Arm complete!

🎯 Part 9: Creating Output Arm (OP)

This arm extends from O through B to P (output tracer).

Step-by-Step: Output Arm

  1. Body: OutputArm

  2. Sketch on XY_Plane

  3. External Geometry:

    • Reference O, B, and P

  4. Draw arm profile:

    • Rectangle from O to P
    • Holes at O and B (PinRadius)
    • Width: LinkWidth (or narrower)
    • Tracer mount at P: Protruding pin or marking feature

  5. Pad: LinkThickness

Output Arm complete!

🏗️ Part 10: Creating the Base

Design Intent

⚓ Base Requirements

Fixed mounting plate providing:

  • Pivot mount at O for all rotating links
  • Stable foundation for the mechanism
  • Mounting holes for securing to work surface

Step-by-Step: Base

  1. Create Body

    • Body: Base

  2. Create Sketch on XY_Plane

  3. Draw base plate:

    • Rectangle centered at origin
    • Width: 150 mm
    • Height: 100 mm
    • Use Symmetric constraints to center about X and Y axes

  4. Add pivot hole at O:

    • Circle at origin
    • Radius: ƒx → Spreadsheet.PinRadius

  5. Optional: Add mounting holes

    • Four circles in corners for bolt holes
    • Radius: 4 mm (M8 clearance)
    • Position: 10mm from edges

  6. Check: Fully constrained

  7. Pad: Thickness = 15 mm

Base complete! All parts are now ready for assembly!

🧩 Part 11: Assembly

Assembly is where the pantograph comes to life! With six separate parts all sharing a common pivot point at O, proper constraint strategy is critical. We’ll use axial alignment to create revolute joints while maintaining the parallelogram geometry.

Assembly Strategy

🎯 Assembly Constraints Plan

  1. Base: Fixed (ground link)
  2. Four links pivot at O: Link_OA, Link_OB, InputArm, OutputArm
  3. Joint at A: Link_OA, Link_AB, InputArm meet
  4. Joint at B: Link_OB, Link_AB, OutputArm meet
  5. All motion in XY plane

Creating the Assembly

  1. Switch to Assembly workbench

    Use workbench dropdown

  2. Create new assembly

    Assembly → Create Assembly

  3. Add all parts

    Drag from tree or use “Add Part” button:

    • Base
    • Link_OA
    • Link_OB
    • Link_AB
    • InputArm
    • OutputArm

✅ Part 12: Verifying the Scaling Ratio

The true test of a pantograph is its scaling accuracy. We’ll verify both the geometric construction and the parametric control to ensure the mechanism works correctly at any scaling ratio.

Verification Methods

Measure actual motion:

  1. Mark starting position

    • Note coordinates of input point I
    • Note coordinates of output point P
    • Record or screenshot

  2. Move input 10mm horizontally

    • Drag input arm to move I exactly 10mm right
    • Use FreeCAD measurement tools if needed

  3. Measure output displacement

    • Check new position of P
    • Calculate displacement
    • Should be 20mm (2× input) with k=2

  4. Test vertical motion

    • Move I 10mm upward
    • P should move 20mm upward

✅ Success indicator: Output displacement = k × Input displacement

📐 Part 13: Technical Drawing

Creating Professional Documentation

  1. Switch to TechDraw workbench

    Use workbench dropdown

  2. Create a page

    • Insert Page
    • Choose template: A3_Landscape

  3. Add assembly view

    • Insert View → Select assembly
    • Position: Front view showing full mechanism
    • Scale: 1:2 or 1:1 depending on size

  4. Add dimensional callout

    Create text box showing:

    Scaling Ratio:

    Link Lengths:

  5. Add motion diagram (optional)

    • Show two positions of mechanism
    • Dimension: ΔI = 10mm, ΔP = 20mm
    • Demonstrates scaling relationship

  6. Title block

    • Part name: “Pantograph Mechanism”
    • Scaling ratio:
    • Scale, date, your name

  7. Export

    Right-click page → Export as PDF

You now have professional documentation for your parametric pantograph!

🔬 Part 14: Testing Parametric Control

This is where expression-based parametric design really shines. Watch as a single parameter change recalculates all dependent dimensions and updates the entire mechanism automatically.

Parametric Experiments

Create a 1:1 copy pantograph:

  1. Open Spreadsheet

  2. Change ScalingRatio

    • Cell B2: Type 1
    • Enter

  3. Recompute (Ctrl+R)

  4. Observe:

    • InputLength = 100mm (same as BaseLength)
    • OutputLength = 100mm (k² = 1)
    • CrossLink = 100mm
    • All arms same length!

  5. Test motion:

    • Input and output now move identically
    • Perfect 1:1 copy!

🎓 Learning Outcomes

By completing this lesson, you have:

  • ✅ Designed a ratio-driven mechanism
  • ✅ Used expressions to link multiple dimensions
  • ✅ Created similar triangle geometry
  • ✅ Implemented parametric scaling control
  • ✅ Designed for smooth planar motion
  • ✅ Reused parametric parts across assembly
  • ✅ Documented ratio-based mechanisms
  • ✅ Verified motion scaling through testing

Design Verification

  1. Does the output point move smoothly as input moves?
  2. Is the scaling ratio correct? (Test with measurements)
  3. When you change ScalingRatio parameter, do all links update correctly?
  4. Does the mechanism maintain similar triangle geometry throughout motion?
  5. Are there any binding points or dead spots?

Mathematical Verification

Calculating Output Position

For a pantograph with scaling ratio k:

Example:

  • Input moves to
  • With
  • Output should be at

Test this in your assembly!

Challenges for Further Practice

  1. Design a reduction pantograph (k = 0.5, output smaller than input)
  2. Add a stylus holder at input point (removable, adjustable)
  3. Add a pen/pencil holder at output point
  4. Create a locking mechanism to fix position
  5. Design a trammel attachment (for drawing ellipses)
  6. Build a 3D pantograph (scales motion in XY plane vertically)

Common Issues and Solutions

“Output doesn’t scale correctly”

  • Cause: Incorrect link length ratios
  • Solution: Verify expressions in spreadsheet
  • Fix: InputLength must = BaseLength × k
  • Fix: OutputLength must = BaseLength × k²

“Mechanism binds or locks up”

  • Cause: Links interfering, or over-constrained assembly
  • Solution: Check clearances, ensure only Base is Fixed
  • Fix: May need to offset arms in Z-direction
  • Cause: Dimensions not using formulas
  • Solution: Check that InputLength cell has =B3*B2 not a hardcoded value
  • Fix: Recreate spreadsheet formulas

“Parts misalign in assembly”

  • Cause: Not referencing master sketch consistently
  • Solution: All part sketches must use External Geometry from same master sketch
  • Fix: Rebuild parts referencing master sketch points

Next Steps

In the next lesson on Cam and Follower Mechanism, we’ll explore:

  • Motion programming through geometry
  • Curve-based sketching
  • Rise-dwell-return profiles
  • Contact-driven motion
  • Datum axes and reference geometry

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