Slider Crank Mechanism Design

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

Stroke Relationship:

where is the stroke and is the crank radius.

Design Guidelines:

• l/r ≥ 3 for minimal side forces
• l/r = 4 to 5 common in engines
• Shorter rods = more compact but higher loads

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

Key Workbenches for This Lesson:

• Part Design - Creating individual parametric parts (primary workbench)
• Sketcher - Creating 2D constraint-based sketches
• Spreadsheet - Parameter tables and calculations
• Assembly - Combining parts with constraints
• TechDraw - Creating engineering drawings

Essential Navigation Controls:

Spend 2 minutes navigating the empty 3D view using these controls. Muscle memory now saves time later!

In the spreadsheet, create this table:

Why Aliases?

Aliases let you reference cells by name instead of “B2”, making formulas readable.

Create aliases:

1. Click cell B2

2. Right-click → Properties

3. In “Alias” field, type: CrankRadius

4. Click OK

5. Click cell B3

6. Right-click → Properties

7. In “Alias” field, type: RodLength

8. Click OK

Now you can use Spreadsheet.CrankRadius anywhere in your model!

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

Geometry Tools:

• Line (L)
• Circle (C)
• Arc
• Rectangle
• B-spline (S)

Constraint Tools:

• Coincident (joins points)
• Horizontal / Vertical
• Parallel / Perpendicular
• Equal (equal lengths)
• Symmetric
• Distance
• Radius
• Angle

Check Status:

• Look at “Solver messages” panel
• “Fully constrained” = perfect!
• “X degrees of freedom” = need more constraints

Make shaft hole concentric with origin (if you did not already ‘Click at the origin’ above):

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!

Make rod pin horizontally aligned (if you did not already ‘Click at the origin horizontal line’ above):

1. Click Horizontal constraint tool
2. Click the center of the offset circle
3. Click the origin
4. Press Escape

Alternative shortcut:

• Select both points (Ctrl+click)
• Press H key

The pin hole is now horizontally aligned!

1. Click the outer circle, then press ‘K’ and ‘R’ in quick succession to activate the Radius Constraint Dimensioning Tool (or go to Sketch → Sketcher Constraints → Constrain Radius).
2. Type 40
3. Click OK.

Crank disk is now 40mm radius.

1. Click the inner circle, then press ‘K’ and ‘R’ in quick succession
2. Type: 8
3. Press Enter

8mm radius shaft hole created.

1. Click the offset circle, then press ‘K’ and ‘R’ in quick succession
2. Type: 5
3. Press Enter

5mm radius pin hole created.

1. Click the origin point, then click the origin point of the Rod Pin Hole circle.
2. Press ‘L’ to activate the Constraint Horizontal Distance Dimensioning Tool. Don’t type a number!
3. Click the small fx button and in the formula editor, start typing Spreadsh… and <<Spreadsheet>> will appear. Then, click it. Next, start typing the alias Crank… and CrankRadius will appear. Click it.
4. Click OK and you will see Radius: 30.00.
5. Click OK again.

Magic! The dimension now shows “30mm” and will update whenever you change the spreadsheet!

1. Select the sketch in the tree (under Crank body)

2. Click Pad tool in Part Design toolbar

3. In the Pad panel (left side):

   • Type: Dimension
   • Length: 10 mm (crank thickness)

4. Click OK

You now have a 3D crank!

Navigate the 3D view:

• Press V then F to fit all
• Rotate view with middle mouse button
• See the disc with holes!

Create the end profiles:

1. Circle tool (press G, C)

2. Click anywhere on the left side of the sketch area and draw the first circle

3. Repeat the process to the right of the first circle (arbitrary distance) to draw the second circle

4. Press Escape

5. Select the left circle

6. Radius constraint: Press K, R

   • Type: 10 mm
   • Enter

7. Repeat for right circle:

   • K, R → Radius = 8 mm
   • Enter

The two circles define the rod ends. Their spacing will be controlled later using constraints.

Create tangent boundaries:

1. Line tool (press G, L)

2. Draw a long horizontal line above both circles

   • Start well before the left circle
   • End well after the right circle

3. Press Escape

4. Draw a second horizontal line below both circles

   • Again, extend it past both circles

5. Press Escape

These lines will later become tangent to the circles and trimmed to form the rod body.

Constrain and clean geometry:

1. Apply tangent constraints:

   • Click top line, then left circle arc, press T
   • Repeat for:
     • Top line → left circle
     • Top line → right circle
     • Bottom line → left circle
     • Bottom line → right circle
       (4 tangents total)

2. Trim excess geometry:

   • Trim tool (G, T)
   • Trim the overextended ends of the top and bottom lines (4 trims)
   • Trim the inner arcs of both circles between the lines

3. Press Escape

The rod outline is now defined by tangency — strong, clean constraints with minimal dimensions.

Align and parametrize the sketch:

1. Align circle centers horizontally:

   • Click left circle center
   • Click right circle center
   • Press H

2. Set rod length parametrically:

   • Click left circle center
   • Click right circle center
   • Press L (horizontal distance)
   • Click ƒx
   • Enter: Spreadsheet.RodLength
   • OK

3. Fix left end to origin:

   • Click left circle center
   • Click origin
   • Press C (coincident)

The rod length is now fully driven by the spreadsheet and anchored to the origin.

Verify and create solid:

1. Confirm Fully constrained
2. Close sketch
3. Pad → Length = 8 mm
4. OK

The outer rod body is complete.

Create pin holes using a secondary sketch:

1. Click the top face of the rod

2. Create sketch (go to Sketch → Create Sketch)

3. Left inner hole:

   • G, C
   • Click the origin
   • K, R → Radius = 8 mm
   • OK

4. Right inner hole:

   • Enable external geometry (G, X)
   • Click the right outer arc
   • G, C
   • Click the arc center
   • K, R → Radius = 6 mm
   • OK

Using external geometry guarantees perfect alignment with the outer profile.

Cut through the body:

1. Close sketch

2. Select one hole circle sketch

   • If hidden, click the eye icon or double-click the sketch

3. Click Hole tool

   • Depth: Through all
   • Diameter: R × 2
   • OK

4. Repeat for the second hole

5. Press V, F → View Fit

6. Save: Ctrl + S

Connecting rod complete and fully parametric!

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

1. Select Frame in assembly tree

2. Click Fixed constraint button

3. Frame is now locked in place (ground link)

Allow crank to rotate:

1. Select crank center hole axis

2. Select frame pivot hole axis

3. Click Axial Align constraint

This aligns the axes and allows rotation! Crank can now spin about its shaft.

Connect rod to crank:

1. Rod left hole axis → Crank offset pin hole axis
2. Axial Align constraint

Connect rod to slider:

1. Rod right hole axis → Slider pin hole axis
2. Axial Align constraint

Constrain slider to linear motion:

1. Select slider bottom face
2. Select frame top face
3. Apply Plane coincident or Linear constraint

This keeps slider on the guide!

Test the mechanism:

Try dragging the crank in the assembly view:

• Crank should rotate
• Rod should follow
• Slider should move linearly!

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!

1. Change RodLength

   • Cell B3: Type 120
   • Enter

2. Recompute (Ctrl+R)

3. Verify:

   • Connecting rod is now longer!
   • Motion profile changes slightly
   • All constraints maintain

✅ Your rod is parametric too!

1. Set CrankRadius = 50
2. Set RodLength = 150
3. Recompute

Entire mechanism scales up!

Try extreme values:

• CrankRadius = 20, RodLength = 80
• CrankRadius = 60, RodLength = 200

Everything should update cleanly!

Try these ratios:

Watch how motion characteristics change!

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

1. Create wrist pin

   Separate part connecting rod and slider

2. Add piston ring groove

   Use Pocket tool to cut groove in slider

3. Exploded view

   Create exploded assembly view in TechDraw

1. Motion study

   Calculate slider velocity and acceleration formulas

2. Multiple configurations

   Create versions with different l/r ratios

3. FEA analysis

   Apply FEM workbench to analyze rod stresses

“Sketch not fully constrained”

“Cannot pad sketch”

“Formula error in dimension”

“Part doesn’t update with parameter”

“Parts don’t move”

“Parts misaligned”