Side Holes

Create the iconic SMARS side profile and motor shaft holes using sketches and pockets

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What We’re Building

This lesson creates two critical features:

1. The SMARS rhombus profile - The distinctive diamond-shaped cutout that defines the SMARS look
2. Motor shaft holes - 4.5mm circles for the N20 motor shafts to pass through

Feature	Dimension	Purpose
Rhombus top	28mm	Visual design, weight reduction
Rhombus bottom	16mm	Tapers toward motor area
Rhombus height	20mm	Maximizes opening while maintaining strength
Motor holes	4.5mm diameter	Fits N20 motor shaft (4mm) with 0.5mm clearance

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Understanding the Design

Why a Rhombus?

The rhombus shape isn’t just aesthetic - it’s clever engineering:

• Weight reduction - Less material = lighter robot = longer battery life
• Visibility - You can see inside to check wiring and components
• Ventilation - Air can flow through to cool electronics
• Distinctive look - Makes SMARS instantly recognizable

Why 4.5mm Motor Holes?

N20 motors have 4mm shafts. We add 0.5mm clearance because:

• 3D prints have slight inaccuracies
• Clearance allows shaft rotation without friction
• If too tight, the motor works harder (wastes battery)

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Step-by-Step: Create the Side Profile Sketch

1. Start a New Sketch on the Side Face

Click on the side face of the base to select it, then click Create Sketch.

2. Draw the Rhombus Shape

Using the Line tool, draw a four-sided rhombus shape (like a squashed diamond). Don’t worry about exact placement yet - we’ll add dimensions next.

3. Add Dimensions to the Rhombus

Use the Dimensions tool to constrain the shape:

• Bottom line: 16mm
• Top line: 28mm
• Total height: 20mm
• Bottom edge position: 10.5mm from the base bottom

Notice the problem? The rhombus might be lopsided. We’ll fix that with a centerline.

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Centering the Rhombus (Professional Technique)

4. Add Midpoints and a Centerline

Using the Point tool, create points at:

• The midpoint of the top line
• The midpoint of the bottom line

The cursor shows a red symmetry indicator when you’re over a midpoint.

Using the Line tool, connect these two midpoints with a line.

Tip: If the main body blocks your view, hide it by clicking the eye icon next to the body in the Model tree.

5. Make the Centerline Vertical

Select the line and use the Vertical Constraint tool to make it perfectly vertical. This forces the rhombus to be symmetric!

Make this line a construction line by selecting it and clicking Toggle construction mode.

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Aligning to the Model Center

Now we need to position our rhombus in the center of the side face.

6. Project External Geometry

Click the Create external geometry button in the toolbar.

Click on the top edge of the base to project it into your sketch. This creates a reference line you can use for alignment.

7. Create and Constrain the Midpoint

Use the Point tool to create a point at the midpoint of the projected top edge.

8. Attach Rhombus to Center

Select the top point of the rhombus, then hold Ctrl and select the midpoint you just created.

Click Constrain Coincident to lock them together.

Now your rhombus is perfectly centered on the side face!

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Step-by-Step: Add Motor Holes

9. Draw the Motor Hole Circles

Using the Circle tool, draw two circles toward the bottom of the body - roughly where the motors will go.

10. Dimension the Circles

Using the Dimensions tool:

• Set each circle diameter to 4.5mm

11. Position the Motor Holes

Each motor hole center should be:

• 8mm from the bottom edge
• 8mm from the respective side edge

Use Create external geometry to project the left and right side edges, then dimension the circles from these edges.

When fully constrained, the circles turn green - this means FreeCAD knows exactly where everything should be!

12. Close the Sketch

Click the Close button in the toolbar.

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Step-by-Step: Cut Through the Base

13. Pocket the Features

With the sketch selected in the Model tree, click the Pocket button.

In the Pocket dialog, set the length to 58mm - this cuts all the way through the base from one side to the other.

Click OK to apply.

14. Verify the Result

You should now see:

• The rhombus profile cut through both sides
• Two motor shaft holes ready for N20 motors

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Understanding External Geometry

Why project edges? External geometry lets you reference existing features in your sketch:

• You can dimension from them
• You can constrain to them
• If the original feature moves, your sketch updates automatically

This is the parametric power of FreeCAD - everything stays connected!

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Try It Yourself

1. Verify symmetry: Look at the model from the top. The rhombus should be perfectly centered.
2. Check hole alignment: Both motor holes should be at identical heights.
3. Test the design: Imagine sliding an N20 motor shaft through - is there enough clearance?

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Common Issues

“My rhombus isn’t symmetric”

Problem: One side is longer than the other. Solution: Ensure the centerline has a Vertical constraint. If not, select it and apply one.

“The pocket didn’t cut all the way through”

Problem: The rhombus or holes only appear on one side. Solution: The pocket length should be 58mm (the full width of the base). Check your dimension.

“Circles show as orange/white, not green”

Problem: The circles aren’t fully constrained. Solution: Make sure both the diameter AND position (distance from edges) are dimensioned.

“I can’t select the side face”

Problem: Clicking selects something else. Solution: Rotate the view so the side face is directly visible. Click in the center of the face, not near edges.

“External geometry isn’t visible”

Problem: Projected lines don’t appear. Solution: Make sure you clicked directly on the edge you want to project. The projected geometry appears as dashed purple lines.

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What You Learned

In this lesson, you mastered:

• External geometry - Referencing existing features in sketches
• Vertical constraints - Forcing perfect alignment
• Multiple features in one sketch - Combining shapes for a single operation
• Through-all pockets - Cutting features that go all the way through

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Next Up

The front and rear of our SMARS base need openings for cables and component access. We’ll create more sketches and pockets to complete the enclosure profile!

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