A Simple Tensegrity Chair

The concept of tensegrity has always been something that tickles me. Structures that hold themselves apart through pure tension it feels like magic that obeys physics. In furniture design, tensegrity chairs sit exactly at the intersection of function and wonder. They hold you up while looking like they shouldn't.

I designed this entirely in SolidWorks, a tool built for precision, part by part, bolt by bolt. Every angle measured. Every cable length calculated. No guesswork

Let's build a chair that floats.

Before You Start

1. Create a folder on your computer. Name it something you'll recognize in three weeks, I called mine Tensegrity_Chair.

2. Set your units to millimeters:

· Go to Options > Document Properties > Units

· Select MMGS (millimeter, gram, second)

· Click OK

Every dimension in this guide is in millimeters. Stick to them and your chair will fit together perfectly.

SolidWorks 2021 (any version with 3D sketch and sweep works)

A working device (laptop, desktop just make sure it turns on)

Consistent power supply

Before any software, draw.

Not because it's nostalgic. Because a 3D model is just a drawing with extra dimensions. If you can't sketch it, you haven't designed it you've only guessed.

Draw your chair from at least two angles. Front. Side. Note your dimensions. This isn't art class. This is your contract with yourself so you know what you're building before you build it.

1. File > New > Part

2. In the feature tree on the left, you'll see three default planes: Front, Top, and Right.

3. Right-click on Top Plane and select Sketch.

The view will automatically orient itself so you're looking straight down at the sketching grid perfect for what we're about to do.

Pro tip: If your view ever looks crooked, press Ctrl + 8 to snap back to "Normal To" view.

This is the foundation of the entire chair. Take your time here get it right and everything else follows.

3.1 Draw the Outer Rectangle

1. Go to the Sketch tab (top of screen) and click the Center Rectangle tool.

(It looks like a rectangle with a cross in the middle this tool draws rectangles centered on your click point.)

2. Click once on the origin point (0,0) that's the crossed circle in the middle of your grid.

3. Move your mouse outward and click again to create a rectangle. Size doesn't matter yet we'll dimension it precisely.

4. Press S to open the shortcut bar and select Smart Dimension (or click its icon in the Sketch tab).

5. Click the top edge of your rectangle, then click the bottom edge drag your mouse outward and click to place the dimension.

6. Type: 600mm and press Enter. (This is the height.)

7. Click the left edge, then the right edge drag outward and click.

8. Type: 580mm and press Enter. (This is the width.)

You should now have a perfect 600mm × 580mm rectangle centered on the origin.

Why centered? Building everything around the origin makes assembly much easier later. Trust me on this.

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3.2 Create the First Cutout (Left Side)

Now we're going to carve out the inner shape where the stands will connect.

1. Still in the same sketch, select the Line tool from the Sketch tab.

2. Click on the top-left corner of your large rectangle.

3. Drag your mouse straight down and click again when the line is roughly 150mm long.

(Don't worry about exact length yet we'll dimension it properly.)

4. Press S, select Smart Dimension, and click the line you just drew.

5. Type: 150mm and press Enter.

This line is just a guide we'll remove it later.

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3.3 Draw the Left Cutout Rectangle

1. At the end of that line, we're going to create a rectangle that shares the same left edge as the main shape.

2. Select the Corner Rectangle tool (not Center Rectangle this one draws from corner to corner).

3. Click at the endpoint of your 150mm line.

(The cursor should show a small yellow dot when you're exactly on the endpoint.)

4. Drag downward and to the right to create a rectangle that touches the left edge of the main shape.

5. Before dimensioning, let's get the proportions right:

· Use Smart Dimension to set the width of this new rectangle: click its left edge, then its right edge type 165mm.

· Set the height: click its top edge, then bottom edge type 250mm.

Important check: This rectangle's left side should be exactly on the left edge of your main rectangle. If it's not, click and drag it until it snaps into place. The cursor will show a yellow dot when it's aligned.

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3.4 Trim the Excess Guide Line

Remember that 150mm line we drew earlier? It's now inside our cutout rectangle and we don't need it anymore. It would cause problems if we left it there.

1. Go to the Sketch tab and click Trim Entities (looks like a pair of scissors).

2. In the Property Manager on the left, make sure the Trim to Closest option is selected (it's usually the first icon).

3. Click on the 150mm line it will disappear instantly, leaving only the clean rectangle edges.

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3.5 Repeat for the Right Side

We're going to do the exact same thing on the right, but mirrored.

1. Select the Line tool again.

2. Start at the top-right corner of the main rectangle.

3. Draw a line straight down and dimension it: 150mm.

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1. Select Corner Rectangle and start from the endpoint of that line.

2. This time, the rectangle's right side should align with the main rectangle's right edge.

3. Dimension it:

· Width: 165mm (from right edge inward)

· Height: 250mm

Trim that 150mm guide line the same way you did on the left.

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3.6 Check Your Work

Before moving on, take a moment to verify you have:

· One large outer rectangle: 600mm tall × 580mm wide

· Two smaller rectangles inside:

· Left side: 165mm wide × 250mm tall, touching left edge

· Right side: 165mm wide × 250mm tall, touching right edge

· Both positioned exactly 150mm down from the top corners

· No extra guide lines just clean, closed rectangles

If something looks off, use Ctrl + Z to undo and check each dimension again. Better to fix it now than later.

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3.7 Turn It Into a 3D Solid

1. Exit the sketch by clicking the Sketch icon again (or press Ctrl + Q).

2. Go to the Features tab and click Extruded Boss/Base.

3. In the Property Manager on the left:

· Direction 1: Make sure the arrow is pointing upward (away from the sketch plane).

· Set Depth: 50mm.

· Look at the preview if the extrude went the wrong direction, click the Flip Direction arrow.

· Click the green check when it looks right.

Congratulations! You now have a 3D base plate with two recessed sections.

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3.8 Save Your Work

1. File > Save As

2. Navigate to the folder you created earlier (Tensegrity_Chair)

3. Name this file: Base (simple and clear)

4. Click Save

Now we'll add the holes where the stand and strings will attach.

4.1 Start a Sketch on the Top Face

1. Right-click on the top face of your base model.

2. Select Sketch from the menu.

The view will automatically orient to look straight down at this face.

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4.2 Draw a Positioning Line

1. Select the Line tool.

2. From the midpoint of the top edge of the base, draw a line straight down.

3. Use Smart Dimension to set its length: 150mm.

This line helps us position the first mounting point accurately.

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4.3 Create the First Mounting Square

1. At the end of that line, select Center Rectangle.

2. Click at the endpoint and drag outward to create a small square.

3. Use Smart Dimension to set both sides: 50mmx50mm.

4. Make sure the square is centered exactly on the endpoint.

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Trim the 150mm guide line we don't need it anymore.

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4.4 Create the First Circle Hole

1. From the top-left corner of the base, draw a line down: 50mm.

2. From the end of that line, draw another line right: 50mm.

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1. At the endpoint of these lines, draw a circle:

· Select the Circle tool

· Click at the endpoint

· Drag outward and set diameter: 5mm using Smart Dimension

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1. You can trim the two guide lines now, or leave them they won't affect the 3D model.

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4.5 Pattern the Circle to All Corners

This is where SolidWorks saves us time. Instead of drawing four circles manually, we'll use Linear Pattern.

1. Select the circle you just drew (click on its edge , it should highlight).

2. Go to the Sketch tab and click Linear Sketch Pattern.

3. In the Property Manager:

· Direction 1 (X axis): Set spacing to 480mm, number of instances to 2

· Direction 2 (Y axis): Set spacing to 500mm, number of instances to 2

· You should see a preview of four circles, one near each corner

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1. Click the green check

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4.6 Select Everything for Cutting

1. Hold Ctrl and click:

· The 50mm square (mounting point)

· All four circles (string holes)

2. Release Ctrl everything should be highlighted.

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4.7 Extrude Cut

1. Exit the sketch.

2. Go to Features > Extruded Cut.

3. Set Depth: 10mm (these are shallow recesses, not through-holes).

4. Check the preview make sure it's cutting into the base, not extending out.

5. Click the green check

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4.8 Save Your Progress

File > Save (or Ctrl + S). The file name is already set just save.

Base is complete!

This part is the vertical support that will hold everything up. We'll make one, but you'll use two copies in the assembly later.

5.1 Start a New Part

1. File > New > Part

2. In the feature tree, right-click on Right Plane and select Sketch.

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5.2 Draw the Profile

We're creating an upside-down L shape like a corner bracket but stretched.

1. Select the Corner Rectangles tool.

2. Start from the origin (0,0) and draw a rectangle

3. Use Smart Dimension to make the width 50mm and the length 460mm

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5.3 Create the Extended Top

Now we add the "top part" of the L the horizontal piece that will connect to the seat.

1. Using the corner rectangle draw a rectangle 150mm wide and 50mm long from the top left corner of the first rectangle.

2. Trim the lines within the contour.

Your profile should now look like an upside-down L.

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5.4 Extrude It Into 3D

1. Exit the sketch.

2. Go to Features > Extruded Boss/Base.

3. Set Depth: 50mm (this gives it thickness).

4. Click the green check

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5.5 Add the Hole (Important!)

This hole is where the tension string will attach.

1. Right-click on the inner face of the vertical leg (the side that will face the other stand).

2. Select Sketch.

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1. From the midpoint of the bottom edge of this face, draw a vertical line up: 25mm.

2. At the end of that line, draw a circle:

· Use Smart Dimension to set diameter: 5mm

· Make sure its center is exactly at the line's endpoint

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1. Exit sketch.

2. Go to Features > Extruded Cut.

3. Set Depth: 10mm (through the thickness of the leg).

4. Click the green check.

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5.6 Save It

1. File > Save As

2. Navigate to your chair folder

3. Name it: Stand

4. Click Sav

e

Remember: You'll need two copies of this in the assembly later.

These are the diagonal cables that keep the chair stable.

1. File > New > Part

2. Select Top Plane Sketch

3. Draw a circle with diameter: 10mm

4. Exit sketch

5. Extruded Boss/Base set to 650mm

6. Save as: String_Long

This one carries the actual weight of the chair and person.

1. Repeat the same process:

· Circle diameter: 10mm

· Extrude length: 200mm

2. Save as: String_Tension

Now for the part you'll actually sit on.

1. File > New > Part

2. Select Top Plane Sketch

3. Draw a center rectangle:

· Height: 600mm

· Width: 580mm

4. Exit sketch

5. Extrude to 50mm

6. Save as: Seat (we'll add details next)

9.1 First Rectangular Cutout

1. Right-click the top face of your seat block Sketch

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1. Draw a rectangle anywhere inside position doesn't matter yet.

2. Use Smart Dimension to position it precisely:

· 25mm away from left edge

· 25mm away from right edge

· 25mm away from bottom edge

· 100mm down from top edge

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9.2 Second Rectangular Cutout

1. Draw another rectangle above the first one.

2. Position it:

· 25mm from top edge

· 25mm from left edge

· 25mm from right edge

· 25mm above the first rectangle

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9.3 Cut Them Out

1. Exit sketch

2. Features > Extruded Cut

3.

Set depth: 10mm

4. Click green

10.1 Flip and Sketch

1. Rotate the model to see the bottom face

2. Right-click bottom face, Sketch

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10.2 First Circle

1. Draw a circle with diameter 10mm

2. Position it 50mm from the top edge and 50mm from the left edge of the face

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10.3 Pattern to All Corners

1. Select the circle

2. Linear Sketch Pattern

3. Set:

· Direction 1 (X): 480mm spacing, 2 instances

· Direction 2 (Y): 500mm spacing, 2 instances

4. Click green

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10.4 Cut the Holes

1. Exit sketch

2. Extruded Cut depth: 10mm

3. Click green

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10.5 Save

the Seat

File > Save (overwrite)

This is where your back rests, slightly angled for comfort.

1. File > New > Part

2. Select Right Plane, Sketch

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1. Draw a rectangle:

· Width: 50mm

· Height: 10mm (this is the bottom connector)

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1. From the top-right corner of this rectangle, draw a line upward at an angle:

· Use Smart Dimension to set the angle between this line and the top side of the rectangle to 85° (not 90°, that slight tilt is the comfort factor)

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1. From the top of that angled line, draw a horizontal line left: 50mm

2. Connect back down to the top-left corner of the original rectangle

Your profile should now look like a slightly tilted rectangle on top of a small base rectangle.

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1. Exit sketch

2. Extrude to 530mm (this is the width of the backrest)

3. Save as: Backrest

Two simple cuboids, one built on top of the other.

1. File > New > Part

2. Select Front Plane, Sketch

3. Draw a 50mmx50mm square

4. Exit sketch

5. Extrude to 330mm

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1. Rotate to see the bottom face

2. Right-click bottom face, Sketch

3. Draw a Corner Rectangle (anywhere)

4. Dimension it:

· 50mmx50mm

· Position it exactly 50mm away from the top edge of the face

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1. Exit sketch

2. Extrude this new rectangle by 210mm (downward)

3. Save as: Handle

You'll need two handles in the assembly.

Simple, curved, comfortable.

1. File > New > Part

2. Select Right Plane, Sketch

3. Draw a rectangle:

· Width: 475mm

· Height: 10mm

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1. Trim the top side, we don't need it

2. Select the 3 Point Arc tool:

· Click the left top point of the rectangle

· Click the right top point of the rectangle

· Drag upward to create an arc

· Set the radius to 750mm using Smart Dimension

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1. Exit sketch

2. Extrude to 530mm

3. Save as: Cushion

1. File > New > Assembly (not Part this time!)

2. In the Property Manager, click Browse

3. Find your Base part and insert it

The first part you insert becomes fixed, it won't move. Perfect for the

base.

1. Click Insert Components (or drag the Stand part from your folder into the workspace)

2. You'll need to rotate it to face the right direction:

· Select the Stand

· Click Move Component dropdown, Rotate Component

· In the Property Manager, change Free Drag to By Delta XYZ

· Set Y-axis to 180° (this flips it to face inward)

· Click Apply

I find the next steps to be easier followed through videos. Please follow it as much as you can and forgive my saving nomenclature. You will find the names don't match as in the videos.

Here are the file name equivalents:

Base : Base

Stand : Stad

Seat : Seat

Cushion : Cso

Tension cable: 1xstrg

Support or balance cable : 4xstrg

Back Rest : Bac

Arm rest: adle

Add there you have it. A simple tensegrity chair made in Solidworks