Open a new part with model units set to millimeters

Go to: File > New > Part 

Create a 2D sketch

Select the Top Plane in the feature tree (menu at the left side) and create a sketch by clicking on the 2D Sketch icon. 

The display changes so the Top plane faces you.

Create a Center Rectangle

Go to Tools > Sketch Entities > Center Rectangle or click at the center rectangle icon 

Create a sketch which starts at the Origin. 

Change the dimensions of the rectangle into 100 and 150 mm by clicking at the dimension button 

Create an Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

The Boss-Extrude menu appears

Direction 1 is set to Blind. When you use the Blind feature you’ll get a solid extrude.

The yellow preview shows the extrusion of the rectangle.

By clicking at the Reverse button  you can change the direction of the extrude.

Click a few times at the Reverse button and notice the differences.

With   you can change the Depth of the extrude.

Change the Depth of the extrusion into 100 mm.

Besides the Blind direction there are a few other Direction Options:

Trough All: Extrude a feature through all the other bodies in the model (this feature is only available when you’ve other bodies into your part)

Up To Vertex: You can use this to extrude a feature to a specific point or edge of another shape.

Up To Surface: Use this option if you want to extrude a shape until a specific surface

Offset From Surface: With this option it’s possible to extrude a shape until a distance from another surface.

Up to Body: You can use this to Extrude a feature to a specific body. This feature is only available when you’ve other bodies into your part. When you get the Rebuild Error:  “Unable to extrude up to selected body” you have to make sure that the next body is bigger as your extrude.

Mid Plane: Extrude a sketch to two equal directions.

Up To Next: Extrude the sketch up to the next body. When you get the Rebuild Error: “Unable to extrude up to selected body” you have to make sure that the next body is bigger as your extrude.

Besides the different options for the direction of the extrude it’s also possible to immediately add a draft to the extrude.

Click at the Draft  icon

Change the draft size into 5 degrees

With the Draft outward option it’s possible to change the direction of the draft.

With the Direction 2 option you can add a second direction to the extrude.

You can also add a second draft to this direction as shown in the picture.

Change the Draft angle into 30 degrees.

Beside the Direction 1 and Direction 2 options there’s also a Thin Feature option

With this feature you can create a Thin Extrude

You can use the  option to change the thickness of the extrusion edge

Change T1 to 10 mm as shown in the picture.

When you check the Cap ends option you can close the top and bottom of the extrusion to get a hollow extrude (all within one single feature!)

When you’ve multiple figures in one sketch you can use the Selected Contours  option to pick only the figures you want to extrude.

Click OK   to apply your Extrude

Well, that’s all for now. Hopefully you’ve learned something from my post about the Extrude feature.

Do you still have questions about it or want to add something? Feel free to leave a comment below.

• Draw a 2d sketch
• Insert a blueprint
• Surface Revolve
• Surface Sweep
• Surface Loft
• Surface Fill
• Surface Knit
• Fillet
• New Axis
• Revolved Cut

Open a new part with model units set to millimeters

Go to: File > New > Part

Create a 2D sketch

Select the Right Plane in the feature tree (menu at the left side) and create a sketch by clicking on the 2D Sketch icon 

The display changes so the Right plane faces you.

Insert a reference picture

For this tutorial we use a blueprint of the Deoroller to approach the organic shape as good as possible.

Download the picture here and save it into your SolidWorks folder

Go to: Tools > Sketch Tools > Sketch Picture 

Go to your SolidWorks folder and select the picture “SIDEVIEW_DEOROLLER.Jpg”

Click: Open

Change the dimensions and position of the picture with the menu as shown in the picture.

Select ‘’Full image’’ in the Transparency tab and change the transparency into 0.40

Click OK 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Insert a second reference picture

Select the Front Plane in the feature tree (menu at the left side) and create a sketch by clicking on the 2D Sketch icon 

Download the picture here and save it into your SolidWorks folder

Go to: Tools > Sketch Tools > Sketch Picture 

Go to your SolidWorks folder and select the picture “FRONTVIEW_DEOROLLER.Jpg”

Click: Open

Change the dimensions and position of the picture with the menu as shown in the picture.

Select ‘’Full image’’ in the Transparency tab and change the transparency into 0.40

Click OK 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the two centerlines as shown in the picture 

Change the dimensions by clicking at the dimension button 

Fix the two lines with the Fix icon 

Draw the two lines as shown in the picture 

Change the dimensions by clicking at the dimension button 

Draw a spline without any midpoints 

Select one of the straight lines, hold down the control key and select the spline

Click at the Tangent icon as shown in the picture 

Repeat this action for the other side of the spline

Change the length of the arrows to approach the curve of the blueprint

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create a Surface Revolve

Go to Insert > Surface > Revolve or click at the Revolve icon 

Click at the blue Centerline to define the Axis of Revolution 

Use the One-Direction option 

Set the Revolution Angle to 360 degrees 

Click OK 

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the line as shown in the picture 

Change the dimensions by clicking at the dimension button 

Make sure that the angle of the line is equal to the front curve of the deoroller

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch4

Double click at Sketch4 in the feature tree and rename it to GUIDELINE_FRONT

Create another 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the line as shown in the picture 

Change the dimensions by clicking at the dimension button 

Make sure that the angle of the line is equal to the back curve of the deoroller

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch5

Double click at Sketch5 in the feature tree and rename it to GUIDELINE_BACK

Create a 2D sketch

Select the Front Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw a spline without midpoints as shown in the picture 

Change the length of the lower arrow to approach the curve of the blueprint

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch6

Double click at Sketch6 in the feature tree and rename it to GUIDELINE_SIDE

Create a 2D sketch

Select the Top Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the centerline as shown in the picture 

Connect the centerline with the endpoints of GUIDELINE_FRONT and GUIDELINE_BACK

Draw a spline with four points as shown in the picture 

Connect three points with GUIDLINE_FRONT, GUIDELINE_BACK and GUIDELINE_SIDE

Draw the fourth point somewhere in the space as shown in the picture

Make the Spline symmetric

Select the right point, hold down the Control key, select the centerline and select the left point.

Click at the Symmetric option in the menu 

Click OK 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch7

Double click at Sketch7 in the feature tree and rename it to PROFILE

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw a line, starting at Origin 

Change the length of the line to 58 mm 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Rename the Sketch8

Double click at Sketch8 in the feature tree and rename it to PATH

Create a Surface Sweep 

Go to Insert > Surface > Sweep or click at the Sweep icon 

Select the PROFILE sketch in the Feature Tree as Sweep Profile

Select the PATH sketch in the Feature Tree as Sweep Path

Select GUIDLINE_FRONT, GUIDELINE_BACK and GUIDELINE_SIDE in the Feature Tree as Sweep Guides

Click OK 

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the line as shown in the picture 

Change the dimensions by clicking at the dimension button 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Trim the upper side of the Surface Sweep

Go to: Insert > Surface > Trim or click at the Trim icon 

Click in the Trim tool box 

Select the line of the new Sketch9 as shown in the picture.

Select the “Remove selections” option.

Select the purple surface above the line as shown in the picture. 

Surface Split Options: Natural

Click OK 

Create a Surface Loft 

Go to Insert > Surface > Loft or click at the Surface icon 

Click in the Profiles box 

Select the two edges as shown in the picture

Make sure that the green balls are both on the same end as shown in the picture

If not, click and drag them to the other side of the sketch

Make the Loft Curvature

Click at the Start/End Contraints box

Set the Start constraint to Curvature To Face as shown in the picture

Set the End constraint to Curvature To Face as shown in the picture

You can optimize the shape of the Loft by changing the Length of the Curvature arrows

Click OK 

Fill the bottom of the Deoroller

Go to: Insert > Surface > Fill or click at the Fill icon 

Click OK 

Knit the surfaces and create a solid body

Go to Insert > Surface > Knit or click at the Surface Knit icon 

Click in the Selections box and select the 4 blue surfaces 

Select the ‘’Try to form solid’’ option

Select the “Merge entities” option

Deselect the ‘’Gap Control’’ option

Click OK 

Create a fillet on the edge of the bottom

Go to: Insert > Features > Fillet/Round or click at the Fillet icon 

Select the edge as shown in the picture.

Change the Radius into 2 mm 

Click OK 

Create a new Axis

Go to: Insert > Reference Geometry

Select the Cylindrical/Conical Face option

Select the blue surface as shown in the picture

Click OK 

Create a 2D sketch

Select the Right Plane in the feature tree and create a sketch by clicking on the 2D Sketch icon 

Draw the rectangle using the 3 Point Corner Rectangle option as shown in the picture and detail 

Change the dimensions by clicking at the dimension button 

Create a Revolved Cut

Go to: Insert > Cut > Revolve or click at the Cut Revolve icon 

Axis of revolution : Select Axis1.

Click OK 

Save  the file with the following name: Deoroller.SLDPRT

Congratulations, you just finished the Deoroller!

Renders made in PhotoView360

Click here to download the blueprints and SolidWorks file of the model

I shared this SolidWorks model of the Sleigh at Grabcad.com The model was downloaded 592 times within 14 days! I received a number of spontaneous reactions and renderings from all over the world. That’s why I thought it would be nice to organize a Render Contest. For this contest I asked the participants to create an eye-catching and spectacular render of the futuristic LearnSolidWorks Sleigh.

Unless it was a very difficuly choice, I am proud to announce the winners of the LearnSolidWorks Render Contest!

The first prize goes to Vincent van Hoogdalem with his view of Santa’s Sleigh (and the successor of Santa ) Vincent has won the SolidWorks Chopper Tutorial and the SolidWorks iPhone Tutorial! Congratulations Vincent!

 The second prize goes to Carco with his render of Santa’s Sleigh on a snowy road. Carco has won the SolidWorks Chopper Tutorial. Enjoy it!

The third prize is for Merrad Fateh. Merrad has won the SolidWorks iPhone Tutorial with his entry. Congratulations Merrad, I hope you will learn a lot of it!

I want to thank all the participants who toke part in this competition.

Below you can see the other entries (random order)

]]> http://learnsolidworks.com/solidworks_tips/and-the-winner-is/feed 6 http://learnsolidworks.com/solidworks_tutorials/how-to-model-a-spring-in-solidworks http://learnsolidworks.com/solidworks_tutorials/how-to-model-a-spring-in-solidworks#comments Wed, 28 Dec 2011 20:04:27 +0000 Jan-Willem Zuyderduyn http://learnsolidworks.com/?p=931 In this SolidWorks tutorial I will show you how to model a spiral spring in SolidWorks. Spring steel is a low alloy, medium carbon steel or high carbon steel with a very high yield strength. This allows objects made of spring steel to return to their original shape despite significant bending or twisting. But how can you draw a shape like a spiral or spring in SolidWorks? This is exactly what I want to show you today.

In this tutorial you will learn how to use the following functions:

• 2D sketch
• Create a 2D Circle
• Create a Helix / Spiral
• Create a Swept Boss/Base

Enjoy it!

Open a new part with model units set to millimeters

Go to: File > New > Part

I made the global shape of this sleigh in SolidWorks. Afterwards I made a render and placed it into a Christmas scene (with Adobe Photoshop). Feel free to download my SolidWorks model to see how it’s made in SolidWorks.

JOIN THE LEARNSOLIDWORKS RENDER CONTEST!

I challenge you to participate the LearnSolidWorks Render Contest. For this contest I ask you to create an eye-catching and spectacular render of Santa’s futuristic toy! You can win one of my SolidWorks Tutorial Courses:

1st Place = SolidWorks Chopper Tutorial & SolidWorks iPhone Tutorial

2nd Place = SolidWorks Chopper Tutorial

3th Place = SolidWorks iPhone Tutorial

The deadline is January 2, 2012. The winners will be announced on January 3, 2012. You can drop your best renders here: http://grabcad.com/library/santas-sleigh-2-dot-0

And of course I also want to wish you a very

MERRY CHRISTMAS AND A HAPPY 2012!

2012 will be a year filled with many SolidWorks Tips, Tricks and Tutorials. I will teach you how to learn SolidWorks with many new exciting SolidWorks tutorials. I will also provide you with detailed SolidWorks models and free E-books like the SolidWorks Panton Chair Tutorial

Click here to download the SolidWorks file (SW2011) and renders of the SolidWorks sleigh:

]]> http://learnsolidworks.com/solidworks_model_downloads/santas-sled-2-0-in-solidworks/feed 15 http://learnsolidworks.com/solidworks_tutorials/new-solidworks-photoview-360-iphone-tutorial http://learnsolidworks.com/solidworks_tutorials/new-solidworks-photoview-360-iphone-tutorial#comments Fri, 09 Dec 2011 11:47:31 +0000 Jan-Willem Zuyderduyn http://learnsolidworks.com/?p=634 Dear SolidWorks,

I am proud to announce that my newest SolidWorks & PhotoView 360 Tutorial is available! In this SolidWorks starter tutorial I will show you how to model the Apple iPhone 4S in SolidWorks and how to render it in PhotoView 360.

Download this exclusive SolidWorks Tutorial Package here including a SolidWorks Kit Car Model for FREE! 

The iPhone is a line of Internet and Multimedia enabled smartphones marketed by Apple. Steve Jobs was the CEO and spirit behind Apple. On October 5, 2011 Steve Jobs passed on Steve was one of the most groundbreaking entrepreneurs of the century. He has literally changed the world with products like the iMac, iPod, iPad and of course the iPhone.

To keep the memory of Steve’s work alive I thought it would be great to write a SolidWorks and PhotoView 360 tutorial about his latest creation, the iPhone 4S.

“Design is not just what it looks like and feels like. Design is how it works.” – R.I.P. Steve Jobs

I’ve developed a Step-by-Step SolidWorks Starter Tutorial to learn how to Model and Render an iPhone 4S in SolidWorks and PhotoView 360 without any SolidWorks experience.

The newest tutorial package of LearnSolidWorks contains the following:

       SolidWorks Modeling Tutorial for the iPhone 4S

       SolidWorks Model of the iPhone 4S

      PhotoView 360 Render Tutorial

      Bonus 1  Free SolidWorks Model of the iPhone charger

      Bonus 2  Free SolidWorks Model of the iPhone 3G

      Bonus 3  Free SolidWorks Model of the iPad

In this SolidWorks Tutorial you will learn how to:

• Create 2D Sketches
• Create Center Rectangles
• Create Corner Rectangles
• Create a Sketch Offset
• Create Text
• Create Extrudes
• Create Cut Extrudes
• Create Chamfers
• Create Revolved Cut
• Create Fillets
• Create Surface Fills
• Create Straight Slots
• Create a Linear Pattern
• Create Sketch Fillets
• Mirror Features
• Change Colors
• Import a Sketch

 ONE TIME OFFER 

We will celebrate the launch of our newest tutorial with a Unique One Time Offer. When you decide to order the iPhone tutorial package you’ll receive temporary a SolidWorks model of a complete Burton kitcar FOR FREE (Regulary price €39)! I modeled this unique car (150+ parts) for the European SolidWorks Car Design Contest in 2008 and ended in the Top 3.

The Feature Manager Design Tree of this kitcar shows how this highly detailed car is modeled by using SolidWorks. You can also use it as a render object for your brand new PhotoView 360 tutorial.

Are you also interested in designing your own Apps and Games for the iPhone and iPad? This might be interesting for you.

One of the ambitions of Verner Panton was to create a plastic chair molded in one single piece. Panton searched a long time for a manufacturer of this modern chair. Finally he found the company Vitra to develop the chair for series production. The Panton chair received many different awards and is now recognized as a classic of modern furniture design.

Because the shape of this chair is so organic and challenging (especially for SolidWorks users) I thought it would be great to make a SolidWorks tutorial about this chair.

In this tutorial you will learn how to use the following functions:

• Draw 2D Sketches
• Draw 3D Sketches
• Insert a Blueprint or Reference Picture
• Improve the shape of a Spline
• Create new Planes
• Create Projected Curves
• Pierce Multiple Sketches with each other
• Create Surface Lofts
• Use Guide Curves
• Hide Bodies
• Hide Pictures
• Knit Surfaces
• Solidify Surface Bodies
• Create Fillets
• Create Variable Fillets
• Change Display Styles
• Mirror and Merge bodies
• Change Colors
• Create Wall Thickness

I hope you will learn something from it. Feel free to share this tutorial with your friends on Facebook, Twitter or Linkedin with the social sharebar at the left side. I am also looking forward to your opinion about LearnSolidWorks.com

In this tutorial you will learn how to use the following functions:

• 2D sketch
• Insert a photo
• Change Transparency
• Revolve
• Fillet
• Shell

Enjoy it!

PhotoView360 visualisation of a double walled Bodum glass

Open a new part with model units set to millimeters

Go to: File > New > Part

Create a 2D sketch

Select the Front Plane in the feature tree (menu at the left side) and create a

sketch by clicking on the 2D Sketch icon 

The display changes so the Front plane faces you.

Insert a reference photo

For this tutorial we use a photo of a Bodum glass to approach the nice shape as good as possible.

Download the photo here and save it into your SolidWorks folder

Go to: Tools > Sketch Tools > Sketch Picture 

Go to your SolidWorks folder and select the photo “SIDEVIEW_BODUM_GLASS.Jpg”

Click: Open

Change the dimensions and position of the photo with the menu as shown in the picture.

Select ‘’Full image’’ in the Transparency tab and change the transparency into 0.50

Click OK 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create another 2D sketch

Select the Front Plane again and create another sketch by clicking on the 2D Sketch icon 

Draw two centerlines

Go to Tools > Sketch Entities > Centerline or click at the Centerline icon 

Draw a vertical centerline that starts at the origin. 

Change the length of the line into 61 mm by clicking at the dimension button 

Draw a horizontal centerline that starts at the upper endpoint of the vertical centerline

Change the length of the line into 26 mm by clicking at the dimension button 

Draw three solid lines

Go to Tools > Sketch Entities > Line or click at the Line icon 

Draw the three lines as shown in the picture

Change the lengths of the lines by clicking at the dimension button 

Draw a spline without midpoints

Go to Tools > Sketch Entities > Spline or click at the Spline icon 

Draw a spline as shown in the picture without a midpoint

Right mouse button > Select

Change the curve of the Spline like the picture

Click at the Top point of the spline > The grey arrows of the Spline appear

Click and drag the round endpoint of the grey arrow as shown in the picture (the orange dot)

Click at the Lower point of the spline > The grey arrows of the Spline appear

Click and drag the round endpoint of the grey arrow as shown in the picture (the orange dot)

Try to create the curve of the glass as shown in the picture

Draw a second spline without midpoints

Go to Tools > Sketch Entities > Spline or click at the Spline icon 

Draw a spline as shown in the picture without a midpoint

Right mouse button > Select

Change the curve of the Spline like the picture

Click at the Top point of the spline > The grey arrows of the Spline appear

Click and drag the round endpoint of the grey arrow as shown in the picture (the orange dot)

Click at the Lower point of the spline > The grey arrows of the Spline appear

Click and drag the round endpoint of the grey arrow as shown in the picture (the orange dot)

Try to create the curve of the glass as shown in the picture

Add a tangency relation add the end of the spline

Click at the orange dot as shown in the picture

Select the Horizontal relation in the Spline menu bar at the left side 

The endpoint of the spline is fully tangent now

Create a Revolve

Go to Insert > Boss/Base > Revolve or click at the Revolve icon 

Click at the vertical Centerline to define the Axis of Revolution 

Use the One-Direction option 

Set the Revolution Angle to 360 degrees 

Click OK 

Create two Fillets

Go to: Insert > Features > Fillet/Round or click at the Fillet icon  

Click at the blue edges as shown in the picture

Change the Radius into 1 mm 

Click OK 

Create another Fillet

Go to: Insert > Features > Fillet/Round or click at the Fillet icon  

Click at the blue edges as shown in the picture

Change the Radius into 5 mm 

Click OK 

Change the transparency of the glass

Select an arbitrary face of the glass

Click at the appearances button 

Click at the Part name 

Click at the dropdown menu called ‘’standard’’

Select the Transparent option

Change the color into white

Click OK 

Create a Shell

Now it’s time to convert the Solid glass into a double walled glass. We will use the Shell feature for  this.

Go to: Insert > Features > Shell or click at the Shell icon 

Change the Thickness into 1 mm 

Click OK 

Congratulations, you just finished your own double walled drinking glass!

Feel free to leave a comment below or to share this tutorial

Click here to download the Photo and SolidWorks file of the Double Walled Bodum Glass

Philippe Starck is a famous French designer. He’s one of the best known designers in the New Design style. The design of Starck range from a luxury private yacht to mass produced consumer products such as chairs, dinnerwair and even complete houses. This citrus suqeezer is also called ‘’Juicy Salif’’ It may look like a spider at a first glance. While this juice squeezer does not serve as a practical tool, it is eye-catching and provocative. I thought it would be awesome to make a SolidWorks tutorial about this famous design squeezer.

In this tutorial I will show you the following features:

• Draw 2D sketches
• Insert a blueprint
• Create a new Plane
• Create a new Axis
• Surface Fill
• Surface Knit
• Solidify surfaces
• Circular Pattern
• Surface Loft
• Solid Loft
• Fillet

I hope you will learn something from it.

Enjoy it!

Render of Starck’s Citrus Squeezer rendered in PhotoView360

Open a new part with model units set to millimeters

Go to: File > New > Part 

Create a 2D sketch

Select the Front Plane in the feature tree (menu at the left side) and create a sketch by clicking on the 2D Sketch icon 

The display changes so the Front plane faces you.

Insert a blueprint

For this tutorial we use a blueprint of the citrus squeezer to create the organic shape.

Download the blueprint here and save it into your SolidWorks folder

Go to: Tools > Sketch Tools > Sketch Picture 

Go to your SolidWorks folder and select the blueprint “SIDEVIEW_CITRUS_SQUEEZER.Jpg”

Click: Open

Change the dimensions and position of the blueprint with the menu as shown in the picture.

Select ‘’Full image’’ in the Transparency tab and change the transparency into 0.50

Click OK 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create another 2D sketch

Select the Front Plane again and create another sketch by clicking on the 2D Sketch icon 

Draw two centerlines

Go to Tools > Sketch Entities > Centerline or click at the Centerline icon 

Draw a vertical centerline that starts at the origin. 

Change the length of the line into 162 mm by clicking at the dimension button 

Draw a horizontal centerline that starts at the origin. 

Change the length of the line into 59 mm by clicking at the dimension button 

Draw a vertical line

Go to Tools > Sketch Entities > Line or click at the Line icon 

Draw a vertical line that starts at the top of the vertical construction line

Change the length of the line into 128 mm by clicking at the dimension button 

Draw a spline without midpoints

Go to Tools > Sketch Entities > Spline or click at the Spline icon 

Draw a spline, starting at the top point of the solid line and ending at the bottom point of the solid line.

Right mouse button > Select

Click at the Top point of the spline > The grey arrows of the Spline appear as shown in the orange circle

Click and drag the round endpoint of the grey arrow as shown in the picture (the orange dot)

Try to create the inner curve of the blueprint as shown in the picture

Add a tangency relation add the end of the spline

Click at the orange dot as shown in the picture

Select the Horizontal relation in the Spline menu bar at the left side 

The endpoint of the spline is fully tangent now

Click at the Sketch button in the upper right corner close the 2D Sketch 

Fill the sketch with a surface

Go to Insert > Surface > Fill or click at the Fill icon 

Select ‘’Sketch 2’’ in the feature tree as Patch Boundary sketch 

Click OK 

Create a Circular Pattern

Go to Insert > Pattern/Mirror > Circular Pattern or click at the Circular Pattern icon 

Click in the ‘’Parameters’’ box at the white Pattern-Axis box 

Select the vertical edge of the surface fill as shown in the picture

Change the Total Angle into 360 degrees 

Change the Number of Instances into 12 

Select the ’’Equal Spacing’’ option

Click at the ‘’Bodies to Pattern’’ box

Select Surface-Fill1 as ‘’Surface to Pattern’’ 

Click OK 

Create a Surface Loft 

Go to Insert > Surface > Loft or click at the Surface icon 

Click in the Profiles box 

Select two outer edges of the Circular Pattern as shown in the picture

Click at the arrow of the Start/End Constraints box to expand this menu

Change the ‘’Start Constraint’’ into Tangency To Face

Change the ‘’Start Tangent Length’’ into 4

Select the Apply to all box

Change the ‘’End Constraint’’ into Tangency To Face

Change the ‘’End Tangent Length’’ into 4

Select the Apply to all box

Make sure that the shape of the Loft looks like the one in the picture. If not, try to change the direction of the Tangency to face by clicking on the ‘’Reverse Tangent Direction’’ button 

Click OK 

Hide all surface bodies except the Surface Loft

Expand the Surface Bodies map in the Feature Tree 

Select all Surfaces except Surface-Loft1

Click at the Glasses to hide the Surface Bodies 

Create an Axis

Go to Insert >Reference Geometry > Axis or click at the Axis icon 

Select the ‘’Two Points/Vertices’’ option 

Click at one of the endpoints of the Surface Loft

Hold down the Control key

Select the other endpoint of the Surface Loft as well

Click OK 

Create another Circular Pattern

Go to Insert > Pattern/Mirror > Circular Pattern or click at the Circular Pattern icon 

Click in the ‘’Parameters’’ box at the white Pattern-Axis box 

Select the new Axis1 as Pattern Axis

Change the Total Angle into 360 degrees 

Change the Number of Instances into 12 

Select the ’’Equal Spacing’’ option

Click at the ‘’Bodies to Pattern’’ box

Select Surface-Loft1 as ‘’Surface to Pattern’’ 

Click OK 

Knit the 12 surfaces and create a solid body

Go to Insert > Surface > Knit or click at the Surface Knit icon 

Click in the Selections box and select the 12 Surface Lofts 

Select the ‘’Try to form solid’’ option

Select the “Merge entities” option

Deselect the ‘’Gap Control’’ option

Click OK 

Create another 2D sketch

Select the Front Plane and create a sketch by clicking on the 2D Sketch icon 

Draw a centerline

Go to Tools > Sketch Entities > Centerline or click at the Centerline icon 

Draw a diagonal centerline

Change the dimensions of the centerline by clicking at the dimension button 

Add the dimensions as shown in the picture

This single centerline we will use to create a new plane

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create a new plane

Go to: Insert > Reference Geometry > Plane or click at the New Plane icon 

Select the new Sketch3 in the feature tree

Hold the Control button and select the Front Plane as shown in the picture

The new plane appears in blue

Click OK 

Create another 2D sketch

Select the new Plane1 and create a sketch by clicking on the 2D Sketch icon 

Convert Sketch 3 into the new Sketch4

Click at the grey centerline of Sketch3

Go to: Tools > Sketch Tools > Convert Entities or click at the Convert Entities icon 

Click OK 

Change the solid line into a centerline

Click at the new line > Select the For Construction option in the menu at the left side

Create an Ellipse

Go to: Tools > Sketch Entities > Ellipse or click at the Ellipse icon 

Start the Ellipse at the midpoint of the centerline

Click at one of the ends of the centerline to set the height of the Ellipse

Click somewhere next to the construction line to set the width of the Ellipse

Change the width by clicking at the dimension button 

The Ellipse is fully defined

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create another 2D sketch

Select the Top Plane and create a sketch by clicking on the 2D Sketch icon 

Create a circle at the end of the construction line of Sketch2

Go to: Tools > Sketch Entities > Circle or click at the Circle icon 

Draw a circle witch starts at the endpoint of the construction line of Sketch3

Change the dimension of the circle into 8 mm  as shown in the picture 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create another 2D sketch

Select the Front Plane and create a sketch by clicking on the 2D Sketch icon 

Draw a spline without midpoints

Go to: Tools > Sketch Entities > Spline or click at the Spline icon 

Connect the Spline with Sketch4 and Sketch5

Select the upper endpoint of the Spline

Hold down the Control key on your keyboard

Click at the lower endpoint of the Ellipse in Sketch4 as shown in the picture

Click at the Coincident icon in the Add Relations box 

Click OK 

Select the lower endpoint of the Spline

Hold down the left key of your mouse and drag the spline to the circle of Sketch5.

SolidWorks will automatically add a Coincident relation with the circle. 

Make sure that the Spline is connected with the edge of the circle instead of the center as shown in the picture

The spline is now connected with two different Sketches

Click OK 

Change viewport to Front Plane

Click at Control+1 or click at the View Orientation box  and click at Front Plane

Change the curve of the Spline like the blueprint

Click at the Top point of the spline > The grey arrows of the Spline appear

Click and drag the round endpoint of the grey arrow as shown in the picture (the orange dot)

Try to create the curve of the blueprint as shown in the picture

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create a Solid Loft

Go to: Insert > Boss/Base > Loft or click at the Loft icon 

Click in the Profiles box 

Select Sketch4 and Sketch5 as shown in the picture

NOTE: The easiest way to select all the profiles and curves for this loft is to select them in the feature tree. This avoids errors and saves time.

Click in the Guide Curves box 

Select Sketch6 as shown in the picture

Guide curves influence: To Next Guide

Click OK 

Create another 2D sketch

Select the Right Plane and create a sketch by clicking on the 2D Sketch icon 

Create a circle

Go to: Tools > Sketch Entities > Circle or click at the Circle icon 

Draw a circle witch starts at the Right Plane as shown in the picture

Change the dimension of the circle into 12 mm  as shown in the picture 

Change the height of the circle into 195 mm starting at the origin 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create a Solid Loft

Go to: Insert > Boss/Base > Loft or click at the Loft icon 

Click in the Profiles box 

Select the new Sketch7

Select the outer edge of Loft1 as shown in the picture

Click OK 

Create a Fillet

Go to: Insert > Features > Fillet/Round or click at the Fillet icon 

Click at the blue edge as shown in the picture

Change the Radius into 2 mm 

Click OK 

Create a Fillet

Go to: Insert > Features > Fillet/Round or click at the Fillet icon 

Click at the blue edge as shown in the picture

Change the Radius into 2 mm 

Click OK 

Create a Circular Pattern

Go to Insert > Pattern/Mirror > Circular Pattern or click at the Circular Pattern icon 

Click in the ‘’Parameters’’ box at the white Pattern-Axis box 

Select Axis1

Change the Total Angle into 360 degrees

Change the Number of Instances into 3 

Select the ’’Equal Spacing’’ option

Click at the ‘’Features to Pattern’’ box

Select Loft1, Loft2, Fillet1, Fillet2 in the feature tree as shown in the picture

Click OK 

Congratulations, you just finished your own Citrus Squeezer!

Citrus Squeezer in SolidWorks                                              Citrus Squeezer l in PhotoView360

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Click here to download the Blueprint and SolidWorks file of the Philippe Starck Citrus Squeezer

In this tutorial you will learn how to use the following functions:

• 2D sketch
• Extruded Boss/Base
• Thin Extrude
• Multi-directed Extrude
• Mirror
• Chamfer

When the model is finished I will show you four different ways to add a color to your part.

Enjoy it!

Render of the final Rietveld Chair in PhotoView360

Open a new part with model units set to millimeters

Go to: File > New > Part 

Create a 2D sketch

Select the Right Plane in the feature tree (menu at the left side) and create a

sketch by clicking on the 2D Sketch icon 

The display changes so the Right plane faces you.

Create a straight line

Go to Tools > Sketch Entities > Line or click at the Line icon 

Draw a diagonal line that starts at the origin. 

Change the length of the line into 900 mm by clicking at the dimension button

Add a Smart Dimension of 63 degrees to the line by clicking on the diagonal line and clicking on the horizontal plane as shown in the picture.

Create an Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

Select the diagonal line

Change   into 179 mm

Enable the Thin Feature option

Change  into 15 mm

Make sure that the extrusion is directed upward and forward as shown in the picture.

If the direction is wrong, change it with the ‘‘Reverse Direction’’ button. 

Click OK 

Create another 2D sketch

Select the Right Plane and create a sketch by clicking on the 2D Sketch icon 

Create a diagonal Line

Go to Tools > Sketch Entities > Line or click at the Line icon 

Create a diagonal line as shown in the picture.

Change the length and position of the line by clicking at the dimension button 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create another Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

Select the diagonal line

Change  into 210 mm

Enable the Thin Feature option

Change  into 15 mm

Make sure that the extrusion is directed upward and forward as shown in the picture.

If the direction is wrong, change it with the ‘‘Reverse Direction’’ button. 

Click OK 

Create a Chamfer

Go to: Insert > Features >Chamfer or click at the Chamfer icon 

Select the light blue edge as shown in the picture

Select the ‘’Distance to distance’’ option

Change  into 460 mm

Change  into 25 mm

Click OK 

Create another 2D sketch

Select the Right Plane and create a sketch by clicking on the 2D Sketch icon 

Create five fully defined squares

Go to Tools > Sketch Entities > Center Rectangle or click at the Center Rectangle icon 

Create the five squares as shown in the picture.

Change the length and position of the squares by clicking at the dimension button 

Click at the Sketch button in the upper right corner close the 2D Sketch 

Create another Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

Select the diagonal line

Change  into 300 mm

Make sure that the extrusion is directed forward as shown in the picture.

If the direction is wrong, change it with the ‘’Reverse Direction’’ button. 

Click OK 

Create another 2D sketch

Select the blue surface and create a sketch by clicking on the 2D Sketch icon 

Go to Tools > Sketch Entities > Corner Rectangle or click at the Corner Rectangle icon 

Create the rectangle as shown in the picture.

Change the length and position of the rectangle by clicking at the dimension button 

Create another Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

Select the rectangle

Change  into 30 mm

Make sure that the extrusion is directed forward as shown in the picture.

If the direction is wrong, change it with the ‘’Reverse Direction’’ button. 

Click OK 

Create another 2D sketch

Select the blue surface and create a sketch by clicking on the 2D Sketch icon 

Go to Tools > Sketch Entities > Corner Rectangle or click at the Corner Rectangle icon 

Create the rectangle as shown in the picture.

Change the length and position of the rectangle by clicking at the dimension button 

Create another Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

Select the rectangle

Change  into 30 mm

Make sure that the extrusion is directed forward as shown in the picture.

If the direction is wrong, change it with the ‘’Reverse Direction’’ button. 

Click OK 

Create another 2D sketch

Select the blue surface and create a sketch by clicking on the 2D Sketch icon 

Go to Tools > Sketch Entities > Corner Rectangle or click at the Corner Rectangle icon 

Create the rectangle as shown in the picture.

Change the length and position of the rectangle by clicking at the dimension button 

Create another Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

Select the rectangle

Change   into 484 mm

Make sure that the extrusion is directed forward as shown in the picture.

If the direction is wrong, change it with the ‘’Reverse Direction’’ button. 

Click OK 

Create another 2D sketch

Select the blue surface and create a sketch by clicking on the 2D Sketch icon 

Go to Tools > Sketch Entities > Corner Rectangle or click at the Corner Rectangle icon 

Create the rectangle as shown in the picture.

Change the length and position of the rectangle by clicking at the dimension button 

Create another Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

Select the rectangle

Change  into 430 mm

Make sure that the extrusion is directed forward as shown in the picture.

If the direction is wrong, change it with the ‘’Reverse Direction’’ button. 

Click OK 

Create another 2D sketch

Select the blue surface and create a sketch by clicking on the 2D Sketch icon 

Go to Tools > Sketch Entities > Corner Rectangle or click at the Corner Rectangle icon 

Create the rectangle as shown in the picture.

Change the length and position of the rectangle by clicking at the dimension button 

Create a multi-direction Extruded Boss/Base

Go to: Insert > Boss/Base > Extrude or click at the Extrude icon 

Select the rectangle

Change   into 655 mm

Enable the Direction 2 option

Change  into 35 mm

Make sure that the extrusions are directed as shown in the picture.

If the direction is wrong, change it with the ‘’Reverse Direction’’ button. 

Click OK 

Mirror and merge the chair

Go to: Insert > Pattern/Mirror > Mirror 

Mirror Face/Plane  : Right Plane

Select the “Bodies to Mirror” option

Select the Merge solids’’ option

Bodies to Mirror  : Select the blue bodies you want to mirror. Note: the ‘’Mirror and Merge’’ option is only available for ‘’half’’ parts as shown in the picture.

Click OK 

Mirror the remaining body

Go to: Insert > Pattern/Mirror > Mirror 

Mirror Face/Plane  : Right Plane

Select the “Bodies to Mirror” option

Bodies to Mirror  : Select the remaining body as shown in the picture. Uncheck the ‘’Merge Solids’’ option

Click OK 

Change the colors of the chair

Select a face of the chair and click at the Appearances button 

A small menu bar pops up as shown in the picture

There are four ways to add colors to your part.

Surface color     Provide one- or multiple specific surfaces with a color by clicking at the ‘’Face’’ option

Feature color     Provide one- or multiple specific features with a color by clicking at the ‘’Feature name’’ option

Body color     Provide one or multiple specific bodies with a color by clicking at the ‘’Body’’ option

Part color     Provide a complete part with a color by clicking at the ‘’Part Name’’ option

The color of a single face is leading above the feature color, the features color is leading above the body color and so on.

We will try to use all the different ways to add a color to this chair.

Change the Part color

Select an arbitrary face of the chair

Click at the Appearances button 

Click at the Part name 

Change the color into dark grey or black

Click OK 

Change a Body color

Select an arbitrary face of the back

Click at the Appearances button 

Click at the Body option 

Change the color into red

Click OK 

Change a Feature color

Select the top and one side face of the seat (Extrude-Thin2 and Chamfer1 in the feature tree)

Click at the Appearances button 

Click at the Features option 

Change the color into blue

Click OK 

(Because the seat is one single body you can also use the Body option)

Change a Face color

Select all the ends of the black beams as shown in the picture

Click at the Appearances button 

Click at the Face option 

Change the color into yellow

Click OK 

Congratulations, you just finished your own Rietveld Chair!

Well, that’s all for now. I hope you learned something from this tutorial! Feel free to leave a message below.

Click here to download the SolidWorks files of the Rietveld Chair