A couple of years ago I developed a SOLIDWORKS tutorial about the Juicy Salif, an amazing citrus squeezer designed for Alessi by Philippe Starck. Today we want to show you how to model another beautiful citrus squeezer of Alessi in SOLIDWORKS.
This piece of art is designed by Roland Kreiter for Alessi. It was awarded with the Pure Creativity award in 2009. This beautiful squeezer is the successor of the iconic Juicy Salif.
In this tutorial, you will discover many interesting features. One of the most remarkable features of this tutorial is the Flex feature. You will discover how to apply this feature to create a beautiful twisted shape.
Hope you like it!
Jan
P.S. Click here to download this SOLIDWORKS tutorial as a free video & eBook (PDF).
Disclaimer: The intellectual property depicted in this 3D model, is not affiliated with or endorsed by the original right holders. This 3D model may not be used for any commercial, promotional, advertising or merchandising use.
Click here to download this SOLIDWORKS tutorial as a free video & eBook (PDF).
Click here to download this SOLIDWORKS tutorial as a free video & eBook (PDF).
Open a New Part with the model units set to millimeters
Go to: File > New > Part 
Save the File with the following name: MySqueeze.SLDPRTÂ 
Create a 2D Sketch on the Front Plane
Select the Front Plane from the Features tree and click on the sketch icon
Go to: Tools > Sketch Entities > Midpoint Line 
Draw a vertical line starting from the origin
Go to: Tools > Dimensions > Smart 
Click on the vertical line and assign a length of 130mm, as shown in the image below
Go to: Tools > Sketch Entities > 3 Point Arc 
Draw a 3 Point Arc by using the end points of the vertical line
Go to: Tools > Dimensions > SmartÂ
Hold the CTRL Key and select the origin and the mid-point of the arc
Assign a horizontal distance of 30mm as shown in the image below
Click on Close sketch 
 to close the sketch area.
Create a Revolve
Go to: Insert > Boss/Base > Revolve… 
 or Click on Revolved Boss/Base
Select the Vertical line of the sketch as the Axis of revolution 
, as shown in the picture below
Click OK 
 to complete the operation.
Create a Shell
Go to: Insert > Features > Shell 
Go to the property manager and assign an inward shell thickness  of 4.5mm
Click OK Â to complete the shell operation.
Create a 2D Sketch on the Front Plane
Select the Front Plane from the Features tree and click on the sketch icon
Go to: Tools > Sketch Tools > Convert Entities 
Select the right hand side arc of the solid body (the blue highlighted arc) as shown in the image below
Click OK Â to complete the operation.
Go to: Tools > Sketch Entities > Line 
Draw an undefined vertical line from the top end of the arc
Go to: Tools > Sketch Entities > 3 Point ArcÂ
Draw a 3 Point Arc starting from the lower end of the vertical line up to the existing arc, as shown in the image below
Hold the CTRL Key, select the lower end of the vertical line and center point of the arc
Assign a Vertical Relation 
 between both points
Again, hold the CTRL Key, select the 3 point arc (Blue) and the existing arc (Black)
Assign a Tangent Relation 
 between them, as shown in the image below:
Go to: Tools > Dimensions > SmartÂ
Click on the 3 point arc and assign a radius of 3mm
Click on Close sketch  to close the sketch area.
Use the Sketch Trim
Go to: Tools > Sketch Tools > TrimÂ
Select Trim to closet 
 from the property manager
Click on the unnecessary part of the arc to trim it, as shown in the image below
Click on the Close sketch  to close the sketch area.
Create a Revolve Cut
Go to: Insert > Cut > Revolve… 
or Click on Revolved Cut
Select the Vertical line of the sketch as an Axis of revolution 
Go to the modelling area and select the recent existing 2D sketch
Click OK Â to complete the operation.
Use the Mirror feature
Go to: Insert > Pattern/Mirror > Mirror 
Go to the Property Manager, Click on Mirror Face/Plane 
Then select Top Plane from the features tree
Go to the Property Manager, Click on Features to Mirror 
Then select Cut Revolve1 from the feature tree, as shown in the image below
Click OK Â to complete the operation.
Create a 2D Sketch on the Top Plane (Sweep Profile)
Select the Top Plane from the Features tree and click on the sketch icon
Go to: Tools > Sketch Tools > Convert EntitiesÂ
Select the outer edge of the circle, as shown in the image below and convert the blue circle edge
Go to: Tools > Sketch Entities > Center Line 
Draw a horizontal construction line from the origin to the right side of the circle
Then draw a diagonal line from the origin to the circle edge
Go to: Tools > Dimensions > Smart
Assign an angle of 15 degrees between these two lines, as shown in the image below
Use the Sketch Trim
Go to: Tools > Sketch Tools > Trim 
Select Power Trim 
 from the property manager
Hold down the left mouse button and drag the cursor over the larger portion of the arc to trim it
After trimming, the sketch will look like the image below
Click OK Â to complete the operation.
Go to: Tools > Sketch Entities > LineÂ
Draw a diagonal line with an angle of 50 degrees, as shown in the picture below
Go to: Tools > Sketch Tools > Mirror 
 or click on the Mirror Entities directly
Go to the property manager, click on the Entities to Mirror  
 icon
Select both lines (Line3 and Arc2) from the 2D sketch
Go to the property manager, click on the Mirror About 
 dialog box
Select the horizontal construction line (Line1), as shown in the image below
Click OK Â to complete the operation.
Use the Sketch Fillet
Go to: Tools > Sketch Tools > Fillet… 
Click on the highlighted corner to apply the fillet, which is shown in the image below
Go to the property manager and assign the Fillet Parameters 
 2mm
Click OK Â to complete the operation.
Then click on the Close  sketch icon to close the sketch area.
Create a 2D Sketch on the Front Plane (This will become the Sweep Path)
Select the Front Plane from the Feature tree and click on the sketch icon
Go to: Tools > Sketch Entities > Midpoint LineÂ
Draw a vertical line starting from the origin
Go to: Tools > Dimensions > SmartÂ
Click on the vertical line and assign a length of 130mm
Right click on the vertical line and select this icon  to convert it into a construction line
Go to: Tools > Sketch Entities > 3 Point ArcÂ
Draw a 3 Point Arc by using the end points of the vertical construction line
Go to: Tools > Dimensions > SmartÂ
Click on the arc and assign a radius of 105mm as shown in the image below
Click on the Close sketch icon  to close the sketch area.
Use the Swept Cut Feature
Go to: Insert > Cut > Sweep… 
  or click directly on Swept Cut
Go to the property manager and click on the first dialog box 
Select the triangular sketch (Sketch3) as sweep profile
Go to the property manager and click on the second dialog box 
Select the 3 point arc (Sketch4) as swept path
Go to the property manager, click on the middle icon 
to create a swept cut in the both directions
Click OK Â to complete the swept cut operation.
Create a Reference Axis
Go to:  Insert > Reference Geometry > Axis…
Select the Two Planes 
 option from the property manager
Select the Front Plane and the Right Plane from the feature tree
A yellow axis gets highlighted as shown in the picture below
Create a Circular Pattern
Go to: Insert > Pattern/Mirror > Circular Pattern 
Select Axis1Â 
as a Reference direction
Assign a Number of instances 
 of 12 with an equal spacing of 360 degrees
Select the Features and Faces box in the property manager
Then select Cut-Sweep1 from the features tree, as shown in the image below
Click OK Â to complete the operation.
Create Fillets
Go to: Insert > Features > Fillet/Round 
Select one of the outer sharp edges of the existing solid body, then a popup icons will appear
Click on the second last icon 
to select all connected edges, as shown in the image below
Go to the property manager and assign a Fillet radius  of 1mm
Click OK Â to complete the operation.
Apply the Flex Feature
Go to: Insert > Features > Flex 
Select the existing solid body from the modeling area
Go to the property manager and select Twisting as the flex type
Assign a twist value 
 of 60 degrees
Go down in the property manager and assign the Triad values (Angular Values) about X, Y and Z Axis to position the trim planes 
 X= 90 degrees, 
 Y= 0 degrees, and 
 Z= 0 degrees
Leave the other values as default
Click OK Â to complete the operation.
Change the Appearance
Go to: PhotoView 360 > Edit Appearance… 
Select Appearances (color) >> Metal >> Steel >> Polished Steel
Double click on the Polished Steel icon
Click OKÂ Â to apply the new appearance.
Save the File againÂ
Congratulations, you’ve just created your own Lemon Squeezer in SOLIDWORKS!
Click here to download a free SOLIDWORKS file, video and eBook of this tutorial.
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Thanks a million!
Jan
1 comment. Leave new
Nice tutorial