How to model an interlinked star geometry in SOLIDWORKS?

Some shapes seem to be impossible to model in SOLIDWORKS… The interlinked star geometry as shown in the renderings below seems one of these shapes. But actually it’s not that hard at all.

In today’s lesson, you will discover how to model this amazing piece of art yourself! We will use many different features throughout this tutorial.

I hope you like it!

Jan

P.S. I encourage you to share this tutorial with your network.

Click here to download this SOLIDWORKS tutorial as a free eBook (PDF).

Open a New Part with model units set to millimeters

Go to: File > New > Part

Save the file with the following name: Interlinked Star Geometry.SLDPRT  

Create a 2D Sketch on the Top Plane

Select the Top Plane from the Features tree and click on the sketch icon 

Go to: Tools > Sketch Entities > Polygon 

Draw a construction pentagon concentric to the origin and assign a vertical relation to one of the lines

Go to: Tools > Dimensions > Smart 

Click on the vertical line and add a length of 50mm

Go to: Tools > Sketch Entities > Centerline

Draw a vertical construction line inside the pentagon, as shown in the image below.

Go to: Tools > Sketch Entities > Polygon 

Draw a construction pentagon concentric to the origin in the same orientation as the previous pentagon.

Select the existing vertical construction line and select the vertical edge of the bigger pentagon by holding down the CTRL Key and assign an equal relation  between them.

Click on Close sketch  to close the 2D sketch.

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 > Centerline

Draw two construction lines coincident to the corners of the pentagons

Go to: Tools > Dimensions > Smart

Click on the diagonal construction line and assign a length of 50mm

Click on Close sketch  to close the 2D sketch.

Create a Reference Plane

Go to:  Insert > Reference Geometry > Plane…

Click on the two construction lines which are highlighted with pink and purple colour in the picture.

Click OK  to complete the operation.

Create a 2D Sketch on Plane1

Select Plane1 in the features tree and click on the sketch icon

Click on the Normal To  icon to get a normal to view on the new plane

Draw a construction pentagon coincident to the existing sketches as shown in the picture below

Click on Close sketch  to close the 2D sketch.

Create a Reference Axis

Go to:  Insert > Reference Geometry > Axis…

Select the Point and Face/ Plane  option from the property manager

Click on the center point of the first pentagon and select the Top Plane

A yellow axis gets highlighted as shown in the picture below

Click OK to complete the operation.

Create a second reference axis

Go to:  Insert > Reference Geometry > Axis…

Select the Point and Face/ Plane option from the property manager

Click on the center point of the second pentagon and select Plane1

A yellow axis gets highlighted as shown in the picture below

Click OK to complete the operation.

Create a Reference Point

Go to: Insert > Reference Geometry > Point…

Select the Intersection  option from the property manager

Click on Axis1 and Axis2 to create an intersection point (Point1)

The purple intersection point gets highlighted as shown in the image below

Click OK  to complete the 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 Entities > CenterPoint Arc 

Draw a quarter circle concentric to Point1

Go to: Tools > Dimensions > Smart 

Click on the arc and assign a radius of 70mm, as shown in the picture below

Click on Close sketch  to close the 2D sketch.

Create a Revolve

Go to: Insert > Surface > Revolve…  or click on the Revolved Surface

Select Axis1 as Axis of revolution, as shown in the picture below

Click OK  to complete the operation.

Create a 2D Sketch on the Top Plane

Select the Top Plane from the features tree and click on the sketch icon 

Go to: Tools > Sketch Entities > Circle 

Draw a construction circle concentric to the origin

Go to: Tools > Dimensions > Smart

Click on the circle and assign a diameter of 40mm

Go to: Tools > Sketch Entities > Center Line 

Draw a horizontal construction line and draw another line at an angle of 72 degrees as shown in the picture below

Go to: Tools > Sketch Entities > Offset Entities

Select both construction lines and assign an inward offset distance  of 3mm, as shown in the picture below

Make sure that Add dimensions and Offset geometry are both checked in the property manager

Go to: Tools > Sketch Entities > Spline 

Draw a spline by using the endpoints of the offset lines

Click on the spline, drag the spline handles one by one and assign a Collinear Relation  to the spline handles by clicking on the endpoint of the spline, hold down the Ctrl key and select the construction line, as shown in the picture below.

Go to: Tools > Dimensions > Smart

Click on each handle and assign a value of 40mm as a handle length

Go to: Tools > Sketch Entities > Line

Draw a vertical line of 6mm as shown in the picture below

Go to: Tools > Sketch Tools > Circular Pattern… 

Select the spline and the vertical line as Pattern Entities 

Go to the property manager and change the number of instances to 5, as shown in the picture below

Make sure that Equal spacing is checked in the property manager

Click OK  to complete the operation.

Make a Surface Trim

Go to:  Insert > Surface > Trim… 

Select the center of the sketch as shown in the picture below (purple area)

Go to the property manager and select Keep Selections and leave other parameters as default

Click OK  to complete the operation.

Create a Reference Plane (Plane2)

Go to: Insert > Reference Geometry > Plane… 

Select the three points which are highlighted with Pink, Blue and Green as shown in the picture below

Click OK  to complete the operation.

Create a new Reference Plane (Plane3)

Go to: Insert > Reference Geometry > Plane… 

Select Plane2 then automatically Plane3 will be generated parallel to Plane2

Go to the property manager and change the offset distance into 5mm

Make sure that the Flip offset option is checked in the property manager so the Plane is directed inwards

Click OK  to complete the operation.

Go to the feature tree and select Sketch1, Sketch2, Sketch3 and Plane2, and Hide  them

Create a new 2D sketch on Plane3

Select Plane3 from the Features Tree and click on the sketch icon 

Click on the Normal To  icon to get a view normal to Plane3

Go to: Tools > Sketch Entities > Circle

Draw a construction circle with a diameter of 30mm concentric to Point1

Go to: Tools > Sketch Entities > Centerline 

Draw a vertical construction line

And draw a second construction line at an angle of 120 degrees, as shown in the picture below

Go to: Tools > Sketch Entities > Offset Entities

Select both construction lines and add an offset distance  of 3mm, as shown in the picture below

Make sure that Add dimensions and Offset geometry are checked in the property manager

Go to: Tools > Sketch Entities > Spline 

Draw a spline by using the endpoints of the offset lines

Click on the spline, drag the spline handles one by one and assign a Collinear Relation  to the spline handles collinear to the underlying construction lines, as shown in the picture below

Go to: Tools > Dimensions > Smart 

Click on each handle and assign a value of 30mm as a handle length

Go to: Tools > Sketch Entities > Line 

Draw a horizontal line of 6mm as shown in the picture

Go to: Tools > Sketch Tools > Circular Pattern…

Select the spline and the horizontal line as pattern entities

By default, the pattern will be generated around the origin with 4 Instances

Go to the property manager, Right click on the parameter box  and select Clear selections

Move the cursor and select Point1 as a new parameter

Move down in the property manager and change the number of instances into 3, as shown in the picture below

Click OK to complete the operation.

Click on Close sketch  to close the 2D sketch.

Create a Planer Surface

Go to: Insert > Surface > Planer…

Select Sketch6 from the Feature Tree

Then, a yellow planer surface is generated as shown in the picture below

Click OK  to complete the operation.

Use the Move/ Copy Body feature

Go to: Insert > Features > Move/ Copy… 

Select the blue surface as shown in the picture below

Go to the property manager and click on the Rotate  box

Go to the modelling area and select Axis1 as a reference axis

Change the rotation value into –18 degrees as shown in the picture below

Click OK to complete the operation.

Create a 2D Sketch on the Planer Surface

Select Surface-Plane1 from the Feature Tree and click on the sketch icon

Click on the Normal To  icon to get a better view normal to plane 3

Go to: Tools > Sketch Entities > Line

Draw three Lines (one vertical construction line and two solid lines) and add the dimensions, as shown in the picture below

Make a Surface Trim

Go to: Insert > Surface > Trim…

Select the purple surface as shown in the picture below

Go to the property manager and select Keep Selections and leave other parameters as default

Click OK to complete the operation.

Create a 2D Sketch on the Top Plane

Select the Top Plane from the Features Tree and click on the sketch icon

Click on the Normal To  icon to get a view normal to the Top Plane

Go to: Insert > Sketch Entities > Line

Draw a vertical line from the origin

Draw another line at an angle of 72 degrees

Make a Surface Trim

Go to: Insert > Surface > Trim… 

Select the purple surface as shown in the picture below

Go to the property manager and select Keep Selections and leave the other parameters as default

Click OK to complete the operation.

Create a Loft Surface

Go to: Insert > Surface > Loft…

Select the two 6mm edges as loft profiles  as shown in the picture below

Go to the property manager, and click on start/ end constraints

Add a Tangency to Face with a tangent length of 3

Also add a Tangency to Face of 3 for the End Constraints

Click OK  to complete the operation.

Knit the 3 surfaces

Go to:  Insert > Surface > Knit

Select the three surfaces as shown in the picture below and check Merge entities

Click OK  to complete the operation.

Create a Thicken

Go to: Insert > Boss/ Base > Thicken 

Select the existing Knitted surface as knit parameter  from the modelling area

Go to the property manager and select the ‘Both side Thicken’  option

Assign a Thickness  of 3mm

Click OK  to complete the operation.

Create Fillets

Go to: Insert > Features > Fillet/Round 

Select the two lower edges of the geometry, as shown in the picture below

Go to the property manager and assign a Fillet radius  of 2.4mm

Click OK  to complete the operation.

Create a Shell

Go to: Insert > Features > Shell 

Go to the property manager and assign a shell thickness of  1.5mm

Select the 7 highlighted blue surfaces, as shown in the picture below

Click OK  to complete the operation.

Create Fillets on the top edges of the geometry

Go to: Insert > Features > Fillet/Round 

Select all the 4 upper edges of the geometry, as shown in the picture

Go to the property manager and add a Fillet radius  of 0.75mm

Click OK  to complete the operation.

Create a Circular Pattern

Go to: Insert > Pattern/Mirror > Circular Pattern 

Select Axis1 as a Reference direction

Change the Number of instances  into 5 with equal spacing 360 degrees

Select Bodies and click on the existing solid body as shown in the picture below

Click OK  to complete the operation.

Combine the bodies:

Go to: Insert > Features > Combine 

Go to the property manager and click on Add

Select the 5 blue bodies as shown in the picture below

Click OK  to complete the operation.

Save the file again  

Use the Move/ Copy Body feature

Go to: Insert > Features > Move/ Copy… 

Select the Star shaped geometry

Go to the property manager and Click on the Rotate  box

Select the small edge as a reference axis (highlighted into the black circle)

Assign a rotation value of 120 degrees

Make sure that the ‘Copy’ option is checked in the property manager

Click OK  to complete the operation.

Create a Circular Pattern

Go to: Insert > Pattern/Mirror > Circular Pattern 

Select Axis1 as a Reference direction

Change the number of instances  into 5 with an equal spacing of 360 degrees

Go down in property manager, select Bodies and click on the blue body as shown in the picture below

Click OK to complete the operation.

Combine the bodies:

Go to: Insert > Features > Combine

Select the 6 bodies in the modelling area

Go to the property manager, Click on Add

Click OK to complete the operation.

Use the Move/ Copy Body feature

Go to: Insert > Features > Move/ Copy…

Select the combined body

Go to the property manager and click on the Rotate  box

Select Point1 as rotation reference as shown in the picture below

Assign the following rotation values:

X= 0 degrees,   Y= 0 degrees, and   Z= 180 degrees

Click OK  to complete the operation.

Combine the bodies:

Go to: Insert > Features > Combine

Select both bodies in the modeling area

Go to the property manager, and click on Add

Click OK to complete the operation.

Save the file again  

Congratulations, you just finished your own Interlinked Stars Dodecahedron!

Click here to download this SOLIDWORKS tutorial as a free eBook (PDF).

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Thanks a million!

Jan