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.
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Disclaimer: This tutorial was originally published on SOLIDWORKSTutorials.net. I really liked the tutorial and also wanted to share it with you. SOLIDWORKS Tutorials is a website that targets professionals, intermediates, and specifically beginners who are new to SOLIDWORKS by posting weekly step by step blog tutorials for its members.
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!
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Thanks a million!
Jan
10 comments. Leave new
I am getting back into solidworks and I have accepted your challenge. What is the dimension of the the larger polygon? I ask because plane 1 is not correctly placed using suggested points to construct plane1 polygon and point 1.
Hi Guy, thanks for your message. T
he length of the vertical construction line is 80,90mm. Make sure to use a 5-sided polygon then you shouldn’t have any issues.
Let me know when you have any other questions.
Cheers,
Jan
Use two construction lines instead of points
This is a great tutorial – Well done Nishant Gautam. Took me 30 minutes – the last combine operations are pretty demanding for the computer. Combine 3 takes 118 seconds on an i7 4790K. Only one issue encountered: When I hide Sketch 1 (as instructed) Solidworks 2014 won’t let me draw a circle coincident with Reference Point 1, so Sketch 1 needs to be visible.
First off: Great tutorial, very happy with the end result
I was just wondering, is there a quick way (not selecting everything separately) to change the appearance, so that it looks like the render at the end of the tutorial
Hi Marcus, you can right click on the geometry and apply the appearance to faces, features or the entire body all at once.
Hope this helps!
Jan
Manage to do it and have not worked with Solid for years, thanks for the great tutorial! 🙂
Thanks Kris, glad you liked it! 🙂
Really nice job. Congratulations!
Regards
I can’t manage to make the trim function worknig on sketch1
also when the spline are created , I need to adjust entity on the construction circle because the offseting does not keep the point coïncident
I have SW 2015