Did you ever wonder how to model a soccer ball in SOLIDWORKS? You’re about to find out! ⚽
Modeling a soccer ball in SOLIDWORKS may sound simple, but the pattern on a soccer ball consists of 12 pentagons and 20 hexagons, so it’s quite interesting to model in SOLIDWORKS.
Happy modeling!
Jan
P.S. I encourage you to share this tutorial with your network.
Click here to download this 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: Soccer Ball.SLDPRT
Create a 2D Sketch on the Top Plane
Select the Top Plane from the Feature tree and click on the sketch icon 
Go to: Tools > Sketch Entities > Polygon 
Draw a pentagon concentric to the origin
Assign a vertical relation to one of the edges
Go to: Tools > Dimensions > Smart 
Click on the vertical line and assign a length of 50mm, as shown in the image below:
Go to: Tools > Sketch Entities > Polygon
Draw a construction pentagon concentric to the origin
Assign a vertical relation to one of the edges
Go to: Tools > Dimensions > Smart
Click on the vertical line and assign a length of 100mm, as shown in the image below:
Click on Close sketch 
to close the sketch area.
Create a 2D sketch on the Front Plane
Select the Front Plane from the feature tree and click on the sketch icon
Go to: Tools > Sketch Entities > Centerline 
Draw a vertical line and an diagonal construction line coincident with the corners of the pentagons as shown in the image below:
Go to: Tools > Dimensions > Smart
Click on the diagonal construction line and assign a length of 50mm, as shown in the image below:
Click on Close sketch to close the sketch area.
Create a Reference Plane (Plane1)
Go to: Insert > Reference Geometry > Plane… 
Go to the modeling area, click on the Pink and Purple lines one by one as shown in the image below:
Click OK 
to complete the operation.
Create a 2D Sketch on the Plane1
Select the Plane1 from the feature tree and click on the sketch icon
Click on the Normal To 
icon
Go to: Tools > Sketch Entities > Polygon
Draw a random hexagon in the sketch area as shown in the image below:
Hold the Ctrl key, select a corner of the hexagon and Point1
Then assign a coincident relation 
between them
Hold the Ctrl key, select the next corner of the hexagon and Point2
Then assign a coincident relation between them, as shown in the image below:
Click on Close sketch to close the sketch area.
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 hexagon and select Plane1
A yellow axis gets highlighted, as shown in the image below:
Click OK to complete the operation.
Select Plane1 from the Feature Tree and click on the Eye 
icon from the pop-up to hide it
Create another 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 pentagon and select the Top Plane
A yellow axis gets highlighted, as shown in the image below:
Click OK to complete the operation.
Create a Reference Point 1
Go to: Insert > Reference Geometry > Point… 
Select the Intersection 
option from the property manager
Click on Axis1 and Axis2 to create the intersection point (Point1)
That intersection point gets highlighted in purple, as shown in the image:
Click OK to complete the operation.
Create a second reference point
Go to: Insert > Reference Geometry > Point…
Select the Intersection option from the property manager
Click on Axis1 and Axis2 to create the intersection point (Point2)
That intersection point gets highlighted in purple, as shown in the image:
Click OK to complete the operation.
Make a Surface Loft
Go to: Insert > Surface > Loft… 
Select Sketch1 and Point1 from the feature tree
The selected profiles 
will create a conical prismatic surface, as shown in the image below:
Make a Surface Loft
Go to: Insert > Surface > Loft…
Select Sketch2 and Point2 from the feature tree
The selected profiles will create a conical prismatic surface, 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 Feature tree and click on the sketch icon
Go to: Tools > Sketch Entities > CenterPoint Arc 
Draw a quarter circle concentric to Point1 (or Point 2)
Go to: Tools > Dimensions > Smart
Click on the arc and assign a radius of 110mm, as shown in the image below:
Go to: Tools > Sketch Entities > Offset Entities 
Select the quarter arc and assign an offset distance of 3mm in the property manager
Go down in the property manager and select the Cap Ends (Lines) option, as shown in the image below
Click OK to complete the operation.
Create a Revolve
Go to: Insert > Boss/Base > Revolve… 
or click directly on Revolved Boss/ Base
Go to the property manager and select Axis2 as an Axis of revolution 
After selecting the axis a revolved volume is generated in yellow, as shown in the image below:
Click OK to complete the operation.
Use the Split Tool
Go to: Insert > Molds > Split 
Go to the property manager and click on the Trim Tools input box
Go to the modeling area and select both the conical prismatic surfaces as a trim tool
Go to the Property Manager > Target Bodies
Choose the Selected Bodies option and click on the selected bodies box
Go to the modeling area and select the revolved solid body as a target body
Go back to the property manager and click on the Cut Bodies button
Move down in the Property manager > Resulting Bodies
Tick the three checkboxes, as shown in the image below:
Go down in the property manager and untick the Consume cut bodies
Click OK to complete the operation.
Go to the modeling area, right-click on the biggest part of the split body
Select the Eye icon from the pop-up to hide that part
Hold the Ctrl key, select the Surface – Loft1 and the Surface – Loft2 from the Feature Tree
Click on the Eye icon from the pop-up to hide both surfaces
Use the Fillet
Go to: Insert > Features > Fillet/Round 
Go to the modeling area and select all the five straight edges of the pentagonal body
Go to the property manager and assign the Fillet radius of 3mm, as shown in the image below:
Click OK to complete the operation.
Make another fillet
Go to: Insert > Features > Fillet/Round
Go to the modeling area and select the upper face of the pentagonal solid body
Go to the property manager and assign a fillet radius of 2mm, as shown in the image below
Click OK to complete the operation.
Make another Fillet
Go to: Insert > Features > Fillet/Round
Go to the modeling area and select all the six straight edges of the hexagonal body
Go to the property manager and assign a fillet radius of 3mm, as shown in the image below:
Click OK to complete the operation.
Use the Fillet
Go to: Insert > Features > Fillet/Round
Go to the modeling area and select the upper face of the hexagonal solid body
Go to the property manager and assign a fillet radius of 2mm, as shown in the image below:
Click OK to complete the operation.
Create a Circular Pattern
Go to: Insert > Pattern/Mirror > Circular Pattern 
Select Axis2 as a Reference direction 
Assign the Number of instances 
5 with equal spacing 360 degrees
Scroll down in the property manager, and thick the Bodies checkbox
Go to the modeling area and select the hexagonal solid body, as shown in the image below:
Click OK to complete the operation.
Use the Move/ Copy Body Tool
Go to: Insert > Features > Move/ Copy… 
Select the blue highlighted pentagonal and the hexagonal solid body from the modeling area
Go to the property manager, tick the Copy checkbox and assign the No. of Copies 
1
Go down in the property manager and click on the Rotate 
box
Go to the modeling area and select Axis2 as a reference axis
Assign the rotation value 
120 degrees, as shown in the image below:
Click OK to complete the operation.
Create a Circular Pattern
Go to: Insert > Pattern/Mirror > Circular Pattern
Select Axis2 as a Reference direction
Assign the Number of instances 5 with equal spacing 360 degrees
Go down in the property manager, select the Bodies checkbox
Go back to the modeling area and select the copies of the pentagonal and the hexagonal solid body
The selected bodies are highlighted in blue as shown in the image below:
Click OK to complete the operation.
Use the Combine feature:
Go to: Insert > Features > Combine 
Select all the 16 solid bodies from the modeling area (manually or by the box selection)
Go to the property manager and choose the operation type Add, as shown in the image below:
Click OK to complete the operation.
Use the Move/ Copy Body Tool
Go to: Insert > Features > Move/ Copy…
Select the existing combined body from the modeling area
Go to the property manager and click on the Rotate box
Go to modeling area and select Point1 or Point2 as rotation reference
Assign rotation values around X, Y, and Z-Axis
X= 0 degrees, 
Y= 0 degrees, and 
Z= 180 degrees
Leave the other values as default
Click OK to complete the operation.
Use the Combine feature:
Go to: Insert > Features > Combine
Select both the combined bodies from the modeling area
Go to the property manager and choose the operation type Add, as shown in the image below:
Click OK to complete the operation.
Insert a sketch block on Plane1
Select Plane1 from the feature tree and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Blocks > Insert 
Click here to download the free Sketch block
Go to the property manager and click on the Browse button
Locate and select the downloaded file LearnSolidworks Logo.SLDBLK
Go to the property manager and assign the angle to orient the logo correctly
Go to the modeling area and place the block in the center of the hexagonal face, as shown in the image below:
Click on Close sketch to close the sketch area.
Use the Split Line Tool
Go to: Insert > Curves > Split Line 
Go to the property manager and choose the Type of Split – Projection
Go down in the selections where Current Sketch 
is automatically selected
Click on the face selection 
input box, move to the modeling area and select the blue hexagonal face
Go back to the property manager, tick the single direction checkbox as shown in the image below:
Click OK to complete the operation.
Change the Appearance
Go to: PhotoView 360 > Edit Appearance… 
Go to the property manager and right-click on the Selected Geometry dialogue box
Click on the Clear Selections from the pop-up options to clear the dialogue box
Click on the Select Bodies 
icon from the five icons
Go back to the modeling area and select the Shell Body, as shown in the image below:
Select Appearances (color) > Plastic > High Gloss > White High Gloss Plastic (or pick any other color you like)
Click on White High Gloss Plastic twice to apply the appearance
Click OK to apply the appearance
Go to the modeling area, select any letter (e.g. S)
Click on the Edit appearance icon > Face 
from the pop-up window
Go to the appearance manager and click on the selected geometry input box
Select all the letters of the LearnSolidWOrks logo, as shown in the image below:
Select Appearances (color) > Plastic > High Gloss > Black High Gloss Plastic
Click on Black High Gloss Plastic twice to apply the appearance on all the letters
Click OK to apply the appearance on all the letters
Use the Move/ Copy Body Tool
Go to: Insert > Features > Move/ Copy…
Select the soccer ball from the modeling area
Go to the property manager and assign rotation values around X, Y and Z-Axis
X= 0 degrees, Y= 36 degrees, and Z= -45 degrees
Leave the other values as default
Note: No need to assign the reference point for rotation
Click OK to complete the operation
Go to: View > Display
Select Shaded 
, Shadows In Shaded Mode 
, and Ambient Occlusion 
(If possible)
The complete Soccer Ball will look like as shown in the image below:
Save the File again 
Congratulations, you just finished your own soccer ball in SOLIDWORKS!
Click here to download this tutorial as a free eBook (PDF).
I hope you liked this LearnSOLIDWORKS tutorial!
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Thanks a million!
Jan
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