Solidworks apple mouse Design

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How to model Apple’s Magic Mouse in SolidWorks?
If you like simplicity, you will definitely love the famous Apple Magic mouse. The Magic
Mouse is the first consumer mouse to have multi-touch capabilities. I really love the
simplicity of the design.
The design looks simple. but like most Apple products, the design is a lot more complex than
the simple shape suggests. We have already seen this with the AirPods tutorial. In today’s
tutorial, you will discover how to model this beautiful piece of art in SolidWorks yourself.
Disclaimer: The intellectual property depicted in this 3D model, is not affiliated with or endorsed by
Philippe Starck or Alessi. This 3D model may not be used for any commercial, promotional,
advertising or merchandising use.

Open a New Part with model units set to millimeters
Go to: File > New > Part
Save the file with the following name: Apple Mouse.SLDPRT
Create a 2D Sketch on the Right Plane (Sketch 1)
Select the Right Plane from the Feature tree and click on the sketch icon
Click on the Normal To icon
Go to: Tools > Sketch Entities > Midpoint Line
Draw a horizontal midpoint line starting from the origin
Go to: Tools > Dimensions > Smart
Click on the horizontal line and assign a length of 135,5mm, as shown in the image below:
Click on the fully defined horizontal midpoint line

Go to the Line Properties > Option
Tick the ‘For Construction’ checkbox
This will convert the horizontal line into a construction line as shown in the image below:
Go to: Tools > Sketch Entities > Centerline
Draw a small vertical centerline at both endpoints of the horizontal centerline
Hold the Ctrl Key, select both vertical centerlines
Assign an Equal relation from the property manager

Click on a vertical centreline and assign a length of 4.5mm, as shown in the image below:
Go to: Tools > Sketch Entities > 3 Point Arc
Draw a 3-point arc by using the upper-end points of the vertical centerlines
Click on the arc and assign a radius of 165mm, as shown in the image below:

Click on the Close sketch to close the sketch area.
Create a 2D Sketch on the Top Plane (Sketch 2)
Select the Top Plane from the Feature tree and click on the sketch icon
Go to: Tools > Sketch Tools > Convert Entities
Select the highlighted vertical line as shown in the image below:
Click OK to complete the operation
Draw a horizontal centerline starting from the origin towards the right

Click on the centreline and assign a length of 28.55mm, as shown in the image below:
Go to: Tools > Sketch Entities > Spline
Draw a 3-point spline by using the red encircled points of the sketch, as shown in the image
below:
Click on the spline and drag both end handles one by one to activate them

Now drag the mid spline handle by holding the Alt key to maintain the tangent symmetry
All the activated spline handles become blue, as shown in the image below:
Click on the upper spline handle and choose the Horizontal relation from the property
manager
Click on the lower spline handle and choose the Horizontal relation from the property
manager
Similarly, click on the mid spline handle

And assign a Vertical relation from the property manager, as shown in the image below:
Click on the upper spline handle and assign a handle length of 85mm
Click on the lower spline handle and assign a handle length of 80mm

Click on the mid spline handle and assign a handle length of 250mm, as shown in the image
below:
Now click on the converted vertical line
Go to the Line Properties > Option
Tick the ‘For Construction’ checkbox
This will convert the vertical solid line into the construction line
Use the Mirror Entities Sketch Tool
Go to: Tools > Sketch Tools > Mirror or click on the Mirror Entities directly from the
sketch tab
Go to the property manager, click on the Entities to Mirror input box
Select the fully defined 3-point spline from the 2D sketch
Go to the property manager, click on the Mirror About input box

Select the vertical centreline from the 2d sketch as a mirror line, as shown in the image
below:
Click OK to complete the operation.
Click on Close sketch to close the sketch area.
Use the Project Curve Tool
Go to: Insert > Curve > Projected
Go to the property manager and select Sketch on Sketch as a projection-type
Go to the feature tree, select Sketch1 and Sketch2

Then a projected curve is generated in yellow as shown in the image below:
Go to: Tools > Sketch Entities > Spline

Draw a 2-point spline by using the red encircled points of the projected sketch, as shown in
the image below:
Click on the spline and drag both end handles one by one to activate them, as shown in the
image below:

Draw a horizontal centerline by using the endpoints of the spline, as shown in the image
below:
Hold the Ctrl key, select the left spline handle and the horizontal centreline
Assign an angular dimension of 45 degrees between them
Similarly, select the right spline handle and the horizontal centreline
Assign an angular dimension of 45 degrees
Click on the left spline handle and assign a handle length of 95mm

Click on the right spline handle and assign a handle length of 95mm, as shown in the image
below:
Create a 2D Sketch on the Front Plane (Sketch 4)
Select the Front Plane from the Feature tree and click on the sketch icon

Draw a 3-point arc anywhere on the front plane, as shown in the image below:
Hold the Ctrl key, select the left endpoint of the arc and the left part of the projected curve
Go to the property manager and assign a Pierce relation
Similarly, select the right endpoint of the arc and the right part of the projected curve

Go to the property manager and assign a Pierce relation, as shown in the image below:
Hold the Ctrl Key, select the mid-point of the arc very carefully
Then select the previously drawn spline sketch (Sketch4)

Make a Reference Plane (Plane1)
Go to: Insert > Reference Geometry > Plane
Select the Front Plane from the feature tree as a First Reference
Go to the property manager and assign an offset value of 27.5mm
Tick the Flip offset checkbox, as shown in the image below:
Create a 2D Sketch on Plane1 (Sketch5)
Select Plane1 from the Features tree and click on the sketch icon

Hold the Ctrl Key, select the mid-point of the arc very carefully
Then select the previously drawn spline sketch (Sketch4)

Make a Reference Plane (Plane2)
Go to: Insert > Reference Geometry > Plane
Select the Front Plane from the feature tree as a First Reference
Go to the property manager and assign an offset value of 27.5mm, as shown in the image
below:
Create a 2D Sketch on Plane2 (Sketch6)
Select Plane2 from the Features tree and click on the sketch icon

Go to the property manager and assign another Pierce relation, as shown in the image
below:
Go to: Tools > Sketch Entities > Point
Click anywhere on the blue arc to create a sketch point on it, as shown in the image below:

Hold the Ctrl Key, select that Sketch Point and the previously drawn spline sketch (Sketch4)
Use the Fill Surface Tool
Go to: Insert > Surface > Fill
Go to the Property Manager > Patch Boundary
Click on the Patch Boundary input box
Go to the modelling area and select the blue Projected Curve (Curve1)
Go to the Property Manager > Constraint Curves
Click on the Constraint Curves input box

Go to the Feature Tree and select Sketch3, Sketch4, Sketch5, and Sketch6, as shown in the
image below:
Make sure that the Optimize Surface checkbox and the Fix Up Boundary checkbox is
selected
Leave the other parameters as default
Click OK to complete the surface fill operation.
Go to: Tools > Sketch Entities > Center Rectangle
Draw the center rectangle starting from the origin point

Assign a length and width of the rectangle, as shown in the image below:
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 menu
Click on the Sketch Selection input box
Go to the modeling area and select the current sketch (Sketch7)
Click on the Faces To Split input box

Go to the modeling area and select the blue highlighted curved surface, as shown in the
image below:
Go to: Tools > Sketch Entities > Line

Draw a vertical line by using the midpoints of the split lines, as shown in the image below:
Go to: Tools > Sketch Tools > Offset Entities
Select the vertical line of the sketch
Go to the property manager and assign an offset value of 6.50mm
Click on the Reverse checkbox to reverse the offset direction

Click on the Cap Ends checkbox and select the Lines, as shown in the image below:
Create a Planar Surface
Go to: Insert > Surface > Planar
The Current Sketch (Sketch8) will automatically get selected
This sketch will create a planar surface in the modeling area, as shown in the image below:

Make a Surface Loft
Go to: Insert > Surface > Loft…
Go to the modeling area and select Edge <1> (Starting Edge)
Now select Edge <2> (Ending Edge), as shown in the image below:
Note: Select the right-hand side edges of both surfaces to get the exact results
Go to the Property Manager > Start/ End Constraints
Click on the Start Constraint box and select the Tangency To Face option
Assign an influence value of 2, as shown in the image below (try different values to see what
happens with the surface)

Click on the End Constraint box and select the Direction Vector option
Open the Feature Tree and select the Top Plane for the direction vector
Set the influence angle to 5 degrees and the influence value to 1, as shown in the image
below:

Click OK to complete the surface loft operation.
Draw the center rectangle starting from the origin point

Go down in the Selections menu
Click on the Sketch Selection input box
Go to the modeling area and select the current sketch (Sketch9)
Click on the Faces To Split input box
Go to the modeling area and select the two blue highlighted faces, as shown in the image
below:
Make a Surface Loft

Assign an influence value of 2, as shown in the image below:

Leave the End Constraint box to None
Make another Surface Loft
Assign an influence value of 2

Leave the End Constraint box to None, as shown in the image below:
Go to the Property Manager > Guide Curves
Click on the guide curve input box
Go to the modeling area, select the blue highlighted edge of the previous loft surface
Go back to the Property Manager > Guide Curves

Set the influence type to Tangency To Face, as shown in the image below:

Assign an influence value of 2, as shown in the image below:

Leave the End Constraint box to None
Assign an influence value of 2

Leave the End Constraint box to None, as shown in the image below:
Go to the Property Manager > Guide Curves
Click on the guide curve input box
Go to the modeling area, select the blue highlighted edge of the previous loft surface
Go back to the Property Manager > Guide Curves

Set the influence type to Tangency To Face, as shown in the image below:
Knit the surface
Go to: Insert > Surface > Knit…
Select the 6 blue highlighted surfaces from the modeling area

Go to the property manager, tick the Merge Entities and the Gap Control checkboxes, as
shown in the image below:
Use the Mirror Feature
Go to: Insert > Pattern/Mirror > Mirror…
Go to the property manager and click on the Mirror Face/Plane input box
Open the features tree and select the Right plane as mirror plane
Go to the property manager and click on Bodies to Mirror input box
Move to the modeling area and select the knitted surface body

Go down to the Options and select the Knit Surface checkbox, as shown in the image below:
Use the Knit Surface
Go to: Insert > Surface > Knit…
Select both surface bodies from the modeling area

Go to the property manager, tick the Merge Entities and all the Gap Control checkboxes, as
shown in the image below:
Go to the Feature Tree > Curve1 > Sketch1
Click on Sketch1 and hit the Eye icon to Unhide the sketch
Select the unhidden sketch (Sketch 10)
Go to the property manager and assign an offset value of 2mm
Click on the Reverse checkbox to reverse the offset direction

Go down in the property manager and tick the Offset Geometry checkbox, as shown in the
image below:
Select the offset entity of the sketch
Go to the property manager and assign an offset value of 2mm
Click on the Bidirectional checkbox to offset in both the direction

Click on the Cap Ends checkbox and select the Lines, as shown in the image below:
Go back to the Feature Tree > Curve1 > Sketch1
Click on Sketch1 and hit the Eye icon to hide the sketch
Use the Surface Trim
Go to: Insert > Surface > Trim…
The current sketch (Sketch10) is pre-selected as a Trim tool in the property manager
Go to the modeling area, select the purple highlighted parts of the surface

Go back to the property manager and select the Keep Selections, as shown in the image
below:
Leave the other parameters as default
Use the Thicken Tool
Go to: Insert > Boss/ Base > Thicken
Go to the modeling area, select the upper highlighted surface body as a Thicken parameter
Go to the property manager, select the first icon as the Thickness type

Assign a thickness value of 1mm, as shown in the image below:
Make another Thicken
Go to: Insert > Boss/ Base > Thicken
Go to the modeling area, select the upper highlighted surface body as a Thicken parameter
Go to the property manager, select the first icon as the Thickness type
Assign a thickness value of 1mm

Uncheck the Merge Result checkbox, as shown in the image below:
Make a Fillet
Go to: Insert > Features > Fillet/Round
Go to the Property Manager > Fillet Type
Click on the 3rd icon to activate the Face Fillet option
Now go down to the Items To Fillet in the property manager
Click on the 1st input box
Go to the modeling area, select the blue highlighted upper face of the solid body
Go back to the Property manager > Items To Fillet
Click on the 2nd input box
Go to the modeling area, select the pink highlighted side face of the same solid body

Go back to the Property manager > Fillet Parameters
Select the Chord Width option (This will give a uniform looking fillet result)
Assign a fillet radius of 1mm, as shown in the image below:
Make another Fillet
Go to the Property Manager > Fillet Parameter
Assign a fillet radius of 0.25mm

Go to the modeling area, select the highlighted outer edge of the upper solid body, as shown
in the image below:
Make another Fillet
Go to the modeling area, right-click on the outer edge of the lower solid body

Choose the Select Tangency from the pop-up options, as shown in the image below:
Draw the horizontal centerline starting from the origin point

Click on the horizontal centreline and assign a length of 12mm, as shown in the image
below:
Draw the center rectangle starting from the right endpoint of the horizontal centerline

Make a Sketch Fillet
Go to: Tools > Sketch Tools > Fillet…
Go to the property manager and assign the sketch fillet radius of 1.5mm

Go to the modeling area, select all the 4 corners of the rectangle, as shown in the image
below:
Make an Extrude Boss/Base
Go to: Insert > Boss/Base > Extrude… or click on Extrude Boss/Base
Select the rectangular sketch (Sketch11) from the modeling area
Go to the Property manager > From
Select the Offset option and click on the Flip Direction icon to reverse the offset
Assign an offset value of 0.3mm
Go to the Property manager > Direction1
Select the Up To Surface option

Go to the modeling area, select the pink highlighted face of the solid body
Uncheck the Merge Result checkbox, as shown in the image below:
Click OK to complete the extrude operation.
Make a Fillet

Go to the modeling area and select the bottom face of the extruded solid body, as shown in
the image below:
Use the Mirror Feature
Go to: Insert > Pattern/Mirror > Mirror…
Go to the property manager and click on the Mirror Face/Plane input box
Open the features tree and select the Right plane as the mirror plane
Go to the property manager and click on Bodies to Mirror input box

Move to the modeling area and select the rectangular solid body, as shown in the image
below:
Make a Sketch Block on the Top Plane
Select the Top plane from the features tree and click on the sketch icon
Click here to download a 2D sketch of the Apple logo.
Go to: Tools > Blocks > Insert
Go to the property manager and click on the Browse button
Locate and select the downloaded file Apple Logo.SLDBLK
Go to the property manager and assign an angle to orient the logo correctly
Go to the Property Manager > Parameters

Assign the scale value of 0.8 to scale down the block
Then assign the angle of 180 degrees to orient the logo correctly
Move to the modeling area, place the block intuitively at the upper middle part of the
mouse, as shown in the image below:
Go down in the selections where Current Sketch is automatically selected
Now click on the second input box (Face Selection input box)

Go to the modeling area and select the upper blue face of the mouse, as shown in the image
below:
Change the Appearance
Go to the modeling area, right-click on the upper solid body of the mouse
Click on the Edit appearance icon > Body from the pop-up icon window
Select the Appearances (color) > Plastic > High Gloss > White High Gloss Plastic

Double click on the White High Gloss Plastic icon, as shown in the image below:
Click OK to change the appearance.
Go to the modeling area, right-click on the lower solid body of the mouse
Select Appearances (color) > Metal > Steel > Satin Finish Stainless Steel

Double click on the Satin Finish Stainless Steel icon, as shown in the image below:
Click OK to change the appearance
Go to the modeling area, hold the Ctrl Key and select both lower pads of the mouse
Select Appearances (color) > Rubber > Matte
Double click on the Matte Rubber icon

Go to the modeling area and select the remaining pad of the mouse, as shown in the image
below:
Go to the modeling area, hold the Ctrl Key and select both faces of the apple logo
Right-click and select the Edit appearance icon > Faces from the pop-up icon window
Select the Appearances (color) > Plastic > High Gloss > White High Gloss Plastic
Double click on the White High Gloss Plastic

Go to the color pallet and select the Light Grey color, as shown in the image below:
Go to: View > Display
Select the Shadows In Shaded Mode , and Real View (if possible)
The completed Apple Mouse will look like as shown in the image below:

Save the File again
Congratulations, you’ve just completed the Apple mouse!
I know it was a lot of work (so was developing this tutorial!) but hopefully you’ve learned a
couple of new things. 😊
Did you like this tutorial and are you eager to learn more? Then you should really check my
SolidWorks Boeing 747 course. In this video training course, I will show you how to model an
incredible Boeing 747-8 in SolidWorks from scratch.
Click here for a free video to start modeling your own Boeing 747-8 in SolidWorks.
Best regards,
Jan-Willem Zuyderduyn

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