Since we’ve been talking about viewing SolidWorks files on an iPhone, how about we talk a little about viewing an iPhone in SolidWorks. Better yet, how about we model up the back of one to see how we can get those continuous smooth shapes in SolidWorks.

We’ll be using surfacing, and the fine art of visual analysis, to create the shell of the first touch-screen device to be held in our sweaty palms. It’s fairly simple and we’ve even included the file for you to download.

Update:This post is one way of approaching a design problem and not intended to go into complex surfacing. Only an example of creating a ROUGH surface model for creating iPhone accessories. As read in the comments, there is a MUCH BETTER way to actually model the part for manufacturing. That post can be found at this link (iPhone 3G model Take 2). Thanks to everyone that commented on how NOT to model this part. 🙂


File Download *Updated*
Here is the part file to see one approach. This could be used for designing around an iPhone, but not for manufacturing something as smooth as an iphone back.
Download iPhone-3G-v2.sldprt (V2 – 2009 – 333kb) – [.x_t][.igs][.step]

Real World Example: Design a Case for an iPhone
We’re knocking two things out here at once. This is a perfect example of using simple surfacing features in SolidWorks to create an iPhone model used to develop a case (or other iPhone accessory). For this, you have a small amount of data to start from and a short amount of time to get it done. Pretty typical of a real project. Here we go.

Step 1: Analyze

First you need to download the iPhone spec at the Apple Developer Connection. It has your typical vague dimensional info, but we’ll take care of that in a minute. First we want to look at the design of the iPhone and start thinking about how were going to model it.

If you use your brilliant powers of observations, you’ll notice a few things:

  • This thing has symmetry
  • There’s a constant section
  • The edge is the same all around
  • The corners are perfect squares

Understanding this will help the modeling go smoother and help define a place to start. Since it has a nice constant section we’ll start there, but first we need to make sure we have the right dimensions for our profiles.

Step 2: Get the Dimensions

We’ll want a good sketch of the constant section, the face and the corner radius. Since every dimension we need isn’t on the spec, we’ll bring it into SolidWorks to infer. Do this by starting a sketch on Plane 1, then go to Tools, Sketch Tools, and select Sketch Picture… near the bottom. Download this .jpg of the spec (right-click, save as…) and insert on the plane.

Draw a line and dimension it with the overall height of the iphone (115.5). Select the sketch and scale it (from the corner) to make the image of the iPhone match the line. Create some other sketches on top of the image to get the profiles of the constant section, top face and corner radius. Here’s some of the dimensions you’ll need.

Step 3: The Constant Section

With the sketch of the constant section defined, Extrude a Surface (Insert, Surface, Extrude). Use a Midplane extrusion at 53.67mm (This dimension was also inferred from the image).

Step 4: Sweep the Corners

Create a Plane (Insert, Reference Geometry, Plane) at the end of the profile (Select a point and Plane 1). Start a Sketch on the new plane and Convert the outermost curves of the extruded surface. Create another sketch on the perpendicular Plane 2 and sketch the top face of the iPhone. Hint: Use relations to attach the sketch lines to the existing geometry.

Step 5: Fill the Space

Select Insert, Surface, Fill. This next part can be tricky. First, set the Edge Settings to Tangent. (Doing this later can give some funky results) Then, select the swept edges, one at a time in order, then select the constant section curve. In the options, make sure Merge Results is NOT checked.

Note: Make sure Optimize Surface is OFF for this. If you turn on Curvature (View, Display, Curvature), otherwise you’ll notice small ridges at the corners.

Step 6: Mirror and Knit

You’re almost there. Go to Insert, Pattern/Mirror, Mirror…, select Plane 1 for the Mirror Plane and select the Surface-Sweep and the Surface-Fill as the bodies to Mirror. Now, knit the surfaces together (Insert, Surface, Knit…) to get a single surface.

That’s it. You now have the back of an iPhone you can use to create a case, a dock or other accessory. IF you happen to have another way of creating this, please mention it down in the comments. SolidWorks is known for having multiple solutions to multiple problems.

ShoutOUT!
I’d also like to think Spencer Nugent of IDSketching.com for sparking the idea for this post. Check out IDSKetching.com for some really excellent video tutorials on Industrial Design and the art of sketching.

Author

Josh is founder and editor at SolidSmack.com, founder at Aimsift Inc., and co-founder of EvD Media. He is involved in engineering, design, visualization, the technology making it happen, and the content developed around it. He is a SolidWorks Certified Professional and excels at falling awkwardly.