With the introduction of the iPhone, there has been much discussion among both the SolidWorks and Pro/Engineer communities about how to model this shape in 3-D CAD. Although it can be done in either CAD system, and has been previously discussed in Josh Mings’s SolidSmack blog (see here) and the Pro-E MCAD forum (see here), I will discuss what I believe to be the most robust / straight-forward approach in creating this model in SolidWorks.

Spline profile / Section

First, create a 2-D sketch of the initial outline or base of the object as if it where resting on a 2-D plane, such as a table surface.  The shape should be rectangular with fillets sketched in each of the four corners. Normal to this sketch, a section representing the “dome” needs to be created using a spline as a sketch entity. To control the spline, three points are used for the shape of the dome. The handle of the midpoint of the spline is parallel to the table top surface (with magnitude dimension), and the ends of the spline have both tangency and equal curvature constraints in relation to the straight line segment (construction) at each end. This line segment represents the section of the skirt which will be later sweep around the base at the assigned draft angle (5 degrees).

Create another sketch of a spline using only two points, and this spline will be used as a path for a sweep feature. This sketch is constructed at a right angle to the previous sketch, and the ends require the same type of constraints.  Now that we have these two sketches, a draping sheet surface can be constructed as the first surface feature, and Pro-E users often refer to this as the “Toupee” method. Create the Sweep Feature selecting the profile & path sketches, and then choose the “keep normal constant” option.

"Toupee" sweep of dome

After creating the “toupee” surface of the dome, a 2-D sketch is created (using offset entities & fit spline) on the base plane, and is used for a trim feature creating a “bald” spot. This sketch is used as the trim tool, and does not require being projected onto the dome surface. Before creating the skirt surface as a sweep, half of the base sketch needs to be copied using the convert entities and fit spline sketch tools, and it will be used as the path for the sweep. Remember; create the sweep for the skirt by selecting a profile / section, and the path using the “flow path” orientation option.

This next part is the “fun” part, and can be done using either a loft or boundary surface. We want to create a surface that bridges the trimmed dome to the skirt (with draft angle) while maintaining the curvature of both surfaces.  Select the edges of the surfaces (not sketches) to be used as the loft profiles using the curvature to face constraint. For a boundary surface, these edges would be direction 1 curves. If the surface is twisted, drag or flip the connections to that they are lined-up with each other.

"skirt" base sweep

Once loft or boundary surface has been completed, merge the surfaces using the knit feature, and then remove the skirt using the delete body feature. As only half of the housing has been modeled, use the mirror feature to complete both halves by selecting the surface body (not features) to mirror, and the “knit surfaces” option. Now, the surface model is complete, but it still needs to be converted into a solid body.

The quickest way to do this using the least amount of features is to thicken the surface (example: 15 mm), and then use the “Cut with Surface” tool. Select the top surface / base plane, and if necessary flip the cut to cut-away the excess material over-hanging the base of the part. From the overhead lights reflecting off-of-the rendered surface, continuous curvature of the model face is shown.  The visual of the last image was achieved using the PhotoWorks add-in for rendering, which is part of SolidWorks Premium package.

dome /skirt blend using loft

Creating this shape is also possible in Pro-E (Pro/Engineer). If I were to try and recreate this model in Pro-E, I would most likely use the Variable Section Sweep (VVS) feature and / or the Boundary Surface feature. If your Pro-E license includes the Interactive Surface Design Extension (ISDX) module, those surfacing tools can be accessed through the Style tool inside Pro-E. I do not believe it is necessary to use the ISDX module to create this shape, and the standard Pro-E surfacing tools should be sufficient.

An issue that is of concern to me when modifying 3-D CAD models created by other Industrial Designers or Engineers is that I frequently find the models use more features than necessary (excessive parent-child relationships) which can cause the model to become unstable when modified. When using surface or hybrid modeling, please remember to think about the next person who will be modifying your model in the future, and spend the additional time to create a more robust model.

Completed model render