Surf and Code: Surface Modeling

In this tutorial you learn :

How to model a Pair of goggles with frame using the BlueSurf command of Solid Edge

How to use the project curve command

Trimming surfaces in Solid Edge

Thicken surfaces to make solids
It is assumed that you are familiar with the basics of Solid Edge Part modeling.

Drawing the profile - Front view Start with creating a sketch in the the x-z plane. Using the Curve tool, create the outline of the goggle frame. You may not be able to close the curve. So create a straight line joining the two open ends of the curve. See the red circled area in figure besides.
Mirror the profile Keep the profile above the x-y plane. Mirror it as shown.
Another Curve in x-y plane Draw an arc in the x-y plane as shown in figure. Keep the arc symmetric about the y-z plane. Keep the arc well behind the mirrored frame curves drawn earlier.
Parallel Plane Create a plane parallel to the x-y plane. Keep the plane well above the top rim of the frame. See figure.
Included Sketch Sketch an arc on the new plane by using the Include tool in the sketcher environment.
More Parallel Planes Create two more planes parallel to the y-z plane. The planes pass through the endpoints of the arc created in last step.
More Arcs Sketch arcs each on the two planes whose end points are well connected to the arcs in the horizontal planes. See figure.
The Overall View Overall the four arcs should nicely enclose both the goggle glasses curves. See figure.
The BlueSurf Click the BlueSurf tool on the surfacing toolbar. Select the right-side vertical arc and click accept on the ribbon bar. Then select the left-side vertical arc. Both - correct and incorrect - ways of picking the second arc are shown in figure. Pick in the correct way.
BlueSurf Appears Click accept and then Preview. A BlueSurf will be created as shown in figure.
Add a Guide Curve Still in the BlueSurf command, Click the Add Guide Curves button on the ribbon bar. Select the arc as shown and click accept
Add Another Guide Curve Similarly, select the other arc as shown in figure. Click the accept Preview and Finish buttons in that order.
BlueSurf Created A BlueSurf, as shown in figure, is finally created . This surface spans the two smaller arcs and is guided by the two larger arcs. You could have build the BlueSurf the other way too, in that, the surface spans the two larger arcs and the two smaller arcs act as guide curves. This is more commonly done when building a BlueSurf using a set of curves - when the bluesurf fails in one way, it sometimes builds the other way.
Project Curve - Curve Step Make visible the two profiles for the goggle frame. Select the Project Curve tool from the Surfacing toolbar. Select one of the profiles of the goggle frame as the curve to project. Click accept on the ribbon bar.
Project Curve - Body Step Select the Bluesurf as the surface to project on.
Project Curve - Direction Step Point the arrow towards the Bluesurf and click. Click Finish on the ribbon bar.
Project Curve - View It Click the Visible and Hidden Edges tool on the Main toolbar to see the projected curve. Similarly, project the other frame curve also.
Trim Surface - Surface Step Select the Trim Surface tool from the Surfacing toolbar. Select the Bluesurf as the surface to trim.
Trim Surface - Surface Step Select the Trim Surface tool from the Surfacing toolbar. Select the Bluesurf as the surface to trim.
Trim Surface - Curve Step Select the projected curves as the trimming curves. Click accept on the ribbon bar.
Trim Surface - Side Step Indicate the arrow pointing away from the frame as the part to trim off. See figure.
Surface Trimmed The Bluesurf is trimmed as shown in figure. Also, I have applied Steel to it using the Part Painter.
Normal Plane Click on the Plane Normal to Curve tool on the features toolbar.
Specify the Curve Select the goggle frame curve as shown in figure.
Plane Created Click at the end point of the curve as shown in figure in last step. The plane is created as seen in figure.
Sketch the Cross Section Sketch a small circle in the newly created plane. See Figure. This circle is the cross section of the goggle frame.
Sweep create a swept protrusion using the circle as cross section and the projected curve as path. Also create the frame for the other frame in the pair. Connect the two frame with another swept protrusion along an arc that connects the two frames. See figure.
Surface to Solid Click the Thicken tool on the Features toolbar. The Thicken tool is in the same flyout as the Thin Wall and Thin Region tools. Select the Trimmed Bluesurf as the surface to thicken. Use a small value of 1 mm to thicken in any direction. Using Part Painter, apply White (clear) to the bluesurf.
The Ear Rest Next, we will create the ear-rest for the goggle.
EarRest - Top View This is not a simple protrusion. When viewed from the top, the ear-rest is bent at two places. First, where the free end goes behind the ears to See figure.
EarRest - Front View Create a sketch in the x-z plane for the front view. See figure.
EarRest - Top View Create a sketch in the x-y plane for the top view. As shown in figure, align the ends with the extremes of the front view.
Cross Curve Select the Cross Curve command from the Surfacing toolbar as shown.
First Curve Select the front view curve as the first curve. Click accept on the ribbon bar.
Second Curve Select the top view curve as the second curve. Click accept on the ribbon bar.
Cross Curve Click Finish on the ribbon bar. Soon the cross curve is formed. The cross curve is neither in the top plane nor in the front plane. It is bent as pointed in the figure besides.
Bounded Surface Hide all sketches. Click the Bounded Surface tool from the Surfacing toolbar. Drag a window around the cross curve to select it. See figure.
Bounded Surface Done Click accept Preview and Finish in that order. A bounded surface will be formed as shown in figure.
Surface to Solid Click the Thicken tool on the Features toolbar. Select the bounded surface as shown in figure. Specify the direction to thicken as shown in figure Type a value for the thickness of the fork in the ribbon bar. Click Finish on the ribbon bar.
Surface to Solid Done This makes it a solid.
Assemble It Finally, assemble the goggle with the ear rest and its ready to use. cMayoCAD is a first of its kind training program where you learn to build your own, brand new, fully functional CAD system using a geometric modeling kernel.