进口造型教程（入关审批耽误了好久）

Solidworks Rant Time:
The spline functionality is still not fully implemented. The spline control handles of 3D sketches are VERY buggy unless you constrain them horizontal, vertical or tangent to a construction line.  
  
eventhough you cannot use spline handles to the same degree in 3D that you can in a 2D sketch they are stiil a big leap over 3d splines in 2004. The curves will just be a little heavier because you use control points to define curvature rather than the spline handles

Tweak the curve to match your sketch lines. You have just defined a 3D character line!

This is what you should see when you open the file from the beginning of the tutorial. You will see a trimmed surface loft and a bunch of curves. I wanted to start with just curves, but the side section curves are created with curves that are tangent to the trimmed loft surface. The side section curves are also constrained to pierce the 3D character line that we previously created

Start a Loft between the Edge of the Trimmed Surface and the 2D sketch "lan View" All required sketches should be in the folder "Sketches for the Main Surfaces" which is nested in the history tree.

Start editing the loft so that it is curvature continuous at the top. This is done by editing the Start Constraint to "Curvature Continuous" in the drop down menu.
  
Define the loft a little more with guide curves. This can get a little squirrelly along the center line because the guide curves at the rear and front (Rear Section of Side Profile and Front Part of Side Profile ) along the center-line are cut (convert entities) from the Profile Sketch. Use the secondary history tree in the modeling window to pick the right sketch
  
To create a smooth connection along the center line click the guide curves and choose Normal to Profile to make the loft smooth along the center line.

Mirror the surface bodies along the Right Plane. Generally mirroring the bodies (as opposed to Faces or features) is the most straight forward because the computer does not have to calculate too much information

If at any point the sketches become annoying or too busy CLick View>Sketches to toggle visibility of Sketches. You can do the same thing with planes, curves, origins etc:  
  
I have toggled sketch visibilty so that I can choose the edges of the surfaces to define a planar surface

Use the bottom edges of the lofts to define the bottom planar surface

Knit all the surfaces together to create a Solid. Check the box that says "Try to form a Solid" (the process is similar to creating a closed polysurface in Rhino)
This will give the model mass properties and gives you the ability to use solid modelling tools on the model

Shell the solid to give wall thickness of 2mm. If you click on any faces that will create an opening in the shell because those selected faces will not be included in the final shell. So in this case Dont click on any faces because we are interested in keeping all the surfaces