GabiJack.com

Archive for January 14th, 2009

It’s amazing how sidetracked one can get! Quite a few months ago, I was very excited about the new SolidWorks Surfacing book that had just come out and adamant to go through it as soon as possible. However, as time went by, I got distracted with other things:  spent some time preparing for the CSWP test, got bitten by the rendering bug, and discovered a fascination for Sheet Metal I never knew I had.  Now I feel bad for not reading the Surfacing book yet!  I feel especially bad every time I bump into something really cool that can be done using surfaces! This is a little something that I learned how to do by examining closely one of the models that served as rendering examples for PhotoView 360 during the hands-on session in Barcelona. The model was a beautiful wine glass with a series of decorative cuts on it.  I’m no expert in surfaces, but this example is simple enough even for me.

 

In this example, surfaces tools are used to create the fancy candy bowl from the rendering. We begin by sketching the profile of the candy bowl on the Front plane and using Revolve to generate the solid.

 

Next, we need to make a few more sketches (all of them on the Front plane) that will be used to create surfaces. In the image, Sketch1 (in green) is the profile of the candy bowl that was used previously in the Revolve feature; Sketch2 (in blue) and Sketch3 (in orange) will be used to create the shapes of the cuts that will decorate the candy bowl. Notice how their endpoints are coincident.  Sketch4 (in red) follows the outside edge of the candy bowl (created by converting Sketch1 and then trimming to those two construction lines) and its endpoints are horizontal to those of Sketch2 and Sketch3. Sketch5 (in purple) will determine how deep into the thickness of the candy bowl the decorative cuts will go. Notice that the endpoints of Sketch5 are also coincident with the endpoints of Sketch4. One more thing to notice is that Sketch2, 3, 4 and 5 are one-curve profiles, with no segments. I used to have a couple of arcs instead, but I ran into trouble down the road while using some of the surfacing tools, so I used Fit Spline to join both segments together in one curve and it all worked out much better. It will all become clearer in a moment.

 

We’ll create an extruded surface using Sketch2. In the feature manager, pre select Sketch2 and from the Surfaces tab (or toolbar) select Extruded Surface.  A property manager displays, which is very similar to that of the Extrude feature.  We only need to extrude the surface far enough to intersect and completely go through the candy bowl, like in the image.

 

We do the same with Sketch3. The extruded surface created above is shown here in blue.

 

 

Now we are going to use Sketch4 and Sketch5 to create a couple of revolved surfaces.  First, pre-select Sketch4 and then, from the Surfaces tab (or toolbar) select Revolved Surface. A property manager, very similar to that for the Revolve feature shows up, as you can see in the image.  Note: the extruded surfaces we created previously are shown in this image in blue and orange. The preview of the revolved surface we are about to create is shown in pale yellow.

 

This image shows all the surfaces created so far: the two extruded surfaces appear in blue and orange, Revolved surface1, created using Sketch4 is shown in red, and, finally, Revolved surface2, created using Sketch5, is shown in purple. The solid body (the candy bowl) has been hidden, but all the sketches are still showing.

 

Now comes the really fun part. Using Trim Surface from the Surfaces tab (or toolbar), I’ll trim the two extruded surfaces, using the two revolved surfaces as trimming tools. I’ll start by trimming Surface Extrude2 using Surface Revolve1 as the trimming tool.  Notice the property manager in the image below.  A Standard Trim Type means simply that I’m using one surface as a tool to trim the other, as opposed to both surfaces trimming each other mutually at their intersection.  The trimming tool could’ve also been a sketch or a plane. Remove Selections means that the pieces of the extruded surfaces on the side I select (shown in purple right where the cursor is) will be discarded and only the pieces on the other side of the intersection (shown in pale orange) will be kept.  A Natural Surface Split Option means that the boundary edges of the extruded surface trimmed this way will be forced to follow the shape or the revolved surface used as trimming tool.

 

The same procedure is used to trim Surface Extrude1, using Surface Revolve2 as the trimming tool. The result of the trimming operations is shown here, where I’ve hidden Surface Revolve1, so you can notice the boundary edges of the extruded surfaces after the trim. Surface Extrude2 is shown in orange, Surface Revolve2 is shown in purple and the edge of Surface Extrude1 is that blue line on top of Surface Revolve2.  Notice the curvy edges of Surface Extrude2. They look that way because now that’s been trimmed, they follow the shape of Surface Revolve1 (the red colored surface not shown here).

 

 

Now I’m also going to hide Surface Revolve2, in order to have a better view of the two extruded surfaces we just trimmed. I’m going to use Boundary Surface to create a couple of surfaces between the boundary edges of the two trimmed surfaces.  It seems to me that this feature is, in a way, very similar to Loft, and, as such, it can become more or less complicated when more edges or curves are involved in the process. In my case, however, I only have a couple of edges, no guide curves and no curvature or draft applied.

 

The two resulting surfaces are now knit together into one using the Knit Surface command from the Surfaces tab (or toolbar). We need them as one single surface for the next step.

 

Next, I’m going to show Revolve1 (the candy bowl) again and cut it using Surface Knit1 as my tool. This is done by using the Cut with Surface command from the Surfaces tab (or toolbar).  This command allows you to cut a solid body or bodies using an intersecting surface. The direction of the arrow in the graphics area points to the part of the solid body that will be discarded.

 

After hiding all the surfaces, the result is a decorative cut that can be mirrored about the Right plane, and patterned to apply it to the rest of the candy bowl.

 

 

 

And voila! Nice, isn’t it? I think I’ll get that Surfacing book off the shelf and start learning about the proper ways to create this and other cool stuff using surfaces in SolidWorks!