Surfacing Tutorial: Chess Piece

This is a tutorial for a part I modeled a few years ago and never did much with. It is a chess piece.  This is not a full step-by-step tutorial, but rather kind of a roll the part back and watch over my shoulder kind of tutorial. If you want to actually model a part like this, my best advice is to read through this, then download the part, roll it back and copy features.

You can download the model here. It is saved in pre-2007 format, although I don’t remember how far back it goes. It may be as far back as 2004. The zip file is 11 mb+.

Most of the concepts used here are fleshed out in more detail in my surfacing book. The book uses more advanced techniques that became available after this part was originally modeled.

First, this part was originally just a modeling/rendering exercise, it was not meant to be a production part. I didn’t take any steps to make sure that all features were manufacturable, several are obviously not. The artistry of the part is questionable because I did it myself, and I’m an engineer. Anyway, people tend to point out the obvious if you don’t do it first.

So where do you start on a part like this? I always start with a layout sketch. A layout sketch is just a sketch in the beginning of the part that you will refer back to frequently. This sketch drives the shapes of the rest of the model. I try not to use the layout sketch in other features directly because I want it to remain at the top of the tree. It would be great if there were a function that allowed you to make a sketch stick at the top of the tree without being consumed by other features.

Here’s the layout sketch that I used. The dimension is just to establish the size of the part so I have an idea of scale. Notice that I used straight line construction lines to establish a centerline of the part and the height. The splines are free hand splines, without relations to other entities. Splines also tend to be overbuilt, meaning that they are longer than they need to be.

Ideally, to avoid consuming the layout sketch, you should make copies of sketch entities using Convert Entities if you want to use any of the splines for something. In practice, I didn’t do that in this part, so you have to refer to the “profile layout” sketch under the first surface loft feature to find the sketch.

I used offset planes and several sketches along with the two roughly vertical roughly parallel splines for the horse’s neck to establish loft profile sketches.

Here I used the Selection Manager to select the two guide curves. The guide curves are individual entities within the layout sketch. Gone are the days when you had to place one sketch element in each sketch. In fact, you could have laid out this whole loft in a single 3D sketch. There are some advantages to doing this, but I recommend against it. Working with 3D sketches is quirky at best. It may be conceptually more intuitive, but practically, it’s buggy and frustrating. Because of that, I tend to use the more traditional approach with several individual 2D sketches and regular Reference Geometry plane features rather than the 3D planes available in 3D sketches.

The construction lines at the end of the loft section splines are just to establish that the tangency was correct at the symmetry line. This technique is a legacy from before spline handles could be used more effectively for the same thing.

Modeling half of the part like this will give you a split around the part when you mirror it. In some cases, a split is not desireable, so you could instead create closed loop spline profiles.

To draw the several splines needed for this, I simply drew the first one with all of the relations and shape, and then copied the spline to the other sketch planes, and reassigned external relations. It would be nice if external relations copied along with a sketch, and reconnected themselves, but they don’t .

The next step with this was difficult. I just identified some geometry that I could actually make. Sometimes you just have to model what you know, and let things fill themselves in as you go. Here again, I used sketch entities from the layout as guide curves.

This step wasn’t as well defined. I extruded a surface for the bottom of the jaw, really not sure what I was going to do with it to be honest. Then I added a projected curve to make part of the mane.

The mane started as a Ruled surface, but I wound up with a sweep because the ruled surface was too perfect, it didn’t waver the way I wanted it to. Notice that I used a 3D sketch to extend the projected curve. You can’t always get away with this. It’s kinda sloppy, but on a part like this, I needed more slop and less precision.

From there I trimmed back part of the neck so it could transition into the rest of the head. Remember that overbuilding splines and surfaces is good. Remember that. Anyway, I used a spline and a projected curve to make the top part of the nose/mouth. Fortunately I wasn’t terribly picky with this. If you are trying to make something anatomically correct, you will need to make more sketches and curves. Also note that the tangency and curvature continuity are not very good at the intersection of the new surface.

I lofted in the chin, trimmed out a nostril, and made a construction surface covering the lower half of the nostril so that I could make the upper nostril cover using a Fill surface. In a more modern release, I would have used some boundary surfaces.

In quickie modeling like this, sometimes you do things without taking much care about it, and in the end stuff like that shows. If this had been a production model, it would have taken me a couple of days instead of a few hours to get through the model, but it serves for reference if you have never done work like it.

The top of the head used surprisingly little data to create the loft. just a couple of sketches and some existing edges. It is best if you can get away with using fewer controls for loft features. Fewer sketches and curves generally lead to a more natural looking loft, although sometimes you do need more profiles to rein in a problem area.

In this case I used a 3D sketch along with an intersection curve, making the 3D spline tangent to the end of the intersection curve to try to make the side of the face transition naturally off of the back of the neck. The flag calling out 3DSketch5 shows how the 3D spline connects to the construction geometry on the face of the first loft.

Some small trims along with a loft to close in the jaw helped to close in the part. Just so it’s clear, SolidWorks is not great at character design. This is the kind of thing probably best done in mesh modelers like 3dsmax or Maya. Because SW is so process-based, everything takes longer to set up. Making a change early on in the model means redoing a good bit of the modeling. Again, this model was done for entertainment and learning, which is the way you should approach it.

Next I used some extruded surfaces to close off around the mane and the mouth to make the part easy to mirror and then solidify. There were a few other minor trims and small lofts in there as well just to blend things together. Notice that there are no fillets used in the model. All of the blends are lofted.

Trimming surfaces is sometimes easy, and sometimes not so easy. For me, when it is not so easy it is because of the visualization, and seeing which part you want to keep and which you need to get rid of. When working with a part in half like this, the visualization is much easier than if the part is hollow.

Mirroring the part shows that some of the surfaces are of better quality than others. Notice the breast of the horse looks good, but the mouth does not. Closer examination shows several areas that could have used more attention.

The ear at this point is a separate body, and was not mirrored with the rest of the part.

One feature that worked out well on this part is the setback fillet used on the mane. You don’t see that many examples of a setback, but this one worked well. Setback fillets can be created with constant or variable radius fillets.

The ears were completed by copying the original loft surface, and then using a solid loft feature to loft between the surface bodies. Lofting a solid between two surface bodies is not a well advertised capability of SolidWorks, but in situations like this, it works well.

And that’s the quick over-the-shoulder walk through on this part. If you make one and would like me to post it here for people to see, just send me a file, and I’ll do it! Best of luck, and I hope you found this a useful quick tutorial.