# Curves Ahead: How to Handle Curves and Splines in SOLIDWORKS

There are two different flavors of shapes we model – prismatic and curvy. We’re going to focus on the latter – geometry that isn’t straight and square but can be swoopy, curvy or organic. In SOLIDWORKS there are a lot of tools and features available to you to help you create your curvy shape. We’re going to take an in-depth look at all of them so you can be an expert on curvy parts and create complex shapes and geometry with confidence and ease.

When we’re talking about curves, we are usually talking about extremely complicated shapes that are uniquely constructed with many shapes. But no matter how complex they become, their origin is always simpler geometry: arcs and splines. Arcs are basic, and they’re introduced on the first day of an “Intro to SOLIDWORKS” class. Splines are a different story.

# Splines

Splines have been around since the early days of SolidWorks 95, which included the traditional B-spline tool. B-spline is short for basis spline. Fast forward to SOLIDWORKS 2020, and the Spline tool has come a long way in terms of features and tools even though it remains essentially the same at its core.

A spline can be defined and modified by 3 basic parts:

## Spline Points

You can drag the spline points around the graphics area to manipulate the shape of the spline. You can remove a spline point by right clicking on it and pressing delete, or you can add a spline point by right clicking on the spline and selecting “insert spline point.”

## Spline Handles

You can manipulate the spline handles at each spline point to edit and define the weight or magnitude and direction of the spline at that point. Pro tip: The color of a spline handle changes from grey to dark blue after you’ve manipulated it.

## Control Polygon

Introduced in SOLIDWORKS 2019 you can manipulate a B-spline using its control polygon. Right click on the spline and choose show control polygon. You can then drag it to manipulate its shape.

# Style Splines

Did you know that a new spline tool was introduced nearly 20 years later? SOLIDWORKS 2014 gave us Style Splines, which are based on Bezier curves and offer an alternative to traditional B-splines. Instead of being sketched directly, the spline is drawn via control points which form its control polygon. This is similar to the pen tool in Adobe Illustrator.

A Style Spline has no through points and only has one span between the two end points. The main difference between B-splines and Style Splines is how you create and add definition to the spline.

# My Top 3 Tips for Working with Splines

1. Draw as few points as possible This enables you to create the smoothest shape. You’d be amazed at the shapes you can create using 2-point splines. You can always add more spline points if you need with a right click on the spline and picking “Insert Spline Point.”
2. Use the evaluation tools – There are many tools you can use to help draw the perfect spline (see more about this below).
3. Use Relations – You can define splines by adding relations to features like the spline handles of B-splines and the control polygon of Style Splines.

# Continuity, Curvature, & Smoothness (Important Update for 2020!)

When creating a curve one of the most important things to consider is its smoothness. Smoothness isn’t a technical word, it’s just what most designers use to describe the curvature of the shape.

Curvature, however, is a technical term – specifically, radius of curvature. This is essentially a measure of the change of shape of a single point, measured at every point along a curve. SOLIDWORKS can measure curvature with the click of a button, even though the complete derivation of a curve is extremely complicated and involves advanced third year calculus topics.

The images below show the complete derivation of radius curvature.

The concept of curvature becomes most important at the boundary between two curves. We call this continuity. Continuity is the mathematical term for describing the smoothness or flow at the intersection of adjacent curves. In SOLIDWORKS, there are levels of continuity that can be achieved using relations—starting at level G0 and increasing to level G3. The G stands for geometric. There is also type C continuity which is a more stringent definition of continuity.

• Level 0 (G0) – Contact
• Level 1 (G1) – Tangent
• Level 2 (G2) – Curvature Continuous
• Level 3 (G3) – Torsional (New to SOLIDWORKS 2020)

One way to think of the level of continuity in SOLIDWORKS is to move from left to right on the context toolbar for adding sketch relations to a shared vertex. See the image, where G0 starts on the left and increases to the right to G3.

Before we continue discussing curvature and continuity, let’s introduce some of the tools that are used to help visualize and evaluate both curvature and continuity. Below are, in my opinion, the two most useful tools: Zebra Stripes and Curvature Combs.

# Zebra Stripes

Using SOLIDWORKS Zebra Stripes to put stripes on a bare zebra may look unnatural, as shown in the image to the right.

However, these are a visualization tool that enables you to easily see changes in a surface. When you turn on Zebra Stripes, the entire model is painted with black and white stripes which show you how adjacent surfaces flow from one to another. A visual inspection of the zebra stripes alone can determine what type of boundary exists between two surfaces.

# Curvature Combs

Curvature combs create “sticks” along a curve which exaggerate and visualize the slope and curvature of the entity. Curvature combs can be displayed on a 3D surface or a 2D sketch entity. To view them in a sketch, just right click on an entity and click “Show Curvature Combs.”

It’s also a good idea to turn on “Curvature Comb Bounding Curve.” It really takes your curvature combs to the next level and helps better visualize the flow of your curves. This is a system option you’ll need to turn on to use. See the comparison below.

Now that we have introduced the tools that can be used to inspect and interpret curvature and continuity, let’s go over the different cases and see how Zebra Stripes and Curvature Combs can be used to visualize these different cases. One thing to keep in mind is that each one of these continuity conditions builds upon the previous one. For example, for G1 continuity to exist, G0 is prerequisite.

# G0 – Contact

The most basic level of continuity is contact. This means adjacent entities share a common end point (they are in contact).

Curvature combs have the same magnitude, but they’re not parallel where they meet.

Zebra stripes do not match up at a G0 boundary.

# G1 – Tangent

The next level of continuity is tangent. This is where adjacent faces share the same angle at the boundary. This is commonly seen at fillets.

Curvature combs are parallel where they meet, but are of different lengths where they meet.

Zebra stripes partially line up, but they may abruptly change direction at the boundary.

# G2 – Curvature Continuous

The next level is curvature continuous. Remember, G2 can’t exist without G0 and G1 continuity existing as well. G2 continuity will have a curvature blend with a lead in. We first saw this as a sketch relation in SOLIDWORKS 2015, and a fillet type in SOLIDWORKS 2016.

Curvature combs are parallel, and they blend together seamlessly.

Zebra stripes line up perfectly and blend in with one another so you can’t see the boundary.

# G3 – Torsional

G3 continuity is new with SOLIDWOKS 2020. This builds upon G2 continuity in that is has equal curvature plus equal rate of curvature. This is important because with G3 you can make true Class A quality blends. Class-A Surfacing has finally arrived in SOLIDWORKS 2020!

You won’t notice an obvious difference in zebra stripes or curvature combs for this type of continuity. However, if you’re designing Class-A surfaces, you’ll definitely want to consider using this relation for added smoothness between curves.

That’s curvature in SOLIDWORKS. There are various levels of smoothness which can be achieved for any type of design project. Plus, there are powerful tools to help you visualize and interpret your model to get its shape just right. After reading this article, you hopefully have the knowledge and confidence to tackle any design challenge no matter how complicated its shape might be.