Alignex Blog

Smooth Sketching: Using Splines in the SOLIDWORKS Sketcher

Jesse Butwinick on June 3, 2016 at 8:58 AM

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Look at any item sitting around you. You will find a majority of them have the company’s brand on it. Whether it is a protrusion, a depression, an engraving, a sticker, or a stamp, the spline tool will allow you to represent your logo on your product and help ensure your customers know who to come back to.

A spline is a special type of sketch entity which allows you to create smooth, rounded, and organic shapes. Find any electrical cord around you; this is a perfect example of a spline where it curves in all sorts of directions but it is one long entity.

Let’s take a look at the various ways to control a spline in the SOLIDWORKS sketcher.

First, the tool can be found under Tools > Sketch Entities > Spline. Under this dropdown you will also see a “Spline Tools” menu, we will get to those tools later.

Similar to a line, you will click to define which locations in space you want the spline to pass through.

After your second click the spline will look like a normal line.Straight Spline in SOLIDWORKS Sketcher
However, as you move to make a third click, you will find the shape begin to change. The entity will pivot about the previous points you selected.

SOLIDWORKS Sketcher gif

We will stick to two selections for now. I hit ESCAPE on my keyboard to end the spline. Selecting the spline now will reveal what are called the handles.Spline Handles in SOLIDWORKS Sketcher
Spline handles allow you to manipulate the geometry about each point you placed. There are three parts to the spline handle:

  1. The diamond shape allows you to change the angular direction through a point.
  2. The arrow allows you to modify the tangent magnitude.
  3. The point on the end allows you to modify both at the same time.

After you have moved one of the handles it will go from grey to blue, indicating it was activated and moved.Modified Spline Handles in SOLIDWORKS SketcherDe-selecting the spline causes the grey handles to disappear, but the blue ones remain visible.

As you manipulate the geometry you may find you need more points to control the spline. You can do this by right clicking on the spline and choosing Insert Spline Point and select anywhere on the spline. A new set of handles will become available. As best practice I always recommend to use as few spline points as possible to reduce the number of places where the geometry pivots. If you ever add too many spline points you can select the point and hit DELETE on your keyboard to remove it.

Bad vs. Good Splines in SOLIDWORKS Sketcher

Advanced spline options can be found under Tools > Spline Tools:

  1. Add Tangency Control: Similar to the spline point, you can select a location to force the spline to be tangent to.
  2. Add Curvature Control: Allows you to define the curvature of the spline at a specific point.
  3. Insert Control Vertex: Allows you to add additional vertices to a Style Spline.
  4. Simplify Spline: Automatically removes points in a spline which can lead to improvements in performance.
  5. Style Spline: Creates a spline based on vertices which form a polygon. This an alternative to the standard spline handle.
  6. Fit Spline: Lets you turn standard sketch entities into a single spline. Sharp corners will be converted to smooth rounds.
  7. Show Spline Handles: Toggles the visibility of the spline handles.
  8. Show Spline Control Polygon: When you select an existing spline, toggle this setting to control the geometry using control polygon nodes.
  9. Show Inflection Points: Toggles the icon displaying where the spline reverses directions, for example from clockwise to counter clockwise.
  10. Show Minimum Radius of Curvature: Toggles the display of the smallest radius along your spline.
  11. Show Curvature: Toggles the curvature scale, which displays the change in curvature and indicates the direction of curvature.


Now that you know some of the basics of splines lets apply this to a real world scenario. I want to use the spline tool to create our company logo. First I will insert a picture of our logo into a sketch.

  1. Start a sketch on your desired face or plane.
  2. Go to Tools > Sketch Tools > Sketch Picture.
  3. Browse for the image and once placed you should ensure it is scaled appropriately so your sketches logo is not too large or too small.

Sketch Picture in SOLIDWORKS Sketcher

With my logo inserted into the sketch I can now trace over the geometry. Remember you can use both splines and other sketch geometries to trace out your logo.

Traced Alignex SOLIDWORKS Logo in SOLIDWORKS Sketcher
Traced Sketch of Alignex Logo in SOLIDWORKS Sketcher

And finally extrude the geometry as needed.

Alignex Logo Sketched in SOLIDWORKS Sketcher

That’s all there is to know! Best of luck modeling up your company logo, and don’t forget our experienced application engineers are here to help you get the most out of this tool.

Plus, be sure to subscribe to the Alignex Blogfor the latest expert advice and updates delivered straight to your inbox.

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