In a previous Tech Tip, we looked at curve driven patterns in SolidWorks using a 2D path. Now, let’s look at using 3D curves to drive the pattern. There are a couple of steps to know about to get the results we want. Here’s a 3D curve and a solid body to pattern along the curve.
If we want the body to keep its orientation in space, we use the “Align to seed” option to get the following pattern:
If we want the solid body to twist in space while following the path (like a string of railroad cars going around a curve), we use the “Tangent to curve” option, and this requires a surface along the curve to control the tangency. The surface has much the same function as a guide curve, and it is selected in the “Face normal” window. What’s essential is understanding the selection must be a single face, not just a surface body, and the face must extend the entire length of the path.
To construct the face, we make a sketch plane normal to the path at its end and sketch a short single line. Then the line is used to sweep a surface along the path:
This sweep doesn’t meet the single face requirement because it has 7 faces. That’s a result of sweeping along a path that has 7 arcs and lines. To create the surface as a single face, we convert the path to a single 3D sketch entity. Fortunately, there’s a tool to do just that. It’s called Fit Spline, and it can be found at Tools>Spline Tools>Fit Spline or in the expanded spline icon on the Sketch toolbar. Here’s the Fit Spline dialogue:
With the 3D sketch open for editing, start the Fit Spline command then uncheck “Delete Geometry” and “Closed Spline”. Next, right click the end element of the sketch and choose the menu option “Select chain” which will select all the sketch elements. The command makes a single, continuous spline that closely matches the original sketch, and turns the original sketch elements into construction geometry. The tolerance setting adjusts how closely the spline follows the sketch. One great advantage is that the original dimensions and constraints still control the construction geometry which in turn controls the spline. This makes editing easy. Exit the sweep command to see the surface is now just a single face:
Next, open the Curve Driven Pattern command but this time click the Tangent to Curve option, and click the swept face for the “Face normal” box. This is the pattern preview:
When the pattern is created, you can hide the 3D sketch and the swept surface.
You can also use an edge of a part (or chain of edges) to guide the pattern. In this case, start a 3D sketch, and start the Fit Spline command. Right click the first edge and click “Select tangency” in the menu. This creates the single composite spline to use the same way as the example above. Edits that change the shape of the part and the selected edges will update the pattern.