Problem

This article is intended to assist in the creation of a Helical pattern. The method in this article can be used for both features and at the assembly level. The example will just be a simple hole-cut pattern cut into a cylinder at the part level, with pegs inserted at the assembly level. To create this, we will be using a Curve-driven pattern with a Helix as the guiding curve, along with options to reorient the patterned feature.

Solution

1. Open SOLIDWORKS
2. Create the Part model and the Feature to be patterned. The example below has a Cylinder with a Circular Hole Cut Extrude cut into it on the side.
3. Using the Helix command (Insert > Curve > Helix), create the path along which the pattern will follow. Height and revolution work well here; if you have specific angles and heights for your pattern, it is easy to extrapolate the curve.

4. The next step is to create the Curve-driven pattern (Insert > Pattern Mirror > Curve Driven Pattern). Select the Helix for direction 1, then select your instance. We recommend working on the helix side and using equal spacing, but you can also select a distance between the features along the path. 
5. Select the features to pattern as well. The important options here are selecting the alignment method 'Tangent to Curve' and selecting the cylindrical face as the Face Normal. This aligns the features to match the cylinder instead of an exact geometrical pattern.

The Curve-driven pattern can also be done at the assembly level with components. Using the same holes and helix from this sketch, we can make a peg stairway. The only main difference is the reference point of the component being patterned, as this can impact the placement of the pattern. In this example, the bounding box center works fine as the peg is simple and symmetrical.

The finished product is a spiral staircase effect with the patterned features.

For additional support, existing customers can submit a ticket or new customers can contact Hawk Ridge Systems.