Pattern commands are a designer’s best friend in terms of replication and improving overall efficiency. Linear, Circular, and Curve driven patterns are all common commands used by the everyday CAD user. This blog will guide you through using these three pattern features in SolidWorks and provide context as to when they can be used to simplify the modeling process.
Linear Driven Pattern
The Linear Pattern Command is used to drive features, faces, or bodies in a linear direction. This feature helps save time by cutting down the repetitive movements of adding a bunch of holes or other forms of geometry. In Figure 1, the location of the linear pattern command in addition to the curve and circular driven pattern commands are shown.
Figure 1: Command Locations
Using an existing hole wizard feature, the linear pattern will systematically generate identical holes across the model. The first step in executing a linear pattern is to select a desired feature in the Features and Faces selection box or by preselecting prior to hitting the Linear Pattern Command (Figure 2).
Figure 2: Selecting the Feature
After selecting “3/4-10 Tapped Hole1” feature in this case, the dimensions defined in the feature appear and can be used to aid in the patterning process (Figure 3). The next step in the command manager is selecting up to two linear pattern directions. For this example, the two 4.00 dimensions were used to define two pattern directions, as they are in the desired linear direction to make an equally spaced square hole pattern. Additionally, there is also the option to select edges, faces, planes, and other geometry in the preferred linear direction.
Figure 3: Setting Direction
Now that the directions are set, the next step is to fill out the necessary parameters for each direction required to make the pattern. The first parameter is the number of instances. As seen in Figure 4, the desired “3/4-10 Tapped Hole1” hole feature pattern will add 2 instances in both directions creating a 2x2 square. The distance in both the vertical and horizontal direction was set to 12 inches in order to keep the pattern centered to the square piece.
Figure 4: Hole Instances
If the desired pattern direction is oriented incorrectly, the opposing arrows button (highlighted) next to the selection box flips the direction relative to the reference selected. Figure 4 also shows a pattern preview on the part (enabled from the checkbox on the bottom of the command manager), which will help verify the orientation and intended pattern direction.
Lastly, as seen in Figure 5 the green check mark in the top left corner of the manager will execute the command and reveal the pattern on the model.
Figure 5: Final Check
Curve Driven Pattern
In the next example, the Curved Pattern Command is used to execute a hole pattern consistently about the outer curvature of a cam (see Figure 6). The setup and command manager layout are nearly identical to the linear pattern and the steps are listed below as follows:
- Select the feature/face/body to pattern
- Select a curved reference (this can be an open or closed curved geometry)
-Adjust the direction, spacing, and number of instances in the desired pattern
-Preview the pattern and then execute.
In this curve driven pattern example (see Figure 6), I selected a hole feature, the edge of the cam as the Direction 1 reference and adjusted my instances and spacing to 4 and 0.425 correspondingly. As with the linear pattern, up to two different directions can be added.
Figure 6: Curved Pattern About an Edge
Circular Driven Pattern
The Circular Pattern Command is an excellent tool used to replicate features, faces, or bodies in a rotational manner about an axis. In this example (see Figure 7), I show how to replicate an extruded cut with filleted corners about a round piece of tubing.
Figure 7: Circular Pattern Overview
Similar to the linear and curve driven pattern, the first step is selecting a feature (or features in this case) to replicate in the Features and Faces selection box or by preselecting prior to hitting the pattern command.
Figure 8: Selecting Features and Faces
After the cut-extrude and fillet are both selected, the intended rotation axis is selected in the top selection box under Direction 1 in the command manager (see Figure 9). The rotation direction can be toggled using the arrow button to the left of the selection box. The next step is to select the degree of spacing and number of instances.
Figure 9: Circular Pattern Parameters & Preview
In this example, since the original extruded cut through both sides of the pipe, the pattern only needed to rotate the feature 180 degrees instead of 360 to complete the cut all the way around, so I chose a 45-degree spacing and 4 instances to complete the pattern across the tube. As with other pattern features discussed, up to two directions can be selected.
That’s all for now! You now know the basics in Linear, Curved, and Circular Patterns. If you like the content or have questions, signup for our email list to stay in the loop for solutions or weekly content.