Creating a pattern is one of the most efficient features available to designers in SOLIDWORKS. By choosing to pattern an existing feature in a model, there is no longer the need to create multiple sketch/feature combinations in the feature tree; instead, there will only be one additional feature, a pattern. While SOLIDWORKS offers several different types of pattern features to create, this article with focus solely on the Linear Pattern Feature and how to properly apply this in 2 directions simultaneously.
So, what exactly is a pattern? Why is a pattern so useful in design? A pattern is a tool that allows the reuse of existing geometry, the seed, to create multiple copies, or instances, with just the click of a few buttons. Imagine the feature being copied took 15 minutes to create once, by using a pattern feature, what would have taken 6 hours of work, will only take 2 minutes to create 20 instances of this feature.
Here we have a simple control panel enclosure that needs ventilation holes along the front face. Instead of having to create a sketch with each individual hole needed, only one seed cut feature was created. This seed cut was then patterned in two directions to create the additional instances. This was achieved by the following selection sequence. In the image below, the first option that was selected was the “Cut-Extrude1” feature. It is considered best practice to select the seed reference before setting up the rest of the pattern details. This not only ensures that we know exactly what is being patterned, but also allows SOLIDWORKS to show a preview of how each setting is affecting the pattern.
This preview allows the user to visualize what is happening in the pattern, and make corrections to the input if there is an issue before even creating the pattern feature. The next step is to select the linear edge that corresponds with the desired direction of the pattern. In this case, Direction 1 is intended to be created in the horizontal direction. Next, Edge 1 (highlighted in red) was selected, and the grey arrow in line with Edge 1 is set to the desired direction so that the pattern is created in the correct direction. The desired spacing between centers of the instances was then input at 6mm, with a total number of instance columns of 46. This will now create 46 cuts, 6mm on center, in the horizontal direction. The same selections can now be made for Direction 2, where Edge 2 (highlighted in red) is selected for the pattern to be created in the vertical direction, and the grey arrow in line with it is set to the correct direction. The same 6 mm spacing between centers is input, but with only 14 rows of instance cuts this time.
Once the directional parameters are set for the pattern, the option of “Instances to Skip” can be activated. With this selection box active, a purple dot is shown at the center of each pattern instance. These dots can be selected to remove a specific instance from being created. In this example, all of the cuts that surround the E-Stop and Start buttonholes are to be removed, as they are not needed. Now that all the desired inputs have been added, the pattern can be created. So, instead of having to create nearly 700 vent holes individually, each instance was able to be patterned in a matter of minutes using the Linear Pattern Feature.
Get Certified SOLIDWORKS Services from Javelin
Javelin Experts can help you to: