Hi there, it’s me again, Peter. This time I’ll teach you something about linear patterns in SolidWorks. Because you need to use them in your designs. If you don’t use them already, please start right now. Because you are wasting money.
Whether you just don’t add all copies of a part to an assembly or you copy in every fastener manually, you are wasting money. If you go through the effort of adding each item by hand, you are wasting time (=money). If you are refusing to add each item by patterns, you are creating technical debt that will come back and bite you. Incomplete models will result in lower estimates for masses, loads and cost. A bolt that isn’t added to a design can’t be checked on interferences with other parts, it can’t be checked on the thread depth or whether a tool can actually reach the bolt. So complete your assembly, and use patterns.
Linear patterns in sketches
You probably know this feature, but I’m stating it anyway for a complete overview. Get a part going, create a sketch entity that you want to copy (I’ve created a Center Rectangle here), select it (I don’t want the center lines to get copied here, so I’ve only selected the contour) and click the Linear Pattern button in the sketch toolbar.
The menu shown below will pop up. It only supports creating a pattern over the X-axis and Y-axis, but you can play with the angles to increase your options. Unfortunately you can’t increase the spacing and the number of instances by scrolling your mouse over the respective fields, that option would’ve been nice to have.
If there are instances that you would like to omit, use the option at the bottom of the menu and select the items that you want to skip.
The linear pattern feature will only add a “Patterned” relation to the copied items. If you choose to add dimensions, it will add the spacing dimension and a connecting line between the first two instances, but the new instances are never fully defined immediately. Making the connection line horizontal or vertical can quickly define all instances fully.
Linear patterns in parts
When you are creating a part, you can pattern features, bodies and/or faces. I usually pattern features, although I learned today that patterning or mirroring bodies instead of features can make large assemblies feel significantly less sluggish.
Pre-selecting is once again possible. I have advised you to add three axes in my post on the best practices in part design, and I’m using the X- and Z-axes here. I have skipped one instance and this a matrix can be seen in the preview. Enabling “Pattern seed only” will result in a horizontal and a vertical array of items instead of a complete matrix.
If you want to vary the increment on one of the instances, enable the bottom option in the menu. You can then select the pink dot (they call it the Instance Modifier) and vary the distance between copies. Feel free to play with the other options in the menu.
Creating the pattern shown above failed by the way. Because I am creating separate bodies, you need to select “Bodies to pattern” instead of “Features to pattern”.
Linear patterns in assemblies
The pattern feature in assembly mode does exactly what you would expect, this can be seen below. I have selected an edge in the Y direction to create the pattern.
In assemblies you have a few more tricks that you can use to your advantage. You can for example right click an instance in the tree and click the Configure Component option to select a configuration for that instance only! This is a killer feature if you have a tapering housing and you want to add multiple stiffener plates with different dimensions, which was the situation I found myself in.
To get a quick overview of what the three features can and cannot do (in Solidworks 2013 at least), here’s a nice table. I really wish SolidWorks would be a little more consistent by enabling all options in all three places, but I guess I’ll have to be patient. I really hope you have learned something from this post, please let me know if you did! Happy patterning 🙂