2019 How to make use of Circular Sketch Pattern in SOLIDWORKS

Summary

What is a Circular Pattern in SolidWorks?

Circular Pattern: A circular pattern is the repetition of a given entity, multiple times around a defined axis or point. They are driven by the number of instances and the angle between them. Circular patterns can be used in many situations and in any application where rotational symmetry is desired, not just circles and spheres

Multiple instances of a specific entity or entities (sketch elements, features, parts, etc.) around a central axis or, in the case of a sketch, a central point. Every option or tool after this is just a modification of this originally definition. Circular patterns can be applied to every level of SolidWorks modeling including sketches, parts, and assemblies.

Getting the most from your patterns

Patterns are a great time saver within SolidWorks. Many people are familiar with basic linear patterning, the ability to continue an instance out as many times as necessary is very useful. Often overlooked, however, are circular patterns. In this article, we are going to go over the circular pattern, how to use all of its different variations, and explain how this tool can be useful even when what you’re after isn’t strictly circular. Keep in mind, this article assumes a basic knowledge of SolidWorks modelling techniques, parts, assemblies, and lingo.

What is a Circular Pattern?

For the uninitiated, the circular pattern can be very confusing, but always keep in mind the basic idea of what a circular pattern is, multiple instances of a specific entity or entities (sketch elements, features, parts, etc.) around a central axis or, in the case of a sketch, a central point. Every option or tool after this is just a modification of this originally definition. Circular patterns can be applied to every level of SolidWorks modelling including sketches, parts, and assemblies. Below, we take a quick look at all of these different variations of the circular pattern and all the options provided by each different version.

Circular Patterns in SolidWorks Sketches

The first place that we are going to look at the circular pattern is the most basic first step in parametric modeling, the sketch. Once a sketch is open, SolidWorks enables the sketch tool, Circular Sketch Pattern.” Upon selecting the circular pattern, the property manager appears as shown in the image here.

In this case we used the circular pattern to quickly make a hexagon with one open side. There are other ways of making this shape that are perhaps faster, but this example starts to hint at the versatility of the circular pattern. Once we click the green check to confirm our choices the viewport looks like this.

Notice that the pattern added a dimension and a series of relations. The dimension can be seen in the upper left of the pattern, and it reads “6”. This is the number of instances that the pattern has created, and it can be changed just like any other dimension. There is also a relation that has been added. This is a “Patterned” relation and maintains the pattern relationship between all the entities that the pattern created. This about wraps it up for Circular sketch patterns, but this isn’t nearly all that SolidWorks can do when it comes to Circular patterning.

Circular Patterns in Parts

When it comes to parts, The “Circular Pattern” feature is very similar to the “Circular sketch pattern” tool. For the purposes of brevity, we will only spend time highlighting the obvious differences. First of all, the selections for the direction will now have to be an axis, and solid geometry can now be selected. Additionally, we see the option for a second direction which, if selected, allows us to pattern in both directions around the same axis, and we can even select a different spacing for each direction. We also see the option between “Instance spacing” and “Equal Spacing” this is the same option as before with a different appearance. The “Equal spacing” option spaces all instances the same throughout the specified angle, whereas the “Instance Spacing” option spaces each instance by the specified angle. The next difference that we notice, is the “Features and Faces” and the “Bodies” options. If you select “Features and Faces” It allows you to pattern design elements of a specific body. In general it is best to pattern features, but in the event you are working with a model without a feature history, patterning faces becomes invaluable. If you select the bodies option, it allows you to pattern entire solid bodies in a multi-body part. There is also a new section labeled options. Checking the “Geometry pattern” option, tells SolidWorks to pattern the exact geometry of the features selected, and ignores solving end conditions for each instance. This can be somewhat complicated to understand, but at the end of the day we tend to recommend leaving this box checked unless you run into an error, as it can drastically reduce rebuild time to use this feature. Checking “Propagate visual properties” tells SolidWorks to keep the same appearances on the patterned faces or bodies. Finally, we see the “Instances to Vary” section. If you activate this section it will allow you to change specific instances by some number of degrees from the location that they would otherwise fall in the pattern. To see Circular patterns in action at the part level, let’s say we have a sheet metal cover that needs identical mounting holes on all 4 sides. If we create the first set of holes, all the others can be created with a circular pattern.

In this case we unchecked the “Geometry pattern” box because each of the holes would need to solve the end condition to intersect the model. If we leave this box checked we only see the holes on the top and bottom flanges.

Assemblies and Circular Patterns

There is one last area we will look at when it comes to circular patterns and with what we’ve learned so far, this one is simple by comparison. This option is an assembly feature listed as “Circular Component Pattern”, and all the options shown in the property manager should be familiar at this point. The only difference is that this pattern is meant to pattern components in an assembly. Let’s take a quick look at one simple way we might use this to achieve a result that at first glance seems as far from a circle as you can get.

In this example we have a simplified, cartoon-like hanging sign. Placing individual components such as these letters and decorative elements can be a time consuming task, and in industry, time is money. Unfortunately these letters need to be read from left to right on both sides of the sign so a traditional mirror cannot be used. There are multiple solutions we could use here, but fortunately for us this is a great place for the creative use of a circular pattern. If we create a pattern around a central axis with the instances set to 2 and “Equal spacing” checked we get exactly what we’re looking for.

Hopefully you’ve learned a thing or two about how to get the most out of SolidWork’s patterning capabilities using circular patterns. Whether you are using them in sketches, parts, or assemblies, circular patterns can be great time saving tools, and they aren’t just for circles.

Trevor Holloway

Trevor Holloway is a mechanical engineer and CAD expert. He is certified in SolidWorks at the expert level (CSWE), and has years of experience in designing products for manufacture. Trevor Holloway is driven by turning ideas into reality through engineering. He consistently seeks to push the limits of his skills and expand his knowledge base with the intent to innovate and solve problems. He enjoys viewing the engineering process holistically, from design to implementation, and always seeks to take a hands on approach. He is certified by SolidWorks as a SolidWorks Experts (CSWE).