2019 How to make use of Circular Sketch Pattern in SOLIDWORKS

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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.

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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.

To get started using this menu, we start from the top down. The first box, sometimes known as “direction,”  is looking for a point that lies in the sketch plane, this will be the center of the circular pattern. The repeated entities will all be rotated some number of degrees around this center. This should be a point or vertex of some sketch entities, and solid geometry cannot be selected. Just to the left of this field is a button. Once you’ve selected your instances to pattern, you can select this button to change the direction that the instances are patterned around the center, clockwise to counter-clockwise or vice versa. The next two fields are called “Center X” and “Center Y” and will have a distance value entered into each of them. This will move your selected center point to some virtual point the specified distance in the local X and Y coordinates away from the originally selected point. In general, we find that it is more advisable to merely place a sketch point in the right location and use it as your defined center, but these fields can be useful in the right circumstances. The next field is “Spacing,” and it takes a value in number of degrees.  It determines the extent of the pattern and is affected by the “Equal Spacing” check box, and the “Number of Instances” field found beneath it. If equal spacing is checked than the pattern will place the number of instances in an arc with the specified value in the “Spacing” field, and with an equal number of degrees between them. If “Equal Spacing” remains unchecked then the “Spacing” field will be the number of degrees between each of the specified instances. Next there are two check boxes, “Dimension radius” and “Dimension angular spacing.” These will determine whether or not a parametric dimension is added to the angular dimension and/or radius of the pattern automatically. Note that “Dimension angular spacing” can only be checked if “Equal spacing” is not checked. Also, keep in mind that “Dimension radius” can cause the center of your circular pattern to be floating and the resulting pattern to be undefined. The “Display instance count” checkbox, if selected, creates a dimension that is simply a whole number that defines the number of times that a pattern is repeated. The next two fields are “Radius” and “Arc Angle” and serve the same purpose as “Center X” and “Center Y.” The “Center X” and “Center Y” fields move the center in cartesian coordinates, whereas “Radius” and “Arc Angle” move the center in polar coordinates. Note that changing one set of these fields will change the other two as well. Finally, The last two fields are “Entities to Pattern” and, if you open the drop down menu, Instances to skip. After highlighting the “Entities to Pattern” field you select all the entities that you would like to be included in this pattern. Once those entities are selected, you can highlight the “Instances to Skip” field by selecting any of the previewed instances shown based on the selected options, the pattern will know to skip over these as if they weren’t in the pattern at all. And that’s it for circular sketch patterns. The best way to internalize and really understand all this is to mess with the settings for yourself, using this guide as a tool for understanding. To give you an idea of what a basic pattern looks like, see the image below.

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.