# Solidworks tutorial: Circular pattern

Today we will learn how to create a Circular Pattern in Solidworks. This command allows you to create copies of objects arranged in a pattern both easier and faster. The type of patterns we are able to construct using this feature can be categorized in the following two types: The Line Patterns   and the Circular Pattern .

In this post, we will focus on creating a circular pattern.

The following image gives an overview of the steps and elements needed to create a circular pattern in Solidworks.

## Circular pattern in Solidworks

### Step 1

First Create a New Part

### Step 2

We need to select the desired plane. click on the front plane and select sketch

### Step 3

Create a circle and make sure its center is at the origin of the sketch, click on Smart Dimension and give 200 mm for diameter.

### Step 4

Select Extruded Boss/Base and give 20 mm thickness then click on okay.

### Step 5

Now create a new sketch on extrude boss surface

### Step 6

Create a small circle as shown on the image below. You will see a vertical line to assist you in centering the line properly. Put the circle 60 mm away from the origin of our cylindrical base with a diameter of 25 mm.

### Step 7

As you might have noticed, the small circle was created 60mm away from the origin of the sketch, but we did not indicate the plane it will be sitting on. We need to define the vertical location of the latter.

To do that, click on the origin of the small circle, hold down the CTRL key, and select the origin of our base. Add a vertical relation to these points in Property Manager.

### Step 8

Now, let’s make an extruded cut on the top face of the circle. First, change your view to isometric view then select Extruded Cut, select the Sketch and select Through All.

### Step 9

the Circular pattern needs an axes of revolution which is the center of our base but we cannot see it. So to activate the axes, select VIEW at the top then select view temporary axes or follow same as picture. You probably won’t see the axes unless you ZOOM in to look at the origin.

### Step 10

Click on the extruded cut in the design. Click on the Circular Pattern from the toolbar. If you do not have pattern in your toolbar you can find it from Insert >> Pattern/Mirror

### Step 11

Select the axes at the center of the base as we want the pattern to revolve around that axes. There are two different ways to create your pattern. If you check “Equal Pattern” then you can simply define the number of elements you want your circular pattern to have. You can activate Full Preview to see the pattern before applying it.

### Step 12

if you happen to uncheck “Equal Pattern”, you will need to indicate the number of elements and the angle between them.

### Step 13

To edit the pattern, you can simply select it from the design tree and select edit feature.

### Step 14

From Instances to Vary tool you can increment the spacing between the centers of the pattern instances and the dimensions of other features as well.

In the graphics area, click the Dimensions of the seed feature to display and populate the table. Add a value in the Increment column to increase or decrease the size and shape of the related dimensions.

You have just learned how to use circular pattern command in Solidworks. Using this trick will in some case cut down your designing time by a lot, therefore making one on the most important command to master.