SolidWork 2013 - Creating Patterns

CREATING PATTERNS

Sometimes, while creating a base feature, you may need to place the sketched entities in a particular arrangement such as along linear edges or around a circle. The tools that are used to create the linear and circular patterns of the sketched entities are discussed below.

Creating Linear Sketch Patterns

CommandManager: Sketch > Linear Sketch Pattern

SolidWorks menus: Tools > Sketch Tools > Linear Pattern

Toolbar: Sketch > Linear Sketch Pattern

In SolidWorks, the linear pattern of the sketched entities is created using the Linear Sketch Pattern tool.

To create the linear pattern, select the sketched entities from the drawing area. Then, choose the Linear Sketch Pattern button from the Sketch CommandManager; the Linear Pattern PropertyManager will be displayed.

Also, the preview of the linear pattern will be displayed in the drawing area. Note that if you have not selected the sketched entities to be patterned before invoking this tool, you will have to select them one by one using the linear pattern cursor. The names of the selected entities are displayed in the Entities to Pattern rollout.

The options in this PropertyManager are discussed below.

Direction 1 Rollout

The options in the Direction 1 rollout are used to define the first direction, distance between instances, number of instances, and the angle of pattern direction. When the Linear Pattern PropertyManager is invoked, you will notice that only the options in the Direction 1 rollout are active. Select the sketched entities to be patterned; a callout will be attached to the direction arrow. The edit boxes in this callout are used to define the number of instances and the distance between the instances to be created. You can also define the distance between the instances by dragging the select point provided on the tip of the direction arrow. By default, direction 1 is parallel to the X-axis. If you need to select any existing line or a model edge to define direction 1, click in the selection box in the Direction 1 rollout and select a line or an edge of the existing feature. Click on the direction arrow or choose the Reverse direction button from this rollout to reverse the pattern direction, if required. The Angle spinner is used to define the angle of the direction of the pattern. By default, the direction of the pattern is set to 0-degree.

Direction 2 Rollout

The options in the Direction 2 rollout are used to create pattern of the selected entities in the second direction. You will notice that the preview is not displayed in the second direction. This is because the value of the number of instances is set to 1 in the Number spinner. This means by default, only one instance will be created in the second direction and that is the parent instance. If you set the value of the number of instances to more than 1, then the options in this rollout will be enabled. All options in this rollout are the same as the direction 1 rollout.

Creating Circular Sketch Patterns

CommandManager: Sketch > Pattern flyout > Circular Sketch Pattern

SolidWorks menus: Tools > Sketch Tools > Circular Pattern

Toolbar: Sketch > Pattern flyout > Circular Sketch Pattern

In SolidWorks, the circular pattern of the sketched entities is created using the Circular Sketch Pattern tool.

To create the circular pattern of an entity, select it and then choose the Circular Sketch Pattern tool from the Pattern flyout in the Sketch CommandManager; the Circular Pattern PropertyManager will be displayed and the preview of the circular pattern will be displayed.

The options in the Circular Pattern PropertyManager are discussed below.

Parameters Rollout

The options in the Parameters rollout are used to define the centerpoint of the circular pattern, coordinates of the centerpoint of the reference circle, number of instances, angle between the instances or the total angle of pattern, radius of the reference circle, and so on.

The Reverse direction button is used to reverse the default direction of the circular pattern. The selection box on the right of this button is used to select the centerpoint of the circular pattern. By default, the origin is selected as the center of the circular pattern. You can modify this location by using the Center X and Center Y spinners. Alternatively, click once in the selection box and select the point that you want to be the new centerpoint or drag the center point to the new point. You can set the value of the number of instances using the Number of Instances spinner.

By default, the Equal spacing check box is selected and the value of angle in the Angle spinner is set to 360-degree. When this check box is selected, the specifi ed number of instances are equi-spaced radially. If you modify the default value in the Angle spinner, the angle between the instances will be adjusted accordingly. However, if the Equal Spacing check box is cleared, then you need to specify the incremental angle between the instances using the Angle spinner.

The Radius spinner is used to modify the radius of the reference circle around which the circular pattern will be created.

The Arc Angle spinner provided in this rollout is used to modify the angle between the centerpoint of the original pattern instance and the center of the reference circle.

The Dimension radius and Dimension angular spacing check boxes are used to display the radius and angle between the pattern instances of the circular pattern. On selecting the Display instance count check box, the number of instances will be displayed in the resulting sketch pattern.

EDITING PATTERNS

You can edit the patterns of the sketched entities by using the shortcut menu that will be displayed when you right-click on any instance of the pattern. Depending on whether you right-click on the instance of the linear or circular pattern, the Edit Linear Pattern or Edit Circular Pattern option will be available in the shortcut menu.