Customization options

The following are some of the different options that accompany the Offset Entities command:

• Add dimensions: This option makes the offset fully defined upon implementation, just like in our previous example. Unchecking this option will create the offset; however, it will not add the offset dimension, thus making it undefined. 
• Reverse: This changes the location of the offset. By default, the offset is applied outward. Checking this option makes the offset go onward.
• Select chain: This command helps us select all the sketch entities that are linked together. For example, with this option, selecting one line of a rectangle will automatically select the whole rectangle since the four lines that make up the rectangle are connected. We should uncheck this option if we only want to offset a part of the shape; for example, to offset only one line of a rectangle.
• Bi-directional: This will apply two offsets in two different directions, outward and inward.
• Caps ends: This command is applied when the offset is not an enclosed shape, such as an enclosed rectangle or a circle. The Caps ends option allows us to easily enclose option loops between the original and the offset sketch entities.
• Construction geometry: This allows us to make the original or the offset sketch entities construction entities (for example, construction lines, arcs, and more). Checking the Base geometry will switch the original sketch entities into construction entities. Checking Offset geometry will do the same for the offset entities.

This concludes the Offset Entities sketching command. We have learned what the Offset Entities command does and how to use it. We also covered the Mirror Entities sketching command. Now, we can start learning about how to create patterns.