3.5 Preparing for orcad layout

Annotation

Now that your schematics are complete, you are ready to prepare to export the design to Layout. From now on, you will be working in both Capture and Layout. The first step in preparing your design is to annotate it. Annotation really involves several steps. First, we will assignunique reference designators to all of the parts in our circuit. Remember reference designators? These are just labels that are used in Layout to uniquely identify different types of parts. If you look at the hierarchy view in the project window, you will see a jumble of reference designators.You might have several capacitors named C1 or a lot of parts that have the label, R?, C?, U?, etc.

To fix this, we will use a few of the annotation tools. In the file view of the project explorer, highlight the top-level design file (the one with the dsn extension) and then select Tools-->Annotate . You will see the Annotate dialog box.

In a new design, it is best to first reset all the part designators. To do this, click the radio button that says Reset Part References to “?” and then click OK . You will be asked if you want to save your design before proceeding. Every part in your design will now have a question mark in its reference designator instead of a number. Now, reopen the annotate dialog box and check the box that says Incremental Reference Update and click OK . This will go through your entire design and number each part starting with 1 for each part type. If you now look in the hierarchy view, you will see that you have a nicely ordered list of parts.

Intersheet references

The next thing we will do is add intersheet references to your schematics. Doing this will place page numbers near each off-page connector that indicate to which other pages that net is connected. This is invaluable during design and debug because it will help you track individual nets across a large designin many pages of schematics. Since we only have two pages of schematics in this design, we could probably get away without adding intersheet references; however, it is a useful tool and should always be used for good design practice. Another reason for using this tool is that it helps to find mistakes in namingnets. For example, say you have a net named CLKIN but on one page of schematics you mislabel this net CLKIM. After annotation, these two off page connectors will not have page numbers next to them, indicating that they are single-pin nets. This would be an immediate warning flag that something isseriously wrong with your schematics. To add intersheet references, bring up the annotate dialog box again. Select the radio button that is labeled Add Intersheet References . You will get a secondary dialog box, and you can leave the default values as they are for now. Just click OK to continue. As far as schematics are concerned, your design is now fairly complete.