3.6 Starting layout in orcad  (Page 6/9)

Now let’s go the other direction. Perhaps we have one to many decoupling capacitors, so we will remove one. On page 2 of your schematics, delete one of the decoupling capacitors.

Next, save the design and regenerate the netlist as described previously. Close your board in Layout, but keep Layout running. In Layout select Tools-->ECOs-->Auto ECO . First, you will be asked for your original board file. Find the file Elec424Tutorial.max in your board directory. Second, you will be asked for the new netlist file that you just created. Find the Elec424Tutorial.mnl file in your sch directory. Finally, you will be asked for a lis file to write to. This file is just a report of the ECO, and it is safe to overwrite the existing one in your board directory. When the ECO is done, you will see the lis file in Notepad with a report of what happened during the ECO.

When you open your board after an ECO, you may get the following message.

Just click OK . We will fix this problem a little bit later.

Deleting this part was just a demonstration. We really want that capacitor in our design, so let’s put it back. Adding new components to a design requires a little more caution than deleting components. Open up page 2 of your schematics and cut and paste one of the other decoupling capacitors.

When you cut and paste a component, every property gets copied, including the reference designator. This design now has two capacitors called C10 . If you were to try and perform an ECO right now, it would cause much confusion. Double-click the new capacitor and change the reference to C? .

Since we have some new parts, we need to annotate the design again. Perform an incremental reference update as you did before. The new part should now have a number. Regenerate the netlist and start an ECO. When done, the part should be back in the design. However, when we cut and paste parts, all properties are copied, and this includes x and y locations on the board. Our new part is probably sitting right on top of another part. Use the components spreadsheet to locate the new part. Give it a new and safe location such as 0,0 and then use the Component Tool to place it in the proper location. You could also avoid this problem by resetting the coordinate properties in Capture before regenerating the netlist.

You will often use ECO to do forward-annotation, but there are only a few occasions where you may want to perform back annotation. One such instance is to rename components. Right now, all the components in your design are named according to their order in schematics. However, in a larger board, it will be very hard to tell where a specific component is during debug. The components on the board will seem to be named in a random manner. Layout can rename your components for you, which will make finding them on the board much easier. To see the results of this operation, make the silkscreen layer visible again ( SST ). Select Options-->Components Renaming… and choose Right, Down… in the Rename Direction dialog.